ANSYS Mechanical Application User's Guide ANSYS, Inc. Southpointe 275 Technology Drive Canonsburg, PA 15317 ansysinfo@ansys.com http://www.ansys.com (T) 724-746-3304 (F) 724-514-9494 Release 14.0 November 2011 ANSYS, Inc. is certified to ISO 9001:2008. Copyright and Trademark Information © 2011 SAS IP, Inc. All rights reserved. Unauthorized use, distribution or duplication is prohibited. ANSYS, ANSYS Workbench, Ansoft, AUTODYN, EKM, Engineering Knowledge Manager, CFX, FLUENT, HFSS and any and all ANSYS, Inc. brand, product, service and feature names, logos and slogans are registered trademarks or trademarks of ANSYS, Inc. or its subsidiaries in the United States or other countries. ICEM CFD is a trademark used by ANSYS, Inc. under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product, service and feature names or trademarks are the property of their respective owners. Disclaimer Notice THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARE CONFIDENTIAL AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The software products and documentation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under a software license agreement that contains provisions concerning non-disclosure, copying, length and nature of use, compliance with exporting laws, warranties, disclaimers, limitations of liability, and remedies, and other provisions. The software products and documentation may be used, disclosed, transferred, or copied only in accordance with the terms and conditions of that software license agreement. ANSYS, Inc. is certified to ISO 9001:2008. U.S. Government Rights For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement, the use, duplication, or disclosure by the United States Government is subject to restrictions stated in the ANSYS, Inc. software license agreement and FAR 12.212 (for non-DOD licenses). Third-Party Software See the legal information in the product help files for the complete Legal Notice for ANSYS proprietary software and third-party software. If you are unable to access the Legal Notice, please contact ANSYS, Inc. Published in the U.S.A. Table of Contents Approach .................................................................................................................................................... 1 Overall Steps to Using the Mechanical Application .................................................................................. 1 Create Analysis System ..................................................................................................................... 1 Define Engineering Data ................................................................................................................... 2 Attach Geometry .............................................................................................................................. 2 Define Part Behavior ......................................................................................................................... 6 Define Connections .......................................................................................................................... 8 Apply Mesh Controls and Preview Mesh ............................................................................................ 9 Establish Analysis Settings ................................................................................................................ 9 Define Initial Conditions ................................................................................................................. 12 Apply Loads and Supports .............................................................................................................. 14 Solve .............................................................................................................................................. 15 Review Results ................................................................................................................................ 16 Create Report (optional) ................................................................................................................. 17 Analysis Types ...................................................................................................................................... 17 Design Assessment Analysis ............................................................................................................ 17 Eigen Response Analysis ................................................................................................................. 20 Linear Buckling Analysis ............................................................................................................ 20 Modal Analysis ......................................................................................................................... 25 Applying Pre-Stress Effects ........................................................................................................ 30 Electric Analysis .............................................................................................................................. 32 Explicit Dynamics Analysis .............................................................................................................. 35 Recommended Guidelines When Using Pre-Stress With Explicit Dynamics ................................. 55 Harmonic Analysis .......................................................................................................................... 57 Harmonic Analysis Using Linked Modal Analysis System ............................................................ 64 Magnetostatic Analysis ................................................................................................................... 66 Random Vibration Analysis ............................................................................................................. 70 Response Spectrum Analysis ........................................................................................................... 75 Static Structural Analysis ................................................................................................................. 79 Steady-State Thermal Analysis ......................................................................................................... 84 Thermal-Electric Analysis ................................................................................................................ 87 Transient Structural and Rigid Dynamics Analyses ........................................................................... 91 Transient Structural Analysis ..................................................................................................... 91 Transient Structural Analysis Using Linked Modal Analysis System ....................................... 99 Rigid Dynamics Analysis ......................................................................................................... 102 Command Reference for Rigid Dynamics Systems .................................................................... 109 Transient Thermal Analysis ............................................................................................................ 133 Special Analysis Topics ........................................................................................................................ 137 Static Analysis From Rigid Dynamics Analysis ................................................................................ 137 Thermal-Stress Analysis ................................................................................................................. 138 Fluid-Structure Interaction (FSI) ..................................................................................................... 142 Fluid-Structure Interaction (FSI) - One-Way Transfer ................................................................. 143 Face Forces at Fluid-Structure Interface ............................................................................. 144 Face Temperatures and Convections at Fluid-Structure Interface ........................................ 145 Volumetric Temperature Transfer ....................................................................................... 145 CFD Results Mapping ........................................................................................................ 145 Fluid-Structure Interaction (FSI) - Two-Way Transfer ................................................................. 146 Ansoft - Mechanical Data Transfer ................................................................................................. 146 Thermal/Structural Load Import .............................................................................................. 146 Thermal/Structural Results Export ........................................................................................... 149 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. iii ANSYS Mechanical Application User's Guide Icepak to Mechanical Data Transfer ............................................................................................... 151 Mechanical-Electronics Interaction (Mechatronics) Data Transfer .................................................... 152 Overall Workflow for Mechatronics Analysis ............................................................................. 152 Set up the Mechanical Application for Export to Simplorer ....................................................... 153 External Data Import ..................................................................................................................... 153 POLYFLOW to Mechanical Data Transfer ......................................................................................... 158 Simplorer/Rigid Dynamics Co-Simulation ..................................................................................... 160 Simplorer Pins ........................................................................................................................ 161 System Coupling .......................................................................................................................... 163 Supported Capabilities and Limitations ................................................................................... 163 System Coupling Related Settings in Mechanical ..................................................................... 164 Restarting Mechanical Analyses as Part of System Coupling ..................................................... 164 Running Mechanical as a System Coupling Participant from the Command Line ....................... 165 Troubleshooting Two-Way Coupling Analysis Problems ........................................................... 165 Tutorials ............................................................................................................................................. 166 Steady-State and Transient Thermal Analysis of a Circuit Board ....................................................... 166 Cyclic Symmetry Analysis of a Rotor - Brake Assembly .................................................................... 175 Using Finite Element Access to Resolve Overconstraint .................................................................. 189 Actuator Mechanism using Rigid Body Dynamics .......................................................................... 220 Wizards .............................................................................................................................................. 229 The Mechanical Wizard ................................................................................................................. 230 Basics ...................................................................................................................................................... 233 The Mechanical Application Interface .................................................................................................. 233 The Mechanical Application Window ............................................................................................. 233 Tree Outline .................................................................................................................................. 235 Tree Outline Conventions ........................................................................................................ 235 Tree Outline Go To Options ..................................................................................................... 237 Environment Filtering ................................................................................................................... 238 Interface Behavior Based on License Levels .................................................................................... 239 Suppress and Unsuppress Items .................................................................................................... 239 Tabs ............................................................................................................................................. 240 Geometry ..................................................................................................................................... 240 Legend Functionality .................................................................................................................... 241 Discrete Legends in the Mechanical Application ...................................................................... 241 Graphical Selection ....................................................................................................................... 241 Windows Management ................................................................................................................. 251 Workbench Windows Manager ............................................................................................... 252 Selection Information Window ................................................................................................ 252 Activating the Selection Information Window .................................................................... 253 Supported Selection Modes and Reported Information ..................................................... 254 Selection Information Toolbar ........................................................................................... 261 Reselect, Export, and Sort .................................................................................................. 264 Worksheet Window ................................................................................................................. 266 Graph and Tabular Data Windows ........................................................................................... 268 Messages Window .................................................................................................................. 270 Graphics Annotation Window ................................................................................................. 271 New Section Plane .................................................................................................................. 271 The Mechanical Wizard Window .............................................................................................. 274 Details View .................................................................................................................................. 274 Parameters ................................................................................................................................... 279 Toolbars ....................................................................................................................................... 280 Main Menu ............................................................................................................................. 280 iv Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS Mechanical Application User's Guide Standard Toolbar .................................................................................................................... 283 Graphics Toolbar ..................................................................................................................... 285 Context Toolbar ...................................................................................................................... 287 Named Selection Toolbar ........................................................................................................ 298 Unit Conversion Toolbar .......................................................................................................... 298 Graphics Options Toolbar ........................................................................................................ 298 Print Preview ................................................................................................................................ 301 Triad and Rotation Cursors ............................................................................................................ 301 Exporting Data ............................................................................................................................. 302 Customizing the Mechanical Application ............................................................................................. 303 The Mechanical Application Options ............................................................................................. 303 Variables ....................................................................................................................................... 313 Macros ......................................................................................................................................... 313 Features .................................................................................................................................................. 315 Geometry in the Mechanical Application ............................................................................................. 315 Assemblies, Parts, and Bodies ........................................................................................................ 315 Multibody Behavior ................................................................................................................ 316 Working with Parts ................................................................................................................. 316 Integration Schemes ............................................................................................................... 317 Color Coding of Parts .............................................................................................................. 317 Working with Bodies ............................................................................................................... 318 Hide or Suppress Bodies ......................................................................................................... 318 Hide or Show Faces ................................................................................................................. 319 Assumptions and Restrictions for Assemblies, Parts, and Bodies ............................................... 319 Solid Bodies .................................................................................................................................. 319 Surface Bodies .............................................................................................................................. 319 Assemblies of Surface Bodies .................................................................................................. 320 Thickness Mode ...................................................................................................................... 320 Importing Surface Body Models .............................................................................................. 320 Importing Surface Body Thickness .......................................................................................... 321 Surface Body Shell Offsets ....................................................................................................... 321 Specifying Surface Body Thickness .......................................................................................... 323 Specifying Surface Body Layered Sections ............................................................................... 325 Defining and Applying a Layered Section .......................................................................... 326 Viewing Individual Layers .................................................................................................. 327 Layered Section Properties ................................................................................................ 327 Notes on Layered Section Behavior ................................................................................... 328 Faces With Multiple Thicknesses and Layers Specified .............................................................. 328 Line Bodies ................................................................................................................................... 329 Rigid Bodies ................................................................................................................................. 331 2-D Analyses ................................................................................................................................. 332 Using Generalized Plane Strain ................................................................................................ 333 Symmetry ..................................................................................................................................... 334 Types of Regions ..................................................................................................................... 335 Symmetry Region ............................................................................................................. 336 Explicit Dynamics Symmetry ....................................................................................... 337 General Symmetry ................................................................................................ 338 Global Symmetry Planes ....................................................................................... 338 Periodic Region ................................................................................................................ 339 Electromagnetic Periodic Symmetry ............................................................................ 339 Periodicity Example .............................................................................................. 340 Cyclic Region .................................................................................................................... 342 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. v ANSYS Mechanical Application User's Guide Cyclic Symmetry in a Static Structural Analysis ............................................................. 343 Applying Loads and Supports for Cyclic Symmetry in a Static Structural Analysis .... 343 Reviewing Results for Cyclic Symmetry in a Static Structural Analysis ..................... 344 Cyclic Symmetry in a Modal Analysis ........................................................................... 345 Applying Loads and Supports for Cyclic Symmetry in a Modal Analysis .................. 345 Analysis Settings for Cyclic Symmetry in a Modal Analysis ...................................... 346 Reviewing Results for Cyclic Symmetry in a Modal Analysis .................................... 346 Cyclic Symmetry in a Thermal Analysis ......................................................................... 351 Applying Loads for Cyclic Symmetry in a Thermal Analysis ..................................... 351 Reviewing Results for Cyclic Symmetry in a Thermal Analysis ................................. 351 Symmetry Defined in DesignModeler ...................................................................................... 351 Symmetry in the Mechanical Application ................................................................................ 352 Named Selections ......................................................................................................................... 354 Defining Named Selections ..................................................................................................... 357 Specifying Named Selections by Geometry Type ............................................................... 358 Specifying Named Selections by Direct Node Selection ..................................................... 358 Specifying Named Selections using Worksheet Criteria ...................................................... 362 Displaying Named Selections .................................................................................................. 367 Using Named Selections ......................................................................................................... 369 Using Named Selections via the Toolbar ............................................................................ 370 Scoping Analysis Objects to Named Selections .................................................................. 371 Including Named Selections in Program Controlled Inflation .............................................. 371 Importing Named Selections ............................................................................................. 372 Exporting Named Selections ............................................................................................. 372 Displaying Interior Mesh Faces ................................................................................................ 372 Converting Named Selection Groups to Mechanical APDL Application Components ................ 373 Mesh Numbering .......................................................................................................................... 374 Path (Construction Geometry) ....................................................................................................... 376 Surface (Construction Geometry) .................................................................................................. 381 Remote Point ................................................................................................................................ 381 Remote Point Overview .......................................................................................................... 381 Connection Lines .................................................................................................................... 384 Promote Remote Point ............................................................................................................ 385 Remote Point Commands Objects ........................................................................................... 385 Point Mass .................................................................................................................................... 385 Thermal Point Mass ....................................................................................................................... 385 Using Gaskets ............................................................................................................................... 387 Gasket Bodies ......................................................................................................................... 387 Gasket Mesh Control ............................................................................................................... 387 Gasket Results ........................................................................................................................ 388 Coordinate Systems Overview ............................................................................................................. 389 Creating Coordinate Systems ........................................................................................................ 389 Initial Creation and Definition ................................................................................................. 389 Establishing Origin for Associative and Non-Associative Coordinate Systems ............................ 390 Setting Principal Axis and Orientation ..................................................................................... 391 Using Transformations ............................................................................................................ 391 Importing Coordinate Systems ...................................................................................................... 392 Applying Coordinate Systems as Reference Locations .................................................................... 392 Using Coordinate Systems to Specify Joint Locations ..................................................................... 392 Creating Section Planes ................................................................................................................ 393 Transferring Coordinate Systems to the Mechanical APDL Application ........................................... 395 Graphics ............................................................................................................................................. 396 vi Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS Mechanical Application User's Guide Annotations ................................................................................................................................. 396 Lighting Controls .......................................................................................................................... 401 Comments, Images, Figures ........................................................................................................... 401 Connections ....................................................................................................................................... 402 Connections Folder ....................................................................................................................... 402 Connection Group Folder .............................................................................................................. 403 Common Connections Folder Operations for Auto Generated Connections .................................... 407 Contact ........................................................................................................................................ 408 Contact Overview ................................................................................................................... 409 Contact Settings ..................................................................................................................... 411 Scope Settings .................................................................................................................. 412 Definition Settings ............................................................................................................ 414 Advanced Settings ............................................................................................................ 418 Setting Contact Conditions Manually ...................................................................................... 426 Contact Ease of Use Features ................................................................................................... 426 Controlling Transparency for Contact Regions ................................................................... 427 Displaying Contact Bodies in Separate Windows ................................................................ 427 Hiding Bodies Not Scoped to a Contact Region .................................................................. 428 Renaming Contact Regions Based on Geometry Names ..................................................... 428 Identifying Contact Regions for a Body .............................................................................. 429 Flipping Contact and Target Scope Settings ....................................................................... 429 Merging Contact Regions That Share Geometry ................................................................. 430 Saving or Loading Contact Region Settings ....................................................................... 430 Resetting Contact Regions to Default Settings ................................................................... 431 Locating Bodies Without Contact ...................................................................................... 431 Locating Parts Without Contact ......................................................................................... 431 Contact in Rigid Dynamics ...................................................................................................... 431 Joints ........................................................................................................................................... 433 Joint Characteristics ................................................................................................................ 433 Types of Joints ........................................................................................................................ 436 Joint Properties and Application ............................................................................................. 442 Example: Assembling Joints .................................................................................................... 448 Example: Configuring Joints .................................................................................................... 458 Automatic Joint Creation ........................................................................................................ 464 Joint Stops and Locks .............................................................................................................. 464 Ease of Use Features ............................................................................................................... 466 Detecting Overconstrained Conditions .................................................................................... 469 Mesh Connection ......................................................................................................................... 470 Springs ......................................................................................................................................... 478 Beam Connections ........................................................................................................................ 483 Spot Welds ................................................................................................................................... 484 End Releases ................................................................................................................................. 486 Body Interactions in Explicit Dynamics Analyses ............................................................................ 487 Properties for Body Interactions Folder .................................................................................... 488 Contact Detection ............................................................................................................ 489 Formulation ...................................................................................................................... 491 Shell Thickness Factor ....................................................................................................... 492 Body Self Contact ............................................................................................................. 492 Element Self Contact ......................................................................................................... 492 Tolerance .......................................................................................................................... 493 Pinball Factor .................................................................................................................... 493 Time Step Safety Factor ..................................................................................................... 493 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. vii ANSYS Mechanical Application User's Guide Limiting Time Step Velocity ............................................................................................... 494 Edge on Edge Contact ...................................................................................................... 494 Interaction Type Properties for Body Interaction Object ........................................................... 494 Frictionless Type ............................................................................................................... 494 Frictional Type .................................................................................................................. 495 Bonded Type .................................................................................................................... 496 Reinforcement Type .......................................................................................................... 497 Analysis Settings ................................................................................................................................. 499 Analysis Settings for Most Analysis Types ....................................................................................... 499 Step Controls .......................................................................................................................... 500 Solver Controls ....................................................................................................................... 501 Restart Analysis ...................................................................................................................... 501 Restart Controls ...................................................................................................................... 502 Creep Controls ........................................................................................................................ 503 Cyclic Controls ........................................................................................................................ 503 Radiosity Controls ................................................................................................................... 504 Nonlinear Controls .................................................................................................................. 505 Output Controls ...................................................................................................................... 506 Options .................................................................................................................................. 507 Damping Controls .................................................................................................................. 508 Visibility ................................................................................................................................. 508 Analysis Data Management ..................................................................................................... 509 Analysis Settings Notes ........................................................................................................... 510 Rotordynamics Controls .......................................................................................................... 510 Analysis Settings for Explicit Dynamics Analyses ............................................................................ 511 Explicit Dynamics Step Controls .............................................................................................. 511 Explicit Dynamics Solver Controls ............................................................................................ 516 Explicit Dynamics Euler Domain Controls ................................................................................ 519 Explicit Dynamics Damping Controls ....................................................................................... 520 Explicit Dynamics Erosion Controls .......................................................................................... 521 Explicit Dynamics Output Controls .......................................................................................... 522 Explicit Dynamics Data Management Settings ......................................................................... 524 Explicit Dynamics Analysis Settings Notes ............................................................................... 525 Steps and Step Controls for Static and Transient Analyses .............................................................. 525 Role of Time in Tracking .......................................................................................................... 525 Steps, Substeps, and Equilibrium Iterations .............................................................................. 526 Automatic Time Stepping ....................................................................................................... 527 Guidelines for Integration Step Size ......................................................................................... 527 Step Controls .......................................................................................................................... 529 Solver Controls ............................................................................................................................. 533 Restart Analysis ............................................................................................................................ 535 Restart Controls ............................................................................................................................ 535 Creep Controls .............................................................................................................................. 537 Cyclic Controls .............................................................................................................................. 537 Radiosity Controls ......................................................................................................................... 537 Options for Modal, Harmonic, Linear Buckling, Random Vibration, and Response Spectrum Analyses ............................................................................................................................................. 538 Damping Controls ........................................................................................................................ 542 Nonlinear Controls ........................................................................................................................ 542 Output Controls ............................................................................................................................ 545 Analysis Data Management ........................................................................................................... 549 Rotordynamics Controls ................................................................................................................ 551 viii Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS Mechanical Application User's Guide Visibility ....................................................................................................................................... 551 Applying Boundary Conditions ........................................................................................................... 551 Types of Supports ......................................................................................................................... 551 Fixed Supports ....................................................................................................................... 552 Displacements ........................................................................................................................ 553 Remote Displacement ............................................................................................................. 555 Velocity .................................................................................................................................. 556 Impedance Boundary ............................................................................................................. 557 Frictionless Face ...................................................................................................................... 558 Compression Only Support ..................................................................................................... 559 Cylindrical Support ................................................................................................................. 560 Simply Supported Edge .......................................................................................................... 560 Simply Supported Vertex ........................................................................................................ 561 Fixed Rotation ........................................................................................................................ 561 Elastic Support ....................................................................................................................... 562 Types of Loads .............................................................................................................................. 562 Acceleration ........................................................................................................................... 563 Standard Earth Gravity ............................................................................................................ 566 Rotational Velocity .................................................................................................................. 567 Pressure ................................................................................................................................. 568 Pipe Pressure .......................................................................................................................... 569 Pipe Temperature ................................................................................................................... 569 Hydrostatic Pressure ............................................................................................................... 569 Force ...................................................................................................................................... 570 Remote Force ......................................................................................................................... 572 Bearing Load .......................................................................................................................... 573 Bolt Pretension ....................................................................................................................... 575 Moment ................................................................................................................................. 577 Generalized Plane Strain ......................................................................................................... 578 Line Pressure .......................................................................................................................... 578 PSD Base Excitation ................................................................................................................ 579 RS Base Excitation ................................................................................................................... 580 Joint Load ............................................................................................................................... 581 Thermal Condition .................................................................................................................. 583 Temperature ........................................................................................................................... 584 Convection ............................................................................................................................. 584 Radiation ................................................................................................................................ 586 Heat Flow ............................................................................................................................... 587 Perfectly Insulated .................................................................................................................. 589 Heat Flux ................................................................................................................................ 589 Internal Heat Generation ......................................................................................................... 590 Voltage ................................................................................................................................... 590 Current ................................................................................................................................... 591 Electromagnetic Boundary Conditions and Excitations ............................................................ 591 Magnetic Flux Boundary Conditions .................................................................................. 592 Conductor ........................................................................................................................ 593 Solid Source Conductor Body ...................................................................................... 594 Voltage Excitation for Solid Source Conductors ............................................................ 596 Current Excitation for Solid Source Conductors ............................................................ 597 Stranded Source Conductor Body ............................................................................... 598 Current Excitation for Stranded Source Conductors ..................................................... 599 Imported Body Force Density .................................................................................................. 601 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ix ANSYS Mechanical Application User's Guide Imported Body Temperature ................................................................................................... 602 Imported Convection Coefficient ............................................................................................ 603 Imported Heat Flux ................................................................................................................. 603 Imported Heat Generation ...................................................................................................... 604 Imported Pressure .................................................................................................................. 604 Imported Surface Force Density .............................................................................................. 605 Imported Temperature ............................................................................................................ 605 Motion Load ........................................................................................................................... 605 Fluid Solid Interface ................................................................................................................ 607 Detonation Point .................................................................................................................... 608 Conditions .................................................................................................................................... 611 Coupling ................................................................................................................................ 612 Constraint Equation ................................................................................................................ 612 Pipe Idealization ..................................................................................................................... 614 Direct FE ....................................................................................................................................... 615 Nodal Orientation ................................................................................................................... 615 Nodal Force ............................................................................................................................ 616 Nodal Pressure ........................................................................................................................ 617 FE Displacement ..................................................................................................................... 618 FE Rotation ............................................................................................................................. 619 Spatial Varying Loads and Displacements ...................................................................................... 620 Specifying Load Values .................................................................................................................. 621 Constant Load Values .............................................................................................................. 621 Constant Load Expressions ...................................................................................................... 621 Tabular Loads ......................................................................................................................... 623 Importing Load History ..................................................................................................... 623 Exporting Load History ..................................................................................................... 624 Spatial Load Tabular Data .................................................................................................. 624 Supported Tabular Loads .................................................................................................. 625 Function Loads ....................................................................................................................... 626 Spatial Load and Displacement Function Data ................................................................... 626 Supported Function Loads ................................................................................................ 627 Remote Boundary Conditions ....................................................................................................... 628 Imported Loads ............................................................................................................................ 630 Direction ...................................................................................................................................... 632 Scope ........................................................................................................................................... 634 Results in the Mechanical Application ................................................................................................. 634 Structural Results .......................................................................................................................... 634 Deformation ........................................................................................................................... 635 Stress and Strain ..................................................................................................................... 639 Equivalent (von Mises) ...................................................................................................... 640 Maximum, Middle, and Minimum Principal ........................................................................ 640 Maximum Shear ............................................................................................................... 641 Intensity ........................................................................................................................... 641 Vector Principals ............................................................................................................... 642 Error (Structural) ............................................................................................................... 642 Thermal Strain .................................................................................................................. 643 Equivalent Plastic Strain .................................................................................................... 644 Equivalent Creep Strain ..................................................................................................... 645 Equivalent Total Strain ...................................................................................................... 645 Membrane Stress .............................................................................................................. 645 Bending Stress .................................................................................................................. 646 x Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS Mechanical Application User's Guide Stabilization Energy ................................................................................................................ 646 Strain Energy .......................................................................................................................... 647 Linearized Stress ..................................................................................................................... 647 Contact Results ....................................................................................................................... 649 Reactions ............................................................................................................................... 651 Energy (Transient Structural and Rigid Dynamics Analyses) ...................................................... 654 Frequency Response and Phase Response ............................................................................... 655 Stress Tools ............................................................................................................................. 658 Maximum Equivalent Stress Safety Tool ............................................................................ 659 Maximum Shear Stress Safety Tool .................................................................................... 661 Mohr-Coulomb Stress Safety Tool ...................................................................................... 662 Maximum Tensile Stress Safety Tool ................................................................................... 664 Fatigue (Fatigue Tool) .............................................................................................................. 666 Contact Tool ........................................................................................................................... 666 Contact Tool Initial Information ......................................................................................... 670 Beam Tool ............................................................................................................................... 670 Structural Probes .................................................................................................................... 671 Joint Probes ...................................................................................................................... 677 Response PSD Probe ......................................................................................................... 679 Spring Probes ................................................................................................................... 679 Beam Probes .................................................................................................................... 680 Beam Results .......................................................................................................................... 680 Shear-Moment Diagram .................................................................................................... 681 Gasket Results ........................................................................................................................ 682 Campbell Diagram Chart Results ............................................................................................. 683 Thermal Results ............................................................................................................................ 685 Temperature ........................................................................................................................... 686 Heat Flux ................................................................................................................................ 686 Heat Reaction ......................................................................................................................... 687 Error (Thermal) ....................................................................................................................... 687 Thermal Probes ....................................................................................................................... 687 Magnetostatic Results ................................................................................................................... 688 Electric Potential ..................................................................................................................... 688 Total Magnetic Flux Density .................................................................................................... 688 Directional Magnetic Flux Density ........................................................................................... 689 Total Magnetic Field Intensity .................................................................................................. 689 Directional Magnetic Field Intensity ........................................................................................ 689 Total Force .............................................................................................................................. 689 Directional Force .................................................................................................................... 689 Current Density ...................................................................................................................... 689 Inductance ............................................................................................................................. 689 Flux Linkage ........................................................................................................................... 690 Error (Magnetic) ...................................................................................................................... 691 Magnetostatic Probes ............................................................................................................. 691 Electric Results .............................................................................................................................. 693 Electric Probes ........................................................................................................................ 694 Fatigue Results ............................................................................................................................. 695 Fatigue Material Properties ..................................................................................................... 695 Fatigue Analysis and Loading Options ..................................................................................... 696 Reviewing Fatigue Results ....................................................................................................... 699 User Defined Results ..................................................................................................................... 702 Overview ................................................................................................................................ 703 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. xi ANSYS Mechanical Application User's Guide Characteristics ........................................................................................................................ 703 Application ............................................................................................................................. 704 Nodal Scoping ........................................................................................................................ 705 User Defined Result Expressions .............................................................................................. 706 User Defined Result Identifier .................................................................................................. 708 Unit Description ..................................................................................................................... 710 User Defined Results for the Mechanical APDL Solver .............................................................. 711 User Defined Results for Explicit Dynamics Analyses ................................................................ 714 Results Related Topics ................................................................................................................... 718 Result Definitions ................................................................................................................... 718 Applying Results Based on Geometry ................................................................................ 719 Averaged vs. Unaveraged Contour Results ......................................................................... 721 Clearing Results Data ........................................................................................................ 722 Peak Composite Results .................................................................................................... 723 Material Properties Used in Postprocessing ....................................................................... 723 Scoping Results ................................................................................................................ 724 Solution Coordinate System .............................................................................................. 726 Surface Body Results ......................................................................................................... 727 Unconverged Results ........................................................................................................ 728 Result Outputs ........................................................................................................................ 729 Chart and Table ................................................................................................................ 729 Contour Results ................................................................................................................ 732 Coordinate Systems Results .............................................................................................. 732 Nodal Coordinate Systems Results ............................................................................... 732 Elemental Coordinate Systems Results ........................................................................ 732 Rotational Order of Coordinate System Results ............................................................ 733 Eroded Nodes in Explicit Dynamics Analyses ..................................................................... 733 The Euler Domain in Explicit Dynamics Analyses ................................................................ 735 Path Results ...................................................................................................................... 736 Probes .............................................................................................................................. 737 Overview and Probe Types .......................................................................................... 737 Probe Details View ..................................................................................................... 739 Surface Results ................................................................................................................. 742 Vector Plots ...................................................................................................................... 743 Result Utilities ......................................................................................................................... 743 Adaptive Convergence ...................................................................................................... 743 Animation ........................................................................................................................ 743 Capped Isosurfaces ........................................................................................................... 745 Dynamic Legend .............................................................................................................. 746 Generating Reports .......................................................................................................... 747 Renaming Results Based on Definition .............................................................................. 747 Results Legend ................................................................................................................. 747 Named Legends ......................................................................................................... 748 Date and Time ............................................................................................................ 749 Max, Min on Color Bar ................................................................................................. 749 Logarithmic Scale ....................................................................................................... 749 All Scientific Notation ................................................................................................. 749 Digits ......................................................................................................................... 749 Independent Bands .................................................................................................... 749 Color Scheme ............................................................................................................. 749 Results Toolbar ................................................................................................................. 750 Solution Combinations ..................................................................................................... 750 xii Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS Mechanical Application User's Guide Solving Overview ................................................................................................................................ 751 Solve Modes and Recommended Usage ........................................................................................ 754 Using Solve Process Settings ......................................................................................................... 755 Solution Restarts .......................................................................................................................... 759 Solving Scenarios .......................................................................................................................... 766 Solution Information Object .......................................................................................................... 769 Postprocessing During Solve ......................................................................................................... 774 Result Trackers .............................................................................................................................. 774 Structural Result Trackers ........................................................................................................ 775 Thermal Result Trackers .......................................................................................................... 776 Explicit Dynamics Result Trackers ............................................................................................ 777 Point Scoped Result Trackers for Explicit Dynamics ............................................................ 777 Body Scoped Result Trackers for Explicit Dynamics ............................................................ 781 Force Reaction Result Trackers for Explicit Dynamics .......................................................... 784 Viewing and Filtering Result Tracker Graphs for Explicit Dynamics ...................................... 785 Result Tracker Features ............................................................................................................ 786 Result Tracker Plot Features ............................................................................................... 786 Renaming Result Trackers ................................................................................................. 787 Exporting Result Trackers .................................................................................................. 787 Adaptive Convergence .................................................................................................................. 787 File Management in the Mechanical Application ............................................................................ 792 Solving Units ................................................................................................................................ 793 Saving your Results in the Mechanical Application ......................................................................... 852 Writing and Reading the Mechanical APDL Application Files .......................................................... 852 Converting Boundary Conditions to Nodal DOF Constraints (Mechanical APDL Solver) ................... 854 Resolving Thermal Boundary Condition Conflicts ........................................................................... 855 Resume Capability for Explicit Dynamics Analyses ......................................................................... 855 Commands Objects ............................................................................................................................ 856 Commands Object Features .......................................................................................................... 857 Using Commands Objects with the MAPDL Solver ......................................................................... 860 Report Preview ................................................................................................................................... 864 Tables ........................................................................................................................................... 865 Figures and Images ....................................................................................................................... 865 Publishing .................................................................................................................................... 865 Sending ........................................................................................................................................ 865 Comparing Databases ................................................................................................................... 865 Customize Report Content ............................................................................................................ 866 Meshing in the Mechanical Application ............................................................................................... 867 Parameters ......................................................................................................................................... 867 Specifying Parameters .................................................................................................................. 867 CAD Parameters ............................................................................................................................ 869 Design Assessment ............................................................................................................................. 871 Predefined Assessment Types ....................................................................................................... 873 Modifying the Predefined Assessment Types Menu .................................................................. 873 Using BEAMST and FATJACK with Design Assessment .............................................................. 874 Using BEAMST with the Design Assessment System ................................................................. 875 Introduction ..................................................................................................................... 875 Information for Existing ASAS Users .................................................................................. 875 Attribute Group Types ....................................................................................................... 877 Code of Practise Selection ........................................................................................... 877 General Text ............................................................................................................... 879 Geometry Definition ................................................................................................... 879 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. xiii ANSYS Mechanical Application User's Guide Load Dependant Factors ............................................................................................. 880 Material Definition ...................................................................................................... 881 Ocean Environment .................................................................................................... 881 Available Results ............................................................................................................... 882 AISC LRFD Results ....................................................................................................... 882 AISC WSD Results ........................................................................................................ 883 API LRFD Results ......................................................................................................... 883 API WSD Results .......................................................................................................... 886 BS5950 Results ........................................................................................................... 890 DS449 High Results ..................................................................................................... 891 DS449 Normal Results ................................................................................................. 893 ISO Results ................................................................................................................. 894 NORSOK Results ......................................................................................................... 896 NPD Results ................................................................................................................ 899 Using FATJACK with the Design Assessment System ................................................................ 901 Introduction ..................................................................................................................... 902 Information for Existing ASAS Users .................................................................................. 902 Solution Selection Customization ...................................................................................... 904 Attribute Group Types ....................................................................................................... 904 Analysis Type Selection ............................................................................................... 905 General Text ............................................................................................................... 905 Geometry Definition ................................................................................................... 906 Joint Inspection Points ............................................................................................... 906 SCF Definitions ........................................................................................................... 907 Material Definition ...................................................................................................... 907 Ocean Environment .................................................................................................... 908 Available Results ............................................................................................................... 908 Damage Values ........................................................................................................... 908 Fatigue Assessment .................................................................................................... 908 SCF Values .................................................................................................................. 908 Stress Histogram Results ............................................................................................. 909 Stress Range Results ................................................................................................... 909 Changing the Assessment Type or XML Definition File Contents ..................................................... 910 Solution Selection ......................................................................................................................... 911 Using the Attribute Group Object .................................................................................................. 912 Developing and Debugging Design Assessment Scripts ................................................................ 914 Using the DA Result Object ........................................................................................................... 914 The Design Assessment XML Definition File ................................................................................... 915 Attributes Format ................................................................................................................... 916 Attribute Groups Format ......................................................................................................... 919 Script Format .......................................................................................................................... 920 Results Format ........................................................................................................................ 922 Design Assessment API Reference ................................................................................................. 925 DesignAssessment class .......................................................................................................... 932 Example Usage ................................................................................................................. 933 Typical Evaluate (or Solve) Script Output ........................................................................... 934 Helper class ............................................................................................................................ 934 Example Usage ................................................................................................................. 935 Typical Evaluate (or Solve) Script Output ........................................................................... 935 Typical Solver Output ........................................................................................................ 936 MeshData class ....................................................................................................................... 936 Example Usage ................................................................................................................. 936 xiv Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS Mechanical Application User's Guide Typical Evaluate (or Solve) Script Output ........................................................................... 937 DAElement class ..................................................................................................................... 937 Example Usage ................................................................................................................. 939 Typical Evaluate (or Solve) Script Output ........................................................................... 939 DANode class ......................................................................................................................... 939 Example Usage ................................................................................................................. 940 Typical Evaluate (or Solve) Script Output ........................................................................... 940 SectionData class .................................................................................................................... 940 Example Usage ................................................................................................................. 941 Typical Evaluate (or Solve) Script Output ........................................................................... 941 AttributeGroup class ............................................................................................................... 942 Example Usage ................................................................................................................. 942 Typical Evaluate (or Solve) Script Output ........................................................................... 942 Attribute class ......................................................................................................................... 943 Example Usage ................................................................................................................. 943 Typical Evaluate (or Solve) Script Output ........................................................................... 944 SolutionSelection class ........................................................................................................... 944 Example Usage ................................................................................................................. 944 Typical Evaluate (or Solve) Script Output ........................................................................... 944 Solution class .......................................................................................................................... 945 Example Usage ................................................................................................................. 946 Typical Evaluate (or Solve) Script Output ........................................................................... 947 SolutionResult class ................................................................................................................ 947 Example Usage ................................................................................................................. 951 Typical Evaluate (or Solve) Script Output ........................................................................... 952 DAResult class ........................................................................................................................ 952 Example Usage ................................................................................................................. 954 Typical Evaluate (or Solve) Script Output ........................................................................... 954 DAResultSet class ................................................................................................................... 955 Example Usage ................................................................................................................. 956 Typical Evaluate (or Solve) Script Output ........................................................................... 957 Examples of Design Assessment Usage ......................................................................................... 957 Using Design Assessment to Obtain Results from Mechanical APDL ......................................... 957 Creating the XML Definition File ........................................................................................ 958 Creating the Script to be Run on Solve, MAPDL_S.py ....................................................... 960 Creating the Script to be Run on Evaluate All Results, MAPDL_E.py .................................. 961 Expanding the Example .................................................................................................... 962 Using Design Assessment to Calculate Complex Results, such as Those Required by ASME ........ 963 Creating the XML Definition File ........................................................................................ 963 Creating the Script to be Run on Evaluate .......................................................................... 965 EvaluateAllResults ....................................................................................................... 965 EvaluateDamage ........................................................................................................ 965 EvaluateCulmativeDamage ......................................................................................... 966 Plot ............................................................................................................................ 966 Using Design Assessment to Perform Further Results Analysis for an Explicit Dynamics Analysis ............................................................................................................................................ 967 Creating the XML Definition File ........................................................................................ 967 Creating the Script to be Run on Evaluate .......................................................................... 968 Expanding the Example .................................................................................................... 970 Using Design Assessment to Obtain Composite Results Using Mechanical APDL ...................... 970 Creating the XML Definition File ........................................................................................ 972 Creating the Script to be Run on Solve, SolveFailure.py ............................................ 974 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. xv ANSYS Mechanical Application User's Guide Creating the Script to be Run on Evaluate All Results, EvaluateFailure.py ................. 974 Using a Dictionary to Avoid a Long if/elif/else Statement. ............................................ 974 Writing the MADPL .inp File from Within Design Assessment .................................... 974 Running Mechanical APDL Multiple Times ................................................................... 975 Expanding the Example .................................................................................................... 976 Virtual Topology in the Mechanical Application ................................................................................... 976 Objects Reference ................................................................................................................................... 977 Alert ................................................................................................................................................... 979 Analysis Settings ................................................................................................................................. 980 Angular Velocity ................................................................................................................................. 980 Beam .................................................................................................................................................. 982 Body .................................................................................................................................................. 983 Body Interactions ................................................................................................................................ 985 Body Interaction ................................................................................................................................. 986 Chart .................................................................................................................................................. 988 Commands ......................................................................................................................................... 988 Comment ........................................................................................................................................... 989 Connections ....................................................................................................................................... 990 Connection Group .............................................................................................................................. 991 Construction Geometry ...................................................................................................................... 993 Contact Region ................................................................................................................................... 994 Object Properties - Most Structural Analyses ................................................................................. 995 Object Properties - Explicit Dynamics Analyses .............................................................................. 995 Object Properties - Thermal and Electromagnetic Analyses ............................................................ 996 Contact Tool (Group) ........................................................................................................................... 997 Convergence ...................................................................................................................................... 998 Coordinate System ............................................................................................................................ 1000 Coordinate Systems .......................................................................................................................... 1000 Direct FE (Group) .............................................................................................................................. 1001 End Release ...................................................................................................................................... 1001 Environment (Group) ........................................................................................................................ 1002 Fatigue Tool (Group) ......................................................................................................................... 1003 Figure ............................................................................................................................................... 1006 Fluid Surface ..................................................................................................................................... 1006 Gasket Mesh Control ......................................................................................................................... 1007 Geometry ......................................................................................................................................... 1008 Global Coordinate System ................................................................................................................. 1010 Image ............................................................................................................................................... 1011 Imported Layered Section ................................................................................................................. 1011 Imported Load (Group) ..................................................................................................................... 1012 Imported Thickness .......................................................................................................................... 1014 Imported Thickness (Group) .............................................................................................................. 1015 Initial Conditions ............................................................................................................................... 1016 Initial Temperature ............................................................................................................................ 1017 Joint ................................................................................................................................................. 1018 Layered Section ................................................................................................................................ 1019 Loads, Supports, and Conditions (Group) ........................................................................................... 1021 Mesh ................................................................................................................................................ 1022 Mesh Connection .............................................................................................................................. 1024 Mesh Control Tools (Group) ............................................................................................................... 1026 Mesh Group (Group) ......................................................................................................................... 1028 Mesh Grouping ................................................................................................................................. 1029 xvi Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS Mechanical Application User's Guide Mesh Numbering .............................................................................................................................. 1029 Modal ............................................................................................................................................... 1030 Model ............................................................................................................................................... 1031 Named Selections ............................................................................................................................. 1032 Numbering Control ........................................................................................................................... 1034 Part .................................................................................................................................................. 1035 Path .................................................................................................................................................. 1037 Periodic/Cyclic Region ....................................................................................................................... 1038 Point Mass ........................................................................................................................................ 1039 Pre-Stress ......................................................................................................................................... 1040 Probe ............................................................................................................................................... 1042 Project .............................................................................................................................................. 1043 Remote Point .................................................................................................................................... 1044 Remote Points .................................................................................................................................. 1044 Result Tracker ................................................................................................................................... 1045 Results and Result Tools (Group) ........................................................................................................ 1047 Solution ............................................................................................................................................ 1050 Solution Combination ....................................................................................................................... 1051 Solution Information ......................................................................................................................... 1051 Spot Weld ......................................................................................................................................... 1052 Spring .............................................................................................................................................. 1054 Stress Tool (Group) ............................................................................................................................ 1055 Surface ............................................................................................................................................. 1057 Symmetry ......................................................................................................................................... 1057 Symmetry Region ............................................................................................................................. 1058 Thermal Point Mass ........................................................................................................................... 1059 Thickness .......................................................................................................................................... 1060 Validation ......................................................................................................................................... 1061 Velocity ............................................................................................................................................ 1063 Virtual Body ...................................................................................................................................... 1064 Virtual Body Group ........................................................................................................................... 1065 Virtual Cell ........................................................................................................................................ 1066 Virtual Hard Vertex ............................................................................................................................ 1067 Virtual Split Edge .............................................................................................................................. 1068 Virtual Split Face ............................................................................................................................... 1068 Virtual Topology ............................................................................................................................... 1069 CAD System Information ...................................................................................................................... 1071 General Information .......................................................................................................................... 1072 Troubleshooting ................................................................................................................................... 1073 Problem Situations ............................................................................................................................ 1073 A Linearized Stress Result Cannot Be Solved. ............................................................................... 1074 A Load Transfer Error Has Occurred. ............................................................................................. 1074 Although the Exported File Was Saved to Disk ............................................................................. 1075 Although the Solution Failed to Solve Completely at all Time Points. ............................................ 1075 An Error Occurred Inside the SOLVER Module: Invalid Material Properties ..................................... 1075 An Error Occurred While Solving Due To Insufficient Disk Space ................................................... 1076 An Error Occurred While Starting the ANSYS Solver Module ......................................................... 1076 An Internal Solution Magnitude Limit Was Exceeded. ................................................................... 1077 An Iterative Solver Was Used for this Analysis ............................................................................... 1077 At Least One Body Has Been Found to Have Only 1 Element ......................................................... 1077 Animation Does not Export Correctly .......................................................................................... 1078 Assemblies Missing Parts ............................................................................................................ 1078 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. xvii ANSYS Mechanical Application User's Guide CATIA V5 and IGES Surface Bodies ............................................................................................... 1079 Constraint Equations Were Not Properly Matched ........................................................................ 1079 Error Inertia tensor is too large .................................................................................................... 1079 Failed to Load Microsoft Office Application .................................................................................. 1079 Illogical Reaction Results ............................................................................................................. 1079 Large Deformation Effects are Active ........................................................................................... 1079 MPC Equations Were Not Built for One or More Contact Regions .................................................. 1080 One or More Contact Regions May Not Be In Initial Contact .......................................................... 1080 One or more MPC contact regions or remote boundary conditions may have conflicts ................. 1081 One or More Parts May Be Underconstrained ............................................................................... 1081 One or More Remote Boundary Conditions is Scoped to a Large Number of Elements .................. 1082 Problems Unique to Background (Asynchronous) Solutions ......................................................... 1082 Problems Using Solution ............................................................................................................. 1083 Running Norton AntiVirusTM Causes the Mechanical Application to Crash .................................... 1084 The Correctly Licensed Product Will Not Run ................................................................................ 1084 The Deformation is Large Compared to the Model Bounding Box ................................................. 1085 The Initial Time Increment May Be Too Large for This Problem ...................................................... 1085 The Joint Probe cannot Evaluate Results ...................................................................................... 1086 The License Manager Server Is Down ........................................................................................... 1086 Linux Platform - Localized Operating System ............................................................................... 1086 The Low/High Boundaries of Cyclic Symmetry ............................................................................ 1087 The Solution Combination Folder ................................................................................................ 1087 The Solver Engine was Unable to Converge ................................................................................. 1087 The Solver Has Found Conflicting DOF Constraints ...................................................................... 1088 Unable to Find Requested Modes ................................................................................................ 1089 You Must Specify Joint Conditions to all Three Rotational DOFs .................................................... 1089 Recommendations ............................................................................................................................ 1089 I. Appendices ......................................................................................................................................... 1091 A. Glossary of General Terms .............................................................................................................. 1093 B. Data Transfer Mesh Mapping .......................................................................................................... 1097 Mapping Validation ..................................................................................................................... 1105 C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis .............................................................. 1107 Supported LS-DYNA Keywords .................................................................................................... 1107 LS-DYNA General Descriptions .................................................................................................... 1133 D. Workbench Mechanical Wizard Advanced Programming Topics ...................................................... 1135 Overview .................................................................................................................................... 1135 URI Address and Path Considerations .......................................................................................... 1136 Using Strings and Languages ...................................................................................................... 1137 Guidelines for Editing XML Files ................................................................................................... 1138 About the TaskML Merge Process ................................................................................................ 1138 Using the Integrated Wizard Development Kit (WDK) ................................................................... 1139 Using IFRAME Elements .............................................................................................................. 1139 TaskML Reference ....................................................................................................................... 1140 Overview Map of TaskML ....................................................................................................... 1140 Document Element ............................................................................................................... 1141 simulation-wizard ........................................................................................................... 1141 External References ............................................................................................................... 1141 Merge ............................................................................................................................. 1141 Script .............................................................................................................................. 1142 Object Grouping ................................................................................................................... 1142 object-group .................................................................................................................. 1142 object-groups ................................................................................................................. 1143 xviii Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS Mechanical Application User's Guide object-type ..................................................................................................................... 1143 Status Definitions .................................................................................................................. 1144 status ............................................................................................................................. 1144 statuses .......................................................................................................................... 1144 Language and Text ................................................................................................................ 1145 data ................................................................................................................................ 1145 language ........................................................................................................................ 1145 string .............................................................................................................................. 1146 strings ............................................................................................................................ 1146 Tasks and Events ................................................................................................................... 1146 activate-event ................................................................................................................. 1146 task ................................................................................................................................ 1147 tasks ............................................................................................................................... 1148 update-event .................................................................................................................. 1148 Wizard Content ..................................................................................................................... 1148 body ............................................................................................................................... 1148 group ............................................................................................................................. 1149 iframe ............................................................................................................................. 1150 taskref ............................................................................................................................ 1150 Rules .................................................................................................................................... 1151 Statements ..................................................................................................................... 1151 and ........................................................................................................................... 1151 debug ...................................................................................................................... 1151 if then else stop ........................................................................................................ 1151 not ........................................................................................................................... 1152 or ............................................................................................................................. 1153 update ..................................................................................................................... 1153 Conditions ...................................................................................................................... 1153 assembly-geometry .................................................................................................. 1153 changeable-length-unit ........................................................................................... 1154 geometry-includes-sheets ......................................................................................... 1154 level ......................................................................................................................... 1154 object ....................................................................................................................... 1155 zero-thickness-sheet ................................................................................................. 1156 valid-emag-geometry ............................................................................................... 1156 enclosure-exists ........................................................................................................ 1156 Actions ........................................................................................................................... 1156 click-button .............................................................................................................. 1157 display-details-callout ............................................................................................... 1157 display-help-topic ..................................................................................................... 1158 display-outline-callout .............................................................................................. 1158 display-status-callout ................................................................................................ 1159 display-tab-callout .................................................................................................... 1159 display-task-callout ................................................................................................... 1160 display-toolbar-callout .............................................................................................. 1160 open-url ................................................................................................................... 1161 select-all-objects ....................................................................................................... 1161 select-field ................................................................................................................ 1162 select-first-object ...................................................................................................... 1163 select-first-parameter-field ........................................................................................ 1164 select-first-undefined-field ........................................................................................ 1164 select-zero-thickness-sheets ..................................................................................... 1165 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. xix ANSYS Mechanical Application User's Guide select-enclosures ...................................................................................................... 1165 send-mail ................................................................................................................. 1165 set-caption ............................................................................................................... 1166 set-icon .................................................................................................................... 1166 set-status .................................................................................................................. 1167 Scripting ............................................................................................................................... 1167 eval ................................................................................................................................ 1167 Standard Object Groups Reference .............................................................................................. 1169 Tutorials ..................................................................................................................................... 1172 Tutorial: Adding a Link ........................................................................................................... 1172 Tutorial: Creating a Custom Task ............................................................................................ 1173 Tutorial: Creating a Custom Wizard ........................................................................................ 1175 Tutorial: Adding a Web Search IFRAME ................................................................................... 1176 Completed TaskML Files ........................................................................................................ 1177 Links.xml ........................................................................................................................ 1177 Insert100psi.xml ............................................................................................................. 1178 CustomWizard.xml .......................................................................................................... 1179 Search.htm ..................................................................................................................... 1179 CustomWizardSearch.xml ............................................................................................... 1181 Wizard Development Kit (WDK) Groups ....................................................................................... 1182 WDK: Tools Group ................................................................................................................. 1182 WDK: Commands Group ........................................................................................................ 1182 WDK Tests: Actions ................................................................................................................ 1183 WDK Tests: Flags (Conditions) ................................................................................................ 1184 E. Material Models Used in Explicit Dynamics Analysis ........................................................................ 1185 Introduction ............................................................................................................................... 1185 Explicit Material Library ............................................................................................................... 1187 Density ....................................................................................................................................... 1193 Linear Elastic ............................................................................................................................... 1193 Isotropic Elasticity ................................................................................................................. 1193 Orthotropic Elasticity ............................................................................................................ 1193 Viscoelastic ........................................................................................................................... 1194 Test Data .................................................................................................................................... 1195 Hyperelasticity ............................................................................................................................ 1195 Plasticity ..................................................................................................................................... 1201 Bilinear Isotropic Hardening .................................................................................................. 1201 Multilinear Isotropic Hardening ............................................................................................. 1201 Bilinear Kinematic Hardening ................................................................................................ 1202 Multilinear Kinematic Hardening ........................................................................................... 1202 Johnson-Cook Strength ........................................................................................................ 1203 Cowper-Symonds Strength ................................................................................................... 1204 Steinberg-Guinan Strength ................................................................................................... 1205 Zerilli-Armstrong Strength .................................................................................................... 1207 Brittle/Granular ........................................................................................................................... 1208 Drucker-Prager Strength Linear ............................................................................................. 1208 Drucker-Prager Strength Stassi .............................................................................................. 1210 Drucker-Prager Strength Piecewise ....................................................................................... 1211 Johnson-Holmquist Strength Continuous .............................................................................. 1211 Johnson-Holmquist Strength Segmented .............................................................................. 1214 RHT Concrete Strength .......................................................................................................... 1216 MO Granular ......................................................................................................................... 1223 Equations of State ....................................................................................................................... 1223 xx Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. ANSYS Mechanical Application User's Guide Background .......................................................................................................................... 1224 Bulk Modulus ........................................................................................................................ 1224 Shear Modulus ...................................................................................................................... 1224 Ideal Gas EOS ........................................................................................................................ 1224 Polynomial EOS .................................................................................................................... 1225 Shock EOS Linear .................................................................................................................. 1227 Shock EOS Bilinear ................................................................................................................ 1228 JWL EOS ............................................................................................................................... 1230 Porosity ...................................................................................................................................... 1232 Porosity-Crushable Foam ...................................................................................................... 1232 Compaction EOS Linear ........................................................................................................ 1235 Compaction EOS Non-Linear ................................................................................................. 1236 P-alpha EOS .......................................................................................................................... 1238 Failure ........................................................................................................................................ 1241 Plastic Strain Failure .............................................................................................................. 1242 Principal Stress Failure ........................................................................................................... 1242 Principal Strain Failure ........................................................................................................... 1243 Stochastic Failure .................................................................................................................. 1244 Tensile Pressure Failure ......................................................................................................... 1246 Crack Softening Failure ......................................................................................................... 1246 Johnson-Cook Failure ............................................................................................................ 1248 Grady Spall Failure ................................................................................................................ 1249 Strength ..................................................................................................................................... 1250 Thermal Specific Heat ................................................................................................................. 1251 Rigid Materials ............................................................................................................................ 1251 F. Explicit Dynamics Theory Guide ...................................................................................................... 1253 Why use Explicit Dynamics? ........................................................................................................ 1253 What is Explicit Dynamics? .......................................................................................................... 1253 The Solution Strategy ............................................................................................................ 1254 Basic Formulations ................................................................................................................ 1254 Implicit Transient Dynamics ............................................................................................ 1254 Explicit Transient Dynamics ............................................................................................. 1255 Time Integration ................................................................................................................... 1256 Implicit Time Integration ................................................................................................. 1256 Explicit Time Integration ................................................................................................. 1256 Mass Scaling ................................................................................................................... 1258 Wave Propagation ................................................................................................................. 1258 Elastic Waves .................................................................................................................. 1259 Plastic Waves .................................................................................................................. 1259 Shock Waves ................................................................................................................... 1260 Reference Frame ................................................................................................................... 1261 Lagrangian and Eulerian Reference Frames ...................................................................... 1261 Eulerian (Virtual) Reference Frame in Explicit Dynamics ................................................... 1262 Post-Processing a Body with Reference Frame Euler (Virtual) ............................................ 1264 Key Concepts of Euler (Virtual) Solutions ......................................................................... 1265 Multiple Material Stress States ................................................................................... 1266 Multiple Material Transport ....................................................................................... 1268 Supported Material Properties .................................................................................. 1268 Explicit Fluid Structure Interaction (Euler-Lagrange Coupling) ................................................ 1268 Shell Coupling ................................................................................................................ 1269 Sub-cycling ..................................................................................................................... 1270 Analysis Settings ......................................................................................................................... 1270 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. xxi ANSYS Mechanical Application User's Guide Step Controls ........................................................................................................................ 1270 Damping Controls ................................................................................................................. 1271 Solver Controls ..................................................................................................................... 1276 Erosion Controls ................................................................................................................... 1283 References .................................................................................................................................. 1284 Index ...................................................................................................................................................... 1287 xxii Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Approach Use the Mechanical application to perform various types of structural, thermal, and electromagnetic analyses. Within the Mechanical application, you define your model's environmental loading conditions, solve the analysis, and review results in various formats depending on the analysis type. The following topics are covered in this section. Overall Steps to Using the Mechanical Application Analysis Types Special Analysis Topics Tutorials Wizards Overall Steps to Using the Mechanical Application This section describes the overall workflow involved when performing any analysis in the Mechanical application. The following workflow steps are described: Create Analysis System Define Engineering Data Attach Geometry Define Part Behavior Define Connections Apply Mesh Controls and Preview Mesh Establish Analysis Settings Define Initial Conditions Apply Loads and Supports Solve Review Results Create Report (optional) Create Analysis System There are several types of analyses you can perform in the Mechanical application. For example, if natural frequencies and mode shapes are to be calculated, you would choose a modal analysis. Each analysis type is represented by an analysis system that includes the individual components of the analysis such as the associated geometry and model properties. Most analyses are represented by one independent analysis system. However, an analysis with data transfer can exist where results of one analysis are used as the basis for another analysis. In this case, an analysis system is defined for each analysis type, where components of each system can share data. An example of an analysis with data transfer is a response spectrum analysis, where a modal analysis is a prerequisite. • To create an analysis system, expand the Standard Analyses folder in the Toolbox and drag an analysis type object “template” onto the Project Schematic. The analysis system is displayed as a vertical array of cells (schematic) where each cell represents a component of the analysis system. Address each cell by right-clicking on the cell and choosing an editing option. • To create an analysis system with data transfer to be added to an existing system, drag the object template representing the upstream analysis directly onto the existing system schematic such that red Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1 Approach boxes enclose cells that will share data between the systems. After you up-click, the two schematics are displayed, including an interconnecting link and a numerical designation as to which cells share data. See Working Through an Analysis System for more information. Unit System Behavior When you start the Mechanical application, the unit system defaults to the same system used in the previous session. You can change this unit system, but subsequent Mechanical editors that you start while the first one is open, will default to the unit system from the initial session. In the event that you change a unit system, numerical values are converted accordingly but there is no change in physical quantity. Define Engineering Data A part’s response is determined by the material properties assigned to the part. • Depending on the application, material properties can be linear or nonlinear, as well as temperaturedependent. • Linear material properties can be constant or temperature-dependent, and isotropic or orthotropic. • Nonlinear material properties are usually tabular data, such as plasticity data (stress-strain curves for different hardening laws), hyperelastic material data. • To define temperature-dependent material properties, you must input data to define a property-versustemperature graph. • Although you can define material properties separately for each analysis, you have the option of adding your materials to a material library by using the Engineering Data workspace. This enables quick access to and re-use of material data in multiple analyses. • For all orthotropic material properties, by default, the Global Coordinate System is used when you apply properties to a part in the Mechanical application. If desired, you can also apply a local coordinate system to the part. To manage materials, right-click on the Engineering Data cell in the analysis system schematic and choose Edit .... See "Basics of Engineering Data" for more information. Attach Geometry There are no geometry creation tools in the Mechanical application so geometry must be attached to the Mechanical application. You can create the geometry for attaching in the Mechanical application in either of the following sources: • From within Workbench using DesignModeler. See the DesignModeler Help for details on the use of the various creation tools available. • From a CAD system supported by Workbench or one that can export a file that is supported by ANSYS Workbench. See the CAD Systems section for a complete list of the supported systems. Before attaching the geometry from either of these sources, you can specify several options that determine the characteristics of the geometry you choose to import. These options are: solid bodies, surface bodies, line bodies, parameters, attributes, named selections, material properties; Analysis Type (2D or 2 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Overall Steps to Using the Mechanical Application 3D), allowing CAD associativity, importing coordinate systems (Import Work Points are only available in the DesignModeler application), saving updated CAD file in reader mode, “smart” refreshing of models with unmodified components, and allowing parts of mixed dimension to be imported as assembly components that have parts of different dimensions. The availability of these options varies across the supported CAD systems. See the Geometry Preferences section for details. Related Procedures Procedure Specifying geometry options Condition Optional task that can be done before attaching geometry. Procedural Steps 1. In an analysis system schematic, perform either of the following: • Right-click on the Geometry cell and choose Properties OR • 2. Attaching DesignModeler geometry to the Mechanical application Check boxes to specify Default Geometry Options and Advanced Geometry Defaults. DesignModeler is running in an analysis system. Double-click on the Model cell in the same analysis system schematic. The Mechanical application opens and displays the geometry. DesignModeler is not running. Geometry is stored in an agdb file. 1. Select the Geometry cell in an analysis system schematic. 2. Browse to the agdb file from the following access points: • Attaching CAD geometry to the Mechanical application Select the Geometry cell in the schematic for a standard analysis, then from the Workspace toolbar drop down menu, choose any option that includes Properties or Components. CAD system is running. CAD system is not running. Geometry is stored in a native CAD system file, or in a CAD “neutral” file such as Parasolid or IGES. Right-click on the Geometry cell in the Project Schematic, Import Geometry and choose Browse. 3. Double-click on the Model cell in the schematic. The Mechanical application opens and displays the geometry. 1. Select the Geometry cell in an analysis system schematic. 2. Right-click on the Geometry cell listed to select geometry for import. 3. If required, set geometry options for import into the Mechanical application by highlighting the Geometry cell and choosing settings under Preferences in the Properties Panel. 4. Double-click on the Model cell in the same analysis system schematic. The Mechanical application opens and displays the geometry. 1. Select the Geometry cell in an analysis system schematic. 2. Browse to the CAD file from the following access points: • Right-click on the Geometry cell in the Project Schematic and choose Import Geometry. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 3 Approach Procedure Condition Procedural Steps 3. Double-click on the Model cell in the Project Schematic. The Mechanical application opens and displays the geometry. CAD Interface Terminology The CAD interfaces can be run in either plug-in mode or in reader mode. • Attaching geometry in plug-in mode: requires that the CAD system be running. • Attaching geometry in reader mode: does not require that the CAD system be running. Updating Geometry from Within the Mechanical Application You can update all geometry by choosing the Refresh Geometry context menu option, accessible by right-clicking on the Geometry tree object or anywhere in the Geometry window. • Comparing Parts on Update • Selective Update • Smart CAD Update Compare Parts on Update When you choose Refresh Geometry, if no changes to the body are detected, you can configure the process such that a re-mesh of the body is not required by setting the following: • Under Tools> Options, in the Common Settings - Geometry Import category, set Compare Parts on Update to Associative or Non-Associative. This preference is used to compare the bodies of parts in the model on update and mark only those that have topological differences as being modified. Those that remain the same will be identified as unchanged and remeshing will not be necessary for that body (assuming the body was meshed prior to the refresh action). If all bodies under a part are unchanged the entire part will not undergo remeshing after refresh. This will reduce the refresh/mesh cycle time in most cases. For detailed information, see Compare Parts on Update in the CAD Integration section of the product help. When accessing the ANSYS Workbench Help from the Help menu, click the Contents tab and open the CAD Integration folder in the hierarchical tree to access the CAD Integration section. Note The Compare Parts on Update feature is not supported for line bodies. Selective Update You can selectively update individual parts by right-clicking on an individual part (or after multiple parts are selected) and choosing Update Selected Parts: • 4 Update: Use Geometry Parameter Values synchronizes the Mechanical application model to the CAD model. This will read the latest geometry and process other data (parameters, attributes, etc.) based on the current user preferences for that model. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Overall Steps to Using the Mechanical Application Note If you change either the number of turns or the thickness properties associated with a body, these changes are not updated to the CAD model when you choose Update: Use Geometry Parameter Values. The selective update feature is applied to selected part(s) only and it does not import new parts added in the CAD system following the original import or last complete update. Parameter values for the assembly are always updated. In addition, this feature is not a tool for removing parts from the Mechanical application tree, however; it will remove parts which have been selected for update in WB, but that no longer exist in the CAD model if an update is successful (if at least one valid part is updated). The selective update feature is supported by the associative geometry interfaces for DesignModeler, Autodesk Inventor, CATIA V5, Creo Elements/Direct Modeling, Creo Parametric (formerly Pro/ENGINEER), Solid Edge, NX, and SolidWorks. Executing the Selective Update on any unsupported interface will complete a full update of the model. Smart CAD Update • In the Geometry Preferences, enable Smart CAD Update. Note that Geometry Preferences are supported by a limited number of CAD packages. See the Project Schematic Advanced Geometry Options table for details. Maintaining Associativity with Geometry Updates in DesignModeler Associativity that you apply to geometry originating from DesignModeler is maintained in the Mechanical and Meshing applications when the geometry is updated despite any part groupings that you may subsequently change in DesignModeler. Types of associativity that you can apply include contact regions, mesh connections, loads, and supports. For example, consider the following scenario: 1. A model is created in DesignModeler and is comprised of six independent parts with one body per part. 2. The model is attached to Mechanical where loads and supports are applied to selected geometry. 3. In DesignModeler, the model is re-grouped into two multibody parts with each part including three bodies. 4. The geometry is updated in Mechanical. The loads and supports remain applied to the same selected geometry. Note This feature does not hold true for instanced parts in DesignModeler. The associativity is maintained only with geometry attached from DesignModeler and Mechanical systems created in release 13.0 or later. To ensure that the data necessary for retaining associativity is present in legacy dsdb/wbpj databases, you should perform the following: 1. Open the Mechanical session and open the DesignModeler session. This will ensure that both the Mechanical and DesignModeler files are migrated to the current version of the software. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 5 Approach 2. Update the geometry model without making any changes to the model. This will ensure that the new data necessary for associativity is transferred from the migrated DesignModeler file into the migrated Mechanical file. 3. You can now modify and update the geometry as necessary. Define Part Behavior After attaching geometry, you can access settings related to part behavior by right-clicking on the Model cell in the analysis system schematic and choosing Edit .... The Mechanical application opens with the environment representing the analysis system displayed under the Model object in the tree. An Analysis Settings object is added to the tree. See the Establish Analysis Settings (p. 9) overall step for details. An Initial Condition object may also be added. See the Define Initial Conditions (p. 12) overall step for details. The Mechanical application uses the specific analysis system as a basis for filtering or making available only components such as loads, supports and results that are compatible with the analysis. For example, a Static Structural analysis type will allow only structural loads and results to be available. Presented below are various options provided in the Details view for parts and bodies following import. Stiffness Behavior In addition to making changes to the material properties of a part, you may designate a part's Stiffness Behavior as being flexible, rigid, or as a gasket. • Setting a part’s behavior as rigid essentially reduces the representation of the part to a single point mass thus significantly reducing the solution time. • A rigid part will need only data about the density of the material to calculate mass characteristics. Note that if density is temperature dependent, density will be evaluated at the reference temperature. For contact conditions, specify Young’s modulus. • Flexible and rigid behaviors are applicable only to static structural, transient structural, rigid dynamics, explicit dynamics, and modal analyses. Gasket behavior is applicable only to static structural analyses. Flexible is the default Stiffness Behavior. To change, simply select Rigid or Gasket from the Stiffness Behavior drop-down menu. Also see the Rigid Bodies (p. 331) section or the Gasket Bodies section. Note Rigid behavior is not available for the SAMCEF solver. Coordinate Systems The Coordinate Systems object and its child object, Global Coordinate System, is automatically placed in the tree with a default location of 0, 0, 0, when a model is imported. For solid parts and bodies: by default, a part and any associated bodies use the Global Coordinate System. If desired, you can apply a apply a local coordinate system to the part or body. When a local coordinate system is assigned to a Part, by default, the bodies also assume this coordinate system but you may modify the system on the bodies individually as desired. 6 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Overall Steps to Using the Mechanical Application For surface bodies, solid shell bodies, and line bodies: by default, these types of geometries generate coordinates systems on a per element type basis. It is necessary for you to create a local coordinate system and associated it with the parts and/or bodies using the Coordinate System setting in the Details view for the part/body if you wish to orient those elements in a specific direction. Reference Temperature The default reference temperature is taken from the environment (By Environment), which occurs when solving. This necessarily means that the reference temperature can change for different solutions. The reference temperature can also be specified for a body and will be constant for each solution (By Body). Selecting By Body will cause the Reference Temperature Value field to specify the reference temperature for the body. It is important to recognize that any value set By Body will only set the reference temperature of the body and not actually cause the body to exist at that temperature (unlike the Environment Temperature entry on an environment object, which does set the body's temperature). Note Selecting By Environment can cause the body to exist at that temperature during the analysis but selecting By Body will only ever effect reference temperature. So if the environment temperature and the body have a different specification, thermal expansion effects can occur even if no other thermal loads are applied. Note If the material density is temperature dependent, the mass that is displayed in the Details view will either be computed at the body temperature, or at 22°C. Therefore, the mass computed during solution can be different from the value shown, if the Reference Temperature is the Environment. Note When nonlinear material effects are turned off, values for thermal conductivity, specific heat, and thermal expansion are retrieved at the reference temperature of the body when creating the ANSYS solver input. Reference Frame The Reference Frame determines the analysis treatment perspective of the body for an Explicit Dynamics analysis. The Reference Frame property is available for solid bodies when an Explicit Dynamics system is part of the solution. The valid values are Langrangian (default) and Eulerian (Virtual). Eulerian is not a valid selection if Stiffness Behavior is set to Rigid. Material Property Assignment Once you have attached your geometry, you can choose a material for the simulation. When you select a part in the tree outline, the Assignment entry under Material in the Details view lists a default material for the part. You can edit material properties in the Engineering Data workspace. Nonlinear Material Effects You can also choose to ignore any nonlinear effects from the material properties. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 7 Approach • By default the program will use all applicable material properties including nonlinear properties such as stress-strain curve data. • Setting Nonlinear Effects to No will ignore any nonlinear properties only for that part. • This option will allow you to assign the same material to two different parts but treat one of the parts as linear. • This option is applicable only for static structural, transient structural, steady state thermal and transient thermal analyses. Thermal Strain Effects For structural analyses, you can choose to have Workbench calculate a Thermal Strain result by setting Thermal Strain Effects to Yes. Choosing this option enables the coefficient of thermal expansion to be sent to the solver. Cross Section When a line body is imported into the Mechanical application, the Details view displays the Cross Section field and associated cross section data. These read-only fields display the name and data assigned to the geometry in DesignModeler or the supported CAD system, if one was defined. See Line Bodies (p. 329) for further information. Model Dimensions When you attach your geometry or model, the model dimensions display in the Details View (p. 274) in the Bounding Box sections of the Geometry or Part objects. Dimensions have the following characteristics: • Units are created in your CAD system. • ACIS and CATIA model units may be set. • Other geometry units are automatically detected and set. • Assemblies must have all parts dimensioned in the same units. Define Connections Once you have addressed the material properties and part behavior of your model, you may need to apply connections to the bodies in the model so that they are connected as a unit in sustaining the applied loads for analysis. Available connection features are: • Contacts: defines where two bodies are in contact or a user manually defines contact between two bodies. • Joints: a contact condition in the application that is defined by a junction where bodies are joined together that has rotational and translational degrees of freedom. • Mesh Connections: used to join the meshes of topologically disconnected surface bodies that reside in different parts. • Springs: defines as an elastic element that connects two bodies or a body to “ground” that maintains its original shape once the specified forces are removed. • Beam Connections: used to establish body to body or body to ground connections. • End Releases are used to release degrees of freedoms at a vertex shared by two or more edges of one or more line bodies. 8 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Overall Steps to Using the Mechanical Application • Spot Welds: connects individual surface body parts together to form surface body model assemblies. Given the complex nature of bodies coming into contact with one another, especially if the bodies are in motion, it is recommended that you review the Connections section of the documentation. Apply Mesh Controls and Preview Mesh Meshing is the process in which your geometry is spatially discretized into elements and nodes. This mesh along with material properties is used to mathematically represent the stiffness and mass distribution of your structure. Your model is automatically meshed at solve time. The default element size is determined based on a number of factors including the overall model size, the proximity of other topologies, body curvature, and the complexity of the feature. If necessary, the fineness of the mesh is adjusted up to four times (eight times for an assembly) to achieve a successful mesh. If desired, you can preview the mesh before solving. Mesh controls are available to assist you in fine tuning the mesh to your analysis. Please refer to the Meshing Help for further details. To preview the mesh in the Mechanical Application: See the Previewing Surface Mesh section. To apply global mesh settings in the Mechanical Application: See the Global Mesh Controls section. To apply mesh control tools on specific geometry in the Mechanical Application: See the Local Mesh Controls section. Establish Analysis Settings Each analysis type includes a group of analysis settings that allow you to define various solution options customized to the specific analysis type, such as large deflection for a stress analysis. Refer to the specific analysis types section for the customized options presented under “Preparing the Analysis”. Default values are included for all settings. You can accept these default values or change them as applicable. Some procedures below include animated presentations. Please view online if you are reading the PDF version of the help. Interface names and other components shown in the demos may differ from those in the released product. To verify/change analysis settings in the Mechanical application: 1. Highlight the Analysis Settings object in the tree. This object was inserted automatically when you established a new analysis in the Create Analysis System (p. 1) overall step. 2. Verify or change settings in the Details view of the Analysis Settings object. These settings include default values that are specific to the analysis type. You can accept or change these defaults. If your analysis involves the use of steps, refer to the procedures presented below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 9 Approach To create multiple steps (applies to structural static, transient structural, rigid dynamics, steady-state thermal, transient thermal, magnetostatic, and electric analyses): You can create multiple steps using any one of the following methods: 1. Highlight the Analysis Settings object in the tree. Modify the Number of Steps field in the Details view. Each additional Step has a default Step End Time that is one second more than the previous step. These step end times can be modified as needed in the Details view. You can also add more steps simply by adding additional step End Time values in the Tabular Data window. The following demonstration illustrates adding steps by modifying the Number of Steps field in the Details view. Or 2. Highlight the Analysis Settings object in the tree. Begin adding each step's end time values for the various steps to the Tabular Data window. You can enter the data in any order but the step end time points will be sorted into ascending order. The time span between the consecutive step end times will form a step. You can also select a row(s) corresponding to a step end time, click the right mouse button and choose Delete Rows from the context menu to delete the corresponding steps. The following demonstration illustrates adding steps directly in the Tabular Data window. Or 3. Highlight the Analysis Settings object in the tree. Choose a time point in the Graph window. This will make the corresponding step active. Click the right mouse button and choose Insert Step from the context menu to split the existing step into two steps, or choose Delete Step to delete the step. The following demonstration illustrates inserting a step in the Graph window, changing the End Time in the Tabular Data window, deleting a step in the Graph window, and deleting a step in the Tabular Data window. Specifying Analysis Settings for Multiple Steps 1. Create multiple steps following the procedure ”To create multiple steps” above. 10 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Overall Steps to Using the Mechanical Application 2. Most Step Controls, Nonlinear Controls, and Output Controls fields in the Details view of Analysis Settings are “step aware”, that is, these settings can be different for each step. Refer to the table in Analysis Settings for Most Analysis Types (p. 499) to determine which specific controls are step aware (designated as footnote 2 in the table). Activate a particular step by selecting a time value in the Graph window or the Step bar displayed below the chart in the Graph window. The Step Controls grouping in the Details view indicates the active Step ID and corresponding Step End Time. The following demonstration illustrates turning on the legend in the Graph window, entering analysis settings for a step, and entering different analysis settings for another step. If you want to specify the same analysis setting(s) to several steps, you can select all the steps of interest as follows and change the analysis settings details. • To change analysis settings for a subset of all of the steps: – From the Tabular Data window: 1. Highlight the Analysis Settings object. 2. Highlight steps in the Tabular Data window using either of the following standard windowing techniques: → Ctrl key to highlight individual steps. → Shift key to highlight a continuous group of steps. – 3. Click the right mouse button in the window and choose Select All Highlighted Steps from the context menu. 4. Specify the analysis settings as needed. These settings will apply to all selected steps. From the Graph window: 1. Highlight the Analysis Settings object. 2. Highlight steps in the Graph window using either of the following standard windowing techniques: → Ctrl key to highlight individual steps. → Shift key to highlight a continuous group of steps. 3. • Specify the analysis settings as needed. These settings will apply to all selected steps. To specify analysis settings for all the steps: 1. Click the right mouse button in either window and choose Select All Steps. 2. Specify the analysis settings as needed. These settings will apply to all selected steps. The following demonstration illustrates multiple step selection using the bar in the Graph window, entering analysis settings for all selected steps, selecting only highlighted steps in the Tabular Data window, and selecting all steps. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 11 Approach The Worksheet for the Analysis Settings object provides a single display of pertinent settings in the Details view for all steps. Details of various analysis settings are discussed in Analysis Settings (p. 499). Define Initial Conditions This step is based upon the selected type analysis. Workbench provides you with the ability to begin your analysis with an initial condition, a link to an existing solved or associated environment, or an initial temperature. For the following analysis types, a tree object is automatically generated allowing you to define specifications. For additional information, please see the individual analysis types section. Analysis Type Tree Object Description Transient Structural Initial Conditions folder A transient structural analysis is at rest, by default. However, you can define velocity as an initial condition by inserting a Velocity object under the Initial Conditions folder. Explicit Dynamics Initial Conditions folder: Because an explicit dynamics analysis is better suited for short duration events, preceding it with an implicit analysis may produce a more efficient simulation especially for cases in which a generally slower (or rate-independent) phenomenon is followed by a much faster event, such as the collision of a pressurized container. For an Explicit Dynamics system, the Initial Conditions folder includes a Pre-Stress object to control the transfer of data from an implicit static or transient structural analysis to the explicit dynamics analysis. Transferable data include the displacements, or the more complete Material State (displacements, velocities, stresses, strains, and temperature). PreStress object See Recommended Guidelines When Using Pre-Stress With Explicit Dynamics (p. 55) for more information. 12 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Overall Steps to Using the Mechanical Application Analysis Type Tree Object Description An explicit dynamics analysis is at rest by default. However, for both Explicit Dynamics and Explicit Dynamics (LS-DYNA Export) systems, you can define velocity or angular velocity as initial conditions by inserting a Velocity object or Angular Velocity object under the Initial Conditions folder. Modal Pre-Stress object A modal analysis can use the stress results from a static structural analysis to account for stress-stiffening effect. See the Modal Analysis section for details. Linear Buckling Pre-Stress object A linear buckling analysis must use the stress-stiffening effects of a static structural analysis. See the Linear Buckling Analysis section for details. Random Vibration, Response Spectrum, or Harmonic (MSUP) linked Modal object A random vibration, response spectrum, or harmonic (MSUP) linked analysis must use the mode shapes derived in a modal analysis. Steady-State Thermal Initial Temperature object For a steady-state thermal analysis, you have the ability to specify an initial temperature. Transient Thermal Initial Temperature object For a transient thermal analysis, the initial temperature distribution should be specified. Note Temperatures from a steady-state thermal or transient thermal analysis can be applied to a static structural or transient structural analysis as a Thermal Condition load. Depending upon the analysis type an object is automatically added to the tree. To define an initial condition in the Mechanical application: • For a Transient Structural analysis, use the Initial Conditions object to insert Velocity. For an Explicit Dynamics analysis, use the Initial Conditions object to insert Velocity, Angular Velocity. These values can be scoped to specific parts of the geometry. • For a Modal, Linear Buckling, or Explicit Dynamics analysis, use the Details view of the Pre-Stress object to define the associated Pre-Stress Environment. For an Explicit Dynamics analysis, use the Details view of this object to select either Material State (displacements, velocities, strains and stresses) or Displacements only modes, as well as the analysis time from the implicit analysis which to obtain the initial condition. For Displacements only, a Time Step Factor may be specified to convert nodal DOF displacements in the implicit solution into constant velocities for the explicit analysis according to the following expression: Velocity = Implicit displacement/(Initial explicit time step x time step factor) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 13 Approach Note The Displacements only mode is applicable only to results from a linear, static structural analysis. • For a Random Vibration or Response Spectrum analysis, you must point to a modal analysis using the drop-down list of the Modal Environment field in the Details view. • For the Steady-State and Transient Thermal analyses, use the Details of the Initial Temperature object to scope the initial temperature value. For a Transient Thermal analysis that has a non-uniform temperature, you need to define an associated Initial Temperature Environment. Apply Loads and Supports You apply loads and support types based on the type of analysis. For example, a stress analysis may involve pressures and forces for loads, and displacements for supports, while a thermal analysis may involve convections and temperatures. Loads applied to static structural, transient structural, rigid dynamics, steady-state thermal, transient thermal, magnetostatic, electric, and thermal-electric analyses default to either step-applied or ramped. That is, the values applied at the first substep stay constant for the rest of the analysis or they increase gradually at each substep. Load Load Full value applied Substep Load step at first substep 1 1 Final load value 2 2 Time (a) Stepped loads Time (b) Ramped loads You can edit the table of load vs. time and modify this behavior as needed. By default you have one step. However you may introduce multiple steps at time points where you want to change the analysis settings such as the time step size or when you want to activate or deactivate a load. An example is to delete a specified displacement at a point along the time history. You do not need multiple steps simply to define a variation of load with respect to time. You can use tables or functions to define such variation within a single step. You need steps only if you want to guide the analysis settings or boundary conditions at specific time points. When you add loads or supports in a static or transient analysis, the Tabular Data and Graph windows appear. You can enter the load history, that is, Time vs Load tabular data in the tabular data grid. Another option is to apply loads as functions of time. In this case you will enter the equation of how the 14 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Overall Steps to Using the Mechanical Application load varies with respect to time. The procedures for applying tabular or function loads are outlined under the Specifying Load Values (p. 621) section. Note • You can also import or export load histories from or to any pre-existing libraries. • If you have multiple steps in your analysis, the end times of each of these steps will always appear in the load history table. However you need not necessarily enter data for these time points. These time points are always displayed so that you can activate or deactivate the load over each of the steps. Similarly the value at time = 0 is also always displayed. • If you did not enter data at a time point then the value will be either a.) a linearly interpolated value if the load is a tabular load or b.) an exact value determined from the function that defines the load. An “=” sign is appended to such interpolated data so you can differentiate between the data that you entered and the data calculated by the program as shown in the example below. Here the user entered data at Time = 0 and Time = 5. The value at Time = 1e-3, the end time of step 1, is interpolated. To apply loads or supports in the Mechanical Application: See the Applying Boundary Conditions (p. 551) section. Solve This step initiates the solution process. The solution could be carried out on your local machine or on a remote machine such as a powerful server you might have access to. Based on the analysis type, the following solvers are available in Mechanical: • Mechanical ANSYS Parametric Design Language (MAPDL) Solver. • ANSYS Rigid Dynamics Solver: only available for Rigid Dynamics Analysis. • LS-DYNA Solver: only available for Explicit Dynamics analysis. • Explicit Dynamics Solver (AUTODYN): only available for Explicit Dynamics analysis. • Samcef Solver: only available for Static Structural and Modal analyses. Since nonlinear or transient solutions can take significant time to complete, a status bar is provided that indicates the overall progress of solution. More detailed information on solution status can be obtained from the Solution Information object which is automatically inserted under the Solution folder for all analyses. You can use the Remote Solve Manager (RSM) to perform solutions on a remote machine. Once the solution is completed the results will be brought back to the local machine for postprocessing. Refer to the Solve Modes and Recommended Usage (p. 754) section for more details. The overall solution progress is indicated by a status bar. In addition you can use the Solution Information object which is inserted automatically under the Solution folder. This object allows you to i) view Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 15 Approach the actual output from the solver, ii) graphically monitor items such as convergence criteria for nonlinear problems and iii) diagnose possible reasons for convergence difficulties by plotting Newton-Raphson residuals. Additionally you can also monitor some result items such as displacement or temperature at a vertex or contact region’s behavior as the solution progresses. Solve References for the Mechanical Application See the Solving Overview (p. 751) section for details on the above and other topics related to solving. Review Results The analysis type determines the results available for you to examine after solution. For example, in a structural analysis, you may be interested in equivalent stress results or maximum shear results, while in a thermal analysis, you may be interested in temperature or total heat flux. The Results in the Mechanical Application (p. 634) section lists various results available to you for postprocessing. To add result objects in the Mechanical application: 1. Highlight a Solution object in the tree. 2. Select the appropriate result from the Solution context toolbar or use the right-mouse click option. To review results in the Mechanical application: 1. Click on a result object in the tree. 2. After the solution has been calculated, you can review and interpret the results in the following ways: • Contour results - Displays a contour plot of a result such as stress over geometry. • Vector Plots - Displays certain results in the form of vectors (arrows). • Probes - Displays a result at a single time point, or as a variation over time, using a graph and a table. • Charts - Displays different results over time, or displays one result against another result, for example, force vs. displacement. • Animation - Animates the variation of results over geometry including the deformation of the structure. • Stress Tool - to evaluate a design using various failure theories. • Fatigue Tool - to perform advanced life prediction calculations. • Contact Tool - to review contact region behavior in complex assemblies. • Beam Tool - to evaluate stresses in line body representations. Note Displacements of rigid bodies are shown correctly in transient structural and rigid dynamics analyses. If rigid bodies are used in other analyses such as static structural or modal analyses, the results are correct, but the graphics will not show the deformed configuration of the rigid bodies in either the result plots or animation. See the Results in the Mechanical Application (p. 634) section for more references on results. 16 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Create Report (optional) Workbench includes a provision for automatically creating a report based on your entire analysis. The documents generated by the report are in HTML. The report generates documents containing content and structure and uses an external Cascading Style Sheet (CSS) to provide virtually all of the formatting information. Report References for the Mechanical Application See the Report Preview (p. 864) section. Analysis Types You can perform several types of analyses in the Mechanical application using pre-configured analysis systems (see Create Analysis System (p. 1)). For doing more advanced analysis you can use Commands objects in the Mechanical interface. This will allow you to enter the Mechanical APDL application commands in the Mechanical application to perform the analysis. If you are familiar with the Mechanical APDL application commands, you will have the capability of performing analyses and techniques that are beyond those available using the analysis systems in Workbench. This section describes the following analysis types that you can perform in the Mechanical interface. Available features can differ from one solver to another. Each analysis section assumes that you are familiar with the nature and background of the analysis type as well as the information presented in the Overall Steps to Using the Mechanical Application (p. 1) section. Design Assessment Analysis Eigen Response Analysis Electric Analysis Explicit Dynamics Analysis Harmonic Analysis Magnetostatic Analysis Random Vibration Analysis Response Spectrum Analysis Static Structural Analysis Steady-State Thermal Analysis Thermal-Electric Analysis Transient Structural and Rigid Dynamics Analyses Transient Thermal Analysis Design Assessment Analysis Introduction The Design Assessment system enables the selection and combination of upstream results and the ability to optionally further assess results with customizable scripts. Furthermore it enables the user to associate attributes, which may be geometry linked but not necessarily a property of the geometry, to the analysis via customizable items that can be added in the tree. Finally, custom results can be defined from the script and presented in the Design Assessment system to enable complete integration of a post finite element analysis process. The scripting language supported is python based. The location of the script and the available properties for the additional attributes and results can be defined via an XML file which can be easily created in any text editor and then selected by right clicking on the Setup cell on the system. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 17 Approach The Design Assessment system must be connected downstream of another analysis system (the allowed system types are listed below in Preparing the Analysis). An Assessment Type must be set for each Design Assessment system. Predefined scripts are supplied to interface with the BEAMCHECK and FATJACK products. Points to Remember • The BEAMCHECK and FATJACK assessment types are not available on Linux. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: Because a design assessment analysis is a postprocessing analysis, one or more upstream analysis systems (at this time, limited to Static Structural, Transient Structural, Harmonic Response, Modal, Response Spectrum, Random Vibration, and Explicit Dynamics systems) are a required prerequisite. The requirement then is for two or more analysis systems, including a Design Assessment analysis system, that share resources, geometry, and model data. From the Toolbox, drag one of the allowed system templates to the Project Schematic. Then, drag a Design Assessment template directly onto the first template, making sure that all cells down to and including the Model cell are shared. If multiple upstream systems are included, all must share the cells above and including the Model cell. Define Engineering Data Basic general information about this topic ... for this analysis type: There are no specific considerations for a design assessment analysis. Attach Geometry Basic general information about this topic ... for this analysis type: There are no specific considerations for a design assessment analysis. Define Part Behavior Basic general information about this topic ... for this analysis type: There are no specific considerations for a design assessment analysis. 18 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Define Connections Basic general information about this topic ... for this analysis type: There are no specific considerations for a design assessment analysis. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: There are no specific considerations for a design assessment analysis. Establish Analysis Settings Basic general information about this topic ... for this analysis type: There are no specific considerations for a design assessment analysis. Define Initial Conditions Basic general information about this topic ... for this analysis type: You must point to a structure analysis in the Initial Condition environment field. Apply Loads and Supports Basic general information about this topic ... for this analysis type: There are no specific considerations for a design assessment analysis. Solve Basic general information about this topic ... for this analysis type: Solution Information continuously updates any listing output from the Design Assessment log files and provides valuable information on the behavior of the structure during the analysis. The file solve.out is provided for log information from any external process your analysis may use. Solve script and Evaluate script log files are produced by the solve and evaluate Python processes respectively. Select the log information that you want to display from the Solution Output drop down. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 19 Approach Review Results Basic general information about this topic ... for this analysis type: The following Mechanical results are available when Solution Combination is enabled for the design assessment analysis: • Stress Tool • Fatigue Tool • Contact Tool (for the following contact results: Frictional Stress, Penetration, Pressure, and Sliding Distance) • Beam Tool • Beam Results • Stresses • Elastic Strains • Deformations The results available for insertion will depend on the types of the systems selected for combination and the setting of the Results Availability field in the Details panel of the Design Assessment Solution object in the tree. In addition, DA Result objects will be available if they are enabled for the design assessment analysis. Note Not all of the standard right click menu options are available for DA Result objects. Cut, Copy, Paste, Copy to Clipboard, Duplicate, Rename, and Export are removed. Eigen Response Analysis The following topics are covered in this section: Linear Buckling Analysis Modal Analysis Applying Pre-Stress Effects Linear Buckling Analysis Introduction Linear buckling (also called as Eigenvalue buckling) analysis predicts the theoretical buckling strength of an ideal elastic structure. This method corresponds to the textbook approach to elastic buckling analysis: for instance, an eigenvalue buckling analysis of a column will match the classical Euler solution. However, imperfections and nonlinearities prevent most real-world structures from achieving their theoretical elastic buckling strength. Thus, linear buckling analysis often yields quick but non-conservative results. 20 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types F F Snap-through buckling Bifurcation point Limit load (from nonlinear buckling) u (a) u (b) (a) Nonlinear load-deflection curve, (b) Linear (Eigenvalue) buckling curve A more accurate approach to predicting instability is to perform a nonlinear buckling analysis. This involves a static structural analysis with large deflection effects turned on. A gradually increasing load is applied in this analysis to seek the load level at which your structure becomes unstable. Using the nonlinear technique, your model can include features such as initial imperfections, plastic behavior, gaps, and large-deflection response. In addition, using deflection-controlled loading, you can even track the post-buckled performance of your structure (which can be useful in cases where the structure buckles into a stable configuration, such as "snap-through" buckling of a shallow dome). Points to Remember • Linear buckling analysis must be preceded by a static structural analysis. • The results calculated by the linear buckling analysis are buckling load factors that scale the loads applied in the static structural analysis. Thus for example if you applied a 10 N compressive load on a structure in the static analysis and if the linear buckling analysis calculates a load factor of 1500, then the predicted buckling load is 1500x10 = 15000 N. Because of this it is typical to apply unit loads in the static analysis that precedes the buckling analysis. • The buckling load factor is to be applied to all the loads used in the static analysis. • A structure can have infinitely many buckling load factors. Each load factor is associated with a different instability pattern. Typically the lowest load factor is of interest. • Note that the load factors represent scaling factors for all loads. If certain loads are constant (for example, self-weight gravity loads) while other loads are variable (for example, externally applied loads), you need to take special steps to ensure accurate results. One strategy that you can use to achieve this end is to iterate on the linear buckling solution, adjusting the variable loads until the load factor becomes 1.0 (or nearly 1.0, within some convergence tolerance). Consider, for example, a pole having a self-weight W0, which supports an externally-applied load, A. To determine the limiting value of A in a linear buckling analysis, you could solve repetitively, using different values of A, until by iteration you find a load factor acceptably close to 1.0. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 21 Approach • You can apply a nonzero constraint in the static analysis. The load factors calculated in the buckling analysis should also be applied to these nonzero constraint values. However, the buckling mode shape associated with this load will show the constraint to have zero value. • Buckling mode shape displays are helpful in understanding how a part or an assembly deforms when buckling, but do not represent actual displacements. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: From the Toolbox, drag the Linear Buckling template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: • Young's modulus (or stiffness in some form) must be defined. • Material properties can be linear, isotropic or orthotropic, and constant or temperaturedependent. • Nonlinear properties, if any, are ignored. Attach Geometry Basic general information about this topic ... for this analysis type: There are no specific considerations for a linear buckling analysis. Define Part Behavior Basic general information about this topic ... for this analysis type: There are no specific considerations for a linear buckling analysis. 22 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Define Connections Basic general information about this topic ... for this analysis type: Springs are taken into account if they are present in the static analysis. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: There are no considerations specifically for a linear buckling analysis. Establish Analysis Settings Basic general information about this topic ... for this analysis type: For linear buckling analysis the basic controls are: Options for Modal, Harmonic, Linear Buckling, Random Vibration, and Response Spectrum Analyses (p. 538): Number of Modes: You need to specify the number of buckling load factors and corresponding buckling mode shapes of interest. Typically the first (lowest) buckling load factor is of interest. Output Controls (p. 545): By default only buckling load factors and corresponding buckling mode shapes are calculated. You can request Stress and Strain results to be calculated but note that “stress” results only show the relative distribution of stress in the structure and are not real stress values. In Analysis Data Management (p. 549), users can set the save the Mechanical APDL application database and delete unneeded file settings. Define Initial Conditions Basic general information about this topic ... for this analysis type: You must point to a static structural analysis of the same model in the initial condition environment. • Linear buckling analysis must be preceded by a static structural analysis. • If the static structural analysis has multiple result sets, the value from any restart point available in the static structural analysis can be used as the basis for the linear buckling analysis. See Restarts from Multiple Result Sets (p. 31) for more information. • The results calculated by the linear buckling analysis are buckling load factors that scale the loads applied in the static structural analysis. Thus for example if you applied a 10 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 23 Approach N compressive load on a structure in the static analysis and if the linear buckling analysis calculates a load factor of 1500, then the predicted buckling load is 1500x10 = 15000 N. Because of this it is typical to apply unit loads in the static analysis that precedes the buckling analysis. • The buckling load factor is to be applied to all the loads used in the static analysis. Apply Loads and Supports Basic general information about this topic ... for this analysis type: No loads are allowed in the linear buckling analysis. The supports as well as the stress state from the static structural analysis are used in the linear buckling analysis. Note If the static analysis has a pressure load applied “normal to” faces (3-D) or edges (2-D), this could result in an additional stiffness contribution called the “pressure load stiffness” effect. This effect plays a significant role in linear buckling analyses. Different buckling loads may be predicted from seemingly equivalent pressure and force loads in a buckling analysis because in the Mechanical application a force and a pressure are not treated the same. As with any numerical analysis, we recommend that you use the type of loading which best models the in-service component. For more information, see the Mechanical APDL Theory Reference, under Structures with Geometric Nonlinearities> Stress Stiffening> Pressure Load Stiffness. Solve Basic general information about this topic ... for this analysis type: Solution Information continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. Review Results Basic general information about this topic ... for this analysis type: You can view the buckling mode shape associated with a particular load factor by displaying a contour plot or by animating the deformed mode shape. The contours represent relative displacement of the part. Buckling mode shape displays are helpful in understanding how a part or an assembly deforms when buckling, but do not represent actual displacements. 24 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types “Stresses” from a modal analysis do not represent actual stresses in the structure, but give you an idea of the relative stress distributions for each mode. Stress and Strain results are available only if requested before solution using Output Controls (p. 545). Modal Analysis Introduction A modal analysis determines the vibration characteristics (natural frequencies and mode shapes) of a structure or a machine component. It can also serve as a starting point for another, more detailed, dynamic analysis, such as a transient dynamic analysis, a harmonic analysis, or a spectrum analysis. The natural frequencies and mode shapes are important parameters in the design of a structure for dynamic loading conditions. You can also perform a modal analysis on a prestressed structure, such as a spinning turbine blade. If there is damping in the structure or machine component, the system becomes a damped modal analysis. For a damped modal system, the natural frequencies and mode shapes become complex. For a rotating structure or machine component, the gyroscopic effects resulting from rotational velocities are introduced into the modal system. These effects in turn change the system’s damping. Such effects are commonly encountered in rotordynamic analysis. The changes in Eigen characteristics at different rotational velocity can be studied with the aid of Campbell Diagram Chart Results. A modal analysis can be performed using the ANSYS or Samcef solver. Any differences are noted in the sections below. Points to Remember • The Rotational Velocity load is not available in Modal Analysis when the analysis is linked to a Static structural analysis. • Prestressed modal analysis requires performing a static structural analysis first. In the modal analysis you can use the Initial Condition object to point to the Static Structural analysis to include prestress effects. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: From the Toolbox, drag a Modal or a Modal (Samcef) template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: Due to the nature of modal analyses any nonlinearities in material behavior are ignored. Optionally, orthotropic and temperature-dependent material properties may be used. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 25 Approach The critical requirement is to define stiffness as well as mass in some form. Stiffness may be specified using isotropic and orthotropic elastic material models (for example, Young's modulus and Poisson's ratio), using hyperelastic material models (they are linearized to an equivalent combination of initial bulk and shear moduli), or using spring constants, for example. Mass may derive from material density or from remote masses. Note Hyperelastic materials are supported for pre-stress modal analyses. They are not supported for standalone modal analyses. Attach Geometry Basic general information about this topic ... for this analysis type: When 2D geometry is used, only the 2D axisymmetric behavior is available for Samcef solvers. When performing a Rotordynamic Analysis, the rotors can be easily generated using the Import Shaft Geometry feature of ANSYS DesignModeler. The feature uses a text file to generate a collection of line bodies with circular or circular tube cross sections. Define Part Behavior Basic general information about this topic ... for this analysis type: You can define a Point Mass for this analysis type. Define Connections Basic general information about this topic ... for this analysis type: • Joints are allowed in a modal analysis. They restrain degrees of freedom as defined by the joint definition. • The stiffness of any spring is taken into account and if specified, damping is also considered. • For the Samcef solver, only contacts, springs, and beams are supported. Joints are not supported. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: 26 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types There are no special considerations for this analysis type. Establish Analysis Settings Basic general information about this topic ... for this analysis type: Number of Modes: You need to specify the number of frequencies of interest. The default is to extract the first 6 natural frequencies. The number of frequencies can be specified in two ways: 1. The first N frequencies (N > 0), or 2. The first N frequencies in a selected range of frequencies. Solver Controls (p. 533): Two settings are available in this control – Damped and Solver Type. For Damped, you can specify if the modal system is undamped or damped. Depending on the selection made for Damped, different solver options are provided accordingly. Damped by default, it is set No and assumes the modal system is an undamped system. Solver Type (p. 533): Typically you should let the program choose the type of solver appropriate for your model in both undamped and damped modal systems. Note If a solver type of Unsymmetric, Full Damped or Reduced Damped is selected, the modal system cannot be followed by Transient, Harmonic, Random Vibration or Response Spectrum systems. However, for MSUP Harmonic Analysis and MSUP Transient Analysis you can use the Reduced Damped solver with Store Complex Solution set to No. Store Complex Solution: This control is only available when a damped solver type of Reduced Damped is selected. This control allows you to solve and store a damped modal system as an undamped modal system. By default, it is set to Yes. Cyclic Controls: When running a cyclic symmetry analysis, set the Harmonic Index Range to Program Controlled to solve for all harmonic indices, or to Manual to solve for a specific range of harmonic indices. Output Controls (p. 545): By default only mode shapes are calculated. You can request Stress and Strain results to be calculated but note that “stress” results only show the relative distribution of stress in the structure and are not real stress values. You can also choose whether or not to have these results stored for faster result calculations in linked systems. Damping Controls (p. 542): Two damping types, Stiffness Coefficient and Mass Coefficient, are available to set up a damped modal system. Stiffness Coefficient can be defined in two ways, either by Direct Input or by Damping Vs Frequency. Rotordynamics Controls (p. 551): Specify Rotordynamics Controls as needed when setting up a Rotordynamic Analysis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 27 Approach Analysis Data Management (p. 549) (applicable to Modal systems only) settings enable you to save specific solution files from the Modal analysis for use in other analyses. You can set the Future Analysis field to PSD/RS Analyses if you intend to use the modal results in a subsequent Modal, Random Vibration (PSD), or Response Spectrum (RS) analysis. When a PSD or RS analysis is linked to a modal analysis, additional solver files must be saved to achieve the PSD or RS solution. If the files were not saved, then the modal analysis has to be solved again and the files saved. Note Solver Type, Scratch Solver Files..., Save ANSYS db, Solver Units, and Solver Unit System are applicable to Modal systems only. Define Initial Conditions Basic general information about this topic ... for this analysis type: You can point to a Static Structural analysis in the Initial Condition environment field if you want to include prestress effects. A typical example is the large tensile stress induced in a turbine blade under centrifugal load that can be captured by a static structural analysis. This causes significant stiffening of the blade. Including this prestress effect will result in much higher, realistic natural frequencies in a modal analysis. If the modal analysis is linked to a static structural analysis for initial conditions and the parent static structural analysis has multiple result sets (multiple restart points at load steps/sub steps), you can start the modal analysis from any restart point available in the static structural analysis. By default, the values from the last solve point are used as the basis for the modal analysis. See Restarts from Multiple Result Sets (p. 31) for more information. Note When you perform a prestressed modal analysis, the support conditions from the static analysis are used in the modal analysis. You cannot apply any new supports in the modal analysis portion of a prestressed modal analysis. Apply Loads and Supports Basic general information about this topic ... for this analysis type: Only Rotational Velocity load is allowed in a stand-alone modal analysis. All structural supports can be applied except the Non-zero Displacement, Remote Displacement, and the Velocity boundary condition. Due to their nonlinear nature, compression only supports are not recommended in a modal analysis. Use of compression only supports may result in extraneous or missed natural frequencies. 28 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types For the Samcef solver, the following supports are not available: Compression Only Support, Elastic Support. Note Pre-stressed Modal Analysis: • In a pre-stressed modal analysis any structural supports used in the static analysis persist. Therefore, you are not allowed to add new supports in the pre-stressed modal analysis • Rotational Velocity is not available for Modal Analysis system in a prestressed modal analysis. Solve Basic general information about this topic ... for this analysis type: Solution Information continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. Review Results Basic general information about this topic ... for this analysis type: Highlight the Solution object in the tree to view a bar chart of the frequencies obtained in the modal analysis. A tabular data grid is also displayed that shows the list of frequencies, stabilities, modal damping ratios and logarithm decrements of each mode. For an undamped modal analysis, only frequencies are available in the Tabular Data window. For a damped modal analysis, real and imaginary parts of the eigenvalues of each mode are listed as Stability and Damped Frequency, respectively, in the Tabular Data window. If the real/stability value is negative, the eigenmode is considered to be stable. For the damped modal analysis, Modal Damping Ratio and Logarithmic Decrement are also included in the Tabular Data window. Like the stability value, these values are an indicator of eigenmode stability commonly used in rotordynamics. If Campbell Diagram is set to On, a Campbell diagram chart result is available for insert under Solution. A Campbell diagram chart result conveys information as to how damped frequencies and stabilities of a rotating structural component evolve/change in response to increased rotational velocities. More detailed information about the result can be found in Campbell Diagram Chart Results (p. 683). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 29 Approach Note The Campbell diagram result chart is only appropriate for a rotating structural component that is axis-symmetrical. It is supported for all body types: solid, shell, and line bodies, but limited to single spool systems. For a single spool system, all bodies in the modal system are subjected to one and only single rotational velocity. The contour and probe results are post-processed using set number, instead of mode number. The total set number is equal to number of modes requested multiplied by number of rotational velocity solve points. You can use the Set, Solve Point and Mode columns in the table to navigate between the set number and mode, and rotational velocity solve point and mode. You can choose to review the mode shapes corresponding to any of these natural frequencies by selecting the frequency from the bar chart or tabular data and using the context sensitive menu (right mouse click) to choose Create Mode Shape Results. You can also view a range of mode shapes. You can view the mode shape associated with a particular frequency as a contour plot. You can also animate the deformed shape including, for a damped analysis, the option to allow or ignore the time decay animation for complex modes. The contours represent relative displacement of the part as it vibrates. When running a cyclic symmetry analysis, additional result object settings in the Details view are available, as well as enhanced animations and graph displays. See Cyclic Symmetry in a Modal Analysis for more information. Note The use of construction geometry is not supported for the postprocessing of cyclic symmetry results. Applying Pre-Stress Effects Mechanical leverages the power of linear perturbation technology for all pre-stress analyses performed within Mechanical. This includes pre-stress modal analyses as well as linear buckling analyses. The following features are available that are based on this technology: • Large deflection static analysis followed by pre-stress modal analysis. Thus the static analysis can be linear or nonlinear including large deflection effects. Note 30 – If performing a pre-stress modal analysis, it is recommended that you always include large deflection effects to produce accurate results in the modal analysis. – Although the modal results (including displacements, stresses, and strains) will be correctly calculated in the modal analysis, the deformed shape picture inside Mechanical will be based on the initial geometry, not the deformed geometry from the static analysis. If you desire to see the mode shapes based on the deformed geometry, you can take the result file into Mechanical APDL. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types • True contact status as calculated at the time in the static analysis from which the eigen analysis is based. • Support for cyclic analysis. • Support for multiple result sets in the static analysis. For a pre-stressed eigen analysis, you can insert a Commands object beneath the Pre-Stress initial conditions object. The commands in this object will be executed just before the first solve for the prestressed modal analysis. Restarts from Multiple Result Sets A property called Pre-Stress Define By is available in the Details view of the Pre-Stress object in the eigen analysis. It is set to Program Controlled by default which means that it uses the last solve point available in the parent static structural analysis as the basis for the eigen analysis. There are three more read only properties defined in the Details view of the Pre-Stress object – Reported Loadstep, Reported Substep and Reported Time which are set to Last, Last, and End Time or None Available by default depending on whether or not there are any restart points available in the parent static structural analysis. These read only properties show the actual load step, sub step and time used as the basis for the eigen analysis. You can change Pre-Stress Define By to Load Step, and then another property called Pre-Stress Loadstep will appear in the Details view. Pre-Stress Loadstep gives you an option to start from any load step in the static structural analysis. If you use this property, then Mechanical will always pick the last substep available in that load step. You can see the actual reported substep and time as read only properties. The input value of load step should be less than or equal to the number of load steps in the parent static structural analysis. Loadstep 0 stands for the last load step available. You can change Pre-Stress Define By to Time, and then another property called Pre-Stress Time will appear in the Details view. Pre-Stress Time gives you an option to start from any time in the static structural analysis. If there is no restart point available at the time of your input, then Mechanical will pick the closest restart point available in the static structural analysis. You can see the actual reported load step, sub step and time as read only properties. The input value of time should be non-negative and it should be less than the end time of parent static structural analysis. Time 0 stands for end time of the parent analysis. If there is no restart point available in the input loadstep and the number of restart points in the parent analysis is not equal to zero, then the following error message appears: “There is no restart point available at the requested loadstep. Please change the restart controls in the parent static structural analysis to use the requested loadstep.” Note If you use Pre-Stress Time, then Mechanical will pick the closest restart point available. It may not be the last sub step of a load step; and if it is some intermediate substep in a load step, then the result may not be reproducible if you make any changes in the parent static structural analysis or you solve it again. If there is no restart point available in the parent static structural analysis, then Reported Loadstep, Reported Substep and Reported Time are set to None Available regardless of the user input of LoadStep/Time but these will be updated to correct values once the analysis is solved with the correct restart controls for the parent structural analysis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 31 Approach Contact Status You may choose contact status for the pre-stressed eigen analysis to be true contact status, force sticking, or force bonded. A property called Contact Status is available in the Details view of the PreStress object in the eigen analysis. This property controls the CONTKEY field of the Mechanical APDL PERTURB command. • Use True Status (default): Uses the current contact status from the restart snapshot. If the previous run for parent static structural is nonlinear, then the nonlinear contact status at the point of restart is frozen and used throughout the linear perturbation analysis. • Force Sticking: Uses sticking contact stiffness for the frictional contact pairs, even when the status is sliding (that is, the no sliding status is allowed). This option only applies to contact pairs whose frictional coefficient is greater than zero. • Force Bonding: Uses bonded contact stiffness and status for contact pairs that are in the closed (sticking/sliding) state. Electric Analysis Introduction An electric analysis supports Steady-State Electric Conduction. Primarily, this analysis type is used to determine the electric potential in a conducting body created by the external application of voltage or current loads. From the solution, other results items are computed such as conduction currents, electric field, and joule heating. An Electric Analysis supports single and multibody parts. Contact conditions are automatically established between parts. In addition, an analysis can be scoped as a single step or in multiple steps. An Electric analysis computes Joule Heating from the electric resistance and current in the conductor. This joule heating may be passed as a load to a Thermal analysis simulation using an Imported Load if the Electric analysis Solution data is to be transferred to Thermal analysis. Similarly, an electric analysis can accept a Thermal Condition from a thermal analysis to specify temperatures in the body for material property evaluation of temperature-dependent materials. Points to Remember A steady-state electric analysis may be either linear (constant material properties) or nonlinear (temperature dependent material properties). Additional details for scoping nonlinearities are described in the Nonlinear Controls section. Once an Electric Analysis is created, Voltage and Current loads can be applied to any conducting body. For material properties that are temperature dependent, a temperature distribution can be imported using the Thermal Condition option. In addition, equipotential surfaces can be created using the Coupling Condition load option. Preparing the Analysis Create Analysis System Basic general information about this topic 32 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types ... for this analysis type: From the Toolbox, drag the Electric template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: When an Emag license is being used only the following material properties are allowed: Isotropic Resistivity, Orthotropic Resistivity, Relative Permeability, Relative Permeability (Orthotropic), Coercive Force & Residual Induction, B-H Curve, B-H Curve (Orthotropic), Demagnetization B-H Curve. You may have to turn the filter off in the Engineering Data workspace to suppress or delete those material properties/models which are not supported for this license. Attach Geometry Basic general information about this topic ... for this analysis type: 3-D shell bodies and line bodies are not supported in an electric analysis. Define Part Behavior Basic general information about this topic ... for this analysis type: There are no specific considerations for an electric analysis. Define Connections Basic general information about this topic ... for this analysis type: In an electric analysis, only bonded, face-face contact is valid. Any joints or springs are ignored. For perfect conduction across parts, use the MPC formulation. To model contact resistance, use Augmented Lagrange or Pure Penalty with a defined Electric Conductance. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: Only higher order elements are allowed for an electric analysis. Establish Analysis Settings Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 33 Approach Basic general information about this topic ... for this analysis type: For an electric analysis, the basic controls are: Step Controls (p. 529): used to specify the end time of a step in a single or multiple step analysis. Multiple steps are needed if you want to change load values, the solution settings, or the solution output frequency over specific steps. Typically you do not need to change the default values. Output Controls (p. 545) allow you to specify the time points at which results should be available for postprocessing. A multi-step analysis involves calculating solutions at several time points in the load history. However you may not be interested in all of the possible results items and writing all the results can make the result file size unwieldy. You can restrict the amount of output by requesting results only at certain time points or limit the results that go onto the results file at each time point. Analysis Data Management (p. 549) settings. Define Initial Conditions Basic general information about this topic ... for this analysis type: There is no initial condition specification for an Electric analysis. Apply Loads and Supports Basic general information about this topic ... for this analysis type: The following loads are supported in a Steady-State Electric analysis: • Voltage • Current • Coupling Condition (Electric) • Thermal Condition Solve Basic general information about this topic ... for this analysis type: The Solution Information object provides some tools to monitor solution progress. 34 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Solution Output continuously updates any listing output from the solver and provides valuable information on the behavior of the model during the analysis. Any convergence data output in this printout can be graphically displayed as explained in the Solution Information section. Review Results Basic general information about this topic ... for this analysis type: Applicable results are all electric result types. Once a solution is available, you can contour the results or animate the results to review the responses of the model. For the results of a multi-step analysis that has a solution at several time points, you can use probes to display variations of a result item over the steps. You may also wish to use the Charts feature to plot multiple result quantities against time (steps). For example, you could compare current and joule heating. Charts can also be useful when comparing the results between two analysis branches of the same model. Explicit Dynamics Analysis Introduction You can perform a transient explicit dynamics analysis in the Mechanical application using an Explicit Dynamics system. Additionally, the Explicit Dynamics (LS-DYNA Export) system is available to export the model in LS-DYNA .k file format for subsequent analysis with the LS-DYNA solver. Unless specifically mentioned otherwise, this section addresses both the Explicit Dynamics and Explicit Dynamics (LS-DYNA Export) systems. Special conditions for the Explicit Dynamics (LS-DYNA Export) system are noted where pertinent. An explicit dynamics analysis is used to determine the dynamic response of a structure due to stress wave propagation, impact or rapidly changing time-dependent loads. Momentum exchange between moving bodies and inertial effects are usually important aspects of the type of analysis being conducted. This type of analysis can also be used to model mechanical phenomena that are highly nonlinear. Nonlinearities may stem from the materials, (for example, hyperelasticity, plastic flows, failure), from contact (for example, high speed collisions and impact) and from the geometric deformation (for example, buckling and collapse). Events with time scales of less than 1 second (usually of order 1 millisecond) are efficiently simulated with this type of analysis. For longer time duration events, consider using a Transient Structural Analysis (p. 91) system. Points to Remember An explicit dynamics analysis typically includes many different types of nonlinearities including large deformations, large strains, plasticity, hyperelasticity, material failure etc. The time step used in an explicit dynamics analysis is constrained to maintain stability and consistency via the CFL condition, that is, the time increment is proportional to the smallest element dimension in the model and inversely proportional to the sound speed in the materials used. Time increments are Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 35 Approach usually on the order of 1 microsecond and therefore thousands of time steps (computational cycles) are usually required to obtain the solution. • Explicit dynamics analyses only support the mm, mg, ms solver unit system . This will be extended to support more unit systems in a future release. • 2-D Explicit Dynamics analyses are supported for Plane Strain and Axisymmetric behaviors. • When attempting to use the Euler capabilities in the Explicit Dynamics analysis system, the following license restrictions are observed: • – Set-up and solve of Euler capabilities in the Explicit Dynamics system are supported for the full ANSYS AUTODYN (acdi_ad3dfull) license. – Set-up but not solve of Euler capabilities in the Explicit Dynamics system are supported for the prepost ANSYS AUTODYN (acdi_prepost) license. – Set-up or solve of Euler capabilities in the Explicit Dynamics system are not supported for the ANSYS Explicit STR (acdi_explprof ) license. – Euler capabilities are not supported for the Explicit Dynamics (LS-DYNA Export) system. (Linux only) In order to run a distributed solution on Linux, you must add the MPI_ROOT environment variable and set it to the location of the MPI software installation. It should be of the form: {ANSYS installation}/commonfiles/MPI/Platform/{version}/{platform} For example: usr/ansys_inc/v140/commonfiles/MPI/Platform/8.1/linx64 • Consideration should be given to the number of elements in the model and the quality of the mesh to give larger resulting time steps and therefore more efficient simulations. • A coarse mesh can often be used to gain insight into the basic dynamics of a system while a finer mesh is required to investigate nonlinear material effects and failure. • The quality of the solution can be monitored by reviewing momentum and energy conservation graphs in the solution output. Low energy errors (<10% of initial energy) are indicative of good quality solutions. • Where more accuracy is required, for example in low velocity impact simulations, then the double precision option may be used. Real values are stored with 64-bit floating point precision. This will also result in an increase in memory usage and the size of the restart files. The double precision option is recommended when breakable bonded connections are used or an implicit pre-stress condition is used as an initial condition. • The Explicit Dynamics (LS-DYNA Export) system allows for an LS-DYNA input file (otherwise known as a “keyword” file or a “.k” file) to be exported. This keyword file contains all the necessary information available in the Mechanical application environment to carry out the analysis with the LS-DYNA solver. The exported keyword file follows the same format as the one exported by the respective Mechanical APDL application. All the LS-DYNA keywords are implemented according to the “LS_DYNA Keyword Users Manual” version 971. All the LS-DYNA keywords that can currently be exported are described in detail in Supported LSDYNA Keywords (p. 1107). Any parameters that are not shown for a card are not used and their default values will be assigned for them by the LS-DYNA solver. Some descriptions of Workbench features that do not relate directly to keywords are given under ”General Descriptions” located at the end of this appendix. Since only an input file is generated during solve of an Explicit Dynamics (LS-DYNA Export) system, the Background and Remote solve options are not supported. 36 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types • When using Commands objects with the Explicit Dynamics (LS-DYNA Export) system, be aware of the following: – Keyword cards read from Commands object content (renamed to "Keyword" snippets for the Explicit Dynamics (LS-DYNA Export) system) should not have any trailing empty lines if they are not intentional. This is due to the fact that some keywords have more than one mandatory card that can be entered as blank lines, in which case the default values for the card will be used. Hence trailing blank lines can be significant only if required, otherwise they may cause solver execution errors. – The first entry in the Commands object content must be a command name which is preceded by the * symbol. – Refer to LS-DYNA General Descriptions (p. 1133) regarding ID numbers entered in Commands object content. An explicit dynamics analysis can contain both rigid and flexible bodies. For rigid/flexible body dynamic simulations involving mechanisms and joints you may wish to consider using either the Transient Structural Analysis (p. 91) or Rigid Dynamics Analysis (p. 102) options. For more information about explicit dynamics analyses, please see Appendix F (p. 1253). Note The intent of this document is to provide an overview of an explicit dynamics analysis. Consult our technical support department to obtain a more thorough treatment of this topic. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: From the Toolbox drag an Explicit Dynamics or an Explicit Dynamics (LS-DYNA Export) template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: Material properties can be linear elastic or orthotropic. Many different forms of material nonlinearity can be represented including hyperelasticity, rate and temperature dependant plasticity, pressure dependant plasticity, porosity, material strength degradation (damage), material fracture/failure/fragmentation. For a detailed discussion on material models used in Explicit Dynamics, please refer to Appendix E (p. 1185). Density must always be specified for materials used in an explicit dynamics analysis. Data for a range of materials is available in the Explicit material library. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 37 Approach For Explicit Dynamics (LS-DYNA Export) systems, only the following material models are supported (also see *MAT_ keywords in Supported LS-DYNA Keywords (p. 1107)). Any models that are not mentioned in this list can be entered through the "Keyword Snippet" facility (see the LS-DYNA General Descriptions section): • Strength models – Linear Elastic → Isotropic → Orthotropic – Plasticity → Bilinear Isotropic Hardening → Multilinear Isotropic Hardening → Bilinear Kinematic Hardening → Johnson Cook – Hyperelastic: → Mooney-Rivlin → Polynomial → Yeoh → Ogden – • • Rigid (there is no entry for this in the Engineering Data workspace of Workbench. See *MAT_RIGID in Supported LS-DYNA Keywords (p. 1107) for more details). Equation of state (EOS) models – Linear (there is no entry for this in the Engineering Data workspace of Workbench. See *EOS_LINEAR_POLYNOMIAL in Supported LS-DYNA Keywords (p. 1107) for more details). – Shock Failure models – Plastic Strain – Johnson Cook Note For line bodies, the LS-DYNA solver only supports the following three material properties from the above list: Isotropic Linear Elastic, Bilinear Kinematic Hardening Plasticity and Rigid bodies. Additional material models that are supported by the LS-DYNA solver for line bodies can be added through the "Keyword Snippet" facility. Attach Geometry Basic general information about this topic ... for this analysis type: 38 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Solid, Surface, and Line bodies can be present in an Explicit Dynamics analysis. Springs and dampers are not available. Only symmetric cross sections are supported for line bodies in Explicit Dynamics analyses, except for the Explicit Dynamics (LS-DYNA Export) systems. The following cross sections are not supported: T-Sections, L-Sections, Z-Sections, Hat sections, Channel Sections. For I-Sections, the two flanges must have the same thickness. For rectangular tubes, opposite sides of the rectangle must be of the same thickness. For LS-DYNA Export systems all available cross sections in DesignModeler will be exported for analysis with the LS-DYNA solver. However there are some limitations in the number of dimensions that the LSDYNA solver supports for the Z, Hat and Channel cross sections. For more information consult the LS-DYNA Keywords manual. To prevent the generation of unnecessarily small elements (and long run times) try using DesignModeler to remove unwanted “small” features or holes from your geometry. Thickness can be specified for selected faces on a surface body by inserting a thickness object. Constant, tabular, and functional thickness are all supported. Note that 2-D analysis is not supported for Explicit Dynamics but may be used to set up 2-D simulations to be transferred to the AUTODYN component system to perform a solve, if a license is available. Symmetry is not supported when exporting to the LS-DYNA .k file. Stiffness Behavior Flexible behavior can be assigned to any body type. Rigid behavior can be applied to Solid and Surface bodies. Coordinate System Local Cartesian coordinate systems can be assigned to bodies. These will be used to define the material directions when using the Orthotropic Elasticity property in a material definition. The material directions 1, 2, 3 will be aligned with the local x, y and z axes of the local coordinate system. Note Cylindrical coordinate systems are not supported for Explicit Dynamics systems. Reference Temperature This option defines the initial (time=0.0) temperature of the body. Reference Frame Available for solid bodies when an Explicit Dynamics system is part of the solution; the user has the option of setting the Reference Frame to Lagrangian (default) or Eulerian (Virtual). If Stiffness Behavior is defined as Rigid, Eulerian is not a valid setting. Rigid Materials Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 39 Approach For bodies defined to have rigid stiffness, only the Density property of the material associated with the body will be used. For Explicit Dynamics systems all rigid bodies must be discretized with a Full Mesh. This will be specified by default for the Explicit meshing physics preference. The mass and inertia of the rigid body will be derived from the elements and material density for each body. By default, a kinematic rigid body is defined and its motion will depend on the resultant forces and moments applied to it through interaction with other Parts of the model. Elements filled with rigid materials can interact with other regions via contact. Constraints can only be applied to an entire rigid body. For example, a fixed displacement cannot be applied to one edge of a rigid body, it must be applied to the whole body. Note • Only symmetric cross-sections are supported for line bodies • Flexible and rigid bodies cannot be combined in Multi-body Parts. Bonded connections can be applied to connect rigid and flexible bodies • The Thickness Mode and Offset Type fields for surface bodies are not supported for Explicit Dynamics systems • Initial over-penetrations of nodes/elements of different bodies should be avoided or minimized if sliding contact is to be used. There are several methods available in Workbench to remove initial penetration Define Part Behavior Basic general information about this topic ... for this analysis type: Nonlinear effects are always accounted for in explicit dynamics analysis. Parts may be defined as rigid or flexible. In the solver, rigid parts are represented by a single point that carries the inertial properties together with a discretized exterior surface that represents the geometry. Rigid bodies should be meshed using similar Method mesh controls as those used for flexible bodies. The inertial properties used in the solver will be derived from the discretized representation of the body and the material density and hence may differ slightly from the values presented in the properties of the body in the Mechanical application GUI. At least one flexible body must be specified when using the ANSYS AUTODYN solver. The solver requires this in order to calculate the time-step increments. In the absence of a flexible body, the time-step becomes underdefined. The boundary conditions allowed for the rigid bodies with explicit dynamics are: • Connections – 40 Contact Regions: Frictionless, Frictional and Bonded. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types – Body Interactions: Frictionless, Frictional and Bonded. Bonded body interactions are not supported for LS-DYNA Export. – For ANSYS AUTODYN, rigid bodies may not be bonded to other rigid bodies. • Initial Conditions: Velocity, Angular Velocity • Supports: Displacement, Fixed Support and Velocity. • Loads: Pressure and Force. Force is not supported for ANSYS AUTODYN. For an Explicit Dynamics analysis, the following postprocessing features are available for rigid bodies: • Results and Probes: Deformation only - that is, Displacement, Velocity. • Result Trackers: Body average data only. If a multibody part consists only of rigid bodies, all of which share the same material assignment, the part will act as a single rigid body, even if the individual bodies are not physically connected. Define Connections Basic general information about this topic ... for this analysis type: Line body to line body contact is possible if: • Contact Detection should be set to Proximity Based in the Body Interactions Details view. • Edge on Edge is set to Yes in the Body Interactions Details view. • The Interaction Type is defined as Frictional or Frictionless – bonded interactions and connections are not supported for line bodies. • LS-DYNA Export systems export the *CONTACT_AUTOMATIC_GENERAL and *CONTACT_AUTOMATIC_SINGLE_SURFACE keywords when a friction or frictionless Body Interaction is scoped to geometry that contains line bodies. The keywords handle contacts between line bodies only, and line bodies to other body types respectively. In the case where the Body Interaction is scoped to only line bodies, then only the *CONTACT_AUTOMATIC_GENERAL keyword is exported. Reinforcement body interaction should be supported in the case when only line bodies are scoped to a Body Interaction of Type = Reinforcement. The line bodies will then be tied to any solid body that they intersect. Reinforcement body interactions are not supported for LS-DYNA Export systems or for 2D Explicit Dynamics analyses. However utilizing Keyword Snippets under Contact Region objects should provide a suitable alternative. Body Interactions, Contact and Spot Welds are all valid in explicit dynamics analyses. Frictional, Frictionless and Bonded body interactions and contact options are available. Conditionally bonded contact can be simulated using the breakable property of each bonded region. Spot Welds can also be made to fail using the breakable property. Joints, Springs and Beam connections are not supported for explicit dynamics analyses. The Contact Tool is also not applicable to explicit dynamics analyses. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 41 Approach By default, a Body Interaction object will be automatically inserted in the Mechanical application tree and will be scoped to all bodies in the model. This object activates frictionless contact behavior between all bodies that come into proximity during the analysis. For Explicit Dynamics (LS-DYNA Export) systems, bonded body interactions are not supported. Also, Contact Region objects with Auto Asymmetric Behavior or just Asymmetric Behavior are treated the same. Symmetric Behavior will create a _SURFACE_TO_SURFACE keyword for the contact and an Asymmetric Behavior will create a _NODES_TO_SURFACE keyword. For Explicit Dynamics (LS-DYNA Export) systems, contacts between line bodies and solids can be implemented using the Keyword Snippets facility available under the Manual Contact Region objects. Bonded contact is not supported in an explicit dynamics analysis for bodies that have their Reference Frame set to Eulerian (Virtual). A solver warning is shown to let the user know that such bodies will be ignored for bonds. Bonded contact is not support in a 2D explicit dynamics analysis. Setting Up Symmetry Basic general information about this topic ... for this analysis type: There are general considerations when using Symmetry for an Explicit Dynamics Analysis. There are additional considerations if an Euler Domain is defined for an analysis. For symmetry to be applied to an Euler Domain, symmetry will have to be defined with the global coordinate system, not a local one, and it will need to be applied on geometry faces which lie on the global coordinate system planes. • If the symmetry is not defined with the global coordinate system, it is ignored and a warning is shown in the messages window saying that such symmetry will be ignored but the analysis continues to solve. • If the symmetry is not applied on faces which lie on the global coordinate system planes then an error is shown and the solution is terminated. In the case where symmetry is valid for use with Euler Domains, if the boundary of the Euler Domain which is parallel to the symmetry plane is bellow the symmetry plane, then that boundary will be moved to lie on the symmetry plane if the following conditions are true: • the Euler Domain Size Definition option in the Analysis settings is set to Program Controlled. • the Euler body is on the positive side of the global coordinate axis. Define Remote Points Basic general information about this topic ... for this analysis type: 42 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types When using Remote Points in explicit dynamics analyses: • Remote points only work with the Explicit Dynamics system, not the Explicit Dynamics (LS-DYNA Export) system. • The Behavior field must be set to Rigid. If it is set to Deformable the solution will terminate and an error will be generated. • Currently, only the Remote Displacement boundary condition is supported for Remote Points in explicit dynamics analyses. • Commands are not supported for Remote Points in explicit dynamics analyses. • Remote Points are not supported for 2D Explicit Dynamics analyses. It is possible to over-constrain bodies by having an incorrect mix of boundary conditions (loads and supports) and remote points applied. Remote points effectively make a face act as rigid, and it is important to remember that remote points are defined per model and therefore may conflict when shared with another analysis type with different constraint requirements. Remote displacements are boundary conditions but are applied to remote points, and for the purpose of this document are not considered as constraining boundary conditions. Constraining boundary conditions (Restricted Use) Fixed Support Velocity Simply Supported Fixed Rotation Displacement Gravity Hydrostatic Pressure Detonation Point Examples of permitted boundary conditions (Unrestricted Use) Pressure Acceleration Force Symmetry Planes Euler Boundary Flow Out Line Pressure Remote point applied boundary conditions Remote Displacement (treated as a Velocity) The following rules apply when applying constraints and Remote Points to Flexible and Rigid Bodies in an Explicit Dynamics analysis. If incompatible conditions are applied, the pre-solve checks will identify the problem and inform the user prior to starting the Solve. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 43 Approach FLEXIBLE BODY Example Conditions Allowed? + Notes Remote Point applied to one face. Yes Remote Point and Remote Displacement applied to one face. Yes Remote Point applied to two adjacent faces. No The 2 faces share common nodes along one edge. Remote Point applied to two faces that do not share any nodes. Yes Remote Point applied to two faces that do not share any nodes, with Remote Displacement applied to one of the Remote Points. Yes Remote Point on one face with Remote Displacement applied. Constraining boundary condition applied to adjacent face. No Remote Point on one face. Constraining boundary condition applied to adjacent face. 44 The boundary condition scope shares nodes with the scope of the Remote Displacement. No The boundary condition scope shares nodes with the scope of the Remote Point. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types FLEXIBLE BODY Example Conditions Allowed? + Notes Remote Point on one face. Constraining boundary condition on another but with no common scoped nodes. Yes Remote Point on one face with Remote Displacement applied. Constraining boundary condition on another but with no common scoped nodes. Yes RIGID BODY Example Conditions Allowed? + Notes Remote Point applied to one face. Yes Remote Point and Remote Displacement applied to one face. Yes Remote Point applied to two adjacent faces. Yes Remote Point applied to two faces that do not share any nodes. Yes This is largely superfluous as the body is rigid already so making the face rigid does not make any difference. This is largely superfluous as the body is rigid already so making the face rigid does not make any difference. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 45 Approach RIGID BODY Example Conditions Allowed? + Notes Remote Point applied to two faces that do not share any nodes, with Remote Displacement applied to one of the Remote Points. Yes Remote Point on one face. Constraining boundary condition on body. Yes Remote Point on one face with Remote Displacement applied. Constraining boundary condition on body. No Two constraining boundary conditions on a Rigid body are not allowed. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: All mesh methods available in the Workbench meshing application can be utilized in Explicit Dynamics systems. • Swept Volume Meshing • Patch Dependant Volume Meshing • Hex Dominant Meshing • Patch Independent Tetrahedral Meshing • Multizone Volume Meshing • Patch dependant shell meshing • Patch independent shell meshing A smooth uniform mesh should be sought in the regions of interest for the analysis. Elsewhere, coarsening of the mesh may help to reduce the overall size of the problem to be solved. Use the Explicit meshing preference (set by default) to auto-assign the default mesh controls that will provide a mesh well suited for Explicit Dynamics analyses. This preference automatically sets the Rigid Body Behavior mesh control to Full Mesh. The Full Mesh setting is only applicable to Explicit Dynamics analyses. Other physics preferences can be used if better consistency is desired between implicit and explicit models. 46 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Swept/multi-zone meshes are preferred in Explicit Dynamics analyses so geometry slicing, combined with multibody part options in DesignModeler are recommended to facilitate hexahedral meshing. Alternatively use the patch independent tetrahedral meshing method to obtain more uniform element sizing and take advantage of automatic defeaturing. Define the element size manually to produce more uniform element size distributions especially on surface bodies. Midside nodes should be dropped from the mesh for all elements types (solids, surface and line bodies). Error/warning messages are provided if unsupported (higher order) elements are present in the mesh. Pyramid elements are not supported in Explicit Dynamics analyses. Any elements of this type are converted into two tetrahedral elements, and will warrant a warning in the message window of the Mechanical application. For Explicit Dynamics (LS-DYNA Export) systems, only the element types listed below are supported (partly due to LS-DYNA limitations). Any parts with a mesh containing unsupported elements will be excluded from the exported mesh. A warning is displayed specifying excluded parts. • • Shells – 1st Order: triangles, quadrilaterals – 2nd Order: none Solids – 1st Order: tetrahedrons, pyramids, wedges, hexahedrons, beams – 2nd Order: tetrahedrons Note Pyramids are not recommended for LS-DYNA, a warning is issued if such elements are present in the mesh. When performing an implicit static structural or transient structural analysis to an Explicit Dynamics analysis, the same mesh is required for both the implicit and explicit analysis and only low order elements are allowed. If high order elements are used, the solve will be blocked and an error message will be issued. Establish Analysis Settings Basic general information about this topic ... for this analysis type: The basic analysis settings for explicit dynamics analyses are: • Step Controls - The required input for step control is the termination time for the analysis. This should be set to your best estimate of the solution time required to simulate the event being modeled. You should normally allow the solver to determine its own time step size based on the smallest CFL condition in the model. The efficiency of the Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 47 Approach solution can be increased with the help of mass scaling options. Use this feature with caution. Too much mass scaling can give rise to non-physical results. An explicit dynamics solution may be started, interrupted and resumed at any point in time. For example, an existing solution that has reached its End Time may be extended to continue to review the progression of the mechanical phenomena simulated. The Resume From Cycle option allows you to select which Restart file you would like the Solve to resume the analysis from. See Resume Capability for Explicit Dynamics Analyses (p. 855) for more information. Explicit dynamics analyses are always solved in a single analysis step. Step Control options • • – Resume from cycle (option not available in LS-DYNA) – Maximum Number of Cycles in ANSYS AUTODYN is replaced by Maximum time steps in LS-DYNA – Reference energy cycle (option not available in LS-DYNA) – The Maximum Element Scaling and Update frequency (options not available in LS-DYNA) Solver Controls – These advanced controls allow you to control a range of solver features including element formulations and solution velocity limits. The defaults are applicable to wide range of applications. – Shell thickness update, shell inertia update, density update, minimum velocity, maximum velocity and radius cutoff options can only be set in ANSYS AUTODYN. – Full shell integration and a selectable Unit System are available only in the LS-DYNA Export system. Euler Domain Controls – There are three sets of parameters that are necessary to define the Euler Domain: the size of the whole domain (Domain Size Definition), the number of computational cells in the domain (Domain Resolution Definition), and the type of boundary conditions to be applied to the edges of the domain. Note Euler capabilities are not supported for the Explicit Dynamics (LS-DYNA Export) system. The domain size can be defined automatically (Domain Size Definition = Program Controlled) or manually (Domain Size Definition = Manual). For both the automatic and manual options, the size is defined from a 3D origin point and the X, Y, and Z dimensions of the domain. For the automatic option, specify the Scope of the Domain Size Definition so that the origin and X, Y, and Z dimensions are set to create a box large enough to include all bodies in the geometry (Scope = All Bodies) or the Eulerian Bodies only (Scope = Eulerian Bodies Only). The automatically determined domain size can be controlled with three scaling parameters, one for each direction (X Scale Factor, Y Scale Factor, Z Scale Factor). The size of the domain is affected by the scale factors according to the following equations: 48 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types ′ =  
 ′ =      ′ = where lx, ly, lz are the lengths of the unscaled domain in the x, y, and z directions respectively. These parameters are obtained automatically from the mesh. l'x, l'y, l'z are the lengths of the scaled domain in the x, y, and z directions respectively. Fx, Fy, Fz are the scale factors for the x, y, and z directions respectively. For the Manual option of the Domain Size Definition, specify the origin of the Euler Domain (Minimum X Coordinate, Minimum Y Coordinate, Minimum Z Coordinate) and the dimension in each direction (X Dimension, Y Dimension, Z Dimension). The domain resolution specifies how many cells should be created in the X, Y, and Z directions of the domain. Use the Domain Resolution Definition field to specify how to determine the resolution: either the cell size (Cell Size), the number of cells in each of the X, Y, and Z directions (Cells per Component), or the total number of cells to be created (Total Cells). – For the Cell Size option, specify the size of the cell in the Cell Size parameter. The value specified is the dimension of the cell in each of the X, Y, and Z directions. The units used for the cell size follow the ones specified in the Mechanical application window and are displayed in the text box. The number of the cells in each direction of the domain are then determined from this cell size and the size of the domain with the following equations: =  =  =       where Nx, Ny, Nz are the number of cells in the X, Y, and Z directions respectively. D is the dimension of the cell in each direction (this is the same in all directions). – For the Cells per Component option, enter the number of cells required in each of the X, Y, and Z directions (Number of Cells in X, Number of Cells in Y, Number of Cells in Z). – For the Total Cells option, specify Total Cells (the default is 250,000). The size of the cells will depend on the size of the Euler Domain. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 49 Approach The size of the cell is calculated from the following equation: 


 =         where Ntot is the total number of cells in the domain. If any bodies are defined as Eulerian (Virtual), when Analysis Settings is selected in the outline view, the Euler domain bounding box is displayed in the graphics window. The Euler domain resolution is indicated by black node markers along each edge line of the Euler domain. The visibility of this can be controlled by the Display Euler Domain option in the Analysis Settings. You can set boundary conditions on each of the faces of the Euler Domain. The faces are labeled Lower X Face, Lower Y Face, Lower Z Face (which correspond to the faces with the minimum X, Y, and Z coordinates) and Upper X Face, Upper Y Face, and Upper Z Face (which correspond to the faces with the maximum X, Y, and Z coordinates). The values of the boundary conditions that can be set for each face are: – Flow Out Use the Flow Out boundary condition to flow out material through cell faces. The boundary condition makes the material state of the dummy cell outside the Euler domain the same as that of the cell adjacent to the Flow Out boundary, thus setting the gradients of velocity and stress to zero over the boundary. This approach simulates a far field solution at the boundary, but is only exact for outflow velocities higher than the speed of sound and is an approximation for lower velocities. Therefore, the Flow Out boundary condition is approximate in many cases, and should be placed as far as possible from region of interest and best at a location where the gradients are small. – Impedance Use the Impedance boundary condition to transmit waves through cell faces without reflection. The boundary condition predicts the pressure P in the dummy cell outside the Euler domain from the impedance, particle velocity, and the pressure of the cell adjacent to the Impedance boundary. Only the perpendicular component of the wave is transmitted without reflection. Therefore, the Impedance boundary condition is only approximate, and should be placed as far as possible from region of interest. – Rigid Use the Rigid boundary condition to prevent flow of material through cell faces. The cell faces are closed for material transport and act as rigid nonslip walls. The Rigid boundary condition takes the material state of the dummy cell outside the Euler domain as a mirrored image of the cell adjacent to the Wall boundary, thus setting the normal material velocity at the rigid wall to zero and leaving the tangential velocity unaffected. 50 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Euler Tracking is currently only By Body, which scopes the results to Eulerian bodies in the same manner as Lagrangian bodies. • Damping Controls – Damping is used to control oscillations behind shock waves and reduce hourglass modes in reduced integration elements. These options allow you to adapt the levels of damping, and formulation used for the analysis being conducted. Elastic oscillations in the solution can also be automatically damped to provide a quasistatic solution after a dynamic event. For Hourglass Damping, only one of either the Viscous Coefficient or Stiffness Coefficient, is used for the Flanagan Belytschko option - when running an explicit dynamics analysis using the LS-DYNA solver, LS-DYNA does not allow for two coefficients to be entered in *CONTROL_HOURGLASS. Thus the non-zero coefficient determines the damping format to be either “Flanagan-Belytschko viscous” or “Flanagan-Belytschko stiffness”, accordingly. if both are non-zero, the Stiffness Coefficient will be used – Linear viscosity in expansion options should be available only for ANSYS AUTODYN. – Hourglass damping in LS-DYNA is standard by default; in ANSYS AUTODYN the same control is AUTODYN Standard. • Erosion Controls – Erosion is used to automatically remove highly distorted elements from an analysis and is required for applications such as cutting and impact penetration. In an explicit dynamics analysis, erosion is a numerical tool to help maintain large time steps, and thus obtain solutions in appropriate time scales. Several options are available to initiate erosion. The default settings will erode elements which experience geometric strains in excess of 100%. The default value should be increased when modeling hyperelastic materials. Geometric strain limit and material failure criteria are not present in LS-DYNA. • Output Controls – Solution output is provided in several ways: – Results files which are used to provide nodal and element data for contour and probe results such as deformation, velocity, stress and strain. Note that probe results will provide a filtered time history of the result data due to the relatively infrequent saving of results files. – Restart files should be stored less frequently than results files and can be used to resume an analysis. – Tracker data is usually stored much more frequently than results or restart data and thus is used to produce full transient data for specific quantities. – Output controls to save result tracker and solution output are not available for LSDYNA. – When performing an implicit to explicit analysis, for a nonlinear implicit analysis, the Strain Details view property must be set to Yes because plastic strains are needed for the correct results. Define Initial Conditions Basic general information about this topic ... for this analysis type: • You can define translational or angular velocity to a single body or to multiple bodies. In an explicit dynamics analysis, by default, all bodies are assumed to be at rest with no Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 51 Approach external constraint or load applied. It is not a requirement to apply these types of initial conditions to a body. • An explicit dynamics solve can be performed if the model contains at least one Initial Condition (translational or angular velocity), or a non-zero constraint (displacement or velocity), or a valid load. • Because an explicit dynamics analysis is better suited for short duration events, preceding it with an implicit analysis may produce a more efficient simulation especially for cases in which a generally slower (or rate-independent) phenomenon is followed by a much faster event, such as the collision of a pressurized container. To produce this combination, you can define pre-stress as an initial condition in an Explicit Dynamics system, specifying the transfer of either displacements only or the more complete Material State (displacements, velocities, stresses and strains), from a static or transient structural analysis to an explicit dynamics analysis. Characteristics of the implicit to explicit pre-stress feature: – Applicable to 3-D analyses only. – The Material State mode, for mapping stresses, plastic strains, displacements, and velocities is valid for solid models only. – The displacements only mode is valid for solid, shell, and beam models. – The same mesh is required for both implicit and explicit analyses and only low order elements are allowed. If high order elements are used, the solve will be blocked and an error message will be issued. – For a nonlinear implicit analysis, the Strain Details view property in Output Controls under the Analysis Settings object must be set to Yes because plastic strains are needed for the correct results. See Recommended Guidelines When Using Pre-Stress With Explicit Dynamics (p. 55) for more information. Apply Loads and Supports Basic general information about this topic ... for this analysis type: • You can apply the following loads and supports in an explicit dynamics analysis: – Acceleration (p. 563) 52 – Standard Earth Gravity (p. 566) – Pressure (p. 568) – Hydrostatic Pressure (p. 569) – Force (p. 570) – Line Pressure (p. 578) – Fixed Face (p. 552) – Fixed Edge (p. 552) – Fixed Vertex (p. 553) – Displacements (p. 553) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types – Displacements (p. 553) – Displacements (p. 553) – Detonation Point (p. 608) – Velocity (p. 556) – Impedance Boundary (p. 557) – Simply Supported Edge (p. 560) – Simply Supported Vertex (p. 561) – Fixed Rotation (p. 561) – Remote Displacement (p. 555) • Cylindrical coordinate systems are supported to define a single rotational displacement or velocity constraint on a rigid or flexible body. These coordinate systems are fixed, that is, they do not move with the body. • For Explicit Dynamics analyses, the y component (that is, Θ direction) of a velocity constraint defined with a cylindrical coordinate system has units of angular velocity. • For Explicit Dynamics analyses, the y component (that is, Θ direction) of a displacement constraint defined with a cylindrical coordinate system has units of rotation. • Step or time varying tabular loads can be applied in an explicit dynamics analysis. However, explicit dynamics does not support tabular data to specify the magnitude or components of Accelerations or Line Pressures. • For Explicit Dynamics analyses, functionally defined loads are supported for Pressure and Velocity but only when defined as varying in time. See Applying Boundary Conditions (p. 551). • For Explicit Dynamics (LS-DYNA) analyses, functionally defined loads are not supported. • Loads must be applied in a single step. • Loads and supports are not valid when applied to bodies having a Reference Frame of Eulerian (Virtual). • Detonation Points are only available for 3D Explicit Dynamics analyses, not for Explicit Dynamics (LS-DYNA Export) or 2D Explicit Dynamics analyses. • For Explicit Dynamics analyses, if multiple constraints (for example, displacements) are applied to a node then they must use the same coordinate system. This restriction is especially applicable at nodes on a shared topology such as an edge, where two adjacent faces, each with different constraints, may come together. These constraints must use the same coordinate system in their specification. • In the LS-DYNA solver, a Velocity or Displacement boundary condition (implemented with the *BOUNDARY_PRESCRIBED_MOTION keyword) will override a Fixed Support or a Simple Support or a Fixed Rotation boundary condition (implemented with the *BOUNDARY_SPC keyword). Hence if a body has a Velocity constraint and a Fixed Support applied to it, the whole body will move in the direction of the applied velocity. • The default unconstrained body is valid. It is not a requirement to constrain any DOF of a body In Explicit Dynamics systems. • An Explicit Dynamics solve can be performed if the model contains at least one Initial Condition (Translational or Rotational velocity) or a non-zero constraint (displacement or velocity) or a valid load. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 53 Approach • The Remote Displacement boundary condition only works with the Explicit Dynamics system for 3D analyses, not the Explicit Dynamics (LS-DYNA Export) system or 2D Explicit Dynamics analyses. • A Remote Displacement boundary condition must have the Behavior field set to Rigid for an Explicit Dynamics analysis. An error will be reported if it is set to Deformable. If the Remote Displacement object is scoped to a Remote Point that has its Behavior set to Rigid, the Remote Displacement Behavior will automatically be set to Rigid also. Solve Basic general information about this topic ... for this analysis type: • Solution output – The Solution Information object provides a summary of the solution time increments and progress is continuously updated in the solution output. For distributed analyses, the parallel load balancing is also displayed. This is calculated for each slave as the CPU time taken on the slave divided by the average CPU time taken on all the slaves. For a perfectly balanced solution, all slaves will have a load balancing of one. Histograms of time step, energy and momentum are also available for real time monitoring of solution progress. Note In Explicit Dynamics analyses, Trajectory Contact Detection is not supported for a distributed solve. If you would like to use Trajectory Contact Detection for a distributed solve, please contact ANSYS Technical Support. – Choose Tools> Solve Process Settings to solve in the background either locally or remotely. Retrieve results while the analysis is running to get immediate feedback on progress and accuracy of the solution. Note If you choose the My Computer, Background setting, it is necessary that you also click the Advanced... button and check Use Shared License, if possible, to obtain a successful solution. • 54 Result Tracker – Full transient time history data can be viewed after the insertion of Result Tracker objects. Body averaged data such as momentum and energy can be selected for display. Data at a specific location (position, velocity, stress etc.) can also be displayed. – The frequency at which Result Tracker information is provided is defined in the Save Result Tracker Data On option of the analysis settings. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types • Solve an Explicit Dynamics (LS-DYNA Export) system to produce the LS-DYNA keyword file. This can be used to directly solve with the LS-DYNA solver, outside of the Workbench environment. Review Results Basic general information about this topic ... for this analysis type: • The following structural result types are available as results of an explicit dynamic analysis: – Deformation (p. 635) • – Stress and Strain (p. 639) – Energy (Transient Structural and Rigid Dynamics Analyses) (p. 654) – Stress Tools (p. 658) – Structural Probes (p. 671) - Limited to: Deformation, Strain, Stress, Position, Velocity, Acceleration. Once a solution is available you can display contour results or animate them to review the response of the structure through time. Note For an explicit dynamics analysis, there is no results interpolation between the results sets. Specifying a time in the GUI will display results for the closest results set. • Eroded nodes can be toggled on or off in the graphics display. • Probes can be used to display the variation in specific results over the saved time points in the analysis. The frequency at which data is available is defined in the Save Results On option of the analysis settings. This data should be specified prior to a solve. • You can use a Solution Information object to track, monitor, or diagnose problems that arise during a solution. • Additional results specific to an explicit dynamics analysis are available via User Defined Results for Explicit Dynamics Analyses (p. 714). • The Explicit Dynamics (LS-DYNA Export) system does not support the ability to review the results of a simulation using the LS-DYNA solver. Nevertheless results can be viewed with the lsprepost.exe application available at the ANSYS installation folder under ANSYS Inc\v140\ansys\bin\. Recommended Guidelines When Using Pre-Stress With Explicit Dynamics The following guidelines are recommended when using pre-stress with an Explicit Dynamics analysis: • Lower order elements must be used in the static or transient structural analysis used to pre-stress the Explicit Dynamics analysis. To do so, drop the element midside nodes in the Mesh object. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 55 Approach • In the Explicit Dynamics analysis, under Analysis Settings, set the Precision option (under Solver Controls) to Double, to obtain the most consistent results between the Static Structural or Transient Structural system and the Explicit Dynamics system. • On the Brick Integration Scheme of all relevant bodies, use the Reduced option, to provide the most consistent results between the Static Structural or Transient Structural system and the Explicit Dynamics system. Such a selection amounts to a single integration point per lower order solid element. • For models containing Line or Surface bodies, the data transfer is limited to displacements only. In this mode, under Analysis Settings, the Static Damping option (under Damping) should be used to remove any dynamic oscillations in the stress state due to the imposed static displacements. • The temperature state is also transferred to the Explicit Dynamics analysis. The Unit System is taken care of automatically, and Internal Energy due to difference in temperature will be added to each element based on: Einternal = Einternal + Cp(T-Tref) Where: Cp = specific heat coefficient Tref = room temperature Please note that stresses may still dissipate because the thermal expansion coefficient is not taken into account in the Explicit Dynamics analysis. Example - Drop Test on Pressurized Container: Pre-stress condition: 56 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Transient stress distribution during drop test: Harmonic Analysis Harmonic analyses are used to determine the steady-state response of a linear structure to loads that vary sinusoidally (harmonically) with time, thus enabling you to verify whether or not your designs will successfully overcome resonance, fatigue, and other harmful effects of forced vibrations. Introduction In a structural system, any sustained cyclic load will produce a sustained cyclic or harmonic response. Harmonic analysis results are used to determine the steady-state response of a linear structure to loads that vary sinusoidally (harmonically) with time, thus enabling you to verify whether or not your designs will successfully overcome resonance, fatigue, and other harmful effects of forced vibrations. This analysis technique calculates only the steady-state, forced vibrations of a structure. The transient vibrations, which occur at the beginning of the excitation, are not accounted for in a harmonic analysis. In this analysis all loads as well as the structure’s response vary sinusoidally at the same frequency. A typical harmonic analysis will calculate the response of the structure to cyclic loads over a frequency range (a sine sweep) and obtain a graph of some response quantity (usually displacements) versus frequency. “Peak” responses are then identified from graphs of response vs. frequency and stresses are then reviewed at those peak frequencies. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 57 Approach Points to Remember A Harmonic Analysis is a linear analysis. Some nonlinearities, such as plasticity will be ignored, even if they are defined. All loads and displacements vary sinusoidally at the same known frequency (although not necessarily in phase). If the Reference Temperature is set as By Body and that temperature does not match the environment temperature, a thermally induced harmonic load will result (from the thermal strain assuming a nonzero thermal expansion coefficient). This thermal harmonic loading is ignored for all harmonic analysis. ANSYS Workbench offers two solution methods for harmonic analyses: Full and Mode Superposition. In the Full method, the harmonic response is obtained through a direct solution of the simultaneous equations of motion. In the Mode Superposition method, the harmonic response to a given loading condition is obtained by calculating the necessary linear combinations of the eigenvectors obtained in a modal analysis. In the latter case, it is advantageous for you to select an existing modal analysis directly (although ANSYS Workbench can automatically perform a modal analysis behind the scene) since calculating the eigenvectors is usually the most computationally expensive portion of the method. In this way, multiple harmonic analyses with different loading conditions could effectively reuse the eigenvectors. For more details, please refer to Harmonic Analysis Using Linked Modal Analysis System (p. 64). Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: From the Toolbox, drag the Harmonic Response template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: Both Young’s modulus (or stiffness in some form) and density (or mass in some form) must be defined. Material properties must be linear but can be isotropic or orthotropic, and constant or temperature-dependent. Nonlinear properties, if any, are ignored. Attach Geometry Basic general information about this topic ... for this analysis type: There are no specific considerations for a harmonic analysis. Define Part Behavior 58 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Basic general information about this topic ... for this analysis type: You can define a Point Mass for this analysis type. Define Connections Basic general information about this topic ... for this analysis type: Any nonlinear contact such as Frictional contact retains the initial status throughout the harmonic analysis. The stiffness contribution from the contact is based on the initial status and never changes. Joints are not allowed in a harmonic analysis. The stiffness as well as damping of springs is taken into account in a Full method of harmonic analysis. In a Mode Superposition harmonic analysis, the damping from springs is ignored. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: There are no specific considerations for harmonic analysis. Establish Analysis Settings Basic general information about this topic ... for this analysis type: For a harmonic analysis the basic controls are: • Options - Here you specify the frequency range and the number of solution points at which the harmonic analysis will be carried out as well as the solution method to use and the relevant controls. Two solution methods are available to perform harmonic analysis: the Mode Superposition method and the Direct Integration (full) method. – Mode Superposition method: In this method a modal analysis is first performed to compute the natural frequencies and mode shapes. Then the mode superposition solution is carried out where these mode shapes are combined to arrive at a solution. This is the default method, and generally provides results faster than the Full method. The Mode Superposition method cannot be used if you need to apply imposed (nonzero) displacements. This method also allows solutions to be clustered about the structure's natural frequencies. This results in a smoother, Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 59 Approach more accurate tracing of the response curve. The default method of equally spaced frequency points can result in missing the peak values. Without Cluster Option: With Cluster Option: A Store Results At All Frequencies option is also available to request that only minimal data be retained to supply just the harmonic results requested at the time of solution. 60 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Note With this option set to No, the addition of new frequency responses to a solved environment requires a new solution. The addition of new contour results or phase responses does not share this requirement; data from the closest available frequency is displayed (the reported frequency is noted on each result). However, data at an even closer frequency may be obtained with a new solution as needed. – Full method: Calculates all displacements and stresses in a single pass. Its chief disadvantages are: → It is more “expensive” in CPU time than the Mode Superposition method. → It does not allow clustered results, but rather requires the results to be evenly spaced within the specified frequency range. • Damping Controls allow you to specify damping for the structure in the harmonic analysis. Beta damping as well as constant damping ratio are available for a harmonic analysis. In addition material dependent damping can also be applied using the Engineering Data workspace. – Constant Damping Ratio: The simplest way of specifying damping in the structure, this value is a constant damping ratio. – Beta Damping: Defines a stiffness matrix multiplier for damping. Beta Damping is the option for Direct Input or Damping versus Frequency. For Direct Input, enter a Beta Damping value. For Damping versus Frequency, you can enter both a Frequency value and a Beta Damping value. – Material Damping: Two types of material-based damping, Material Dependent Damping and Constant Material Damping Coefficient are available for use with harmonic analyses. These are defined as material properties in Engineering Data. The Constant Material Damping Coefficient is used only in a Full method harmonic analysis. – Element Damping: You can also apply damping through spring-damper elements. The damping from these elements is used only in a Full method harmonic analysis. Note If multiple damping specifications are made the effect is cumulative. • Analysis Data Management settings enable you to save solution files from the harmonic analysis. The default behavior is to only keep the files required for postprocessing. You can use these controls to keep all files created during solution or to create and save the Mechanical APDL application database (db file). Define Initial Conditions Basic general information about this topic ... for this analysis type: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 61 Approach Initial condition is not applicable for Harmonic analyses. Apply Loads and Supports Basic general information about this topic ... for this analysis type: The following loads are allowed in a harmonic analysis: • Acceleration (p. 563) • Pressure (p. 568) • Pipe Pressure (p. 569) • Force (p. 570) (applied to a face, edge, or vertex) • Bearing Load (p. 573) • Moment (p. 577) • Given (Specified) Displacement • Remote Force • Remote Displacement (p. 555) • Line Pressure (p. 578) In a harmonic analysis the loads have the following characteristics: 62 • You can apply multiple loads to the same face. • All loads must be sinusoidally time-varying. • Transient effects are not calculated. • All loads must have the same frequency. • Loads can be out of phase with each other. You can specify a phase shift using the Phase Angle Details view entry for each load. You can specify the preferred unit for phase angle (in fact all angular inputs) to be degrees or radians using the Units toolbar. • Thermal Condition is not supported. • Any type of linear Support can be used in harmonic analyses. The Compression Only support is nonlinear but will behave linearly in harmonic analyses similar to a Frictionless Support, so it should not be utilized in order to avoid confusion. • Pressure loads and Force loads can be applied, with magnitude and phase angle input. Line Pressure loads allow magnitude input but no phase angle input. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Remote Force, Moment, and Acceleration loads may be defined, although these loads are assumed to act at a phase angle of zero. • The Bearing Load, as shown below, acts on one side of the cylinder. In harmonic analyses, you may expect that the other side of the cylinder is loaded in reverse, but the applied load simply reverses sign (goes in tension). Therefore the use of Bearing Loads is not recommended. Solve Basic general information about this topic ... for this analysis type: Solution Information continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. Review Results Basic general information about this topic ... for this analysis type: Two types of results can be requested for harmonic analyses: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 63 Approach • Contour plots include stress, elastic strain, and deformation, and are basically the same as those for other analyses. For these results, you must specify a frequency and phase angle. You can then see the total response of the structure at a given point in time, as shown below. Since each node may have different phase angles from one another, the complex response can also be animated to see the time-dependent motion. • Frequency Response and Phase Response charts which give data at a particular location over a frequency range. Graphs can be either Frequency Response graphs that display how the response varies with frequency or Phase Response plots that show how much a response lags behind the applied loads. Note You can create a contour result from a Frequency Response result type in a Harmonic Analysis using the Create Contour Result From Result feature. This feature creates a new result object in the tree with the same type, orientation, frequency, and phase angle as the frequency result type. Harmonic Analysis Using Linked Modal Analysis System Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: As this analysis is linked to (or based on) modal responses, a modal analysis is a prerequisite. This setup allows the two analysis systems to share resources such as engineering data, geometry and boundary condition type definitions made in modal analysis. Note The Mode Superposition harmonic is allowed to be linked to a pre-stressed modal analysis. 64 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types From the Toolbox, drag a Modal template to the Project Schematic. Then, drag a Harmonic Response template directly onto the Solution cell of the Modal template. Establish Analysis Settings Basic general information about this topic ... for this analysis type: Options - Only the Mode Superposition option is applicable, and therefore is read-only. Also, Mode Frequency Range is not applicable because available modes are defined in the Modal system. Output Controls - You can request Stress, Strain, Nodal Force, and Reaction results to be calculated. For better performance, you can also choose to have these results expanded from Harmonic or Modal solutions. Define Initial Conditions Basic general information about this topic ... for this analysis type: The harmonic analysis must point to a modal analysis in the Modal initial conditions object. The modal analysis must extract enough modes to cover the frequency range. A conservative rule of thumb is to extract enough modes to cover 1.5 times the maximum frequency in the excitation. Apply Loads and Supports Basic general information about this topic ... for this analysis type: The following loads are allowed for the linked analysis: • Acceleration (p. 563) • Pressure (p. 568) • Pipe Pressure (p. 569) • Force (p. 570) (applied to a face, edge, or vertex) • Line Pressure (p. 578) • Bearing Load (p. 573) • Moment (p. 577) • Remote Force (p. 572) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 65 Approach Note Remote Force is not supported for vertex scoping. Also, Moment is not supported for vertex scoping on 3-D solid bodies because a beam entity is created for the load application. Magnetostatic Analysis Introduction Magnetic fields may exist as a result of a current or a permanent magnet. In the Mechanical application you can perform 3-D static magnetic field analysis. You can model various physical regions including iron, air, permanent magnets, and conductors. Typical uses for a magnetostatic analysis are as follows: • Electric machines • Transformers • Induction heating • Solenoid actuators • High-field magnets • Nondestructive testing • Magnetic stirring • Electrolyzing cells • Particle accelerators • Medical and geophysical instruments. Points to Remember • This analysis is applicable only to 3-D geometry. • The geometry must consist of a single solid multibody part. • A magnetic field simulation requires that air surrounding the physical geometry be modeled as part of the overall geometry. The air domain can be easily modeled in DesignModeler using the Enclosure feature. Ensure that the resulting model is a single multibody part which includes the physical geometry and the air. • In many cases, only a symmetric portion of a magnetic device is required for simulation. The geometry can either be modeled in full symmetry in the CAD system, or in partial symmetry. DesignModeler has a Symmetry feature that can slice a full symmetry model, or identify planes of symmetry for a partial symmetry model. This information is passed to the Mechanical application for convenient application of symmetry plane boundary conditions. • A Magnetostatic analysis supports a multi-step solution. Preparing the Analysis Create Analysis System Basic general information about this topic 66 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types ... for this analysis type: From the Toolbox, drag the Magnetostatic template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: • Magnetic field simulation support 4 categories of material properties: 1. Linear “soft” magnetic materials - typically used in low saturation cases. A Relative Permeability is required. This may be constant, or orthotropic with respect to the coordinate system of the body (See Details view). Orthotropic properties are often used to simulate laminate materials. 2. Linear “hard” magnetic materials - used to model permanent magnets. The demagnetization curve of the magnet is assumed to be linear. Residual Induction and Coercive Force are required. 3. Nonlinear “soft” magnetic material - used to model devices which undergo magnetic saturation. A B-H curve is required. For orthotropic materials, you can assign the BH curve in any of the orthotropic directions, while specifying a constant Relative Permeability in the other directions. (Specifying a value of “0” for Relative Permeability will make use of the B-H curve in that direction.) 4. Nonlinear “hard” magnetic material - used to model nonlinear permanent magnets. A B-H curve modeling the material demagnetization curve is required. • When an Emag license is being used only the following material properties are allowed: Isotropic Resistivity, Orthotropic Resistivity, Relative Permeability, Relative Permeability (Orthotropic), Coercive Force & Residual Induction, B-H Curve, B-H Curve (Orthotropic), Demagnetization B-H Curve. You may have to turn the filter off in the Engineering Data workspace to suppress or delete those material properties/models which are not supported for this license. • Conductor bodies require a Resistivity material property. Solid source conductor bodies can be constant or orthotropic with respect to the coordinate system of the body. Stranded source conductor bodies can only be modeled as isotropic materials. • For convenience, a library of common B-H curves for soft magnetic material is supplied with the product. Use the Import tool in Engineering Data to review and retrieve curves for use. Note In a magnetostatic analysis, you can orient a polarization axis for a Linear or Nonlinear Hard material in either the positive or negative x direction with respect to a local or global coordinate system. Use the Material Polarization setting in the Details view for each body to establish this direction. The Material Polarization setting appears only if a hard material property is defined for the body. For a cylindrical coordinate system, a positive x polarization is in the positive radial direction, and a negative x polarization is in the negative radial direction. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 67 Approach Attach Geometry Basic general information about this topic ... for this analysis type: There are no specific considerations for a magnetostatic analysis. Define Part Behavior Basic general information about this topic ... for this analysis type: There are no specific considerations for a magnetostatic analysis. Define Connections Basic general information about this topic ... for this analysis type: Connections are not supported in a magnetostatic analysis. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: • Although your body is automatically meshed at solve time, it is recommended that you select the Electromagnetic Physics Preference in the Details view of the Mesh object folder. • Solution accuracy is dependent on mesh density. Accurate force or torque calculations require a fine mesh in the air regions surrounding the bodies of interest. • The use of pyramid elements in critical regions should be minimized. Pyramid elements are used to transition from hexagonal to tetrahedral elements. You can eliminate pyramid elements from the model by specifying Tetrahedrons using a Method mesh control tool. Establish Analysis Settings Basic general information about this topic ... for this analysis type: The basic controls are: Step Controls (p. 529): used to specify the end time of a step in a single or multiple step analysis. 68 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Multiple steps are needed if you want to change load values, the solution settings, or the solution output frequency over specific steps. Typically you do not need to change the default values. Solver Controls (p. 533) allow you to select either a direct or iterative solver. By default the program will use the direct solver. Convergence is guaranteed with the direct solver. Use the Iterative solver only in cases where machine memory is an issue. The solution is not guaranteed to converge for the iterative solver. Nonlinear Controls (p. 542) allow you to modify convergence criteria and other specialized solution controls. These controls are used when your solution is nonlinear such as with the use of nonlinear material properties (B-H curve). Typically you will not need to change the default values for this control. CSG convergence is the criteria used to converge the magnetic field. CSG represents magnetic flux. AMPS convergence is only used for temperature-dependent electric current conduction for solid conductor bodies. AMPS represents current. Output Controls (p. 545) allow you to specify the time points at which results should be available for postprocessing. A multi-step analysis involves calculating solutions at several time points in the load history. However you may not be interested in all of the possible results items and writing all the results can make the result file size unwieldy. You can restrict the amount of output by requesting results only at certain time points or limit the results that go onto the results file at each time point. Analysis Data Management (p. 549) settings enable you to save solution files from the magnetostatic analysis. The default behavior is to only keep the files required for postprocessing. You can use these controls to keep all files created during solution or to create and save the Mechanical APDL application database (db file). Define Initial Conditions Basic general information about this topic ... for this analysis type: There is no initial condition specification for a magnetostatic analysis. Apply Loads and Supports Basic general information about this topic ... for this analysis type: • You can apply electromagnetic boundary conditions and excitations in the Mechanical application. See Electromagnetic Boundary Conditions and Excitations (p. 591) for details. • Boundary conditions may also be applied on symmetry planes via a Symmetry. A Symmetry folder allows support for Electromagnetic Symmetry, Electromagnetic AntiSymmetry, and Electromagnetic Periodicity conditions. Solve Basic general information about this topic Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 69 Approach ... for this analysis type: The Solution Information object provides some tools to monitor solution progress in the case of a nonlinear magnetostatic analysis. Solution Output continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. Any convergence data output in this printout can be graphically displayed as explained in the Solution Information section. Adaptive mesh refinement is available for magnetostatic analyses. Review Results Basic general information about this topic ... for this analysis type: A magnetostatic analysis offers several results for viewing. Results may be scoped to bodies and, by default, all bodies will compute results for display. For Inductance or Flux Linkage, define these objects prior to solution. If you define these after a solution, you will need to re-solve. Random Vibration Analysis Introduction This analysis enables you to determine the response of structures to vibration loads that are random in nature. An example would be the response of a sensitive electronic component mounted in a car subjected to the vibration from the engine, pavement roughness, and acoustic pressure. Loads such as the acceleration caused by the pavement roughness are not deterministic, that is, the time history of the load is unique every time the car runs over the same stretch of road. Hence it is not possible to predict precisely the value of the load at a point in its time history. Such load histories, however, can be characterized statistically (mean, root mean square, standard deviation). Also random loads are non-periodic and contain a multitude of frequencies. The frequency content of the time history (spectrum) is captured along with the statistics and used as the load in the random vibration analysis. This spectrum, for historical reasons, is called Power Spectral Density or PSD. In a random vibration analysis since the input excitations are statistical in nature, so are the output responses such as displacements, stresses, and so on. Typical applications include aerospace and electronic packaging components subject to engine vibration, turbulence and acoustic pressures, tall buildings under wind load, structures subject to earthquakes, and ocean wave loading on offshore structures. Points to Remember • 70 The excitation is applied in the form of Power Spectral Density (PSD). The PSD is a table of spectral values vs. frequency that captures the frequency content. The PSD captures the frequency and mean square amplitude content of the load’s time history. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types • The square root of the area under a PSD curve represents the root mean square (rms) value of the excitation. The unit of the spectral value of acceleration, for example, is G2/Hertz. • The input excitation is expected to be stationary (the average mean square value does not change with time) with a zero mean. • This analysis is based on the mode superposition method. Hence a modal analysis that extracts the natural frequencies and mode shapes is a prerequisite. • This feature covers one type of PSD excitation only- base excitation. • The base excitation could be an acceleration PSD (either in acceleration2 units or in G2 units), velocity PSD or displacement PSD. • The base excitation is applied in the specified direction to all entities that have a Fixed Support boundary condition. Other support points in a structure such as Frictionless Surface are not excited by the PSD. • Multiple uncorrelated PSDs can be applied. This is useful if different, simultaneous excitations occur in different directions. • If stress/strain results are of interest from the random vibration analysis then you will need to request stress/strain calculations in the modal analysis itself. Only displacement results are available by default. • Postprocessing: – The results output by the solver are one sigma or one standard deviation values (with zero mean value). These results follow a Gaussian distribution. The interpretation is that 68.3% of the time the response will be less than the standard deviation value. – You can scale the result by 2 times to get the 2 sigma values. The response will be less than the 2 sigma values 95.91% of the time and 3 sigma values 99.737% of the time. – The Coordinate System setting for result objects is, by default, set to Solution Coordinate System and cannot be changed because the results only have meaning when viewed in the solution coordinate system. – Since the directional results from the solver are statistical in nature they cannot be combined in the usual way. For example the X, Y, and Z displacements cannot be combined to get the magnitude of the total displacement. The same holds true for other derived quantities such as principal stresses. – A special algorithm by Segalman-Fulcher is used to compute a meaningful value for equivalent stress. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: Because a random vibration analysis is based on modal responses, a modal analysis is a required prerequisite. The requirement then is for two analysis systems, a modal analysis system and a random vibration analysis system that share resources, geometry, and model data. From the Toolbox, drag a Modal template to the Project Schematic. Then, drag a Random Vibration template directly onto the Modal template. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 71 Approach Define Engineering Data Basic general information about this topic ... for this analysis type: Both Young’s modulus (or stiffness in some form) and density (or mass in some form) must be defined in the modal analysis. Material properties must be linear but can be isotropic or orthotropic, and constant or temperature-dependent. Nonlinear properties, if any, are ignored. Attach Geometry Basic general information about this topic ... for this analysis type: There are no specific considerations for a random vibration analysis. Define Part Behavior Basic general information about this topic ... for this analysis type: There are no specific considerations for a random vibration analysis. Define Connections Basic general information about this topic ... for this analysis type: Only linear behavior is valid in a random vibration analysis. Nonlinear elements, if any, are treated as linear. If you include contact elements, for example, their stiffnesses are calculated based on their initial status and are never changed. Joints are not allowed in a random vibration analysis. Only the stiffness of springs are taken into account in a random vibration analysis. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: There are no specific considerations for a random vibration analysis. Establish Analysis Settings Basic general information about this topic 72 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types ... for this analysis type: For a random vibration analysis the basic controls are: Options for Modal, Harmonic, Linear Buckling, Random Vibration, and Response Spectrum Analyses (p. 538). You can specify the number of modes to use from the modal analysis. A conservative rule of thumb is to include modes that cover 1.5 times the maximum frequency in the PSD excitation table. You can also exclude insignificant modes by setting a mode significance level between 0 (all modes selected) and 1 (no modes selected). Damping Controls (p. 542) allow you to specify damping for the structure in the random vibration analysis. Beta damping as well as constant damping ratio are available for a random vibration analysis. In addition material dependent damping can also be applied using the Engineering Data workspace. Analysis Data Management (p. 549) settings enable you to save solution files from the Random Vibration analysis. The default behavior is to only keep the files required for postprocessing. You can use these controls to keep all files created during solution or to create and save a the Mechanical APDL application database (db file). Note The Inertia Relief option (under Analysis Settings) for an upstream static structural analysis is not supported in a random vibration analysis. Define Initial Conditions Basic general information about this topic ... for this analysis type: You must point to a modal analysis in the Initial Condition environment field. The modal analysis must extract enough modes to cover the PSD frequency range. A conservative rule of thumb is to extract enough modes to cover 1.5 times the maximum frequency in the PSD excitation. When a PSD analysis is linked to a modal analysis, additional solver files must be saved to achieve the PSD solution. (See Analysis Data Management (p. 549).) If the files were not saved, then the modal analysis has to be solved again and the files saved. Apply Loads and Supports Basic general information about this topic ... for this analysis type: • Any support boundary condition must be defined in the modal analysis itself. You cannot add any new support boundary conditions in the random vibration analysis. • The only applicable load is a PSD Base Excitation of spectral value vs. frequency. • Remote displacement cannot coexist with other boundary condition types (for example, fixed support or displacement) on the same location for excitation. The remote displacement will be ignored due to conflict with other boundary conditions. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 73 Approach • Four types of base excitation are supported: PSD Acceleration, PSD G Acceleration, PSD Velocity, and PSD Displacement. • Each PSD base excitation should be given a direction in the nodal coordinate of the excitation points. • Multiple PSD excitations (uncorrelated) can be applied. Typical usage is to apply 3 different PSDs in the X, Y, and Z directions. Correlation between PSD excitations is not supported. Solve Basic general information about this topic ... for this analysis type: Solution Information continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. In addition to solution progress you will also find the participation factors for each PSD excitation. The solver output also has a list of the relative importance of each mode in the modal covariance matrix listing. Review Results Basic general information about this topic ... for this analysis type: 74 • If stress/strain results are of interest from the random vibration analysis then you will need to request stress/strain calculations in the modal analysis itself. You can use the Output Controls under Analysis Settings in the modal analysis for this purpose. Only displacement results are available by default. • Applicable results are Directional (X/Y/Z) Displacement/Velocity/Acceleration, normal and shear stresses/strains and equivalent stress. These results can be displayed as contour plots. • The displacement results are relative to the base of the structure (the fixed supports). • The velocity and acceleration results include base motion effects (absolute). • Since the directional results from the solver are statistical in nature they cannot be combined in the usual way. For example the X, Y, and Z displacements cannot be combined to get the magnitude of the total displacement. The same holds true for other derived quantities such as principal stresses. • For directional acceleration results, an option is provided to displayed acceleration in G (gravity) by selecting Yes in the Acceleration in G field. • By default the 1 σ results are displayed. You can apply a scale factor to review any multiples of σ such as 2 σ or 3 σ. The Details view as well as the legend for contour results also reflects the percentage (using Gaussian distribution) of time the response is expected to be below the displayed values. • Meaningful equivalent stress is computed using a special algorithm by Segalman-Fulcher. Note that the probability distribution for this equivalent stress is neither Gaussian nor is the mean value zero. However, the “3 σ” rule (multiplying the RMS value by 3) yields a conservative estimate on the upper bound of the equivalent stress. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types • Force Reaction and Moment Reaction probes can be scoped to a Remote Displacement boundary condition to view Reactions Results. Response Spectrum Analysis Introduction Response spectrum analyses are widely used in civil structure designs, for example, high-rise buildings under wind loads. Another prime application is for nuclear power plant designs under seismic loads. A response spectrum analysis has similarities to a random vibration analysis. However, unlike a random vibration analysis, responses from a response spectrum analysis are deterministic maxima. For a given excitation, the maximum response is calculated based upon the input response spectrum and the method used to combine the modal responses. The combination methods available are: the Square Root of the Sum of the Squares (SRSS), the Complete Quadratic Combination (CQC) and the Rosenblueth’s Double Sum Combination (ROSE). See Response Spectrum - Options Control Settings (p. 541) for further details. Points to Remember • The excitation is applied in the form of a response spectrum. The response spectrum can have displacement, velocity or acceleration units. For each spectrum value, there is one corresponding frequency. • The excitation must be applied at fixed degrees of freedom. • The response spectrum is calculated based on modal responses. A modal analysis is therefore a prerequisite. • If response strain/stress is of interest, then the modal strain and the modal stress need to be determined in the modal analysis. • Because a new solve is required for each requested output, for example, displacement, velocity and acceleration, the content of Commands objects inserted in a response spectrum analysis is limited to SOLUTION commands. • The results from the ANSYS solver are displayed as the model’s contour plot. The results are in terms of the maximum response. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: Because a response spectrum analysis is based on modal responses, a modal analysis is a required prerequisite. The modal analysis system and the response spectrum analysis system must share resources, geometry, and model data. From the Toolbox, drag a Modal template to the Project Schematic. Then, drag a Response Spectrum template directly onto the Modal template. Define Engineering Data Basic general information about this topic Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 75 Approach ... for this analysis type: Material properties must be defined in a modal analysis. Nonlinear material properties are not allowed. Attach Geometry Basic general information about this topic ... for this analysis type: There are no specific considerations for a response spectrum analysis. Define Part Behavior Basic general information about this topic ... for this analysis type: There are no specific considerations for a response spectrum analysis. Define Connections Basic general information about this topic ... for this analysis type: Nonlinear element types are not supported. They will be treated as linear. For example, the contact stiffness is calculated using the initial status without convergence check. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: There are no specific considerations for a response spectrum analysis. Establish Analysis Settings Basic general information about this topic ... for this analysis type: Options for Response Spectrum Analyses: 76 • Specify the Number of Modes To Use for the response spectrum calculation. It is recommended to include the modes whose frequencies span 1.5 times the maximum frequency defined in the input response spectrum. • Specify the Spectrum Type to be used for response spectrum calculation as either Single Point or Multiple Points. If the input response spectrum is applied to all fixed degrees of freedom, use Single Point, otherwise use Multiple Points. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types • Specify the Modes Combination Type to be used for response spectrum calculation. In general, the SRSS method is more conservative than the CQC and the ROSE methods. Note The Inertia Relief option (under Analysis Settings) for an upstream static structural analysis is not supported in a response spectrum analysis. Output Controls (p. 545). By default, only displacement responses are calculated. To include velocity and/or acceleration responses, set their respective Output Controls to Yes. Damping Controls (p. 542) allow you to specify damping for the structure in the response spectrum analysis. Note that damping will only have an effect if a damping-dependent spectrum table is available; the effect of damping in a response spectrum analysis is applied by looking up the spectrum value at each frequency for the specified or calculated amount of damping in each material. For the CQC mode combination type, a non-zero constant damping ratio is required. Analysis Data Management (p. 549) settings enable you to save solution files from the response spectrum analysis. An option to save the Mechanical APDL application database (db file) from the analysis is provided. Define Initial Conditions Basic general information about this topic ... for this analysis type: A specific Modal Environment must be set as an initial condition/environment for response spectrum analysis to be solved. Apply Loads and Supports Basic general information about this topic ... for this analysis type: • Supported boundary condition types include fixed support, displacement, remote displacement and body-to-ground spring. If one or more fixed supports are defined in the model, the input excitation response can be applied to all fixed supports. • Remote displacement cannot coexist with other boundary condition types (for example, fixed support or displacement) on the same location for excitation. The remote displacement will be ignored due to conflict with other boundary conditions. • Note that the All boundary condition types for Single Point Response Spectrum only includes those fixed degree of freedoms defined using Fixed Support, Displacement, Remote Displacement and Body-to-Ground Spring. To apply an RS load to All boundary condition types for Single Point Response Spectrum, at least one allowed boundary condition must be defined. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 77 Approach • For a Single Point spectrum type, input excitation spectrums are applied to all boundary condition types defined in the model. For Multiple Points however, each input excitation spectrum is associated to only one boundary condition type. • Three types of input excitation spectrum are supported: displacement input excitation (RS Displacement), velocity input excitation (RS Velocity) and acceleration input excitation (RS Acceleration). See RS Base Excitation (p. 580) for further details. • The input excitation spectrum direction is defined in the global coordinate system for Single Point spectrum analysis. For Multiple Points spectrum analysis, however, the input excitation is defined in the nodal coordinate systems (if any) attached to the constrained nodes. • More than one input excitation, with any different combination of spectrum types, are allowed for the response spectrum analysis. • Specify option to include or not include contribution of high frequency modes in the total response calculation by setting Missing Mass Effect to Yes or No. The option for including the modes is normally required for nuclear power plant design. • Specify option to include or not include rigid responses to the total response calculation by setting Rigid Response Effect to Yes or No. The rigid responses normally occur in the frequency range that is lower than that of missing mass responses, but is higher than that of periodic responses. • Missing Mass Effect and Rigid Response Effect are only applicable to RS Acceleration excitation. • For a Single Point spectrum type, the entire table of input excitation spectrum can be scaled using the Scale Factor setting. The factor must be greater than 0.0. The default is 1.0. Solve Basic general information about this topic ... for this analysis type: It is recommended that you review the Solution Information page for any warnings or errors that might occur during the ANSYS solve. Some warning messages will still enable the solve. Review Results Basic general information about this topic ... for this analysis type: 78 • To view strain/stress results, a selection must be made in Output Controls of the modal analysis. By default, only displacement results are available. • Applicable results are directional (X/Y/Z) displacement, velocity and acceleration. If strain/stress are requested, applicable results are normal strain and stress, shear strain and stress, and equivalent stress. • Equivalent stress is a derived stress calculated using component stresses. • Results are displayed as a contour plot on the model. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types • In addition to standard files generated by the Mechanical APDL application after the solve, the file Displacement.mcom is also made available. If the Output Controls are set to Yes for Calculate Velocity and/or Calculate Acceleration, the corresponding Velocity.mcom and/or Acceleration.mcom are also made available. These files contain the combination instructions including mode coefficients. • Force Reaction and Moment Reaction probes can be scoped to a Remote Displacement boundary condition to view Reactions Results. Static Structural Analysis Introduction A static structural analysis determines the displacements, stresses, strains, and forces in structures or components caused by loads that do not induce significant inertia and damping effects. Steady loading and response conditions are assumed; that is, the loads and the structure's response are assumed to vary slowly with respect to time. A static structural load can be performed using the ANSYS or Samcef solver. The types of loading that can be applied in a static analysis include: • Externally applied forces and pressures • Steady-state inertial forces (such as gravity or rotational velocity) • Imposed (nonzero) displacements • Temperatures (for thermal strain) Point to Remember A static structural analysis can be either linear or nonlinear. All types of nonlinearities are allowed large deformations, plasticity, stress stiffening, contact (gap) elements, hyperelasticity and so on. This chapter focuses on linear static analyses, with brief references to nonlinearities. Details of how to handle nonlinearities are described in Nonlinear Controls (p. 542). Note that available nonlinearities can differ from one solver to another. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: From the Toolbox, drag a Static Structural or Static Structural (Samcef) template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: Material properties can be linear or nonlinear, isotropic or orthotropic, and constant or temperature-dependent. You must define stiffness in some form (for example, Young's Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 79 Approach modulus, hyperelastic coefficients, and so on). For inertial loads (such as Standard Earth Gravity), you must define the data required for mass calculations, such as density. Attach Geometry Basic general information about this topic ... for this analysis type: When 2D geometry is used, only the 2D axisymmetric behavior is available for the Samcef solver. Define Part Behavior Basic general information about this topic ... for this analysis type: You can define a Point Mass for this analysis type. A “rigid” part is essentially a point mass connected to the rest of the structure via joints. Hence in a static structural analysis the only applicable loads on a rigid part are acceleration and rotational velocity loads. You can also apply loads to a rigid part via joint loads. The output from a rigid part is the overall motion of the part plus any force transferred via that part to the rest of the structure. Rigid behavior cannot be used with Samcef. If your model includes nonlinearities such as large deflection or hyperelasticity, the solution time can be significant due to the iterative solution procedure. Hence you may want to simplify your model if possible. For example you may be able to represent your 3-D structure as a 2-D plane stress, plane strain, or axisymmetric model or you may be able to reduce your model size through the use of symmetry or antisymmetry surfaces. Similarly if you can omit nonlinear behavior in one or more parts of your assembly without affecting results in critical regions it will be advantageous to do so. Define Connections Basic general information about this topic ... for this analysis type: Contact, joints, springs, beams, mesh connections, and end releases are all valid in a static structural analysis. For the Samcef solver, only contacts, springs, and beams are supported. Joints are not supported. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: 80 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Provide an adequate mesh density on contact surfaces to allow contact stresses to be distributed in a smooth fashion. Likewise, provide a mesh density adequate for resolving stresses; areas where stresses or strains are of interest require a relatively fine mesh compared to that needed for displacement or nonlinearity resolution. If you want to include nonlinearities, the mesh should be able to capture the effects of the nonlinearities. For example, plasticity requires a reasonable integration point density (and therefore a fine element mesh) in areas with high plastic deformation gradients. Establish Analysis Settings Basic general information about this topic ... for this analysis type: For simple linear static analyses you typically do not need to change these settings. For more complex analyses the basic controls are: Large Deflection (p. 534) is typically needed for slender structures. A rule of thumb is that you can use large deflection if the transverse displacements in a slender structure are more than 10% of the thickness. Small deflection and small strain analyses assume that displacements are small enough that the resulting stiffness changes are insignificant. Setting Large Deflection to On will take into account stiffness changes resulting from changes in element shape and orientation due to large deflection, large rotation, and large strain. Therefore the results will be more accurate. However this effect requires an iterative solution. In addition it may also need the load to be applied in small increments. Therefore, the solution may take longer to solve. You also need to turn on large deflection if you suspect instability (buckling) in the system. Use of hyperelastic materials also requires large deflection to be turned on. Step Controls (p. 529) are used to i) control the time step size and other solution controls and ii) create multiple steps when needed. Typically analyses that include nonlinearities such as large deflection or plasticity require control over time step sizes as outlined in the Automatic Time Stepping (p. 527) section. Multiple steps are required for activation/deactivation of displacement loads or pretension bolt loads. This group can be modified on a per step basis. Note Time Stepping is available for any solver. Output Controls (p. 545) allow you to specify the time points at which results should be available for postprocessing. In a nonlinear analysis it may be necessary to perform many solutions at intermediate load values. However i) you may not be interested in all the intermediate results and ii) writing all the results can make the results file size unwieldy. This group can be modified on a per step basis except for Stress and Strain. Nonlinear Controls (p. 542) allow you to modify convergence criteria and other specialized solution controls. Typically you will not need to change the default values for this control. This group can be modified on a per step basis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 81 Approach Analysis Data Management (p. 549) settings enable you to save specific solution files from the Static Structural analysis for use in other analyses. You can set the Future Analysis field to Pre-Stressed Analysis if you intend to use the static structural results in a subsequent Modal or Linear Buckling (Linear Buckling is applicable to Static Structural systems only) analysis. A typical example is the large tensile stress induced in a turbine blade under centrifugal load. This causes significant stiffening of the blade resulting in much higher, realistic natural frequencies in a modal analysis. More details are available in the section Define Initial Conditions (p. 12). Note Scratch Solver Files, Save ANSYS db, Solver Units, and Solver Unit System are applicable to Static Structural systems only. Define Initial Conditions Basic general information about this topic ... for this analysis type: Initial condition is not applicable for Static Structural analyses. Apply Loads and Supports Basic general information about this topic ... for this analysis type: For a static structural analysis applicable loads/supports are all inertial and structural loads, and all structural supports. For the Samcef solver, the following loads and supports are not available: Hydrostatic Pressure, Bearing Load, Bolt Pretension, Joint Load, Fluid Solid Interface, Motion Loads, Compression Only Support, Elastic Support. Loads and supports vary as a function of time even in a static analysis as explained in the Role of Time in Tracking (p. 525). In a static analysis, the load’s magnitude could be a constant value or could vary with time as defined in a table or via a function. Details of how to apply a tabular or function load are described in Specifying Load Values (p. 621). In addition, see the Apply Loads and Supports section for more information about time stepping and ramped loads. 82 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Note A static analysis can be followed by a “pre-stressed” analysis such as modal or linear (eigenvalue) buckling analysis. In this subsequent analysis the effect of stress on stiffness of the structure (stress-stiffness effect) is taken into account. If the static analysis has a pressure or force load applied on faces (3D) or edges (2-D) this could result in an additional stiffness contribution called “pressure load stiffness” effect. This effect plays a significant role in linear (eigenvalue) buckling analysis. This additional effect is computed during the eigen analysis using the pressure or force value calculated at the time in the static analysis from which the perturbation occurs. Please see the Applying Pre-Stress Effects section of the Eigen Response Analysis for more information on this topic. Solve Basic general information about this topic ... for this analysis type: When performing a nonlinear analysis you may encounter convergence difficulties due to a number of reasons. Some examples may be initially open contact surfaces causing rigid body motion, large load increments causing non-convergence, material instabilities, or large deformations causing mesh distortion that result in element shape errors. To identify possible problem areas some tools are available under Solution Information object Details view. Solution Output continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. Any convergence data output in this printout can be graphically displayed as explained in the Solution Information section. You can display contour plots of Newton-Raphson Residuals in a nonlinear static analysis. Such a capability can be useful when you experience convergence difficulties in the middle of a step, where the model has a large number of contact surfaces and other nonlinearities. When the solution diverges identifying regions of high Newton-Raphson residual forces can provide insight into possible problems. Result Tracker (applicable to Static Structural systems only) is another useful tool that allows you to monitor displacement and energy results as the solution progresses. This is especially useful in case of structures that possibly go through convergence difficulties due to buckling instability. Review Results Basic general information about this topic ... for this analysis type: All structural result types except frequencies are available as a result of a static structural analysis. You can use a Solution Information object to track, monitor, or diagnose problems that arise during a solution. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 83 Approach Once a solution is available you can contour the results or animate the results to review the response of the structure. As a result of a nonlinear static analysis you may have a solution at several time points. You can use probes to display the variation of a result item as the load increases. An example might be large deformation analyses that result in buckling of the structure. In these cases it is also of interest to plot one result quantity (for example, displacement at a vertex) against another results item (for example, applied load). You can use the Charts feature to develop such charts. Steady-State Thermal Analysis Introduction You can use a steady-state thermal analysis to determine temperatures, thermal gradients, heat flow rates, and heat fluxes in an object that are caused by thermal loads that do not vary over time. A steadystate thermal analysis calculates the effects of steady thermal loads on a system or component. Engineers often perform a steady-state analysis before performing a transient thermal analysis, to help establish initial conditions. A steady-state analysis also can be the last step of a transient thermal analysis, performed after all transient effects have diminished. Point to Remember A steady-state thermal analysis may be either linear, with constant material properties; or nonlinear, with material properties that depend on temperature. The thermal properties of most material do vary with temperature, so the analysis usually is nonlinear. Including radiation effects or temperature dependent convection coefficient also makes the analysis nonlinear. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: From the Toolbox, drag a Steady-State Thermal template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: Thermal Conductivity must be defined for a steady-state thermal analysis. Thermal Conductivity can be isotropic or orthotropic, and constant or temperature-dependent. Attach Geometry Basic general information about this topic ... for this analysis type: 84 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types There are no specific considerations for a steady-state thermal analysis. Define Part Behavior Basic general information about this topic ... for this analysis type: There are no specific considerations for a steady-state thermal analysis. Define Connections Basic general information about this topic ... for this analysis type: In a thermal analysis only contact is valid. Any joints or springs are ignored. With contact the initial status is maintained throughout the thermal analysis, that is, any closed contact faces will remain closed and any open contact faces will remain open for the duration of the thermal analysis. Heat conduction across a closed contact face is set to a sufficiently high enough value (based on the thermal conductivities and the model size) to model perfect contact with minimal thermal resistance. If needed, you can model imperfect contact by manually inputting a Thermal Conductance value. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: There are no specific considerations for steady-state thermal analysis itself. However if the temperatures from this analysis are to be used in a subsequent structural analysis the mesh must be identical. Therefore in this case you may want to make sure the mesh is fine enough for structural analysis. Establish Analysis Settings Basic general information about this topic ... for this analysis type: For a steady-state thermal analyses you typically do not need to change these settings. The basic controls are: Step Controls (p. 529) allow you to control the rate of loading which could be important in a steady-state thermal analysis if the material properties vary rapidly with temperature. When such nonlinearities are present it may be necessary to apply the loads in small increments and perform solutions at these intermediate loads to achieve convergence. You may wish to use multiple steps if you a) want to analyze several different loading scenarios within the same analysis or b) if you want to change the analysis settings such as the time step size or the solution output frequency over specific time ranges. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 85 Approach Output Controls (p. 545) allow you to specify the time points at which results should be available for postprocessing. In a nonlinear analysis it may be necessary to perform many solutions at intermediate load values. However i) you may not be interested in all the intermediate results and ii) writing all the results can make the results file size unwieldy. In this case you can restrict the amount of output by requesting results only at certain time points. Nonlinear Controls (p. 542) allow you to modify convergence criteria and other specialized solution controls. Typically you will not need to change the default values for this control. Analysis Data Management (p. 549) settings enable you to save specific solution files from the steady-state thermal analysis for use in other analyses. Define Initial Conditions Basic general information about this topic ... for this analysis type: For a steady-state thermal analysis you can specify an initial temperature value. This uniform temperature is used during the first iteration of a solution as follows: • To evaluate temperature-dependent material properties. • As the starting temperature value for constant temperature loads. Apply Loads and Supports Basic general information about this topic ... for this analysis type: The following loads are supported in a steady-state thermal analysis: • Temperature (p. 584) • Convection (p. 584) • Radiation (p. 586) • Heat Flow (p. 587) • Perfectly Insulated (p. 589) • Heat Flux (p. 589) • Internal Heat Generation (p. 590) • Imported Temperature (p. 605) • Imported Convection Coefficient (p. 603) Loads and supports vary as a function of time even in a static analysis as explained in the Role of Time in Role of Time in Tracking (p. 525). In a static analysis, the load’s magnitude could be a constant value or could vary with time as defined in a table or via a function. Details of how to apply a tabular or function load are described in Specifying Load Values (p. 621). In addition, see the Apply Loads and Supports section for more information about time stepping and ramped loads. 86 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Solve Basic general information about this topic ... for this analysis type: The Solution Information object provides some tools to monitor solution progress. Solution Output continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. Any convergence data output in this printout can be graphically displayed as explained in the Solution Information section. You can also insert a Result Tracker object under Solution Information. This tool allows you to monitor temperature at a vertex as the solution progresses. Review Results Basic general information about this topic ... for this analysis type: Applicable results are all thermal result types. Once a solution is available you can contour the results or animate the results to review the response of the structure. As a result of a nonlinear analysis you may have a solution at several time points. You can use probes to display the variation of a result item over the load history. Also of interest is the ability to plot one result quantity (for example, maximum temperature on a face) against another results item (for example, applied heat generation rate). You can use the Charts feature to develop such charts. Note that Charts are also useful to compare results between two analyses of the same model. Thermal-Electric Analysis Introduction A Steady-State Thermal-Electric Conduction analysis allows for a simultaneous solution of thermal and electric fields. This coupled-field capability models joule heating for resistive materials and contact electric conductance as well as Seebeck, Peltier, and Thomson effects for thermoelectricity, as described below. • Joule heating - Heating occurs in a resistive conductor carrying an electric current. Joule heating is proportional to the square of the current, and is independent of the current direction. Joule heating is also present and accounted for at the contact interface between bodies in inverse proportion to the contact electric conductance properties. (Note however that the Joule Heat results object will not display contact joule heating values. Only solid body joule heating is represented). • Seebeck effect - A voltage (Seebeck EMF) is produced in a thermoelectric material by a temperature difference. The induced voltage is proportional to the temperature difference. The proportionality coefficient is know as the Seebeck Coefficient (α). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 87 Approach • Peltier effect - Cooling or heating occurs at a junction of two dissimilar thermoelectric materials when an electric current flows through that junction. Peltier heat is proportional to the current, and changes sign if the current direction is reversed. • Thomson effect - Heat is absorbed or released in a non-uniformly heated thermoelectric material when electric current flows through it. Thomson heat is proportional to the current, and changes sign if the current direction is reversed. Points to Remember Electric loads may be applied to parts with electric properties and thermal loads may be applied to bodies with thermal properties. Parts with both physics properties can support both thermal and electric loads. See the Steady-state Thermal Analysis section and the Electric Analysis section of the help for more information about applicable loads, boundary conditions, and results types. In addition to calculating the effects of steady thermal and electric loads on a system or component, a Steady-State Thermal-Electric analysis supports a multi-step solution. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: From the Toolbox, drag the Thermal-Electric template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: To have Thermal and/or Electrical effects properly applied to the parts of your model, you need to define the appropriate material properties. For a steady-state analysis, the electrical property Resistivity is required for Joule Heating effects and Thermal Conductivity for thermal conduction effects. Seebeck/Peltier/Thomson effects require you to define the Seebeck Coefficient material property. Attach Geometry Basic general information about this topic ... for this analysis type: There are no specific considerations for a thermal-electric analysis. Define Part Behavior Basic general information about this topic ... for this analysis type: 88 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types There are no specific considerations for a thermal-electric analysis. Define Connections Basic general information about this topic ... for this analysis type: Contact across parts during a thermal-electric analysis consider thermal and/or electric effects based on the material properties of adjacent parts. That is, if both parts have thermal properties, thermal contact is applied and if both parts have electric properties, electric contact is applied. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: There are no specific considerations regarding meshing for a thermal-electric analysis. Establish Analysis Settings Basic general information about this topic ... for this analysis type: For a thermal-electric analysis, the basic controls are: Step Controls (p. 529): used to specify the end time of a step in a single or multiple step analysis. Multiple steps are needed if you want to change load values, the solution settings, or the solution output frequency over specific steps. Typically you do not need to change the default values. Typical thermal-electric problems contain temperature dependent material properties and are therefore nonlinear. Nonlinear Controls for both thermal and electrical effects are available and include Heat and Temperature convergence for thermal effects and Voltage and Current convergence for electric effects. The Program Controlled option for Nonlinear Formulation defaults to the Quasi option, but the Full option is used in cases when a Radiation load is present or when a distributed solver is used during the solution. Output Controls (p. 545) allow you to specify the time points at which results should be available for postprocessing. A multi-step analysis involves calculating solutions at several time points in the load history. However you may not be interested in all of the possible results items and writing all the results can make the result file size unwieldy. You can restrict the amount of output by requesting results only at certain time points or limit the results that go onto the results file at each time point. Analysis Data Management (p. 549) settings. The default Solver Controls setting for thermal-electric analysis is the Direct (Sparse) solver. The Iterative (PCG) solver may be selected as an alternative solver. If Seebeck effects are included, the solver is automatically set to Direct. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 89 Approach Define Initial Conditions Basic general information about this topic ... for this analysis type: There is no initial condition specification for a thermal-electric analysis. Apply Loads and Supports Basic general information about this topic ... for this analysis type: The following loads are supported in a Thermal-Electric analysis: • Voltage • Current • Coupling Condition • Temperature • Convection • Radiation • Heat Flow • Perfectly Insulated • Heat Flux • Internal Heat Generation Solve Basic general information about this topic ... for this analysis type: The Solution Information object provides some tools to monitor solution progress. Solution Output continuously updates any listing output from the solver and provides valuable information on the behavior of the model during the analysis. Any convergence data output in this printout can be graphically displayed as explained in the Solution Information section. Review Results Basic general information about this topic ... for this analysis type: Applicable results include all thermal and electric results. 90 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Once a solution is available, you can contour the results or animate the results to review the responses of the model. For the results of a multi-step analysis that has a solution at several time points, you can use probes to display variations of a result item over the steps. You may also wish to use the Charts feature to plot multiple result quantities against time (steps). For example, you could compare current and joule heating. Charts can also be useful when comparing the results between two analysis branches of the same model. Transient Structural and Rigid Dynamics Analyses A transient analysis, by definition, involves loads that are a function of time. In the Mechanical application, you can perform a transient analysis on either a flexible structure or a rigid assembly. For a flexible structure, the Mechanical application uses the ANSYS Mechanical APDL solver to solve a Transient Structural analysis, and for a rigid assembly, the Mechanical application uses the ANSYS Rigid Dynamics solver to solve a Rigid Dynamics analysis. Please see the following subsections based on your need. Transient Structural Analysis Rigid Dynamics Analysis Command Reference for Rigid Dynamics Systems Transient Structural Analysis Introduction You can perform a transient structural analysis (also called time-history analysis) in the Mechanical application using the transient structural analysis that specifically uses the ANSYS Mechanical APDL solver. This type of analysis is used to determine the dynamic response of a structure under the action of any general time-dependent loads. You can use it to determine the time-varying displacements, strains, stresses, and forces in a structure as it responds to any transient loads. The time scale of the loading is such that the inertia or damping effects are considered to be important. If the inertia and damping effects are not important, you might be able to use a static analysis instead. Points to Remember A transient structural analysis can be either linear or nonlinear. All types of nonlinearities are allowed - large deformations, plasticity, contact, hyperelasticity and so on. ANSYS Workbench offers an additional solution method of Mode Superposition to perform linear transient structural analysis. In the Mode Superposition method, the transient response to a given loading condition is obtained by calculating the necessary linear combinations of the eigenvectors obtained in a modal analysis. For more details, please refer to Transient Structural Analysis Using Linked Modal Analysis System. A transient dynamic analysis is more involved than a static analysis because it generally requires more computer resources and more of your resources, in terms of the “engineering” time involved. You can save a significant amount of these resources by doing some preliminary work to understand the physics of the problem. For example, you can: 1. Try to understand how nonlinearities (if you are including them) affect the structure's response by doing a static analysis first. In some cases, nonlinearities need not be included in the dynamic analysis. Including nonlinear effects can be expensive in terms of solution time. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 91 Approach 2. Understand the dynamics of the problem. By doing a modal analysis, which calculates the natural frequencies and mode shapes, you can learn how the structure responds when those modes are excited. The natural frequencies are also useful for calculating the correct integration time step. 3. Analyze a simpler model first. A model of beams, masses, springs, and dampers can provide good insight into the problem at minimal cost. This simpler model may be all you need to determine the dynamic response of the structure. Note Refer to the following sections of the Mechanical APDL application documentation for a more thorough treatment of dynamic analysis capabilities: • The Transient Dynamic Analysis chapter of the Structural Analysis Guide - for a technical overview of nonlinear transient dynamics. • The Multibody Analysis Guide - for a reference that is particular to multibody motion problems. In this context, “multibody” refers to multiple rigid or flexible parts interacting in a dynamic fashion. Although not all dynamic analysis features discussed in these manuals are directly applicable to Workbench features, the manuals provide an excellent background on general theoretical topics. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: From the Toolbox, drag a Transient Structural template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: Material properties can be linear or nonlinear, isotropic or orthotropic, and constant or temperature-dependent. Both Young’s modulus (and stiffness in some form) and density (or mass in some form) must be defined. Attach Geometry Basic general information about this topic ... for this analysis type: There are no specific considerations for a transient structural analysis. Define Part Behavior 92 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Basic general information about this topic ... for this analysis type: You can define a Point Mass for this analysis type. In a transient structural analysis, rigid parts are often used to model mechanisms that have gross motion and transfer loads between parts, but detailed stress distribution is not of interest. The output from a rigid part is the overall motion of the part plus any force transferred via that part to the rest of the structure. A “rigid” part is essentially a point mass connected to the rest of the structure via joints. Hence in a transient structural analysis the only applicable loads on a rigid part are acceleration and rotational velocity loads. You can also apply loads to a rigid part via joint loads. If your model includes nonlinearities such as large deflection or hyperelasticity, the solution time can be significant due to the iterative solution procedure. Hence, you may want to simplify your model if possible. For example, you may be able to represent your 3-D structure as a 2-D plane stress, plane strain, or axisymmetric model, or you may be able to reduce your model size through the use of symmetry or antisymmetry surfaces. Similarly, if you can omit nonlinear behavior in one or more parts of your assembly without affecting results in critical regions, it will be advantageous to do so. Define Connections Basic general information about this topic ... for this analysis type: Contact, joints and springs are all valid in a transient structural analysis. In a transient structural analysis, you can specify a damping coefficient property in longitudinal springs that will generate a damping force proportional to velocity. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: Provide an adequate mesh density on contact surfaces to allow contact stresses to be distributed in a smooth fashion. Likewise, provide a mesh density adequate for resolving stresses; areas where stresses or strains are of interest require a relatively fine mesh compared to that needed for displacement or nonlinearity resolution. If you want to include nonlinearities, the mesh should be able to capture the effects of the nonlinearities. For example, plasticity requires a reasonable integration point density (and therefore a fine element mesh) in areas with high plastic deformation gradients. In a dynamic analysis, the mesh should be fine enough to be able to represent the highest mode shape of interest. Establish Analysis Settings Basic general information about this topic Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 93 Approach ... for this analysis type: For transient structural analyses, the basic controls are: Large Deflection (p. 534) is typically needed for slender structures. A rule of thumb is that you can use large deflection if the transverse displacements in a slender structure are more than 10% of the thickness. Small deflection and small strain analyses assume that displacements are small enough that the resulting stiffness changes are insignificant. Setting Large Deflection to On will take into account stiffness changes resulting from change in element shape and orientation due to large deflection, large rotation, and large strain. Therefore the results will be more accurate. However this effect requires an iterative solution. In addition it may also need the load to be applied in small increments. Therefore the solution may take longer to solve. You also need to turn on large deflection if you suspect instability (buckling) in the system. Use of hyperelastic materials also requires large deflection to be turned on. Step Controls (p. 529) allow you to control the time step size in a transient analysis. Refer to the Guidelines for Integration Step Size (p. 527) section for further information. In addition this control also allows you create multiple steps. Multiple steps are useful if new loads are introduced or removed at different times in the load history, or if you want to change the analysis settings such as the time step size at some points in the time history. When the applied load has high frequency content or if nonlinearities are present, it may be necessary to use a small time step size (that is, small load increments) and perform solutions at these intermediate time points to arrive at good quality results. This group can be modified on a per step basis. Output Controls (p. 545) allow you to specify the time points at which results should be available for postprocessing. In a transient nonlinear analysis it may be necessary to perform many solutions at intermediate time values. However, i) you may not be interested in all the intermediate results, and ii) writing all the results can make the results file size unwieldy. This group can be modified on a per step basis except for Stress and Strain. Nonlinear Controls (p. 542) allow you to modify convergence criteria and other specialized solution controls. Typically you will not need to change the default values for this control. This group can be modified on a per step basis. Damping Controls (p. 542) allow you to specify damping for the structure in a transient analysis. The following forms of damping are available for a transient analysis: Beta damping and Numerical damping. In addition, element based damping from spring elements as well as material based damping factors are also available for the transient structural analysis. Analysis Data Management (p. 549) settings enable you to save specific solution files from the transient structural analysis for use in other analyses. The default behavior is to only keep the files required for postprocessing. You can use these controls to keep all files created during solution or to create and save the Mechanical APDL application database (db file). Define Initial Conditions 94 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Basic general information about this topic ... for this analysis type: 1. A transient analysis involves loads that are functions of time. The first step in applying transient loads is to establish initial conditions (that is, the condition at Time = 0). 2. The default initial condition for a transient structural analysis is that the structure is “at rest”, that is, both initial displacement and initial velocity are zero. A transient structural analysis is at rest, by default. The Initial Conditions object allows you to specify Velocity. 3. In many analyses one or more parts will have an initial known velocity such as in a drop test, metal forming analysis or kinematic analysis. In these analyses, you can specify a constant Velocity initial condition if needed. The constant velocity could be scoped to one or more parts of the structure. The remaining parts of the structure which are not part of the scoping will retain the “at rest” initial condition. 4. Initial Condition using Steps: You can also specify initial conditions using step controls, that is, by specifying multiple steps in a transient analysis and controlling the time integration effects along with activation/deactivation of loads. This comes in handy when, for example, you have different parts of your model that have different initial velocities or more complex initial conditions. The following are approaches to some commonly encountered initial condition scenarios: a. Initial Displacement = 0, Initial Velocity ≠ 0 for some parts: The nonzero velocity is established by applying small displacements over a small time interval on the part of the structure where velocity is to be specified. i. Specify 2 steps in your analysis. The first step will be used to establish initial velocity on one or more parts. ii. Choose a small end time (compared to the total span of the transient analysis) for the first step. The second step will cover the total time span. iii. Specify displacement(s) on one or more faces of the part(s) that will give you the required initial velocity. This requires that you do not have any other boundary condition on the part that will interfere with rigid body motion of that part. Make sure that these displacements are ramped from a value of 0. iv. Deactivate or release the specified displacement load in the second step so that the part is free to move with the specified initial velocity. For example, if you want to specify an initial Y velocity of 5 inch/second on a part, and your first step end time is 0.001 second, then specify the following loads. Make sure that the load is ramped from a value of 0 at time = 0 so that you will get the required velocity. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 95 Approach In this case the end time of the actual transient analysis is 30 seconds. Note that the Y displacement in the second step is deactivated. v. In the Analysis Settings Details view, set the following for first step: vi. You can choose appropriate time step sizes for the second step (the actual transient). Make sure that time integration effects are turned on for the second step. In the first step, inertia effects will not be included but velocity will be computed based on the displacement applied. In the second step, this displacement is released by deactivation and the time integration effects are turned on. b. Initial Displacement ≠ 0, Initial Velocity ≠ 0: This is similar to case a. above except that the imposed displacements are the actual values instead of “small” values. For example if the initial displacement is 1 inch and the initial velocity is 2.5 inch/sec then you would apply a displacement of 1 inch over 0.4 seconds. i. Specify 2 steps in your analysis. The first step will be used to establish initial displacement and velocity on one or more parts. ii. Choose a small end time (compared to the total span of the transient analysis) for the first step. The second step will cover the total time span. iii. Specify the initial displacement(s) on one or more faces of the part(s) as needed. This requires that you do not have any other boundary condition on the part that will interfere with rigid body motion of that part. Make sure that these displacements are ramped from a value of 0. iv. Deactivate or release the specified displacement load in the second step so that the part is free to move with the specified initial velocity. For example if you want to specify an initial Z velocity on a part of 0.5 inch/sec and have an initial displacement of 0.1 inch, then your first step end time = (0.1/0.5) = 0.2 second. Make sure that the displacement is ramped from a value of 0 at time = 0 so that you will get the required velocity. In this case the end time of the actual transient analysis is 5 seconds. Note that the Z displacement in the second step is deactivated. v. 96 In the Analysis Settings Details view, set the following for first step: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types vi. You can choose appropriate time step sizes for the second step (the actual transient). Make sure that time integration effects are turned on for the second step. In the first step, inertia effects will not be included but velocity will be computed based on the displacement applied. In the second step, this displacement is released by deactivation and the time integration effects are turned on. c. Initial Displacement ≠ 0, Initial Velocity = 0: This requires the use of two steps also. The main difference between b. above and this scenario is that the displacement load in the first step is not ramped from zero. Instead it is step applied as shown below with 2 or more substeps to ensure that the velocity is zero at the end of step 1. i. Specify 2 steps in your analysis. The first step will be used to establish initial displacement on one or more parts. ii. Choose an end time for the first step that together with the initial displacement values will create the necessary initial velocity. iii. Specify the initial displacement(s) on one or more faces of the part(s) as needed. This requires that you do not have any other boundary condition on the part that will interfere with rigid body motion of that part. Make sure that this load is step applied, that is, apply the full value of displacements at time = 0 itself and maintain it throughout the first step. iv. Deactivate or release the specified displacement load in the second step so that the part is free to move with the initial displacement values. For example if you want to specify an initial Z displacement of 0.1 inch and the end time for the first step is 0.001 seconds, then the load history displays as shown below. Note the step application of the displacement. In this case the end time of the actual transient analysis is 5 seconds. Note that the Z displacement in the second step is deactivated. v. In the Analysis Settings Details view, set the following for first step. Note that the number of substeps must be at least 2 to set the initial velocity to zero. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 97 Approach vi. You can choose appropriate time step sizes for the second step (the actual transient). Make sure that time integration effects are turned on for the second step. In the first step, inertia effects will not be included but velocity will be computed based on the displacement applied. But since the displacement value is held constant, the velocity will evaluate to zero after the first substep. In the second step, this displacement is released by deactivation and the time integration effects are turned on. Apply Loads and Supports Basic general information about this topic ... for this analysis type: For a transient structural analysis applicable loads/supports are all inertial and structural loads, and all structural supports. Joint Loads are used to kinematically drive joints. See the Joint Load (p. 581) section for details. In this analysis, the load’s magnitude could be a constant value or could vary with time as defined in a table or via a function. Details of how to apply a tabular or function load are described in Specifying Load Values (p. 621). In addition, see the Apply Loads and Supports section for more information about time stepping and ramped loads. For the solver to converge, it is recommended that you ramp joint load angles and positions from zero to the real initial condition over one step. Solve Basic general information about this topic ... for this analysis type: When performing a nonlinear analysis, you may encounter convergence difficulties due to a number of reasons. Some examples may be initially open contact surfaces causing rigid body motion, large load increments causing non-convergence, material instabilities, or large deformations causing mesh distortion that result in element shape errors. To identify possible problem areas some tools are available under Solution Information object Details view. Solution Output continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. Any convergence data output in this printout can be graphically displayed as explained in the Solution Information section. 98 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types You can display contour plots of Newton-Raphson Residuals in a nonlinear static analysis. Such a capability can be useful when you experience convergence difficulties in the middle of a step, where the model has a large number of contact surfaces and other nonlinearities. When the solution diverges, identifying regions of high Newton-Raphson residual forces can provide insight into possible problems. Result Tracker is another useful tool that allows you to monitor displacement and energy results as the solution progresses. This is especially useful in case of structures that possibly go through convergence difficulties due to buckling instability. Review Results Basic general information about this topic ... for this analysis type: All structural result types except frequencies are available as a result of a transient structural analysis. You can use a Solution Information object to track, monitor, or diagnose problems that arise during a solution. Once a solution is available you can contour the results or animate the results to review the response of the structure. As a result of a nonlinear static analysis, you may have a solution at several time points. You can use probes to display the variation of a result item as the load increases. Note Fixed body-to-body joints between two rigid bodies will not produce a joint force or moment in a transient structural analysis. Also of interest is the ability to plot one result quantity (for example, displacement at a vertex) against another result item (for example, applied load). You can use the Charts feature to develop such charts. Charts are also useful to compare results between two analyses of the same model. For example, you can compare the displacement response at a vertex from two transient structural analyses with different damping characteristics. Transient Structural Analysis Using Linked Modal Analysis System Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: As this analysis is linked to (or based on) modal responses, a modal analysis is a prerequisite. This setup allows the two analysis systems to share resources such as engineering data, geometry and boundary condition type definitions made in modal analysis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 99 Approach Note The Mode Superposition transient structural analysis is not allowed to be linked to a pre-stressed modal analysis. From the Toolbox, drag a Modal template to the Project Schematic. Then, drag a Transient Structural template directly onto the Solution cell of Modal template. Establish Analysis Settings Basic general information about this topic ... for this analysis type: Step Controls - The analysis is only compatible with constant time stepping. So, auto time stepping is turned off and will always be in read only mode. The user specified substep or time step value is applicable to all the load steps. All the step controls settings applied to this analysis are not step aware. The time integration is turned on by default and will always be in read only mode. A Time Step value that results in an integral number of sub steps over the load step must be selected. Output Controls - You can request Stress, Strain, Nodal Force, and Reaction results to be calculated. For better performance, you can also choose to have these results expanded from transient or modal solutions. The Contact Miscellaneous option is not available. Damping Controls - Numerical Damping Value defaults to 0.005 for this analysis. To edit the numerical damping value, please change the Numerical Damping field to Manual from Program Controlled. Note Solver Controls, Restart Controls, Nonlinear Controls and Creep Controls are not applicable to the current analysis. Define Initial Conditions Basic general information about this topic ... for this analysis type: The transient structural analysis must point to a modal analysis in the Modal initial conditions object. The modal analysis must extract all modes that may contribute to the dynamic response. Apply Loads and Supports Basic general information about this topic ... for this analysis type: 100 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types The following loads are allowed for the linked analysis: • Acceleration (p. 563) • Pressure (p. 568) • Pipe Pressure (p. 569) • Force (p. 570) (applied to a face, edge, or vertex) • Line Pressure (p. 578) • Moment (p. 577) • Remote Force (p. 572) • Standard Earth Gravity (p. 566) Support Limitations Please note the following limitations: • If the Reference Temperature is set as By Body and that temperature does not match the environment temperature, a thermally induced transient load will result (from the thermal strain assuming a nonzero thermal expansion coefficient). This thermal transient loading is ignored for Transient Structural Analysis using Linked Modal Analysis System. • Remote Force is not supported for vertex scoping. • Remote Force and Moment applied to a rigid body is not supported. • Moment is not supported for vertex scoping on 3-D solid bodies because a beam entity is created for the load application. The beam entity changes the stiffness of the structural component shared and solved by the preceding modal analysis. • Joint probes, Energy Probe, and Strain Energy results are not supported when expanded from a Modal solution. • Remote Force and Moment loading along with the rigid contact behavior is not allowed as it changes the stiffness of structural component shared and solved by the preceding modal analysis. • Spring probe only supports Elastic force result when expanded from modal solution where as it supports both Elastic force and Elongation results when expanded from transient solution. The Elastic force results include the spring damping effect if the Reduced method is selected from Modal Solver controls, and Store Complex Solution is set to No. Notes • To obtain the most accurate results, it is recommended that you specify Bonded as the contact Type and set the contact Formulation to MPC in the Details for the Contact Region. See the Contact Definition and Contact Advanced Category for more detailed information about these settings. • When the result is expanded from Modal Solution or when Reaction Object is scoped to a Contact Region, the Reaction Object requires both Nodal Forces and Calculate Reactions Output Controls settings to be turned On. If they are not set, the error message “A result is invalid with current output control settings” displays. For other cases, the Reaction Object requires only the Calculate Reactions Output Controls setting to be turned On. • The default value of numerical damping is different for full and mode superposition transient structural analyses. So, the results comparison of a model must be done by matching the numerical damping value settings in the Damping Controls section. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 101 Approach Rigid Dynamics Analysis Introduction You can perform a rigid dynamics analysis in the Mechanical application using the ANSYS Rigid Dynamics solver. This type of analysis is used to determine the dynamic response of an assembly of rigid bodies linked by joints and springs. You can use this type of analysis to study the kinematics of a robot arm or a crankshaft system for example. Points to Remember • Inputs and outputs are forces, moments, displacements, velocities and accelerations. • All parts are rigid such that there are no stresses and strain results produced, only forces, moments, displacements, velocities and accelerations. • The solver is tuned to automatically adjust the time step. Doing it manually is often inefficient and results in longer run times. • Viscous damping can be taken into account through springs. Note Refer to the Multibody Analysis Guide for a reference that is particular to multibody motion problems. In this context, “multibody” refers to multiple rigid parts interacting in a dynamic fashion. Although not all dynamic analysis features discussed in this manual are directly applicable to Workbench features, it provides an excellent background on general theoretical topics. Preparing the Analysis Create Analysis System Basic general information about this topic ... for this analysis type: From the Toolbox, drag a Rigid Dynamics template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: Density is the only material property utilized in a rigid dynamics analysis. Models that use zero or nearly zero density fail to solve with the ANSYS Rigid Dynamics solver. Attach Geometry Basic general information about this topic 102 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types ... for this analysis type: Sheet and solid bodies are supported by the ANSYS Rigid Dynamics solver. Plane bodies and line bodies cannot be used. Define Part Behavior Basic general information about this topic ... for this analysis type: You can define a Point Mass for this analysis type. Part stiffness behavior is not required for the ANSYS Rigid Dynamics solver in ANSYS Workbench. Define Connections Basic general information about this topic ... for this analysis type: Applicable connections are joints, springs, and frictionless contact. When an assembly is imported from a CAD system, joints or constraints are not imported, but joints may be created automatically after the model is imported. You can also choose to create the joints manually. Each joint is defined by its coordinate system of reference. The orientation of this coordinate system is essential as the free and fixed degrees of freedom are defined in this coordinate system. Automatic contact generation is also available after the model is imported. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: Mesh controls are not applicable for the ANSYS Rigid Dynamics solver. Establish Analysis Settings Basic general information about this topic ... for this analysis type: For rigid dynamics analyses the basic controls are: Step Controls (p. 529) allow you to create multiple steps. Multiple steps are useful if new loads are introduced or removed at different times in the load history. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 103 Approach Rigid dynamics analyses use an explicit time integration scheme. Unlike the implicit time integration, there are no iterations to converge in an explicit time integration scheme. The solution at the end of the time step is a function of the derivatives during the time step. As a consequence, the time step required to get accurate results is usually smaller than is necessary for an implicit time integration scheme. Another consequence is that the time step is governed by the highest frequency of the system. A very smooth and slow model that has a very stiff spring will require the time step needed for the stiff spring itself, which generates the high frequencies that will govern the required time step. Because it is not easy to determine the frequency content of the system, an automatic time stepping algorithm is available, and should be used for the vast majority of models. This automatic time stepping algorithm is governed by Initial Time Step, Minimum Time Step, and Maximum Time Step under Step Controls; and Energy Accuracy Tolerance under Nonlinear Controls. • Initial Time Step: If the initial time step chosen is vastly too large, the solution will typically fail, and produce an error message that the accelerations are too high. If the initial time step is only slightly too large, the solver will realize that the first time steps are inaccurate, automatically decrement the time step and start the transient solution over. Conversely, if the chosen initial time step is excessively small, and the simulation can be accurately performed with higher time steps, the automatic time stepping algorithm will, after a few gradual increases, find the appropriate time step value. Choosing a good initial time step is a way to reduce the cost of having the solver figure out what time step size is optimal to minimize run time. While important, choosing the correct initial time step typically does not have a large influence on the total solution time due to the efficiency of the automatic time stepping algorithm. • Minimum Time Step: During the automatic adjustment of the time step, if the time step that is required for stability and accuracy is smaller than the specified minimum time step, the solution will not proceed. This value does not influence solution time or its accuracy, but it is there to prevent Workbench from running forever with an extremely small time step. When the solution is aborting due to hitting this lower time step threshold, that usually means that the system is over constrained, or in a lock position. Check your model, and if you believe that the model and the loads are valid, you can decrease this value by one or two orders of magnitude and run again. That can, however generate a very large number of total time steps, and it is recommended that you use the Output Controls settings to store only some of the generated results. • Maximum Time Step: Sometimes the time step that the automatic time stepping settles on produces too few results outputs for precise postprocessing needs. To avoid these postprocessing resolution issues, you can force the solution to use time steps that are no bigger than this parameter value. Solver Controls: for this analysis type, allows you to select a time integration algorithm (Runge-Kutta order 4 or 5) and select whether to use constraint stabilization. The default time integration option, Runge-Kutta 4, provides the appropriate accuracy for most applications. When constraint stabilization is employed, Stabilization Parameters are an automatic option. The default, Program Controlled is valid for most applications, however; you may wish to set this option to User Defined and manually enter customized settings for weak spring and damping effects. The default is Off. Nonlinear Controls (p. 542) allow you to modify convergence criteria and other specialized solution controls. Typically you will not need to change the default values for this control. 104 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types • Energy Accuracy Tolerance: This is the main driver to the automatic time stepping. The automatic time stepping algorithm measures the portion of potential and kinetic energy that is contained in the highest order terms of the time integration scheme, and computes the ratio of the energy to the energy variations over the previous time steps. Comparing the ratio to the Energy Accuracy Tolerance, Workbench will decide to increase or decrease the time step. Note For systems that have very heavy slow moving parts, and also have small fast moving parts, the portion of the energy contained in the small parts is not dominant and therefore will not control the time step. It is recommended that you use a smaller value of integration accuracy for the motion of the small parts. Spherical, slot and general joints with three rotation degrees of freedom usually require a small time step, as the energy is varying in a very nonlinear manner with the rotation degrees of freedom. Output Controls (p. 545) allow you to specify the time points at which results should be available for postprocessing. In a transient nonlinear analysis it may be necessary to perform many solutions at intermediate time values. However i) you may not be interested in reviewing all of the intermediate results and ii) writing all the results can make the results file size unwieldy. This group can be modified on a per step basis. Define Initial Conditions Basic general information about this topic ... for this analysis type: Before solving, you can configure the joints and/or set a joint load to define initial conditions. 1. Define a Joint Load to set initial conditions on the free degrees of freedom of a joint. For the ANSYS Mechanical APDL solver to converge, it is recommended that you ramp the angles and positions from zero to the real initial condition over one step. The ANSYS Rigid Dynamics solver does not need these to be ramped. For example, you can directly create a joint load for a revolute joint of 30 degrees, over a short step to define the initial conditions of the simulation. If you decide to ramp it, you have to keep in mind that ramping the angle over 1 second, for example, means that you will have a non-zero angular velocity at the end of this step. If you want to ramp the angle and start at rest, use an extra step maintaining this angle constant for a reasonable period of time or, preferably, having the angular velocity set to zero. Another way to specify the initial conditions in terms of positions and angles is to use the Configure tool, which eliminates the time steps needed to apply the initial conditions. To fully define the initial conditions, you must define position and velocities. Unless specified by joint loads, if your system is initially assembled, the initial configuration will be unchanged. If the system is not initially assembled, the initial configuration Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 105 Approach will be the “closest” configuration to the unassembled configuration that satisfies the assembly tolerance and the joint loads. Unless specified otherwise, relative joint velocity is, if possible, set to zero. For example, if you define a double pendulum and specify the angular velocity of the grounded revolute joint, by default the second pendulum will not be at rest, but will move rigidly with the first one. 2. Configure a joint to graphically put the joint in its initial position. See Joint Initial Conditions (p. 434) for further details. Apply Loads and Supports Basic general information about this topic ... for this analysis type: The following loads and supports can be used in a rigid dynamics analysis: • Acceleration • Standard Earth Gravity • Joint Load • Remote Displacement • Remote Force • Constraint Equation Both Acceleration and Standard Earth Gravity must be constant throughout a rigid dynamics analysis and cannot be deactivated. For a Joint Load, the joint condition’s magnitude could be a constant value or could vary with time as defined in a table or via a function. Details of how to apply a tabular or function load are described in Specifying Load Values (p. 621). Details on the Joint Load are included below. In addition, see the Apply Loads and Supports section for more information about time stepping and ramped loads. Joint Load Interpolation/Derivation For joint loads applied through tabular data values, because the number of points input will very likely be less than the number of time steps required to solve the system, a cubic spline interpolation is performed, as shown on the following graph: 106 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Sometimes, the difference between the interpolated curve and the linear interpolation is high, and the solution cannot proceed. In these cases, If your intent is to use the linear interpolation, you can simply use multiple time steps, as the interpolation is done only within a time step. When defining a joint load for a position and an angle, the corresponding velocities and accelerations will be computed internally. When defining a joint load for a translational and angular velocity, corresponding accelerations are also computed internally. By activating and deactivating joint loads, you can generate some forces/accelerations/velocities, and position discontinuities. Always consider what the implications of these discontinuities are for velocities and accelerations. Force and acceleration discontinuities are perfectly valid physical situations. No special attention is required to define these velocity discontinuities, that can, for example be obtained by changing the slope of a relative displacement joint load on a translational joint as shown on the following graph, using two time steps: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 107 Approach The corresponding velocity profile is shown here. This discontinuity of velocity is physically equivalent to a shock, and implies infinite acceleration if the change of slope is over a zero time duration. The ANSYS Rigid Dynamics solver will handle these discontinuities, and redistribute velocities after the discontinuity according to all active joint loads. This process of redistribution of velocities usually provides accurate results, however no shock solution is performed, and this process is not guaranteed to produce proper energy balance. A closer look at the total energy probe will tell you if the solution is valid. In case the redistribution is not done properly, use one step instead of two to use an interpolated, smooth position variation with respect to time. Discontinuities of positions and angles are not a physically acceptable situation. Results obtained in this case are very likely to make no physical sense. Workbench cannot detect this situation up front. If you proceed with position discontinuities, the solution either may abort, or, if it does solve completely, false results may be produced. Joint Load Rotations For fixed axis rotations, it is possible to count a number of turns. For 3-D general rotations, it is not possible to count turns. In a single axis case, although it is possible to prescribe angles higher than 2π, it is not recommended because Workbench can lose count of the number of turns based on the way you ramp the angle. It is highly recommended that you use an angular velocity joint load instead of an angle value to ramp a rotation, whenever possible. For example, replace a rotation joint load designed to create a joint rotation from an angle from 0 to 720 degrees over 2 seconds by an angular velocity of 360 degrees/second. The second solution will always provide the right result, while the behavior of the first case can sometimes lead to the problems mentioned above. For 3-D rotations on a general joint for example, no angle over 2π can be handled. Use an angular velocity joint load instead. 108 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Multiple Joint Loads On The Same Joint When prescribing a position or an angle on a joint, velocities and acceleration are also prescribed. The use of multiple joint loads on the same joint motion can cause for joint loads to be determined inaccurately. Solve Basic general information about this topic ... for this analysis type: Only synchronous solves are supported for rigid dynamics analyses. Review Results Basic general information about this topic ... for this analysis type: Use a Solution Information object to track, monitor, or diagnose problems that arise during solution. Applicable results are Deformation and Probe results. Note If you highlight Deformation results in the tree that are scoped to rigid bodies, the corresponding rigid bodies in the Geometry window are not highlighted. To plot different results against time on the same graph or plot one result quantity against a load or another results item, use the Chart and Table (p. 729) feature. If you duplicate a rigid dynamics analysis, the results of the duplicated branch are also cleared. Joint Conditions and Expressions When a rotation, position, velocity or angular velocity uses an expression that user the power (^) operator, such as (x)^(y), the table will not be calculated properly if the value x is equal to zero. This is because it's time derivative uses log(x), which is not defined for x = 0. An easy workaround is to use x*x*x... (y times), which assumes that y is an integer number and thus can be derived w.r.t time without using the log operator. Command Reference for Rigid Dynamics Systems This section contains a list of commands for Rigid Dynamics, arranged by parent object. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 109 Approach IronPython References Rigid dynamics uses an object-based approach. Hence it is advantageous to have some knowledge of object oriented programming and the Python language for writing commands for the solver. ANSYS Workbench scripting is based on IronPython 2.6 which is well integrated with the rest of the .NET Framework (on Windows) and Mono CLR (on Linux). It makes all related libraries easily available to Python programmers while maintaining compatibility with the Python language. For more information on IronPython, see http://ironpython.codeplex.com/. IronPython is compatible with existing Python scripts. However, not all C-based Python library modules are available under IronPython. For details, refer to the IronPython website. For more information on Python, including a standard language reference, see http://www.python.org/. The Rigid Dynamics Object Model Rigid dynamics uses an object-based approach. The Environment is the top level object that allows access to all other underlying objects. The Environment is associated to an environment object in the Mechanical tree. Many environments can exist on the same model. This model is called the System in the Rigid Dynamics Object model. The system contains the physical representation of the model, and the environment contains the representation of a given simulation done on the model. This means that Bodies and Joints will belong to the systems, and Joint Conditions or Loads will be available on the environment. An alternate way to access the objects is by ID. Each object has a unique ID that is also the ID that Mechanical uses. Global object tables help you to get a handle on an object for which you have an ID. For example, accessing the Joint having _jid as the ID is done using the following call: Joint= CS_Joint.Find(_jid) CS_xxx is the table of all xxx type objects. Whenever the ID of an object is not known or if only one occurrence of the object exists in the object model, query the object table to find the first occurrence of a given object type. This is explained in the following example: Environment = CS_Environment.FindFirstNonNull() GetId() Using this call, each object can return its ID. GetName() Using this call, each object can return its name. SetName(name) Using this call, each name can be set or changed. Some objects will have to be created. For that purpose, you have to call the constructor of the object. For example, to create a constant variable, use: Var = CS_ConstantVariable() Rigid Dynamics Objects The following rigid dynamics objects are available: Actuator 110 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Body Body Coordinate System Condition Driver Environment Joint JointDOFLoad Load Measure PointTable Relation Spring System Variable Actuator The actuator is the base class for all the Loads and Drivers. ID table: CS_Actuator Members: Condition: All actuators can be conditional. See Condition to create this condition. Member Functions: SetInputMeasure(measure): “measure” is typically the time measure object, but other measures can be used as well. When using an expression to define a load variation, the measure must have only one component (it cannot be a vector measure). The variation can be defined by a constant, an expression, or a table. SetConstantValues(value): “value” is a python float constant. See Relation object for defining a constant. SetTable(table): “table” is a CS_PointTable. SetFunc(string, is_degree): “string” is an expression similar to the one used in the user interface when defining a joint condition by a function. Note that the literal variable is always called “time”, even if you are using another measure as input. "is_degree" is a boolean argument. If the expression uses trigonometric function, it specifies that the input variable should be expressed in degrees. Body A body corresponds to a Part in the geometry node of the Mechanical tree. The preset “_bid” variable can be used to find a corresponding body. ID table: CS_Body Example: MyBody = CS_Body.Find(_bid) print MyBody.Name Members: Name: Name of the body. Origin: Origin Coordinate System of the body. This Coordinate System is the moving coordinate system of one of the joints connected to the body. The choice of this joint, called parent joint, is the result of an optimization that will minimize the number of degrees of freedom of the system. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 111 Approach InertiaBodyCoordinateSystem: Inertia body coordinate system of the body. Member Functions: SetMassAndInertia(double mass, double Ixx, double Iyy, double Izz, double Ixy, double Iyz, double Ixz ): Allows you to overwrite the mass and inertia values of a body. SetCenterOfMassAndOrientationAngles(double Xg, double Yg, double Zg, double XYAngle, double YZAngle, double XZAngle): Allows you to overwrite the position of the center of mass and the orientation of the inertia coordinate system. Body Coordinate System The body coordinate system is used to connect a body to joints, to hold the center of mass, or to define load. See Joint to access existing coordinate systems. ID table: CS_BodyCoordinateSystem Members: None Member Functions: RotateArrayThroughTimeToLocal(MeasureValues): Rotates the transient values of a measure to a coordinate system. MeasureValues is a python two-dimensional array, such as that coming out of FillValuesThroughTime or FillDerivativesThroughTime. This function works for 3-D vectors such as relative translation between two coordinate systems or 6-D vectors such as forces/moments. RotateArrayThroughTimeToGlobal(MeasureValues): Rotates the transient values of a measure from a coordinate system to the global coordinate system. Derived Classes: None Example: jointRotation = J1.GetRotation() jointVelocity = J1.GetVelocityMeasure() jointAcceleration = J1.GetAccelerationMeasure() jointForce = J1.GetForceMeasure() jointRotationValues =jointRotation.FillDataThroughTime() jointVelocityValues =jointVelocity.FillDataThroughTime() jointAccelerationValues =jointAcceleration.FillDataThroughTime() jointForceValues =jointForce.FillDataThroughTime() nbValues = jointRotationValues.GetLength(0) print jointRotation.Id print ' Time Rotation Velocity Acceleration' for i in range(0,nbValues): print jointRotationValues[i,0],jointRotationValues[i,1],jointVelocityValues[i,1],jointAccelerationValues[i,1] fich.close() Condition Condition is a way to make a load or a joint condition to be active only under some circumstances. A condition is expressed in one of the following forms: 112 1. MeasureComponent operator threshold 2. LeftThreshold < MeasureComponent < RightThreshold Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types 3. LeftCondition operator RightCondition For case 1: • MeasureComponent is a scalar Measure. • Operator is a math operator chosen from the following list: E_GreaterThan E_LessThan E_DoubleEqual E_ExactlyEqual • Threshold is the threshold value. Example: DispCond = CS_Condition(CS_Condition.E_ConditionType.E_GreaterThan,DispX,0.1) For case 2: • MeasureComponent is a scalar Measure. • LeftThreshold and RightThreshold are the bounds within which the condition will be true. Example: RangeCond = CS_Condition(DispX,0.0,0.1) For case 3: • LeftThreshold and RightThreshold are two conditions (case 1, 2 or 3). • Operator is a boolean operator chosen from the following list: E_Or E_And Example: BoolCond = CS_Condition(CS_Condition.E_ConditionType.E_Or, RangeCond, DispCond) Driver A driver is a position, velocity or acceleration, translational or rotational joint condition. Drivers derive from the Actuator class. Corresponding ID table: CS_Actuator Constants: E_Acceleration, E_Position, E_Velocity Members: None Member Functions: CS_Driver(CS_Joint joint, int[] components, E_MotionType driverMotionType): Creation of a joint driver, on joint “joint”, degree of freedom “components”, and with motion type “driverMotionType”. Note that the same driver can prescribe more than one joint motion at the same time. This can be useful if you want to add the same condition to all components of a prescribed motion, for example. Components must be ordered, are zero based, and refer to the actual free degrees of freedom of the joint. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 113 Approach Environment This is the top level of the Rigid Dynamics model. ID table: CS_Environment Members: System: Corresponding system. Example: Env=CS_Environment.FindFirstNonNull() Sys = Env.System Loads: The vector of existing loads. This includes Springs that are considered by the solver as loads, as well as force and torque joint conditions. Example: Xdof = 0 Friction=CS_JointDOFLoad(PlanarJoint,Xdof) Env.Loads.Add(Friction) Relations: The vector of external constraint equations. Example: rel3=CS_Relation() rel3.MotionType=CS_Relation.E_MotionType.E_Velocity var30=CS_ConstantVariable() var30.SetConstantValues(System.Array[float]([0.])) var31=CS_ConstantVariable() var31.SetConstantValues(System.Array[float]([23.])) var32=CS_ConstantVariable() var32.SetConstantValues(System.Array[float]([37.])) var33=CS_ConstantVariable() var33.SetConstantValues(System.Array[float]([-60.+37.])) rel3.SetVariable(var30) rel3.AddTerm(jp,0,var31) rel3.AddTerm(js3,0,var32) rel3.AddTerm(jps,0,var33) Env.Relations.Add(rel3) Drivers: The vector of Displacements, Velocity and Acceleration joint conditions. InitialConditions: The vector of Displacements, Velocity, and Acceleration joint conditions to be used only at time=0. PotentialEnergy: Gets the Potential Energy Measure. KineticEnergy: Gets the Kinetic Energy Measure. 114 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types TotalEnergy: Gets the Total Energy Measure. ActuatorEnergy: Gets the Actuator Energy Measure. Member Functions: FindFirstNonNull(): Returns the first environment in the global list. Usually, the table contains only one environment. Hence, thus it is the common way to access the current environment. Example: Env=CS_Environment.FindFirstNonNull() Derived Classes: None Joint ID table: CS_Joint Constants: For the joint type (E_JointType): E_2DSlotJoint, E_BushingJoint, E_CylindricalJoint, E_GeneralJoint, E_FreeJoint, E_PlanarJoint, E_PointOnCurveJoint , E_RevoluteJoint, E_ScrewJoint, E_SingleRotationGeneralJoint, E_SlotJoint, E_SphericalJoint, E_TranslationalJoint, E_TwoRotationGeneralJoint, E_UniversalJoint, Members: Name: Name of the joint ReferenceCoordinateSystem: Joint reference coordinate system Example: J1 = CS_Joint.Find(_jid) CSR = J1.ReferenceCoordinateSystem MovingCoordinateSystem: Joint moving coordinate system Example: J1 = CS_Joint.Find(_jid) CSM = J1. MovingCoordinateSystem Type: Joint type IsRevert: The internal representation of the joint can use flipped reference and mobile coordinate systems. In that case, all the joint results (e.g., forces, moments, rotation, velocities and acceleration) must be multiplied by -1 to go from their internal representation to the user representation. As transient values of joint measures are giving the internal representation, use this IsRevert information to know if results should be negated. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 115 Approach AccelerationFromVelocitiesDerivatives: When extracting joint degrees of freedom on joints that return true, accelerations should be done by using the time derivatives of the joint velocity measure. On joints that return false, extracting of the joint DOFs derivatives should be done using the joint acceleration measure. It is important to check this flag first. Using the wrong method to query joint acceleration would fail or give incorrect results. Example: if Universal.AccelerationFromVelocitiesDerivatives: UniversalAccelerationValues=UniversalVelocityM.FillDerivativesThroughTime() else: UniversalAcceleration = Universal.GetAcceleration() UniversalAccelerationValues=UniversalAcceleration.FillDataThroughTime() Member Functions: GetVelocity(): Returns the joint velocity measure. The size of this measure is the number of degrees of freedom of the joint. The derivatives of this measure give access to the joint accelerations. GetRotation(): Returns the joint rotation measure. The type of measure depends on the joint number of rotational degrees of freedom (E_1DRotationMeasure, E_3DRotationMeasure, E_UniversalAngles). These rotations components are relative to the reference coordinate system of the joint. GetTranslation(): Returns the joint translation measure. The length of this measure will be the number of translational degrees of freedom of the joint. The translation components are expressed in the reference coordinate system of the joint. GetForce(): Returns the joint force measure. The length of this measure is always 6 (3 forces components, 3 torque component). This force measure is the total force/moment, including constraint forces/moment, external forces/moment applied to the joint, and joint internal forces/moment, such as elastic moment in a revolute joint that has a stiffness on the Z rotation axis. The force measure components are expressed in the global coordinate system. Note that the sign convention is different from the sign convention used in the Joint Probes in Mechanical. GetAcceleration(): Returns the joint acceleration measures on the joints that are constraint equations based. See the AccelerationFromVelocitiesDerivatives member to see when this function should be used. Example: J1 = CS_Joint.Find(_jid) jointRotation = J1.GetRotation() jointVelocity = J1.GetVelocityMeasure() jointAcceleration = J1.GetAccelerationMeasure() jointForce = J1.GetForceMeasure() Derived Classes: On SphericalJoint, SlotJoint, BushingJoint, FreeJoint, GeneralJoint. Member Function AddStop(angle_max, restitution_factor): Adds a spherical stop to a joint that has three rotations. A spherical stop constrains the motion of the X and Y rotational degrees of freedom, to give to the joint the behavior of a loose revolute joint, with a 116 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types rotational gap. This will allow easier handling of over-constrained systems and building higher fidelity models without having to use contact. angle_max is the angle between the reference coordinate system Zr axis and the moving coordinate system Zm. Zr is the natural revolute axis. restitution_factoris the restitution factor, similar to other joint stops. Zr Zm Yr n θ Xr On CylindricalJoint: ReplaceByScrew(pitch): Creates a relation between the translational and the rotational degrees of freedom of a cylindrical joint. Note that the pitch is in the current length unit. JointDOFLoad JointDOFLoads are loads applied on a given degree of freedom of a joint. The load is applied in the joint reference coordinate system. JointDOFLoad derives from Load. The constructor for CS_JointDOFLoad is called as follows : Load=CS_JointDOFLoad(joint,dof) • “joint” is a joint object. • “dof” is an integer that defines the joint degree of freedom to be included in the term. The ordering of the degrees of freedom sets the translation degrees of freedom first. The degrees of freedom numbering is zero based. For example, in a slot joint, the translational degree of freedom is 0, while the third rotational degree of freedom is 3. Members: None Member functions: None Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 117 Approach Load Loads derive from the Actuator class. They are derived from various types of loads, such as the CS_JointDOFLoad. Corresponding ID table: CS_Actuator Members: None Members Functions: None Measure: Most of the useful measures are already pre-existing on the rigid dynamics model, and you need to use other object “get” functions to access them but others can be created before solving, in order to perform custom postprocessing or to use their value as input for a joint condition. Other measures can be created, for example to express conditions. In that case, for the measure to be computed at each time step, it needs to be added to the system (see component measure example below) ID table: CS_Measure Constants: For the measure type (E_MeasureType): E_1DRotationJoint, E_3DRotationJoint, E_Acceleration, E_ActuatorEnergy, E_AnsysJointForceAndTorque, E_BodyAcceleration, E_BodyIntertialBCSQuaternion, E_BodyTranslation, E_BodyRotation, E_CenterOfGravity, E_Component, E_Constant, E_Contact, E_ContactForce, E_ContactVelocity, E_Counter, E_Displacement, E_Distance, E_DistanceDot, E_Divides, E_EigenValue, E_Dot, E_ElasticEnergy, E_Energy, E_EulerAngles, E_ForceMagnitude, E_Forces, E_IntegratedOmega, E_JointAcceleration, E_JointDOFFrictionCone, E_JointDriverForce, E_JointForce, E_JointMBDVelocity, E_JointNormalForce, E_JointTranslation, E_JointRotation, E_JointVelocity, E_KineticEnergy, E_MassMomentsOfInertia, E_MeasureDotInDirectionOfLoad, E_Minus, E_Multiplies, E_Norm , E_Omega, E_OmegaDot, E_OutputContactForce, E_Plus, E_PointToPointRotation, E_PointToPointRotationDot, E_Position, E_PotentialEnergy, E_ReferenceEnergy, E_RelativeAcceleration, E_RelativePosition, E_RelativeVelocity, E_RotationalRelativeDOF, E_SphericalStop, E_StopVelocity, E_StopStatus, E_Time, E_TimeStep, E_TranslationalJoint, E_UniversalAngles, E_User, E_Velocity, E_Violation, E_XYZAnsysRotationAngles, E_ZYXRotationAngles, Members: Length: Number of components of the measure Example: nbValues = Measure.Length Type: Measure type Calculation Method: A measure can use direct calculation, or be time integrated. On a measure that uses direct calculation, it is possible to retrieve the measure value through time. On a measure that is time-integrated, both values and time derivatives can be retrieved. 118 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Name: Measure Name Member Functions: FillValuesThroughTime(): Returns a two dimensional array. This function shall be called after the solution has been performed. The first dimension of the returned array is the number of time values in the transient. The second dimension is the size of the measure plus one: the first column contains the time values, while the subsequent columns contain the corresponding measure values. FillDerivativesThroughTime(): Returns a two dimensional array. This function shall be called after the solution has been performed. The first dimension of the returned array is the number of time values in the transient. The second dimension is the size of the measure plus one: the first column contains the time values, while the subsequent columns contain the corresponding measure derivatives. These derivatives are available on measures that are time integrated. To know if a measure is time integrated, use the CalculationMethod member. Derived Classes: CS_JointVelocityMeasure: Joint velocities, both translational and rotational, are expressed in the joint reference coordinate system. The number of components is the number of translational degrees of freedom plus the number of rotational degrees of freedom. For example, for a revolute joint, the size of the joint velocity measure is 1. It contains the relative joint rotation velocity along the z axis of the joint reference coordinate system. For a slot joint, the size of the measure will be 4; one component for the relative translational velocity, and the 3 components of the relative rotational velocity. The joint velocity measure can be obtained from the joint using the “GetVelocity” function. Rotational velocities are expressed in radians/second. CS_JointAccelerationMeasure: Joint accelerations, both translational and rotational, are expressed in the joint reference coordinate system. The number of components is the number of translational degrees of freedom plus the number of rotational degrees of freedom. The joint acceleration measure can be obtained from the joint using the “GetAcceleration” function. CS_JointRotationMeasure: • For revolute joints, cylindrical joints, or single rotation general joints, this measure has only one component — the relative angle between the reference and the moving coordinate system of the joint. Rotations are expressed in radians. • For slots, spherical joints, bushing joints, and 3 rotation vectors, this measure contains values that are not directly usable. • For universal joints, it contains the two joint axis rotational velocities. (The first one along the X axis of the reference coordinate system and the second along the Z axis of the moving coordinate system). These angles are expressed in radians. CS_JointTranslationMeasure: : This measure contains only the joint relative translations, expressed in the joint reference coordinate system. The joint translation measure can be obtained from the joint using the “GetTranslation” function. CS_JointForceMeasure: This measure contains the total forces and moment that develop in the joint. This includes constraint forces, elastic forces and external forces. The joint velocity measure can be obtained from the joint using the “GetForce” function. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 119 Approach CS_ComponenetMeasure: This measure allows the extraction of one component of an existing measure. This component can be expressed in a non default coordinate system. Example: Planar = CS_Joint.Find(_jid) Vel = Planar.GetVelocity() Xglobaldirection = 0 VelX = CS_ComponentMeasure(Vel,Xglobaldirection) Sys.AddMeasure(VelX) PointTable Corresponding ID table: CS_PointTable Members Functions: CS_PointTable( tab ): “tab” is a two dimensional array, where the first column contains the input values, and the second column contains the corresponding output values. Example: tab = System.Array.CreateInstance(float,6,2) tab[0,0]=-100. tab[1,0]=-8. tab[2,0]=-7.9 tab[3,0]= 7.9 tab[4,0]= 8. tab[5,0]= 100. tab[0,1]=1.0 tab[1,1]=1.0 tab[2,1]=0.1 tab[3,1]=0.1 tab[4,1]=1.0 tab[5,1]=1.0 Table = CS_PointsTable(tab); Here, the output (shown as Stiffness in the chart above) varies in a linear, piece-wise manner. For values of input less than -8.0 or greater than 8.0, the output is equal to 1.0. For values between -7.9 and +7.9, the output is 0.1. The transition is linear between -8.0 and -7.9 , and as well between +7.9 and +8.0. Relation The relation object allows you to write constraint equations between degrees of freedom of the model. For example, two independent lines of shaft can be coupled using a relation between their rotational velocities. 120 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types If you have a gear coupling between two shafts where the second shaft rotates twice faster than the first one, you can write the following equation: 2.0 X Ω1 + Ω2 = 0 where Ω1 and Ω2 are joint rotational velocities. This relation contains two terms and a constant right hand side equal to zero. The first term (2 X Ω1) can be described using the following information: • A joint selection • A joint degree of freedom selection • The nature of motion that is used in the equation (joint velocities, which is the most common case). For convenience purpose, the nature of motion on which the constraint equation is formulated is considered as being shared by all the terms in the relation. This information defines Ω1 • The factor 2.0 in the equation can be described by a constant variable, whose value is 2.0 ID table: CS_Actuator The coefficients of the relation can be constant or variable; however, the use of non-constant coefficients is limited to relations between velocities and relations between accelerations. If non-constant coefficients are used for relations between positions, the solution will not proceed. Constants: E_Acceleration, E_Position, E_Velocity Members: None Member Functions: SetRelationType(type): type of relation, with type selected in the previous enumeration AddTerm(joint, dof, variable): Adds a term to the equation. • “joint” is a joint object. • “dof” is an integer, defining the joint degree of freedom to be included in the term. The ordering of the degrees of freedom sets the translation degrees of freedom first, and that the degrees of freedom numbering is zero based. For example, in a slot joint, the translational degrees of freedom is 0, while the third rotational degree of freedom is 3. • “variable” is a variable object. SetVariable(variable): sets the right hand side of the relation. “variable” is a variable object. Spring Corresponding ID table: CS_Actuator Members: None Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 121 Approach Member Functions: ToggleCompressionOnly() Calling this function on a translational spring will make the spring develop elastic forces only if its length is less than the spring free length. The free length has to be defined in the regular spring properties. ToggleTensionOnly() Calling this function on a translational spring will make the spring develop elastic forces only if its length is greater than the free length of spring. The free length has to be defined in the regular spring properties. SetLinearSpringProperties(system, stiffness, damping) Allows you to overwrite damping and stiffness of a translational spring. This can be useful to parameterize these properties. For example, system is the system object, stiffness and damping are the double precision values of stiffness and damping. SetNonLinearSpringProperties(table_id) Allows you to replace the constant stiffness of a spring with a table of ID table_id that gives the force as a function of the elongation of the spring. The table gives the relation between the force and the relative position of the two ends. GetDamper() The user interface has stiffness and damping properties of the spring. Internally, the Spring is made of two objects; a spring and a damper. This function allows you to access the internal damper using the Spring object in the GUI. Derived Classes: None System Corresponding ID table: CS_System Members: None Member Functions: AddMeasure(measure): Adds a measure to the system, to be calculated during the simulation. This function has to be called prior to solving so that the measure values through time can be retrieved. (istat,found,measure)=FindOrCreateInternalMeasure( MeasureType): Extracts an existing global measure on the system. Supported measure types are: E_Energy, E_PotentialEnergy, E_ElasticEnergy, E_KineticEnergy, and E_Time. Derived Classes: None Variable A variable is an n-dimensional vector quantity that varies over time. It is used to define the variation of a load or a joint condition, or to express the coefficients in a relation between degrees of freedom. For convenience purpose, the solver allows the creation of constant variables, where only the value of the constant has to be provided. More complex variables can be built using a function variable. A function variable is a function of input , where input is given by a measure and function is described by a table. In some cases, you will be able to replace the table or the measure of an internal variable as used in a joint condition. ID table: CS_Variable 122 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Members: None Member Functions: SetConstantValues(value): “value” is an array, whose size is equal to the size of the table. To create a constant scalar variable, the value can be defined as shown in the following example: value = System.Array[float]([1.0]): “System”, “Array”, and “float” are part of the Python language. The result of this is an array of size one, containing the value 1.0. AddInputMeasure(measure): “measure” is a measure object. The same variable can have more than one measure. The input variable of the variable is formed by the values of the input measure in the order that they have been added to the list of input measures. SetTable(table): “table” is a CS_PointTable. SetFunc(string, is_degree): “string” is an expression similar to the one used in the user interface when defining a joint condition by a function. Note that the literal variable is always called “time”, even if you are using another measure as input. "is_degree" is a boolean argument. If the expression uses a trigonometric function, it specifies that the input variable should be expressed in degrees. Derived Classes: ConstantVariable Examples Screw Joint Example The screw joint is not displayed by the Mechanical GUI. Basically, there are two ways of creating a screw joint. • Use a cylindrical joint and link translation and rotation by a relation, Tz = Pitch X Rz • Modify an existing cylindrical joint into the specialized screw joint. This approach is described as follows: Joint = CS_Joint.Find(_jid) Pitch = 2 Joint.ReplaceByScrew(Pitch) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 123 Approach Assign an ID (_jid) to the joint. Replace the joint by a screw joint giving the pitch. The pitch value is unit dependant. The joint where these commands are inserted must be a cylindrical joint. Constraint Equation This example shows the consideration of a gear mechanism. That is, creation of relation between two revolute joints in order to simulate a gear with a ratio 2. M. Commands will be used to enforce the ratio of velocities between the two wheels. That is, commands will create a linear relation between rotational velocities as: (1) X ω_1 + (-2) X ω_2 = 0 124 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types First retrieve the joint objects given their IDs. j1id = CS_Joint.Find(_jid) j2id = CS_Joint.Find (_jid) 1. A relation object is created and typed as a relation between velocities. rel=CS_Relation() rel.MotionType=CS_Relation.E_MotionType.E_Velocity 2. The constant coefficients that appear in the relation are created. For instance, the first constant term is created by: var1=CS_ConstantVariable() var1.SetConstantValues(System.Array[float]([1.])) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 125 Approach 3. Similarly, the second coefficient and constant right hand side are created by: var2=CS_ConstantVariable() var2.SetConstantValues(System.Array[float]([-2.])) varrhs=CS_ConstantVariable() varrhs.SetConstantValues(System.Array[float]([0.])) 4. The first term of relation (1) X ω_1 is added to the relation object via: rel.AddTerm(j1id,0,var1) The first argument here is the joint object. The second one prescribes the dof (degrees of freedom) of the joint which is involved in the relation. Here, 0 stands for the rotation as the joint has only one dof which is the rotation. 5. The second term and right hand side are introduced in the same manner. rel.AddTerm(j2id,0,var2) rel.SetVariable (varrhs) 6. The relation is added to the list of relations. Env=CS_Environment.GetDefault() Env.Relations.Add(rel) Joint Condition: Initial Velocity This example shows how to impose an initial velocity to a joint. More specifically, a velocity driver (joint condition) is created using commands and added to the list of initial conditions. During the transient solve, initial conditions are applied only at t=0. The complete list of commands is as follows. Joint=CS_Joint.Find(_jid) driver=CS_Driver(joint,System.Array[int]([0]),CS_Driver.E_MotionType.E_Velocity) Env=CS_Environment.GetDefault() Sys=Env.System (ret,found,time) = Sys.FindOrCreateInternalMeasure(CS_Measure.E_MeasureType.E_Time) driver.SetInputMeasure(time) driver.SetConstantValues(System.Array[float]([-4.9033])) Env.InitialConditions.Add(driver) The commands can be explained as follows: Joint=CS_Joint.Find(_jid) This allows you to retrieve the joint given its ID(_jid). Then, a velocity driver (imposed velocity) is created on this joint. driver=CS_Driver(joint,System.Array[int]([0]),CS_Driver.E_MotionType.E_Velocity) The driver constructor takes the joint instance as the first argument. The second argument is an array of integer that defines which DOFs are active. The physical meaning of these integers is dependent of the joint. For instance, if the underlying joint is a translation joint, 0 stands for the translation along x. But if the joint is a revolute, 0 now means the rotation along z axis. Similarly, for a cylindrical joint, 0 is used for the translation along z and 1 for the rotation. The last argument gives the type of driver here velocity. Drives can be of three types: position, velocity, or acceleration. Then, retrieve the default environment Env=CS_Environment.GetDefault() and the corresponding system 126 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Sys=Env.System This command returns an instance on an internal measure. It is often used to obtain the instance of the time measure. (ret,found,time) = Sys.FindOrCreateInternalMeasure(CS_Measure.E_MeasureType.E_Time) The time measure is specified as the input measure for the driver and a constant value is given to the driver. As the driver may be applied to several component of the joint, the values are given as an array of float. driver.SetInputMeasure(time) driver.SetConstantValues(System.Array[float]([-4.9033])) The driver is added to the list of initial conditions. Consequently, it will be active only at t=0 and will give an initial velocity to the joint. Env.InitialConditions.Add(driver) Joint Condition: Control Using Linear Feedback (Method 1) In this example, an existing load is modified in order to applied a torque proportional to the joint velocity. Obtain the velocity measure from the joint. Modify an existing moment in order to use the velocity measure as its input measure. Joint Condition: Control Using Linear Feedback (Method 2) Here, the load is entirely created using commands. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 127 Approach Non-Linear Spring Damper The following example shows how the behavior of a spring can be altered in order to introduce a nonlinear force-displacement relationship. Get the ID of the spring object. Spring=CS_Actuator.Find(_sid) An array of real values is created and filled with the pairs of values (elongation, force). Spring_table=System.Array.CreateInstance(float,7,2) Here, 7 stands for the number of rows and 2 for the number of columns. The first column gives elongation and the second, the corresponding force value. A PointsTable is created and assigned to the spring. 128 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Each spring object in Mechanical GUI is actually a combination of a spring and a damper. The GetDamper method allows you to retrieve the damper object on a given spring. Damper=spring.GetDamper() Introduce a table is to define a non-linear force velocity relation. Spherical stop Joint that has 3 rotations (spherical, slot, bushing, free and general joints) is called a spherical stop. The aim of this specific type of stop is to give a limit to the angle between z-axis of the reference frame and z-axis of the moving frame. This functionality is available through the command: AddStop(angle_max, restitution_factor) For instance, the following line Joint.AddStop(0.45,1.0) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 129 Approach Adds a spherical stop for an angle value equals to 0.45 radians. The restitution factor is equal to 1.0. An example of the model and the results are as follows: 130 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Extract Joint forces in the local coordinate system, rotate them into the global coordinate system, and write them into an ASCII file. Get the joint by inserting a command on the corresponding joint in the tree: TopRevolute = CS_Joint.Find(_jid) Insert a commands object in the result node: In this command: Get measures from the joint: TopRevoluteRotation = TopRevolute.GetRotation() Extract transient values for this measure: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 131 Approach TopRevoluteRotationValues=TopRevoluteRotation.FillValuesThroughTime() Get angle derivatives by extracting the time derivatives of the measure: TopRevoluteRotationDerivatives=TopRevoluteRotation.FillDerivativesThroughTime() Count the number of components of this array: nbValues = TopRevoluteRotationValues.GetLength(0) Open the ASCII output file: fich=open(r"TopRevoluteRotation.csv",'w') fich.write('Time,Rotation,Velocity\n') Loop over all time values, and write values for i in range(0,nbValues): fich.write('{0:4.3f},{1:11.4e},{2:11.4e}\n'.format(TopRevoluteRotationValues[i,0],TopRevoluteRotationValues[i,1], fich.close() Check if joint is « revert » or not : IsRevert = TopRevolute.IsRevert if IsRevert: fact = -1.0 else: fact = 1.0 Extract Force Measure and write them into the file TopRevoluteForce = TopRevolute.GetForce(); TRF=TopRevoluteForce.FillValuesThroughTime() fich=open(r"TopRevoluteForce.csv",'w') fich.write('Time,FX,FY,FZ,MX,MY,MZ\n') for i in range(0,nbValues): fich.write('{0:4.3f},{1:11.4e},{2:11.4e},{3:11.4e},{4:11.4e}, {5:11.4e},{6:11.4e}\n'.format(TRF[i,0],fact*TRF[i,1], fact*TRF[i,2],fact*TRF[i,3],fact*TRF[i,4],fact*TRF[i,5],fact*TRF[i,6])) fich.close() Get the joint reference coordinate system, and rotate the forces from the global coordinate system to the joint coordinate system: TopRevolute.ReferenceCoordinateSystem.RotateArrayThroughTimeToLocal(TRF) fich=open(r"TopRevoluteForceRotated.csv",'w') fich.write('Time,FX,FY,FZ,MX,MY,MZ\n') for i in range(0,nbValues): fich.write('{0:4.3f},{1:11.4e},{2:11.4e},{3:11.4e},{4:11.4e},{5:11.4e}, {6:11.4e}\n'.format(TRF[i,0],fact*TRF[i,1],fact*TRF[i,2],fact*TRF[i,3], fact*TRF[i,4],fact*TRF[i,5],fact*TRF[i,6])) fich.close() “Breakable” Joint Example Get the joint by inserting a command on a planar joint: joint=CS_Joint.Find(_jid) Create a joint condition to prescribe zero velocity on the two translational degrees of freedom: driver=CS_Driver(joint,System.Array[int]([0,1]),CS_Driver.E_MotionType.E_Velocity) Define the value of the velocity, then retrieve the time measure: 132 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types Env=CS_Environment.GetDefault() Sys=Env.System (ret,found,time)=Sys.FindOrCreateInternalMeasure(CS_Measure.E_MeasureType.E_Time) Define the time as variable, and use constant values for the two components: driver.SetInputMeasure(time) driver.SetConstantValues(System.Array[float]([0.,0.])) Next, make the driver only active if the force in the joint is less than a maximum threshold of 3N. To do that, create a Condition based on the joint force measure norm. Retrieve the force on the joint: force=joint.GetForce() Create a component measure, that is the norm 2 of the force. To be computed at each time step, this measure has to be added to the system. norm=CS_ComponentMeasure(force,-2) Sys.AddMeasure(norm) Now, create the condition and assign it to the driver: cond=CS_Condition(CS_Condition.E_ConditionType.E_LessThan,norm,3.0) driver.Condition=cond Finally, add the driver to the environment: Env.Drivers.Add(driver) Transient Thermal Analysis Introduction Transient thermal analyses determine temperatures and other thermal quantities that vary over time. The variation of temperature distribution over time is of interest in many applications such as with cooling of electronic packages or a quenching analysis for heat treatment. Also of interest are the temperature distribution results in thermal stresses that can cause failure. In such cases the temperatures from a transient thermal analysis are used as inputs to a structural analysis for thermal stress evaluations. Many heat transfer applications such as heat treatment problems, electronic package design, nozzles, engine blocks, pressure vessels, fluid-structure interaction problems, and so on involve transient thermal analyses. Point to Remember A transient thermal analysis can be either linear or nonlinear. Temperature dependent material properties (thermal conductivity, specific heat or density), or temperature dependent convection coefficients or radiation effects can result in nonlinear analyses that require an iterative procedure to achieve accurate solutions. The thermal properties of most materials do vary with temperature, so the analysis usually is nonlinear. Preparing the Analysis Create Analysis System Basic general information about this topic Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 133 Approach ... for this analysis type: From the Toolbox, drag the Transient Thermal template to the Project Schematic. Define Engineering Data Basic general information about this topic ... for this analysis type: Thermal Conductivity, Density, and Specific Heat must be defined for a transient thermal analysis. Thermal Conductivity can be isotropic or orthotropic. All properties can be constant or temperature-dependent. Attach Geometry Basic general information about this topic ... for this analysis type: There are no specific considerations for a transient thermal analysis. Define Part Behavior Basic general information about this topic ... for this analysis type: You can define a Thermal Point Mass for this analysis type. Define Connections Basic general information about this topic ... for this analysis type: In a thermal analysis only contact is valid. Any joints or springs are ignored. With contact the initial status is maintained throughout the thermal analysis, that is, any closed contact faces will remain closed and any open contact faces will remain open for the duration of the thermal analysis. Heat conduction across a closed contact face is set to a sufficiently high enough value (based on the thermal conductivities and the model size) to model perfect contact with minimal thermal resistance. If needed, you can model imperfect contact by manually inputting a Thermal Conductance value. Apply Mesh Controls/Preview Mesh Basic general information about this topic ... for this analysis type: 134 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Types There are no specific considerations for transient thermal analysis itself. However if the temperatures from this analysis are to be used in a subsequent structural analysis the mesh must be identical. Therefore in this case you may want to make sure the mesh is fine enough for a structural analysis. Establish Analysis Settings Basic general information about this topic ... for this analysis type: For a transient thermal analysis the basic controls are: Step Controls (p. 529), used to: i) specify the end time of the transient analysis ii) control the time step size and iii) create multiple steps when needed. The rate of loading could be important in a transient thermal analysis if the material properties vary rapidly with temperature. When such nonlinearities are present it may be necessary to apply the loads in small increments and perform solutions at these intermediate loads to achieve convergence. Multiple steps are needed if you want to change the solution settings, for example, the time step size or the solution output frequency over specific time spans in the transient analysis. Output Controls (p. 545) allow you to specify the time points at which results should be available for postprocessing. A transient analysis involves calculating solutions at several time points in the load history. However: i) you may not be interested in all the intermediate results and ii) writing all the results can make the results file size unwieldy. In this case you can restrict the amount of output by requesting results only at certain time points. Nonlinear Controls (p. 542) allow you to modify convergence criteria and other specialized solution controls. Typically you will not need to change the default values for this control. Analysis Data Management (p. 549) settings enable you to save specific solution files from the transient thermal analysis for use in other analyses. Define Initial Conditions Basic general information about this topic ... for this analysis type: A transient thermal analysis involves loads that are functions of time. The first step in applying transient thermal loads is to establish initial temperature distribution at Time = 0. The default initial condition for a transient thermal analysis is a uniform temperature of 22°C or 71.6°F. You can change this to an appropriate value for your analysis. An example might be modeling the cooling of an object taken out of a furnace and plunged into water. You can also use the temperature results from a steady-state analysis of the same model for the initial temperature distribution. A casting solidification study might start Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 135 Approach with different initial temperatures for the mold and the metal. In this case a steady-state analysis of the hot molten metal inside the mold can serve as the starting point for the solidification analysis. In the first iteration of a transient thermal analysis, this initial temperature is used as the starting temperature value for the model except where temperatures are explicitly specified. In addition this temperature is also used to evaluate temperature-dependent material property values for the first iteration. If the Initial Temperature field is set to Non-Uniform Temperature, a Time field is displayed where you can specify a time at which the temperature result of the steadystate thermal analysis (selected in Initial Condition Environment field) will be used as the initial temperature in the transient analysis. A zero value will be translated as the end time (of the steady-state thermal analysis) and this value can not be greater than the end time. Apply Loads and Supports Basic general information about this topic ... for this analysis type: The following loads are supported in a transient thermal analysis: • Temperature (p. 584) • Convection (p. 584) • Radiation (p. 586) • Heat Flow (p. 587) • Perfectly Insulated (p. 589) • Heat Flux (p. 589) • Internal Heat Generation (p. 590) • Imported Temperature (p. 605) • Imported Convection Coefficient (p. 603) In this analysis, the load’s magnitude could be a constant value or could vary with time as defined in a table or via a function. Details of how to apply a tabular or function load are described in Specifying Load Values (p. 621). In addition, see the Apply Loads and Supports section for more information about time stepping and ramped loads. Solve Basic general information about this topic ... for this analysis type: The Solution Information object provides some tools to monitor solution progress. Solution Output continuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. Any conver- 136 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics gence data output in this printout can be graphically displayed as explained in the Solution Information section. You can also insert a Result Tracker object under Solution Information. This tool allows you to monitor temperature at a vertex as the solution progresses. Review Results Basic general information about this topic ... for this analysis type: Applicable results are all thermal result types. Once a solution is available you can contour the results or animate the results to review the response of the structure. As a result of a nonlinear analysis you may have a solution at several time points. You can use probes to display the variation of a result item over the load history. Also of interest is the ability to plot one result quantity (for example, maximum temperature on a face) against another results item (for example, applied heat generation rate). You can use the Charts feature to develop such charts. Note that Charts are also useful to compare results between two analyses of the same model. Special Analysis Topics This section includes special topics available the Mechanical application for particular applications. The following topics are included: Static Analysis From Rigid Dynamics Analysis Thermal-Stress Analysis Fluid-Structure Interaction (FSI) Ansoft - Mechanical Data Transfer Icepak to Mechanical Data Transfer Mechanical-Electronics Interaction (Mechatronics) Data Transfer External Data Import POLYFLOW to Mechanical Data Transfer Simplorer/Rigid Dynamics Co-Simulation System Coupling Static Analysis From Rigid Dynamics Analysis You can perform a Rigid Dynamics Analysis (p. 102) and then change it to a Static Structural Analysis (p. 79) for the purpose of determining deformation, stresses, and strains - which are not available in the Rigid Dynamics analysis. Creating an Analysis System 1. From the toolbox, drag and drop a Rigid Dynamics template onto the project schematic. Follow the procedure for creating a rigid dynamics analysis. Apply forces and/or drivers, and insert any valid solution result object(s). 2. Specify the time of interest in the tabular data table or in the Graph window. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 137 Approach 3. Select a solution result object and click the right mouse to display the popup menu. Select Export Motion Loads and specify a load file name. 4. In the project schematic, duplicate the Rigid Dynamics analysis system. Replace the duplicated analysis system with a Static Structural analysis system. Note If you do not need to keep the original Rigid Dynamics analysis, you can replace it with the Static Structural analysis system. 5. Edit the Static Structural analysis (using Model, Edit) by suppressing all parts except the desired part for the Static Structural analysis. 6. Change the Stiffness Behavior of the part to be analyzed from Rigid to Flexible. 7. Change mesh solver preference to be ANSYS Mechanical instead of ANSYS Rigid Dynamics. 8. Delete or suppress all loads used in the Rigid Dynamics analysis. 9. Import the motion loads that were exported from the Rigid Dynamics analysis. Highlight the Static Structural branch and then right mouse click, Insert> Motion Loads.... Note Moments and forces created for the static structural analysis can be in an invalid state if all three components of the force/moment are almost equal to zero. 10. Delete the result objects and add new ones. 11. Solve the single part model with the static structural analysis and evaluate the results. Point to Remember It is important that you create the Static Structural analysis after the Rigid Dynamics analysis is finished and the export load is done. Thermal-Stress Analysis The Mechanical application allows you to apply temperatures from a thermal analysis as loads in a structural analysis for thermal stress evaluations. The load transfer is applicable for cases when the thermal and structural analyses share the mesh as well as for cases when the two analyses are solved using different meshes. For cases when the meshes are different, the temperature values are mapped and interpolated between the source and target meshes. Workflow for performing a thermal stress analysis with: • 138 Shared Model 1. From the toolbox, drag and drop a transient or steady-state thermal template onto the project schematic. Perform all steps to set up a Steady-State Thermal or Transient Thermal. Specify mesh controls, boundary conditions, and solution settings as you normally would and solve the analysis. 2. Drag and drop a Static Structural or Transient Structural template on top of the thermal systems solution cell to enable the data transfer. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics 3. Double-click the structural systems Setup cell. In the Mechanical application an Imported Body Temperature load is automatically added into the structural system's tree under an Imported Load folder. 4. Select appropriate geometry in the Details view of the Imported Body Temperature object using the Geometry or Named Selection scoping option. If the load is scoped to one or more surface bodies, the Shell Face option in the details view allows you to apply the temperatures to Both faces, to the Top face(s) only, or to the Bottom face(s) only. See Imported Body Temperature for additional information. 5. Change any of the columns in the Data View tab as needed: – Source Time - Time at which the temperatures will be imported from the thermal analysis. – Analysis Time - Choose the analysis time at which the load will be applied. This must coincide with the end time of a step defined in the Analysis Settings object in the tree. 6. Right-click the Imported Body Temperature object and click Import Load to import the load. When the load has been imported successfully, a contour plot of the temperatures will be displayed in the Geometry window. 7. To preview the imported load contour that applies to a given row in the Data View, use the Preview Row option in the Details view. Note You can also create the linked thermal and structural systems by choosing the predefined Thermal-Stress template from the Custom Systems toolbox in the project schematic. • Unshared Model 1. From the toolbox, drag and drop a transient or steady-state thermal template onto the project schematic. Perform all steps to set up a Steady-State Thermal or Transient Thermal. Specify mesh controls, boundary conditions, and solution settings as you normally would and solve the analysis. 2. Drag and drop a Static Structural or Transient Structural template onto the project schematic. Share the Engineering Data and Geometry cells if required and then drag the Solution cell of the thermal system onto the Setup cell of the structural system. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 139 Approach 3. Double-click the structural systems Setup cell. In the Mechanical application, an Imported Body Temperature load is automatically added into the structural system's tree under an Imported Load folder. 4. Select appropriate geometry in the Details view of the Imported Body Temperature object using the Geometry or Named Selection scoping option. If the load is scoped to one or more surface bodies, the Shell Face option in the details view allows you to apply the temperatures to Both faces, to the Top face(s) only, or to the Bottom face(s) only. See Imported Body Temperature for additional information. Note In a 3D analysis, if the Triangulation mapping algorithm is used, the Transfer Type mapping option defaults to Surface when the load is scoped to shell bodies. 5. The Source Bodies option in the Details view allows you to select the bodies, from the thermal analysis, that make up the source mesh for mapping the data. You can choose one of the following options: – Automatic- Heuristics based on the geometry are used to automatically match source and target bodies and map temperature values. A source body is matched with a target body if it satisfies the below criteria. a. The percent volume difference is within the user defined tolerance. b. The distance between the centroid locations divided by the diagonal of the bounding box is within the user defined tolerance. The percent tolerance values can be specified in the Tolerance field. The default is set at 1%. The matching process is done in increments of 0.1 of the tolerance value, up to the defined tolerance. The process fails if multiple source bodies are found to match a target body or if no match is found for a target body. After the import is completed, a Load Transfer Summary is displayed as a comment object in the particular load branch. The summary shows the matched source and target bodies as well as the values that were used to determine the match. It is recommended that you verify the import using this information. 140 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics Important This option requires the element volume results to be present in the thermal results file. Make sure that the Calculate Thermal Flux or the General Miscellaneous Details view property under the Analysis Settings object in the thermal analysis is set to Yes, so that this result is available. – All- The source mesh in this case will comprise of all the bodies that were used in thermal analysis. For cases where the temperature values are significantly different at the boundaries across two or more bodies, this option could result in mapped target values that are generated by taking a weighted average of the source values across multiple bodies. Target regions can exists where the mapped temperatures differ significantly from the source. – Manual- This option allows you to select one or more source bodies to make up the source mesh. The source body selections are made in the Material IDs field by entering the material IDs that correspond to the source bodies that you would like to use. Type material IDs and/or material ID ranges separated by commas to specify your selection. For example, type 1, 2, 5-10. The material IDs for the source bodies can be seen in Solution Information Object of the source analysis. In the example below, text is taken from a solver output, ***********Elements for Body 1 "coil" *********** ***********Elements for Body 2 "core" *********** ***********Elements for Body 3 "bar" ************ body 'coil' has material ID 1, body 'core' has material ID 2 and body 'bar' has material ID 3. 6. Change any of the columns in the Data View tab as needed: – Source Time - Time at which the temperatures will be imported from the thermal analysis. – Analysis time - Choose the analysis time at which the load will be applied. This must coincide with the end time of a step defined in the Analysis Settings object in the tree. 7. You can modify the Mapper Settings to achieve the desired mapping accuracy. 8. Right-click the Imported Body Temperature object and click Import Load to import the load. When the load has been imported successfully, a contour plot of the temperatures will be displayed in the Geometry window. 9. To preview the imported load contour that applies to a given row in the Data View, use the Preview Row option in the Details view. Note a. You can add a template for the linked thermal and structural systems by creating your own template. b. The transfer of temperatures is not allowed between a 2D analysis and 3D analysis or vice-versa. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 141 Approach Note When there is a shared model that includes a thermal-stress analysis and the structural system is duplicated using the Engineering Data, Geometry or Model cell context menu, the result is the Setup cell of the Thermal system linked to the Solution cell of the duplicated structural system. Temperature transfer to the duplicated structural system will require the data to be mapped and interpolated between the source and target meshes. Fluid-Structure Interaction (FSI) Fluid-Structure Interaction (FSI) analysis is an example of a multiphysics problem where the interaction between two different analyses is taken into account. The FSI analysis in the Mechanical application involves performing a structural analysis in the Mechanical application taking into account the interaction with the corresponding fluid or previous CFD analysis. The interaction between the two analyses typically takes place at the boundary of the Mechanical application model - the fluid-structure interface, where the results of one analysis is passed to the other analysis as a load. A structural stress analysis can also be performed in the Mechanical application by transferring temperatures across solid bodies from a previously calculated heat transfer CFD analysis. The Mechanical application supports two types of Fluid-Structure Interaction: One-way FSI: The result (forces or temperature or convection load) from a CFD analysis at the fluidstructure interface is applied as a load to the Mechanical application analysis. The boundary displacement from the Mechanical application is not passed back to the CFD analysis, that is, the result from the Mechanical application is not considered to have significant impact on the fluid analysis. Temperature results from a heat transfer CFD analysis are directly input as body loads in a structural analysis to determine the corresponding displacement and stresses. Two-way FSI: In this analysis the results of structural analysis in the Mechanical application are transferred to the CFD analysis as a load. Similarly the results of the CFD analysis are passed back to the Mechanical application analysis as a load. For example, the fluid pressure at the boundary can be applied as a load on the structural analysis in the Mechanical application and the resulting displacement, velocity or acceleration obtained in the Mechanical application could be passed on as a load to the CFD analysis. The analyses will continue until overall equilibrium is reached between the Mechanical application solution and CFD solution. Two-way FSI is supported between Mechanical and FLUENT and Mechanical and CFX. Typical applications of FSI include: • Biomedical applications, such as drug delivery pumps, intravenous catheters, elastic artery modeling for stent design. • Aerospace applications, such as airfoil flutter and turbine engines. • Automotive applications, such as under hood cooling, HVAC heating/cooling, and heat exchangers. • Fluid handling applications, such as valves, fuel injection components, and pressure regulators. • Civil engineering applications, such as wind and fluid loading of structures. • Electronics cooling. 142 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics Fluid-Structure Interaction (FSI) - One-Way Transfer This feature enables you to import fluid forces, temperatures, and convections from a steady-state or transient CFD analysis into a Mechanical application analysis. This one-way transfer of face forces (tractions) at a fluid-structure interface allows you to investigate the effects of fluid flow in a static or transient structural analysis. Similarly the one-way transfer of temperatures or convection information from a CFD analysis can be used in determining the temperature distribution on a structure in a steady-state or transient thermal analysis or to determine the induced stresses in a structural analysis. To import loads from a CFD analysis: 1. In the Project Schematic, add an appropriate analysis with data transfer to create a link between the solution of a CFD analysis and the newly added analysis. 2. Attach geometry to the analysis system, and then double-click Setup to open the Mechanical window. An Imported Load folder is added under the Environment folder, by default. 3. To add an imported load, click the Imported Load folder to make the Environment toolbar available or right mouse click on the Imported Load folder and select the appropriate load from the context menu. 4. On the Environment toolbar, click Imported Load, and then select an appropriate load. 5. Select appropriate geometry, and then click Apply. 6. In a structural analysis, if the Imported Body Temperature load is scoped to one or more surface bodies, the Shell Face option in the details view allows you to apply the temperatures to Both faces, to the Top face(s) only, or to the Bottom face(s) only. See Imported Body Temperature for additional information. 7. Select appropriate options in the Details view. a. b. Under Transfer Definition, • For surface transfer, click the CFD Surface list, and then select the corresponding CFD surface. • For volumetric transfer, click the CFD Domain list, and then select the corresponding CFD Domain. For CFD Convection loads only: Select the appropriate Ambient Temperature Type. Note CFD Near-Wall Ambient (bulk) Temperature (default): This option uses the fluid temperature in the near-wall region as the ambient temperature for the film coefficient calculation. This value will vary along the face. Constant Ambient Temperature: This constant value applies to the entire scoped face(s). The film coefficient will be computed based on this constant ambient temperature value. Use of a constant ambient temperature value in rare cases may produce a negative film coefficient if the ambient temperature is less than the local face temperature. If this is the case, you can define a Supplemental Film Coefficient. This value will be used in place of the negative computed film coefficient and the ambient temperature adjusted to maintain the proper heat flow. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 143 Approach 8. Under Data View, select the Source Time, for the imported load. The Source Time Step value changes based on the source time you select. If the selected source time corresponds to more than one source time step, you will also need to select the desired time step value. You can also change the Analysis Time and specify Scale and Offset values for the imported loads. 9. In the Project tree, right-click the imported load, and then click Import Load to import the load. When the load has been imported successfully, a contour plot will be displayed in the Geometry window. After the solution is complete, a CFD Load Transfer Summary is displayed as a Comment in the particular CFD load branch. The summary contains the following information: • For a CFD Pressure load: the net force, due to shear stress and normal pressure, on the face computed in CFD and the net force transferred to the Mechanical application faces. • For a CFD Temperature load: For surface transfers - the average computed temperature on the CFD boundary and the corresponding average mapped temperature on the Mechanical application faces. For volumetric transfers – the average, maximum, and minimum temperature of the CFD domain and the corresponding Mechanical Application body selection(s). • For a CFD Convection load: the total heat flow across the face, and the average film coefficient and ambient temperature on the face. The computed and mapped face data may be compared in order to get a qualitative assessment of the accuracy of the mapped data. The following is an example of a CFD Load Transfer Summary for a CFD Pressure load. Note The force values shown in the CFD Load Transfer Summary should only be used as a qualitative measure of the load transferred from CFD to the Mechanical application mesh. In the example above, the closer the CFD Computed forces are to the Mechanical application Mapped Forces, the better the mapping. The actual force transferred to the Mechanical application is reflected in the reaction forces. The following topics are covered in this section: Face Forces at Fluid-Structure Interface Face Temperatures and Convections at Fluid-Structure Interface Volumetric Temperature Transfer CFD Results Mapping Face Forces at Fluid-Structure Interface You can use results at a fluid-structure interface from a CFD analysis as face forces (from the vector sum of the normal pressures and shear stresses) on corresponding faces in the Mechanical application. The import process involves interpolating a CFD solution onto the Mechanical application face mesh. This requires that the following conditions are met: 144 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics • The fluid-structure interface must be a defined boundary in CFD. • The location of the CFD boundary (with respect to the global Cartesian coordinate system) must be the same as the corresponding face(s) in the Mechanical application model. Refer to the Imported Loads (p. 630) section for more information. Face Temperatures and Convections at Fluid-Structure Interface This feature allows the transfer of either of the following thermal solutions from a CFD solution boundary to a corresponding face in the Mechanical application model: • Temperatures at the fluid-structure interface. • Film coefficients and bulk temperature values at the fluid-structure interface. The import process involves interpolating a CFD solution onto the Mechanical application face mesh. This requires that the following conditions are met: • The fluid-structure interface must be a defined boundary in CFD. • The location of the CFD boundary (with respect to the global Cartesian coordinate system) must be the same as the corresponding face(s) in the Mechanical application model. Refer to the Imported Loads section for more information. Volumetric Temperature Transfer You can transfer temperature results from a CFD analysis and apply them as body loads in the Mechanical application. The import process involves interpolating a CFD solution onto the mesh for the bodies selected in the Mechanical application. This requires that the following condition is met: • The location of the bodies in the Mechanical application model (with respect to the global Cartesian coordinate system) must be the same as the corresponding CFD domains. CFD Results Mapping When mapping CFD results onto the Mechanical application face(s) the Mechanical nodes are projected on to the CFD face. All the Mechanical application face nodes will map to the CFD face according to the following rules: a. Project normal to the CFD mesh faces. b. If rule a fails, project to the closest edge. c. If rule b. fails, project to the closest node on the CFD face. Rule c. will always work, so in the end every node will get some kind of mapping. However the most accurate load mapping occurs for nodes projected normal to the mesh face. The percentage of the Mechanical application nodes that mapped successfully using rule a. above is reported in the diagnostics. When the Mechanical application mesh is very coarse, there can be some misses near the edges of the CFD boundary. However all nodes become mapped eventually. The accuracy of force transfer improves as the Mechanical application mesh is refined. When mapping CFD domain results onto the corresponding Mechanical Application body selection(s), all the Mechanical Application nodes that cannot be mapped to the CFD domain will be set to the average temperature. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 145 Approach Fluid-Structure Interaction (FSI) - Two-Way Transfer This feature enables you to perform a two-way fluid structure interaction problem by setting up the static or transient structural portion of the analysis in the Mechanical application that includes defining faces associated with the fluid-structure interface, continuing the analysis in CFD-Solve, and viewing the structural results in the Mechanical application. Two-way FSI is supported between Mechanical and FLUENT and Mechanical and CFX. For more information on two-way FSI using Mechanical and FLUENT, see System Coupling (p. 163). For more information on two-way FSI using Mechanical and CFX, see Coupling CFX to an External Solver: ANSYS Multi-field Simulations in the CFX-Solver Modeling Guide. Ansoft - Mechanical Data Transfer You can import a thermal load generated by the HFSS, Maxwell, or Q3D Extractor application and perform an analysis using the load. In the case of loads originating from HFSS and Maxwell, you can also export the thermal results obtained from the Mechanical analysis so that they can be imported back into HFSS or Maxwell. You can also import force densities generated by the Maxwell application and perform a structural analysis using the load. The resulting deformation results can also be exported and applied during the subsequent solve of the upstream Maxwell analysis. Overall Workflow for an Ansoft - Mechanical Analysis 1. Create and solve the electromagnetic application using HFSS, Maxwell, or Q3D Extractor. 2. Drag and drop a steady-state thermal, transient thermal, static structural or transient structural template on top of the HFSS, Maxwell, or Q3D Extractor systems solution cell to enable the data transfer. 3. Attach geometry to the Mechanical application, and then double-click Setup to open the Mechanical window. An Imported Load folder is added under the Environment folder, by default. 4. Add appropriate imported loads and set their options. 5. Perform all steps to set up a steady-state thermal, transient thermal, static structural or transient structural analysis. Specify mesh controls, boundary conditions, and solution settings as you normally would. 6. Solve the ANSYS thermal or structural analysis. 7. If applicable, export your results to be imported by those applications. Thermal/Structural Load Import This feature enables you to perform a one-way Ansoft - Mechanical interaction problem by solving the electromagnetic analysis of the geometry in the HFSS, Maxwell, or Q3D Extractor applications, importing the thermal or structural results into the ANSYS Mechanical application where the defined load is applied to a thermal or structural analysis which is then solved and post processed. For a thermal analysis the allowed imported load types are: • Imported Heat Generation • Imported Heat Flux For a structural analysis the allowed imported load types are: • 146 Imported Body Force Density Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics • Imported Surface Force Density Add the Imported Ansoft Load Follow these steps to add an imported Ansoft load and associate it with parts of the geometry. 1. Double-click on the Model cell in your analysis system to open the Mechanical application. 2. Click on the Imported Load group object. In the Details view, set the following field as needed: • 3. If you want to suppress all of the loads under this Imported Load group, set the Suppressed field to Yes. There are several ways to select an imported load and associate it with a part of your model. • Click on an Imported Load Group object in the tree, click on a part of the model, then right click on Imported Loads (Ansoft) and from the Import menu item select the desired load type from the allowed imported load types. The load will be applied to the object you selected on the model. • Click on an Imported Load Group object in the tree, then click on the Imported Loads button in the toolbar and select the desired load type from the allowed imported load types. In the Details view, click on the Geometry field. Select the objects in the model to which you want to apply the load and click the Apply button in the Geometry field. • Right click on the Imported Loads Group object that was just added to the tree and select the desired load type from the allowed imported load types. In the Details view, click on the Geometry field. Select the objects in the model to which you want to apply the load and click the Apply button in the Geometry field. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 147 Approach Note Heat generation loads scoped to a surface body use the constant thickness value specified in the details view of the surface body object when data is imported. Surface body thickness defined using the thickness object is not accounted for when data is imported. Set the Imported Load Options 1. Click on the imported load object that you've added to the tree. 2. Select the desired Ansoft solution you would like to import the load from. Some of the properties in the Details view and Data View tab are filtered based on this selection. 3. Change any of the fields in the Details View as needed: • Scoping Method– Select the method of choosing objects to which the load is applied: Geometry Selection or Named Selection. • Geometry or Named Selection– Use these fields to choose the objects to which the load is applied, as appropriate from your Scoping Method choice. • Suppressed– Select Yes to suppress this load • Ansoft Surface(s)– Select the Ansoft Surface(s) for a Heat Flux or Surface Force Density load or Ansoft Volume(s)– Select the Ansoft Volume(s) for a Heat Generation or Body Force Density load Set the Imported Load Analysis Options You can specify when the imported data should be applied and also modify the imported data, either by adding an offset or by using a scale factor. To see the analysis setting for a load, click on the object that you've added to the tree. The analysis options appear in the Data View tab of the window below the model. Make any changes to the load's analysis options as indicated below. Change any of the columns in the Data View tab as needed: • Source Frequency– Select from the drop-down list one of the frequencies supplied from the transfer file. The load values associated with this frequency will be imported. • Source Time– Select from the drop-down list one of the Source Times supplied from the transfer file. The load values associated with this time will be imported. • For thermal loads from Maxwell transient solutions, you must select from the drop-down list the desired Source Start Time and Source Stop Time to define the interval for integrating the power loss density distribution. • Analysis Time– Choose the analysis time at which the load will be applied. This must coincide with the end time of a step defined in the Analysis Settings object in the tree. • Scale– The amount by which the imported load values are scaled before applying them. • Offset– An offset that is added to the imported load values before applying them. 148 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics You must re-solve after making any changes to the analysis options of a load. You can define multiple rows in the Data View tab to import additional data from the selected Ansoft solution and apply the rows at different analysis times. If multiple rows are defined in the Data View tab, you can display imported values at different time steps by changing the Active Row option in the Details pane. Right-click the Imported Load object and click Import Load to import the load. When the load has been imported successfully, a contour plot of the temperatures will be displayed in the Geometry window and a summary of the transfer is displayed as a comment in the particular load branch. Thermal/Structural Results Export If you have solved an analysis containing loads imported from Maxwell or HFSS, you can choose to export temperature or deformation results and apply them during the subsequent solve of the upstream analysis, if this option was previously set in the upstream analysis. • Temperature results can be exported back to HFSS or Maxwell from a thermal analysis • Deformation results can be exported to Maxwell from a structural analysis. Click on the Imported Load Group object in the tree to view the Details for the load. If the export option is set, you will see an Export Definition section in the Details View. The Setup field allows you to specify the Ansoft Setup for which the exported results will be written. The All option for the Setup field exports results to all the setups requesting feedback. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 149 Approach In the Details view you can also set the analysis time at which results are exported. The default is the end time of the analysis, which you select by entering 0. You must enter a value between 0 and the end time of the analysis. If you want to export the results automatically at the end of the analysis, click on the Imported Load (Ansoft) object in the tree before you start the analysis. In the Details panel, set the Export After Solve field to Yes. The results will be written when the solution has finished. If you want to export the results manually after the analysis, click on the Imported Load (Ansoft) object in the tree before you start the analysis. In the Details panel, set the Export After Solve field to No. To export the file after the solution, right click on the Imported Load (Ansoft) object in the tree. Select Export Results. The results will be written to the file. If necessary, you can modify the load transfer Mapper Settings for the export. Note Refer to the Ansoft application documentation for more details on settings required to support the export from the Mechanical application to the Ansoft application. Results can only be exported to setups that have contributed to the current solution. 150 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics Icepak to Mechanical Data Transfer The Mechanical application allows you to transfer temperature data from Icepak into Mechanical. This process involves the import of temperature data from the solid objects defined in Icepak onto the geometry defined in Mechanical. As the meshes used in Icepak and Mechanical could be quite different, mapping the temperatures involves an interpolation method between the two. Once the mapping is completed, it is possible to view the temperatures and utilize them to perform a Mechanical analysis. The workflow is outlined below. Workflow for Icepak Data Transfer 1. In Icepak, perform all steps for an Icepak analysis by creating the Icepak model, meshing and solving the model. After the solution has finished, Icepak writes out the temperature data for each of the solid objects to a file with the extension loads. In addition, a summary file with the extension load summary is written out. 2. Drag and drop a Mechanical cell, which could be one of Static Structural, Steady-State Thermal, Transient Structural, Transient Thermal, or Thermal-Electric analysis on top of the Icepak Solution cell. 3. Import the geometry or transfer the geometry into the Mechanical application. Double click the Setup cell to display the Mechanical application. 4. In the Details section of Imported Temperature or Imported Body Temperature under Imported Loads, you will first select the Scoping method. Select Geometry Selection as the Scoping method unless you have created a Named Selection. See Scoping Analysis Objects to Named Selections (p. 371) for a detailed description. 5. If Geometry Selection is selected as the Scoping method, pick the geometry using Single select or Box select and click Apply or select a Named Selection object in the drop down list. 6. In a structural analysis, if the Imported Body Temperature load is scoped to one or more surface bodies, the Shell Face option in the details view allows you to apply the temperatures to Both faces, to the Top face(s) only, or to the Bottom face(s) only. See Imported Body Temperature for additional information. 7. To suppress this load, select Yes. Otherwise, retain the default setting. 8. In the drop-down field next to Icepak Body, select one body at a time, All or a Named Selection. If selecting an individual body, make sure your selection corresponds to the volume selected in step 5. If All bodies were selected, select All. 9. The Icepak Data Solution Source field displays the Icepak temperature source data file. 10. You can modify the Mapper Settings to achieve the desired mapping accuracy. 11. Click on the imported load object, then right-click and select Import Load. This process first generates a mesh, if one doesn't already exist, and then interpolates the temperatures from the Icepak mesh onto the Mechanical mesh. This process might take long if the mesh size or the number of bodies is large. Improving the quality of the mesh will improve the interpolation results but the computation time may be higher. Note If the import is successful, you can see the temperature plot in the graphics display window. If multiple time steps refer to the same time, an error will be displayed in the Mechanical message window. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 151 Approach 12. You can apply other boundary conditions and click Solve to solve the analysis. How to Set up a Transient Problem 1. In Icepak, perform all steps for a transient Icepak analysis and solve the model. 2. Perform steps 2 – 9 as described above. 3. Click the Analysis Settings object in the tree. Begin adding each step's End Time values for the various steps to the tabular data window. You can enter the data in any order but the step end time points will be sorted into ascending order. The time span between the consecutive step end times will form a step. You can also select a row(s) corresponding to a step end time, click the right mouse button and choose Delete Rows from the context menu to delete the corresponding steps. See Establish Analysis Settings (p. 9) for further information. Whenever a new row is added or deleted, the imported body temperature data view will be updated to match the number of rows in the Analysis Settings. 4. Click on the imported load object and the Data View tab with updated Analysis Times is displayed. If the Analysis Time is different, the Source Time will display the original time, matching to the closest available Source Time coming from Icepak. If the match is not satisfactory, you can select a Source Time(s) from the drop-down list and Mechanical will calculate the source node and temperature values at that particular time. This combo box will display the union of source time and analysis time values. The values displayed in the combo box will always be between the upper and lower bound values of the source time. If the user modifies the source time value, the selection will be preserved until the user modifies the value even if the step's end time gets changed on the analysis settings object. If a new end time value is added/deleted, Source Time will get the value closest to the newly added Analysis time value. 5. Click on the imported load object, then right-click and select Import Load. This will interpolate the value at all the selected time steps. 6. User can display interpolated temperature values at different time steps by changing the Active Row option in the detail pane. 7. Apply required boundary conditions, continue with any further analysis and solve. Mechanical-Electronics Interaction (Mechatronics) Data Transfer You can export a reduced model that can be imported into Simplorer. Overall Workflow for Mechatronics Analysis 1. Create a modal analysis system. 2. Define the inputs using Remote Points and/or Named Selections. The names of the entities created must include the prefix input_ and the degree of freedom in the trailing suffix, signified by an underbar (e.g. "input_MyName_ux"). 152 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics Note The Named Selection can only be scoped to a vertex. 3. Define the outputs using Named Selection. The names of the entities created must include the prefix output_ and the degree of freedom in the suffix (e.g. "output_MyName2_rotx”). Note The Named Selection can only be scoped to a vertex. 4. Specify the modal damping in a Commands Object under an Environment, e.g.: dmprat,.02 mdamp,1,.05 5. ! 2% damping on all modes ! 5% damping on mode 1 At Solution level, add a Commands Object and import the macro ExportStateSpaceMatrices.mac to export the reduced model. It is located at the installation folder under: ANSYS Inc\v121\AISOL\DesignSpace\DSPages\macros Note The macro is based on the APDL command SPMWRITE. 6. Solve the Modal Analysis. 7. The reduced model file (file.spm) and the graphics file (file_spm.png) will exist in the solver files directory and can then be imported into Simplorer. (See Project File Management in Workbench User Guide for more information on solver files directories.) Set up the Mechanical Application for Export to Simplorer To set up the Mechanical application to retrieve the inputs and outputs defined so they can be used in the reduced model exported to Simplorer: 1. From the Tools menu in the Mechanical application, select Variable Manager. 2. In the Variable Manager window, add/activate the variable ExportToSimplorer and set it to 1. External Data Import This feature enables you to import data from one or more text files and apply it in a Mechanical application analysis. Data can be imported into a static structural, transient structural1, steady state thermal, transient thermal or thermal-electric analysis. To import data from an external file: 1. 1 In the Project Schematic, add any number of files to an External Data system and specify the necessary details. The rigid dynamics solver is not supported. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 153 Approach 2. 3. • When multiple files are added to the same External Data system, each file is given a unique identifier (that is, File1, File2, and so on). These identifiers are used in conjunction with the data identifiers (Pressure1, Thickness1, and so on) to identify and apply the dataset(s) within Mechanical. • If your files contain data for the same nodal coordinates, or if only one of your files contains the nodal information, you can choose the Master option in the External Data system to designate a master file. This option notifies the mapping utility that the group of files, defined in the External Data system, share the same nodal information. The nodal information is therefore processed and stored only from the master file. This greatly reduces the memory usage by only allocating space for the nodes once, not once per file. It can also result in much faster import times as only one mapping operation will be required. To transfer data to Mechanical, create a link between the Setup cell of the External Data system and that of an applicable downstream system. • To transfer shell thickness data to Mechanical, right-click the Setup cell of the External Data system and select Transfer Data to New, a link is created to the Model cell of a new Static Structural system. If you select Transfer Data to New > <mechanical system>, this operation automatically creates a link to the Model cell of the Mechanical system. Alternatively, you can drag the Setup cell of the External Data and drop it onto the Model cell of a Mechanical system to create the link. • To transfer load data to Mechanical, drag the Setup cell of the External Data system and drop it onto the Setup cell of an applicable Mechanical system. Attach geometry to the analysis system, and then double-click Setup to open the Mechanical window. If your simulation has a shell thickness defined from an External Data system2, an Imported Thickness folder is added under the Geometry folder. 1. Select appropriate geometry in the Details view, and then click Apply. 2. Select appropriate options in the Details view. You can modify the mapping settings to achieve the desired mapping accuracy. 3. You can specify a thickness value for the unmapped target nodes using the Unmapped Data Value property. By default, a zero thickness value is assigned to the unmapped nodes. Important For the ANSYS solver, the thickness value at each node must be greater than zero. 4. Right-click the Imported Thickness, and then click Import Thickness to import the thickness. When the thickness has been imported successfully, a contour plot will be displayed in the Geometry window and any mesh display will be based upon the mapped thickness of the elements. If your simulation has load data defined from an External data system, an Imported Load folder is added under the Environment folder. 1. To add an imported load, click the Imported Load folder to make the Environment toolbar available, or right-click the Imported Load folder and select the appropriate load from the context menu. 2 That is, from another application such as static structural, structural transient, structural buckling, structural harmonic, structural modal, structural response spectrum, thermal steady state, or thermal transient. 154 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics 2. Select appropriate geometry in the Details view, and then click Apply. 3. In a 3D structural analysis, if the Imported Body Temperature load is scoped to one or more surface bodies, the Shell Face option in the details view enables you to apply the temperatures to Both faces, to the Top face(s) only, or to the Bottom face(s) only. See Imported Body Temperature for additional information. 4. When mapping data to surface bodies, you can control the effective offset and thickness value at each target node, and consequently the location used during mapping, by using the Shell Thickness Factor property. By default, the thickness value at each target node is ignored when data is mapped. You can choose to enter a positive or negative value for the Shell Thickness Factor. This value is multiplied by each target node’s physical thickness and is used along with the node’s offset to determine the top and bottom location of each target node. A positive value for the Shell Thickness Factor uses the top location of each node during mapping, while a negative value uses the bottom location of each node. For example: • A value of 0.0 means that the physical thickness and offset of the surface body nodes will be ignored; all target nodes are mapped at default surface body locations. • A value of 1.0 means that the thickness used for a target node will be equal to the physical thickness value specified for that node. The top location of the node will be used during the mapping process. • A value of -2.0 means that the thickness used for a target node will be equal to twice the physical thickness value specified for that node. The bottom location of the node will used during the mapping process. The Viewer will look similar to the following for a value of –1.0: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 155 Approach 5. 6. 156 Select appropriate options in the Details view. You can modify the mapper settings to achieve the desired mapping accuracy. • For pressure loads, you can apply the load in the direction normal to the face or by specifying a direction. Setting Define By to Components enables you to define the direction by specifying the x, y, and z magnitude components of the load. The z component is not applicable for 2-D analyses. • In a 3D analysis, if the Triangulation mapping algorithm is used, the Transfer Type mapping option defaults to Surface when an Imported Temperature or Imported Body Temperature load scoping is only on shell bodies. If the scoping is on shell bodies and other geometry types, the Transfer Type mapping option will default to Volumetric. In such cases, to obtain a more accurate mapping, you should create a separate imported load for geometry selections on shell bodies, and use the Surface option for Transfer Type. Under Data View, select the desired data Identifier, for the imported load. The data identifier (File Identifier: Data Identifier) strings are specified in the upstream External Data system. You can also change the Analysis Time and specify Scale and Offset values for the imported loads. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics • For pressure loads, if the Define By property is set to Components you should select data identifiers that represent the x, y, and z magnitude components of the load. The z component is not applicable for 2-D analyses. • For convection loads, you should select data identifiers for film coefficient and ambient temperature. You can also specify Scale and Offset values for both film coefficient and ambient temperature. 7. Right-click in the Data View and select Add row to specify additional data for a different analysis time. 8. In the project tree, right-click the Imported Load, and then click Import Load to import the load. When the load has been imported successfully, a contour plot will be displayed in the Geometry window. 9. For convection loads, contours plots of film coefficient or ambient temperature can be viewed by changing the Data option in the details pane. 10. If multiple rows are defined in the Data View, imported values at different time steps can be displayed by changing the Active Row option in the details pane. 11. Change any of the columns in the Data View tab as needed: • Magnitude \ Film Coefficient \ Ambient Temperature Select the appropriate data identifier that represents the load values to be applied from the drop down list. • X Component Select the appropriate data identifier that represents the x component of the load values to be applied from the drop down list. • Y Component Select the appropriate data identifier that represents the y component of the load values to be applied from the drop down list. • Z Component Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 157 Approach Select the appropriate data identifier that represents the z component of the load values to be applied from the drop down list. Not applicable for 2-D analyses. Note If multiple files have been used in the upstream External Data system, the data identifiers for component-based loads must come from the same file. For example, you can select File1:PressureX, File1:PressureY, and File1:PressureZ, but you cannot select File1:PressureX, File2:PressureY, File3.PressureZ. • Analysis Time Choose the analysis time at which the load will be applied. For the ANSYS solver, this must coincide with the end time of a step defined in the Analysis Settings object in the tree. • Scale The amount by which the imported load values are scaled before applying them. • Offset An offset that is added to the imported load values before applying them. 12. To activate or deactivate the load at a step, highlight the specific step in the Graph or Tabular Data window, and choose Activate/Deactivate at this step! See Activation/Deactivation of Loads for additional rules when multiple load objects of the same type exist on common geometry selections. POLYFLOW to Mechanical Data Transfer This feature enables you to import data from a POLYFLOW system and apply it in a Mechanical application analysis. Temperature data can be imported into a static structural, transient structural3 steady state thermal, transient thermal or thermal-electric analysis. To import data from a POLYFLOW system: • In the Project Schematic, right-click the Solution cell of the POLYFLOW system and select Transfer Data to New><mechanical system>, a link is created to the Model cell of the selected Mechanical system. If you select Transfer Data to New > <mechanical system>, this operation automatically creates a link to the Model cell of the Mechanical system. Alternatively, you can drag the Solution cell of the POLYFLOW system and drop it onto the Model cell of a Mechanical system to create the link. • To transfer temperature data to Mechanical, drag the Solution cell of the POLYFLOW system and drop it onto the Setup cell of an applicable Mechanical system. • To transfer thickness data to Mechanical, drag the Solution cell of the POLYFLOW system and drop it onto the Model cell of an applicable Mechanical system. If your simulation has thickness defined from a POLYFLOW system, an Imported Thickness folder is added under the Geometry folder. 1. 3 Select appropriate geometry in the Details view, and then click Apply. The rigid dynamics solver is not supported. 158 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics 2. Select appropriate options in the Details view. You can modify the mapping settings to achieve the desired mapping accuracy. 3. You can specify a thickness value for the unmapped target nodes using the Unmapped Data Value property. By default, a zero thickness value is assigned to the unmapped nodes. Important For the ANSYS solver, the thickness value at each node must be greater than zero. 4. Right-click the Imported Thickness object, and then click Import Thickness to import the thickness. When the thickness has been imported successfully, a contour plot will be displayed in the Geometry window and any mesh display will be based upon the mapped thickness of the elements. If your simulation has temperature data defined from a POLYFLOW system, an Imported Load folder is added under the Environment folder. 1. To add an imported temperature load, click the Imported Load folder to make the Environment toolbar available, or right-click the Imported Load folder and select the appropriate load from the context menu. 2. Select appropriate geometry in the Details view, and then click Apply. 3. In a 3D structural analysis, if the Imported Body Temperature load is scoped to one or more surface bodies, the Shell Face option in the details view enables you to apply the temperatures to Both faces, to the Top face(s) only, or to the Bottom face(s) only. See Imported Body Temperature for additional information. 4. Select appropriate options in the Details view. You can modify the mapper settings to achieve the desired mapping accuracy. • In a 3D analysis, if the Triangulation mapping algorithm is used, the Transfer Type mapping option defaults to Surface when an Imported Temperature or Imported Body Temperature load scoping is only on shell bodies. If the scoping is on shell bodies and other geometry types, the Transfer Type mapping option will default to Volumetric. In such cases, to obtain a more accurate mapping, you should create a separate imported load for geometry selections on shell bodies, and use the Surface option for Transfer Type. 5. Under Data View, select the desired data Identifier, for the imported load. The data identifier (File Identifier: Data Identifier) strings are specified by the upstream POLYFLOW system. You can also change the Analysis Time and specify Scale and Offset values for the imported loads. 6. Right-click in the Data View and select Add row to specify additional data for a different analysis time. 7. In the project tree, right-click the Imported Load object, and then click Import Load to import the load. When the load has been imported successfully, a contour plot will be displayed in the Geometry window. 8. If multiple rows are defined in the Data View, imported values at different time steps can be displayed by changing the Active Row option in the details pane. 9. Change any of the columns in the Data View tab as needed: • Magnitude Select the appropriate data identifier that represents the load values to be applied from the drop down list. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 159 Approach • Analysis Time Choose the analysis time at which the load will be applied. For the ANSYS solver, this must coincide with the end time of a step defined in the Analysis Settings object in the tree. • Scale The amount by which the imported load values are scaled before applying them. • Offset An offset that is added to the imported load values before applying them. 10. To activate or deactivate the load at a step, highlight the specific step in the Graph or Tabular Data window, and choose Activate/Deactivate at this step! See Activation/Deactivation of Loads for additional rules when multiple load objects of the same type exist on common geometry selections. Simplorer/Rigid Dynamics Co-Simulation This feature is a co-simulation link (transient-transient) between Simplorer and the ANSYS Rigid Dynamics solver. This link enables you to combine detailed rigid mechanics models with system models such as complex electronic semiconductor device models used in controls. You can export a rigid dynamics sub-circuit and perform an analysis of the structure in Simplorer. • Simplorer and rigid dynamics models are connected by Simplorer Pins (p. 161). • Simulation is driven by Simplorer. • Results can be reviewed in Simplorer, and then imported back to ANSYS Mechanical. Preparing the Analysis Create a Rigid Dynamics Analysis System Basic general information about this topic Define Engineering Data Basic general information about this topic ... for this analysis type: Density is the only material property utilized in a rigid dynamics analysis. Models that use zero or nearly zero density fail to solve using the ANSYS Rigid Dynamics solver. Attach Geometry Basic general information about this topic ... for this analysis type: Only sheet and solid bodies are supported by the ANSYS Rigid Dynamics solver. Plane bodies and line bodies cannot be used. Define Part Behavior 160 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics Basic general information about this topic ... for this analysis type: You can define a Point Mass for this analysis type. Part stiffness behavior is not required for the ANSYS Rigid Dynamics solver in ANSYS Workbench. Define Joints and Springs Basic general information about this topic ... for this analysis type: Applicable connections for this type of analysis are joints or springs. When an assembly is imported from a CAD system, joints and constraints are not imported; however, joints can be created automatically or manually after the model has been imported. Each joint is defined by its coordinate system of reference. The orientation of this coordinate system is essential, as free and fixed degrees of freedom are defined in this coordinate system. Contact is not supported for this analysis type. Define Input and Output Pins Basic general information about this topic ... for this analysis type: The quantities that are driven by Simplorer are defined as input pins. The quantities that are monitored by Simplorer are defined as output pins. Define Analysis Settings Basic general information about this topic ... for this analysis type: Some of the analysis settings might be overwritten by those defined in Simplorer, because Simplorer drives the co-simulation. Simplorer Pins Simplorer Pins are connection points that describe the interface between a rigid dynamics model and a Simplorer model. Pins have two distinct natures: • Input Pins are used by Simplorer to drive the rigid dynamics model. • Output Pins are sensors used by Simplorer to monitor the rigid dynamics model state. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 161 Approach Pins are defined by the degrees of freedom of joints. One pin can be attached to each degree of freedom of a joint. The type of joint quantity attached to pin depends on the nature of the degrees of freedom. Translational degrees of freedom can have Displacement, Velocity, Acceleration, and Force pins. Rotational degrees of freedom can have Rotation, Angular Velocity, Angular Acceleration, and Moment pins. Note It is not recommended that you place additional joint conditions on degrees of freedom that are associated with pins. To create pins for a Rigid Dynamics analysis system: 1. Open a Rigid Dynamics analysis system in Workbench, then double-click on the Model field to open the model for editing in the Mechanical application. 2. In the Mechanical application tool bar, click the New Simplorer Pin button as shown below to add a new pin. If you click the New Simplorer Pin button while a joint is selected, the pin will automatically have joint information associated with it. If no joint is selected, you will need to associate the pin with a joint at a later time. 3. With the new pin selected in the Outline view, edit the DOF, Type, and Pin Nature fields in the Details view to complete the pin setup. 162 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics 4. Rename the pin as it should appear in Simplorer. 5. Repeat steps 2, 3, and 4 to add all pins of interest. 6. When finished adding pins, refer to Set up the Mechanical Application for Export to Simplorer (p. 153) for more information. System Coupling You can perform a one-way or two-way fluid-structure interaction (FSI) analysis by connecting a System Coupling component system to Mechanical and FLUENT systems. The Mechanical (Static Structural or Transient Structural) and FLUENT systems are dragged onto the Project Schematic from the Analysis Systems toolbox and the System Coupling component system is dragged onto the Project Schematic from the Component System toolbox. The participating systems are connected to the System Coupling component system (via the Setup cells). Once a System Coupling component system is connected to the participating systems, the System Coupling component system requests information from each. The information exchange includes system information (system type, units, file names, etc.), the number of coupling interface regions, and the number and type of variables involved in the coupling. Once connected and set up, the System Coupling component system controls the solver execution for the Mechanical and FLUENT systems and manages the coupled-field analysis. Additional information can be found in the following sections: Supported Capabilities and Limitations System Coupling Related Settings in Mechanical Restarting Mechanical Analyses as Part of System Coupling Running Mechanical as a System Coupling Participant from the Command Line Troubleshooting Two-Way Coupling Analysis Problems Supported Capabilities and Limitations Mechanical supports the following capabilities when used in a System Coupling analysis: • Two-way data exchange across the fluid-solid interface. The fluid-solid interface defines the interface between the fluid in the FLUENT system and the solid in the Mechanical system. This interface is defined on regions in the Mechanical model. • Distributed parallel mode. Note that in order to run Mechanical in distributed parallel mode from within Workbench interface, the working directory must be a shared network directory with the same path for all computer servers. Alternatively, the analysis can run in different working directories on all servers if Mechanical is run as a System Coupling Participant from the command line. For more information, see Running Mechanical as a System Coupling Participant from the Command Line (p. 165). • SOLID and SHELL elements. For a complete list of elements, see Load Transfer Coupled Analysis Workbench: System Coupling in the Coupled-Field Analysis Guide. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 163 Approach Note Force can be received and displacements can be sent to/from regions upon which the Fluid Solid Interface condition is applied. Note If Mechanical is set to run in the Remote Solver Manager (RSM), the user will get the following message: The solve process setting will use RSM. Coupled updates are only supported via RSM when the compute server is localhost. Coupled updates may fail if the compute server is a remote machine. System Coupling Related Settings in Mechanical For transient analyses, the participating systems respect the System Coupling application end time setting. The maximum allowable end time is the minimum of the end times specified by the participants. For static analyses, if you use more than one coupling step, the loads are ramp-applied over the duration. For example, coupling step 1 applies 1/N of the received load, coupling step 2 applied 2/N of the updated load, etc. The full load is applied at the last coupling step. Note To apply the full value of the load for each coupling step, use a Solution Command Object with "KBC,1". For more information on using the Mechanical application for FSI analyses, see Fluid-Structure Interaction (FSI) (p. 142). Refer to the System Coupling User's Guide for a complete description of how to perform FSI analyses using a System Coupling component system. Restarting Mechanical Analyses as Part of System Coupling Mechanical writes out restart points that contain information related to the simulation that can be used to restart the analysis. These files are subsequently used when Mechanical is restarted during system coupling simulations. Generating Restart Files Restarts of a system coupling analysis requires compatible restart points to exist in the coupling service and in each of the solvers participating in the analysis. In order to generate the restart files in Mechanical, you need to ensure that Analysis Settings > Restart Controls > Retain Files After Full Solve setting is set to Yes. Executing the Restart Run Once the coupled analysis run is finished or interrupted, the user can restart this run from any of the saved restart points. 164 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Special Analysis Topics Note The restart point selected in the Mechanical solver must be consistent with the restart points selected for the System Coupling service and other coupling participants. To specify a current restart point, follow these steps: 1. Double-click the Mechanical’s Solution cell in Workbench. 2. In the Outline view tree, select Analysis Settings. 3. In the Details view, under Restart Analysis, set Restart Type to Manual and select the desired restart point from the drop-down menu of Current Restart Point. 4. Close the Mechanical application. 5. Update the Setup cell of the Mechanical application in Workbench. Sometimes, setup changes are required to avoid failure of the coupled analysis. To modify the settings in the Mechanical application, make sure the correct restart point is selected (see above). Once this is done, you can modify any of the settings, save the project and close the Mechanical application. Any of the setup changes will be applied for the subsequent coupled analyses. Running Mechanical as a System Coupling Participant from the Command Line System Coupling analyses can be run via the command line (described in Executing System Couplings Using the Command Line in the System Coupling User's Guide). To run Mechanical as a coupling participant, execute the following steps: • Complete the System Coupling–related settings in Mechanical (see System Coupling Related Settings in Mechanical (p. 164)) • Write the Mechanical APDL application input file: • • – Highlight the Solution object folder in the tree – From the Main Menu, choose Tools>Write Input File... – In the Save As dialog box, specify a location and name for the input file Start the coupling service and obtain the following information from the System Coupling Server (SCS) file: – the port and host on which the service is being run, and – the identifier (or name) for Mechanical Use this SCS information to set the Mechanical–specific system coupling command line options (described in Starting an ANSYS Session from the Command Level in the Operations Guide). Troubleshooting Two-Way Coupling Analysis Problems The following files, found in the Mechanical run directory (SYS/MECH under a Workbench design point directory), may prove useful in troubleshooting coupled analysis problems: • file.err: This file contains a summary of all of the errors that occurred during the run. • solve.out (or other output file): This file contains a complete summary of the current/latest run's evolution. This is one of the most useful files to determine why the coupled analysis failed. To generate extensive debug output during the analysis, enter the following command as a command snippet in the analysis branch when completing the Mechanical problem setup: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 165 Approach /debug,-1,,,,,2 Please provide all of these files when submitting a request for service to ANSYS personnel. Tutorials This section includes step-by-step tutorials that represent some of the basic analyses you can perform in the Mechanical Application. The tutorials are designed to be self-paced and each have associated geometry input files. You will need to download all of these input files before starting any of the tutorials. You can download the files from the ANSYS Download Center, which is accessible from the ANSYS Customer Portal. You will need to navigate through the Download Wizard and select the ANSYS Structural Mechanics Tutorial Input Files download, which is listed in the ANSYS Documentation and Examples section. The input files for these tutorials are included under Mechanical. The following tutorials are included within this section: Steady-State and Transient Thermal Analysis of a Circuit Board Cyclic Symmetry Analysis of a Rotor - Brake Assembly Using Finite Element Access to Resolve Overconstraint Actuator Mechanism using Rigid Body Dynamics Steady-State and Transient Thermal Analysis of a Circuit Board Problem Description The circuit board shown below includes three chips that produce heat during normal operation. One chip stays energized as long as power is applied to the board, and two others energize and de-energize periodically at different times and for different durations. A steady-state thermal analysis and transient thermal analysis are used to study the resulting temperatures caused by the heat developed in these chips. Features Illustrated • Linked analyses • Attaching geometry • Model manipulation • Mesh method and sizing controls 166 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials • Constant and time-varying loads • Solving • Time-history results • Result probes • Charts Procedure 1. Create analysis system. You need to establish a transient thermal analysis that is linked to a steady-state thermal analysis. 2. a. Start ANSYS Workbench. b. From the Toolbox, drag a Steady-State Thermal system onto the Project Schematic. c. From the Toolbox, drag a Transient Thermal system onto the Steady-State Thermal system such that cells 2, 3, 4, and 6 are highlighted in red. d. Release the mouse button to define the linked analysis system. Attach geometry. a. In the Steady-State Thermal schematic, right-click the Geometry cell, and then choose Import Geometry. b. Browse to open the file BoardWithChips.x_t. This file is included in the tutorial input file download. See the introductory Tutorials (p. 166) section for downloading instructions if needed. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 167 Approach 3. Continue preparing the analysis in the Mechanical Application. a. In the Steady-State Thermal schematic, right-click the Model cell, and then choose Edit.... The Mechanical Application opens and displays the model. b. For convenience , use the Rotate toolbar button to manipulate the model so it displays as shown below. Note You can perform the same model manipulations by holding down the mouse wheel or middle button while dragging the mouse. c. 4. From the main menu, choose Units> Metric (m, kg, N, s, V, A) . Set mesh controls and generate mesh. Setting a specific mesh method control and mesh sizing controls will ensure a good quality mesh. Mesh Method: a. Right-click Mesh in the tree and choose Insert> Method. b. Select all bodies by choosing Edit> Select All from the toolbar, then clicking the Apply button in the Details view. c. In the Details view, set Method to Hex Dominant, and Free Face Mesh Type to All Quad. Mesh Body Sizing – Board Components: a. Right-click Mesh in the tree and choose Insert> Sizing. b. Select all bodies except the board by first enabling the Body selection toolbar button, then holding the Ctrl keyboard button and clicking on the 15 individual bodies. Click the Apply button in the Details view when you are done selecting the bodies. c. Change Element Size from Default to 0.0009 m. Mesh Body Sizing – Board: 168 a. Right-click Mesh in the tree and choose Insert> Sizing. b. Select the board only and change Element Size from Default to 0.002 m. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials Generate Mesh: • 5. Right-click Mesh in the tree and choose Generate Mesh. Apply internal heat generation load to chip. The chip on the board that is constantly energized represents an internal heat generation load of 5e7 W/m3. a. Select the chip shown below by first enabling the Body selection toolbar button, then clicking on the chip. b. Right-click Steady-State Thermal in the tree and choose Insert> Internal Heat Generation. c. Type 5e7 in the Magnitude field and press Enter. General items to note: • The applied loads are shown using color coded labels in the graphics. • Time is used even in a steady-state thermal analysis. • The default end time of the analysis is 1 second. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 169 Approach 6. • In a steady-state thermal analysis, the loads are ramped from zero. You can edit the table of load vs. time to modify the load behavior. • You can also type in expressions that are functions of time for loads. Apply a convection load to the entire circuit board. The entire circuit board is subjected to a convection load representing Stagnant Air - Simplified Case. a. Select all bodies by choosing Edit> Select All. b. Choose Convection from the toolbar. c. Import temperature dependent convection coefficient and choose Stagnant Air - Simplified Case. Note that the Ambient Temperature defaults to 22oC. 7. i. Click the flyout menu in the Film Coefficient field and choose Import... (adjacent to the thermometer icon). ii. Click the radio button for Stagnant Air - Simplified Case, then click OK. Prepare for a temperature result. The resulting temperature of the entire model will be reviewed. • 8. Solve the steady-state thermal analysis. • 9. Right-click Solution in the tree under Steady-State Thermal and choose Insert> Thermal> Temperature. Choose Solve from the toolbar. Review the temperature result. • Highlight Temperature in the tree. You have completed the steady-state thermal analysis, which is the first part of the overall objective for this tutorial. You will perform the transient thermal analysis in the remaining steps. Items to note in preparation for the transient thermal analysis: • 170 If you highlight Initial Temperature under Transient Thermal in the tree, you will notice in the Details view, the read only displays of Initial Temperature and Initial Temperature Environment. In general, the initial temperature can be: – Uniform Temperature - where you specify a temperature for all bodies in the structure at time = 0, or – Non-Uniform Temperature - (as in this example) where you import the temperature specification at time = 0 from a steady-state analysis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials • The initial temperature environment is from the steady-state thermal analysis that you just performed. By default the last set of results from the steady-state analysis will be used as the initial condition. You can specify a different set (different time point) if multiple result sets are available. 10. Specify a time duration for the transient analysis. A time duration of the transient study will be 200 seconds. • Under Transient Thermal, highlight the Analysis Settings object and enter 200 in either the Step End Time field in the Details view or in the End Time column in the Tabular Data window. Also note and accept the default initial, maximum, and minimum time step controls for this analysis. 11. Apply internal heat generation to simulate on/off switching on first chip. A chip on the board is energized between 20 and 40 seconds and represents an internal heat generation load of 5e7 W/m3 during this period. a. Select the chip shown below by first enabling the Body selection toolbar button, then clicking on the chip. b. Right-click Transient Thermal in the tree and choose Insert> Internal Heat Generation. c. Enter the following data in the Tabular Data window: • Time = 0; Internal Heat Generation = 0 Note Enter each of the following sets of data in the row beneath the end time of 200 s. • Time = 20; Internal Heat Generation = 0 • Time = 20.1; Internal Heat Generation = 5e7 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 171 Approach • Time = 40; Internal Heat Generation = 5e7 • Time = 40.1; Internal Heat Generation = 0 The Graph window reflects the data that you entered. General items to note: • Loads can be specified as one of three types: – Constant – remains constant throughout the time history of the transient. – Tabular (Time) – (as in this example) define a table of load vs. time. – Function – enter a function such as “=10*sin(time)” to define a variation of load with respect to time. The function definition requires you to start with a ‘=‘ as the first character. 12. Apply internal heat generation to simulate on/off switching on second chip. Another chip on the board is energized between 60 and 70 seconds and represents an internal heat generation load of 1e8 W/m3 during this period. a. Select the chip shown below by first enabling the Body selection toolbar button, then clicking on the chip. b. Right-click Transient Thermal in the tree and choose Insert> Internal Heat Generation. c. Enter the following data in the Tabular Data window: • Time = 0; Internal Heat Generation = 0 Note Enter each of the following sets of data in the row beneath the end time of 200 s. 172 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials • Time = 60; Internal Heat Generation = 0 • Time = 60.1; Internal Heat Generation = 1e8 • Time = 70; Internal Heat Generation = 1e8 • Time = 70.1; Internal Heat Generation = 0 The Graph window reflects the data that you entered. 13. Prepare for a temperature result. The resulting temperature of the entire model will be reviewed. • Right-click Solution in the tree under Transient Thermal and choose Insert> Thermal> Temperature. 14. Solve the transient thermal analysis. • Click the right mouse button again on Solution and choose Solve. The solution is complete when green checks are displayed next to all of the objects. You can ignore the Warning message and click the Graph tab. 15. Review the time history of the temperature result for the entire model. • Highlight the Temperature object. The time history of the temperature result for the entire model is evaluated and displayed. – The Tabular Data window shows the min/max values of temperature at a time point. – By moving the mouse, you can move the bar along the Graph as shown, to any time, click the right mouse button and Retrieve this Result to review the results at a particular time. – You can also animate the solution. 16. Review the time history of the temperature result for each of the chips. Temperature probes are used to obtain temperatures at specific locations on the model. a. Right-click Solution and choose Insert> Probe> Temperature. b. Select the chip to which internal heat generation was applied in the steady state analysis and click the Apply button in the Details view. c. Follow the same procedure to insert two more probes for the two chips with internal heat generations in the transient thermal analysis. d. Right-click Solution or Temperature Probe and choose Evaluate All Results. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 173 Approach 17. Plot probe results on a chart. a. Select the three temperature probes in the tree and select the New Chart and Table button from the toolbar. A Chart object is added to the tree. b. Right-click in the white space outside the chart in the Graph window and choose Show Legend. c. In the Details view, you can change the X Axis variable as well as selectively omit data from being displayed. You have completed the transient thermal analysis and accomplished the second part of the overall objective for this tutorial. End of tutorial. 174 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials Cyclic Symmetry Analysis of a Rotor - Brake Assembly Program Description This tutorial demonstrates the use of cyclic symmetry analysis features in the Mechanical Application to study a sector model consisting of a rotor and brake assembly in frictional contact. With increased loading of the brake, the contact status between the pad and the rotor changes from “near”, to “sliding”, to “sticking”. Each of these contact states affects the natural frequencies and resulting mode shapes of the assembly. Three pre-stress modal analyses are used to verify this phenomenon. Features Demonstrated • Cyclic Regions • Named Selections based on Criteria • Thermal Steady-State Analysis with Cyclic Symmetry • Static Structural Analysis with Cyclic Symmetry • Modal Analysis with Cyclic Symmetry • Generation of Restart Points • Modal Analysis with Nonlinear Prestress (Linear Perturbation) Note The procedural steps in this tutorial assume that you are familiar with basic navigation techniques within the Mechanical application. If you are new to using the application, consider running the tutorial: “Steady-State and Transient Thermal Analysis of a Circuit Board” before attempting to run this tutorial. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 175 Approach Analysis System Layout We will tour the different analysis systems that can leverage cyclic symmetry functionality. These comprise thermal, static structural and modal analyses: • A steady-state thermal analysis will be used to calculate the temperature distribution for the evaluation of any temperature-dependent material properties or thermal expansions in subsequent analyses. • A nonlinear static structural analysis is configured to represent the mechanical loading of the brake onto the rotor. Nonlinearities from large deformation and changes in contact status are included. • Modal analyses, each at different stages of frictional contact status, are established to compare the free vibration responses of the model. 1. Create the analysis systems. You need to establish a static structural analysis that is linked to a steady-state thermal analysis, then establish three modal analyses that are linked to the static structural analysis. 176 a. Start ANSYS Workbench. b. From the Toolbox, drag a Steady-State Thermal system onto the Project Schematic. c. From the Toolbox, drag and drop a Static Structural system onto the Steady-State Thermal system such that cells 2, 3, 4, and 6 are highlighted in red. d. The systems are displayed as follows: e. To measure the free vibration response, go to the Toolbox, drag and drop a Modal system onto the Static Structural system such that cells 2, 3, 4, and 6 are highlighted in red. f. Repeat step e two more times to complete adding the remaining analysis systems. The layout of the analysis systems and interconnections in the Project Schematic should appear as shown below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials 2. Assign materials. Accept Structural Steel (typically the default material) for the model. 3. a. In the Steady-State Thermal schematic, right-click the Engineering Data cell and choose Edit.... The Engineering Data workspace opens and displays Structural Steel as the default material. b. Click the Return to Project toolbar button. Attach geometry. a. In the Steady-State Thermal schematic, right-click the Geometry cell, and then choose Import Geometry. b. Browse to open the file Rotor_Brake.agdb. This file is included in the tutorial input file download. See the introductory Tutorials (p. 166) section for downloading instructions if needed. Define the Cyclic Symmetry Model We now specify the cyclic symmetry for our quarter sector model (N = 4, 90 degrees) and prepare other general aspects of modeling in the Mechanical application. To setup a cyclic symmetry analysis, Mechanical uses a Cyclic Region object. This object requires selection of the sector boundaries, together Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 177 Approach with a cylindrical coordinate system whose Z axis is colinear with the axis of symmetry, and whose Y axis distinguishes the low and high boundaries. 1. 2. 3. 4. 178 Enter the Mechanical Application and set unit systems. a. In the Steady-State Thermal schematic, right-click the Model cell, and then choose Edit.... The Mechanical Application opens and displays the model. b. From the main menu, choose Units> Metric (mm, kg, N, s, mV, mA) . Define the Coordinate System to specify the axis of symmetry. a. Right-click Coordinate Systems in the tree and choose Insert> Coordinate System. b. In the Details view of the newly-created Coordinate System, set Type to Cylindrical and Define By to Global Coordinates. Define the Cyclic Region object. a. Right-click Model in the tree and choose Insert> Symmetry. b. Right-click Symmetry and choose Insert> Cyclic Region. The direction of the Y-axis should be compatible with the selection of low and high boundaries. The low boundary is designated as the one with a lower value of Y or azimuth. c. Select the three faces that have lower azimuth for the low boundary. These faces are highlighted in blue in the figure below. d. Select the three matching faces on the opposite end of the sector for the high boundary. These faces are highlighted in red in the figure below Define Connections. Frictional contact exists between the rotor and brake pad, whereas bonded contact exists between the wall and the rotor. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials a. Expand the Connections folder in the tree, then expand the Contacts folder. Within the Contacts folder, two contact regions were detected automatically and displayed as Contact Region and Contact Region 2. b. Right-click the Contacts folder and choose Renamed Based on Definition. The contact region names automatically change to Bonded - Pad to Rotor and Bonded - Blade to Wall respectively. c. Highlight Bonded - Pad to Rotor and in the Details view, set Type to Frictional. Note that the name of the object changes accordingly. d. In the Friction Coefficient field, type 0.2 and press Enter. Note For higher values of contact friction coefficient a damped modal analysis would be needed. At a level of 0.2 damping effects are being neglected. Generate the Mesh In the following section we’ll use mesh controls to obtain a mesh of regular hexahedral elements. The Cyclic Region object will guarantee that matching meshes are generated on the low and high boundaries of the cyclic sector. Taking advantage of the shape and dimensions of the model, Named Selections will be used to choose the edge selections for each mesh control. Mesh control: Element Size on Pad-Wall-Rotor: 1. Create a Named Selection for this Mesh Control. a. Right-click on Model and choose Insert> Named Selection. b. Highlight the Selection object, and set Scoping Method to Worksheet. c. Program the Worksheet, as shown below, to select the edges at 90 degrees of azimuth in the cylindrical coordinate system, keeping those in the z-axis range [1mm, 6 mm] (to remove the thickness of the wall). To add rows to the Worksheet, right-click in the table and select the option from the flyout menus. d. Click the Generate button. You should see 11 edges. e. Rename the object to Edges for Wall Rotor Pad Sector Boundary. The selection should display as follows:. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 179 Approach Note It may be useful to undock the Worksheet window and tile it with the Geometry view as shown above. 2. Insert a Mesh Sizing control. a. Right-click on Mesh and choose Insert> Sizing. b. Set Scoping Method to Named Selection. c. Choose the named selection defined in the previous step. d. Set its Element Size to 0.5 mm. e. Set Behavior to Soft. Mesh control: Number of Divisions on Pad-Rotor: 1. Create a Named Selection to pick the circular edges in the orifice of the pad and rotor. This Named Selection will pick the circular edges in the orifice of the pad and rotor, which is within a radius of 5 mm. 180 a. Right-click on Model and choose Insert> Named Selection. b. Highlight the Selection object, and set Scoping Method to Worksheet. c. Rename the object to Edges for Rotor Pad Orifice. d. Program the Worksheet, as shown below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials e. 2. Click the Generate button. You should see 4 edges. Insert a Mesh Sizing Control as before to select this Named Selection. a. Right-click on Mesh and choose Insert> Sizing. b. Set Scoping Method to Named Selection. c. Choose the named selection defined in the previous step. d. Set its Type to Number of Divisions and specify 9. e. Set Behavior to Hard. Mesh control: Element Size on Wall-Blade 1. 2. Create a Named Selection object to pick the thicknesses of the Wall and Blade. a. Right-click on Model and choose Insert> Named Selection. b. Highlight the Selection object, and set Scoping Method to Worksheet. c. Rename the object to Edges for Wall Blade Thicknesses. d. Program the Worksheet as shown below. e. Click the Generate button. You should see 16 edges. Insert a Mesh Sizing Control as before to select this Named Selection. a. Right-click on Mesh and choose Insert> Sizing. b. Set Scoping Method to Named Selection. c. Choose the named selection defined in the previous step. d. Set its Element Size to 1 mm. e. Set Behavior to Hard. Mesh Control: Number of Divisions on Blade - Longer Edges 1. Create a Named Selection object to pick the longer edges of the Blade. a. Right-click on Model and choose Insert> Named Selection. b. Highlight the Selection object, and set Scoping Method to Worksheet. c. Rename the object to Edges for Blade. d. Program the Worksheet as shown below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 181 Approach e. 2. Click the Generate button. You should see 2 edges. Insert a Mesh Sizing Control as before to select this Named Selection. a. Right-click on Mesh and choose Insert> Sizing. b. Set Scoping Method to Named Selection. c. Choose the named selection defined in the previous step. d. Set its Type to Number of Divisions and specify 14. e. Set Behavior to Hard. Mesh Control: Number of Divisions on Blade - Shorter Edges 1. 2. Create a Named Selection object to pick the shorter edges of the Blade. a. Right-click on Model and choose Insert> Named Selection. b. Highlight the Selection object, and set Scoping Method to Worksheet. c. Rename the object to Edges for Blade 2. d. Program the Worksheet as shown below. e. Click the Generate button. You should see 2 edges. Insert a Mesh Sizing Control as before to select this Named Selection. a. Right-click on Mesh and choose Insert> Sizing. b. Set Scoping Method to Named Selection. c. Choose the named selection defined in the previous step. d. Set its Type to Number of Divisions and specify 1. e. Set Behavior to Hard. Mesh Control: Method on Pad-Rotor-Wall-Blade 1. Insert a Sweep Method control. a. Right-click Mesh in the tree and choose Insert> Method. b. Select all the bodies by choosing Edit> Select All from the toolbar, then click the Apply button. c. In the Details view, set Method to Sweep. d. Set Free Face Mesh Type to All Quad. Generate the Mesh 182 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials • For convenience, select all 6 mesh controls defined, right-click and choose Rename Based on Definition. • Right-click Mesh in the tree and choose Generate Mesh. The mesh should appear as shown below: Steady-State Thermal Analysis We now proceed to define the boundary conditions for a thermal analysis featuring cyclic symmetry. Thermal boundary conditions are prescribed throughout the model while steering clear of the faces comprising the sector boundaries since temperature constraints are already implied there. 1. 2. Define a convection interface. a. Right-click Steady-State Thermal in the tree and choose Insert> Convection. b. Select the outer faces of the Wall and the Blade as shown in the figure (8 faces). c. Specify a Film Coefficient of air by right-clicking on the property and choosing Import... upon which you choose Stagnant Air - Simplified Case . Insulate the upper and lower faces of the Wall. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 183 Approach • 3. 4. Select the upper and lower faces of the Wall, then right-click and choose Insert> Perfectly Insulated. Apply a temperature load to the Pad and Rotor. a. Select the remaining faces on the assembly on the Pad and the Rotor, then right-click and choose Insert> Temperature. Exclude any faces on the sector boundaries or in the frictional contact. b. Type 100°C as the Magnitude and press Enter. Solve and review the temperature distribution. a. Right-click Solution under Steady-State Thermal and choose Insert> Thermal> Temperature. b. Solve the steady-state thermal analysis. c. Review the temperature result by highlighting the Temperature result object. Note Although insignificant in this model, temperature variations and their effect on the structural material properties are generally important to the formulation of physically accurate models. Static Structural Analysis In this analysis, the brake is loaded onto the rotor in a single load step. The contact status is monitored at various stages of loading and three points are selected as pre-stress conditions for subsequent 184 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials modal analyses. Because both contact and geometric nonlinearities are present, each pre-stress condition will present a different effective stiffness matrix to its corresponding modal analysis. The solver uses restart points, generated in the static analysis, to record the snapshot of the nonlinear tangent stiffness matrices and transfers them into the subsequent linear systems. This technique is referred to as Linear Perturbation. 1. 2. Apply the pressure and boundary conditions to engage the brake pad into the rotor. a. Select the bottom face of the Pad as shown below. Right-click the Static Structural object in the tree and choose Insert> Pressure. b. In the Details view, click the Magnitude flyout menu, choose Function, and specify: =time*time*4000, then press Enter. This represents a quadratic function reaching 4000 MPa by the end of the load step. c. Set up the frictionless supports on the faces of Blade, Wall and Pad as shown below. Configure the Analysis Settings. a. Set Auto Time Stepping to On. b. Set Define By to Substeps. c. Set Initial Substeps to 30. d. Set Minimum Substeps to 10. e. Set Maximum Substeps to 30. f. Set Large Deflection to On to activate geometric nonlinearities. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 185 Approach g. 3. To ensure that Restart Points are generated, under Restart Controls, set Generate Restart Points to Manual, and request to retain All Files for load steps and substeps. Maximum Points to Save should also be set to All. Proceed to solve the model using the standard procedure. Reviewing the contact status changes during the course of the load application The contact status will change with increasing loads from Near, to Sliding, to Sticking. A status change from Near to Sliding reflects the engagement of contact impenetrability conditions (normal direction). A change from Sliding to Sticking, reflects additional engagement of contact friction conditions (tangential direction). This progression will generally reflect an increased effective stiffness in the tangent stiffness matrix, which can be illustrated by a Force-deflection curve: To review the contact status, insert a Contact Tool in the Solution folder. To display only the contact results at the frictional contact, unselect Bonded - Wall To Blade in the Contact Tool Worksheet. Insert three different Contact Status results with display times at 0.03, 0.5 and 0.8 seconds, which should reveal the progression in contact status as shown below (from left to right): The legend for these contact status plots is as follows: • Yellow - Near • Light Orange - Sliding 186 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials • Dark Orange - Sticking Modal Analysis There are three modal analyses to study the effect of contact status and stress stiffening on the free vibration response of the structure. Each of these will be based on a different restart point in the static structural analysis. To see all available restart points, you can inspect the timeline graph displayed when the Analysis Settings object of the Static Structural analysis is selected after solving. Restart points are denoted as blue triangle marks atop the graph: To select the restart point of interest, go to the Pre-Stress (Static Structural) object under each Modal Analysis. Make sure Pre-Stress Define By is set to Time and specify the time. The object will acknowledge the restart point in the Reported Loadstep, Reported Substep and Reported Time fields. Configure the Modal analyses as follows: • In Modal 1 set Pre-Stress Time to 0.033 seconds. • In Modal 2 set Pre-Stress Time to 0.5 seconds. • In Modal 3 set Pre-Stress Time to 0.8 seconds. Because the boundary conditions (that is, the frictionless supports) are automatically imported from the static analysis, we can proceed directly to solve. Solving and Reviewing Modal Results We'll monitor the lowest frequencies of vibration which belong to Harmonic Indices 0 (symmetric) and 2 (anti-symmetric). 1. Right-click on the Solution folder of each Modal analysis and choose Solve. 2. When the solutions complete, go to the Tabular Data window of each modal analysis. You can inspect the listing of modes and their frequencies. Because our structure has a symmetry of N=4, there will be three solutions, namely for Harmonic Indices 0, 1 and 2. 3. In the Tabular Data window of each modal analysis, select the two rows for Harmonic Index 0 - Mode 1 and Harmonic Index 2 - Mode 1. Right-click and choose Create Mode Shape Results. The image below shows this view for the first Modal analysis: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 187 Approach An interesting alternative to this view is to see the sorted frequency spectrum. You may review this by setting the X-Axis to Frequency on any of the Total Deformation results in each modal analysis: At this point, each modal analysis should have two results for Total Deformation to inspect the first Mode of Harmonic Indices 0 and 2. Recall the meaning of Harmonic Index solutions and how they apply to the model. Harmonic Index 0 represents the constant offset in the discrete Fourier Series representation of the model and corresponds to equal values of every transformed quantity, for example, displacements in X, Y and Z directions, in consecutive sectors. Thus deformations that are axially positive in one sector will have the same axially positive value in the next. The following picture compiles, from left to right, the mode shapes for the Near, Sliding and Sticking status at Harmonic Index 0: Notice how increased engagement of the frictional contact in the assembly has the effect of producing higher frequency vibrations. Also, the mode of vibration goes from being localized at the contact interface when the contact is Near, but is forced to distribute throughout the wall of the rotor as the contact sticks. Note You may need to specify Auto Scale on the Results toolbar so the mode shapes are plotted as shown. 188 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials Harmonic Index 2 solutions correspond to N/2 for our sector (90 degrees or N = 4). This Harmonic Index, sometimes called the asymmetric term in the Fourier Series, represents alternation of quantities in consecutive sectors. A positive axial displacement at a node in one sector becomes negative in the next, a radially outward displacement in one sector will become inward in the next, and so on. The following are the results for the first mode of this Harmonic Index: The lowest mode shows nearly independent vibration of the rotor relative to the blade. On the highest mode, sticking reduces this relative movement. For a continued discussion on post-processing for Cyclic Symmetry and especially on features for postprocessing degenerate Harmonic Indices (those between 0 and N/2), please see Reviewing Results for Cyclic Symmetry in a Modal Analysis in the Mechanical help. End of tutorial. Using Finite Element Access to Resolve Overconstraint Problem Description This tutorial demonstrates the use of Finite Element (FE) types exposed in the Mechanical application by examining an analysis of a bracket assembly with contacts. This tutorial attempts to show the features related to FE types in the context of resolving an over-constraint issue in a Static Structural Analysis. Features Demonstrated • Create Node-based Named Selections – Using Worksheet Criterion – Using Node Selection Tool • Scope FE (node-based) Boundary Conditions • Display FE Connections • Scope Results to FE Nodes Setting Up the Analysis System 1. Create Static Structural Analysis. a. Open ANSYS Workbench. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 189 Approach b. 2. On the Workbench Project page, drag a Static Structural system from the Toolbox to the Project Schematic. The Project Schematic should appear as follows: Assign Materials. For this tutorial we will accept Structural Steel (typically the default material) for the model and add Aluminum Alloy as a material option. 190 a. In the Static Structural schematic, right-click the Engineering Data cell and choose Edit. The Engineering Data workspace opens and displays Structural Steel as the default material. b. Right-click the box below Structural Steel, where it says "Click here to add new material" and select Engineering Data Sources. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials c. Select the General Materials check box and then click the Add button for Aluminum Alloy. A book icon appears in the column next to the Add button (plus symbol) to indicate that the material is selected. d. Click the Return to Project toolbar button to return to the Project Schematic. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 191 Approach 3. Attach Geometry. a. In the Static Structural schematic, right-click the Geometry cell and choose Import Geometry>Browse. b. Browse to the proper location and open the file Bracket_Assembly.agdb. Define the Model 1. Launch Mechanical by right-clicking the Model cell and then choosing Edit. (Tip: You can also doubleclick the cell to launch Mechanical). 2. Define Unit System: from the Main Menu, select Units> Metric (mm, kg, N, s, mV, mA). 3. Define Part Material and Create Named Selection. 192 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials a. For this model, all of the parts have been defined as Structural Steel. However, we want to change the Material type of the Clevis to Aluminum Alloy. To do this, first expand the Geometry object in the tree. b. Select the Clevis object under Geometry. In the Details under the Material category, click the Structural Steel option in the Assignment field to display the drop-down list. Change the material to Aluminum Alloy. c. Right-click on Clevis and select Create Named Selection. Enter the Selection Name "Clevis" and click the OK button. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 193 Approach The Selection Name window is shown below. 4. 194 Define Connections. a. Expand the Connections folder in the tree, and then expand the Contacts folder. b. Right-click the Contacts folder and choose Renamed Based on Definition. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials Renaming is illustrated below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 195 Approach Refine and Generate Mesh To be able to create and modify node-based boundary conditions, you must first generate the model’s mesh. In addition, for this example, we will use the Body Sizing feature to define certain local mesh sizing. 1. Insert Body Sizing. a. 196 Right-click on the Mesh object and select Sizing. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials b. In the Details view, select the Scoping Method option in the Scope field and set it to Named Selection. c. Select the Named Selection field and select Clevis from the drop-down menu. d. In the Element Size field, enter 4 (mm). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 197 Approach e. Right-click the Body Sizing object and select Rename Based on Definition. As illustrated here, the object is renamed. 198 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials 2. Generate Mesh: Right-click on the Mesh object select Generate Mesh. The completed mesh is shown here. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 199 Approach Static Structural Analysis At this time, we will specify the following boundary conditions: • Moment • Displacement • Fixed Support 1. 200 Define Analysis Settings: Select the Analysis Settings object in the tree. In Details view change the Solver Controls>Large Deflection to On. This selection allows the solver to account for large deformation effects such as large deflection, large rotation, and large strain. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials 2. Insert a Moment Load. a. Select the Static Structural object, right-click the mouse, and then choose Insert>Moment. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 201 Approach b. 3. 202 Select the inner face of the Clevis (1 Face) as illustrated here. In the Details for the Scope category, select the Geometry field and click Apply. Enter 1e5 N mm as the Magnitude and change the Behavior to Rigid. Insert a Displacement and Fixed Support. a. With the Moment object still highlighted, right-click the mouse and select Insert>Displacement. b. Select the inner face of the circular hole highlighted here. Make sure that the model is oriented as shown (note the direction of the bolts) and then click the Apply button in the Geometry field. Set the values of X Component, Y Component, and Z Component, to 0 mm. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials c. Finally, let’s immobilize the assembly by specifying Fixed Supports on the faces illustrated below. Under the Supports menu, select Fixed Support, select one of the faces, press and hold the [CTRL] key, and then select the remaining three faces. Once all of the faces are selected, click the Apply button in the Geometry field. Results and Solution This section outlines the steps to add result objects, solve your analysis, and review your results. 1. Specify Result Object and Solve. a. Highlight the Solution object, select the Deformation Menu on the Solution Context Toolbar, and select Total. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 203 Approach b. 2. Right-click the Solution object and select Solve. Review the Results. a. Select the Total Deformation object. The solved model should display as follows: The bulk of the result displays in blue, indicating no deformations on the assembly. This cannot be correct. In addition to that condition, the following Warning Messages display: 204 • Large deformation effects are active which may have invalidated some of your applied supports such as displacement, cylindrical, frictionless, or compression only. Refer to Troubleshooting in the Help System for more details. • One or more MPC contact regions or remote boundary conditions may have conflicts with other applied boundary conditions or other contact regions. Refer to Troubleshooting in the Help System for more details. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials This second message indicates that one of the nodes is likely over-constrained. You can graphically display FE Connections from the Solution Information object, as illustrated below. In the Details, specify the Display control as CE Based and the Display Type as Lines. As you can see there is an abundance of Constraint Equations. Using FE Types to Identify Over-Constraints Now, let’s look at Solver Output to track down the over-constraint issue. 1. Select the Solution Information object. The Worksheet displays. The contents of the Worksheet display output messages, including Warnings. Scroll through the messages, searching for over-constraint messages/warnings. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 205 Approach The warning highlighted here provides a starting point to correct the over-constraint. Node 390 is identified as a node that is over-constrained; specifically that it has multiple constraints on degree of freedom 3. FE access makes it possible to select a single node using the Node ID. That is, Mechanical allows us to create a Named Selection that consists of Node 390 so we can that identify it specifically and view it graphically. 2. 206 Select the Named Selections object and then click the Named Selection button on the toolbar. A Selection object is generated. In the Details for the Selection object, change the Scoping Method to Worksheet. The Worksheet view automatically displays. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 207 Approach 3. Right-click in the first row of the table and select Add Row. 4. Specify the criteria as follows: 208 • Entity Type = Mesh Node • Criterion = Node ID • Operator = Equal • Value = 390 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials 5. Click the Generate button. 6. Right-click on Selection and select Rename. Change the name to "Node 390". A selection is generated that is just the one node, Node 390, that is over-constrained. Select the Graphics tab to view the generated node. 7. With node-based Named Selections, it is possible to view the Constraint Equations (CEs) attached to a single node. Select Solution Information in the tree, select the Graphics tab at the bottom of the window, and then select Node 390 as the option for the control, Draw Connections Attached To. You should see the following illustration. The CEs are displayed as lines (note Display Type in the Details). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 209 Approach The Display Type specified as Points is illustrated below. You can see Node 390 as well as all of the other nodes used to calculate CEs. All nodes other than Node 390 are hollow. This indicates that each node is connected to Node 390. In addition, the Visible on Results control has been set to Yes. This facilitates the display of the contour results for the Total Deformation result and the CEs, also shown below. Here is an illustration of the CEs while the Total Deformation object is selected. 210 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials We have identified the over-constrained node, now, let’s correct the issue. Using FE Type to Correct Over-Constraints A starting point to correct the over-constraint is to remove the Displacement at Node 390. But looking at the scoping of the Moment and Displacement, it is clear that they share the edge nodes on the hole on the side of the face where the Moment is applied. As a result, when the CE's are generated from the Moment load, the solver tries to impose displacements on the edge nodes which may conflict with the Displacement already imposed due to the Displacement constraint. So, it is reasonable to try to remove the Displacement on the edge nodes. While a typical Displacement Boundary Condition does not allow for this option, it can be accomplished with FE Displacement. 1. Create Geometry-based Named Selection. a. Select the Named Selections object and then click the Named Selection button on the toolbar. A Selection object is generated. b. Make sure that the Face selection toolbar option is chosen and then select the hole in the Clevis. In the Details for the Selection object, the Scoping Method should be set to Geometry. In the Geometry field, click the Apply button to specify the hole as the Geometry. c. Right-click on Selection and select Rename. Change the name to "Hole Face". Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 211 Approach 2. 212 Create Criterion-based Named Selection. a. Select the Named Selections object and then click the Named Selection button on the toolbar. A new Selection object is generated. b. Right-click on the new Selection object and select Rename. Change the name to "Hole Face Nodes". c. In the Details for the Selection object, change the Scoping Method to Worksheet. The Worksheet view automatically displays. d. Specify the criteria as illustrated here. e. Take a moment to review and consider the criterion you have defined and then click the Generate button. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials 3. Convert Edge to Nodes and Remove it from the Geometry. Now, let’s use a criterion-based Named Selection to create a Named Selection for the hole that subtracts (removes) the nodes of the hole’s edge. a. Select the Named Selections object and then click the Named Selection button on the toolbar. A Selection object is generated. b. Make sure that the Edge selection option is chosen and then select the edge of the hole. In the Details for the Selection object, the Scoping Method should be set to Geometry. In the Geometry field, click the Apply button to specify the hole as the Geometry. c. Right-click on Selection and select Rename. Change the name to "Hole Edge". d. Select the Named Selections object and then click the Named Selection button on the toolbar. A new Selection object is generated. e. Right-click on the new Selection object and select Rename. Change the name to "Hole Edge Nodes". f. In the Details for the Selection object, change the Scoping Method to Worksheet. The Worksheet view automatically displays. Specify the criteria as illustrated here and then click the Generate button. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 213 Approach One more Named Selection is required. This Named Selection will remove the edge nodes from the hole nodes. g. Select the Named Selections object and then click the Named Selection button on the toolbar. A new Selection object is generated. h. Right-click on the new Selection object and select Rename. Change the name to "Hole Face Minus Edge". i. In the Details for the Selection object, change the Scoping Method to Worksheet. Specify the criteria as illustrated here and then click the Generate button. We now have a node-based Named Selection that includes all of the nodes of the hole, minus the nodes of the inner edge of the hole. 4. Suppress the existing Displacement: select the Displacement object, right-click the mouse, and select Suppress. If desired, you could instead delete the load. 5. Create FE Displacement and Solve. Now let’s define the scope of the FE Displacement and re-solve the analysis. 214 a. Select the Static Structural object, click the Direct FE menu in the toolbar, and then select FE Displacement. b. Node-based boundary conditions can only be scoped to Named Selections. In the Details for the FE Displacement, specify Hole Face Minus Edge as the Named Selection and then specify each Component (X, Y, and Z) as 0. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials c. Click the Solve button. The solution should appear as shown here. The Constraint Equations should appear with a uniform pattern, as illustrated here for the Solution Information object. And once again, the Visible on Results control has been set to Yes so that you can view Constraint Equations and contour results (make sure to select the Graphics tab). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 215 Approach 6. 216 Examine Equivalent Stresses. Now, let’s examine the Equivalent Stresses on the model. a. Highlight the Solution object, right-click, and select Insert>Equivalent Stress. b. Right-click the mouse and select Evaluate Results. The result should appear as illustrated here. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials A zero Displacement was applied and this is reflected in the above result. c. Examine the stresses on the hole using direct node selection. i. Graphically Select Nodes. Select the Mesh object and then open the Select Type (Geometry/Mesh) menu and choose Select Mesh. ii. Open the Select Mode menu and choose Box Select. iii. Drag your cursor over the Clevis hole in a pattern similar to what is illustrated here to directly select the nodes in and around the hole. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 217 Approach iv. 218 Right-click the mouse and select Named Selection. Enter "Stress Nodes" as the Selection Name. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials v. Select the Equivalent Stress object, right click the mouse and choose Clear Generated Data. vi. Right-click the mouse and select Evaluate Results. Results can be scoped to FE-based Named Selections as illustrated here, where the Equivalent Stress result was scoped to the Named Selection Stress Nodes. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 219 Approach End of tutorial. Actuator Mechanism using Rigid Body Dynamics This example problem demonstrates the use of a Rigid Dynamic analysis to show the kinematic behavior of an actuator after moment force is applied to the flywheel. Features Demonstrated • Joints • Joint loads • Springs • Coordinate system definition • Body View • Joint probes Setting Up the Analysis System 1. Create the analysis system. Start by creating a Rigid Dynamics analysis system and importing geometry. 2. 220 a. Start ANSYS Workbench. b. From the Toolbox, drag a Rigid Dynamics system into the Project Schematic. c. Right-click the Geometry cell of the Rigid Dynamics system, and select Import Geometry>Browse.... d. Browse to open the file Actuator.agdb. This file is included in the tutorial input file download. See the introductory Tutorials (p. 166) section for download instructions if needed. A check mark appears next to the Geometry cell in the Project Schematic. Continue preparing the analysis in the Mechanical Application. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials a. In the Rigid Dynamics schematic, right-click the Model cell, and then choose Edit.... The Mechanical Application opens and displays the model. The actuator mechanism model consists of four parts: (from left to right) the drive, link, actuator, and guide. b. From the main menu, choose Units>Metric (mm, kg, N, s, mV, mA). Note Stiffness behavior for all geometries are rigid by default. 3. Remove surface-to-surface contact. The focus of this tutorial is a rigid dynamic analysis. Rigid dynamic models employ joints to describe the relationships between parts in an assembly. As such, we will not need the surface-to-surface contacts that were transferred from the geometry model in this case. a. Expand the Connections branch in the Outline, then expand the Contacts branch. Highlight all of the contact regions in the Contacts branch. b. Right-click the highlighted contact regions, then select Delete. Note that this step is not needed if your Mechanical options configured so that automatic contact detection is not performed upon attachment. 4. Define joints. We will define joints in the model from left to right as shown below, using Body-Ground and Body-Body joints as necessary to solve the model. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 221 Approach Prior to defining joints, it is useful to select the Body Views button in the Connections toolbar. The Body Views button splits the graphics window into three sections: the main window, reference body window, and mobile body window. Each window can be manipulated independently. This makes it easier to select desired regions on the model when scoping joints. To define joints: a. 222 Select the drive pin face and link center hole face as shown below, then select Revolute from the Body-Body drop-down in the Connections toolbar. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials b. Select the drive center hole face as shown below, then select Revolute from the Body-Ground drop-down in the Connections toolbar. c. Select the link and actuator center hole faces as shown below, then select Revolute from the Body-Body drop-down in the Connections toolbar. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 223 Approach 224 d. Select the actuator face and guide face, then select Translational from the Body-Body dropdown in the Connections toolbar, as shown below. e. Select the guide top face, then select Fixed from the Body-Ground drop-down in the Connections toolbar, as shown below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials 5. Define joint coordinate systems. You must properly define the coordinate systems for each new joint to ensure correct joint motion. Realign each joint coordinate system so that they match the corresponding systems pictured in step 4. To specify a joint coordinate system: a. In the Outline, highlight a joint in the Joints branch. b. In the joint Details view, click the Coordinate System field. The coordinate field becomes active. c. Click the axis you want to change (i.e., X, Y, or Z). All 6 directions become visible as shown below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 225 Approach 6. d. Click the desired new axis to realign the joint coordinate system. e. Click Apply in the Details view once the desired alignment is achieved. Define a local coordinate system. Now we will create a local coordinate system that will be used to define a spring that will be added to the actuator. 226 a. Right-click the Coordinate Systems branch in the Outline, then select Insert>Coordinate System. b. Right-click the new coordinate system, then select Rename. Enter Spring_fix as the name. c. In the Spring_fix Details view, define the Origin fields as shown below: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials 7. Add a spring to the actuator. a. Select the bottom face of the Actuator, then select Spring from the Body-Ground drop-down in the Connections toolbar, as shown below. b. In the Reference section of the spring Details view, set the Coordinate System to Spring_fix. c. In the Definition section of the spring Details view, specify: Longitudinal Stiffness = 0.005 N/mm Longitudinal Damping = 0.01 N*s/mm 8. Define analysis settings. To define the length of the analysis: a. Select Analysis Settings in the Overview, then Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 227 Approach b. 9. In the Analysis Settings Details view, specify Step End Time = 60. s Define a joint load. A joint load must be defined to apply a kinematic driving condition to the joint object. To define a joint load: a. Right-click the Transient branch in the Outline, then select Insert>Joint Load. b. In the Joint Load Details view, specify: Joint = Revolute - Ground To Drive Type = Moment Magnitude = Tabular (Time) Graph and Tabular Data windows will appear. c. In the Tabular Data window, specify that Moment = 5000 at Time = 60, as shown below. 10. Prepare the solution a. Select Solution in the Outline, then select Deformation>Total from the Solution toolbar. b. In the Outline, click and drag the link to actuator revolute joint to the Solution branch. Joint Probe will appear under the Solution branch. This is a shortcut for creating a joint probe that is already scoped to the joint in question. Because we want to find the forces acting on this joint, the default settings in the details of the joint probe are used. c. Click the Solve button in the main toolbar. 11. Analyze the results 228 a. After the solution is complete, select Total Deformation under the Solution branch in the Outline. A timeline animation of max/min deformation vs. time appears in the Graph window. b. In the Graph window, select the Distributed animation type button, and specify 100 frames and 4 seconds, as shown below. (These values have been chosen for efficiency purposes, but they can be adjusted to user preference.) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Wizards c. Click the Play button to view the animation. d. Select the Joint Probe branch in the Outline, e. In the Joint Probe Details view, specify X Axis in the Result Selection field. f. Right-click the Joint Probe branch, then select Evaluate All Results. The results from the analysis show that the spring-based actuator is adding energy in to the system which is reducing the cycle time. End of tutorial. Wizards Wizards provide a layer of assistance above the standard user interface. They are made up of tasks or steps that help you interpret and work with simulations. Conceptually, the wizards act as an agent between you and the standard user interface. Wizards include the following features: • An interactive checklist for accomplishing a specific goal • A reality check of the current simulation • A list of a variety of high-level tasks, and guidance in performing the tasks • Links to useful resources • A series of Callout windows which provide guidance for each step Note Callouts close automatically, or you may click inside a Callout to close it. Wizards use hyperlinks (versus command buttons) because they generally represent links to locations within the standard user interface, to content in the help system, or to a location accessible by a standard HTML hyperlink. The status of each step is taken in context of the currently selected Tree Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 229 Approach Outline (p. 235) object. Status is continually refreshed based on the Outline state (not on an internal wizard state). As a result you may: • Freely move about the Tree Outline (p. 235) (including between branches). • Make arbitrary edits without going through the wizards. • Show or hide the wizards at any time. Wizards are docked to the right side of the standard user interface for two reasons: • The Tree Outline (p. 235) sets the context for status determination. That is, the wizards interpret the Outline rather than control it. (The user interface uses a top-down left-right convention for expressing dependencies.) • Visual symmetry is maintained. To close wizards, click the . To show/hide tasks or steps, click the section header. Options for wizards are set in the Wizard (p. 312) section of the Options dialog box under the Mechanical application. The The Mechanical Wizard (p. 230) is available for your use in the Mechanical application. The Mechanical Wizard The Mechanical Wizard appears in the right side panel whenever you click the in the toolbar. You can close the Mechanical Wizard at any time by clicking at the top of the panel. To show or hide the sections of steps in the wizard, click the section header. Features of the Mechanical Wizard The Mechanical Wizard works like a web page consisting of collapsible groups and tasks. Click a group title to expand or collapse the group; click a task to activate the task. When activated, a task navigates to a particular location in the user interface and displays a callout with a message about the status of the task and information on how to proceed. Activating a task may change your tab selection, cursor mode, and Tree Outline (p. 235) selection as needed to set the proper context for proceeding with the task. You may freely click tasks to explore the Mechanical application. Standard tasks WILL NOT change any information in your simulation. Callouts close automatically based on your actions in the software. Click inside a callout to close it manually. Most tasks indicate a status via the icon to the left of the task name. Rest your mouse on a task for a description of the status. Each task updates its status and behavior based on the current Tree Outline (p. 235) selection and software status. Tasks are optional. If you already know how to perform an operation, you don't need to activate the task. Click the Choose Wizard task at the top of the Mechanical Wizard to change the wizard goal. For example, you may change the goal from Find safety factors to Find fatigue life. Changing the wizard goal does not modify your simulation. 230 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Wizards At your discretion, simulations may include any available feature not covered under Required Steps for a wizard. The Mechanical Wizard does not restrict your use of the Mechanical application. You may use the Mechanical Wizard with databases from previous versions of the Mechanical application. To enable the Mechanical Wizard, click or select View> Windows> the Mechanical Wizard. Types of the Mechanical Wizards There are wizards that guide you through the following simulations: • Safety factors, stresses and deformation • Fatigue life and safety factor • Natural frequencies and mode shapes • Optimizing the shape of a part • Heat transfer and temperatures • Magnetostatic results • Contact region type and formulation Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 231 232 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Basics • The Mechanical Application Interface • Customizing the Mechanical Application The Mechanical Application Interface The following topics are covered in this section: The Mechanical Application Window Tree Outline Environment Filtering Interface Behavior Based on License Levels Suppress and Unsuppress Items Tabs Geometry Legend Functionality Graphical Selection Windows Management Details View Parameters Toolbars Print Preview Triad and Rotation Cursors Exporting Data The Mechanical Application Window The following is an example of the Mechanical application interface. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 233 Basics The functional elements of the interface include the following. Window Component Description Main Menu This menu includes the basic menus such as File and Edit. Standard Toolbar This toolbar contains commonly used application commands. Graphics Toolbar This toolbar contains commands that control pointer mode or cause an action in the graphics browser. Context Toolbar This toolbar contains task-specific commands that change depending on where you are in the Tree Outline. Unit Conversion Toolbar Not visible by default.This toolbar allows you to convert units for various properties. Named Selection Toolbar Not visible by default.This toolbar contains options to manage named selections. Graphics Options Toolbar This toolbar provides quick access to features that are intended to improve your ability to distinguish edge and mesh connectivity in a surface body model. Tree Outline Outline view of the simulation project. Always visible. Location in the outline sets the context for other controls. Provides access to object's context menus. Allows renaming of objects. Establishes what details display in the Details View. Details View The Details View corresponds to the Outline selection. Displays a details window on the lower left panel of the Mechanical application window which contains details about each object in the Outline. 234 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Window Component Description Geometry Displays and manipulates the visual representation of the object selected in the Outline. This window displays: • 3D Geometry • 2D/3D Graph • Spreadsheet • HTML Pages Note The Geometry window may include splitter bars for dividing views. Reference Help Opens an objects reference help page for the highlighted object. Tabs The document tabs that are visible on the lower right portion of the Mechanical application Window. Status Bar Brief in-context tip. Selection feedback. Splitter Bar Application window has up to 3 splitter bars. Tree Outline The object Tree Outline matches the logical sequence of simulation steps. Object sub-branches relate to the main object. For example, an analysis environment object, such as Static Structural, contains loads. You can right-click on an object to open a context menu which relates to that object. You can rename objects, provided the objects are not being solved. Refer to the Mechanical application objects reference pages for more information. Note Numbers preceded by a space at the end of an object's name are ignored. This is especially critical when you copy objects or duplicate object branches. For example, if you rename two force loads as Force 1 and Force 2, then copy the loads to another analysis environment, the copied loads will be named Force and Force 1. However, if you rename the loads as Force_1 and Force_2, the copied loads will retain the same names as the two original loads. The following topics present further details related to the tree outline. Tree Outline Conventions Tree Outline Go To Options Tree Outline Conventions The Tree Outline uses the following conventions: • Icons appear to the left of objects in the tree. Their intent is to provide a quick visual reference to the identity of the object. For example, icons for part and body objects (within the Geometry object folder) can help distinguish solid, surface and line bodies. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 235 Basics • A symbol to the left of an item's icon indicates that it contains associated subitems . Click to expand the item and display its contents. • To collapse all expanded items at once, double-click the Project name at the top of the tree. • Drag-and-drop function to move and copy objects. • To delete a tree object from the Tree Outline (p. 235), right-click on the object and select Delete. A confirmation dialog asks if you want to delete the object. Status Symbols A small status icon displays just to the left of the main object icon in the Tree Outline (p. 235) Status Symbol Name Symbol Example Underdefined A load requires a nonzero magnitude. Error Load attachments may break during an Update. Mapped Face or Match Control Failure Face could not be mapped meshed, or mesh of face pair could not be matched. Ok Everything is ok. Needs to be Updated Equivalent to "Ready to Answer!" Hidden A body or part is hidden. Meshed The symbol appears for a meshed body within the Geometry folder, or for a multibody part whose child bodies are all meshed. Suppress An object is suppressed. Solve • Yellow lightning bolt: Item has not yet been solved. • Green lightning bolt: Solve in progress. • Green check mark: Successful solution. • Red lightning bolt: Failed solution. An overlaid pause icon indicates the solution could resume with the use of restart points. • Green down arrow: Successful background solution ready for download. • Red down arrow: Failed background solution ready for download. See also Tree Outline (p. 235). Note The state of an environment folder can be similar to the state of a Solution folder. The solution state can indicate either solved (check mark) or not solved (lightening bolt) depending on whether or not an input file has been generated. 236 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Tree Outline Go To Options The Go To feature provides you with instant visual correlation of objects in the tree outline as they relate to various characteristics of the model displayed in the Geometry window. To activate this feature, right-click anywhere in the Geometry window, choose Go To, then choose an option in the context menu. In some cases (see table below), you must select geometry prior to choosing the Go To feature. The resulting objects that match the correlation are highlighted in the tree outline and the corresponding geometry is highlighted on the model. For example, you can identify contact regions in the tree that are associated with a particular body by selecting the geometry of interest and choosing the Contacts for Selected Bodies option. The contact region objects associated with the body of the selected items will be highlighted in the tree and the contact region geometry will be displayed on the model. Several options are filtered and display only if specific conditions exist within your analysis. The Go To options are presented in the following table along with descriptions and conditions under which they appear in the context menu. Go To Option Description / Application Required Conditions for Option to Appear Corresponding Bodies in Tree Identifies body objects in the tree that correspond to selections in the Geometry window. At least one vertex, edge, face, or body is selected. Hidden Bodies in Tree Identifies body objects in the tree that correspond to hidden bodies in the Geometry window. At least one body is hidden. Suppressed Bodies in Tree Identifies body objects in the tree that correspond to suppressed bodies in the Geometry window. At least one body is suppressed. Bodies Without Contacts in Tree Identifies bodies that are not in contact with any other bodies. More than one body in an assembly. When you are working with complex assemblies of more than one body, it is helpful to find bodies that are not designated to be in contact with any other bodies. Bodies that are not in contact with other bodies generally cause problems for a solution. They are prone to rigid body movements. Parts Without Contacts in Tree Identifies parts that are not in contact with any other parts. More than one part in an assembly. When you are working with complex assemblies of more than one multibody part, it is helpful to find parts that are not designated to be in contact with any other parts. For example, this is useful when dealing with shell models which can have parts that include many bodies each. Using this feature is pre- Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 237 Basics Go To Option Description / Application Required Conditions for Option to Appear ferred over using the Bodies Without Contact in Tree option when working with multibody parts mainly because contact is not a typical requirement for bodies within a part. Such bodies are usually connected by shared nodes at the time of meshing. Contacts for Selected Bodies Identifies contact region objects in the tree that are associated with selected bodies. At least one vertex, edge, face, or body is selected. Contacts Common to Selected Bodies Identifies contact region objects in the tree that are shared among selected bodies. At least one vertex, edge, face, or body is selected. Joints for Selected Bodies Identifies joint objects in the tree that are associated with selected bodies. At least one vertex, edge, face, or body is selected. Joints Common to Selected Bodies Identifies joint objects in the tree that are shared among selected bodies. At least one vertex, edge, face, or body is selected. Springs for Selected Bodies Identifies spring objects in the tree that are associated with selected bodies. At least one vertex, edge, face, or body is selected. Mesh Controls for Selected Bodies Identifies mesh control objects in the tree that are associated with selected bodies. At least one vertex, edge, face, or body is selected. Mesh Connections for Selected Bodies Highlights mesh connection objects in the tree that are associated with the selection. At least one vertex, edge, face, or body is selected and at least one mesh connection exists. Mesh Connections Common to Selected Bodies Highlights mesh connection objects in the tree that are shared among selected bodies. At least one vertex, edge, face, or body is selected. Field Bodies in Tree Identifies enclosure objects in the tree that are associated with selected bodies. At least one body is an enclosure. Bodies With One Element Through the Thickness Identifies bodies in the tree with one element in at least two directions (through the thickness). At least one body with one element in at least two directions (through the thickness). This situation can produce invalid results when used with reduced integration. See At Least One Body Has Been Found to Have Only 1 Element (p. 1077) in the troubleshooting section for details. Thicknesses for Selected Faces Identifies objects with defined thicknesses in the tree that are associated with selected faces. At least one face with defined thickness is selected. Environment Filtering The Mechanical interface includes a filtering feature that only displays model-level items applicable to the particular analysis type environments in which you are working. This provides a simpler and more focused interface. 238 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface The environment filter has the following characteristics: • Model-level objects in the tree that are not applicable to the environments under a particular model are hidden. • The user interface inhibits the insertion of model-level objects that are not applicable to the environments of the model. • Model-level object properties (in the Details view of objects) that are not applicable to the environments under the model are hidden. The filter is enabled by default when you enter the Mechanical application. You can disable the filter by highlighting the Model object, clicking the right mouse button, and choosing Disable Filter from the context menu. To enable the filter, repeat this procedure but choose Auto Filter from the context menu. You can also check the status of the filter by highlighting the Model object and in the Details view, noting whether Control under Filter Options is set to Enabled or Disabled. The filter control setting (enabled or disabled) is saved when the model is saved and returns to the same state when the database is resumed. Interface Behavior Based on License Levels The licensing level that you choose automatically allows you to exercise specific features and blocks other features that are not allowed. Presented below are descriptions of how the interface behaves when you attempt to use features not allowed by a license level. • If the licensing level does not allow an object to be inserted, it will not show in the Insert menus. • If you open a database with an object that does not fit the current license level, the database changes to "read-only" mode. • If a Details view option is not allowed for the current license level, it is not shown. • If a Details view option is not allowed for the current license level, and was preselected (either through reopening of a database or a previous combination of settings) the Details view item will become invalid and shaded yellow. Note When you attempt to add objects that are not compatible with your current license level, the database enters a read-only mode and you cannot save data. However, provided you are using any license, you can delete the incompatible objects, which removes the read-only mode and allows you to save data and edit the database. Suppress and Unsuppress Items Several items in the Mechanical application tree outline can be suppressed, meaning that they can be individually removed from any further involvement in the analysis. For example, suppressing a part removes the part from the display and from any further loading or solution treatment. For Geometry and Environment folders, the objects that you Suppress are removed from the solved process. For Solution folder, if you suppress a solved result object, the result information will be deleted for the suppressed result object. The suppressed object is not considered in the subsequent result evaluations. You can use this feature to leave out an under-defined result object and obtain values for other results Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 239 Basics under Solution. You can Unsuppress the result object and evaluate all results to get an updated result value. To suppress results objects from the context menu, right-click the result object, and then click Suppress. Click Yes to suppress the object, or No to cancel the message box. How to Suppress/Unsuppress an Item If available, set the Suppressed option in the Details view to Yes. Conversely, you can unsuppress items by setting the Suppressed option to No. You can also suppress/unsuppress these items through context menu options available via a right mouse button click. Included is the context menu option Invert Suppressed Body Set, which allows you to reverse the suppression state of all bodies (unsuppressed bodies become suppressed and suppressed bodies become unsuppressed). You can suppress the bodies in a named selection using either the context menu options mentioned above , or through the Named Selection Toolbar. Another way to suppress a body is by selecting it in the graphics window, then using a right mouse button click in the graphics window and choosing Suppress Body in the context menu. Conversely, the Unsuppress All Bodies option is available for unsuppressing bodies. Options are also available in this menu for hiding or showing bodies. Hiding a body only removes the body from the display. A hidden body is still active in the analysis. Tabs The bottom of the browser pane in the application window contains the three main document tabs shown above. The tabs provide alternative views of the current Outline object. You can move among the Geometry (p. 240), Print Preview (p. 301), and Report Preview (p. 864) tabs at any time by clicking the tabs. The Outline remains visible. Geometry The Geometry window displays the geometry model. All view manipulation, geometry selection and graphics display of a model occurs in the Geometry window. The window contains: • 3D Graphics. • A scale ruler. • A legend and a triad control (when you display the solution). • Contour results objects. Note When you insert a Comment, the Geometry window splits horizontally, and the HTML comment editor displays in the bottom of the window. The Geometry representation of the model displays at the top. For more information about editing comments, refer to the Comment object reference. 240 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Displaying Shells for Large Deflections The display of shells may become distorted for large deformations such as in large deflection, explicit dynamics analyses, etc. A workaround is to disable shell thickness by toggling View> Thick Shells and Beams on the Main Menu (p. 280). Or, set a Workbench variable, UsePseudoShellDisp = 1, via Tools> Variable Manager. It may be necessary to toggle the deformation scaling from True Scale to Undeformed to True Scale again. Note that this option requires True Scaling to work properly. Legend Functionality To view the legend, confirm that Legend is selected in the View menu. The legend is displayed in the top left corner of the graphics window when you select an object in the tree outline. Note that the legend is not accessible via any of the toolbars in any of the modules. Repositioning Legend To reposition the legend within the graphics window, select the legend with your mouse, hold down the left mouse button and drag the mouse. Note that the multiple view window configuration does not allow for the legend to be permanently saved in a unique location. Resumption of a database file and toggling between a single view and multiple views will result in the legend being saved to its default position in the upper left corner of the graphics window. Discrete Legends in the Mechanical Application • Geometry Legend: Contents is driven by Display Style selection in the Details view panel. • Joint Legend: Depicts the free degrees of freedom characteristic of the type of joint. • Results Legend: Content is accessible via the right mouse when the legend for a solved object in the Solution folder is selected. Graphical Selection Tips for working with graphics • You can use the ruler, shown at the bottom of the Geometry window, to obtain a good estimate of the scale of the displayed geometry or results (similar to using a scale on a geographic map). The ruler is useful when setting mesh sizes. • You can rotate the view in a geometry selection mode by dragging your middle mouse button. You can zoom in or out by rolling the mouse wheel. • Hold the control key to add or remove items from a selection. You can paint select faces on a model by dragging the left mouse button. • You can pan the view by using the arrow keys. You can rotate the view by using the control key and arrow keys. • Click the interactive Triad and Rotation Cursors (p. 301) to quickly change the graphics view. • Use the stack of rectangles in the lower left corner of the Geometry (p. 240) to select faces hidden by your current selection. • To rotate about a specific point in the model, switch to rotate mode and click the model to select a rotation point. Click off the model to restore the default rotation point. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 241 Basics • To multi-select one or more faces, hold the CTRL key and click the faces you wish to select, or use Box Select to select all faces within a box. The CTRL key can be used in combination with Box Select to select faces within multiple boxes. • Click the Viewports (p. 250) icon to view up to four images in the Geometry (p. 240) window. • Controls are different for Graphs & Charts. Rotation Cursors for Display (p. 242) Pointer Modes (p. 242) Defining Direction (p. 242) Direction Defaults (p. 243) Highlighting Geometry in Select Direction Mode (p. 243) Selecting Direction by Face (p. 243) Selecting Direction Using the Triad and Rotation Cursors (p. 301) Highlighting (p. 244) Picking (p. 244) Blips (p. 244) Painting (p. 245) Depth Picking (p. 245) Selection Filters (p. 245) Extend Selection Menu (p. 246) The Select Command Viewports (p. 250) Graph Chart Control (p. 251) Rotation Cursors for Display Activates rotational controls in the Geometry window (left mouse button). The cursor changes appearance depending on its window location. Pointer Modes The pointer in the graphics window is always either in a picking filter mode or a view control mode. When in a view control mode the selection set is locked. To resume the selection, repress a picking filter button. The Graphics Toolbar offers several geometry filters and view controls as the default state, for example, face, edge, rotate, and zoom. If a Geometry field in the Details View (p. 274) has focus, inappropriate picking filters are automatically disabled. For example, a pressure load can only be scoped to faces. If the Direction field in the Details View (p. 274) has focus, the only enabled picking filter is Select Direction. Select Direction mode is enabled for use when the Direction field has focus; you never choose Select Direction manually. You may manipulate the view while selecting a direction. In this case the Select Direction button allows you to resume your selection. Defining Direction Orientation may be defined by any of the following geometric selections: • A planar face (normal to). • A straight edge. 242 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface • Cylindrical or revolved face (axis of ). • Two vertices. Direction Defaults If you insert a load on selected geometry that includes both a magnitude and a direction, the Direction field in the Details view states a particular default direction. For example, a force applied to a planar face by default acts normal to the face. One of the two directions is chosen automatically. The load annotation displays the default direction. Highlighting Geometry in Select Direction Mode Unlike other picking filters (where one specific type of geometry highlights during selection) the Select Direction filter highlights any of the following during selection: • Planar faces • Straight edges • Cylindrical or revolved faces • Vertices If one vertex is selected, you must hold down the CTRL key to select the other. When you press the CTRL key, only vertices highlight. Selecting Direction by Face The following figure shows the graphic display after choosing a face to define a direction. The same display appears if you edit the Direction field later. • The selection blip indicates the hit point on the face. • Two arrows show the possible orientations. They appear in the lower left corner of the Geometry (p. 240) window. If either arrow is clicked, the direction flips. When you finish editing the direction, the hit point (initially marked by the selection blip) becomes the default location for the annotation. If the object has a location as well as a direction (e.g. Remote Force), the location of the annotation will be the one that you specify, not the hit point. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 243 Basics Note The scope is indicated by painting the geometry. Highlighting Hovering your cursor over a geometry entity highlights the selection and provides visual feedback about the current pointer behavior (e.g. select faces) and location of the pointer (e.g. over a particular face). As illustrated here, the face edges are highlighted in colored dots. Picking A pick means a click on visible geometry. A pick becomes the current selection, replacing previous selections. A pick in empty space clears the current selection. By holding the CTRL key down, you can add unselected items to the selection and selected items can be removed from the selection. Clicking in empty space with CTRL depressed does not clear current selections. Blips A crosshair blip appears at the location where you release the mouse button: A blip serves to: • Mark a picked point on visible geometry. • Represent a ray normal to the screen passing through all hidden geometry. Note This is important for depth picking, a feature discussed below. Blips disappear when you clear the selection or make another pick. 244 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Painting Painting means dragging the mouse on visible geometry to select more than one entity. A pick is a trivial case of painting. Without holding the CTRL key down, painting picks all appropriate geometry touched by the pointer. Depth Picking Depth Picking allows you to pick geometry through the Z-order behind the blip. Whenever a blip appears above a selection, the graphics window displays a stack of rectangles in the lower left corner. The rectangles are stacked in appearance, with the topmost rectangle representing the visible (selected) geometry and subsequent rectangles representing geometry hit by a ray normal to the screen passing through the blip, front to back. The stack of rectangles is an alternative graphical display for the selectable geometry. Each rectangle is drawn using the same edge and face colors as its associated geometry. Highlighting and picking behaviors are identical and synchronized for geometry and its associated rectangle. Moving the pointer over a rectangle highlights both the rectangle its geometry, and vice versa. CTRL key and painting behaviors are also identical for the stack. Holding the CTRL key while clicking rectangles picks or unpicks associated geometry. Dragging the mouse (Painting (p. 245)) along the rectangles picks geometry front-to-back or back-to-front. Selection Filters The mouse pointer in the graphics window is either in a picking filter mode or a view control mode. A depressed button in the graphics toolbar indicates the current mode. Filter Behavior Vertices Vertices are represented by concentric circles about the same size as a blip.The circumference of a circle highlights when the pointer is within the circle. Edges Painting may be used to pick multiple edges or to "paint up to" an edge (to avoid tediously positioning the pointer prior to clicking). Faces Allows selection of faces. Highlighting occurs by dotting the banding edges of the face. Bodies Picking and painting: select entire bodies. Highlighted by drawing a bounding box around the body.The stack shows bodies hidden behind the blip (useful for selecting contained bodies). Selection Modes The Select Mode toolbar button allows you to select items designated by the Selection Filters through the Single Select or Box Select drop-down menu options. • Single Select (default): Click on an item to select it. • Box Select: Define a box that selects filtered items. When defining the box, the direction that you drag the mouse from the starting point determines what items are selected, as shown in the following figures: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 245 Basics – Dragging to the right to form the box selects entities that are completely enclosed by the box. – Visual cue: 4 tick marks completely inside the box. – Dragging to the left to form the box selects all entities that touch the box. – Visual cue: 4 tick marks that cross the sides of the box. • Box Volume Select: Available for node-based Named Selections only. Selects all the surface and internal node within the box boundary across the cross-section. The line of selection is normal to the screen. • Lasso Select: Available for node-based Named Selections only. Selects surface nodes that occur within the shape you define. • Lasso Volume Select: Available for node-based Named Selections only. Selects nodes that occur within the shape you define. You can use the CTRL key for multiple selections in both modes. Extend Selection Menu The Extend Selection drop-down menu is enabled only for edge or face selection mode and only with a selection of one or more edges or faces. The following options are available in the drop-down menu: • Extend to Adjacent – 246 For faces, Extend to Adjacent searches for faces adjacent to faces in the current selection that meet an angular tolerance along their shared edge. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Single face selected in part on the left. – For edges, Extend to Adjacent searches for edges adjacent to edges in the current selection that meet an angular tolerance at their shared vertex. Single edge selected in part on the left. • Additional adjacent faces selected after Extend to Adjacent option is chosen. Additional adjacent edges selected after Extend to Adjacent option is chosen. Extend to Limits – For faces, Extend to Limits searches for faces that are tangent to the current selection as well as all faces that are tangent to each of the additional selections within the part. The selections must meet an angular tolerance along their shared edges. Single face selected in part on the left. – Additional tangent faces selected after Extend to Limits option is chosen. For edges, Extend to Limits searches for edges that are tangent to the current selection as well as all edges that are tangent to each of the additional selections within the part. The selections must meet an angular tolerance along their shared vertices. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 247 Basics Single edge selected in part on the left. • Additional tangent edges selected after Extend to Limits option is chosen. Extend to Instances (available only if CAD pattern instances are defined in the model): When a CAD feature is repeated in a pattern, it produces a family of related topologies (for example, vertices, edges, faces, bodies) each of which is named an "instance". Using Extend to Instances, you can use one of the instances to select all others in the model. As an example, consider three parts that are instances of the same feature in the CAD system. First select one of the parts. Then, choose Extend to Instances. The remaining two part instances are selected. 248 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface See CAD Instance Meshing for further information. • Extend to Connection – As described in Define Connections (p. 8), connections can be contact regions, joints, mesh connections, and so on. Available for faces only, the Extend to Connection option is especially useful for assembly meshing as an aid in picking faces related to flow volumes. For example, if you are using a Fluid Surface object to help define a virtual body, you can generate connections, pick one face on each body of the flow volume, and then select Extend to Connection. As a result, the faces related to the flow volume are picked to populate the Fluid Surface object. Extend to Connection searches for faces that are adjacent to the current selection as well as all faces that are adjacent to each of the additional selections within the part, up to and including all connections on the selected part. This does not include all faces that are part of a connection—it includes only those faces that are part of a connection and are also on the selected part. If an edge used by a connection is encountered, the search stops at the edge; a face across the edge is not selected. If there are no connections, all adjacent faces are selected. If the current selection itself is part of a connection, it remains selected but the search stops. Note → The extent of the faces that will be included depends greatly on the current set of connections, as defined by the specified connections criteria (for example, Connection Type, Tolerance Value, and so on). By modifying the criteria and regenerating the connections, a different set of faces may be included. Refer to Common Connections Folder Operations for Auto Generated Connections (p. 407) for more information. → The figures below illustrate simple usage of the Extend to Connection option. Refer to Defining Virtual Bodies in the Meshing help for a practical example of how you can use the Extend to Connection option and virtual bodies together to solve assembly meshing problems. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 249 Basics Single face selected in part. Additional connected faces selected after Extend to Connection option is chosen. Single face selected in part. In this example, a multiple edge to single face connection is defined. Additional connected faces selected after Extend to Connection option is chosen. When the connection is encountered, search stops at edge. For all options, you can modify the angle used to calculate the selection extensions in the Workbench Options dialog box setting Extend Selection Angle Limit under Graphics Interaction. Viewports The Viewports toolbar button allows you to split the graphics display into a maximum of four simultaneous views. You can see multiple viewports in the Geometry (p. 240) window when any object in the tree is in focus except Project. You can choose one, horizontal, vertical, or four viewports. Each viewport can have separate camera angles, labels, titles, backgrounds, etc. Any action performed when viewports 250 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface are selected will occur only to the active viewport. For example, if you animate a viewport, only the active viewport will be animated, and not the others. A figure can be viewed in a single viewport only. If multiple viewports are created with the figure in focus, all other viewports display the parent of the figure. Note Each viewport has a separate Slice tool, and therefore separate Slice Plane. The concept of copying a Slice Plane from one window to the next does not exist. If you want Slice Planes in a new window, you must create them in that window. Viewports are not supported in stepped analyses. Graph Chart Control The following controls are available for Graphs/Charts for Adaptive Convergence (p. 787), and Fatigue Results (p. 695) result items. Feature Control Pan Right Mouse Button Zoom Middle Mouse Button Box Zoom Alt+Left Mouse Button Rotate (3D only) Left Mouse Button Perspective Angle (3D only) Shift+Left Mouse Button Display Coordinates (2D only) Ctrl+Left Mouse Button along graph line Tips for working with graphs and charts: • Some features are not available for certain graphs. • Zoom will zoom to or away from the center of the graph. Pan so that your intended point of focus is in the center prior to zooming. • If the graph has a Pan/Zoom control box, this can be used to zoom (shrink box) or pan (drag box). • Double-clicking the Pan/Zoom control box will return it to its maximum size. Windows Management This section includes descriptions of the various windows that are displayed within the Mechanical Application. The following topics are covered: Workbench Windows Manager Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 251 Basics Selection Information Window Worksheet Window Graph and Tabular Data Windows Messages Window Graphics Annotation Window New Section Plane The Mechanical Wizard Window Workbench Windows Manager The Workbench window contains a number of panes that house graphics, outlines, details and other views and controls. The window manager allows you to move, resize, tab dock and autohide panes. Tab dock means that two or more panes reside in the tabs in the same space on screen. Autohide means that a pane (or tab docked group of panes) automatically collapses when not in use to free screen space. Restore Original Window Layout Choose "Restore Original Window Layout" from the View menu to return to the default original pane configuration. Window Manager Features AutoHiding Panes are either pinned or unpinned . Toggle this state by clicking the icon in the pane title bar. A pinned pane occupies space in the Workbench window. An unpinned pane collapses to a tab on the periphery of the window when inactive. To work with an unpinned pane, move the mouse pointer into the tab; the pane will fly out on top of other panes in the Workbench window. The pane will remain visible as long as it is active or contains the mouse pointer. Pin the pane to restore its previous configuration. Moving and Docking Drag the title bar to move a pane, or drag a tab to undock panes. Once the drag starts a number of dock targets (blue-filled arrows and circle) appear above the Workbench window: Move the mouse pointer over a target to preview the resulting location for the pane. Arrow targets indicate adjacent locations; a circular target allows tab-docking of two or more panes (to share screen space). Release the button on the target to move the pane. Abort the drag operation by pressing the ESC key. Resize panes by dragging the borders. Selection Information Window The Selection Information window provides a quick and easy way for you to interrogate and find geometric information on items that you have selected on the model. The following topics are covered in this section: 252 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Activating the Selection Information Window Supported Selection Modes and Reported Information Selection Information Toolbar Reselect, Export, and Sort Activating the Selection Information Window You can display the Selection Information window using any of the following methods: • Select the Selection Information button on the Standard Toolbar (p. 283). • Choose View>Windows>Selection Information from the Main Menu (p. 280). • Double-click the field on the Status Bar that displays the geometry description. An example Selection Information window is illustrated below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 253 Basics Supported Selection Modes and Reported Information The supported selection modes are vertex, edge, face, body, and coordinate. Reported information for each mode is described below. Vertex Individual vertex location and average location are reported. If two vertices are selected, their distance and x, y, z distances are reported. The bodies that the vertex attaches to are also reported. 254 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Node The information displayed for selected node is similar to a vertex with addition of the Node ID. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 255 Basics Edge Combined and individual edge length and centroid are reported. The bodies that the edge attaches to are reported. The type of the edge is also reported. If an edge is of circle type, the radius of the edge is reported. Face Combined and individual area and centroid are reported. The bodies that the face attaches to are reported. The type of the face is reported. If a face is of cylinder type, the radius of the face is also reported. 256 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Body Combined and individual volume, mass, and centroid are reported. The body name is reported. Your choice of the mass moment of inertia in the selected coordinate system or the principal is also reported. The choice is provided in the Selection Information Column Control dialog box (accessible from the Selection Information Toolbar (p. 261)). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 257 Basics 258 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Coordinate If there is a mesh present, the picked point location and the closest mesh node ID and location are reported. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 259 Basics In the case of a surface body model, the closest node will be located on the non-expanded mesh (that can be seen if you turn off the option View> Thick Shells and Beams). Non-expanded shell view: Expanded shell view: 260 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Selection Information Toolbar The toolbar located at the top of the Selection Information window includes the following controls: Each of these controls is described below. Coordinate System A Coordinate System drop down selection box is provided on the toolbar. You can select the coordinate system under which the selection information is reported. The centroid, location, and moment of inertia information respect the selected coordinate system. For example, if a cylindrical coordinate system is selected, the vertex location is reported using the cylindrical coordinates. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 261 Basics Selection Information Column Control If you click the Selection Information Column Control, a column control dialog box appears to give you control over what columns are visible and what columns you can hide. The choices that you made with the column control are retained for the application. 262 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Note The Moment of Inertia option is unchecked by default. The following example shows the effects of un-checking the centroid for face. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 263 Basics Selection Information Row Control The Selection Information Row Control has three options: Show Individual and Summary, Show Individual, and Show Summary. Depending upon your choice, the individual and/or summary information is reported. Reselect, Export, and Sort This section describes how you can reselect rows, export data, and sort data in the Selection Information window. Each function is described below. 264 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Reselect Right click to reselect the highlighted rows. Export Right click to export the table to a text file or Excel file. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 265 Basics Sort Click on the column header to sort the table. Worksheet Window The worksheet presents you with information about objects in the tree in the form of tables, charts and text, thereby supplementing the Details view. It is typically intended to summarize data for a collection of objects (for example, the Connections folder worksheet reveals the inputs for all contacts, joints and 266 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface others) or to receive tabular inputs (for example, to specify the coefficients and the analyses to include in Solution Combinations). Behavior • Dockable Worksheet By default, when you select an applicable object in the tree, a dockable Worksheet window will display alongside the Geometry window, allowing you to review both at once. You may, however, disable the display of the Worksheet window using the Worksheet toolbar button (see below). This preference is persisted in future sessions of the product. There are specific objects that ignore the preference, as outlined below. Worksheet Function • Worksheet Behavior When Object is Selected Example Objects Data input and display information Automatically appears and gains focus Constraint Equation, Solution Combination Display information related to object settings Automatically appears but does not gain focus Analysis Settings Display information related to objects within a folder Appears only if display is turned on manually using the Worksheet toolbar button (see below) Geometry folder, Contact folder Worksheet Toolbar Button For tree objects that include an associated Worksheet, the Worksheet button on the standard toolbar allows you to toggle the Worksheet window display on or off. The button is not available (grayed out) for objects that do not include a Worksheet. Worksheets designed to display many data items do not automatically display the data. The data readily appears however when you click the Worksheet button. This feature applies to the worksheets associated with the following object folders: Geometry, Coordinate System, Contact, Remote Points, Mesh, and Solution. Features • Go To Selected items This useful feature allows you to find items in either the tree or Geometry window that match one or more rows of the worksheet. If the worksheet displays a tabular summary of a number of objects, select the rows of interest, right-click, and choose Go To Selected Items in Tree to instantly highlight items that match the contents of the Name column (leftmost column). Control is thus transferred to the tree or Geometry window, as needed. • Viewing Selected Columns When a worksheet includes a table with multiple columns, you can control which columns to display. To do so, right-click anywhere inside the table. From the context menu, check the column names of interest to activate their display. Some columns may ignore this setting and remain hidden should they be found inapplicable. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 267 Basics To choose the columns that will display, right mouse click anywhere inside the worksheet table. From the context menu, click on any of the column names. A check mark signifies that the column will appear. There are some columns in the worksheet that will not always be shown even if you check them. For example, if all contact regions have a Pinball Region set to Program Controlled, the Pinball Radius will not display regardless of the setting. Graph and Tabular Data Windows Whenever you highlight the following objects in the Mechanical application tree, a Graph window and Tabular Data window appear beneath the Geometry window. • Analysis Settings • Loads • Contour Results • Probes • Charts These windows are designed to assist you in managing analysis settings and loads and in reviewing results. The Graph window provides an instant graphical display of the magnitude variations in loads and/or results, while the Tabular Data window provides instant access to the corresponding data points. Below are some of the uses of these windows. Analysis Settings For analyses with multiple steps, you can use these windows to select the step(s) whose analysis settings you want to modify. The Graph window also displays all the loads used in the analysis. These windows are also useful when using restarts. See Solution Restarts (p. 759) for more information. Loads Inserting a load updates the Tabular Data window with a grid to enable you to enter data on a perstep basis. As you enter the data, the values are reflected in the Graph window. A check box is available for each component of a load in order to turn on or turn off the viewing of the load in the Graph window. Components are color-coded to match the component name in the Tabular Data window. Clicking on a time value in the Tabular Data window or selecting a row in the Graph window will update the display in the upper left corner of the Geometry window with the appropriate time value and load data. As an example, if you use a Displacement load in an analysis with multiple steps, you can alter both the degrees of freedom and the component values for each step by modifying the contents in the Tabular Data window as shown above. If you wish for a load to be active in some steps and removed in some other steps you can do so by following the steps outlined in Activation/Deactivation of Loads (p. 531). 268 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Contour Results and Probes For contour results and probes, the Graph and Tabular Data windows display how the results vary over time. You can also choose a time range over which to animate results. Typically for results the minimum and maximum value of the result over the scoped geometry region is shown. To view the results in the Geometry window for the desired time point, select the time point in the Graph window or Tabular Data window, then click the right mouse button and choose Retrieve Results. The Details view for the chosen result object will also update to the selected step. Charts With charts, the Graph and Tabular Data windows can be used to display loads and results against time or against another load or results item. Context Menu Options Presented below are some of the commonly used options available in a context menu that displays when you click the right mouse button within the Graph window and/or the Tabular Data window. The options vary depending on how you are using these windows (for example, loads vs. results). • Retrieve This Result: Retrieves and presents the results for the object at the selected time point. • Insert Step: Inserts a new step at the currently selected time in the Graph window or Tabular Data window. The newly created step will have default analysis settings. All load objects in the analysis will be updated to include the new step. • Delete Step: Deletes a step. • Copy Cell: Copies the cell data into the clipboard for a selected cell or group of cells. The data may then be pasted into another cell or group of cells. The contents of the clipboard may also be copied into Microsoft Excel. Cell operations are only valid on load data and not data in the Steps column. • Paste Cell: Pastes the contents of the clipboard into the selected cell, or group of cells. Paste operations are compatible with Microsoft Excel. • Delete Rows: Removes the selected rows. In the Analysis Settings object this will remove corresponding steps. In case of loads this modifies the load vs time data. • Select All Steps: Selects all the steps. This is useful when you want to set identical analysis settings for all the steps. • Select All Highlighted Steps: Selects a subset of all the steps. This is useful when you want to set identical analysis settings for a subset of steps. • Activate/Deactivate at this step!: This allows a load to become inactive (deleted) in one or more steps. By default any defined load is active in all steps. • Zoom to Range: Zooms in on a subset of the data in the Graph window. Click and hold the left mouse at a step location and drag to another step location. The dragged region will highlight in blue. Next, select Zoom to Range. The chart will update with the selected step data filling the entire axis range. This also controls the time range over which animation takes place. • Zoom to Fit: If you have chosen Zoom to Range and are working in a zoomed region, choosing Zoom to Fit will return the axis to full range covering all steps. Result data is charted in the Graph window and listed in the Tabular Data window. The result data includes the Maximum and Minimum values of the results object over the steps. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 269 Basics Messages Window The Messages Window is a Mechanical application feature that prompts you with feedback concerning the outcome of actions you have taken in the Mechanical application. For example, Messages display when you resume a database, Mesh a model, or when you initiate a Solve. Messages come in three forms: • Error • Warning • Information By default the Messages Window is hidden, but displays automatically as a result of irregularities during Mechanical application operations. To display the window manually: select View>Windows>Messages. An example of the Messages Window is shown below. In addition, the status bar provides a dedicated area (shown above) to alert you should one or more messages become available to view. The Messages Window can be auto-hidden or closed using the buttons on the top right corner of the window. Note You can toggle between the Graph and Messages windows by clicking a tab. Once messages are displayed, you can: • Double-click a message to display its contents in a pop-up dialog box. • Highlight a message and then press the key combination CTRL+C to copy its contents to the clipboard. • Press the Delete key to remove a selected message from the window. • Select one or more messages and then use the right mouse button click to display the following context menu options: 270 – Go To Object - Selects the object in the tree which is responsible for the message. – Show Message - Displays the selected message in a popup dialog box. – Copy - Copies the selected messages to the clipboard. – Delete - Removes the selected messages. – Refresh - Refreshes the contents of the Messages Window as you edit objects in the Mechanical application tree. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Graphics Annotation Window This window is displayed when you choose the New Graphics Annotation button located on the Standard Toolbar. See the description of that button in the Standard Toolbar (p. 283) section for more information. New Section Plane Use the Section Plane feature to create a cut or slice on your model so that you can view internal geometry, or mesh, and results displays. Selecting the New Section Plane button ( ) in the graphics toolbar displays the Section Planes window below the Details view, and initiates the New Section Plane function. Icon Button Application-level command New Section Plane Delete Section Plane Show Whole Elements (available when the Mesh object is selected) Example 1 Section Plane Usage • You can add a Section Plane by selecting the New Section Plane button and then dragging the mouse across the part. Each plane is created with a default name, “Section Plane 1”, “Section Plane 2”, etc. The newly created section plane will become active as indicated by the checkmark next to the plane’s name. To view the newly created plane, rotate the model. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 271 Basics • You can construct additional Section Planes by clicking the New Section Plane button and dragging additional lines across the model. • Activating multiple planes displays multiple sections • You can highlight a section plane’s name in the pane to display the plane’s anchor. • Click on the line on either side of the anchor to view the exterior on that side of the plane. The anchor displays a solid line on the side where the exterior is being displayed. Clicking on the same side a second time toggles between solid line and dotted line, i.e. exterior display back to section display. Note that for Geometry, display a capped view is always shown. • Drag the Section Plane or Capping Plane anchor to change the position of the plane. • You can maneuver between multiple planes by simply highlighting the plane names • To delete the selected Section Plane or Capping Plane, use the Delete Section Plane button. • When you are on a Mesh display you can use the Show Whole Elements button to display the adjacent elements to the slice plane which may be desirable in some cases. • For result displays, if the Section Plane feature is active, choosing Show Undeformed WireFrame from the Edges Options drop down menu on the Result Context Toolbar (p. 291) actually displays the wireframe with the deformations added to the nodes. This is intended to help you interpret the image when you drag the anchor across smaller portions of the model. • Unchecking all the planes effectively turns the Section Plane feature off. 272 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Note that in incidences such as very large models where the accessible memory is exhausted, the New Section Plane tool will revert to a Hardware Slice Mode that prohibits visualization of the mesh on the cut-plane. The Section Plane acts differently depending if you are viewing a result, mesh, or geometry display. When viewing a result or a mesh, the cut is performed by a software algorithm. When viewing geometry, the cut is performed using a hardware clipping method. This hardware clipping cuts away the model in a subtractive method. The software algorithm cuts away the model but always starts with the whole model. Note that the software algorithm caps the surfaces created by the section plane as opposed to the hardware clipping method. When capping, the software algorithm creates a visible surface at the intersection of the object and the section plane." As an example, consider the model shown below that is subjected to a horizontal and a vertical slice. The mesh display will show 75 % of the model while the geometry display will show 25 % of the model. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 273 Basics The Mechanical Wizard Window The Mechanical Wizard window appears in the right side panel whenever you click the Standard Toolbar (p. 283). See the The Mechanical Wizard (p. 230) section for details. in the Details View The Details view is located in the bottom left corner of the window. It provides you with information and details that pertain to the object selected in the Tree Outline (p. 235). Some selections require you to input information (e.g., force values, pressures). Some selections are drop-down dialogs, which allow you to select a choice. Fields may be grayed out. These cannot be modified. The following example illustrates the Details view for the object called Geometry. 274 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface For more information, see: Features (p. 275) Header (p. 276) Categories (p. 276) Undefined or Invalid Fields (p. 276) Decisions (p. 276) Text Entry (p. 277) Numeric Values (p. 278) Ranges (p. 278) Increments (p. 278) Geometry (p. 278) Exposing Fields as Parameters (p. 279) Options (p. 279) Features The Details view allows you to enter information that is specific to each section of the Tree Outline. It automatically displays details for branches such as Geometry, Model, Connections, etc. Features of the Details view include: • Collapsible bold headings. • Dynamic cell background color change. • Row selection/activation. • Auto-sizing/scrolling. • Sliders for range selection. • Combo boxes for boolean or list selection. • Buttons to display dialog box (e.g. browse, color picker). • Apply / Cancel buttons for geometry selection. • Obsolete items are highlighted in red. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 275 Basics Header The header identifies the control and names the current object. The header is not a windows title bar; it cannot be moved. Categories Category fields extend across both columns of the Details Pane: This allows for maximum label width and differentiates categories from other types of fields. To expand or collapse a category, double-click the category name. Undefined or Invalid Fields Fields whose value is undefined or invalid are highlighted in yellow: Decisions Decision fields control subsequent fields: 276 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Note The left column always adjusts to fit the widest visible label. This provides maximum space for editable fields in the right column. You can adjust the width of the columns by dragging the separator between them. Text Entry Text entry fields may be qualified as strings, numbers, or integers. Units are automatically removed and replaced to facilitate editing: Inappropriate characters are discarded (for example, typing a Z in an integer field). A numeric field cannot be entered if it contains an invalid value. It is returned to its previous value. Separator Clarification Some languages use “separators” within numerical values whose meanings may vary across different languages. For example, in English the comma separator [,] indicates “thousand” (“2,300” implies “two thousand three hundred”), but in German the comma separator indicates “decimal” (“2,300” implies “two and three tenths”, equivalent to “2.300” in English). To avoid misinterpretation of numerical values you enter that include separators, you are asked to confirm such entries before they are accepted. For example, in English, if you enter “2,300”, you receive a message stating the following: “Entered value is 2,300. Do you want to accept the correction proposed below? 2300 To accept the correction, please click Yes. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 277 Basics To close this message and correct the number yourself, please click No.” Note If an invalid entry is detected, an attempt is made to interpret the entry as numerical and you receive the message mentioned above if an alternate value is found. If an invalid value is entered, for example "a1.3.4", and no numerical alternative is found, the entry is rejected and the previous value is re-displayed. Numeric Values You can enter numeric expressions in the form of a constant value or expression, tabular data, or a function. See Specifying Load Values (p. 621) for further information. Ranges If a numeric field has a range, a slider appears to the right of the current value: If the value changes, the slider moves; if the slider moves the value updates. Increments If a numeric field has an increment, a horizontal up/down control appears to the right of the current value: The arrow button controls behave the same way a slider does. Geometry Geometry fields filter out inappropriate selection modes. For example, a bearing load can only be scoped to a face. Geometries other than face will not be accepted. 278 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Direction fields require a special type of selection: Clicking Apply locks the current selection into the field. Other gestures (clicking Cancel or selecting a different object or field) do not change the field's preexisting selection. Exposing Fields as Parameters A P appears beside the name of each field that may be treated as a parameter. Clicking the box exposes the field as a parameter. For more information, see Parameters (p. 279). Options Option fields allow you to select one item from a short list. Options work the same way as Decisions (p. 276), but don't affect subsequent fields. Options are also used for boolean choices (true/false, yes/no, enabled/disabled, fixed/free, etc.) Double-clicking an option automatically selects the next item down the list. Selecting an option followed by an ellipsis causes an immediate action. Parameters To parameterize a variable, click the box next to it. A P appears in the box. Items that cannot be parameterized do not display a check box and are left-aligned to save space. The boxes that appear in the Mechanical application apply only to the Parameter Workspace. Checking or unchecking these boxes will have no effect on which CAD parameters are transferred to Design Exploration. For more information, see Parameters (p. 867). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 279 Basics Toolbars Toolbars are displayed across the top of the window, below the menu bar. Toolbars can be docked to your preference. The layouts displayed are typical. You can double-click the vertical bar in the toolbar to automatically move the toolbar to the left. The various toolbars are described in the following sections: Main Menu Standard Toolbar Graphics Toolbar Context Toolbar Named Selection Toolbar Unit Conversion Toolbar Graphics Options Toolbar Main Menu The Main Menu includes the following items. File Menu Function Description Refresh All Data Updates the geometry, materials, and any imported loads that are in the tree. Save Project Allows you to save the project. Export Allows you to export outside of the project.You can export a .mechdat file (when running the Mechanical application) that later can be imported into a new Workbench project. Note that only the data native to the Mechanical application is saved to the .mechdat file. External files (such as solver files) will not be exported.You can also export the mesh for input to any of the following: FLUENT (.msh), POLYFLOW (.poly), CGNS (.cgns), and ICEM (.prj). Clear Generated Data Clears all results and meshing data from the database depending on the object selected in the tree. Close Mechanical Exits the Mechanical application session. Edit Menu Function Description Duplicate Duplicates the object you highlight.The model and environment duplication is performed at the Project Schematic level (see Duplicating, Moving, Deleting, and Replacing Systems for details). Duplicate Without Results (Only available on solved result objects.) Duplicates the object you highlight, including all subordinate objects. Because the duplicated objects have no result data the process is faster than performing Duplicate. Copy Copies an object. Cut Cuts the object and saves it for pasting. Paste Pastes a cut or copied object. Delete Deletes the object you select. 280 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Function Description Select All Selects all items in the Model of the current selection filter type. Select All is also available in a context menu if you click the right mouse button in the Geometry window. View Menu Function Description Shaded Exterior and Edges Displays the model in the graphics window with shaded exteriors and distinct edges. This option is mutually exclusive with Shaded Exterior and Wireframe. Shaded Exterior Displays the model in the graphics window with shaded exteriors only.This option is mutually exclusive with Shaded Exterior and Edges and Wireframe. Wireframe Displays the model in the graphics window with distinct edges only (recommended for seeing gaps in surface bodies).This option is mutually exclusive with Shaded Exterior and Edges and Shaded Exterior. A model's geometry, mesh, or named selection displayed as a mesh can be viewed in wireframe mode. Graphics Options Allows you to change the drawing options for edge connectivity. These options are discussed in more detail in the Graphics Options Toolbar (p. 298) section. This menu also allows you to change how faces are displayed as a function of Back-face Culling. Options include: • Auto Face Draw (default) - turning back-face culling on or off is program controlled. Using Section Planes is an example of when the application would turn this feature off. • Draw Front Faces - face culling is forced to stay on. Back-facing faces will not be drawn in any case, even if using Section Planes. • Draw Both Faces - back-face culling is turned off. Both front-facing and back-facing faces are drawn. Cross Section Solids (Geometry) Displays line body cross sections in 3-D geometry. See Viewing Line Body Cross Sections for details. Thick Shells and Beams Toggles the visibility of the thickness applied to a shell or beam in the graphics window when the mesh is selected. See notes below. Visual Expansion Toggles the visibility of either a single cyclic sector model result or the full symmetry model result in a cyclic symmetry analysis. Annotations Toggles the visibility of annotations in the graphics window. Custom Annotations Toggles the visibility of custom user annotations in the graphics window. Ruler Toggles the visibility of the visual scale ruler in the graphics window. Legend Toggles the visibility of the results legend in the graphics window. Triad Toggles the visibility of the axis triad in the graphics window. Eroded Nodes Toggles the visibility of eroded nodes for explicit dynamics analyses. Annotation Labels Toggles the visibility of annotation labels in the graphics window. Large Vertex Contours Used in mesh node result scoping to toggle the size of the displayed dots that represent the results at the underlying mesh nodes. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 281 Basics Function Description Display Edge Direction Displays model edge directions. The direction arrow appears at the midpoint of the edge. The size of the arrow is proportional to the edge length. Outline Expand All - Restores tree objects to their original expanded state. Collapse Environments - Collapses all tree objects under the Environment object(s). Collapse Models - Collapses all tree objects under the Model object(s). Toolbars Named Selections - Displays the Named Selection Toolbar. Unit Conversion - Displays the Unit Conversion Toolbar. Graphics Options - Displays theGraphics Options Toolbar. Windows Messages - Toggles the display of the Messages window. Mechanical Wizard - Toggles the display of a wizard on the right side of the window which prompts you to complete tasks required for an analysis. Graphics Annotations - Toggles the display of the Annotations window. Section Planes - Toggles the display of the Section Planes window. Selection Information - Toggles the display of the Selection Information window. Reset Layout - Restores the Window layout back to a default state. Notes: • Displaying Shells for Large Deflections: The display of shells may become distorted for large deformations such as in large deflection or during an Explicit Dynamics analyses. A workaround for this is to disable Shell Thickness by toggling View>Thick Shells and Beams. Or, set a Workbench variable, UsePseudoShellDisp = 1, through Tools> Variable Manager. It may be necessary to toggle the deformation scaling from True Scale to Undeformed to True Scale again (see Scaling Deformed Shape in the Context Toolbar Section). Note that this option requires True Scaling to work properly. • Displaying Shells on Shared Entities: The display of shells is done on a nodal basis. Therefore, graphics plot only 1 thickness per node, although node thickness can be prescribed and solved on a per elemental basis. When viewing shell thickness at sharp face intersections or a shared body boundary, the graphics display may become distorted. Units Menu Function Description Metric (m, kg, N, s, V, A) Sets unit system. Metric (cm, g, dyne, s, V, A) Metric (mm, kg, N, s, mV, mA) Metric (mm, t, N, s, mV, mA) Metric (mm, dat, N, s, mV, mA) Metric (µm, kg, µN, s, V, mA) U.S. Customary (ft, lbm, lbf, °F, s, V, A) U.S. Customary (in, lbm, lbf, °F, s, V, A) Degrees Sets angle units to degrees. Radians Set angle units to radians. 282 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Function Description rad/s Sets angular velocity units to radians per second. RPM Sets angular velocity units to revolutions per minute. Celsius Sets the temperature values to degree Celsius (not available if you choose either of the U.S. Customary settings). Kelvin Sets the temperature values to Kelvin (not available if you choose either of the U.S. Customary settings). Tools Menu Function Description Write Input File... Writes the Mechanical APDL application input file from the active Solution branch. This option does not initiate a Solve. Read Result File... Reads the Mechanical APDL application result files (.rst, solve.out, and so on) in a directory and copies the files into the active Solution branch. Solve Process Settings Allows you to configure solve process settings. Addins... Launches the Addins manager dialog that allows you to load/unload third-party addins that are specifically designed for integration within the Workbench environment. Options... Allows you to customize the application and to control the behavior of Mechanical application functions. Variable Manager Allows you to enter an application variable. Run Macro... Opens a dialog box to locate a script (.vbs , .js ) file. Help Menu Function Description Mechanical Help Displays the Help system in another browser window. About Mechanical Provides copyright and application version information. Note View menu settings are maintained between Mechanical application sessions except for the Outline items and Reset Layout in the Windows submenu. Standard Toolbar The Standard Toolbar contains application-level commands, configuration toggles and important general functions. Each icon button and its description follows: Icon Button Application-level command Description View Mechanical Wizard Activates the Mechanical Wizard in the user interface. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 283 Basics Icon Button Application-level command Description Solve analysis with a given solve process setting. Drop-down list to select a solve process setting. New Section Plane View a section cut through the model (geometry, mesh and results displays) as well as obtained capped displays on either side of the section. Refer to the New Section Plane section for details. New Graphics Annotation Adds a text comment for a particular item in the Geometry window.To use: • Select button in toolbar. • Click a placement location on the geometry. A chisel-shaped annotation is anchored in 3D. • A blank annotation appears and the Graphics Annotation window is made visible or brought forward. • A new row is created for the annotation. • Type entry. To edit, double click the corresponding entry in the Graphics Annotation window and type new information.To delete, select the entry and press the delete key.To move, select the annotation in the geometry window and move while pressing down the left mouse button.To exit without creating an annotation, re-click the annotation button. 284 New Chart and Table Refer to the Chart and Table section for details. New Simplorer Pin For Rigid Dynamic analyses, Simplorer Pins are used to define/describe interface points between a Simplorer model and the joints of the Rigid Dynamics model. New Comment Adds a comment within the currently highlighted outline branch. New Figure Captures any graphic displayed for a particular object in the Geometry window. New Image Adds an image within the currently highlighted outline branch. Image from File Imports an existing graphics image. Image to File Saves the current graphics image to a file (.png, .jpg, .tif, .bmp, .eps). Show/Hide Worksheet Window Enables Worksheet window to be displayed for specific objects. Selection Information Activates the Selection Information Window. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Graphics Toolbar The Graphics Toolbar sets the selection/manipulation mode for the cursor in the graphics window. The toolbar also provides commands for modifying a selection or for modifying the viewpoint. Each icon button and its description follows: Icon Button Tool Tip Name Displayed Description Label Allows you to move and place the label of a load anywhere along the feature that the load is currently scoped to. Direction Chooses a direction by selecting either a single face, two vertices, or a single edge (enabled only when Direction field in the Details view has focus). See Pointer Modes. Coordinates (Active only if you are setting a location, for example, a local coordinate system.) Enables the exterior coordinates of the model to display adjacent to the cursor and updates the coordinate display as the cursor is moved across the model. If you click with the cursor on the model, a label displays the coordinates of that location.This feature is functional on faces only. It is not functional on edges or line bodies. Select Type • Select Geometry: This option allows you to select geometric entities (bodies, faces, edges, and vertices). • Select Mesh: This option allows you to select nodes or a group of nodes. See the Specifying Named Selections by Node-Based Meshing Entities section of the Help for specific creation steps. Nodes must be scoped as a Named Selection. Select Mode Defines how geometry or node selections are made: • Single Select • Box Select • Box Volume Select • Lasso Select • Lasso Volume Select These options are used in conjunction with the selection filters (Vertex, Edge, Face, Body) Vertex Designates vertices only for picking or viewing selection. Edge Designates edges only for picking or viewing selection. Face Designates faces only for picking or viewing selection. Body Designates bodies only for picking or viewing selection. Extend Selection Adds adjacent faces (or edges) within angle tolerance, to the currently selected face (or edge) set, or adds tangent faces (or edges) within angle tolerance, to the currently selected face (or edge) set. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 285 Basics Icon Button Tool Tip Name Displayed Description Rotate Activates rotational controls based on the positioning of the mouse cursor. Pan Moves display model in the direction of the mouse cursor. Zoom Displays a closer view of the body by dragging the mouse cursor vertically toward the top of the graphics window, or displays a more distant view of the body by dragging the mouse cursor vertically toward the bottom of the graphics window. Box Zoom Displays selected area of a model in a box that you define. Fit Fits the entire model in the graphics window. Toggle Magnifier Window On/Off Displays a Magnifier Window, which is a shaded box that functions as a magnifying glass, enabling you to zoom in on portions of the model. When you toggle the Magnifier Window on, you can: • Pan the Magnifier Window across the model by holding down the left mouse button and dragging the mouse. • Increase the zoom of the Magnifier Window by adjusting the mouse wheel, or by holding down the middle mouse button and dragging the mouse upward. • Recenter or resize the Magnifier Window using a right mouse button click and choosing an option from the context menu. Recenter the window by choosing Reset Magnifier. Resizing options include Small Magnifier, Medium Magnifier, and Large Magnifier for preset sizes, and Dynamic Magnifier Size On/Off for gradual size control accomplished by adjusting the mouse wheel. Standard model zooming, rotating, and picking are disabled when you use the Magnifier Window. 286 Previous View To return to the last view displayed in the graphics window, click the Previous View button on the toolbar. By continuously clicking you can see the previous views in consecutive order. Next View After displaying previous views in the graphics window, click the Next View button on the toolbar to scroll forward to the original view. Set (ISO) The Set ISO button allows you to set the isometric view.You can define a custom isometric viewpoint based on the current viewpoint (arbitrary rotation), or define the "up" direction so that geometry appears upright. Look at Centers the display on the currently selected face or plane. Rescale Annotation Adjusts the size of annotation symbols, such as load direction arrows. Viewports Splits the graphics display into a maximum of four simultaneous views. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Keyboard Support The same functionality is available via your keyboard provided the NumLock key is enabled. The numbers correlate to the following functionality: 0 = View Isometric 1 = +Z Front 2 = -Y Bottom 3 =+X Right 4 = Previous View 5 = Default Isometric 6 = Next View 7 = -X Left 8 = +Y Top 9 = -Z Back . (dot) = Set Isometric Context Toolbar The Context Toolbar configures its buttons based on the type of object selected in the Tree Outline (p. 235). The Context Toolbar makes a limited number of relevant choices more visible and readily accessible. Context Toolbars include: • Model Context Toolbar (p. 288) • Geometry Context Toolbar (p. 289) • Virtual Topology Context Toolbar (p. 289) • Symmetry Context Toolbar (p. 290) • Connections Context Toolbar (p. 290) • Coordinate Systems Context Toolbar • Meshing Context Toolbar (p. 291) • Gap Tool Context Toolbar (p. 291) • Environment Context Toolbar (p. 291) • Solution Context Toolbar (p. 291) • Vector Display Context Toolbar Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 287 Basics • Result Context Toolbar (p. 291) • Capped Isosurface Context Toolbar • Comment Context Toolbar (p. 297) • Print Preview Context Toolbar (p. 297) • Report Preview Context Toolbar (p. 297) Note • Some Context Toolbar items, such as Connections or Mesh Controls, can be hidden. • The Context Toolbar cannot be hidden (for simplicity and to avoid jumbling the screen). The toolbar appears blank when no options are relevant. • The toolbar displays a text label for the current set of options. • A Workbench Options dialog box setting turns off button text labels to minimize context toolbar width. Model Context Toolbar The Model Context toolbar becomes active when a Model is selected in the tree. The Model Context toolbar contains options for creating objects related to the model, as described below. Construction Geometry See Path (Construction Geometry) (p. 376) and Surface (Construction Geometry) (p. 381) for details. Virtual Topology You can use the Virtual Topology option to reduce the number of elements in a model by merging faces and lines. This is particularly helpful when small faces and lines are involved. The merging will impact meshing and selection for loads and supports. See Virtual Topology Overview for details. Symmetry For symmetric bodies, you can remove the redundant portions based on the inherent symmetry, and replace them with symmetry planes. Boundary conditions are automatically included based on the type of analyses. Remote Point See Remote Point (p. 381) for details. Connections The Connections button is available only if a connection object is not already in the tree (such as a model that is not an assembly), and you wish to create a connections object. Connection objects include contact regions, joints, and springs. You can transfer structural loads and heat flows across the contact boundaries and “connect” the various parts. See the Contact section for details. 288 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface A joint typically serves as a junction where bodies are joined together. Joint types are characterized by their rotational and translational degrees of freedom as being fixed or free. See the Joints section for details. You can define a spring (longitudinal or torsional) to connect two bodies together or to connect a body to ground. See the Springs section for details. Mesh Numbering The Mesh Numbering feature allows you to renumber the node and element numbers of a generated meshed model consisting of flexible parts. See the Mesh Numbering (p. 374) section for details. Solution Combination Use the Solution Combination option to combine multiple environments and solutions to form a new solution. A solution combination folder can be used to linearly combine the results from an arbitrary number of load cases (environments). Note that the analysis environments must be static structural with no solution convergence. Results such as stress, elastic strain, displacement, contact, and fatigue may be requested. To add a load case to the solution combination folder, right click on the worksheet view of the solution combination folder, choose add, and then select the scale factor and the environment name. An environment may be added more than once and its effects will be cumulative. You may suppress the effect of a load case by using the check box in the worksheet view or by deleting it through a right click. For more information, see Solution Combinations (p. 750). Named Selection You can create named selections to specify and control like-grouped items such as types of geometry. For more information, see Named Selections (p. 354). Geometry Context Toolbar The Geometry Context toolbar is active when you select the Geometry branch in the tree or any items within the Geometry branch. If you are using an assembly meshing algorithm, you can use the Geometry toolbar to insert a virtual body. Using the Geometry toolbar you can also apply a Point Mass or a Thermal Point Mass. You can also add a Commands object to individual bodies. For surface bodies, you can add a Thickness object or an Imported Thickness object to define variable thickness, or Layered Section objects to define layers applied to surfaces. Construction Geometry See Path (Construction Geometry) (p. 376) and Surface (Construction Geometry) (p. 381) for details. Virtual Topology Context Toolbar The Virtual Topology Context toolbar includes the following controls: • Merge Cells button: For creating Virtual Cell objects in which you can group faces or edges. • Split Edge at + and Split Edge buttons: For creating Virtual Split Edge objects, which allow you to split an edge to create two virtual edges. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 289 Basics • Split Face at Vertices button: For creating Virtual Split Face objects, which allow you to split a face along two vertices to create 1 to N virtual faces. The selected vertices must be located on the face that you want to split. • Hard Vertex at + button: For creating Virtual Hard Vertex objects, which allow you to define a hard point according to your cursor location on a face, and then use that hard point in a split face operation. • and buttons: For cycling through virtual topology entities in the sequence in which they were created. If any virtual topologies are deleted or merged, the sequence is adjusted automatically. See Cycling Through Virtual Entities in the Geometry Window. • Edit button: For editing virtual topology entities. • Delete button: For deleting selected virtual topology entities, along with any dependents if applicable. Symmetry Context Toolbar The Symmetry Context toolbar includes an option to insert Symmetry Region, Periodic Region, or Cyclic Region objects where you can define symmetry planes. Connections Context Toolbar The Connections context toolbar includes the following settings and functions: • Connection Group button: Inserts a Connection Group object. • Contact drop down menu: Inserts one of the following: a manual Contact Region object set to a specific contact type, a Contact Tool object (for evaluating initial contact conditions), or a Solution Information object. • Spot Weld button: Inserts a Spot Weld object. • Mesh Connection button: Inserts a Mesh Connection object. • End Release button: Inserts an End Release object. • Body Interactions See Body Interactions in Explicit Dynamics Analyses (p. 487) for details. • Body-Ground drop-down menu: Inserts a type of Joint object, Spring object, or a Beam object, whose reference side is fixed. • Body-Body drop-down menu: Inserts a type of Joint object, Spring object, or a Beam object, where neither side is fixed. • Body Views toggle button: For joints, Mesh Connections, and Contacts, displays parts and connections in separate auxiliary windows. • Sync Views toggle button: When the Body Views button is engaged, any manipulation of the model in the Geometry window will also be reflected in both auxiliary windows. • Configure, Set, and Revert buttons; and ∆ = field: Graphically configures the initial positioning of a joint. Refer to Example: Configuring Joints (p. 458) for details. • Assemble button: For joints, performs the assembly of the model, finding the closest part configuration that satisfies all the joints. • Commands icon button: Inserts a Commands object. 290 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Meshing Context Toolbar The Meshing Context toolbar includes the following controls: • Update button - for updating a cell that references the current mesh. This will include mesh generation as well as generating any required outputs. • Mesh drop down menu - for implementing meshing ease of use features. • Mesh Control drop down menu - for adding Mesh Controls to your model. • Metric Graph button - for hiding and showing the Mesh Metrics bar graph. Gap Tool Context Toolbar The Gap Tool Context toolbar is used to have the Mechanical application search for face pairs within a specified gap distance that you specify. Environment Context Toolbar The Environment Context toolbar allows you to apply loads to your model. The toolbar display varies depending on the type of simulation you choose. For example, the toolbar for a Static Structural analysis is shown below. Solution Context Toolbar The Solution toolbar applies to Solution level objects that either: • Never display contoured results (such as the Solution object), or • Have not yet been solved (no contours to display). The options displayed on this toolbar are based on the type of analysis that is selected. The example shown below displays the solution options for a static structural analysis. Objects created via the Solution toolbar are automatically selected in the Outline. Prior to a solution this toolbar always remains in place (no contours to display). A table in the Applying Results Based on Geometry (p. 719) section indicates which bodies can be represented by the various choices available in the drop-down menus of the Solution toolbar. Inserting some other tools changes the solution context toolbar to other toolbars (e.g., Solution Information). Result Context Toolbar Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 291 Basics The Result toolbar applies to Solution level objects that display contour or vector results. Scaling Deformed Shape For results with an associated deformed shape, the Scaling combo box provides control over the onscreen scaling: Scale factors precede the descriptions in parentheses in the list. The scale factors shown above apply to a particular model's deformation and are intended only as an example. Scale factors vary depending on the amount of deformation in the model. You can choose a preset option from the list or you can type a customized scale factor relative to the scale factors in the list. For example, based on the preset list shown above, typing a customized scale factor of 0.6 would equate to approximately 3 times the Auto Scale factor. • Undeformed does not change the shape of the part or assembly. • True Scale is the actual scale. • Auto Scale scales the deformation so that it's visible but not distorting. • The remaining options provide a wide range of scaling. The system maintains the selected option as a global setting like other options in the Result toolbar. As with other presentation settings, figures override the selection. For results that are not scaled, the combo box has no effect. Note Most of the time, a scale factor will be program chosen to create a deformed shape that will show a visible deflection to allow you to better observe the nature of the results. However, under certain conditions, the True Scale displaced shape (scale factor = 1) is more appropriate and is therefore the default if any of the following conditions are true: • Rigid bodies exist. • A user-defined spring exists in the model. • Large deflection is on. This applies to all analyses except for modal and linear buckling analyses (in which case True Scale has no meaning). Relative Scaling The combo list provides five "relative" scaling options. These options scale deformation automatically relative to preset criteria: • 292 Undeformed Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface • True Scale • 0.5x Auto • Auto Scale • 2x Auto • 5x Auto Geometry You can observe different views from the Geometry drop-down menu. • Exterior This view displays the exterior results of the selected geometry. • IsoSurfaces This view displays the interior only of the model at the transition point between values in the legend, as indicated by the color bands. • Capped IsoSurfaces This view displays contours on the interior and exterior. When you choose Capped IsoSurfaces, a Capped Isosurface toolbar appears beneath the Result context toolbar. Refer to Capped Isosurfaces for a description of the controls included in the toolbar. • Slice Planes This view displays planes cutting through the result geometry; only previously drawn slice planes are visible. The model image changes to a wireframe representation. Contours Options To change the way you view your results, click any of the options on this toolbar. • Smooth This view displays gradual distinction of colors. • Contour This view displays the distinct differentiation of colors. • Isolines Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 293 Basics This view displays a line at the transition between values. • Solid This view displays the model only with no contour markings. Edges Options You can switch to wireframe mode to see gaps in surface body models. Red lines indicate shared edges. In addition, you can choose to view wireframe edges, include the deformed model against the undeformed model, or view elements. Showing a subdued view of the undeformed model along with the deformed view is especially useful if you want to view results on the interior of a body yet still want to view the rest of the body's shape as a reference. An example is shown here. The Show Undeformed Model option is useful when viewing any of the options in the Geometry dropdown menu. • No Wireframe This view displays a basic picture of the body. • Show Undeformed Wireframe This view shows the body outline before deformation occurred. If the New Section Plane (p. 271) feature is active, choosing Show Undeformed WireFrame actually displays the wireframe with the deformations added to the nodes. This is intended to help you interpret the image when you drag the section plane anchor across smaller portions of the model. • Show Undeformed Model This view shows the deformed body with contours, with the undeformed body in translucent form. • 294 Show Elements Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface This view displays element outlines. Vector Display Context Toolbar Using the Graphics button, you can display results as vectors with various options for controlling the display. • Click the Graphics button on the Result context toolbar to convert the result display from contours (default) to vectors. • When in vector display, a Vector Display toolbar appears with controls as described below. Displays vector length proportional to the magnitude of the result. Displays a uniform vector length, useful for identifying vector paths. Controls the relative length of the vectors in incremental steps from 1 to 10 (default = 5), as displayed in the tool tip when you drag the mouse cursor on the slider handle. Displays all vectors, aligned with each element. Displays vectors, aligned on an approximate grid. Controls the relative size of the grid, which determines the quantity (density) of the vectors.The control is in uniform steps from 0 [coarse] to 100 [fine] (default = 20), as displayed in the tool tip when you drag the mouse cursor on the slider handle. Note This slider control is active only when the adjacent button is chosen for displaying vectors that are aligned with a grid. Displays vector arrows in line form. Displays vector arrows in solid form. • When in vector display, click the Graphics button on the Result context toolbar to change the result display back to contours. The Vector Display toolbar is removed. Presented below are examples of vector result displays. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 295 Basics Uniform vector lengths identify paths using vector arrows in line form. Course grid size with vector arrows in solid form. Same using wireframe edge option. Uniform vector lengths , grid display on slice plane with vector arrows in solid form. 296 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Zoomed-in uniform vector lengths , grid display with arrow scaling and vector arrows in solid form. Max, Min, and Probe Annotations Toolbar buttons allow for toggling Max and Min annotations and for creating probe annotations. See also Annotations (p. 396). Comment Context Toolbar When you select the Comment button in the standard toolbar or when you select a Comment object already in the tree, the Comment Context toolbar and Comment Editor appear. The buttons at the top allow you to insert an image or apply various text formatting. To insert an image, click the button whose tool tip is Insert Image, then complete the information that appears in the dialog box . For the Image URL, you can use a local machine reference (C:\...) or a web reference (http:\\...). Print Preview Context Toolbar The Print Preview toolbar allows you to print the currently-displayed image, or send it to an e-mail recipient or to a Microsoft Word or PowerPoint file. Report Preview Context Toolbar The Report Preview toolbar allows you to send the report to an e-mail recipient or to a Microsoft Word or PowerPoint file, print the report, save it to a file, or adjust the font size. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 297 Basics Named Selection Toolbar Named Selections enable you to specify and control like-grouped geometry items. See the Named Selections (p. 354) section for details. Unit Conversion Toolbar The Unit Conversion toolbar is a built-in conversion calculator. It allows conversion between consistent unit systems. The Units menu sets the active unit system. The status bar shows the current unit system. The units listed in the toolbar and in the Details view are in the proper form (i.e. no parenthesis). The Unit Conversions toolbar is hidden by default. To see it, select View> Toolbars> Unit Conversion. Graphics Options Toolbar The Graphics Options toolbar provides quick access to features that are generally useful for controlling the graphics display of models. These features are also included under View> Graphics Options. See Assemblies of Surface Bodies (p. 320) for details. The Graphics Options toolbar is displayed by default, but can be hidden using View> Toolbars> Graphics Options. Icon Button Tool Tip Name Displayed Description Toggle Show Vertices On or Off Enabling the Show Vertices button highlights all vertices on the model.This feature is especially useful when examining complex assemblies where vertices might normally be hidden from view. It can also be used to ensure that edges are complete and not segmented unintentionally. Wireframe Mode On or Off Enabling the Wireframe button displays the model in the Geometry window with distinct edges only (recommended for seeing gaps in surface bodies). Edge Coloring By Body Color: Displays body colors to represent boundary edges. By Connection: Displays five different colors corresponding to five different categories of connectivity.The categories are: free (blue), single (red), double (black), triple (pink) and multiple (yellow). Free means that the edge is not shared by any faces. Single means that the edge is shared by one face and so on.The color 298 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Icon Button Tool Tip Name Displayed Description scheme is also displayed in the Edge/Face Connectivity legend. Black:Turns off the edge/face connectivity display.The entire model is displayed in black. Free Hide Free: Hides only edges not shared by any faces. Show Free: Displays only edges not shared by any faces. Thick Free: Displays only edges not shared by any faces at a different edge thickness compared to the rest of the model. Single Hide Single: Hides only edges that are shared by one face. Show Single: Displays only that are shared by one face. Thick Single: Displays only edges that are shared by one face at a different edge thickness compared to the rest of the model. Double Hide Double: Hides only edges that are shared by two faces. Show Double: Displays only that are shared by two faces. Thick Double: Displays only edges that are shared by two faces at a different edge thickness compared to the rest of the model. Triple Hide Triple: Hides only edges that are shared by three faces. Show Triple: Displays only that are shared by three faces. Thick Triple: Displays only edges that are shared by three faces at a different edge thickness compared to the rest of the model. Multiple Hide Multiple: Hides only edges that are shared by more than three faces. Show Multiple: Displays only that are shared by more than three faces. Thick Multiple: Displays only edges that are shared by more than three faces at a different edge thickness compared to the rest of the model. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 299 Basics Icon Button Tool Tip Name Displayed Description Edge Direction Displays model edge directions. The direction arrow appears at the midpoint of the edge. The size of the arrow is proportional to the edge length. Edges Joined by Mesh Connection Display the edges using coloring schema, by taking into account the mesh connection information. Thicken annotations scoped to lines For annotations scoped to lines (for example, annotations representing loads, named selections, point masses, and so on), enabling this button thickens these lines so they are more easily identifiable on the screen. Show Mesh Enabling the Show Mesh button displays the model’s mesh regardless of the selected tree object. When enabled, to make sure that Annotations display properly, also turn on Wireframe mode. See Note below. Show Coordinate Systems Enabling the Show Coordinate Systems button displays all available coordinate systems associated with the model – default as well as user defined. Note The following restrictions apply when using the Graphics Options functions on the mesh, as compared to their use on geometry: 300 • Not all the buttons / options are functional, for example, Double always displays thin black lines. The width of the colored lines cannot be changed. They are always thick. • During slicing, the colors of shared element edges are not drawn. They display as black and appear only when the selected slice plane is losing focus in the slice tool pane. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. The Mechanical Application Interface Note As illustrated below, annotations may not always display properly when the Show Mesh button is activated. Turning on Wireframe mode accurately displays Annotations when Show Mesh is selected. Print Preview Print Preview runs a script to generate an HTML page and image. The purpose of the Print Preview tab is to allow you to view your results or graphics image. The title block is an editable HTML table. The table initially contains the Author, Subject, Prepared For and Date information supplied from the details view of the Project tree node. To change or add this information, double click inside the table. The information entered in the table does not propagate any changes back to the details view and is not saved after exiting the Print Preview tab. The image is generated in the same way as figures in Report. Triad and Rotation Cursors The triad and rotation cursors allow you to control the viewing orientation as described below. Triad Rotation Cursors • Located in lower right corner. • Visualizes the world coordinate system directions. • Positive directions arrows are labeled and color-coded. Negative direction arrows display only when you hover the mouse cursor over the particular region. • Clicking an arrow animates the view such that the arrow points out of the screen. • Arrows and the isometric sphere highlight when you point at them. • Isometric sphere visualizes the location of the isometric view relative to the current view. • Clicking the sphere animates the view to isometric. Click the Rotate button to display and activate the following rotation cursors: • Free rotation. • Rotation around an axis that points out of the screen (roll). • Rotation around a vertical axis relative to the screen ("yaw" axis). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 301 Basics • Rotation around a horizontal axis relative to the screen ("pitch" axis). Cursor Location Determines Rotation Behavior The type of rotation depends on the starting location of the cursor. In general, if the cursor is near the center of the graphics window, the familiar 3D free rotation occurs. If the cursor is near a corner or edge, a constrained rotation occurs: pitch, yaw or roll. Specifically, the circular free rotation area fits the window. Narrow strips along the edges support pitch and yaw. Corner areas support roll. The following figure illustrates these regions. Exporting Data Export Tabular Data Most of the loads and results in the Mechanical application are supported through the Graph and Tabular data windows. You can export the data in the Tabular Data window in a Text and Excel File Format. To export the data in the table, right-click the table, and then select Export. The right-click menu also provides copy and paste features for this same purpose. Export Model Information You can also export a variety of model information to a tab delimited file that Excel can read directly. The data will appear in Excel if it’s currently running, or will be written to a file for later processing. The following objects allow exporting without access to worksheet data: Contour Results Nodal Based Named Selections Imported Loads The following objects require the worksheet data to be active in order to export: Connections Contact Group Contact Initial Information Contact Tool Convergence 302 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Customizing the Mechanical Application Coordinate Systems Fatigue Sensitivities Frequency Response Geometry Mesh Solution Thermal Condition Note When you select Top/Bottom as the Shell setting in the Details view for a surface body and export the result contours (such as stresses and strains), the export file contains two results for every node on a shell element. The first result is for the bottom face and the second result is for the top face. Steps to export 1. Select an object in the tree. 2. Click the Worksheet to give it focus (if applicable). 3. Right-mouse click the selected object in the tree to produce the menu, then select Export. 4. Specify a filename for the Excel file. Note You must right-mouse click on the selected object in the tree to use this Export feature. On Windows platforms, if you have the Microsoft Office 2002 (or later) installed, you may see an Export to Excel option if you right-mouse click in the Worksheet. This is not the Mechanical application Export feature but rather an option generated by Microsoft Internet Explorer. Options Settings The Export the Mechanical application settings in the Options dialog box allows you to: Automatically Open Excel (Yes by default) Include Node Numbers (Yes by default) Include Node Location (No by default) Customizing the Mechanical Application The Mechanical Application Options (p. 303) Variables (p. 313) Macros (p. 313) The Mechanical Application Options You can control the behavior of functions in the Mechanical application through the Options dialog box. To access the Mechanical application options: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 303 Basics 1. From the main menu, choose Tools> Options. An Options dialog box appears and the Mechanical application options are displayed on the left. 2. Click on a specific option. 3. Change any of the option settings by clicking directly in the option field on the right. You will first see a visual indication for the kind of interaction required in the field (examples are drop-down menus, secondary dialog boxes, direct text entries). 4. Click OK. Note • If you enter a number with the thousand separator (in English, the thousand separator is a comma [,]), you will be asked to confirm the entry before it is accepted. For example, if you enter “2,300”, you receive a message stating the following: “Entered value is 2,300. Do you want to accept the correction proposed below? 2300 To accept the correction, please click Yes. To close this message and correct the number yourself, please click No.” • Option settings within a particular language are independent of option settings in another language. If you change any options from their default settings, then start a new Workbench session in a different language, the changes you made in the original language session are not reflected in the new session. You are advised to make the same option changes in the new language session. The following Common Settings option appears in the Options dialog box: Geometry Import The Geometry Import category includes the following: • Compare Parts on Update: When you choose the Refresh Geometry context menu option (right-click on the Geometry tree object or anywhere in the Geometry window), if no changes to the body are detected, then the body is not re-meshed. Note A change that you make to the Compare Parts on Update option in one application is not seen by other applications that are running. For example, if you change this option from within Mechanical or Meshing, and DesignModeler is running, the option change is not seen in DesignModeler. Note The Compare Parts on Update feature is not supported for line bodies. The following Mechanical application options appear in the Options dialog box: 304 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Customizing the Mechanical Application Connections Convergence Export Fatigue Frequency Geometry Graphics Miscellaneous Report Analysis Settings and Solution Visibility Wizard Connections The Auto Detection category allows you to change the default values in the Details view for the following: • Tolerance: Sets the default for the contact detection slider; i.e., the relative distance to search for contact between parts. The higher the number, the tighter the tolerance. In general, creating contacts at a tolerance of 100 finds less contact surfaces than at 0. The default is 0. The range is from -100 to +100. • Face/Face: Sets the default preference1 for automatic contact detection between faces of different parts. The choices are Yes or No. The default is Yes. • Face/Edge: Sets the default preference1 for automatic contact detection between faces and edges of different parts. The choices are: – Yes – No (default) – Only Solid Body Edges – Only Surface Body Edges • Edge/Edge: Sets the default preference1 for automatic contact detection between edges of different parts. The choices are Yes or No. The default is No. • Priority: Sets the default preference1 for the types of contact interaction priority between a given set of parts. The choices are: – Include All (default) – Face Overrides – Edge Overrides • Revolute Joints: Sets the default preference for automatic joint creation of revolute joints. The choices are Yes and No. The default is Yes. • Fixed Joints: Sets the default preference for automatic joint creation of fixed joints. The choices are Yes and No. The default is Yes. 1 Unless changed here in the Options dialog box, the preference remains persistent when starting any Workbench project. The Transparency category includes the following exclusive controls for this category. There are no counterpart settings in the Details view. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 305 Basics • Parts With Contact: Sets transparency of parts in selected contact region so the parts are highlighted. The default is 0.8. The range is from 0 to 1. • Parts Without Contact: Sets transparency of parts in non-selected contact regions so the parts are not highlighted. The default is 0.1. The range is from 0 to 1. The Default category allows you to change the default values in the Details view for the following: • • • • • Type: Sets the definition type of contact. The choices are: – Bonded (default) – No Separation – Frictionless – Rough – Frictional Behavior: Sets the contact pair. The choices are: – Program Controlled (default) – Asymmetric – Symmetric – Auto Asymmetric Formulation: Sets the type of contact formulation method. The choices are: – Program Controlled (default) – Augmented Lagrange – Pure Penalty – MPC – Normal Lagrange Update Stiffness: Enables an automatic contact stiffness update by the program. The choices are: – Program Controlled (default) – Never – Each Iteration – Each Iteration, Aggressive Auto Rename Connections: Automatically renames joint, spring, contact region, and joint condition objects when Type or Scoping are changed. The choices are Yes and No. The default is Yes. Convergence The Convergence category allows you to change the default values in the Details view for the following: • Target Change: Change of result from one adapted solution to the next. The default is 20. The range is from 0 to 100. • Allowable Change: This should be set if the criteria is the max or min of the result. The default is Max. The Solution category allows you to change the default values in the Details view for the following: • Max Refinement Loops: Allows you to change the number of loops . The default is 1. The range is from 1 to 10. 306 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Customizing the Mechanical Application Export The Export category includes the following exclusive controls for this category. There are no counterpart settings in the Details view. • Automatically Open Excel: Excel will automatically open with exported data. The default is Yes. • Include Node Numbers: Nodal numbers will be included in exported file. The default is Yes. • Include Node Location: Nodal location can be included in exported file. The default is No. Fatigue The General category allows you to change the default values in the Details view for the following: • Design Life: Number of cycles that indicate the design life for use in fatigue calculations. The default is 1e9. • Analysis Type: The default fatigue method for handling mean stress effects. The choices are: – SN - None (default) – SN - Goodman – SN - Soderberg – SN - Gerber – SN - Mean Stress Curves The Goodman, Soderberg, and Gerber options use static material properties along with S-N data to account for any mean stress while Mean-Stress Curves use experimental fatigue data to account for mean stress. The Cycle Counting category allows you to change the default values in the Details view for the following: • Bin Size: The bin size used for rainflow cycle counting. A value of 32 means to use a rainflow matrix of size 32 X 32. The default is 32. The range is from 10 to 200. The Sensitivity category allows you to change the default values in the Details view for the following: • Lower Variation: The default value for the percentage of the lower bound that the base loading will be varied for the sensitivity analysis. The default is 50. • Upper Variation: The default value for the percentage of the upper bound that the base loading will be varied for the sensitivity analysis. The default is 150. • Number of Fill Points: The default number of points plotted on the sensitivity curve. The default is 25. The range is from 10 to 100. • Sensitivity For: The default fatigue result type for which sensitivity is found. The choices are: – Life (default) – Damage – Factor of Safety Frequency The Frequency category allows you to change the default values in the Details view for the following: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 307 Basics • Max Number of Modes: The number of modes that a newly created frequency branch will contain. The default is 6. The range is from 1 to 200. • Limit Search to Range: You can specify if a frequency search range should be considered in computing frequencies. The default is No. • Min Range: Lower limit of search range. The default is 0. • Max Range: Upper limit of search range. The default is 100000000. • Cyclic Phase Number of Steps: The number of intervals to divide the cyclic phase range (0 - 360 degrees) for frequency couplet results in cyclic modal analyses. Geometry The Geometry category allows you to change the default values in the Details view for the following: • Nonlinear Material Effects: Indicates if nonlinear material effects should be included (Yes), or ignored (No). The default is Yes. • Thermal Strain Calculation: Indicates if thermal strain calculations should be included (Yes), or ignored (No). The default is Yes. Note This setting applies only to newly attached models, not to existing models. Graphics The Default Graphics Options category allows you to change the default values in the Details view for the following: • Show Min Annotation: Indicates if Min annotation will be displayed by default (for new databases). The default is No. • Show Max Annotation: Indicates if Max annotation will be displayed by default (for new databases). The default is No. • Contour Option: Selects default contour option. The choices are: • • 308 – Smooth Contour – Contour Bands (default) – Isolines – Solid Fill Edge Option: Selects default edge option. The choices are: – No Wireframe (default) – Show Undeformed Wireframe – Show Undeformed Model – Show Elements Highlight Selection: Indicates default face selection. The choices are: – Single Side (default) – Both Sides Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Customizing the Mechanical Application • Number of Circular Cross Section Divisions: Indicates the number of divisions to be used for viewing line body cross sections for circular and circular tube cross sections. The range is adjustable from 6 to 360. The default is 16. • Allow Section Plane Editing: Enables or disables the editing capability of the New Section Plane feature. The default value of the option is Yes (enabled). Miscellaneous The Miscellaneous category allows you to change the default values in the Details view for the following: • Load Orientation Type: Specifies the orientation input method for certain loads. This input appears in the Define By option in the Details view of the load, under Definition. – Vector (default) – Component The Image category includes the following exclusive controls for this category. There are no counterpart settings in the Details view. • Image Transfer Type: Defines the type of image file created when you send an image to Microsoft Word or PowerPoint, or when you select Print Preview. The choices are: – PNG (default) – JPEG – BMP The Post Processing (MAPDL Only) category includes the following controls for results files written by the Mechanical APDL solver: • Result File Caching: By holding substantial portions of a file in memory, caching reduces the amount of I/O associated with result file reading. The cache can, however, reduce memory that would otherwise be used for other solutions. The choices are: – System Controlled (default): The operating system determines whether or not the result file is cached for reading. – Off: There is no caching during the reading of the result file. – Programmed Controlled: The Mechanical application determines whether or not the result file is cached for reading. The Ansoft Executable Locations category includes the following controls where you define file locations for the following: • HFSS: • Maxwell: • Q3D Extractor: The Save Options category includes the following controls for this category. • Save Project Before Solution: Sets the Yes / No default for the Save Project Before Solution setting located in the Project Details panel. Although you can set the default here, the solver respects the latest Save Project Before Solution setting in the Details panel. The default for this option is No. Selecting Yes saves the entire project immediately before solving (after any required meshing). If the project had never been previously saved, you can now select a location to save a new file. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 309 Basics • Save Project After Solution: Sets the Yes / No default for the Save Project After Solution setting in the Project Details panel . The default for this option is No Selecting Yes Saves the project immediately after solving but before postprocessing. If the project had never been previously saved, nothing will be saved. Note The save options you specify on the Project Details panel override the options specified in the Options dialog box and will be used for the current project. Report The Figure Dimensions (in Pixels) category includes the following controls that allow you to make changes to the resolution of the report for printing purposes. • Chart Width - Default value equals 600 pixels. • Chart Height - Default value equals 400 pixels. • Graphics Width - Default value equals 600 pixels. • Graphics Height - Default value equals 500 pixels. • Graphics Resolution - Resolution values include: – Optimal Onscreen Display (1:1) – Enhanced Print Quality (2:1) – High-Resolution Print Quality (4:1) The Customization category includes the following controls: • Maximum Number of Table Columns - (default = 6 columns) Changes the number of columns used when a table is created. • Merge Identical Table Cells - Merges cells that contain identical values. The default value is Yes. • Omit Part and Joint Coordinate System Tables - Chooses whether to include or exclude Coordinate System data within the report. This data can sometimes be cumbersome. The default value is Yes. • Include Figures - Specifies whether to include Figure objects as pictures in the report. You may not want to include figures in the report when large solved models or models with a mesh that includes many nodes and elements are involved. In these cases, figure generation can be slow, which could significantly slow down report generation. The default value is Yes. Note This option applies only to Figure objects as pictures. Graph pictures, Engineering Data graphs, and result graphs (such as phase response in a harmonic analysis) are not affected and will appear regardless of this option setting. • 310 Custom Report Generator Folder - Reports can be run outside of the Workbench installation directory by copying the Workbench Report2006 folder to a new location. Specify the new folder location in this field. Please see the Customize Report Content section for more information. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Customizing the Mechanical Application Analysis Settings and Solution The Solver Controls category allows you to change the default values in the Details view for the following: • • Solver Type: Specifies which ANSYS solver will be used. The choices are: – Program Controlled (default) – Direct – Iterative Use Weak Springs: Specifies whether weak springs are added to the model. The Programmed Controlled setting automatically allows weak springs to be added if an unconstrained model is detected, if unstable contact exists, or if compression only supports are active. The choices are:. – Program Controlled (default) – On – Off The Output Controls category allows you to change the default values in the Details view for the following: • Stress (Default setting = Yes) • Strain (Default setting = Yes) • Calculate Thermal Flux (Default setting = No) • Nodal Forces (Default setting = No) • Contact Miscellaneous (Default setting = No) • General Miscellaneous (Default setting = No) • Calculate Reactions (Default setting = Yes) • Calculate Thermal Flux (Default setting = Yes) • Max Number of Result Sets (Default setting = 0) Note The default value (0) for the Max Number of Result Sets option displays as "Program Controlled" in the Output Controls category of the GUI. The Output Control (Modal) category allows you to change the default value in the Details for the Store Modal Results option. The default setting is Program Controlled. The Restart Controls category allows you to change the default value in the Details view for the following: • Retain Restart Files: When restart points are requested, the necessary restart files are always retained for an incomplete solve due to a convergence failure or user request. However, when the solve completes successfully, you have the option to request to either keep the restart points by setting this field to Yes, or to delete them by setting this field to No. You can control this setting in the Details view of the Analysis Settings object under Restart Controls (p. 535), or here under Tools> Options in the Analysis Settings and Solution preferences list. The setting in the Details view overrides the preference setting. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 311 Basics The Solution Information category allows you to change the default value in the Details view for the following: • Refresh Time: Specifies how often any of the result tracking items under a Solution Information object get updated while a solution is in progress. The default is 2.5 s. The Solution Settings category allows you to set the default value in the Details view for the following: • Results Availability: Specifies what results to allow under the Solution object in Design Assessment systems when the Solution Selection object allows combinations. The default is Filter Combination Results. The Analysis Data Management category allows you to set the default value in the Details view for the Save MAPDL db control. Values are No (default) or Yes. The setting of the Future Analysis control (see Analysis Data Management Help section) can sometimes require the db file to be written. In this case, the Save MAPDL db control is automatically set to Yes. Visibility The Visibility category includes the following exclusive controls for this category. There are no counterpart settings in the Details view. • Mesh Folder: Indicates if mesh folder should appear in the Tree Outline. You may not want to see or know about meshes. The default is Visible. • Part Mesh Statistics: Indicates if mesh information (the number of nodes and elements) should show in the Details view of a part. The default is Visible. • Fatigue Tool: Turns on/off Fatigue tool capability. The default is Visible. • Contact Tool: Turns on/off Contact Tool capability. The default is Visible. Wizard The Wizard Options category includes the following exclusive controls for this category. There are no counterpart settings in the Details view. • Default Wizard: This is the URL to the XML wizard definition to use by default when a specific wizard isn't manually chosen or automatically specified by a simulation template. The default is StressWizard.xml. • Flash Callouts: Specifies if callouts will flash when they appear during wizard operation. The default is Yes. The Skin category includes the following exclusive controls for this category. There are no counterpart settings in the Details view. • Cascading Style Sheet: This is the URL to the skin (CSS file) used to control the appearance of the Mechanical Wizard. The default is Skins/System.css. The Customization Options category includes the following exclusive controls for this category. There are no counterpart settings in the Details view. • Mechanical Wizard URL: For advanced customization. See Appendix: Workbench Mechanical Wizard Advanced Programming Topics for details. • Enable WDK Tools: Advanced. Enables the Wizard Development Kit. The WDK adds several groups of tools to the Mechanical Wizard. The WDK is intended only for persons interested in creating or modifying 312 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Customizing the Mechanical Application wizard definitions. The default is No. See the Appendix: Workbench Mechanical Wizard Advanced Programming Topics for details. Note • URLs in the Mechanical Wizard follow the same rules as URLs in web pages. • Relative URLs are relative to the location of the Mechanical Wizard URL. • Absolute URLs may access a local file, a UNC path, or use HTTP or FTP. User Preferences File The Mechanical application stores the configuration information from the Options dialog box in a file called a User Preference File on a per user basis. This file is created the first time you start the Mechanical application. Its default location is: C:\Documents and Settings\<user initials>\Application Data\Ansys\v140\enus\dsPreferences.xml Variables Variables provide you the capability to override default settings. To set variables: 1. Choose Variable Manager from the Tools menu. 2. Right-click in the row to add a new variable. 3. Enter a variable name and type in a value. 4. Click OK. Variable name Allowable Values Description DSMESH OUTPUT filename Writes mesher messages to a file during solve (default = no file written). If the value is a filename, the file is written to the temporary working folder (usually c:\temp).To write the file to a specific location, specify the full path. DSMESH DEFEATUREPERCENT a number between 1e-6 and 1e-3 Tolerance used in simplifying geometry (default = .0005). Status The status box indicates if a particular variable is active or not. Checked indicates that the variable is active. Unchecked indicates that the variable is available but not active. This saves you from typing in the variable and removing it. Macros The Mechanical application allows you to execute custom functionality that is not included in a standard Mechanical application menu entry via its Run Macro feature. The functionality is defined in a macro a script that accesses the Mechanical application programming interface (API). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 313 Basics Macros can be written in Microsoft's JScript or VBScript programming languages. Several macro files are provided with the ANSYS Workbench installation under \ANSYS Inc\v140\AISOL\DesignSpace\DSPages\macros. Macros cannot currently be recorded from the Mechanical application. To access a macro from the Mechanical application: 1. Choose Run Macro... from the Tools menu. 2. Navigate to the directory containing the macro. 3. Open the macro. The functionality will then be accessible from the Mechanical application. 314 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Features The following topics are included in this section: Geometry in the Mechanical Application Coordinate Systems Overview Graphics Connections Analysis Settings Applying Boundary Conditions Results in the Mechanical Application Solving Overview Commands Objects Report Preview Meshing in the Mechanical Application Parameters Design Assessment Virtual Topology in the Mechanical Application Geometry in the Mechanical Application The following topics are included in this section: Assemblies, Parts, and Bodies Solid Bodies Surface Bodies Line Bodies Rigid Bodies 2-D Analyses Symmetry Named Selections Mesh Numbering Path (Construction Geometry) Surface (Construction Geometry) Remote Point Point Mass Thermal Point Mass Using Gaskets Assemblies, Parts, and Bodies While there is no limit to the number of parts in an assembly that can be treated, large assemblies may require unusually high computer time and resources to compute a solution. Contact boundaries can be automatically formed where parts meet. The application has the ability to transfer structural loads and heat flows across the contact boundaries and to "connect" the various parts. Parts are a grouping or a collection of bodies. Parts can include multiple bodies and are referred to as multibody parts. The mesh for multibody parts created in DesignModeler will share nodes where the Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 315 Features bodies touch one another, that is, they will have common nodes at the interfaces. This is the primary reason for using multibody parts. Parts may consist of: • One or more solid bodies. • One or more surface bodies. • One or more line bodies. • Combinations of line and surface bodies. All other combinations are not practically supported. Note Body objects in the tree that represent a multibody part do not report centroids or moments of inertia in their respective Details view. The following topics are addressed in this section: Multibody Behavior Working with Parts Integration Schemes Color Coding of Parts Working with Bodies Hide or Suppress Bodies Hide or Show Faces Assumptions and Restrictions for Assemblies, Parts, and Bodies Multibody Behavior Associativity that you apply to geometry attached from DesignModeler is maintained in the Mechanical and Meshing applications when updating the geometry despite any part groupings that you may subsequently change in DesignModeler. See Maintaining Associativity with Geometry Updates in DesignModeler (p. 5) for further information. When transferring multibody parts from DesignModeler to the Meshing application, the multibody part has the body group (part) and the prototypes (bodies) beneath it. When the part consists of just a single body the body group is hidden. If the part has ever been imported as a multibody part you will always see the body group for that component, regardless of the number of bodies present in any subsequent update. Working with Parts There are several useful and important manipulations that can be performed with parts in an assembly. • Each part may be assigned a different material. • Parts can be hidden for easier visibility. • Parts can be suppressed, which effectively eliminates the parts from treatment. • The contact detection tolerance and the contact type between parts can be controlled. • When a model contains a Coordinate Systems object, by default, the part and the associated bodies use the Global Coordinate System to align the elements. If desired, you can apply a local coordinate 316 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application system to the part or body. When a local coordinate system is assigned to a Part, by default, the bodies also assume this coordinate system but you may modify the system on the bodies individually as desired. Integration Schemes Parts can be assigned Full or Reduced integration schemes. The full method is used mainly for purely linear analyses, or when the model has only one layer of elements in each direction. This method does not cause hourglass mode, but can cause volumetric locking in nearly incompressible cases. The reduced method helps to prevent volumetric mesh locking in nearly incompressible cases. However, hourglass mode might propagate in the model if there are not at least two layers of elements in each direction. Color Coding of Parts You can visually identify parts based on a property of that part. For example, if an assembly is made of parts of different materials, you can color the parts based on the material; that is, all structural steel parts have the same color, all aluminum parts have the same color and so on. Select a color via the Display Style field of the Details view when the Geometry branch in the feature Tree is selected. You can specify colors based on: • Body Color (default): Assigns different colors to the bodies within a part. • Part Color: Assigns different colors to different parts. • Material: The part colors are based on the material assignment. For example in a model with five parts where three parts use structural steel and two parts use aluminum, you will see the three structural steel parts in one color and the two aluminum parts in another color. The legend will indicate the color used along with the name of the material. • Nonlinear Material Effects: Indicates if a part includes nonlinear material effects during analysis. If you chose to exclude nonlinear material effects for some parts of a model, then the legend will indicate Linear for these parts and the parts will be colored accordingly. • Stiffness Behavior: Identifies a part as Flexible, Rigid, or Gasket during analysis. Note A maximum of 15 distinct materials can be shown in the legend. If a model has more then 15 materials, coloring by material will not have any effect unless enough parts are hidden or suppressed. You can reset the colors back to the default color scheme by right clicking on the Geometry object in the tree and selecting Reset Body Colors. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 317 Features Example 1 Color by Parts Working with Bodies There are several useful and important manipulations that can be performed with bodies in a part. • Bodies grouped into a part result in connected geometry and shared nodes in a mesh. • Each body may be assigned a different material. • Bodies can be hidden for easier visibility. • Bodies in a part group can be individually suppressed, which effectively eliminates these bodies from treatment. A suppressed body is not included in the statistics of the owning part or in the overall statistics of the model. • Bodies can be assigned Full or Reduced integration schemes, as described above for parts. • When bodies in part groups touch they will share nodes where they touch. This will connect the bodies. If a body in a part group does not touch another body in that part group, it will not share any nodes. It will be free standing. Automatic contact detection is not performed between bodies in a part group. Automatic contact detection is performed only between part groups. • Bodies that are not in a part group can be declared as rigid bodies. • When a model contains a Coordinate Systems object, by default, bodies use the Global Coordinate System. If desired, you can apply a local coordinate system. Hide or Suppress Bodies For a quick way to hide bodies (that is, turn body viewing off ) or suppress bodies (that is, turn body viewing off and remove the bodies from further treatment in the analysis), select the bodies in the tree or in the Geometry window (choose the Body select mode, either from the toolbar or by a right-click in the Geometry window). Then right-click and choose Hide Body or Suppress Body from the context menu. Choose Show Body, Show All Bodies, Unsuppress Body, or Unsuppress All Bodies to reverse the states. The following options are also available: • Hide All Other Bodies, allows you to show only selected bodies. • Suppress All Other Bodies, allows you to unsuppress only selected bodies. 318 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Hide or Show Faces You can hide selected faces on a model such that you are able to see inside the model. This feature is especially useful for bodies with interior cavities, such as engine blocks. To use the feature, first select faces on the model that you want to hide, then right-click anywhere in the Geometry window and choose Hide Face(s) in the context menu. This menu choice is only available if you have already selected faces. Choose Show Hidden Face(s) from the context menu to restore the visibility of faces previously hidden using Hide Face(s). The Show Hidden Face(s) menu choice is only available if there are hidden faces from choosing Hide Face(s). It cannot be used to restore the visibility of faces previously hidden by setting Visible to No in the Details view of a Named Selection object. Note The selected faces will appear hidden only when you view the geometry. The feature is not applicable to mesh displays or result displays. Assumptions and Restrictions for Assemblies, Parts, and Bodies Thermal and shape analysis is not supported for surface bodies or line bodies. In order for multiple bodies inside a part to be properly connected by sharing a node in their mesh the bodies must share a face or edge. If they do not share a face or an edge the bodies will not be connected for the analysis which could lead to rigid body motion. Automatic contact detection will detect contact between bodies within a multibody part. Solid Bodies You can process and solve solid models, including individual parts and assemblies. An arbitrary level of complexity is supported, given sufficient computer time and resources. Surface Bodies You can import surface bodies from an array of sources (see Geometry Preferences). Surface bodies are often generated by applying mid-surface extraction to a pre-existing solid. The operation abstracts away the thickness from the solid and converts it into a separate modeling input of the generated surface. Surface body models may be arranged into parts. Within a part there may be one or more surface bodies; these may even share the part with line bodies. Parts that feature surface bodies may be connected with the help of spot welds and contacts. The following topics are addressed in this section. Assemblies of Surface Bodies Thickness Mode Importing Surface Body Models Importing Surface Body Thickness Surface Body Shell Offsets Specifying Surface Body Thickness Specifying Surface Body Layered Sections Faces With Multiple Thicknesses and Layers Specified Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 319 Features Assemblies of Surface Bodies While preparing an assembly of surface bodies for solution you may find the need to understand and modify the connectivity of the bodies involved. Mechanical offers tools to help you accomplish these tasks. For example, you may: • Confirm whether two surface bodies are topologically connected. This may be especially useful for surface bodies obtained from a mid-surface operation on solids and created artificial gaps in their proximity. • Confirm the connectivity of individual elements in the mesh of the surface bodies. • Mend missing connections between surface bodies by joining their meshes with shared nodes. To confirm the connectivity of surface bodies it is useful to review the connectivity of their edges using a number of features in both Mechanical and DesignModeler. Edges can be classified depending on the number of faces they topologically connect. For example, the boundary edge of a surface body connects to a single face and is classified as a "single edge”, whereas an interior edge connecting two faces of the surface body will be classified as a "double edge". Single and double edges can be distinguished visually using the Graphics Options Toolbar (p. 298). As an alternative, you can create a Named Selection that groups all edges of a given topological connectivity by using the Face Connections criterion. The Graphics Options toolbar can also be used to review the connectivity of not only the geometry, but also the mesh elements. The same principles applied to the connectivity of a surface body edge apply to element edges. Mechanical provides Mesh Connections to mend surface body assemblies at locations that are disjointed. With this feature, the meshes of surface bodies that may reside in different parts can be connected by joining their underlying elements via shared nodes. The Mesh Connection does not alter the geometry although the effect can be conveniently previewed and toggled using the Graphics Options toolbar. Thickness Mode You can determine the source that controls the thickness of a surface body using the Thickness Mode indication combined with the Thickness field, both located in the Details view of a surface Body object. Upon attaching a surface body, the Thickness Mode reads either Auto or Manual. • In Auto Mode the value of thickness for a given surface body is controlled by the CAD source. Future CAD updates will synchronize its thickness value with the value in the CAD system. • In Manual mode the thickness for the surface body is controlled by the Mechanical application, so future updates from the CAD system will leave this value undisturbed. • A Thickness Mode will be Automatic until the Thickness is changed to some non-zero value. Once in Manual mode, it can be made Automatic once again by changing the Thickness value back to zero. A subsequent CAD update will conveniently synchronize the thickness with the value in the CAD system. Thicknesses for all surface bodies are represented in a dedicated column on the Worksheet that is displayed when you highlight the Geometry object. Importing Surface Body Models To import a surface body model (called a sheet body in NX), open the model in the CAD system and import the geometry as usual. If your model mixes solid bodies and surface bodies, you should select which type of entity you want to import via the Geometry preferences in the Workbench Properties 320 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application of the Geometry cell in the Project Schematic. Once in the Mechanical application, you can adjust the Geometry preferences in the Details view, where they take effect upon updating. Note If you want to retain a preference selection in the Workbench Properties, you must first save before exiting the ANSYS Workbench. Importing Surface Body Thickness When thickness is defined on the entire surface body Surface body thickness will be imported from CAD (including DesignModeler) if, and only if, the existing surface body thickness value in the Mechanical application is set to 0 (zero). This is true on initial attach and if you set the surface body thickness value to zero prior to an update. This allows you the flexibility of updating surface body thickness values from CAD or not. Surface Body Shell Offsets Surface bodies have a normal direction, identified by a green coloring when the surface body face is selected. Shell elements have a “top” surface (farthest in the positive normal direction) and a “bottom” (farthest in the negative normal direction). By default, the shell section midsurface is aligned with the surface body, but you can use the Offset Type drop down menu located in the Details view of a Surface Body object or an object scoped to a surface body to offset the shell section midsurface from the surface body: • Top - the top of the shell section is aligned with the surface body. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 321 Features • Middle (Membrane) (default) - the middle of the shell section is aligned with the surface body. • Bottom - the bottom of the shell section is aligned with the surface body. 322 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application • User Defined - the user defines the amount of offset (Membrane Offset), measured in the positive normal direction from the middle of the shell section to the surface body (may be positive or negative value). Specifying Surface Body Thickness The thickness of surface bodies can be prescribed in several ways: 1. A uniform thickness over the entire body which can be defined inside Mechanical or imported from a CAD system. Thicknesses imported from CAD can be overridden by the Thickness Mode 2. A constant or spatially varying thickness applied to a selection of surfaces or bodies. 3. Thickness values imported from an upstream system. 4. Layer information can be specified using a Layered Section, or imported through an Imported Layered Section. See Faces With Multiple Thicknesses and Layers Specified (p. 328) for information on how Mechanical resolves conflicts when multiple thickness specifications are applied to the same geometry. To specify the thickness of an entire surface body: Highlight the Surface Body object and, in the Details view, enter a value in the Thickness field. A value greater than 0 must be present in this field. To specify the thickness of selected faces on a surface body: 1. Highlight the Geometry folder in the tree and insert a Thickness object from the Geometry toolbar or choose Insert> Thickness (right-click and choose from context menu). Note The Thickness object overwrites any element that is scoped to the selected surfaces that has thickness greater than 0 defined in the Details view of the Surface Body object (See above). 2. Apply scoping to selected faces on surface bodies. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 323 Features 3. Set the desired shell offset. 4. Define the thickness as a constant (default), with a table, or with a function: a. To define the thickness as a constant, enter the value in the Thickness field in the Details view. b. To define the thickness with a table: c. i. Click the Thickness field in the Details view, then click Tabular from the flyout menu. ii. Set the Independent Variable in the Details view to X, Y, or Z. iii. Choose a Coordinate System. The Global Coordinate System (Cartesian) is the default. iv. Enter data in the Tabular Data window. The Graph window displays the variation of the thickness. To define the thickness with a function: i. Click the Thickness field in the Details view, then click Function from the flyout menu. ii. Enter the function in the Thickness field. (Example: 45+10*x/591) iii. Adjust properties in the Graph Controls category as needed: • Number of Segments - The function is graphed with a default value of 200 line segments. You can change this value to better visualize the function. • Range Minimum - The minimum range of the graph. • Range Maximum - The maximum range of the graph. Note 324 • Surface body thicknesses must be greater than zero. Failures will be detected by the solver. • When importing surfaces bodies from DesignModeler, the associated thickness is automatically included with the import. See Importing Surface Body Thickness (p. 321) for details. • Face based thickness specification is not used for the following items. Instead the body based thickness will be used: – Assembly properties: volume, mass, centroid, and moments of inertia. This is for display in the Details view only. The correct properties based on any variable thickness are correctly calculated in the solver and can be verified through miscellaneous record results for Mechanical APDL based solutions. – Meshing: auto-detection based on surface body thickness, automatic pinch controls, surface body thickness used as mesh merging tolerance. – Solution: Heuristics used in beam properties for spot welds. • Face based thickness is not supported for rigid bodies. • Variable thickness is displayed only for mesh and result displays. Location probes, Path scoped results and Surface scoped results do not display nor account for variable thickness. They assume constant thickness. • If multiple Thickness objects are applied to the same face, only those properties related to the last defined object will be sent to the solver, regardless of whether the object was defined in DesignModeler or in Mechanical. See Faces With Multiple Thicknesses and Layers Specified (p. 328) for details. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application You can import thicknesses from an upstream system. Basic setup steps are given below. You can find more information on mapping data in the Mechanical application in the appendix (Appendix B (p. 1097)). Note Thickness import is supported for 3D shell bodies or planar 2D bodies using Plane Stress. The MAPDL Solver for 3D shell bodies will use the nodal thicknesses directly via the SECFUNCTION command. For the Explicit Solver or MAPDL solver for 2D bodies, the element's nodal thicknesses are converted to an average element thickness. To import thicknesses from an upstream system: 1. In the project schematic, create a link between the Solution cell of a system and the Model cell of an upstream system. 2. Attach geometry to the analysis system, and then double-click Model to open the Mechanical window. An Imported Thickness folder is added under the Geometry folder and an imported thickness is added to the Imported Thickness folder, by default. 3. Select the appropriate options in the Details view. 4. Select Imported Thickness and select Import Thickness from the context menu. Specifying Surface Body Layered Sections Layers applied to a surface body can be prescribed in several ways: • A defined Layered Section object can be scoped to a selection of surfaces on the geometry. • An Imported Layered Section can provide layer information for the elements within a surface body. Note Layered Section objects can only be used in the following analysis types: • Explicit Dynamics • Harmonic Response • Linear Buckling • Modal • Random Vibration • Response Spectrum • Static Structural • Transient Structural The following sections describe the use of the Layered Section object. Defining and Applying a Layered Section Viewing Individual Layers Layered Section Properties Notes on Layered Section Behavior Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 325 Features Defining and Applying a Layered Section 1. Highlight the Geometry object in the tree and insert a Layered Section object from the Geometry toolbar or choose Insert > Layered Section (right-click and choose from context menu). 2. Select the Scoping Method that you will use: • Geometry Selection - Click in the Geometry field that appears, to enable you to pick surface bodies or individual faces from the model and select Apply. • Named Selection - Click on the Named Selection drop down that appears and select one of the available named selections. 3. Choose a Coordinate System. You may choose any user-defined Cartesian or Cylindrical coordinate system. The Body Coordinate System option specifies that the coordinate system selected for each body will be used. There is no default. 4. Set the desired Offset Type. Offset Type is not supported in Explicit Dynamics analyses. 5. Click on the arrow to the right of Worksheet in the Layers field then select Worksheet... to enter the layer information for this Layered Section. The Layered Section worksheet can also be activated by the Worksheet toolbar button. The worksheet displays a header row, and two inactive rows labeled +Z and -Z to indicate the order in which the materials are layered. Layer one will always be the layer at the bottom of the stack (closest to -Z). When you insert a layer, all of the layers above it will renumber. To add the first layer, right click anywhere in the Layered Section Worksheet and select Add Layer. Once the layer is added: • Click in the Material column of the row and select the material for that layer from the drop-down list. • Click in the Thickness column and define the thickness of that layer. Individual layers may have zero thickness, but the total layered-section thickness must be nonzero. • Click in the Angle column and define the angle of the material properties. The angle is measured in the element X-Y plane with respect to the element X axis. This value can be entered as degrees or radians, depending on how units are specified. To add another layer, do one of the following: • With no layers selected, you can right click the header row, +Z row, or -Z row to display a context menu. Select Add Layer to Top to add a layer row at the top (+Z) of the worksheet. Select Add Layer to Bottom to add a layer row to the bottom of the worksheet (-Z). • With one or more layers selected, you can right click any selected layer to display a context menu. Select Insert Layer Above (which inserts a layer row above the selected row in the +Z direction) or Insert Layer Below (which inserts a layer row below the selected row in the -Z direction). To delete a layer, select one or more rows, right click on any selected row, and select Delete Layer. 6. Select the Nonlinear Effects and Thermal Strain Effects settings in the Material category of the Details view. The reference temperature specified for the body on which a layered section is defined is used as the reference temperature for the layers. Nonlinear Effects and Thermal Strain Effects are not supported in Explicit Dynamics analyses. 326 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Viewing Individual Layers In the Graphics Properties section of the Details panel, the Layer To Display field allows the visualization of the thickness/offset/layer sequence of the layers composing a Layered Section object. To view a particular layer, click on the field and enter the layer number. You can use the up and down buttons or enter a layer number directly. If you enter a number larger than the maximum number of layers in that layered section, the value will be set to the maximum number of layers in that layered section. If layer zero is selected, all the layers will be drawn (without the delineation between layers) as a compact entity, shown the same as when the Mesh node is selected in the tree. All other geometry not scoped to the current Layered Section object is shown with thickness zero. Individual layers will be visible only when Show Mesh is enabled (if the model has been meshed previously), and only on Layered Section objects. If Show Mesh is not enabled, just the geometry and the scoping will be shown on the model. When a layer is selected to display, the layer with its defined thickness, offset, and sequence will be displayed in the graphics window. Due to the limitations described for the Show Mesh option, it is recommended that the user switch back and forth if needed to Wireframe/ Shaded Exterior View mode to properly see annotations. Note When viewing Imported Layered Sections, the thickness that you see is not relative to the geometry like it is with a Layered Section object. Layered Section Properties The following Properties are displayed in Details panel for Layered Sections: • Total Thickness - Total thickness of the section, including all of the layers defined for the section. Used when displaying the mesh. • Total Mass - Total mass of all of the layers in the section. The density of the material for each layer is calculated at a reference temperature of 22° C. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 327 Features Notes on Layered Section Behavior Note • If multiple thickness objects (including Layered Section objects) are applied to the same face, only those properties related to the last defined object will be sent to the solver, regardless of whether the object was defined in DesignModeler or in Mechanical. See Faces With Multiple Thicknesses and Layers Specified (p. 328) for details. • If adjacent elements within the same part have different thickness values, the elements will appear to be ramped. • Layered Sections cannot be scoped to rigid bodies. • Layered Sections do not affect the following items: – Assembly properties: volume, mass, centroid, and moments of inertia. This is for display in the Details view only. The correct properties based on any variable thickness are correctly calculated in the solver and can be verified through miscellaneous record results for Mechanical APDL based solutions. – Meshing: auto-detection based on surface body thickness, automatic pinch controls, surface body thickness used as mesh merging tolerance. – Solution: Heuristics used in beam properties for spot welds. • A Thermal Condition applied to a Layered Section is only valid if applied to both shell faces (Shell Face is set to Both, not to Top or Bottom). • Layered Sections are not valid with cyclic symmetry. • The following material properties are supported by Layered Sections in an Explicit Dynamics analysis: • – Isotropic Elasticity, Orthotropic Elasticity – Johnson Cook Strength, Zerilli Armstrong Strength, Steinberg Guinan Strength, Cowper Symonds Strength – Orthotropic Stress Limits, Orthotropic Strain Limits, Tsai-Wu Constants – Plastic Strain, Principal Stress, Stochastic Failure, For orthotropic materials in Explicit Dynamics, the Z material direction is always defined in the shell normal direction. The X material direction in the plane of each element is determined by the x-axis of the coordinate system associated with the Layered Section. If the x-axis of this coordinate system does not lie in the element plane, then the x-axis is projected onto the shell in the coordinate system z-axis direction. If the z-axis is normal to the element plane, then the projection is done in the coordinate system y-axis. For cylindrical systems, it is the y-axis that is projected onto the element plane to find the Y material direction. Faces With Multiple Thicknesses and Layers Specified Thickness and Layered Section objects may be scoped to more than one face of a surface body. As a result, a face may have more than one thickness definition. The order of precedence used to determine the thickness that will be used in the analysis is as follows: 1. 328 Imported Layered Section objects Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application 2. Imported Thickness objects 3. Layered Section objects 4. Thickness objects 5. Thickness as a property of a body/part For multiple objects of the same type, the object lower in the tree (more recently created) will be used in the analysis. This thickness may not be the desired thickness to be used in the analysis. In a large model, you may want to fix this problem prior to solving the model. You can search for faces with multiple thicknesses by selecting Search Faces with Multiple Thicknesses from the context menu of any of the following: the Geometry folder, a Body object (individual or group of objects), a Thickness object or a Layered Section object. For each face found with multiple thicknesses, a warning message similar to the one shown below will be displayed in the message box. This face has more than one thickness defined. You may graphically select the face via RMB on this warning in the Messages window. To find the face and its corresponding thickness objects for a particular message, highlight that message in the message pane, right-click on the message and choose Go To Face With Multiple Thicknesses from the context menu. The face associated with this message is highlighted in the Geometry window and the corresponding thickness objects are highlighted in the tree. If there is no face with multiple definitions, the following information will be displayed in the message box. No faces with multiple thicknesses have been found. A related Go To option is also available. If you highlight one or more faces with thickness definition of a surface body, then right-click in the Geometry window and choose Go To> Thicknesses for Selected Faces, the corresponding thickness objects will be highlighted in the tree. Note You cannot search for Imported Layered Sections that overlap with other thickness objects. However a warning will be generated during the solution if this situation might exist. Line Bodies A line body consists entirely of edges and does not have a surface area or volume. You can import line bodies from DesignModeler or other CAD sources (see Geometry Preferences). Once imported, a line body is represented by a Line Body object in the tree, where the Details view includes the associated cross section information of the line body that was defined in DesignModeler or supported CAD system. Depending on your application, you can further define the line body as either a beam or a pipe. Here are some guidelines: • Beam is usually a suitable option when analyzing thin to moderately thick beam structures. A variety of cross-sections can be associated with beams. • Pipes are more suitable for analyzing initially circular cross-sections and thin to moderately thick pipe walls. Users can apply special loads on pipes such as Pipe Pressure and Pipe Temperature. Curved pipe zones or high deformation zones in pipes can be further modeled using the Pipe Idealization object. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 329 Features To define your line body, highlight the Line Body object and set the following in the Details view: 1. Offset Mode: to Refresh on Update (default) to enable the values in the Details view to update when the CAD system updates, or to Manual, to enable the Details view values to override the CAD system updates. 2. Model Type: to Beam or Pipe. 3. Offset Type: to Centroid, Shear Center, Origin, or User Defined, where Offset X and Offset Y are available. The following read-only information is used in the definition of both beam and pipe: • Cross Section • Cross Section Area • Cross Section IYY • Cross Section IZZ Note • Beams can also be used as connections within a model. See Beam Connections (p. 483) for further information on this application. • Pipes are only realized in structural analyses. All line bodies defined in other analysis types are always realized as beams. This extends to linked analyses as well. For example, in a thermal-structural linked analysis where line bodies are defined as pipes, the thermal component of the analysis will only realize the line bodies as beams. Viewing Line Body Cross Sections By default, line bodies are displayed simply as lines in the Geometry window, with no graphical indication of cross sections. If cross sections are defined in line bodies and you choose View> Cross Section Solids (Geometry), you enable a feature where line bodies are displayed as solids (3-D), allowing you to visually inspect the cross sections. This visualization can be useful in determining the correct orientation of the line bodies. For circular and circular tube cross sections, the number of divisions used for rendering the line bodies as solids has an adjustable range from 6 to 360 with a default of 16. You can make this adjustment by choosing Tools> Options, and under Graphics, entering the number in the Number of Circular Cross Section Divisions field. The Cross Section Solids (Geometry) feature has the following characteristics: • By default, this feature is disabled. However, the setting persists as a session preference. • Only geometry displays are applicable. The feature is not available for mesh displays. • When the feature is enabled, both normal lines and solid representations are drawn. • The solid representation of the geometry cannot be selected nor meshed, and has no effect on quantitative results. • The feature supports section planes and works with all line body cross sections (primitive and user defined). • User integrated sections (direct entry of properties) will have no display. • The feature is not available for use with viewports. 330 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Rigid Bodies You can declare the stiffness behavior of a single solid body (a body that is not a component of a multibody part), a body group, surface bodies, and 2D models to be rigid or flexible. A rigid body will not deform during the solution. This feature is useful if a mechanism has only rigid body motion or, if in an assembly, only some of the parts experience most of the strains. It is also useful if you are not concerned about the stress/strain of that component and wish to reduce CPU requirements during meshing or solve operations. To set the stiffness behavior in the Mechanical application 1. Select a body in the tree. 2. In the Details view, set Stiffness Behavior to Rigid or Flexible. To define a rigid body, set the field of the Details view to Rigid when the body object is selected in the tree. If rigid, the body will not be meshed and will internally be represented by a single mass element during the solution. (The mass element’s mass and inertial properties will be maintained.) The mass, centroid, and moments of inertia for each body can be found in the Details view of the body object. The following restrictions apply to rigid bodies: • • Rigid bodies are only valid in static structural, Transient Structural, Rigid Dynamics, and modal analyses for the objects listed below. Animated results are available for all analysis types except modal. – Point mass – Joint – Spring – Remote displacement – Remote force – Moment – Contact Rigid bodies are valid when scoped to solid bodies, surface bodies, or line bodies in Explicit Dynamics Analysis (p. 35) for the following objects: – Fixed support – Displacement – Velocity The following outputs are available for rigid bodies, and are reported at the centroid of the rigid body: • Results: Displacement, Velocity, and Acceleration • Probes: Deformation, Position, Rotation, Velocity, Acceleration, Angular Velocity, and Angular Acceleration Note • If you highlight Deformation results in the tree that are scoped to rigid bodies, the corresponding rigid bodies in the Geometry window are not highlighted. • You cannot define a line body, 2D plane strain body, or 2D axisymmetric body as rigid. • All the bodies in a body group (part) must have similar stiffness behavior. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 331 Features 2-D Analyses The Mechanical application has a provision that allows you to run structural and thermal problems that are strictly two-dimensional (2-D). For models and environments that involve negligible effects from a third dimension, running a 2-D simulation can save processing time and conserve machine resources. You can configure Workbench for a 2-D analysis by first creating or opening a surface body model in DesignModeler, or in any supported CAD system that has provisions for surface bodies. The model must be in the x-y plane. 2-D planar bodies are supported, 2-D wire bodies are not. Then, with the Geometry cell selected in the Project Schematic, expose the Properties Details of Geometry window using the toolbar Workspace drop-down menu, and choose 2-D in the Analysis Type drop-down menu (located under Advanced Geometry Defaults). Attach the model into the Mechanical application by doubleclicking on the Model cell. You can specify a 2-D analysis only when you attach the model. After attaching, you cannot change from a 2-D analysis to a 3-D analysis or vice versa. A 2-D analysis has the following characteristics: • For Geometry items in the tree, you have the following choices located in the 2D Behavior field within the Details view: – Plane Stress (default): Assumes zero stress and non-zero strain in the z direction. Use this option for structures where the z dimension is smaller than the x and y dimensions. Example uses are flat plates subjected to in-plane loading, or thin disks under pressure or centrifugal loading. A Thickness field is also available if you want to enter the thickness of the model. – Axisymmetric: Assumes that a 3-D model and its loading can be generated by revolving a 2-D section 360o about the y-axis. The axis of symmetry must coincide with the global y-axis. The geometry has to lie on the positive x-axis of the x-y plane. The y direction is axial, the x direction is radial, and the z direction is in the circumferential (hoop) direction. The hoop displacement is zero. Hoop strains and stresses are usually very significant. Example uses are pressure vessels, straight pipes, and shafts. – Plane Strain: Assumes zero strain in the z direction. Use this option for structures where the z dimension is much larger than the x and y dimensions. The stress in the z direction is non-zero. Example uses are long, constant, cross-sectional structures such as structural line bodies. Plane Strain behavior cannot be used in a thermal analysis (steady-state or a transient). Note Since thickness is infinite in plane strain calculations, different results (displacements/stresses) will be calculated for extensive loads (that is, forces/heats) if the solution is performed in different unit systems (MKS vs. NMM). Intensive loads (pressure, heat flux) will not give different results. In either case, equilibrium is maintained and thus reactions will not change. This is an expected consequence of applying extensive loads in a plane strain analysis. In such a condition, if you change the Mechanical application unit system after a solve, you should clear the result and solve again. – Generalized Plane Strain: Assumes a finite deformation domain length in the z direction, as opposed to the infinite value assumed for the standard Plane Strain option. Generalized Plane Strain provides more practical results for deformation problems where a z direction dimension exists, but is not considerable. See Using Generalized Plane Strain (p. 333) for more information. Generalized Plane Strain needs the following three types of data: 332 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application → Fiber Length: Sets the length of the extrusion. → End Plane Rotation About X: Sets the rotation of the extrusion end plane about the x-axis. → End Plane Rotation About Y: Sets the rotation of the extrusion end plane about the y-axis. – By Body: Allows you to set the Plane Stress (with Thickness option), Plane Strain, or Axisymmetric options for individual bodies that appear under Geometry in the tree. If you choose By Body, then click on an individual body, these 2-D options are displayed for the individual body. • For a 2-D analysis, use the same procedure for applying loads and supports as you would use in a 3-D analysis. The loads and results are in the x-y plane and there is no z component. • You can apply all loads and supports in a 2-D analysis except for the following: Bolt Pretension Load, Line Pressure, Simply Supported, and Fixed Rotation. • A Pressure load can only be applied to an edge. • A Bearing Load and a Cylindrical Support can only be applied to a circular edge. • For analyses involving axisymmetric behavior, a Rotational Velocity load can only be applied about the y-axis. • For loads applied to a circular edge, the direction flipping in the z axis will be ignored. • Only Plain Strain and Axisymmetric are supported for Explicit Dynamics analyses. Using Generalized Plane Strain The generalized plane strain feature can be used in structural, modal, and linear buckling analyses. Stepped analyses are not supported. The feature assumes a finite deformation domain length in the z direction, as opposed to the infinite value assumed for standard plane strain. It provides a more efficient way to simulate certain 3-D deformations using 2-D options. The deformation domain or structure is formed by extruding a plane area along a curve with a constant curvature, as shown below. Y Starting Plane Starting Point Ending Plane X Fiber Direction Z Ending Point The extruding begins at the starting (or reference) plane and stops at the ending plane. The curve direction along the extrusion path is called the fiber direction. The starting and ending planes must be perpendicular to this fiber direction at the beginning and ending intersections. If the boundary conditions and loads in the fiber direction do not change over the course of the curve, and if the starting plane and ending plane remain perpendicular to the fiber direction during deformation, then the amount of deformation of all cross sections will be identical throughout the curve, and will not vary at any curve position in the fiber direction. Therefore, any deformation can be represented by the deformation on the starting plane, and the 3-D deformation can be simulated by solving the deformation problem on the starting plane. The Plane Strain and Axisymmetric options are particular cases of the Generalized Plane Strain option. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 333 Features All inputs and outputs are in the global Cartesian coordinate system. The starting plane must be the xy plane, and must be meshed. The applied nodal force on the starting plane is the total force along the fiber length. The geometry in the fiber direction is specified by the rotation about the x-axis and y-axis of the ending plane, and the fiber length passing through a user-specified point on the starting plane called the starting or reference point. The starting point creates an ending point on the ending plane through the extrusion process. The boundary conditions and loads in the fiber direction are specified by applying displacements or forces at the ending point. The fiber length change is positive when the fiber length increases. The sign of the rotation angle or angle change is determined by how the fiber length changes when the coordinates of the ending point change. If the fiber length decreases when the x coordinate of the ending point increases, the rotation angle about y is positive. If the fiber length increases when the y coordinate of the ending point increases, the rotation angle about x is positive. For linear buckling and modal analyses, the Generalized Plane Strain option usually reports fewer Eigenvalues and Eigenvectors than you would obtain in a 3-D analysis. Because it reports only homogeneous deformation in the fiber direction, generalized plane strain employs only three DOFs to account for these deformations. The same 3-D analysis would incorporate many more DOFs in the fiber direction. Because the mass matrix terms relating to DOFs in the fiber direction are approximated for modal and transient analyses, you cannot use the lumped mass matrix for these types of simulations, and the solution may be slightly different from regular 3-D simulations when any of the three designated DOFs is not restrained. Overall steps to using Generalized Plane Strain 1. Attach a 2-D model in the Mechanical application. 2. Click on Geometry in the tree. 3. In the Details view, set 2D Behavior to Generalized Plane Strain. 4. Define extrusion geometry by providing input values for Fiber Length, End Plane Rotation About X, and End Plane Rotation About Y. 5. Add a Generalized Plane Strain load under the analysis type object in the tree. Note The Generalized Plane Strain load is applied to all bodies. There can be only one Generalized Plane Strain load per analysis type so this load will not be available in any of the load drop-down menu lists if it has already been applied. 6. In the Details view, input the x and y coordinates of the reference point , and set the boundary conditions along the fiber direction and rotation about the x and y-axis. 7. Add any other loads or boundary conditions that are applicable to a 2-D model. 8. Solve. Reactions are reported in the Details view of the Generalized Plane Strain load. 9. Review results. Symmetry You can use the inherent geometric symmetry of a body to model only a portion of the body for simulation. Using symmetry provides the benefits of faster simulation times and less use of system resources. 334 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application For example, the model below can be simplified by modeling only ¼ of the geometry by taking advantage of two symmetry planes. Introduction Making use of the Symmetry feature requires an understanding of the geometry symmetry and the symmetry of loading and boundary conditions. If geometric symmetry exists, and the loading and boundary conditions are suitable, then the model can be simplified to just the symmetry sector of the model. DesignModeler can be used to simplify a full model into a symmetric model. This is done by identifying symmetry planes in the body. DesignModeler will then slice the full model and retain only the symmetry portion of the model. (See Symmetry in the DesignModeler help). To further understand the use of Symmetry in the Mechanical application, examine the following topics: Types of Regions Symmetry Defined in DesignModeler Symmetry in the Mechanical Application Types of Regions When the Mechanical application attaches to a symmetry model from DesignModeler, a Symmetry folder is placed in the tree and each Symmetry Plane from DesignModeler is given a Symmetry Region object in the tree. In addition, Named Selection objects are created for each symmetry edge or face. (See Symmetry Defined in DesignModeler (p. 351).) The Symmetry folder supports the following objects: • Symmetry Region – supported for structural analyses. • Periodic Region – supported for magnetostatic analyses. • Cyclic Region – supported for structural and thermal analyses. See the individual sections for additional information about each of these symmetry objects. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 335 Features Periodic and Cyclic regions also ensure that a mesh is cyclic and suitable for fluids analyses (the mesh is then matched, however, users must re-assign periodic regions in the solver). For models generated originally as symmetry models, you may create a Symmetry folder and manually identify Symmetry Region objects or Periodic/Cyclic Region objects. (See Symmetry in the Mechanical Application (p. 352).) Symmetry Region A symmetry region refers to dimensionally reducing the model based on a mirror plane. Symmetry regions are supported for: • Structural Symmetry • Structural Anti-Symmetry • Electromagnetic Symmetry • Electromagnetic Anti-Symmetry • Explicit Dynamics Symmetry Structural Symmetry A symmetric structural boundary condition means that out-of-plane displacements and in-plane rotations are set to zero. The following figure illustrates a symmetric boundary condition. Structural symmetry is applicable to solid and surface bodies. Structural Anti-Symmetry An anti-symmetric boundary condition means that the rotation normal to the anti-symmetric face is constrained. The following figure illustrates an anti-symmetric boundary condition. Structural antisymmetry is applicable to solid and surface bodies. 336 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Note The Anti-Symmetric option does not prevent motion normal to the symmetry face. This is appropriate if all loads on the structure are in-plane with the symmetry plane. If applied loads, or loads resulting from large deflection introduce force components normal to the face, an additional load constraint on the normal displacement may be required. Electromagnetic Symmetry Symmetry conditions exist for electromagnetic current sources and permanent magnets when the sources on both sides of the symmetry plane are of the same magnitude and in the same direction as shown in the following example. Electromagnetic symmetric conditions imply Flux Normal boundary conditions, which are naturally satisfied. Electromagnetic Anti-Symmetry Anti-Symmetry conditions exist for electromagnetic current sources and permanent magnets when the sources on both sides of the symmetry plane are of the same magnitude but in the opposite direction as shown in the following example. Electromagnetic anti-symmetric conditions imply Flux Parallel boundary conditions, which you must apply to selected faces. Explicit Dynamics Symmetry Symmetry regions can be defined in explicit dynamics analyses. Symmetry objects should be scoped to faces of flexible bodies defined in the model. All nodes lying on the plane, defined by the selected face will be constrained to give a symmetrical response of the structure. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 337 Features Note • Anti-symmetry, periodicity and anti-periodicity symmetry regions are not supported in Explicit Dynamics systems. • Symmetry cannot be applied to rigid bodies. • Only the General Symmetry interpretation is used by the solver in 2D Explicit Dynamics analyses. Symmetry conditions can be interpreted by the solver in two ways: General Symmetry Global Symmetry Planes General Symmetry In general, a symmetry condition will result in degree of freedom constraints being applied to the nodes on the symmetry plane. For volume elements, the translational degree of freedom normal to the symmetry plane will be constrained. For shell and beam elements, the rotational degrees of freedom in the plane of symmetry will be additionally constrained. For nodes which have multiple symmetry regions assigned to them (for example, along the edge between two adjacent faces), the combined constraints associated with the two symmetry planes will be enforced. Note • Symmetry regions defined with different local coordinate systems may not be combined, unless they are orthogonal with the global coordinate system. • General symmetry does not constrain eroded nodes. Thus, if after a group of elements erodes, a “free” eroded node remains, the eroded node will not be constrained by the symmetry condition. This can be resolved in certain situations via the special case of Global symmetry, described in the next section. Global Symmetry Planes If a symmetry object is aligned with the Cartesian planes at x=0, y=0 or z=0, and all nodes in the model are on the positive side of x=0, y=0, or z=0, the symmetry condition is interpreted as a special case termed Global symmetry plane. In addition to general symmetry constraints: • If a symmetry plane is coincident with the YZ plane of the global coordinate system (Z=0), and no parts of the geometry lie on the negative side of the plane, then a symmetry plane is activated at X=0. This will prevent any nodes (including eroded nodes) from moving through the plane X=0 during the analysis. • If a symmetry plane is coincident with the ZX plane of the global coordinate system (Y=0), and no parts of the geometry lie on the negative side of the plane, then a symmetry plane is activated at Y=0. This will prevent any nodes (including eroded nodes) from moving through the plane Y=0 during the analysis. • If a symmetry plane is coincident with the XY plane of the global coordinate system (Z=0), and no parts of the geometry lie on the negative side of the plane, then a symmetry plane is activated at Z=0. This 338 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application will prevent any nodes (including eroded nodes) from moving through the plane Z=0 during the analysis. Note Global symmetry planes are only applicable to 3D Explicit Dynamics analyses. Periodic Region The Periodic Region object is used to define for Electromagnetic analysis Periodical or Anti–Periodical behavior in a particular model. Electromagnetic Periodicity A model exhibits angular periodicity when its geometry and sources occur in a periodic pattern around some point in the geometry, and the repeating portion that you are modeling represents all of the sources, as shown below. Electromagnetic Anti-Periodicity A model exhibits angular anti-periodicity when its geometry and sources occur in a periodic pattern around some point in the geometry and the repeating portion that you are modeling represents a subset of all of the sources, as shown below. Electromagnetic Periodic Symmetry Electric machines and generators, solenoid actuators and cyclotrons are just a few examples of numerous electromagnetic devices that exhibit circular symmetrical periodic type of symmetry. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 339 Features An automated periodic symmetry analysis conserves time and CPU resources and delivers analysis results that correspond to the entire structure. The overall procedure in ANSYS Workbench for simulating structures that are periodically symmetric is to run a magnetostatic analysis and perform the following specialized steps: 1. Insert a Periodic Region symmetry object in the tree. This step is necessary to enable ANSYS Workbench to perform a periodic symmetry analysis. 2. Define the low and high boundaries of the Periodic Region by selecting the appropriate faces in the Low Boundary and High Boundary fields. 3. Define type of symmetry as Periodic or Anti-Periodic (see Periodicity Example (p. 340)). 4. The solver will automatically take into account defined periodicity, and reported results will correspond to the full symmetry model (except volumetric type results as Force Summation, Energy probe, and so on). Note For a magnetic field simulation with periodic regions, you must be careful when applying flux parallel boundary conditions to adjoining faces. If the adjoining faces of the periodic faces build up a ring and all are subject to flux parallel conditions, that implies a total flux of zero through the periodic face. In some applications that is not a physically correct requirement. One solution is to extend the periodic sector to include the symmetry axis. See the Periodicity Example (p. 340) section for further details. Periodicity Example Periodicity is illustrated in the following example. A coil arrangement consists of 4 coils emulated by stranded conductors. A ½ symmetry model of surrounding air is created. The model is conveniently broken into 16 sectors for easy sub-division into periodic sectors and for comparison of results. 340 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Below is a display of the Magnetic Field Intensity for the ½ symmetry model at the mid-plane. The arrows clearly indicate an opportunity to model the domain for both Periodic or Anti-periodic sectors. Periodic planes are shown to exist at 180 degree intervals. Anti-periodic planes are shown to exist at 90 degree intervals. The model can be cut in half to model Periodic planes. Applying periodic symmetry planes at 90 degrees and 270 degrees leads to the following results. The model can be cut in half again to model Anti-Periodic planes. Applying anti-periodic symmetry planes at 0 degrees and 90 degrees leads to the following results. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 341 Features Cyclic Region Fan wheels, spur gears, and turbine blades are all examples of models that can benefit from cyclic symmetry. An automated cyclic symmetry analysis conserves time and CPU resources and allows you to view analysis results on the entire structure (for a structural analysis). ANSYS Workbench automates cyclic symmetry analysis by: • Solving for the behavior of a single symmetric sector (part of a circular component or assembly). See The Basic Sector in the Advanced Analysis Techniques Guide for more information. • Using the single-sector solution to construct the response behavior of the full circular component or assembly (as a postprocessing step). For example, by analyzing a single 10° sector of a 36-blade turbine wheel assembly, you can obtain the complete 360° model solution via simple postprocessing calculations. Using twice the usual number of degrees of freedom (DOFs) in this case, the single sector represents a 1/36th part of the model. Note Layered Sections cannot be applied to a model that uses cyclic symmetry. The overall procedure in ANSYS Workbench for simulating models that are cyclically symmetric is to run a static structural, modal, or thermal analysis and perform the following specialized steps: 1. Insert a Cyclic Region symmetry object in the tree. This step is necessary to enable ANSYS Workbench to perform a cyclic symmetry analysis. Multiple Cyclic Region objects are permitted but they must refer to the same Coordinate System to specify the symmetry axis. 2. Define the low and high boundaries of the Cyclic Region by selecting the appropriate faces in the Low Boundary and High Boundary fields. Each selection can consist of one or more faces over one or more parts, but they must be paired properly. To be valid, each face in Low Boundary must be accompanied by its twin in High Boundary. Also, ensure that each face and its twin belong to the same multibody part (although it is not necessary that they belong to the same body), using DesignModeler to adjust your multibody parts as needed. Your selections will be used to match the mesh of these two boundaries. The example shown below illustrates two equally valid Low Boundary and High Boundary twin faces. One twin set of faces, located in the corner body, includes faces that are both included in that same body. Another twin set includes faces that are not on the same body, but are included in the same multibody part, as shown in the second figure. 342 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Note High Boundary and Low Boundary should be exactly same in shape and size, otherwise Mechanical will not be able to map nodes from Low Boundary to High Boundary to create full model from a single sector. 3. Continue with the remainder of the analysis. Consult the sections below as applicable to the analysis type. Refer to the following sections for further details on cyclic symmetry: Cyclic Symmetry in a Static Structural Analysis Cyclic Symmetry in a Modal Analysis Cyclic Symmetry in a Thermal Analysis Cyclic Symmetry in a Static Structural Analysis When you perform a static structural analysis that involves cyclic symmetry, unique features are available for loads/supports and reviewing results. These features are described in the following sections: Applying Loads and Supports for Cyclic Symmetry in a Static Structural Analysis Reviewing Results for Cyclic Symmetry in a Static Structural Analysis Applying Loads and Supports for Cyclic Symmetry in a Static Structural Analysis In the presence of cyclic symmetry, the Point Mass object is not valid for a structural analysis. Also, the following loads are not available: Remote Force, Moment, Bearing, Joint, Hydrostatic Pressure and Fluid Solid Interface. Inertial loads are restricted to the axial direction. To comply, Rotational Velocity, Acceleration and Standard Earth Gravity loads must be defined by components: only the Z component can be non-zero and the Coordinate System specified must match that used in the Cyclic Region. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 343 Features Additional restrictions apply while specifying supports for a static structural analysis. For example, Elastic Supports, Compression Only Supports, Remote Displacement, and Constraint Equations are not available. Also, the loads and supports should not include any face selections (for example, on 3D solids) that already belong to either the low or high boundaries of the cyclic symmetry sector. Loads and supports may include edges (for example, on 3D solids) on those boundaries, however. Loads and supports are assumed to have the same spatial relation for the cyclic axis in all sectors. In preparation for solution, the boundary conditions on the geometry are converted into node constraints in the mesh (see Converting Boundary Conditions to Nodal DOF Constraints (Mechanical APDL Solver) (p. 854) for more information). When these boundary conditions involve nodes along the sector boundaries (low, high and axial boundaries), their constraints are integrated to properly reflect the symmetry. As an example, the low and high edges may feature more node constraints than are applied to each individually, in order to remain consistent with an equivalent full model. Reviewing Results for Cyclic Symmetry in a Static Structural Analysis When simulating cyclic symmetry in a static structural analysis, the same results are available as results in static structural analyses that involve full symmetry, with the exception of Linearized Stresses, Force Reaction probes, and Moment Reaction probes. Although one cyclic sector is analyzed, the results are valid for the full symmetry model. You can display either the one cycle result sector or the full symmetry model result by choosing Visual Expansion from the View menu. Unexpanded One Sector Model Display: 344 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Expanded Full Symmetry Model Display: Note • Unaveraged contact results do not expand to all expanded sectors in a cyclic analysis. • Animation is not supported for an unexpanded display. Cyclic Symmetry in a Modal Analysis When you perform a modal analysis that involves cyclic symmetry, unique features are available for loads/supports, analysis settings, and reviewing results. These features are described in the following sections: Applying Loads and Supports for Cyclic Symmetry in a Modal Analysis Analysis Settings for Cyclic Symmetry in a Modal Analysis Reviewing Results for Cyclic Symmetry in a Modal Analysis Applying Loads and Supports for Cyclic Symmetry in a Modal Analysis In the presence of cyclic symmetry, the Point Mass object is not valid for a modal analysis. Additional restrictions apply while specifying supports for a modal analysis in the presence of cyclic symmetry. For example, Elastic Supports, Compression Only Supports, and Constraint Equations are not permitted. Also, the supports should not include any face selections (for example, on 3D solids) that already belong to either the low or high boundaries of the cyclic symmetry sector. Supports may include edges (for example, on 3D solids) on those boundaries, however. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 345 Features In preparation for solution, the boundary conditions on the geometry are converted into node constraints in the mesh (see Converting Boundary Conditions to Nodal DOF Constraints (Mechanical APDL Solver) (p. 854) for more information). When these boundary conditions involve nodes along the sector boundaries (low, high and axial boundaries), their constraints are integrated to properly reflect the symmetry. As an example, the low and high edges may feature more node constraints than are applied to each individually, in order to remain consistent with an equivalent full model. If the modal analysis is activated as pre-stressed, no other modal loads/supports are allowed. On the other hand you can apply all pertinent structural loads/supports in the previous cyclic static analysis. Analysis Settings for Cyclic Symmetry in a Modal Analysis A modal analysis involving cyclic symmetry includes a Cyclic Controls (p. 537) category that enables you to solve the harmonic index for all values, or for a range of values. This category is available if you have defined a Cyclic Region in the analysis. Reviewing Results for Cyclic Symmetry in a Modal Analysis A modal analysis involving cyclic symmetry includes additional options to help you navigate and interpret the results. In particular, there are features to: • Review the complete range of modes: you may request the modes to be sorted by their serial number in the results file or by their frequency value in the spectrum. • Review combinations of degenerate modes through the complete range of phase angles. You can display either the one cycle result sector or the full symmetry model result by choosing Visual Expansion from the View menu. Because these features involve reviewing the mode shapes and contours at individual points within a range, they leverage the charting facilities of the Graph and Tabular Data windows together with the 3D contour plotting of the Graphics view. Reviewing the Complete Range of Modes You may request the modes to be sorted in the Graph window by their set number in the results file or by their frequency value in the spectrum. You may then interact with the plot to generate specific mode shapes and contours of interest. To control how modes are sorted, use the X-Axis setting under Graph Controls in the Details view of the result and set to either Mode or Frequency: • 346 Mode: This choice will designate the x-axis in the Graph window to indicate the set numbers for each mode (within a harmonic index) in the results file. Each mode will have a vertical bar whose height represents its frequency of vibration. The columns in the Tabular Data window are displayed in the order of: Mode, Harmonic Index and Frequency. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application When X-Axis is set to Mode, the Definition category includes settings for Cyclic Mode and Harmonic Index. • Frequency: This choice will designate the x-axis in the Graph window to indicate the mode Frequency. Modes are thus sorted by their frequencies of vibration. Each mode will have a vertical bar whose height, for cross-reference, corresponds to the mode number (within its harmonic index). The columns in the Tabular Data window are displayed in the order of: Frequency, Mode and Harmonic Index. When X-Axis is set to Frequency, the Definition category includes a setting for Cyclic Phase. Read-only displays of the Minimum Value Over Phase and the Maximum Value Over Phase are also available. • Phase: For degenerate modes or couplets, a third option for the X-Axis setting under Graph Controls is available. This choice will designate the x-axis in the Graph window to indicate the phase angle. The graph will show the variation of minimum and maximum value of the result with change in phase angle for the concerned couplet. This setting allows you to analyze the result for a particular mode (for couplets only). The columns in the Tabular Data window are displayed in the order of: Phase, Minimum and Maximum. For details on couplets, read the section below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 347 Features Reviewing results for frequency couplets as a function of cyclic phase angles An inspection of the results for harmonic indices between 0 and N/2 (that is, 0 < Harmonic Index < N/2) reveals that natural frequencies are reported in pairs by the solver. These pairs of equal value are often termed “couplets”. The corresponding mode shapes in each couplet represent two standing waves, one based on a sine and another on a cosine solution of the same spatial frequency, thus having a phase difference of 90o. To appreciate the full range of vibrations possible at a given frequency couplet, it is necessary to review not only the individual mode shapes for sine and cosine (e.g., at 0o and 90o) but also their linear combinations which sweep a full cycle of relative phases from 0o to 360o. This sweep is displayed by Mechanical as an animation called a "traveling wave". The following is an example: Note The following demos are presented in animated GIF format. Please view online if you are reading the PDF version of the help. Animations for mode shapes in other harmonic indices, that is, 0 or, for N even, N/2, will yield standing waves. The following animation is an example of a standing wave. 348 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application There are options to review the dependence of a result on cyclic phase angle quantitatively. For applicable harmonic indices, results can be defined by: • Cyclic Phase: Use in combination with the Cyclic Phase setting to report the contour at a specific phase. Under this setting, the result will also report the Minimum Value Over Cyclic Phase and the Maximum Value Over Cyclic Phase. • Maximum over Cyclic Phase: this contour reveals the peak value of the result as a function of cyclic phase for every node/element. • Cyclic Phase of Maximum: this contour reveals the cyclic phase at which the peak value of the result is obtained for every node/element. When the result is defined by Cyclic Phase, it may be convenient to use the interaction options to pick the value of phase from the Tabular Data window as an alternative to direct input in the Details view. To access this feature, set the X-Axis to Phase under Graph Controls. To control the density of the cyclic phase sweep, choose Tools> Options from the main menu, then under Mechanical choose Frequency and Cyclic Phase Number of Steps. The phase sweep can be disabled individually on a result by setting Allow Phase Sweep to No in the Details view. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 349 Features Interaction Options The Graph, Tabular Data and the Graphics view can be used in concert while reviewing modal cyclic results. For example, if you click in the Tabular Data window, a black vertical cursor moves to the corresponding position in the chart. Conversely, if you click on a bar (for Mode or Frequency display) or a node in the chart (for a Phase display), the corresponding row is highlighted in the Tabular Data window. Multi-selection is also available by dragging the mouse over a range of bars or nodes (in the chart) or rows in the Tabular Data window. These are useful in identifying the mode number and harmonic index with specific values of the frequency spectrum. Also, the Graph or Tabular Data windows can be used to request a specific mode shape at a phase value of interest (if applicable) using context sensitive options. To access these, select an item in the Graph or Tabular Data windows and click the right mouse button. The following are the most useful options: • Retrieve This Result: Auto-fills the Mode and Harmonic Index ( for a Mode or Frequency display) or the Phase angle (for a Phase display) into the Details view of the result and will force the evaluation of the result with the parameters that were recently changed. • Create Mode Shape Results: processes the selected pairs (Mode, Harmonic Index defined by dragging in the Graph window to produce a light blue rectangle) and inserts results under the Solution folder. You must then evaluate these results, since they are not evaluated automatically. This option is not available for Phase display. The following two options are available only if you click the right mouse button in the Graph window: 350 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application • Zoom to Range: Zooms in on a subset of the data in the Graph window. Click and hold the left mouse at a step location and drag to another step location. The dragged region will highlight in blue. Next, select Zoom to Range. The chart will update with the selected step data filling the entire axis range. This also controls the time range over which animation takes place. • Zoom to Fit: If you have chosen Zoom to Range and are working in a zoomed region, choosing Zoom to Fit will return the axis to full range covering all steps. Cyclic Symmetry in a Thermal Analysis When you perform a steady state thermal analysis or transient thermal analysis that involves cyclic symmetry, unique features are available for loads/supports and reviewing results. These features are described in the following sections: Applying Loads for Cyclic Symmetry in a Thermal Analysis Reviewing Results for Cyclic Symmetry in a Thermal Analysis Applying Loads for Cyclic Symmetry in a Thermal Analysis For a thermal analysis, in the presence of cyclic symmetry, Coupling loads are not available and the Point Mass object is not valid. Also, loads should not include any face selections (for example, on 3D solids) that already belong to either the low or high boundaries of the cyclic symmetry sector. Loads may include edges (for example, on 3D solids) on those boundaries, however. Loads are assumed to have the same spatial relation for the cyclic axis in all sectors. In preparation for solution, the boundary conditions on the geometry are converted into node constraints in the mesh (see Converting Boundary Conditions to Nodal DOF Constraints (Mechanical APDL Solver) (p. 854) for more information). When these boundary conditions involve nodes along the sector boundaries (low, high and axial boundaries), their constraints are integrated to properly reflect the symmetry. As an example, the low and high edges may feature more node constraints than are applied to each individually, in order to remain consistent with an equivalent full model. Reviewing Results for Cyclic Symmetry in a Thermal Analysis When simulating cyclic symmetry in a thermal analysis, the same results are available as results in a thermal analysis that involve full symmetry. Note Radiation Probe results are calculated for the full symmetry model. Symmetry Defined in DesignModeler The following procedure describes the steps use to working with Symmetry in DesignModeler. 1. While in DesignModeler, from the Tools menu, apply the Symmetry feature to the model or define an Enclosure. 2. Enter the Mechanical application by double-clicking on the Model cell in the Project Schematic. The Mechanical application screen appears and includes the following objects in the tree: • A Symmetry object. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 351 Features 3. • Symmetry Region objects displayed under the Symmetry folder. The number of Symmetry Region objects corresponds to the number of symmetry planes you defined in DesignModeler. • A Named Selections folder object. Each child object displayed under this folder replicates the enclosure named selections that were automatically created when you started the Mechanical application. In the Details view of each Symmetry Region object, under Definition, specify the type of symmetry by first clicking on the Type field, then choosing the type from the drop down list. Boundary conditions will be applied to the symmetry planes based on both the simulation type and what you specify in the symmetry Type field. The Scope Mode read-only indication is Automatic when you follow this procedure of defining symmetry in DesignModeler. The Coordinate System and Symmetry Normal fields include data that was “inherited” from DesignModeler. You can change this data if you wish. The Symmetry Normal entry must correspond to the Coordinate System entry. Symmetry in the Mechanical Application The following procedure describes the steps that you’ll use to implement feature during an analysis using the Mechanical Application. 1. Insert a Symmetry object in the tree. 2. Insert a Symmetry Region object, a Periodic Region object, or a Cyclic Region object to represent each symmetry plane you want to define. Refer to Symmetry Region (p. 336) to determine which object to insert. 3. For each Symmetry Region object or Periodic/Cyclic Region object, complete the following in the Details view: a. Scoping Method - Perform one of the following: • Choose Geometry Selection if you want to define a symmetry plane by picking in the Geometry window. Pick the geometry, then click on the entry field for Geometry Selection (labeled No Selection) and click the Apply button. For a Periodic/Cyclic Region object, perform the same procedure for the Low Boundary and High Boundary entries, where Low Boundary and High Boundary represent the two opposite face selections or edge selections on the different sides of the periodic sector of the model. Note A Symmetry Region object can only be scoped to a flexible body. • 352 Choose Named Selection if you want to define a symmetry plane using geometry that was pre-defined in a named selection. Click on the entry field for Named Selection and, from the drop down list, choose the particular named selection to represent the symmetry plane. For a Periodic/Cyclic Region object, you perform the same procedure, where Low Selection corresponds to the Low Boundary component and High Selection corresponds to the High Boundary component. b. Type - For a Symmetry Region or Periodic Region only, click on the entry field, and, from the drop down list, choose the symmetry type. Boundary conditions will be applied to the symmetry planes based on both the simulation type and the value you specify in the symmetry Type field. The Scope Mode read-only indication is Manual when you follow this procedure of defining symmetry directly in the Mechanical application. c. Coordinate System - Select an appropriate coordinate system from the drop down list. You must use a Cartesian coordinate system for a Symmetry Region and a cylindrical coordinate system Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application for a Periodic/Cyclic Region. See the Coordinate Systems section, Initial Creation and Definition, for the steps to create a local coordinate system. d. Symmetry Normal - For a Symmetry Region object only, specify the normal axis from the drop down list that corresponds to the coordinate system that you chose. The following example shows a body whose Symmetry Region was defined in the Mechanical application. Note You can select multiple faces to work with a symmetry region. For non-periodic/non-cyclic symmetry regions, all faces selected (or chosen through Named Selection folder) must have only one normal. For periodic/cyclic types, you should additionally choose the proper cylindrical coordinate system with the z-axis showing the rotation direction, similar to the Matched Face Mesh meshing option. The following example shows a body whose Periodic Region was defined in the Mechanical application. The following example shows a body whose Cyclic Region was defined in the Mechanical application. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 353 Features Note When using a Periodic/Cyclic Region, the mesher will automatically set up match face meshing on the opposite Low Boundary and High Boundary faces. A useful feature available when using a periodic/cyclic region is the ability to swap Low Boundary and High Boundary settings under Scope in the Details view. You accomplish this by clicking the right mouse button on the specific periodic/cyclic regions (Ctrl key or Shift key for multiple selections) and choosing Flip High/Low. Named Selections The Named Selection feature allows you to create groupings of similar geometry or meshing entities. The section describes the steps to create Named Selections objects and prepare them for data definition. Subsequent sections further define and build upon these techniques, and include: Defining Named Selections Displaying Named Selections Using Named Selections Displaying Interior Mesh Faces Converting Named Selection Groups to Mechanical APDL Application Components Create a Named Selection Object Creating Named Selections objects is easy and can be accomplished by several different methods, including: • 354 Select the Model object and click the Named Selection button on the Model Context Toolbar or select the Model object, right-click the mouse, and then select Insert>Named Selection. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application • Select desired geometry entities from the Geometry object, right-click the mouse, and then select Create Named Selection. • Select desired geometry entities in the graphical interface (bodies, faces, etc.- bodies are show below), right-click the mouse, and then select Create Named Selection. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 355 Features As illustrated below, these methods, by default, place a Named Selections folder object into the tree that includes a child object titled Selection. This Selection object, and any subsequent Selection objects that are inserted into the parent folder, require geometry or meshing entity scoping. If a direct selection method (via Geometry object or graphical selection) was used, the Geometry entities may already be defined. These Selection objects are the operable “named selections” of your analysis. You may find it beneficial to rename these objects based on the entities to which they are scoped or the purpose that they will serve in the analysis. For example, you may wish to rename a Named Selection containing edges to "Edges for Contact Region". 356 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Add Selection Objects If a Named Selections folder object exists in the tree, insert additional named Selection objects using the same methods as above: (1) click the Named Selection button on the Named Selection context toolbar or (2) when either the Named Selections parent folder object or another Selection object is highlighted, right-click the mouse and select Insert>Named Selection. Defining Named Selections This section describes the methods used to define the characteristics of your Named Selection, such as geometry, and includes: Specifying Named Selections by Geometry Type Specifying Named Selections by Direct Node Selection Specifying Named Selections using Worksheet Criteria Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 357 Features Specifying Named Selections by Geometry Type Once you create Named Selections/Selection objects, you need to define the geometry or node-based meshing entities that you would like to scope to the object. Scoping method options include: • Geometry - geometry-based or nodal-based entries/selections • Worksheet - criteria-based entries/selections. Use the steps shown below to define the Details of your Named Selections based on geometry types (body, face, edge, or vertex). To scope your Named Selection to nodes or by using the Worksheet, see one of the following sections: • Specifying Named Selections by Direct Node Selection (p. 358) • Specifying Named Selections using Worksheet Criteria (p. 362) Named Selections defined by geometry types: To define geometry-based named selections: 1. Highlight the Selection object in the tree. In the Details view, set Scoping Method to Geometry Selection. 2. Select the geometry entities in the graphics window to become members of the Named Selection. 3. Click in the Geometry field in the details view, then click the Apply button. The named selection is indicated in the graphics window. You can rename the object by right-clicking on it and choosing Rename from the context menu. Tip To allow the Named Selection criteria to be automatically generated after a geometry update, highlight the Named Selections folder object and set Generate on Refresh to Yes (default). This setting is located under the Worksheet Based Named Selections category. Note • If you change the Scoping Method from Geometry Selection to Worksheet, the original geometry scoping will remain until you select Generate. • For geometric entity Named Selections, a Named Selection object status can only be fully defined (check mark) if a valid geometry is applied, or suppressed (“x”) if either no geometry is applied or if all geometry applied to the Named Selection is suppressed. • For a Named Selection created using the Graphics Viewer, the selections must be manually updated after you change the geometry. Specifying Named Selections by Direct Node Selection You create node-based Named Selections in the graphical viewer by scoping selections to single nodes, a group of surface nodes, or a group of nodes across a geometry cross-section. To define node-based Named Selections: 1. 358 Generate a mesh by highlighting the Mesh object and clicking the Update button. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application 2. From the Select Type list, choose Select Mesh. 3. Choose the appropriate selection tool in the Select Mode list. See the Selection Modes section below. Note • The Vertex geometry selection option is the only selection option available to picks nodes. • When working with Line Bodies: Nodes can be selected using volume selection modes only (Box Volume Select or Lasso Volume Select). • When working with Line Bodies and Surface Bodies: it is recommended that you turn off the Thick Shells and Beams option (View>Thick Shells and Beams). This option changes the graphical display of the model’s thickness and as a result can affect how your node selections are displayed. 4. Select individual nodes or define the shape to select nodes. 5. Make sure that the cursor is in the graphic viewer and then right-click the mouse. Select Create Named Selection from the menu. 6. Type a name for the Named Selection and then click OK. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 359 Features Note • The Select All option in the RMB menu selects all surface nodes. • If you select a large number of nodes (order of magnitude: 10,000), you are prompted with a warning message regarding selection information time requirements. • Following a remesh or renumber, all nodes are removed from named selections. If named selections were defined with Scoping Method set to Worksheet and if the Generate on Remesh field was set to Yes in the Details view of the Named Selection folder, then the nodes are updated. Otherwise, node scoping does not occur and the named selection will be empty. Selection Modes Selects individual nodes or a group of nodes on the surface. Single Select Selects all the surface nodes within the box boundary for all the surfaces oriented toward the screen. Box Select Selects all the surface and internal nodes within the box boundary across the crosssection.The line of selection is normal to the screen. Box Volume Select 360 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Is similar to the Box Select mode. Selects surface nodes that occur within the shape you define for surfaces oriented toward the screen. Lasso Select Similar to Box Volume Select mode. Selects the nodes that occur within the shape you define. Lasso Volume Select Tip • To select multiple nodes, press the CTRL key or press the left mouse and then drag over the surface. You can also create multiple node groups at different locations using the CTRL key. • To select all internal and surface nodes, use the Box Volume Select or Lasso Select tool and cover the entire geometry within the selection tool boundary. Viewing Node Information You can view information such as location of the each selected node and a summary of the group of nodes in the Selection Information window. A brief description of the selected nodes is also available on the Status Bar of the application window. To view node id and location information: 1. Select the nodes you want to include in a Named Selection. 2. Click View>Windows >Selection Information The following options are available as drop-down menu items in the Selection Information window. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 361 Features Selection Information Field Description Coordinate System Updates the X,Y, and Z information based on the selected coordinate system. Show Individual and Summary Shows both the node Summary and information on each node. Show Individual Shows information related to each node. Show Summary Shows only a summary of selected nodes. For more information see the Selection Information Toolbar section. Specifying Named Selections using Worksheet Criteria As described in the Specifying Named Selections by Geometry Type (p. 358) section, you can specify the Worksheet as your Scoping Method. Worksheet data defines the criteria for Named Selections based on geometric or meshing entities. Each row of the worksheet performs a calculation for the specified criteria. If multiple rows are defined, the calculations are evaluated and completed in descending order. To define named selections using Worksheet criteria: 1. Highlight the Selection object. In the Details view, set Scoping Method to Worksheet. 2. As needed, right-click the mouse and select Add Row. 3. Enter data in the worksheet for specifying the criteria that will define a Named Selection. See the Worksheet Entries and Operation section below for specific entry information. 4. Click the Generate button located on the Worksheet, to create the Named Selection based on the specified criteria. Alternatively, you can right-click on the Named Selection object and choose Generate Named Selection from the context menu. Note • If you change the Scoping Method from Geometry Selection to Worksheet, the original geometry scoping will remain until you select Generate. • When you select Generate, and the generation fails to produce a valid selection, any prior scoping will be removed, and the Named Selection will not have any scoping associated with it. • If there is no indication that the worksheet has been changed and the Named Selection should be regenerated, you still may want to select Generate to ensure that the item is valid. • If a row inside the worksheet has no effect on the selection, there are no indications related to this. Worksheet Entries and Operation A sample worksheet is illustrated below. 362 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Once a row has been placed in the Worksheet, the right-click context menu actives options to Insert additional rows, Modify rows, and/or Delete rows. Criteria of the Worksheet is defined by making selections in the drop-down menus of the columns for each row. Certain values are read-only or they are only available as the result of other criterion being specified. The content of each Worksheet column is described below. Action column: • Add: Adds the information defined in the current row to information in the previous row, provided the item defined in the Entity Type column is the same for both rows. • Remove: Removes the information defined in the current row from information in the previous row, provided the geometry defined in the Entity Type column is the same for both rows. • Filter: Establishes a subset of the information defined in the previous row. • Invert: Selects all items of the same Entity Type that are not currently in the named selection. • Convert To: Changes the geometric Entity Type selected in the previous row. The change is in either direction with respect to the topology (for example, vertices can be converted “up” to edges, or bodies can be converted “down” to faces). When going up in dimensionality, the higher level topology is selected if you select any of the lower level topology (for example, a face will be selected if any of its edges are selected). You can also convert from a geometry selection (bodies, edges, faces, vertices) to mesh nodes. The nodes that exist on the geometry (that is, the nodes on a face/edge/vertex or nodes on and within a body) will be selected. Note The conversion from geometry selection to mesh nodes is analogous to using Mechanical APDL commands NSLK, NSLL, NSLA, and NSLV. Entity Type column: • Body • Face • Edge • Vertex • Mesh Node Criterion column: • Size - available when Entity Type = Body, Face, or Edge. • Type - available when Entity Type = Body, Face,Edge, or Mesh Node. • Location X • Location Y Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 363 Features • Location Z • Face Connections - available when Entity Type = Edge. • Radius - available when Entity Type = Face or Edge. Applies to faces that are cylindrical and edges that are circular. • Named Selection • Material • Node ID — Available when Entity Type is Mesh Node. Operator column: • Equal • Not Equal • Less Than • Less Than or Equal • Greater Than • Greater Than or Equal • Range includes Lower Bound and Upper Bound numerical values that you enter. Units column: read-only display of the current units for Criterion = Size or Location X, Y, or Z. Value column: • For Criterion = Size, enter positive numerical value. • For Criterion = Location X, Y, or Z, enter numerical value. Note Selection location is at the centroids of edges, faces, and bodies. • • • 364 For Criterion = Type and Entity Type = Body: – Solid – Surface – Line For Criterion = Type and Entity Type = Face: – Plane – Cylinder – Cone – Torus – Sphere – Spline – Faceted For Criterion = Type and Entity Type = Edge: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application • – Line – Circle – Spline – Faceted For Criterion = Type and Entity Type = Mesh Node: – Corner – Midside • For Criterion = Face Connections and Entity Type = Edge, enter the number of shared edge connections. For example, enter Value = 0 for edges not shared by any faces, enter Value = 1 for edges shared by one face, and so on. • For Criterion = Named Selection, you can include a previously-defined named selection from the Value field. Only the named selections that appear in the tree before the current named selection are listed in Value. For example, if you have defined two named selections prior to the current named selection and two named selections after, only the two prior to the current named selection are shown under Value. When you define a named selection to include an existing named selection, you should choose Generate Named Selections from the Named Selections folder object in the tree to ensure that all of the latest changes to all named selections are captured. Named selections are generated in the order listed in the tree. However, if you choose to generate only one named selection, no other named selections will be updated. • For Criterion = Material, select the desired material from the drop-down list. See the Material Property Assignment topic for more information. Lower Bound column: enter numerical value. Upper Bound column: enter numerical value. Coordinate System column: • Global Coordinate System • Any defined local coordinate systems Adjusting Tolerance Settings for Named Selections by Worksheet Criteria If you wish to adjust the tolerance settings for worksheet criteria, use the Tolerance settings in the Selection Details View. Tolerance values apply to the entire worksheet. By default, the zero tolerance is 1.e-008 and the relative tolerance is 1.e-003. By default, the zero tolerance is 1.e-008, which is past the number of significant digits that Mechanical shows by default. As a result, items can appear to be at zero but are not. Adjusting the tolerance settings manually can be useful in these situations, such as when the CAD units are very small dimensions (like micrometers). Setting the tolerance values manually can also be useful in meshing, when small variances are present in node locations and the default relative tolerance of .001 (.1 %) can be either too small (not enough nodes selected) or too big (too many nodes selected). 1. In the Details view, set Tolerance Type to Manual. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 365 Features 2. Specify either a Zero Tolerance or a Relative Tolerance. Tolerance values are dimensionless. Relative tolerance is a multiplying factor applied to the specified worksheet value. For example, if you want a tolerance of 1%, enter .01 in the Relative Tolerance field. All comparisons are done in the CAD unit system. Criteria Named Selections Based on Selected Geometry You may have the need to create Named Selections that use criteria but are based on pre-selected geometry. For example, the criteria may be to pick every face that shares both the same X location and the same size as the selected face. For these situations, you can first select the geometry, then, instead of configuring the Worksheet directly, you can use the following more direct procedure to define the criteria for the Named Selection. 1. After selecting geometry, choose Create Named Selection (left button on the Named Selection Toolbar (p. 298) or right-click context menu choice). 2. In the Selection Name dialog box that appears, you can enter a name for the particular Named Selection or accept Selection as the default name. a. To define the Named Selection based only on the selected geometry without defining any criteria, choose Apply selected geometry and choose OK. b. To define the Named Selection based on criteria related to the selected geometry, choose Apply geometry items of same:, then check one or more applicable criteria items and choose OK. These items are sensitive to the selected geometry (for example, if vertex is selected, there are no Size or Type entries). The Named Selection is automatically generated and listed as a Selection object (default name) under the Named Selections folder. If you specified criteria and highlight the Selection object, the associated Worksheet is populated automatically with the information you entered in the Selection Name dialog box. To illustrate the example presented above: 1. Select a face. 2. Choose Create Named Selection. 366 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application 3. Choose Apply geometry items of same: 4. Check Size and Location X, then choose OK. The Worksheet associated with the new Named Selection would be populated automatically with the following information: First Row • Action = Add • Entity Type = Face • Criterion = Size • Operator = Equal Second Row • Action = Filter • Entity Type = Face • Criterion = Location X • Operator = Equal Displaying Named Selections You can use geometry entity Named Selections to inspect only a portion of the total mesh. Although this feature is available regardless of mesh size, it is most beneficial when working with a large mesh (greater than 5 - 10 million nodes). After you have designated a Named Selection group, you can use any of the following features to assist you in this task: • Show Mesh object property in the Details view of the Named Selections folder object. By setting this property to Yes, if a mesh was generated, all items in the Named Selection groups within the Named Selections folder object are displayed in their meshed state. An example is shown below of a Named Selection that is comprised of 3 faces in their meshed display. • As illustrated below, selecting the Named Selection folder displays all of the user-defined Named Selection annotations in the Graphics pane. This display characteristic can be turned On or Off using the Show Annotation category in the Named Selections Details view. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 367 Features Selecting an individual Named Selection displays the annotation specific to that Named Selection in the Graphics pane. • Visible object property in the Details view of an individual Named Selection object (that is, a child object within the Named Selections folder object). By setting this property to No, the Named Selection can be made invisible meaning it will not be drawn and more importantly not taken into consideration for picking or selection. This should allow easier inspection inside complicated models having many layers of faces where the inside faces are hardly accessible from the outside. You can define Named Selections and make them invisible as you progress from outside to inside, similar to removing multiple shells around a core. The example shown below displays the same 3 Faces Named Selection where Visible has been set to No. • View> Wireframe in the Main Menu (p. 280). By displaying the model as a wireframe and setting the Named Selection Show Mesh to Yes, you can display an enhanced version of the meshed items in the Named Selection as shown below. 368 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Notes • The Visible option is different from the Hide or Suppress options in the right mouse button context menu. These two options will hide/suppress the full body containing a given Named Selection. However, the Visible option will hide only the specified Named Selection. • When a Named Selection's Visible setting is set to No: – Just the faces from that Named Selection are not drawn, but the edges are always drawn. – The Named Selection will not appear in any drawing of the geometry (regardless of which object is selected in the tree). Unless... – The Named Selection is displayed as meshed, it displays the mesh, but only if you have the Named Selection object or the Named Selections folder object selected in the tree. This behavior is the same as the behavior of the red annotation in the Geometry window for Named Selections (that is, the annotation appears only when the current selected object is the specific Named Selection object or the Named Selections folder object). • When the Wireframe option is specified, Named Selections (displayed as mesh) as well as the full geometry are drawn in wireframe, not just the meshes. • When the View> Wireframe option is set, just the exterior faces of the meshed models are shown, not the interior elements. • After at least one Named Selection is hidden, normally you can see the inside of a body, so displaying both sides of each face is enabled (otherwise displaying just the exterior side of each face is enough). But if a selection is made, the selected face is always displayed according to the option in Tools> Options> Mechanical> Graphics> Single Side (can be one side or both sides). • If the Wireframe display option is used and Show Mesh is Yes, any face selected is displayed according to the option in Tools> Options> Mechanical> Graphics> Single Side (can be one side or both sides). Using Named Selections This section describes available features for managing and employing Named Selections, including: Using Named Selections via the Toolbar Scoping Analysis Objects to Named Selections Including Named Selections in Program Controlled Inflation Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 369 Features Importing Named Selections Exporting Named Selections Using Named Selections via the Toolbar The Named Selection Toolbar can be turned on or off by selecting View> Toolbars> Named Selections. To use a Named Selection: 1. Select the name of the group in the Named Selection display in the Named Selection Toolbar. 2. Choose any of the following options that are available using the remaining controls in the Named Selection Toolbar: • Selection drop-down menu (or in context menu from a right mouse button click on individual Named Selection object): controls selection options on items that are part of the group whose name appears in the Named Selection display. – Select Items in Group: selects only those items in the named group. – Add to Current Selection: Selects items in the named group combined with other items that are already selected. This option is grayed out if the entity in the Named Selection does not match the entity of the other selected items. – Remove from Current Selection: Removes the selection of items in the named group from other items that are already selected. Selected items that are not part of the group remain selected. This option is grayed out if the entity in the Named Selection does not match the entity of the other selected items. Note Choosing any of these options affects only the current selections in the Geometry view, These options have no effect on what is included in the Named Selection itself. • Visibility drop-down menu: controls display options on bodies that are part of the group whose name appears in the Named Selection display. – Hide Bodies in Group: Turns off display of bodies in the named group (toggles with next item). Other bodies that are not part of the group are unaffected. – Show Bodies in Group: Turns on display of bodies in the named group (toggles with previous item). Other bodies that are not part of the group are unaffected. – Show Only Bodies in Group: Displays only items in the named group. Other items that are not part of the group are not displayed. You can also hide or show bodies associated with a Named Selection using a right mouse button click on the particular tree item under the Named Selections object and choosing Hide or Show from the context menu. • Suppression drop-down menu: controls options on items that affect if bodies of the group whose name appears in the Named Selection display are to be suppressed, meaning that, not only are they not displayed, but they are also removed from any treatment such as loading or solution. – 370 Suppress Bodies in Group: Suppresses bodies in the named group (toggles with next item). Other bodies that are not part of the group are unaffected. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application – Unsuppress Bodies in Group: Unsuppresses bodies in the named group (toggles with previous item). Other bodies that are not part of the group are unaffected. – Unsuppress Only Bodies in Group: Unsuppresses only bodies in the named group. Other bodies that are not part of the group are suppressed. You can also suppress or unsuppress bodies associated with a Named Selection using a right mouse button click on the particular tree item under the Named Selections object and choosing Suppress Bodies In Group or Unsuppress Bodies In Group from the context menu. The Suppress Bodies In Group and Unsuppress Bodies In Group options are also available if you select multiple Named Selection items under a Named Selections object. The options will not be available if your multiple selection involves invalid conditions (for example, if you want to suppress multiple items you have selected and one is already suppressed, the Suppress Bodies In Group option will not be available from the context menu. The status bar shows the selected group area only when the areas are selected. The group listed in the toolbar and in the Details View (p. 274) provides statistics that can be altered. Scoping Analysis Objects to Named Selections Many items can be scoped to Named Selections. Some examples are contact regions, mesh controls, loads, supports, and results. To scope an item to a Named Selection: 1. Insert or select the object/item in the tree. 2. Under the Details view, in the Scoping Method drop-down menu, choose Named Selection. 3. In the Named Selection drop-down menu, choose the particular name. Notes on scoping items to a Named Selection: • Only Named Selections valid for the given analysis object are displayed in the Named Selection dropdown menu. If there are no valid Named Selections, the drop-down menu is empty. No two Named Selections branches can have the same name. It is recommended that you use unique and intuitive names for the Named Selections. • If you change a Named Selection that is used by an item, the associated entities will update accordingly. • If you delete a Named Selection used by an item, the item becomes underdefined. • If all the components in a Named Selection cannot be applied to the item, the Named Selection is not valid for that item. This includes components in the Named Selection that may be suppressed. For example, in the case of a bolt pretension load scoped to cylindrical faces, only 1 cylinder can be selected for its geometry. If you have a Named Selection with 2 cylinders, one of which is suppressed, that particular Named Selection is still not valid for the bolt pretension load. Including Named Selections in Program Controlled Inflation By default, faces in Named Selections are not selected to be inflation boundaries when the Use Automatic Inflation control is set to Program Controlled. However, you can select specific Named Selections to be included in Program Controlled inflation. To do so: 1. Create a Named Selection. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 371 Features 2. Click the desired Named Selection in the tree and then in the Details view, set the Program Controlled Inflation option to Include. 3. In the mesh controls, set the Use Automatic Inflation control to Program Controlled. As a result, the Named Selection you chose in step 2 is selected to be an inflation boundary, along with any other faces that would have been selected by default. Importing Named Selections You can import geometric entity Named Selections that you defined in a CAD system or in DesignModeler. A practical use in this case is if you want the entities of the Named Selection group to be selected for the application of loads or boundary conditions. To import a Named Selection from a CAD system or from DesignModeler: 1. In the Geometry preferences, located in the Workbench Properties of the Geometry cell in the Project Schematic, check Named Selections and complete the Named Selection Key; or, in the Geometry Details view under Preferences, set Named Selection Processing to Yes and complete the Named Selection Prefixes field (refer to these entries under Geometry Preferences for more details). 2. A Named Selections branch object is added to the Mechanical application tree. In the Named Selection Toolbar, the name of the selection appears as a selectable item in the Named Selection display (located to the right of the Create Selection Group button), and as an annotation on the graphic items that make up the group. Exporting Named Selections You can export the Named Selection that you create using the Graphics Viewer and Worksheet, and save the contents to a text or Microsoft Excel file. To export the Named Selection object: • Right click the Named Selection object you want to export, and then click Export to save the file at the location you want. The text or Microsoft Excel file you export includes a list of generated node ids, by default. You can also include the location information of the generated node ids in the exported file. To include node id location information in the exported file: 1. Click Tools > Options 2. Expand the Mechanical folder, and then click Export 3. Under Export, click the Include Node Location drop-down list, and then select Yes. Note • The Named selection Export feature is available only for node based Named Selection objects. • Node Numbers are always shown in the exported text or Microsoft Excel file irrespective of setting for Include Node Numbers in Tools > Options > Export. Displaying Interior Mesh Faces There are special instances when a Named Selection is an interior “back-facing face”. This is a unique case that occurs when the external faces of the geometry are hidden allowing interior faces to become visible. 372 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application To display the faces of the mesh, the Named Selections object must be highlighted in the tree and the Show Mesh field under the Display category in the Details view must be set to Yes. Then, to correct the display, use the Draw Face Mode options available under View>Graphics Options, which include: • Auto Face Draw (default) - turning back-face culling on or off is program controlled. Using Section Planes is an example of when the application would turn this feature off. • Draw Front Faces - face culling is forced to stay on. Back-facing faces will not be drawn in any case, even if using Section Planes. • Draw Both Faces - back-face culling is turned off. Both front-facing and back-facing faces are drawn. Incorrect Display Correct Display using Draw Face Mode Converting Named Selection Groups to Mechanical APDL Application Components When you write a Mechanical APDL application input file that includes a Named Selection group, the group is transferred to the Mechanical APDL application as a component provided the name contains only standard English letters, numbers, and underscores. The Named Selection will be available in the input file as a Mechanical APDL component for use in a Commands object. Geometry scoping to bodies will result in an element based component. All other scoping types will result in a nodal component. The following actions occur automatically to the group name in the Mechanical application to form the resulting component name in the Mechanical APDL application: • A name exceeding 32 characters is truncated. • A name that begins with a number is renamed to include “C_” before the number. • Spaces between characters in a name are replaced with underscores. Example: The Named Selection group in the Mechanical application called 1 Edge appears as component C_1_Edge in the Mechanical APDL application input file. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 373 Features Note Named selections starting with ALL, STAT, or DEFA will not be sent to the Mechanical APDL application. Mesh Numbering The Mesh Numbering feature allows you to renumber the node and element numbers of a generated meshed model consisting of flexible parts. The feature is useful when exchanging or assembling models and could isolate the impact of using special elements such as superelements. The Mesh Numbering feature is available for all analysis systems except Rigid Dynamics analyses. To activate Node Number Compression: By default node numbers will not be compressed to eliminate gaps in the numbering that can occur from events such as remeshing or suppression of meshed parts. This allows maximum reuse of mesh based Named Selections but can result in node numbers that are higher than required. Node number compression can be turned on by setting Compress Numbers to Yes. If compression is turned on, the compression will occur before any other numbering controls are applied. To activate Mesh Numbering: 1. Insert a Mesh Numbering folder by highlighting the Model folder, then: a. Selecting the Mesh Numbering toolbar button. Or... b. Right-clicking on the Model folder and choosing Insert> Mesh Numbering. Or... c. Right-clicking in the Geometry window and choosing Insert> Mesh Numbering. 2. In the Details view, set Node Offset or Element Offset values for the entire assembly, as needed. For example, specifying a Node Offset of 2 means that the node numbering for the assembly will start at 2. 3. Insert a Numbering Control object by highlighting the Mesh Numbering folder (or other Numbering Control object), then: a. Selecting the Numbering Control toolbar button. Or... b. Right-clicking on the Mesh Numbering folder (or other Numbering Control object) and choosing Insert> Numbering Control. Or... c. 4. Right-clicking in the Geometry window and choosing Insert> Numbering Control. Specify a part, a vertex, or a Remote Point in the model whose node or element numbers in the corresponding mesh are to be renumbered. a. To specify a part: i. 374 Select the part. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application b. c. 5. ii. In the Details view, set Scoping Method to Geometry Selection, click the Geometry field and click Apply. iii. Enter numbers in the Begin Node Number and/or Begin Element Number fields. Also, if needed, change the End Node Number and End Element Number from their default values. To specify a vertex: i. Select the vertex. ii. In the Details view, set Scoping Method to Geometry Selection, click the Geometry field and click Apply. iii. Enter the Node Number. To specify a Remote Point that has already been defined: i. In the Details view, set Scoping Method to Remote Point, click the Remote Points field and choose the specific Remote Point in the drop down menu. ii. Enter the Node Number. Right-click the Mesh Numbering folder, or a Numbering Control object, and choose Renumber Mesh. If the model is not meshed, it will first generate a mesh and then perform mesh numbering. The nodes and elements are numbered based on the values that you specified. Note During the mesh numbering process, the user interface enters a waiting state, meaning you cannot perform any actions such as clicking objects in the tree. In addition, you cannot cancel the process once it is started and must wait for its completion. However, a progress dialog box appears to report status during the operation. Mesh Numbering Characteristics • The Mesh Numbering feature is available in both the Mechanical application and the Meshing applications. • Geometry selection is part-based, not body-based. • Selecting Update at the Model level in the Project Schematic updates the mesh renumbering. • The Solve is aborted if mesh renumbering fails. • Whenever a control is changed, added, or removed, the mesh renumbering states are changed for all controls where mesh numbering is needed. • When exporting mesh information to Fluent, Polyflow, CGNS, or ICEM CFD format, the last status is retained at the time of export. If renumbering has been performed, the mesh is exported with nodes and elements renumbered. If not, the original mesh numbering is used. • Mesh renumbering of a Point Mass is not supported. • The Convergence object is not supported with Mesh Numbering folder. Note Be cautious when deleting the Mesh Numbering folder. Deleting this folder leaves the mesh in the numbered state that you specified. There is no way to know that the existing mesh has been renumbered. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 375 Features Path (Construction Geometry) A path is categorized as a form of construction geometry and is represented as a spatial curve to which you can scope path results. The results are evaluated at discrete points along this curve. A path can be defined in two principal ways: • By start point and end point. These points can be specified directly or can be calculated from the entry and exit point (intersections) of the positive X-axis of a coordinate system through a mesh. The path may be a straight line segment or a curve depending on the type of coordinate system (Cartesian or Cylindrical). You can control the discretization by specifying the number of sampling points, and these will be evenly distributed along the path up to a limit of 200. Note Paths defined in this manner will only be mapped onto solid or surface bodies. If you wish to apply a path to a line body you must define the path by an edge (as described below). • By an edge. The discretization will include all nodes in the mesh underlying the edge. Multiple edges may be used but they must be continuous. For each result scoped to a Path, the Graph Controls category provides an option to display the result in the Graph on X-axis, as a function of Time or with S, the length of the path. Note that Path results have the following restrictions: They are calculated on solids and surfaces but not on lines. They can be collected into charts as long as all of the other objects selected for the chart have the same X-axis (Time or S). You can define a path in the geometry by specifying two points, an edge, or an axis. Before you define a path, you must first add the Path object from the Construction Geometry context toolbar. You can then define the path using any of the three methods presented below. Defining a Path using Two Points Using this method you define the path by specifying two points in any of the following ways: 376 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application To define the path using the Coordinate toolbar button: 1. In the Details view, select Two Points in the Path Type list. 2. Under Start, choose Click to Change in the Location row . 3. Depress the Coordinate toolbar button. As you move the cursor across the model, the coordinates display and update as you reposition the cursor. 4. Click at the desired start location for the path. A small cross hair appears at this location. You can click again to change the cross hair location. 5. Click Apply. A “1” symbol displays at the start location. Also, the coordinates of the point display in the Details view. You can change the location by repositioning the cursor, clicking at the new location, and then clicking Click to Change and Apply, or by editing the coordinates in the Details view. 6. Repeat steps 2 through 5 to define the end point of the path under End in the Details view. A “2” symbol displays at the end location. 7. Enter the Number of Sampling Points. To define the path using coordinates: 1. In the Details view, select Two Points in the Path Type list. 2. Under Start, enter the X, Y, and Z coordinates for the starting point of the path. 3. Under End, enter the X, Y, and Z coordinates for the ending point of the path. 4. Enter the Number of Sampling Points. To define a Path using a vertex, edge or face: 1. In the Details view, select Two Points in the Path Type list. 2. Select a vertex, edge or face where you want to start the path, and then click Apply under Start, Location. 3. Select a vertex, edge, or face where you want to end the path, and then click Apply under End, Location. 4. Enter the Number of Sampling Points. Note The start and end points need not both be specified using the same procedure of the three presented above. For example, if you specify the start point using the Coordinate toolbar button, you can specify the end point by entering coordinates or by using a vertex, edge, or face. Any combination of the three procedures can be used to specify the points. Snap to Mesh Nodes When solving linearized stresses, the path you define by two points must be contained within the finite element mesh to avoid an error. Because the two points can be derived from the tessellation of the geometric model, the points may be contained within the geometry but may not be contained within the mesh. This is especially true for curved geometry faces. After defining the two points using the Coordinate toolbar button method (see above), you can ensure that the path is contained within the mesh by using the Snap to mesh nodes feature. To use the feature, set Show Mesh to Yes in the Details Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 377 Features view of the Path object in order to see the location of the nodes in the mesh. Then, right click on the Path object and select Snap to mesh nodes from the context menu. This action alters the path, as necessary, such that both the start point and end point of the path snap to the closest node in the mesh. The Snap to mesh nodes feature avoids the error and allows the solve to continue provided the path you define does not traverse through any discontinuities in the model, such as a hole. For these cases, even though the Snap to mesh nodes feature alters the path endpoints to coincide with the nearest nodes in the mesh, the linearized stress result still fails because the path is defined through the discontinuity. The following pictures illustrate this feature. Attempt to solve for linearized stress. Path defined within geometric model: Corresponding mesh used for geometric model, obtained by setting Show Mesh to Yes: 378 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Path contained within mesh after choosing Snap to mesh nodes. Solution completes: Note If the model is re-meshed after choosing Snap to mesh nodes, the feature is not automatically applied to the newly meshed model. You must choose Snap to mesh nodes again to alter the path start and end points to the new mesh. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 379 Features Defining a Path using an Edge This method helps you define a path by selecting an edge. To define a path: 1. In the Details view, select Edge in the Path Type list. 2. Select a geometry edge, and then click Apply under Scope. Defining a Path from Results Scoped to Edges In order to help better quantify the variation of a result along a set of edges, path results are available. For a result that is scoped to an edge or multiple contiguous edges, you can convert the scoping to the equivalent Path, by: 1. Selecting the result object that is scoped to an edge or contiguous edges. 2. Display the context menu by right-clicking the mouse, and the select Convert To Path Result. A Path is automatically created and a corresponding Path object is displayed in the tree with a Path Type of Edge. Defining a Path using X-axis Intersection Depending on the coordinate system you select, Workbench creates a Path from the coordinate system origin to the point where the X-axis of the selected coordinate system intersects a geometry boundary. Workbench computes intersections of the axis with the mesh and displays more precise locations for path endpoints for the path results. The endpoints for the path are not modified, and remain as the intersections with the geometry. The first compact segment of the path inside a single body is included in the path definition. 1. In the Details view, select X Axis Intersection in the Path Type list. 2. Select the coordinate system you want to use to define the x-axis. 3. Enter the Number of Sampling Points. Defining a Path from Probe Labels While reviewing results, you can define a path automatically from two probe labels. To define the path: 1. Create two probe annotations by choosing the Probe button from the Result Context Toolbar (p. 291). 2. Choose the Label button from the Graphics Toolbar (p. 285) and select the two probe annotations. (Hold Ctrl key to select both probe annotations.) 3. Right-click in the Geometry window and choose Create Path From Probe Labels from the context menu. 4. A path is automatically created between the probe annotations. A corresponding Path object is displayed in the tree with a Path Type of Two Points. Exporting Path Data You can export coordinate data for a defined path by clicking the right mouse button on a Path object and choosing Export from the context menu. 380 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Surface (Construction Geometry) A surface is categorized as a form of construction geometry and is represented as a section plane to which you can scope surface results. To define a surface: 1. Highlight the Model object and click the Construction Geometry toolbar button to produce a Construction Geometry object. 2. Highlight the Construction Geometry object and click the Surface toolbar button to produce a Surface object. 3. Define a coordinate system whose X-Y plane will be used as a cutting plane, as follows: a. Create a local coordinate system. b. Define the origin of the local coordinate system. Note With respect to the facets of the surface: • For a Cartesian coordinate system, the surface is the intersection of the model with the X-Y plane of the coordinate system. • For a cylindrical coordinate system, the surface is the intersection of the model with the cylinder whose axis is the Z axis of the coordinate system. In this case, you must specify the radius in the Details view of the Surface object. Remote Point The following topics are addressed in this section: Remote Point Overview Connection Lines Promote Remote Point Remote Point Commands Objects Remote Point Overview You use a Remote Point as a scoping mechanism for remote boundary conditions. Remote points are a way of abstracting connection to geometry. They are similar to the various remote loads available in the Mechanical application (displayed in the list below). Remote points provide a way to establish a point in space associated to a portion of geometry that can have multiple boundary conditions scoped to it. The single remote association will avoid overconstraint conditions that can occur when multiple remote loads are scoped to the same geometry. The overconstraint occurs because multiple underlying contact elements are used for the individual remote loads when applied as usual to the geometry. When the multiple remote loads are applied to a single remote point scoped to the geometry the possibility of overconstraint is greatly reduced. To insert a Remote Point, select a Model branch and either select the Remote Point button from the toolbar, or right-click the mouse and select Insert> Remote Point from the context menu. You then apply it to: • A face, edge, or vertex of a solid body or of a 3D surface body. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 381 Features • An edge or vertex of a 2D surface body or a line body. A remote point or multiple remote points work in tandem with the remote boundary conditions listed below. Remote Point definable settings include a Geometry selection, a Coordinate System, Location, Behavior (Deformable or Rigid) as well as a Pinball Region. • Point Mass • Thermal Point Mass • Joints • Springs • Remote Displacement • Remote Force • Moment These objects acquire data from remote points and eliminate the need to define the objects individually. You can scope one or more of the above objects to a defined Remote Point. This provides a central object to which you can make updates that will affect the scoping of multiple objects. Note Following are important points to keep in mind when using Remote Points: • A Remote Point can reference only one Remote Force and one Moment. If you scope a Remote Point to multiple remote forces or moments, duplicate specifications are ignored and a warning message is generated. • A Remote Point with Deformable behavior should not be used on surfaces that are modeled with symmetry boundary conditions. The internally generated weight factors only account for the modeled geometry. Therefore, remote points with deformable behavior should only be used on the “full” geometry. The Details view of each of the above objects contains a Scoping Method setting that can be set to Remote Point, once a Remote Point is defined, as illustrated below for the details of a Remote Force. Once you scope the object with a Remote Point and define which remote point (Remote Point or Remote Point2) if more than one exists, all of the inputs from that remote point become read-only for the object and use the remote point's data. Scope to Remote Point 382 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Choose Appropriate Remote Point Example Data for Selected Remote Point Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 383 Features Once a remote force is directed to a Remote Point, additional data may be required, such as Magnitude, as shown above. Connection Lines The connection between the underlying geometry associated with a remote point and the remote point itself can be visualized by connection lines. You can enable this feature through the Show Connection Lines property under Graphics in the Details view of the Remote Points object. If a mesh was generated, the connection lines are drawn between a remote point and the nodes on the corresponding meshed underlying geometry. The connection lines take the Pinball radius into account, and only those nodes that are inside that radius will be connected with the remote point. Any remote loads that have been promoted to reference remote points will have these lines drawn when their object is selected as well. An example illustration of connection lines is shown below. 384 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Promote Remote Point The Promote Remote Point feature helps you add a remote point from the context menu for remote boundary conditions. When you use Promote Remote Point, Workbench adds a remote point object with the remote boundary condition name and the associated data in the Project tree. To add a remote point from the remote boundary conditions: 1. On the Environment context toolbar, click the appropriate boundary condition. 2. Right-click the remote boundary condition object, and then click Promote Remote Point. A remote point with the boundary condition name and data is added to the Project tree. 3. In the Project tree, select the new remote point object and modify its data as necessary. Remote Point Commands Objects A Commands object can be placed in the tree as a child object of a Remote Point providing you programmable access to the Remote Point pilot node. This is useful if you wish to apply conditions to the Remote Point that are not supported in Workbench, such as beam or constraint equations. Point Mass You can idealize the inertial effects from a body using a Point Mass. Applications include applying a force with an acceleration or any other inertial load; or adding inertial mass to a structure, which affects modal and harmonic solutions. To insert a Point Mass, select a Geometry branch and either choose Point Mass from the toolbar, or right mouse button click and choose Insert> Point Mass from the context menu. You then apply it on a face of a solid or surface model, or on an edge of a surface model. You cannot apply a Point Mass on any shared topology surface. Also, the scoping of a Point Mass cannot span multiple bodies if the Stiffness Behavior of the bodies is declared as Rigid (see Rigid Bodies section for additional information). The location of the Point Mass can be anywhere in space and can also be defined in a local coordinate system if one exists. The default location is at the centroid of the geometry. The Point Mass will automatically be rotated into the selected coordinate system if that coordinate system differs from the global coordinate system. You can also input moment of inertia values for each direction. A Point Mass is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 628) section for a listing of all remote boundary conditions and their characteristics. Note This boundary condition cannot be applied to a vertex scoped to an end release. Thermal Point Mass For transient thermal analyses, you can idealize the thermal capacitance of a body using a thermal point mass. Thermal Capacitance replaces the need to calculate the body's internal thermal gradient. The Thermal Point Mass is commonly used as a medium to store or draw heat from surrounding objects. Applications includes the heat dissipation of refrigerators, cooling electronic devices, and heat sinks of computer motherboards. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 385 Features To insert a Thermal Point Mass object in a transient thermal analysis, select a Geometry branch and either choose Thermal Point Mass from the toolbar, or right-click and choose Insert> Thermal Point Mass from the context menu. You then apply it on a face/edge/vertex of a solid or surface model, or on an edge/vertex of a surface model. You cannot apply a Thermal Point Mass on any shared topology surface. The location of the Thermal Point Mass can be anywhere in space. The default location is at the centroid of the geometry. You can also input Thermal Capacitance in the Details view. Thermal capacitance refers to ability of material to store heat. The higher the thermal capacitance, the more heat can be stored for each degree rise in temperature of the Thermal Point Mass. The Thermal Point Mass includes two Behavior options in the Details View that control its interaction with the bodies in the geometry selection: Isothermal and Heat-Flux Distributed: • In the Isothermal behavior, temperatures throughout the geometry selections and the Thermal Point Mass are constrained to be the same. The following is an example of a Thermal Point Mass using Isothermal behavior applied to the FACE while a temperature boundary condition is located at the EDGE. While there is a temperature distribution from the boundary condition (EDGE) up to the surface (FACE), the temperature on the FACE in the pinball region, itself takes a single value that matches that of the Thermal Point Mass. • For Heat-Flux Distributed behavior, however, the temperature of the geometry selection and the point mass are not constrained to be the same. The temperature of the Thermal Point Mass becomes a weighted average of those on the geometry selection. For comparison, the previous example has been modified to use the Heat-Flux Distributed behavior. The FACE, no longer constrained to be isothermal to the point mass, displays a gradient. Resembling Point Mass, Thermal Point Mass is classified as a remote boundary condition, meaning the boundary condition is not applied directly on node(s) of a body. Refer to the Remote Boundary Conditions (p. 628) section for a listing of all remote boundary conditions and their characteristics. 386 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry in the Mechanical Application Note This boundary condition cannot be applied to a vertex scoped to an end release. Using Gaskets Gasket joints are essential components in most structural assemblies. Gaskets as sealing components between structural components are usually very thin and made of various materials, such as steel, rubber and composites. From a mechanics perspective, gaskets act to transfer force between components. The primary deformation of a gasket is usually confined to one direction, namely, through thickness. The stiffness contributions from membrane (in plane) and transverse shear are much smaller in general compared to the through thickness. A typical example of a gasket joint is in engine assemblies. A thorough understanding of the gasket joint is critical in engine design and operation. This includes an understanding of the behavior of gasket joint components themselves in an engine operation, and the interaction of the gasket joint with other components. The overall procedure for simulating gaskets in ANSYS Workbench is to run a static structural analysis and perform the following specialized steps: 1. Specify a material with a valid gasket model in Engineering Data. 2. Set the Stiffness Behavior of the Body object to Gasket. This produces a Gasket Mesh Control object beneath the Body object. 3. Adjust Details view settings for the Gasket Mesh Control object and generate the mesh. 4. Solve and review the gasket result. Refer to the following sections for further details. Gasket Bodies Gasket Mesh Control Gasket Results Gasket Bodies You can conveniently specify a solid body to be treated as a gasket by settings its Stiffness Behavior to Gasket. A Gasket body will be meshed with special elements that have a preferential or sweep direction. The mesh will consist of a single layer of solid elements with all mid-side nodes dropped along this direction. You must also specify a material with a valid gasket model in Engineering Data. The following restrictions apply to Gasket bodies: • Gasket bodies are valid only in static structural analyses. • Gasket bodies are valid for 3-D solids only, that is, 2-D gasket bodies cannot be specified. • A valid gasket material model must be specified. • In addition to gasket bodies, a multibody part may also include flexible bodies but not rigid bodies. Gasket Mesh Control Upon specifying a Gasket body, a Gasket Mesh Control object is added beneath the Body object in the tree. The meshing method for the control will be set to sweep and allow you to indicate the sweep Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 387 Features direction. This control instructs the application to drop mid-side nodes on gasket element edges that are parallel to the sweep direction. To use gasket element meshing after setting the 3-D Body object's Stiffness Behavior to Gasket: 1. In the Details view of the Gasket Mesh Control object, ensure that Mesh Method is set to Sweep and Src/Trg Selection is set to Manual Source. These are the default settings. 2. Select a Source face. The selected face must lie on the gasket body. 3. The Target selection is Program Controlled by default. If desired, you can set Src/Trg Selection to Manual Source and Target. Then you can choose Target manually. 4. If desired, you can change the value of the Free Face Mesh Type control to All Quad, Quad/Tri, or All Tri. When generating the gasket element mesh, the application drops the midside nodes on the edges that are parallel to the sweep direction. For example, consider the mesh shown below. To define the sweep method, Src/Trg Selection was set to Manual Source; one face (the “top” face) was selected for Source. In the resulting mesh, the gasket element faces on the source and target are quadratic, but the faces on the sides are linear. Note When Element Midside Nodes is set to either Program Controlled or Kept results in quadratic elements with midside nodes are dropped in the normal direction. When Element Midside Nodes is set to Dropped the midside nodes are dropped, resulting in linear elements. Gasket Results Specialized results are available for analyzing gaskets. See Gasket Results (p. 682) for details. 388 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Coordinate Systems Overview Coordinate Systems Overview All geometry in the Mechanical application is displayed in the global coordinate system by default. The global coordinate system is the fixed Cartesian (X, Y, Z) coordinate system originally defined for a part. In addition, you can create unique local coordinate systems to use with springs, joints, various loads, supports, and result probes. Cartesian coordinates apply to all local coordinate systems. In addition, you can apply cylindrical coordinates to parts, displacements, and forces applied to surface bodies. Note Cylindrical coordinate systems are not supported by the Explicit Dynamics solvers, but may be used for some postprocessing operations. The following topics are covered in this section: Creating Coordinate Systems Importing Coordinate Systems Applying Coordinate Systems as Reference Locations Using Coordinate Systems to Specify Joint Locations Creating Section Planes Transferring Coordinate Systems to the Mechanical APDL Application Creating Coordinate Systems The following topics involve the creation of local coordinate systems: Initial Creation and Definition Establishing Origin for Associative and Non-Associative Coordinate Systems Setting Principal Axis and Orientation Using Transformations Initial Creation and Definition Creating a new local coordinate system involves adding a Coordinate System object to the tree and addressing items under the Definition category in the Details view. To create and define a new local coordinate system: 1. Highlight the Coordinate Systems folder in the tree and choose the Coordinate Systems button from the toolbar or from a right mouse click (Insert> Coordinate System). A Coordinate System object is inserted into the tree. The remainder of the toolbar buttons involve the use of transformations discussed in a later section. 2. In the Details view Definition group, set the following: • Type: to Cartesian or Cylindrical. • Coordinate System: to Program Controlled or Manual. This assigns the coordinate system reference number (the first argument of the Mechanical APDL LOCAL command). Choose Program Controlled to have the reference number assigned automatically, or choose Manual to assign a particular Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 389 Features reference number in the Coordinate System ID field for identification or quick reference of the coordinate system within the input file. You should set the Coordinate System ID to a value greater than or equal to 12. If you create more than one local coordinate system, you must ensure that you do not duplicate the Coordinate System ID. Establishing Origin for Associative and Non-Associative Coordinate Systems After creating a local coordinate system, you can further designate it as being associative or non-associative with geometry and define its origin. • An associative coordinate system remains joined to the face or edge on which it is applied throughout preprocessing. Its position and orientation is thus affected by modifications to the geometry during updates and use of the Configure tool. The coordinate system does not follow the geometry and its mesh during solution. • A non-associative coordinate system is independent of any geometry. You establish the origin for either an associative or non-associative coordinate system in the Origin category in the Details view. To establish the origin for an associative coordinate system: 1. In the Details view Origin group of a Reference Coordinate System, set Define By to Geometry Selection. For a Reference Coordinate System attached to a joint, work with the Orientation About Principal Axis group to make the coordinate system associative. 2. Select a vertex or vertices, edge, face, cylinder, circle, or circular arc. 3. Choose Click to Change in the Geometry row. 4. Click Apply. A coordinate system symbol displays at the origin location as determined by the following: • Select a vertex. The origin will be on the vertex. • Select multiple vertices. The origin will be at the center of the area or volume enclosed by the selected vertices. • Select a face or an edge. The origin will be at the centroid of the face or edge. • Select a cylinder. The origin will be at the center of the cylinder. • Select a circle or a circular arc. The origin will be at the center of the circle or circular arc. Preselecting one or more topologies and then inserting a Coordinate System will automatically locate its origin as stated above. To establish the origin for a non-associative coordinate system: • In the Details view Origin group, set Define By to Global Coordinates. You then define the origin in either of the following ways: • 390 Selecting any point on the exterior of the model: 1. Set Define By to Global Coordinates. 2. Choose Click to Change in the Location row. 3. Depress the Coordinate toolbar button. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Coordinate Systems Overview • 4. Move the cursor across the model and notice that the coordinates display and update as you reposition the cursor. 5. Click at the desired origin location. A small cross hair appears at this location. You can click again to change the cross hair location. 6. Click Apply. A coordinate system symbol displays at the origin location. Also, the coordinates display in the Details view. You can change the location by repositioning the cursor, clicking at the new location, and then clicking Click to Change and Apply, or by editing the coordinates in the Details view. Entering the coordinates directly in the Details view. 1. Set Define By to Global Coordinates. 2. Type the Origin X, Y, Z coordinates. The origin will be at this location. Setting Principal Axis and Orientation The definition of the coordinate system involves two vectors, the Principal Axis vector and the Orientation About Principal Axis vector. The coordinate system respects the plane formed by these two vectors and aligns with the Principal Axis. Use the Principal Axis category in the Details view to define one of either the X, Y, or Z axes in terms of a: • Geometry Selection - Associatively align axis to a topological feature in the model. When a change occurs to the feature, the axis automatically updates to reflect the change. • Fixed Vector – Depending upon the Geometry Selection, this option preserves the current Geometry Selection without associativity. When a change occurs to the feature the axis will not update automatically to reflect that change. • Global X, Y, Z axis – Force the axis to align to a global X, Y, or Z axis. Use the Orientation About Principal Axis category in the Details view to define one of the orientation X, Y, or Z axes in terms of the Default, Geometry Selection, the Global X, Y, Z axes, or Fixed Vector. Using Transformations Transformations allow you to “fine tune” the original positioning of the coordinate system. Options are available for offsetting the origin by a translation in each of the x, y and z directions, as well as by rotation about each of the three axes. Flipping of each axis is also available. To exercise transformations, you use buttons on the Coordinate Systems toolbar and settings in the Transformations category in the Details view . To transform a coordinate system: 1. Choose a transformation (translation, rotation, or flip) from the Coordinate Systems toolbar. Entries appear in the Details view as you add transformations. 2. Enter information in the Details view for each transformation. 3. If required: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 391 Features • Reorder a transformation by highlighting it in the Details view and using the Move Transform Up or Move Transform Down toolbar button. • Delete a transformation by highlighting it in the Details view and using the Delete Transform toolbar button. Importing Coordinate Systems Coordinate systems defined when geometry is imported from DesignModeler, Creo Parametric, or SolidWorks will automatically be created in the Mechanical application. For more information, see the Attaching Geometry section under DesignModeler, or see the Notes section under Creo Parametric or SolidWorks in the CAD Integration section of the ANSYS Workbench help. If you update the model in the Mechanical application, coordinate systems from these products are refreshed, or newly defined coordinate systems in these products are added to the model. If a coordinate system was brought in from one of these products but changed in the Mechanical application, the change will not be reflected on an update. Upon an update, a coordinate system that originated from DesignModeler, Creo Parametric, or SolidWorks will be re-inserted into the object tree. The coordinate system that was modified in the Mechanical application will also be in the tree. Applying Coordinate Systems as Reference Locations Any local coordinate systems that were created in the Mechanical application, or imported from DesignModeler, Creo Parametric, or SolidWorks, can be applied to a part, or to a Point Mass, Spring, Acceleration, Standard Earth Gravity, Rotational Velocity, Force, Bearing Load, Remote Force, Moment, Displacement, Remote Displacement, or Contact Reaction. This feature is useful because it avoids having to perform a calculation for transforming to the global coordinate system. To apply a local coordinate system: 1. Select the tree object that represents one of the applicable items mentioned above. 2. For an Acceleration, Rotational Velocity, Force, Bearing Load, or Moment, in the Details view, set Define By, to Components, then proceed to step 3. For the other items, proceed directly to step 3. 3. In the Details view, set Coordinate System to the name of the local coordinate system that you want to apply. The names in this drop-down list are the same names as those listed in the Coordinate Systems branch of the tree outline. Note If you define a load by Components in a local coordinate system, changing the Define By field to Vector will define the load in the global coordinate system. Do not change the Define By field to Vector if you want the load defined in a local coordinate system. Using Coordinate Systems to Specify Joint Locations Whenever you create a joint, an accompanying reference coordinate system is also created. The intent of this coordinate system is for positioning the joint. See the Joint Properties and Application (p. 442) section for further details. 392 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Coordinate Systems Overview Creating Section Planes For viewing purposes, you can use the Create Section Plane option to slice the graphical image of your model based on a predefined coordinate system. Note The Section Plane feature does not support Cylindrical Coordinate Systems. 1. Select the desired Coordinate Systems object. The User-Defined Coordinate System illustrated here slices the model along the X-Y plane. 2. Right-click the mouse and select Create Section Plane. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 393 Features As illustrated here, the model is sliced based on the User-Defined Coordinate System. 394 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Coordinate Systems Overview Note This option is also available for Coordinate System objects in the Meshing Application. Transferring Coordinate Systems to the Mechanical APDL Application You can transfer coordinate systems to the Mechanical APDL application using any of the following methods: • Main Menu> Tools > Write Input File... • Load the Mechanical APDL application. • Commands Objects Any coordinate system defined in the Mechanical application and sent to the Mechanical APDL application as part of the finite element model, will be added to the Mechanical APDL application input file as LOCAL commands. For example: /com,*********** Send User Defined Coordinate System(s) *********** local,11,0,0.,0.,0.,0.,0.,0. local,12,1,11.8491750582796,3.03826387968126,-1.5,0.,0.,0. csys,0 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 395 Features Graphics The following topics are covered in this section: Annotations Lighting Controls Comments, Images, Figures Annotations Basics (p. 396) Highlight and Selection Graphics (p. 396) Scope Graphics (p. 397) Annotation Graphics and Positioning (p. 397) Environment Annotations (p. 398) Rescaling Annotations (p. 398) Solution Annotations (p. 399) Message Annotations (p. 400) Basics Annotations provide the following visual information: • Boundary of the scope region by coloring the geometry for edges, faces or vertices. • An explicit vertex within the scope. • A 3D arrow to indicate direction, if applicable. • Text description or a value. • A color cue (structural vs. thermal, etc.). Note The custom annotations you add using Label remain visible even when you suppress the body. Highlight and Selection Graphics You can interactively highlight a face. The geometry highlights when you point to it. 396 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Graphics See Graphical Selection (p. 241) for details on highlighting and selection. Scope Graphics In general, selecting an object in the Tree Outline (p. 235) displays its Scope by painting the geometry and displays text annotations and symbols as appropriate. The display of scope via annotation is carried over into the Report Preview (p. 864) if you generate a figure. Contours are painted for results on the scoped geometry. No boundary is drawn. Annotation Graphics and Positioning A label consists of a block arrow cross-referenced to a color-coded legend. For vector annotations, a 3D arrow originates from the tip of the label to visualize direction relative to the geometry. Figure: Annotation of a force on a face Use the pointer after selecting the Label toolbar button the annotation to a different location within the scope. for managing annotations and to drag • If other geometry hides the 3D point (e.g. the point lies on a back face) the block arrow is unfilled (transparent). • The initial placement of an annotation is at the pick point. You can then move it by using the Label toolbar button for managing annotations. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 397 Features • Drag the label to adjust the placement of an annotation. During the drag operation the annotation moves only if the tip lies within the scope. If the pointer moves outside the scope, the annotation stops at the boundary. Environment Annotations With an environment object selected in the Tree Outline (p. 235), an annotation for each load and support appears on the geometry (limit 10, based on selection in tree): The scope of loads and supports is usually displayed. Rescaling Annotations This feature modifies the size of annotation symbols, such as load direction arrows, displayed in the Mechanical application. For example, and as illustrated below, you can reduce the size of the pressure direction arrow when zooming in on a geometry selection. To change the size of an annotation, click the Rescale Annotation toolbar button ( 398 ). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Graphics Solution Annotations Solution annotations work similar to Environment Annotations (p. 398). The Max annotation has red background. The Min annotation has blue background. Probe annotations have cyan backgrounds. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 399 Features Figure: Max and Min annotations and two "probe" annotations: • By default, annotations for Max and Min appear automatically for results but may be controlled by buttons in the Result Context Toolbar (p. 291). • You may create "probe" annotations by clicking in the Result Context Toolbar (p. 291). Probe annotations show the value of the result at the location beneath the tip, when initially constructed. When probe annotations are created, they do not trigger the database to be marked as save being needed (i.e. you will not be prompted to save). Be sure to issue a save if you wish to retain these newly created probe annotations in the database. Changes to the unit system deletes active probe annotations. In addition, probe annotations are not displayed if a Mechanical application database is opened in a unit system other than the one in which it was saved; however, the probe annotations are still available and display when the Mechanical application database is opened in the original unit system. • If you apply a probe annotation to a very small thickness, such as when you scope results to an edge, the probe display may seem erratic or non-operational. This is because, for ease of viewing, the colored edge result display is artificially rendered to appear larger than the actual thickness. You can still add a probe annotation in this situation by zooming in on the thin region before applying the probe annotation. • To delete a probe annotation, activate the Label button Delete key. • Probes will be cleared if the results are re-solved. • After adding one or more probe annotations, if you increase the number of viewports, the probe annotations only appear in one of the viewports. If you then decrease the number of viewports, you must first highlight the header in the viewport containing the probe annotations in order to preserve the annotations in the resulting viewports. • See the Solution Context Toolbar (p. 291) for more information. , select the probe, and then press the Message Annotations If an error occurs during meshing, the application attempts to annotate the problem geometry. 400 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Graphics Lighting Controls When you click Model in the Tree Outline (p. 235), you can view details that control lighting in the Geometry (p. 240) window. Comments, Images, Figures You can insert Comment objects, Image objects, or Figure objects under various parent objects in the Mechanical tree to add text or graphical information that pertain specifically to those parent objects. Refer to their individual objects reference pages for descriptions. Additional information on Figure objects is presented below. Figures allow you to: • Preserve different ways of viewing an object (viewpoints and settings). • Define illustrations and captions for a report. • Capture result contours, mesh previews, environment annotations etc., for later display in Report. Clicking the Figure button in the Standard Toolbar (p. 283) creates a new Figure object inside the selected object in the Tree Outline (p. 235). Any object that displays 3D graphics may contain figures. The new figure object copies all current view settings and gets focus in the Outline automatically. View settings maintained by a figure include: • Camera settings • Result toolbar settings • Legend configuration A figure's view settings are fully independent from the global view settings. Global view settings are maintained independently of figures. Behaviors: • If you select a figure after selecting its parent in the Outline, the graphics window transforms to the figure's stored view settings automatically (e.g. the graphics may automatically pan/zoom/rotate). • If you change the view while a figure is selected in the Outline, the figure's view settings are updated. • If you reselect the figure's parent in the Outline, the graphics window resumes the global view settings. That is, figure view settings override but do not change global view settings. • Figures always display the data of their parent object. For example, following a geometry Update and Solve, a result and its figures display different information but reuse the existing view and graphics options. Figures may be moved or copied among objects in the Outline to display different information from the same view with the same settings. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 401 Features • You may delete a figure without affecting its parent object. Deleting a parent object deletes all figures (and other children). • In the Tree Outline (p. 235), the name of a figure defaults to simply Figure appended by a number as needed. • You may enter a caption for a figure as a string in the figure's details. It is your responsibility to maintain custom captions when copying figures. Connections Supported connection features consist of Contact, Mesh Connection, Joint, Spring, Beam Connection, End Release, Spot Weld and Body Interaction (Explicit Dynamics only). Each of these connections can be created manually in the application. Only Contact, Joint, and Mesh Connection can also be generated automatically. This section describes Connections folder, Connection Group folder, Automatic Generated Connections, as well as each connection type as outlined below. Connections Folder Connection Group Folder Common Connections Folder Operations for Auto Generated Connections Contact Joints Mesh Connection Springs Beam Connections Spot Welds End Releases Body Interactions in Explicit Dynamics Analyses Connections Folder The Connections folder is the container for all types of connection objects except for the three types that can be automatically generated (Contact, Joint, and Mesh Connection). The objects of each of these three types are placed in a sub-folder called the Connection Group folder. As illustrated below, the Details view of the Connections folder provides the following two properties. 402 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Auto Detection • Generate Automatic Connection On Refresh: options are Yes (default) or No. This is a setting to turn on/off for auto generation of connection objects when the geometry is refreshed. The process of automatically creating the contact and mesh connection objects is additive. Any existing connection objects of these types that were created manually may be duplicated when the connections are automatically regenerated. To avoid duplication, you should first delete any existing contact and mesh connection objects before the geometry is refreshed. Note Special conditions apply to updating geometry that includes Spot Welds. The process of automatically creating joint objects is not additive. Any existing joint objects are note duplicated when connections are automatically regenerated. Transparency • Enabled: options are Yes (default) or No. This is a setting to enable or disable transparency of the bodies not associated with the connection in the graphics display. Connection Group Folder The role of a Connection Group folder is to provide you with the ability to automatically generate Contact, Joint, or Mesh Connection objects for the whole model or for a group of bodies within the model with a tolerance value applied only to this group. Only these three types of connections are provided with the automatic detection capability and only one type of connection objects can be included in a Connection Group folder with the exception of Spot Weld (see details in the Spot Weld section). The generated objects are placed in a Connection Group folder which is automatically renamed to "Contacts", "Joints", or "Mesh Connections" depending on the type. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 403 Features When a model is imported into the Mechanical application, if the Auto Detect Contact On Attach is requested (in the Workbench Tools>Options>Mechanical), auto contact detection is performed using the detection criteria based on the user preferences (in the Mechanical Tools>Options>Connections). Detail steps for auto/manual generating connection objects are presented in the Common Connections Folder Operations for Auto Generated Connections (p. 407) section. The Connection Group has the following properties. Definition • Connection Type: options include Contact, Joint, and Mesh Connections. Scope • 404 Scoping Method: options include Geometry Selection (default) and Named Selection. – Geometry – appears if Scoping Method is set to Geometry Selection. – Named Selection – appears if Scoping Method is set to Named Selection. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Auto Detection • Tolerance Type: options include Slider, Value, and Use Sheet Thickness. Bodies in an assembly that were created in a CAD system may not have been placed precisely, resulting in small overlaps or gaps along the connections between bodies. You can account for any imprecision by specifying connection detection tolerance. This tolerance can be specified by value when the type is set to Slider and Value, or sheet thickness of surface bodies when the type is set to Use Sheet Thickness. This option is only applicable to Contact and Mesh Connection and available when the Group By property (see below) is set to None or Bodies. • Tolerance Slider: appears if Tolerance Type is set to Slider. To tighten the connection detection, move the slider bar closer to +100 and to loosen the connection detection, move the slider bar closer to -100. A tighter tolerance means that the bodies have to be within a smaller region (of either gap or overlap) to be considered in connection; a looser tolerance will have the opposite effect. Be aware that as you adjust the tolerance, the number of connection pairs could increase or decrease. • Tolerance Value: appears if Tolerance Type is set to Slider or Value. This field will be read-only if the Tolerance Type is set to Slider showing the actual tolerance value based on the slider setting. When the Tolerance Type is set to Value, you will be able to provide an exact distance for the detection tolerance. After you provide a greater than zero value for the Tolerance Value, a circle appears around the current cursor location as shown below. The radius of the circle is a graphical indication of the current Tolerance Value. The circle moves with the cursor, and its radius will change when you change the Tolerance Value or the Tolerance Slider. The circle appropriately adjusts when the model is zoomed in or out. • • Use Range: appears if Tolerance Type is set to Value. Options include Yes and No (default). If set to Yes, you will have the connection detection searches within a range from Tolerance Value to Min Distance Value inclusive. – Min Distance Percentage: appears if Use Range is set to Yes. This is the percentage of the Tolerance Value to determine the Min Distance Value. The default is 10 percent. You can move the slider to adjust the percentage between 1 and 100. – Min Distance Value: appears if Use Range is set to Yes. This is a read-only field that displays the value derived from: Min Distance Value = Min Distance Percentage * Tolerance Value/100. • Thickness Scale Factor: appears if Tolerance Type is set to Use Sheet Thickness. The default value is 1. For Edge/Edge pairing (see below), the largest thickness among the surface bodies involved is used; however, if the pairing is Face/Edge, the thickness of the surface body with the face geometry is used. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 405 Features • Face/Face: (Contacts only) options include Yes (default) and No. Detects connection between the faces of different bodies. For Joints, Face/Face is the only detection type allowed. That is why the property does not appear in the Details view when the Connection Type is Joint. • Face/Edge: (Contacts and Mesh Connections only) options include Yes, No (default), Only Solid Body Edges and Only Surface Body Edges. Detects connection between faces and edges of different bodies. Faces are designated as targets and edges are designated as contacts. For Only Solid Body Edges, the face to edge connection uses the edges of solid bodies to determine connection with all faces. Likewise, for Only Surface Body Edges, face to edge connection uses only edges of surface bodies to determine connection with all faces. • Edge/Edge: (Contacts and Mesh Connections only) options include Yes and No. Detects connection between edges of different bodies. • Priority: (Contacts and Mesh Connections only) options include All, Face Overrides and Edge Overrides. For very large models the number of connection objects can sometimes become overwhelming and redundant, especially when multiple detection types are chosen. Selecting some type of priority other than Include All will lessen the number of connection objects generated during Create Automatic Connections by giving designated connection types precedence over other types. Face Overrides gives Face/Face option precedence over both Face/Edge and Edge/Edge options. It also gives Face/Edge option precedence over Edge/Edge option. In general, when Face Overrides priority is set with Face/Edge and Edge/Edge options, no Edge/Edge connection pairs will be detected. Edge Overrides gives Edge/Edge option precedence over both Face/Edge and Face/Face options, no Face/Face connections pairs will be detected. • Group By: options include None, Bodies and Parts. This property allows you to group the automatically generated connections objects. Setting Group By to Bodies (default) or to Parts means that connection faces and edges that lie on the same bodies or same parts will be included into a single connection object. Setting Group By to None means that the grouping of geometries that lie on the same bodies or same parts will not occur. Any connection objects generated will have only one entity scoped to each side (that is, one face or one edge). Applications for choosing None in the case of contact are: • – If there are a large number of source/target faces in a single region. Choosing None avoids excessive contact search times in the ANSYS solver. – If you want to define different contact behaviors on separate regions with contact of two parts. For example, for a bolt/bracket contact case, you may want to have bonded contact between the bolt threads/bracket and frictionless contact between the bolt head/bracket. Search Across: This property enables automatic connection detection through the following options: – Bodies (default): Between bodies. – Parts: Between bodies of different parts, that is, not between bodies within the same multibody part. – Anywhere: Detects any connections regardless of where the geometry lies, including different parts. However, if the connections are within the same body, this option finds only Face/Face connections, even if the Face/Edge setting is turned On. • Fixed Joints: (Joint only) options include Yes and No. This property determines if Fixed Joints are to be automatically generated. See the Automatic Joint Creation section for details. • Revolute Joints: (Joint only) options include Yes and No. This property determines if Revolute Joints are to be automatically generated. See the Automatic Joint Creation section for details. 406 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Common Connections Folder Operations for Auto Generated Connections You can automatically generate supported connections for a group of bodies in a model and use a separate tolerance value for that group. The supported connection types are Contact Region, Joint, and Mesh Connection. To automatically generate connections for a group of bodies: 1. Insert a Connection Group object under the Connections folder either from the toolbar button or by choosing Insert from the context menu (right mouse click) for this folder. 2. From the Details view of the Connection Group object, select the desired Connection Type. The default is Contact. 3. Select some bodies in the model based on the Scoping Method. The default is Geometry Selection scoped to All Bodies. 4. If applicable, set the Auto Detection properties. Note that these properties will be applied only to scoped geometries for this connection group. 5. Choose Create Automatic Connections from the context menu (right mouse click) for the Connection Group . The resulting connection objects will be placed under this folder and the folder name will be changed from its default name Connection Group to a name based on the connection type. The folder name for contacts will be Contacts, for mesh connections it will be Mesh Connections, and for joints it will be Joints. Once the Connection Group folder contains a child object, the Connection Type property cannot be changed. Each Connection Group folder will hold objects of the same type and will include a worksheet that displays only content pertaining to that folder. When two or more Connection Group folders are selected and you choose Create Automatic Connections, auto detection for the selected Connection Group folders will be performed. The Create Automatic Connections option is also available from the context menu (right mouse click) for the Connections folder provided there is at least one Connection Group folder present. When you choose this command from the Connections folder, auto detection will be performed for all connection groups under this folder. Manually Inserting Connection Objects You can insert any supported connection objects manually either from the toolbar or by choosing Insert from the context menu (right mouse click) on the Connections or Connection Group folder. When inserting a connection object from the Connections folder, a Connection Group object will automatically be created in addition to the connection object itself. When inserting a connection object from Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 407 Features a Connection Group folder, if it is an empty folder, any supported type of object can be inserted. However, if the folder already contains at least one object, only objects of the same type can be inserted. Searching for Duplicate Pairs Generating connections (Contacts, Mesh Connections or Joints) either automatically or manually may result in the same geometry pair being scoped by more than one connection object. This may over constrain the model that may lead to convergence difficulty problems in the solver. If this situation occurs, you can take corrective action by modifying the geometry scoping of the duplicated pairs or by deleting the duplicating connection objects. When generating connection objects automatically, each newly generated connection will be checked against existing connection objects for possible duplicate pairs. If one or more duplicate pairs are found in the existing connection objects, the following warning message will appear in the message box for a connection object that shares the same geometry pair: "This connection object shares the same geometries with one or more connection objects. This may overconstrain the model. Consider eliminating some connection objects." To find the connection object for a particular message, highlight that message in the message pane and right-click on that message and choose Go To Object from the context menu. The connection object will be highlighted in the tree. In order to find other connection objects that share the same geometry pair, right-click on the highlighted object and choose the Go To Connections for Duplicate Pairs from the context menu; all connection objects that share the same geometry pair will be highlighted. To search for connection objects that share the same geometry pair manually for one or more connection objects, select Search Connections for Duplicate Pairs from the context menu of these connection objects (by highlighting these connection objects first). If this command is issued from a Connection Group folder, the search will be carried out for all connection objects under this folder. When this command is issued from the Connections folder, the search will be for the entire connection objects under this folder. Moving and Copying Connection Objects To move a connection object to another folder of the same connection type, drag the object and drop it on that folder. For example, to move a contact region object, drag the object from its current Contacts folder and drop it on another folder whose Connection Type is Contact (possibly named Contacts 2). To copy a connection object to another folder of the same connection type, hold the Ctrl key while performing the move procedure described above. Treatment of Legacy Databases Supported connection objects from databases of previous versions of ANSYS Workbench will be grouped based on their types and migrated into Connection Group folders. Contact The following topics are covered in this section: Contact Overview Contact Settings Setting Contact Conditions Manually 408 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Contact Ease of Use Features Contact in Rigid Dynamics Contact Overview Contact conditions are created when an assembly is imported into the application and it detects that two separate bodies (solid, surface, and line bodies) touch one another (they are mutually tangent). Bodies/surfaces in contact: • Do not “interpenetrate”. • Can transmit compressive normal forces and tangential friction forces. • Can be bonded together (Linear) • Able to separate and collide (Nonlinear) Surfaces that are free to separate and move away from one another are said to have changing-status nonlinearity. That is, the stiffness of the system depends on the contact status, whether parts are touching or separated. Contact Formulations Contact solutions are often very complicated. It is recommended that, whenever possible, that user employ the Program Controlled settings. However, in order to better understand your selections, this section examines the specifics of Formulations. Because physical contacting bodies do not interpenetrate, the application must establish a relationship between the two surfaces to prevent them from passing through each other in the analysis. When the application prevents interpenetration, it is said to enforce “contact compatibility”. In order to enforce compatibility at the contact interface, Workbench Mechanical offers several different contact Formulations. These Formulations define the solution method used. Formulations include the following and are discussed in detail in the Formulations section. • Pure Penalty (Default - Program Controlled) • Augmented Lagrange • MPC • Normal Lagrange For nonlinear solid body contact of faces, Pure Penalty or Augmented Lagrange formulations can be used. Both of these are penalty-based contact formulations: FNormal = kNormalxPenetration Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 409 Features The finite contact Force, Fn, is a concept of contact stiffness, kNormal. The higher the contact stiffness, the lower the penetration, xp, as illustrated here. Ideally, for an infinite kNormal, one would get zero penetration. This is not numerically possible with penalty-based methods, but as long as xp is small or negligible, the solution results are accurate. The main difference between Pure Penalty and Augmented Lagrange methods is that Augmented Lagrange augments the contact force (pressure) calculations: Pure Penalty: FNormal = kNormalxPenetration Augmented Lagrange: FNormal = kNormalxPenetration + λ Because of the extra term λ, the Augmented Lagrange method is less sensitive to the magnitude of the contact stiffness kNormal. Another available option is Normal Lagrange. This formulation adds an extra degree of freedom (contact pressure) to satisfy contact compatibility. Consequently, instead of resolving contact force as contact stiffness and penetration, contact force (contact pressure) is solved for explicitly as an extra DOF. FNormal = DOF Specifications: • Enforces zero/nearly zero penetration with pressure DOF. • Does not require a normal contact stiffness (zero elastic slip) • Requires Direct Solver, which can increase computation requirements. Normal Lagrange Chattering Chattering is an issue which often occurs with Normal Lagrange method. If no penetration is allowed (left), then the contact status is either open or closed (a step function). This can sometimes make convergence more difficult because contact points may oscillate between open/closed status and is called "chattering". If some slight penetration is allowed (right), it can make it easier to converge since contact is no longer a step change. 410 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections For the specific case of Bonded and No Separation Types of contact between two faces, a Multi-Point constraint (MPC) formulation is available. MPC internally adds constraint equations to “tie” the displacements between contacting surfaces. This approach is not penalty-based or Lagrange multiplier-based. It is a direct, efficient way of relating surfaces of contact regions which are bonded. Large-deformation effects are supported with MPC-based Bonded contact. Comparison of Formulations Some of the primary aspects of contact formulations are compared below. Pure Penalty Augmented Lagrange Normal Lagrange MPC Good convergence behavior (few equilibrium iterations). Additional equilibrium iterations needed if penetration is too large. Additional equilibrium iterations if needed chattering is present. Good convergence behavior (few equilibrium iterations). Sensitive to selection of normal contact stiffness. Less sensitive to selection of normal contact stiffness. Contact penetration is present and uncontrolled. Contact penetration is present but controlled to some degree. No normal contact stiffness is required. Usually, penetration is near-zero. Only Bonded & No Separation behaviors. Useful for any type of contact behavior. Iterative or Direct Solvers can be used. No Penetration. Only Direct Solver can be Used. Iterative or Direct Solvers can be used. Symmetric or Asymmetric contact available. Asymmetric contact Only Contact detection at integration points. Contact Detection at Nodes. Contact Settings When a model is imported into Workbench Mechanical, the default setting of the application automatically detects instances where two bodies are in contact and generates corresponding Contact Region objects in the Tree Outline. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 411 Features When a Contact Region is selected in the Tree Outline, as illustrated here, contact settings are available in the Details view, and are included in the following categories: • Scope: settings for displaying, selecting, or listing contact and target geometries. • Definition: commonly used contact settings. • Advanced: advanced controls that are primarily program controlled. Scope Settings An example of the Scope category is illustrated below. 412 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections The controls for the Scope category are described in the following table. Property Description/Selections Scoping Method Specifies whether the Contact Region is applied to a Geometry Selection (dafault) or to a Named Selection. Contact Displays/selects which geometries (faces or edges) are considered as contact. The geometries can be manually selected or automatically generated. For a Face/Edge contact, the edge must be designated as Contact. A contact pair can have a flexible-rigid scoping, but the flexible side of the pair must always be the Contact side. If the Contact side of the contact pair is scoped to multiple bodies, all of the bodies must have the same Stiffness Behavior, either Rigid or Flexible. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 413 Features Property Description/Selections Note that if you click on this field, the bodies are highlighted. Target Displays which body element (face or edge) is considered Target (versus Contact). This element can be manually set or automatically generated. For Face/Edge contact, the face must be designated as Target. If the Contact side of the contact pair has a flexible Stiffness Behavior then the Target side can be rigid. Multiple rigid bodies cannot be selected for the Target side scoping of the contact pair. The selection of multiple rigid bodies for the Target invalidates the Contact Region object and an error message is generated following the solution process. Note that if you click on this field, the bodies are highlighted. Contact Bodies This read only property displays which bodies have faces or edges in the Contact list. Target Bodies This read only property displays which bodies have faces or edges in the Target list. Contact Shell Face Specifies whether the Contact should be applied on a surface body’s top face or bottom face. If you set Contact Shell Face to the default option, Program Controlled, then the Target Shell Face option must also be set to Program Controlled.The Program Controlled default option is not valid for nonlinear contact types.This option displays only when you scope a surface body to Contact Bodies. Target Shell Face Specifies whether the Target should be applied on a surface body’s top face or bottom face. If you set Target Shell Face to the default option, Program Controlled, then the Contact Shell Face option must also be set to Program Controlled.The Program Controlled default option is not valid for nonlinear contact types.This option displays only when you scope a surface body to Target Bodies. Note • All bodies selected for the Target or Contact side of a contact pair must have the same stiffness behavior. • You cannot scope the target side in a contact pair to more than one rigid body. • If any of the bodies you scope have rigid stiffness behavior, you must select Asymmetric behavior under Definition in the Details view. • If you have both rigid and flexible bodies in your contact pair, you must scope the rigid body as a Target. Definition Settings An example of the Definition category is illustrated below. 414 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections The differences in the contact settings determine how the contacting bodies can move relative to one another. This category describes the following controls. Type Choosing the appropriate contact type depends on the type of problem you are trying to solve. If modeling the ability of bodies to separate or open slightly is important and/or obtaining the stresses very near a contact interface is important, consider using one of the nonlinear contact types (Frictionless, Rough, Frictional), which can model gaps and more accurately model the true area of contact. However, using these contact types usually results in longer solution times and can have possible convergence problems due to the contact nonlinearity. If convergence problems arise or if determining the exact area of contact is critical, consider using a finer mesh (using the Sizing control) on the contact faces or edges. The available contact Types are listed below. Most of the types apply to Contact Regions made up of faces only. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 415 Features • Bonded: This is the default configuration and applies to all contact regions (surfaces, solids, lines, faces, edges). If contact regions are bonded, then no sliding or separation between faces or edges is allowed. Think of the region as glued. This type of contact allows for a linear solution since the contact length/area will not change during the application of the load. If contact is determined on the mathematical model, any gaps will be closed and any initial penetration will be ignored. • No Separation: This contact setting is similar to the Bonded case. It only applies to regions of faces (for 3-D solids) or edges (for 2-D plates). Separation of the geometries in contact is not allowed, but small amounts of frictionless sliding can occur along contact geometries. [Not supported for Explicit Dynamics analyses.] • Frictionless: This setting models standard unilateral contact; that is, normal pressure equals zero if separation occurs. Thus gaps can form in the model between bodies depending on the loading. This solution is nonlinear because the area of contact may change as the load is applied. A zero coefficient of friction is assumed, thus allowing free sliding. The model should be well constrained when using this contact setting. Weak springs are added to the assembly to help stabilize the model in order to achieve a reasonable solution. • Rough: Similar to the frictionless setting, this setting models perfectly rough frictional contact where there is no sliding. It only applies to regions of faces (for 3-D solids) or edges (for 2-D plates). By default, no automatic closing of gaps is performed. This case corresponds to an infinite friction coefficient between the contacting bodies. [Not supported for Explicit Dynamics analyses.] • Frictional: In this setting, the two contacting geometries can carry shear stresses up to a certain magnitude across their interface before they start sliding relative to each other. This state is known as "sticking." The model defines an equivalent shear stress at which sliding on the geometry begins as a fraction of the contact pressure. Once the shear stress is exceeded, the two geometries will slide relative to each other. The coefficient of friction can be any nonnegative value. • Friction Coefficient: Allows you to enter a friction coefficient. Displayed only for frictional contact applications. Note A Friction Coefficient greater than 0.2 will require the use of the Unsymmetric eigensolver in downstream analyses; for example, in Modal with Pre-Stress. Note Refer to KEYOPT(12) in the Mechanical APDL Contact Technology Guide for more information about modelling different contact surface behaviors. 416 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Scope Mode This is a read-only property that displays how the selected Contact Region was generated. Either automatically generated by the application (Automatic) or constructed or modified by the user (Manual). Behavior This property will appear only for 3-D Face/Face or 2-D Edge/Edge contacts. For 3-D Edge/Edge or Face/Edge contacts, internally the program will set the contact behavior to Asymmetric (see below). Sets contact pair to one of the following: • Program Controlled (Default for the Mechanical APDL solver): internally the contact behavior is set to the following options based on the stated condition: – Auto Asymmetric (see below) - for Flexible-Flexible bodies. – Asymmetric (see below) - for Flexible-Rigid bodies. For Rigid-Rigid contacts, the Behavior property is under-defined for the Program Controlled setting. The validation check is performed at the Contact object level when all environment branches are using the Mechanical APDL solver. If the solver target for one of the environments is other than Mechanical APDL, then this validation check will be carried out at the environment level; the environment branch will become under-defined. • Asymmetric: Contact will be asymmetric for the solve. All face/edge and edge/edge contacts will be asymmetric. [Not supported for Explicit Dynamics analyses.] Asymmetric contact has one face as Contact and one face as Target (as defined under Scope Settings), creating a single contact pair. This is sometimes called "one-pass contact," and is usually the most efficient way to model face-to-face contact for solid bodies. The Behavior must be Asymmetric if the scoping includes a body specified with rigid Stiffness Behavior. • Symmetric: Contact will be symmetric for the solve. • Auto Asymmetric: Automatically creates an asymmetric contact pair, if possible. This can significantly improve performance in some instances. When you choose this setting, during the solution phase the solver will automatically choose the more appropriate contact face designation. Of course, you can designate the roles of each face in the contact pair manually. [Not supported for Explicit Dynamics analyses.] Note Refer to KEYOPT(8) in the Mechanical APDL Contact Technology Guide for more information about asymmetric contact selection. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 417 Features Suppressed Specifies whether or not the contact region is included in the solution. Advanced Settings The default setting for all Advanced category options is Program Controlled. The Advanced category provides the following controls. Formulation Formulation options allow you to specify which algorithm the software uses for a particular Contact pair computation. 418 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Property Description Program Controlled This is the default setting. For nonlinear solid body contact of faces, the application selects Pure Penalty for contact between two rigid bodies and Augmented Lagrange for all other contact situations.These selections are described below. Pure Penalty Basic contact formulation based on Penalty method. KEYOPT(2) = 1 Augmented Lagrange Also a penalty-based method. Compared to the Pure Penalty method, this method usually leads to better conditioning and is less sensitive to the magnitude of the contact stiffness coefficient. However, in some analyses, the Augmented Lagrange method may require additional iterations, especially if the deformed mesh becomes too distorted. KEYOPT(2) = 0 MPC Available for Bonded and for No Separation contact Types. Multipoint Constraint equations are created internally during the Mechanical APDL application solve to tie the bodies together.This can be helpful if truly linear contact is desired or to handle the nonzero mode issue for free vibration that can occur if a penalty function is used. Note that contact based results (such as pressure) will be zero. KEYOPT(2) = 2 Enforces zero penetration when contact is closed making use of a Lagrange multiplier on the normal direction and a penalty method in the tangential direction. Normal Stiffness is not applicable for this setting. Normal Lagrange adds contact traction to the model as additional degrees of freedom and requires additional iterations to stabilize contact conditions. It often increases the computational cost compared to the Augmented Lagrange setting. The Iterative setting (under Solver Type) cannot be used with this method. KEYOPT(2) = 3 Normal Lagrange MAPDL - For additional MAPDL specific information, see KEYOPT(2) in the Mechanical APDL Contact Technology Guide. Note Cases involving large gaps and faces bonded together can result in fictitious moments being transmitted across a boundary. Detection Method Detection Method allows you to choose the location of contact detection used in the analysis in order to obtain a good convergence. It is applicable to 3-D face-face contacts and 2-D edge-edge contacts. The Detection Method property provides the following options. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 419 Features Property Description Program Controlled This is the default setting. The application uses Gauss integration points (On Gauss Point) when the formulation is set to Pure Penalty and Augmented Lagrange. It uses nodal point (Nodal-Normal to Target) for MPC and Normal Lagrange formulations. On Gauss Point The contact detection location is at the Gauss integration points. This option is not applicable to contacts with MPC or Normal Lagrange formulation. Nodal - Normal From Contact The contact detection location is on a nodal point where the contact normal is perpendicular to the contact surface. Nodal - Normal To Target The contact detection location is on a nodal point where the contact normal is perpendicular to the target surface. Nodal - Projected Normal From Contact The contact detection location is at contact nodal points in an overlapping region of the contact and target surfaces (projection-based method). For additional MAPDL specific information, see Selecting Location of Contact Detection (specifically, KEYOPT(4) related information) in the Mechanical APDL Contact Technology Guide. Constraint Type Controls the type of MPC constraint to be created for bonded contact. This setting is displayed only if Formulation is set to MPC and if either Contact Bodies or Target Bodies are scoped to a surface body. The Constraint Type option provides the following controls. Property Description Target Normal, Couple U to ROT (Default) Represents the most common type of surface body contact. Constraints are constructed to couple the translational and rotational DOFs. In most types of surface body contact, an offset will exist. Due to this offset there will be a moment created. To get the correct moment, the rotation/displacement DOF's must be coupled together. If the program cannot detect any contact in the target normal direction, it will then search anywhere inside the pinball for contact. Target Normal, Uncouple U to ROT The rotational and displacement constraints will not be coupled together. This option can model situations where the surface body edges line up well and a moment is not created from the physical surface body positions. Thus it is most 420 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections accurate for the constraints to leave the displacements/rotations uncoupled. This provides an answer which is closer to a matching mesh solution. Using a coupled constraint causes artificial constraints to be added causing an inaccurate solution. Inside Pinball, Couple U to ROT Constraints are coupled and created anywhere to be found inside the pinball region. Thus the pinball size is important as a larger pinball will result in a larger constraint set. This option is useful when you wish to fully constrain one contact side completely to another. Interface Treatment This property defines how the contact interface for the pair is treated. It becomes active when contact Type is set to Frictionless, Rough or Frictional (nonlinear contact). The Interface Treatment property provides the following options. When active, the Interface Treatment option provides the following controls. • Adjust to Touch: Any initial gaps are closed and any initial penetration is ignored creating an initial stress free state. Contact pairs are “just touching” as shown. Contact pair before any Interface Treatment. Gap exists. Contact pair after Adjust to Touch treatment. Gap is closed automatically. Pair is “just touching”. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 421 Features Contact pair before any Interface Treatment. Penetration exists. Contact pair after Adjust to Touch treatment. Pair touches at interface. This setting is useful to make sure initial contact occurs even if any gaps are present (as long as they are within the pinball region). Without using this setting, the bodies may fly apart if any initial gaps exist. Although any initial gaps are ignored, gaps can still form during loading for the nonlinear contact types. For nonlinear contact types (Frictionless, Rough, and Frictional), Interface Treatment is displayed where the choices are Adjust to Touch, Add Offset, Ramped Effects, and Add Offset, No Ramping. • Add Offset, Ramped Effects: Models the true contact gap/penetration plus adds in any user defined offset values. This setting is the closest to the default contact setting used in the Mechanical APDL application except that the loading is ramped. Using this setting will not close gaps. Even a slight gap may cause bodies to fly apart. Should this occur, use a small contact offset to bring the bodies into initial contact. Note that this setting is displayed only for nonlinear contact. • Add Offset, No Ramping (default): This option is the same as Add Offset, Ramped Effects but loading is not ramped. • Offset: appears if Interface Treatment is set to Add Offset, Ramped or Add Offset, No Ramping. This property defines the contact offset value. A positive value moves the contact closer together (increase penetration/reduce gap) and a negative value moves the contact further apart. Contact pair before any Interface Treatment. Gap exists. Contact pair after Add Offset treatment (either option). Gap is closed "manually” based on value entered for Offset (positive value shown that includes some penetration). Normal Stiffness Defines a contact Normal Stiffness factor. The usual factor range is from 0.01-10, with the default selected programmatically. A smaller value provides for easier convergence but with more penetration. The default value is appropriate for bulk deformation. If bending deformation dominates, use a smaller value (0.01-0.1). Option Description Program Controlled (Default) The Normal Stiffness Factor is calculated by the program. If only Bonded or No Separation contact exists, the value is set to 10. If any other type of contact exists, all the program controlled regions (including Bonded or No Separation) will use the Mechanical APDL application default (real constant FKN). Manual The Normal Stiffness Factor is input directly by the user. 422 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Normal Stiffness Factor This property appears when the Normal Stiffness is set to Manual. It allows you to input the normal stiffness factor. Only non-zero positive values are allowed. This choice is displayed only if Manual is specified for Normal Stiffness. Update Stiffness Allows you to specify if the program should update (change) the contact stiffness during the solution. If you choose any of these stiffness update settings, the program will modify the stiffness (raise/lower/leave unchanged) based on the physics of the model (that is, the underlying element stress and penetration). This choice is displayed only if you set the Formulation to Augmented Lagrange or Pure Penalty, the two formulations where contact stiffness is applicable. An advantage of choosing either of the program stiffness update settings is that stiffness is automatically determined that allows both convergence and minimal penetration. Also, if this setting is used, problems may converge in a Newton-Raphson sense, that would not otherwise. You can use a Result Tracker to monitor a changing contact stiffness throughout the solution. The update choices are listed below. Property Description Program Controlled (Default as set in Tools->Options). Internally set based on the following criteria: if the Interface Treatment property is available and it is set to Add Offset, Ramped Effects, the update stiffness property should be set to Never; otherwise, set the update stiffness property to Never for contacts between two rigid bodies and to Each Iteration for others. Never (Default) Turns off the program's automatic Update Stiffness feature. Each Iteration Sets the program to update stiffness at the end of each equilibrium iteration. This choice is recommended if you are unsure of a Normal Stiffness Factor to use in order to obtain good results. Each Iteration, Aggressive Sets the program to update stiffness at the end of each equilibrium iteration, but compared to the Each Iteration, this option allows for a more aggressive changing of the value range. Stabilization Damping Factor A contact you define may initially have a near open status due to small gaps between the element meshes or between the integration points of the contact and target elements. The contact will not get detected during the analysis and can cause a rigid body motion of the bodies defined in the contact. The stabilization damping factor provides a certain resistance to damp the relative motion between Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 423 Features the contacting surfaces and prevents rigid body motion. This contact damping factor is applied in the contact normal direction and it is valid only for frictionless, rough and frictional contacts. The damping is applied to each load step where the contact status is open. The value of the stabilization damping factor should be large enough to prevent rigid body motion but small enough to ensure a solution. A value of 1 is usually appropriate. Property Description MAPDL Stabilization Damping Factor If this factor is 0 (default), the damping is activated only in the first load step (KEYOPT(15) = 0, the default). If its value is greater than 0, the damping is activated for all load steps (KEYOPT(15) = 2). FDMN KEYOPT(15) = 2. Damping is activated for all load steps. Thermal Conductance Controls the thermal contact conductance value used in a thermal contact simulation. Property Description Program Controlled (Default) The program will calculate the value for the thermal contact conductance.The value will be set to a sufficiently high enough value (based on the thermal conductivities and the model size) to model perfect contact with minimal thermal resistance. Manual The Thermal Conductance Value is input directly by the user. Thermal Conductance Value Allows input of the Thermal Conductance Value (in units of heat transfer film coefficient). Only positive values are allowed. This choice is displayed only if Manual is specified for Thermal Conductance. Pinball Region This option allows you to specify the contact search size, commonly referred to as the pinball region. Setting a pinball region can be useful in cases where initially, bodies are far enough away from one another that, by default, the program will not detect that they are in contact. You could then increase the pinball region as needed. Consider an example of a surface body that was generated by offsetting a face of a solid body, possibly leaving a large gap, depending on the thickness. Another example is a large deflection problem where a considerable pinball region is required due to possible large amounts of over penetration. In general though, if you want two regions to be bonded together that may be far apart, you should specify a pinball region that is large enough to ensure that contact indeed occurs. For bonded and no separation contact types, you must be careful in specifying a large pinball region. For these types of contact, any regions found within the pinball region will be considered to be in contact. For other types of contact, this is not as critical because additional calculations are performed to determine if the two bodies are truly in contact. The pinball region defines the searching range where these calculations will occur. Further, a large gap can transmit fictitious moments across the boundary. Property Description Program Controlled (Default) The pinball region will be calculated by the program. Auto Detection Value This option is only available for contacts generated automatically.The pinball region will be equal to the tolerance value used in generating the contacts.The value is displayed 424 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections as read-only in the Auto Detection Value field.Auto Detection Value is the recommended option for cases where the automatic contact detection region is larger than a Program Controlled region. In such cases, some contact pairs that were detected automatically may not be considered in contact for a solution. Radius Specifies that you directly enter a radius value for the pinball. Pinball Radius The numerical value for the Pinball Radius. This choice is displayed only if Pinball Region is set to Radius. Electric Conductance Controls the electric contact conductance value used in an electric contact simulation. Property Description Program Controlled (Default) The program will calculate the value for the electric contact conductance. The value will be set to a sufficiently high enough value (based on the electric conductivities and the model size) to model perfect contact with minimal electric resistance. Manual The Electric Conductance Value is input directly by the user. Note The Electric Analysis result, Joule Heat, when generated by nonzero contact resistance is not supported. Electric Conductance Value Allows input of the Electric Conductance Value (in units of electric conductance per area). Only positive values are allowed. This choice is displayed only if Manual is specified for Electric Conductance. Time Step Controls Allows you to specify if changes in contact behavior should control automatic time stepping. This choice is displayed only for nonlinear contact (Type is set to Frictionless, Rough, or Frictional). Property Description None (Default) - Contact behavior does not control automatic time stepping. This option is appropriate for most analyses when automatic time stepping is activated and a small time step size is allowed. Automatic Bisection Contact behavior is reviewed at the end of each substep to determine whether excessive penetration or drastic changes in contact status have occurred. If so, the substep is reevaluated using a time increment that is bisected (reduced by half ). Predict for Impact Performs same bisection on the basis of contact as the Automatic Bisection option and also predicts the minimal time increment needed to detect changes in contact behavior. This option is recommended if you anticipate impact in the analysis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 425 Features Setting Contact Conditions Manually Manual contact regions represent contact over the entire extent of the contact scope, for example, faces of the contact region. Automatic contact regions represent contact only to the extent of the scope where the corresponding bodies initially are close to one another. For automatic contact, the contact elements are “trimmed” before solution. The trimming is based on the detection tolerance. The tighter the tolerance, the less number of generated contact elements. Note that if you set Large Deflection effects to On in the Details view of a Solution object, no trimming will be done due to the possibility of large sliding. Valid reasons to manually change or add/delete contact regions include: • Modeling "large sliding" contact. Contact regions created through auto-detection assume "assembly contact," placing contact faces very near to one another. Manual contact encompasses the entire scope so sliding is better captured. In this case, you may need to add additional contact faces. • Auto-detection creates more contact pairs than are necessary. In this case, you can delete the unnecessary contact regions. • Auto-detection may not create contact regions necessary for your analysis. In this case, you must add additional contact regions. You can set contact conditions manually, rather than (or in addition to) letting the application automatically detect contact regions. Within a source or target region, the underlying geometry must be of the same geometry type (for example, all surface body faces, all solid body faces). The source and target can be of different geometry types, but within itself, a source must be of the same geometry type, and a target must be of the same geometry type. To set contact regions manually: 1. Click the Connections object in the Tree Outline (p. 235). 2. Click the right mouse button and choose Insert> Manual Contact Region. You can also select the Contact button on the toolbar. 3. A Contact Region item appears in the Outline. Click that item, and under the Details View (p. 274), specify the Contact and Target regions (faces or edges) and the contact type. See the Contact and Target topics in the Scope Settings section for additional Contact Region scoping restrictions. Contact Ease of Use Features The following features are intended to assist you in performing simulations involving contact: Controlling Transparency for Contact Regions Displaying Contact Bodies in Separate Windows Hiding Bodies Not Scoped to a Contact Region Renaming Contact Regions Based on Geometry Names Identifying Contact Regions for a Body Flipping Contact and Target Scope Settings Merging Contact Regions That Share Geometry Saving or Loading Contact Region Settings Resetting Contact Regions to Default Settings Locating Bodies Without Contact Locating Parts Without Contact 426 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Controlling Transparency for Contact Regions As shown below, you can graphically highlight an individual contact region. The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the help. Interface names and other components shown in the demo may differ from those in the released product. • Click on a contact region to highlight the bodies in that region. • Highlighting is due to internal transparency settings: – Transparency is set to 0.8 for bodies in selected contact region. – Transparency is set to 0.1 for bodies not in selected contact region(s). – You can change the default transparency values in the Mechanical application Connections settings of the Options dialog box. • You can disable the contact region highlighting feature in either the Details view of a contact group branch, or by accessing the context menu (right mouse click) on a contact region or contact group branch of the tree, and choosing Disable Transparency. Displaying Contact Bodies in Separate Windows Use the Body Views button on the Connections Context Toolbar to display parts in separate auxiliary windows. As illustrated and highlighted below, the different contact bodies (Contact and Target) have colors codes associated with them. In the Details as well as the graphic windows. Contact Bodies View Target Bodies View Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 427 Features Hiding Bodies Not Scoped to a Contact Region You can hide all bodies except those that are scoped to a specific contact region. To Hide All Bodies Not Scoped to a Contact Region: 1. Select the Contact Region object whose bodies you do not want to hide. 2. Right-click to display the context menu. 3. Select Hide All Other Bodies in the menu. All bodies are hidden except those that are part of the selected contact region. Renaming Contact Regions Based on Geometry Names You can change the name of any contact region using the following choices available in the context menu that appears when you click the right mouse button on a particular contact region: • Rename: Allows you to change the contact region name to a name that you type (similar to renaming a file in Windows Explorer). • Rename Based on Definition: Allows you to change the contact region name to include the corresponding names of the items in the Geometry branch of the tree that make up the contact region. The items are separated by the word “To” in the new contact region name. You can change all the contact region names at once by clicking the right mouse button on the Connections branch, then choosing Rename Based on Definition from that context menu. A demonstration of this feature follows. The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the help. Interface names and other components shown in the demo may differ from those in the released product. 428 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections When you change the names of contact regions that involve multiple bodies, the region names change to include the word Multiple instead of the long list of names associated with multiple bodies. An example is Bonded – Multiple To Multiple. Identifying Contact Regions for a Body See the description for Contacts for Selected Bodies in the Tree Outline Go To Options (p. 237) section. Flipping Contact and Target Scope Settings A valuable feature available when using asymmetric contact is the ability to swap contact and target face or edge Scope settings in the Details view. You accomplish this by clicking the right mouse button on the specific contact regions (Ctrl key or Shift key for multiple selections) and choosing Flip Contact/Target. This is illustrated below for a single region. The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the help. Interface names and other components shown in the demo may differ from those in the released product. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 429 Features Note This feature is not applicable to Face/Edge contact where faces are always designated as targets and edges are always designated as contacts. Merging Contact Regions That Share Geometry You can merge two or more contact regions into one contact region, provided they share the same type of geometry (edges or faces). To Merge Contact Regions That Share Geometry: 1. Select two or more contact regions in the tree that share the same type of geometry (edges or faces). Use the Shift or Ctrl key for multiple selections. 2. Right-click to display the context menu. 3. Select Merge Selected Contact Regions in the menu. This option only appears if the regions share the same geometry types. After selecting the option, a new contact region is appended to the list in the tree. The new region represents the merged regions. The individual contact regions that you selected to form the merged region are no longer represented in the list. Saving or Loading Contact Region Settings You can save the configuration settings of a contact region to an XML file. You can also load settings from an XML file to configure other contact regions. To Save Configuration Settings of a Contact Region: 1. Select the contact region whose settings you want to save. 2. Right-click to display the context menu. 3. Select Save Contact Region Settings in the menu. This option does not appear if you selected more than one contact region. 4. Specify the name and destination of the file. An XML file is created that contains the configuration settings of the contact region. Note The XML file contains properties that are universally applied to contact regions. For this reason, source and target geometries are not included in the file. To Load Configuration Settings to Contact Regions: 1. Select the contact regions whose settings you want to assign. Use the Shift or Ctrl key for multiple selections. 2. Right-click to display the context menu. 3. Select Load Contact Region Settings in the menu. 4. Specify the name and location of the XML file that contains the configuration settings of a contact region. Those settings are applied to the selected contact regions and will appear in the Details view of these regions. 430 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Resetting Contact Regions to Default Settings You can reset the default configuration settings of selected contact regions. To Reset Default Configuration Settings of Contact Regions: 1. Select the contact regions whose settings you want to reset to default values. Use the Shift or Ctrl key for multiple selections. 2. Right-click to display the context menu. 3. Select Reset to Default in the menu. Default settings are applied to the selected contact regions and will appear in the Details view of these regions. Locating Bodies Without Contact See the description for Bodies Without Contacts in Tree in the Tree Outline Go To Options (p. 237) section. Locating Parts Without Contact See the description for Parts Without Contacts in Tree in the Tree Outline Go To Options (p. 237) section. Contact in Rigid Dynamics Contact conditions are formed where rigid bodies meet. Though the default contact settings and automatic detection capabilities are sufficient, the default contact definition sometimes needs to be extended to adjacent surfaces. This is due to the nature of rigid dynamics, that usually implies very large displacements and rotations. In rigid dynamics, only frictionless contact is supported. The contact is always based on Pure Lagrange formulation. Contact constraint equations are updated at each time step, and added to the system matrix through additional forces of degrees of freedom called Lagrange Multipliers. In this formulation, there is no contact stiffness. Contact constraints are satisfied when the bodies are touching and they are nonexistent when bodies are separated. Contact and Rigid Bodies The contact is formulated between rigid bodies. Hence there is no possibility of deforming the bodies to satisfy the contact constraint equations. If the contact equations cannot be satisfied at one point in time, the solution will not proceed further. To illustrate this, we will consider two examples. Example 1: Shaft in a cylindrical hole. In this example of cylindrical shaft in a block Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 431 Features • If the diameter of the shaft is smaller than that of the hole, motion is possible. • If the diameter is larger than that of the hole, the simulation is not possible. • If the two diameters are equal, then the analysis might fail. Example 2: Block sliding on two blocks. • If the green block slides horizontally from left to right and height of the right block is less than that of the left block, motion is possible. • If the height of the two bottom blocks is identical, but if a vertical contact surface between these two bottom block is defined, then the block might or might not hit the vertical surface, and the solution may or may not proceed. • If the right block is higher than the left block, the green block will move back to the left. Note Whenever possible avoid such ambiguous configurations. A workaround is to create fillets on sharp edges. 432 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Contact Mesh You can scope the contact objects to rigid bodies using 3D faces in solid bodies. When you create this type of contact, the surface and edges in the contact region are meshed. The mesh helps to speed up the solution and drive the number of contact points used between the bodies when in contact. As each body has up to 6 degrees of freedom, a contact between two rigid bodies will restraint up to 6 relative degrees of freedom. This means that usually, a reasonably coarse mesh is sufficient to define the contact surface. The contact solver will use this mesh to initiate the contact geometry calculation, but will then project back the contact to CAD geometry. Refining the mesh can increase the solution time without always increasing the quality of the solution. However, when the geometry is concave, and if the solver reports a lot of shocks for the pair involving the concave surfaces, refining the mesh can be useful. Contact and Time Step The rigid solver uses event based time integration. Over each time step, the solver evaluates the trajectory of the bodies, and checks when these trajectories interfere. When interference is found, similarly to stops on joints, a shock will be analyzed, leading to a new velocity distribution. The physics of the velocity redistribution during the shock is based on the conservation of energy. The amount of energy lost during the shock is quantified by the coefficient of restitution. For details see, Joint Stops and Locks. The trajectory detection of interferences allows the use of large time steps without missing the contacts. As opposed to Penalty based simulation that introduces an artificial deformation of the bodies, and thus high frequencies in the simulation, the pure Lagrange formulation used in the rigid dynamics formulation does not change the frequency content of the simulation. However, the amount of geometrical calculation necessary for a solution including contact makes that the overall simulation time will be significantly higher than this of a solution without contact. Whenever possible, it is recommended to use joints stops rather than contacts. Limitations For models with sliding contacts, e.g., cams, guiding grooves, etc., small bounces due to nonzero restitution factors can cause and increase the simulation time and instabilities. Using a restitution factor of zero will help the simulation significantly. Joints The following topics are covered in this section: Joint Characteristics Types of Joints Joint Properties and Application Example: Assembling Joints Example: Configuring Joints Automatic Joint Creation Joint Stops and Locks Ease of Use Features Detecting Overconstrained Conditions Joint Characteristics Joints are supported in the following structural analyses: rigid dynamics, static, modal, harmonic, random vibration, response spectrum, and transient structural. A joint typically serves as a junction where bodies are joined together. Joint types are characterized by their rotational and translational degrees of freedom as being fixed or free. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 433 Features Note This boundary condition cannot be applied to a vertex scoped to an end release. Nature of Joint Degrees of Freedom • • For all joints that have both translational degrees of freedom and rotational degrees of freedom, the kinematics of the joint is as follows: 1. Translation: The moving coordinate system translates in the reference coordinate system. If your joint is a slot for example, the translation along X is expressed in the reference coordinate system. 2. Once the translation has been applied, the center of the rotation is the location of the moving coordinate system. For the ANSYS Mechanical APDL solver, the relative angular positions for the spherical, general, and bushing joints are characterized by the Cardan (or Bryant) angles. This requires that the rotations about the local Y axis be restricted between –π/2 to +π/2. Thus, the local Y axis should not be used to simulate the axis of rotation if the expected rotation is large. Joint Abstraction Joints are considered as point to point in the solution but the user interface shows the actual geometry. Due to this abstraction to a point to point joint, geometry interference and overlap between the two parts linked by the joint can be seen during an animation. Joint Initial Conditions The nature of the degrees of freedom differs based on the selected solver. For the ANSYS Rigid Dynamics solver, the degrees of freedom are the relative motion between the parts. For the ANSYS Mechanical solver, the degrees of freedom are the location and orientation of the center of mass of the bodies. Unless specified otherwise by using joint conditions, both solvers will start with initial velocities equal to zero, but that means two different things, as explained below. • For the ANSYS Mechanical APDL solver, not specifying anything means that the bodies will be at rest. • For the ANSYS Rigid Dynamics solver, not specifying anything means that the relative velocities will be at rest. Taking the example of an in-plane double pendulum, and prescribing a constant velocity for the first grounded link will be interpreted as follows: • The second link has the same rotational velocity as the first one for the ANSYS Rigid Dynamics solver, as the relative velocity is initially equal to zero. • The second link will start at rest for the ANSYS Mechanical APDL solver. Joint DOF Zero Value Conventions Joints can be defined using one or two coordinate systems: the Reference Coordinate System and the Mobile Coordinate System. The use of two coordinate systems provides benefits. An example is when a CAD model is not imported in an assembled configuration. In addition, it is important to define two coordinate systems so that you can employ the Configure and Set (see Applying Joints (p. 446)) features as well as having the ability to update a model following a CAD update. 434 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections For the ANSYS Rigid Dynamics solver, the zero value of the degrees of freedom corresponds to the matching reference coordinate system and moving coordinate system. If a joint definition includes only the location of the Mobile Coordinate System (see Joint Coordinate Systems (p. 443)), then the DOF of this joint are initially equal to zero for the geometrical configuration where the joints have been built. If the Reference Coordinate System is defined using the Override option, then the initial value of the degrees of freedom can be a nonzero value. Consider the example illustrated below. If a Translational joint is defined between the two parts using two coordinate systems, then the distance along the X axis between the two origins is the joint initial DOF value. For this example, assume it is 65 mm. On the other hand, if the joint is defined using a single coordinate, as shown below, then the same geometrical configuration has a joint degree of freedom that is equal to zero. For the ANSYS Mechanical APDL solver, having one or two coordinate systems has no impact. The initial configuration corresponds to the zero value of the degrees of freedom. Joint Condition Considerations When applying a Joint Condition, differences between the two solvers can arise. For example, consider the right part illustrated above moving 100 mm towards the other part over a 1 second period. (The distance along the X axis is 65 mm.) Solver ANSYS Rigid Dynamics – Two Coordinate Systems ANSYS Rigid Dynamics – One Coordinate System ANSYS Mechanical APDL – Two Coordinate Systems Displacement Joint Condition Time Displacement 0 65 1 165 0 0 1 100 0 0 1 100 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 435 Features ANSYS Mechanical APDL – One Coordinate System 0 0 1 100 You can unify the joint condition input by using a Velocity Joint Condition. Solver ANSYS Rigid Dynamics – Two Coordinate Systems ANSYS Rigid Dynamics – One Coordinate System ANSYS Mechanical APDL – Two Coordinate Systems ANSYS Mechanical APDL – One Coordinate System Velocity Joint Condition Time Displacement 0 100 1 100 0 100 1 100 0 100 1 100 0 100 1 100 Types of Joints You can create the following types of joints in the Mechanical application: • Fixed Joint (p. 436) • Revolute Joint (p. 436) • Cylindrical Joint (p. 437) • Translational Joint (p. 437) • Slot Joint (p. 438) • Universal Joint (p. 438) • Spherical Joint (p. 439) • Planar Joint (p. 439) • Bushing Joint (p. 440) • General Joint (p. 442) The following sections include animated visual joint representations. Please view online if you are reading the PDF version of the help. Fixed Joint • Constrained degrees of freedom: All Revolute Joint • 436 Constrained degrees of freedom: UX, UY, UZ, ROTX, ROTY Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections • Example: Cylindrical Joint • Constrained degrees of freedom: UX, UY, ROTX, ROTY • Example: Translational Joint • Constrained degrees of freedom: UY, UZ, ROTX, ROTY, ROTZ Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 437 Features • Example: Slot Joint • Constrained degrees of freedom: UY, UZ • Example: Universal Joint • 438 Constrained degrees of freedom: UX, UY, UZ, ROTY Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections • Example: Spherical Joint • Constrained degrees of freedom: UX, UY, UZ • Example: Planar Joint • Constrained degrees of freedom: UZ, ROTX, ROTY Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 439 Features • Example: Bushing Joint • Constrained degrees of freedom: None • Example: 440 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections • A Bushing has six degrees of freedom, three translations and three rotations, all of which can potentially be characterized by their rotational and translational degrees of freedom as being free or constrained by stiffness. For a Bushing, the rotational degrees of freedom are defined as follows: – The first is a rotation around the reference coordinate system X Axis. – The second is a rotation around the Y Axis after the first rotation is applied. – The third is a rotation around the Z Axis after the first and second rotations are applied. The three translations and the three rotations form a set of six degrees of freedom. In addition, the bushing behaves, by design, as an imperfect joint, that is, some forces developed in the joint oppose the motion. The three translational degrees of freedom expressed in the reference coordinate system and the three rotations are expressed as: Ux, Uy, Uz, and Ψ, Θ, φ. The relative velocities in the reference coordinate system are expressed as: Vx, Vy, and Vz. The three components of the relative rotational velocity are expressed as: Ωx, Ωy, and Ωz. Please note that these values are not the time derivatives of [Ψ, Θ, φ]. They are a linear combination. The forces developed in the Bushing are expressed as: Where: [F] is force and [T] is Torque, and [K] and [C] are 6x6 matrices (defined using Stiffness Coefficients and Dampening Coefficients options). Off diagonal terms in the matrix are coupling terms between the DOFs. You can use these joints to introduce flexibility to an over-constrained mechanism. Please note that very high stiffness terms introduce high frequencies into the system and may penalize the solution time when using the ANSYS Rigid Dynamics solver. If you want to suppress motion in one direction entirely , it is more efficient to use Joint DOF Zero Value Conventions instead of a very high stiffness. Scoping You can scope a bushing to single or multiple faces, single or multiple edges, or to a single vertex. The scoping can either be from body-to-body or body-to-ground. For body-to-body scoping, there is a reference and mobile side. For body-to-ground scoping, the reference side is assumed to be grounded (fixed); scoping is only available on the mobile side. In addition to setting the scoping Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 441 Features (where the bushing attaches to the body), you can set the bushing location on both the mobile and reference side. The bushing reference and mobile location cannot be the same. Applying a Bushing To add a bushing: 1. After importing the model, highlight the Connections object in the tree. 2. Choose either Body-Ground>Bushing or Body-Body>Bushing from the toolbar, as applicable. 3. Highlight the new Bushing object and enter information in the Details view. Note that matrix data for the Stiffness Coefficients and Dampening Coefficients is entered in the Worksheet. Entries are based on a Full Symmetric matrix. General Joint • Constrained degrees of freedom: Fix All, Free X, Free Y, Free Z, and Free All. A general joint has six degrees of freedom, three translations and three rotations, all of which can potentially be characterized by their rotational and translational degrees of freedom as being free or constrained by stiffness. All the degrees of freedom are set to fixed by default. You can free the X translation, free the Y translation, free the Z translation and free all rotations. All the translational degrees of freedom can be controlled individually to be fixed or free. But there are no individual controls for rotational degrees of freedom. You can either set all rotations fixed, or just one of them (X, Y or Z) free or all free. Also, similar to a bushing, you can enter matrix data for the Stiffness Coefficients and Damping Coefficients in the Worksheet. Coupled terms (off diagonal terms in the matrix) are only allowed when all DOFs are free. Joint Properties and Application This section discusses joint properties and manual joint creation in the Mechanical application. Joints can also be created automatically as discussed in Automatic Joint Creation (p. 464). A Joint is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 628) section for a listing of all remote boundary conditions and their characteristics. Connection Type You can scope a joint to single or to multiple faces. The scoping can either be from body-to-body or body-to-ground. For body-to-body scoping, there is a reference and mobile side. For body-to-ground scoping, the reference side is assumed to be grounded (fixed); scoping is only available on the mobile side. Type Refer to the Types of Joints (p. 436) section for descriptions of each type of joint you can create in the Mechanical application. In addition to these types, you can create a General joint where you can specify each degree of freedom as being either Fixed or Free. 442 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Torsional Stiffness Torsional stiffness is the measure of the resistance of a shaft to a twisting or torsional force. You can add torsional stiffness only for cylindrical and revolute joints. Torsional Damping Torsional damping is the measure of resistance to the angular vibration to a shaft or body along its axis of rotation. You can add torsional damping only for cylindrical and revolute joints. Joint Coordinate Systems The scoping of a joint must be accompanied by the definition of a joint coordinate system. This coordinate system defines the location of the joint. It is imperative that the joint coordinate system be fully associative with the geometry, otherwise, the coordinate system could move in unexpected ways when the Configure tool is used to define the initial position of the joint (see step 5 in the “Applying Joints” section below). A warning message is issued if you attempt to use the Configure tool with a joint whose coordinate system is not fully associative. The following types of coordinate systems apply specifically to joints: • A reference coordinate system accompanies a joint when the joint is added to the tree. This applies for joints whose connection type is either body-to ground or body-to-body. When a joint is added, an associated coordinate system is automatically generated at a location based on your face selection. • To support the relative motion between the parts of a joint, a mobile coordinate system is also automatically defined but is only displayed in the tree when the Initial Position is set to Override in the Details view of the Joint object. For either reference or mobile joint coordinate systems, both the original location and the orientation of the coordinate system can be changed as shown below. Caution If you are scoping a joint to a Remote Point, you cannot scope the Initial Position setting of a Joint's Mobile group as Unchanged. The Unchanged setting indicates the use of the same coordinate system for the Reference group and the Mobile group. To move a joint coordinate system to a particular face: 1. Highlight the Coordinate System field in the Details view of the Joint object. The origin of the coordinate system will include a yellow sphere indicating that the movement “mode” is active. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 443 Features 2. Select the face that is to be the destination of the coordinate system. The coordinate system in movement mode relocates to the centroid of the selected face, leaving an image of the coordinate system at its original location. 3. Click the Apply button. The image of the coordinate system changes from movement mode to a permanent presence at the new location. To change the orientation of a joint coordinate system: 1. Highlight the Coordinate System field in the Details view of the Joint object. The origin of the coordinate system will include a yellow sphere indicating that the movement “mode” is active. 2. Click on any of the axis arrows you wish to change. Additional “handles” are displayed for each axis. 444 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections 3. Click on the handle or axis representing the new direction to which you want to reorient the initially selected axis. The axis performs a flip transformation. 4. Click the Apply button. The image of the coordinate system changes from movement mode to a permanent presence at the new orientation. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 445 Features You can change or delete the status of the flip transformation by highlighting the Reference Coordinate System object or a Mobile Coordinate System object and making the change or deletion under the Transformations category in the Details view of the child joint coordinate system. When selecting either a Reference Coordinate System object or a Mobile Coordinate System object, various settings are displayed in the Details view. These are the same settings that apply to all coordinate systems, not just those associated with joints. See the following section on coordinate systems: Initial Creation and Definition (p. 389) for an explanation of these settings. Behavior Use the Behavior property to specify scoped geometry as either Rigid or Deformable. Refer to the Geometry Behavior (p. 629) section for more information. In addition, if you scope a Joint's Reference group and a Joint's Mobile group to separate Remote Points, you can scope the Behavior of each group independently. Pinball Region Use the Pinball Region to define where the joint attaches to face(s) if the default location is not desirable. By default, the entire face is tied to the joint element. This may not be desirable, warranting the input of a Pinball Region setting, for the following reasons: • If the scoping is to a topology with a large number of nodes, this can lead to an inefficient solution in terms of memory and speed. • Overlap between the joint scoped faces and other displacement type boundary conditions can lead to over constraint and thus solver failures. Note The Pinball Region and Behavior settings are applicable to underlying bodies that are flexible. Stops See Joint Stops and Locks (p. 464). Applying Joints To add a joint manually: 1. 446 After importing the model, highlight the Model object in the tree and choose the Connections button from the toolbar. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections 2. Highlight the new Connections object and choose either Body-Ground> {type of joint} or BodyBody> {type of joint} from the toolbar, as applicable. Refer to the Types of Joints (p. 436) section for details. 3. Highlight the new Joint object and scope the joint to a face. 4. Reposition the coordinate system origin location or orientation as needed. The Body Views button in the toolbar displays Reference and Mobile bodies in separate windows with appropriate transparencies applied. You have full body manipulation capabilities in each of these windows. 5. Configure the joint. The Configure button in the toolbar positions the Mobile body according to the joint definition. You can then manipulate the joint interactively (for example, rotate the joint) directly on the model. See the Example: Configuring Joints (p. 458) section for an application of using the Configure tool. Also see the “Notes on the Configure and Assemble Tools” below for more information. The Set button in the toolbar locks the changed assembly for use in the subsequent analysis. Note The triad position and orientation may not display correctly until you click on the Set button. The Revert button in the toolbar restores the assembly to its original configuration from DesignModeler or the CAD system. 6. Consider renaming the joint objects based on the type of joint and the names of the joined geometry. 7. Display the Joint DOF Checker and modify joint definitions if necessary. 8. Create a redundancy analysis to interactively check the influence of individual joint degrees of freedom on the redundant constraints. Notes on the Configure and Assemble Tools The Configure and Assemble tools are a good way to exercise the model and joints before starting to perform a transient analysis. They are also a way to detect locking configurations. The Assemble tool performs the assembly of the model, finding the closest part configuration that satisfies all the joints. The Configure tool performs the assembly of the model, with a prescribed value of the angle or translational degree of freedom that you are configuring. For the Assemble tool, all the joints degrees of freedom values are considered to be free. For the Configure joint, the selected DOF is considered as prescribed. In both cases, the solver will apply all constraint equations, solve the nonlinear set of equations, and finally verify that all of them are satisfied, including those having been considered as being redundant. The violation of these constraints is compared to the model size. The model size is not the actual size of the part – as the solver does not use the actual geometry, but rather a wireframe representation of the bodies. Each body holds some coordinate systems – center of mass, and joint coordinate systems. For very simple models, where the joints are defined at the center of mass, the size of the parts is zero. The violation of the constraint equations is then compared to very small reference size, and the convergence becomes very difficult to reach, leading the Configure tool or the Assemble tool to fail. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 447 Features Example: Assembling Joints This section illustrates the details of assembling geometry using an example of a three-part a pendulum joint model. The Assemble feature allows you to bring in CAD geometry that may initially be in a state of disassembly. After importing the CAD geometry, you can actively assemble the different parts and Set them in the assembled configuration for the start of the analysis. The geometry shown for the example in Figure: Initial Geometry (p. 448) was imported into a Rigid Dynamics Analysis System. Figure: Initial Geometry This geometry consists of three bodies. In Figure: Initial Geometry (p. 448) they are (from left to right) the Basis, the Arm, and the PendulumAxis. These three bodies have been imported completely disjointed/separate from each other. The first step to orient and assemble the bodies is to add a Body-Ground Fixed joint to the body named Basis. To do this: 1. Select Connections from the Outline. 2. From the context sensitive menu, choose Body-Ground > Fixed. 448 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections 3. Click on a flat external face on the Basis body as seen in Figure: Selecting a Face for a Body-Ground Fixed Connection (p. 450). 4. In the Details view under Mobile, click in the Scope field and select Apply. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 449 Features Figure: Selecting a Face for a Body-Ground Fixed Connection Next, you need to join the PendulumAxis to the Basis. Since they are initially disjoint, you need to set two coordinate systems, one for the Basis and the other for the PendulumAxis. Additionally, to fully define the relative position and orientations of the two bodies, you must define a fixed joint between them. To do this: 1. From the context sensitive menu, click on Body-Body > Fixed. 2. Highlight the face on the Basis as shown below. 450 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections 3. In the Details view, click on the Scope field under Reference and select Apply. 4. Select the cylindrical face on the PendulumAxis. 5. In the Details view, select the Scope field under Mobile and select Apply. Figure: Creating a Mobile Coordinate System 6. Also, change the Initial Position value under Mobile from Unchanged to Override. Now, the joint has two coordinate systems associated with it: A Reference and a Mobile coordinate system. Next, you must associate the Reference and the Mobile Coordinate Systems to the respective bodies with the appropriate orientations. To associate the Reference Coordinate System to the respective bodies: 1. In the Outline, highlight Reference Coordinate System. 2. In the Details view, click on the box next to Geometry under Origin. 3. Select the two internal rectangular faces on the Basis as shown in Figure: Creating the Reference Coordinate System (p. 452) and in the Details view, select Apply. This will center The Reference Coordinate System at the center of the hole on the Basis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 451 Features Figure: Creating the Reference Coordinate System To associate the Mobile Coordinate System to the respective bodies: 1. Highlight the Mobile Coordinate System (this coordinate system is associated with the Basis). 2. In the Details view, click in the Geometry field under Origin. 3. Select the cylindrical surface on the PendulumArm. 4. In the Details view, click Apply. 452 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Figure: Creating the Mobile Coordinate System Next, you will need to orient the PendulumAxis coordinate system so that it is oriented correctly in the assembly: 1. In the Mobile Coordinate System associated with the PendulumAxis, click in the box next to Geometry under Principal Axis (set to Z). 2. Select one of the vertical edges on the PendulumAxis such that the Z axis is parallel to it as shown in Figure: Orienting the Pendulum Axis (p. 454). In the Details view, click Apply. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 453 Features Figure: Orienting the Pendulum Axis 3. With Mobile Coordinate System highlighted in the Outline, select the x-offset button in the context sensitive menu. 4. In the Details view, enter an Offset X value of 2.5mm to align the faces of the PendulumAxis with the Basis. Note The transformations available allow you to manipulate the coordinate systems by entering offsets or rotations in each of the 3 axis. The two coordinate systems that were just defined should look similar to the figure below. Figure: Oriented Coordinate Systems Next, you will need to define the coordinate systems to join the Arm to the PendulumAxis during assembly. 1. 454 From the context sensitive menu, select Body-Body > Fixed. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections 2. To define the Reference Scope, choose one of the faces of the Arm that will be connected to the PendulumAxis then select Apply. Figure: Selecting an Arm Face for Connection 3. Now, configure the Mobile Scope by selecting the flat end face of the PendulumAxis as shown in Figure: Scoping the Mobile Coordinate Systems (p. 456), then select Apply. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 455 Features Figure: Scoping the Mobile Coordinate Systems 4. Set the Initial Position under Mobile from Unchanged to Override. 5. Finally, set the Origin of the Reference Coordinate System to the center of the hole in the Arm using the same procedure described above for the Basis. Next, you will need to offset the Coordinate System associated with the Arm so that the faces on the Arm are aligned with the end face of the PendulumAxis. 1. With Reference Coordinate System highlighted, choose the x-offset button in the context sensitive menu. 2. Enter an Offset X value of -5mm. Note The transformations available allow you to manipulate the coordinate systems by entering offsets or rotations in each of the 3 axis. 3. Next, Highlight the Mobile Coordinate System. This coordinate system is associated with the Arm. Click the box next to Geometry under Origin 4. Select the flat surface on the PendulumArm and click Apply. 456 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Now you will need to orient the PendulumAxis so that its faces are aligned with the faces on the Arm during the Assemble process. 1. Highlight the Mobile Coordinate System that is assigned to the PendulumAxis. 2. From the Details view, click the in the Geometry field under Principal Axis and select an edge of the PendulumAxis as shown in the figure. Figure: Choose an Edge to Orient the PendulumAxis Geometry 3. Under Principal Axis In the Details view, select Apply in the Geometry field to orient the PendulumAxis to this edge. Now that the three bodies have been oriented and aligned, they are ready to be assembled. 1. In the Outline, highlight Connections. 2. From the context sensitive menu, click Assemble. The parts should snap together in place and resemble Figure: Assembled Geometry (p. 458). If the geometry you're attempting to assemble has not snapped into place as expected, you should retrace your previous Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 457 Features steps to make sure that the coordinate systems are properly oriented. If your assembly has been successfully performed, then click Set in the context sensitive menu to place the assembly in its assembled position to start the analysis. Figure: Assembled Geometry Example: Configuring Joints This section illustrates the details of configuring joints using an example of creating a pendulum from the two links shown below. To achieve the result, the following two revolute joints were configured: • The first joint is intended to allow rotation of the top link's upper hole referenced to a stationary point. • The second joint is intended to allow rotation of the bottom link's upper hole referenced to the top link's lower hole. The following steps illustrate the details of the joint configurations: 1. 458 After attaching the model to the Mechanical application, create the first joint. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections • 2. Scope the mobile side of the first joint to the top link's upper hole. • 3. Select inside surface of hole, then under Mobile in the Details view, click the Apply button for Scope. Create the second joint. • 4. Highlight Model object folder and choose Connections from the toolbar. Then choose BodyGround> Revolute from the toolbar. Choose Body-Body> Revolute from the toolbar. Scope the reference side of the second joint to the top link's lower hole. • Select inside surface of hole, then under Reference in the Details view, click the Apply button for Scope. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 459 Features 5. Scope the mobile side of the second joint to the bottom link's upper hole. • 6. Select inside surface of hole, then under Mobile in the Details view, click the Apply button for Scope. The two holes intended to form the second joint are not aligned to correctly create the joint. To align the holes, first create a coordinate system for the mobile side of the second joint, then align the mobile and reference coordinate systems. Create the mobile coordinate system in this step. 460 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections • 7. Scope the new mobile coordinate system to the back edge of the bottom link's upper hole. • 8. Highlight Joint 2 in the tree and choose Override in the Initial Position drop down list. Note the creation of the new coordinate system. Select the back edge of the bottom link's upper hole, then under Mobile, click the Coordinate System field and the Apply button. Scope the existing reference coordinate system to the back edge of the top link's lower hole. • Select the back edge of the top link's lower hole, then under Reference, click the Coordinate System field and the Apply button. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 461 Features The holes are now correctly aligned for creation of the joint. 9. Establish the initial position of each joint. • 462 Highlight one of the joint objects in the tree and click the Configure button in the toolbar. The joint is graphically displayed according to your configuration. In addition, a triad appears with straight lines representing translational degrees of freedom and curved lines representing rotational degrees of freedom. Among these, any colored lines represent the free degrees of freedom for the joint type. For the joint that is being configured, the translational displacement degrees of freedom always follow the Geometry units rather than the current Mechanical units. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections By dragging the mouse cursor on a colored line, the joint will move allowing you to set the initial position of the joint through the free translational or rotational degrees of freedom. For rotations, holding the Ctrl key while dragging the mouse cursor will advance the rotation in 10 degree increments. You can also type the value of the increment into the ∆ = field on the toolbar. Clicking the Configure button again cancels the joining and positioning of the joint. 10. Create the joints. • After configuring a joint's initial position, click the Set button to create the joint. At this point, you also have the option of returning the configuration to the state it was in before joint creation and upon attaching to the Mechanical application by clicking the Revert toolbar button. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 463 Features Automatic Joint Creation This section discusses the automatic joint creation in the Mechanical application. You can also create joints manually as discussed in Joint Properties and Application (p. 442). Creating Joints Automatically You can direct the Mechanical application to analyze your assembly and automatically create fixed joints and/or revolute joints. To create joints automatically: 1. Insert a Connection Group object under the Connections folder either from the toolbar button or by choosing Insert from the context menu (right mouse click) for this folder. 2. From the Details view of the Connection Group object, choose Joint from the Connection Type drop down menu. 3. Select some bodies in the model based on the Scoping Method. The default is Geometry Selection scoped to All Bodies. 4. Configure the types of joints (fixed and/or revolute) you want the Mechanical application to create automatically through the appropriate Yes or No settings in the Details view. These properties will be applied only to scoped geometries for this connection group. You can set defaults for these settings using the Options dialog box under Connections. Note When both the Fixed Joints and Revolute Joints properties are set to Yes, the revolute joints have priority; the search for revolute joints will be processed first followed by the search for fixed joints. 5. Choose Create Automatic Connections from the context menu (right mouse click) for the Connection Group. Appropriate joint types are created and appear in the tree as objects under the Joints folder. Each joint also includes a reference coordinate system that is represented as a child object to the joint object. 6. Display the Joint DOF Checker or the redundancy analysis and modify joint definitions if necessary. Joint Stops and Locks Stops and Locks are optional constraints that may be applied to restrict the motion of the free relative degree(s) of freedom (DOF) of most types of joints. Any analysis that includes a valid joint type can involve Stops and/or Locks. For the applicable joint types, you can define a minimum and maximum (min, max) range inside of which the degrees of freedom must remain. A Stop is a computationally efficient abstraction of a real contact, which simplifies geometry calculations. For Stops, a shock occurs when a joint reaches the limit of the relative motion. A Lock is the same as a Stop except that when the Lock reaches the specified limit for a degree of freedom the Lock becomes fixed in place. For joints with free relative DOFs, the Details view displays a group of options labeled Stops. This grouping displays the applicable free DOFs (UX, UY, UZ, ROTX. etc.) for the joint type from which you specify the constraint as a Stop or a Lock. By default, no Stop or Lock is specified, as indicated by the 464 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections default option, None. You can select any combination of options. For stops and locks, the minimum and maximum values you enter are relative to the joint’s coordinate system. Stops and Locks are applied to the following Joint Types. Joint Type Stop/Lock Revolute Yes Cylindrical Yes Translational Yes Slot Translational Universal Yes Spherical No Planar Yes General Translational Note • When using the ANSYS Mechanical solver, Stops and Locks are active only when Large Deflection is set to On (under Analysis Settings (p. 980)). This is because Stops and Locks make sense only in the context of finite deformation/rotation. If Large Deflection is Off, all calculations are carried out in the original configuration and the configuration is never updated, preventing the activation of the Stops and Locks. • It is important to apply sensible Stop and Lock values to ensure that the initial geometry configuration does not violate the applied stop/lock limits. Also, applying conflicting boundary conditions (for example, applying Acceleration on a joint that has a Stop, or applying Velocity on a joint that has a Stop) on the same DOF leads to non-physical results and therefore is not supported. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 465 Features Solver Implications Stops and Locks are available for both the ANSYS Rigid Dynamics and ANSYS Mechanical solvers, but are handled differently in certain circumstances by the two independent solvers. • For the ANSYS Rigid Dynamics solver the shock is considered as an event with no duration, during which the forces and accelerations are not known or available for postprocessing, but generate a relative velocity "jump". • For the ANSYS Mechanical solver the stop and lock constraints are implemented via the Lagrange Multiplier method. The constraint forces due to stop and lock conditions are available when stop is established Coefficient of Restitution For the ANSYS Rigid Dynamics solver, Stops require you to set a coefficient of restitution value. This value represents the energy lost during the shock and is defined as the ratio between the joint’s relative velocity prior to the shock and the velocity following the shock. This value can be between 0 and 1. For a restitution value of zero, a Stop is released when the force in the joint is a traction force, while a Lock does not release. A restitution factor equal to 1 indicates that no energy is lost during the shock, that is, the rebounding velocity equals the impact velocity (a perfectly elastic collision). The coefficient of restitution is not applicable to the stops on the joints when using the ANSYS Mechanical solver. Ease of Use Features The following ease of use features are available when defining joints: • Renaming Joint Objects Based on Definition (p. 466) • Joint Legend (p. 467) • Disable/Enable Transparency (p. 467) • Hide All Other Bodies (p. 468) • Flip Reference/Mobile (p. 468) • Joint DOF Checker (p. 468) • Analyze Joint Redundancies (p. 468) Renaming Joint Objects Based on Definition When joints are created, the Mechanical application automatically names each of the joint objects with a name that includes the type of joint followed by the names of the joined parts included as child objects under the Geometry object folder. For example, if a revolute joint connects a part named ARM to a part named ARM_HOUSING, then the object name becomes Revolute - ARM To ARM_HOUSING. The automatic naming based on the joint type and geometry definition is by default. You can however change the default from the automatic naming to a generic naming of Joint, Joint 2, Joint 3, and so on by choosing Tools> Options and under Connections, setting Auto Rename Connections to No. If you then want to rename any joint object based on the definition, click the right mouse button on the object and choose Rename Based on Definition from the context menu. You can rename all joints by clicking the right mouse button on the Joints folder then choosing Rename Based on Definition. 466 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections The behavior of this feature is very similar to renaming manually created contact regions. See Renaming Contact Regions Based on Geometry Names (p. 428) for further details including an animated demonstration. Joint Legend When you highlight a joint object, the accompanying display in the Geometry window includes a legend that depicts the free degrees of freedom characteristic of the type of joint. A color scheme is used to associate the free degrees of freedom with each of the axis of the joint's coordinate system shown in the graphic. An example legend is shown below for a slot joint. You can display or remove the joint legend using View> Legend from the main menu. Disable/Enable Transparency The Enable Transparency feature allows you to graphically highlight a particular joint that is within a group of other joints, by rendering the other joints as transparent. The following example shows the same joint group presented in the Joint Legend (p. 467) section above but with transparency enabled. Note that the slot joint alone is highlighted. To enable transparency for a joint object, click the right mouse button on the object and choose Enable Transparency from the context menu. Conversely, to disable transparency, click the right mouse button on the object and choose Disable Transparency from the context menu. The behavior of this feature is very similar to using transparency for highlighting contact regions. See Controlling Transparency for Contact Regions (p. 427) for further details including an animated demonstration. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 467 Features Hide All Other Bodies You can hide all bodies except those associated with a particular joint. To use this feature, click the right mouse button on the object and choose Hide All Other Bodies from the context menu. Conversely, to show all bodies that may have been hidden, click the right mouse button on the object and choose Show All Bodies from the context menu. Flip Reference/Mobile For body-to-body joint scoping, you can reverse the scoping between the Reference and Mobile sides in one action. To use this feature, click the right mouse button on the object and choose Flip Reference/Mobile from the context menu. The change is reflected in the Details view of the joint object as well as in the color coding of the scoped entity on the joint graphic. The behavior of this feature is very similar to the Flip Contact/Target feature used for contact regions. See Flipping Contact and Target Scope Settings (p. 429) for further details including an animated demonstration. Joint DOF Checker Once joints are created, fully defined, and applied to the model, a Joint DOF Checker calculates the total number of free degrees of freedom. The number of free degrees of freedom should be greater than zero in order to produce an expected result. If this number is less than 1, a warning message is displayed stating that the model may possibly be overconstrained, along with a suggestion to check the model closely and remove any redundant joint constraints. To display the Joint DOF Checker information, highlight the Connections object and click the Worksheet button. The Joint DOF Checker information is located just above the Joint Information heading in the worksheet. Analyze Joint Redundancies Using this feature allows you to analyze an assembly which is held together by joints. Also, this analysis will assist in helping you solve over constrained assemblies. Each body in an assembly has a limited degree of freedom set. The joint constraints must be consistent to the motion of each body, otherwise the assembly can be locked or the bodies may move in directions other than you want. The redundancy analysis checks the joints you define and indicates the joints that over constrain the assembly. To analyze an assembly for joint redundancies: 1. Right-click the Connections object, and then click Redundancy Analysis to open a worksheet with a list of joints. 2. Click Analyze to perform a redundancy analysis. All the over constrained joints are indicated as redundant. 3. Click the Redundant label, and then select Fixed or Free to resolve the conflict manually. or Click Convert Redundancies to Free to remove all over constrained degrees of freedom. 4. Click Set to update the Joint definitions. Note Click Export to save the worksheet to an Excel/text file. 468 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Detecting Overconstrained Conditions Overconstrained conditions can occur when more constraints than are necessary are applied to a joint's degrees of freedom. These conditions may arise when rigid bodies are joined together using multiple joints. The overconstraints could be due to redundant joints performing the same function, or contradictory motion resulting from improper use of joints connecting different bodies. • For the Transient Structural analysis type, when a model is overconstrained, nonconvergence of the solution most often occurs, and in some cases, overconstrained models can yield incorrect results. • For the Rigid Dynamics analysis type, when a model is overconstrained, force calculation cannot be done properly. The following features exist within the Mechanical application that can assist you in detecting possible overconstrained conditions: • Use the Joint DOF Checker (p. 468) for detecting overconstrained conditions before solving (highlight Connections object and view the Worksheet). In the following example, the original display of the Joint DOF Checker warns that the model may be overconstrained. After modifying the joint definitions, the user displays the Joint DOF Checker again, which shows that the overconstrained condition has been resolved. • After solution, you can highlight the Solution Information object, then scroll to the end of its content to view any information that may have been detected on model redundancies that caused overconstrained conditions. An example is presented below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 469 Features Mesh Connection The mesh connection feature allows you to join the meshes of topologically disconnected surface bodies that may reside in different parts. In the past, this process was done at the geometry level (for example, by using the DesignModeler application to repair small gaps). However, geometry tolerances are tighter than the tolerances used by mesh connections and often lead to problems in obtaining conformal mesh. With mesh connections, the connections are made at the mesh level and tolerance is based locally on mesh size. A connection can be edge-to-edge or edge-to-face. The mesh connection feature automatically generates post pinch controls internally at meshing time, allowing the connections to work across parts so that a multibody part is not required: • Edge-to-edge – Connect an edge on one face to edge(s) on another face to pinch out mesh/gap in between. • Edge-to-face – Connect edge(s) on face(s) to another face to pinch out the gap and create conformal mesh between the edge(s) and face(s). Although pinch controls can be pre or post, all mesh connections are post. “Post” indicates that the mesh is pinched in a separate step after meshing is complete, whereas in a “pre” pinch control, the boundary mesh is pinched prior to face mesh generation. Since mesh connections are a post mesh process, the base mesh is stored to allow for quicker updates. That is, if you change a mesh connection or meshing control, only local re-meshing is required to clean up the neighboring mesh. Surface Bodies With No Shared Topology: Same Surface Bodies With Edge-To-Edge Mesh Connection Established: 470 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Enabling Mesh Connections To enable the mesh connection feature: 1. Insert Mesh Connection objects manually or automatically. • For more control, or to control the engineering design, you may want to insert mesh connections manually. • Alternatively, you can use automatic mesh connections, and then review and adjust each connection as appropriate. The automatic mesh connections feature is very helpful, but it can also find and create connections that you may not want. It is best practice to review the connections, or at least be aware that if problems arise, they may be due to automatic mesh connections. See Automatic Mesh Connection and Common Connections Folder Operations for Auto Generated Connections (p. 407) for details. 2. In the Details view specify Master Geometry and Slave Geometry. • “Master” indicates the topology that will be captured after the operation is complete. In other words, it is the topology to which other topologies in the connection are projected. • “Slave” indicates the topology that will be pinched out during the operation. In other words, it is the topology that is projected to other topologies involved in the connection. The master geometry can be one or more faces or edges while the slave geometry can only be one or more edges. When specifying faces, the annotation is displayed on both sides of the faces. Note Mesh connections support common imprints, which involve multiple slaves connected at the same location to a common master. See Common Imprints and Mesh Connections (p. 474). 3. In the Details view specify Tolerance. The Tolerance here has a similar meaning to the Tolerance Value global connection setting, and is represented as a transparent sphere. See Tolerances Used in Mesh Connections (p. 472) for details about Tolerance and how it relates to the Snap Tolerance described below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 471 Features 4. For edge-to-face mesh connections only, in the Details view specify Snap to Boundary and Snap Type. When Snap to Boundary is Yes (the default) and the distance from a slave edge to the closest mesh boundary of the master face is within the specified snap to boundary tolerance, nodes from the slave edge are projected onto the boundary of the master face. The joined edge will be on the master face along with other edges on the master face that fall within the defined pinch control tolerance. See Pinch Control for details. Snap Type appears only when the value of Snap to Boundary is Yes. • If Snap Type is set to Manual Tolerance (the default), a Snap Tolerance field appears where you may enter a numerical value greater than 0. By default, the Snap Tolerance is set equal to the pinch tolerance but it can be overridden here. See Tolerances Used in Mesh Connections (p. 472) for details about Snap Tolerance and how it relates to the Tolerance described above. • If Snap Type is set to Element Size Factor, a Master Element Size Factor field appears where you may enter a numerical value greater than 0. The value entered should be a factor of the local element size of the master topology. Note For edge-to-edge mesh connections (or edge-to-edge pinch controls), the snap tolerance is set equal to the pinch tolerance internally and cannot be modified. 5. Highlight the Mesh folder and choose Generate Mesh (right-click and choose from context menu). The surface bodies are displayed and show the mesh connections. Tolerances Used in Mesh Connections You can set two separate tolerances to define mesh connections. Setting appropriate tolerances is often critical to obtaining high quality mesh that adequately represents the geometry you want to capture. • Tolerance – Projection tolerance to close gaps between bodies. • Snap Tolerance – Snap to boundary tolerance to sew up mesh at the connection (applicable to edgeto-face mesh connections only). The Tolerance value is used to find which bodies should be connected to which other bodies. Setting a larger Tolerance connects more bodies together, while setting it smaller may cause some connections to be missed. For this reason, you may be motivated to set this to a larger value than needed. Setting a smaller value can avoid problems in automatic mesh connection creation, but also can result in other problems because the tolerance used in meshing is inherited from automatic mesh connection detection settings. 472 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Using a Large Tolerance Value For a large assembly for which you do not want to define mesh connections manually, automatic mesh connection detection provides many benefits. Setting a large Tolerance value to find connections yields more connections, which provides a higher level of comfort that the model is fully constrained. However, larger values can be problematic for the following reasons: • When more automatic mesh connections are created, more duplicates can be created and the mesher decides ultimately which connections to create. In general, making these decisions yourself is a better approach. • The Snap Tolerance defaults to the same value as the Tolerance. If the value of Tolerance is too large for Snap Tolerance, the mesher may be too aggressive in pinching out mesh at the connection, and hence the mesh quality and feature capturing may suffer. Using a Small Tolerance Value When mesh connections are generated automatically, the Tolerance is used on the geometry edges and faces to determine which entities should be connected. However, the connections themselves are not generated until meshing occurs. Because the connections are made on nodes and elements of the mesh rather than on the geometry, the tolerances do not translate exactly. For example, in the case below, you would want to set a Tolerance that is slightly larger than the gap in the geometry. If the gap is defined as x and the tolerance is set to x, automatic mesh connection detection could find the connection, but the meshing process may result in mesh that is only partially connected. Tips for Setting Tolerances As detailed above, setting the correct tolerance can be very important, and in some cases may require some speculation and/or experimentation. The following tips may help: • You can adjust the Tolerance used to generate automatic mesh connections after the connections are found. Sometimes it is a good idea to use one Tolerance value to find the mesh connections, select all the mesh connections, and then reduce or increase the Tolerance later. • Having Snap to Boundary turned on and using a Snap Tolerance are not always advisable. It depends on the model and the features you want to capture. Mesh Sizing and Mesh Connections Mesh size has an effect on the quality and feature capture of a mesh connection as follows: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 473 Features • Mesh size always affects the base mesh, as features are only captured relative to mesh size. • During mesh connection processing, the base mesh is adjusted according to the common imprint/location. In cases where there is a large projection or a large difference in mesh sizes between the master entity and the slave entity, the common edge between bodies can become jagged. Also, as local smoothing takes place, there can be some problems in transition of element sizes. You can often use one of the following strategies to fix the problem: – Use more similar sizes between source and target. – Improve the tolerance used by mesh connections (either for projection, or for snapping to boundary). – Adjust the geometry's topology so that the base mesh is more accommodating to the mesh connection. See Common Imprints and Mesh Connections (p. 474). Common Imprints and Mesh Connections The tolerance for common imprints comes from the minimum element size in the footprint mesh, which is the horizontal plate in the example below. Common imprints are made if the gap between imprints is smaller than or equal to the minimum element size in the connection region. For this reason, setting the mesh size appropriately is important to control whether the imprints will be common or not. For example, in the case shown below, if you want a common imprint, the minimum element size (or element size if Use Advanced Size Function is Off) should be > x. In this case, you could scope local face mesh sizing on the horizontal plate to control the sizing. Automatic Mesh Connection Mesh connections can be automatically generated using the Create Automatic Connections option available from the right-click context menu of the Connections or Connection Group folder. See Automatically Generated Connections for details. The Tolerance Value, pairing type and other properties used for auto detection can be set in the Details view of the Connection Group folder under the Auto Detection group. Sheet thickness can also be used as a tolerance value (see Common Connections Folder Operations for Auto Generated Connections (p. 407) for details). 474 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Mesh Connections for Selected Bodies You can select a geometric entity and lookup the Mesh Connection object in the tree outline. To find the relevant mesh connection object: • Right-click a geometric entity, and then click Go To > Mesh Connections for Selected Bodies. Mesh Connections Common to Selected Bodies You can select a pair of geometric entities and lookup the shared Mesh Connection object in the tree outline. To find a relevant mesh connection object: • Select the appropriate pair, and then click Go To > Mesh Connections Common to Selected Bodies. This option can be helpful for finding spurious mesh connections, in which case duplicates can be removed. Displaying Multiple Views of Mesh Connections Use the Body Views button on the Connections Context Toolbar to display parts in separate auxiliary windows. For closer inspection of mesh connections, you can use the Show Mesh option on the Graphics Options Toolbar along with Body Views. Diagnosing Failed Mesh Connections General Failures In the event of a general mesh connection failure, the following approach is recommended: 1. If a message provides “Problematic Geometry” information, select the message, right-click, and select Show Problematic Geometry from the context menu. This action highlights the geometry in the Geometry window that is responsible for the message. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 475 Features Note Any error message that is related to a specific mesh connection will be associated with the slave geometry in the connection. 2. Select the problematic bodies, right-click, and select Go To > Mesh Connections for Selected Bodies. This action highlights all mesh connections attached to the problematic geometry. 3. Review the tolerances and mesh sizes associated with the highlighted connections. Failures Due to Defeaturing from Uniform Quad/Tri Meshing and/or Pinch Controls Due to the patch independent nature of the Uniform Quad/Tri and Uniform Quad mesh methods, a connection may fail because the mesh is associated with some face of the body but not with the face that is involved in the connection. This type of mesh connection failure, which may also occur when pinch controls are defined, is the result of the part mesh being significantly defeatured prior to mesh connection generation. To avoid mesh connection failures when using Uniform Quad(/Tri) and/or pinch controls, use one of the following approaches: • Use virtual topology to merge the faces of interest with the adjacent faces to create large patches, and then apply mesh connections to the patches. • Protect small faces in mesh connections by defining Named Selections. The software does not automatically extend the connection region because doing so may lose the engineering intent of the model. For example, consider the two parts shown below. If you are using the Uniform Quad(/Tri) mesh method or pinch controls, the part mesh may look like the one shown below. Notice that one face has been defeatured out. In this case: • 476 If the defeatured face is the one defined in the mesh connection, the connection will fail. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections • If the other face is the one defined in the mesh connection, the connection will succeed. • If you include both faces in the mesh connection, the connection will succeed. Since you cannot always control which face is defeatured, the most robust and recommended approach is to include both faces in the mesh connection. Points to Remember • Toggling suppression of mesh connections or changing their properties causes bodies affected by those mesh connections to have an unmeshed state. However, when you subsequently select Generate Mesh, only the connections will be regenerated. Since mesh connections are a post mesh process, a re-mesh is not necessary and will not occur. • Mesh connections cannot be generated incrementally. Anytime you add or change mesh connections and select Generate Mesh, processing starts with the mesh in its unsewn (pre-joined) state and then re-sews the entire assembly. This approach is necessary as mesh connections often have interdependencies which can have a ripple effect through the assembly of parts. It is often the case that a connection must be reevaluated across the assembly as a single connection may invalidate many. • With mesh connections, you can mix and match mesh methods and/or use selective meshing. • When using selective meshing and you generate mesh, only out-of-date parts are re-meshed but all mesh connections are regenerated. • Although the tolerance used for finding mesh connections and for generating mesh connections may be the same value, the tolerance itself has slightly different meanings in the two operations. When finding mesh connections, the tolerance is used to identify pairs of geometry edges or face(s)/edge(s). When generating mesh connections, the tolerance is used in pinching together the edge mesh or edge/face mesh. Since the geometry consists of NURBS, and the mesh consists of linear edges, the same tolerance may mean something slightly different in the two operations. For example, consider a geometry that consists of two cylindrical sheet parts that share an interface constructed from the same circle. Also consider that you are finding mesh connections with a tolerance of 0.0. In this case, the mesh connection is easily found because the two edges are exactly the same. However, when the mesh connection is being formed, some segments of the edge may fail to be pinched together if the mesh spacing of the two parts is different and thus the tolerance of the edge mesh is different. Also see Tolerances Used in Mesh Connections (p. 472). • For a higher order element, a midside node along the connection between a slave and a master is located at the midpoint between its end nodes, instead of being projected onto the geometry. • Although mesh connections do not alter the geometry, their effects can be previewed and toggled using the Graphics Options toolbar. • For the Shape Checking control, mesh connections support the Standard Mechanical option only. • If you define a mesh connection on topology to which a match control, mapped face meshing control, or inflation control (global or local) is already applied, a warning will be issued when you generate the mesh. The warning will indicate that the mesh connection may alter the mesh, which in turn may eliminate or disable the match, mapped face meshing, or inflation control. • Mesh connections and post pinch controls cannot be mixed with refinement or post inflation controls. • Refer to Clearing Generated Data for information about using the Clear Generated Data option on parts and bodies that have been joined by mesh connections or post pinch controls. • Refer to Using the Mesh Worksheet to Create a Selective Meshing History for information about how mesh connection operations are processed by the Mesh worksheet. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 477 Features Springs A spring is an elastic element that is used to store mechanical energy and which retains its original shape after a force is removed. Springs are typically defined in a stress free or “unloaded” state. This means that no longitudinal loading conditions exist unless preloading is specified (see below). In Workbench, the Configure feature is used to modify a Joint. If you configure a joint that has an attached spring, the spring must be redrawn in the Geometry window. In effect, the spring before the Configure action is replaced by a new spring in a new unloaded state. Springs are defined as longitudinal and they connect two bodies together or connect a body to ground. Longitudinal springs generate a force that depends on linear displacement. Longitudinal springs can be used as a damping force, which is a function of velocity or angular velocity, respectively. Springs can also be defined directly on a Revolute Joint (p. 436) or a Cylindrical Joint (p. 437). Note This boundary condition cannot be applied to a vertex scoped to an end release. Spring Behavior (applicable only to rigid dynamics analyses) You can define a longitudinal spring to support only tension loads or only compression loads. A property called Spring Behavior is available in the Details view for this purpose. You can set this property to Both (Linear), Compression Only or Tension Only. The tension only spring does not provide any restoring force against compression loads. The compression only spring does not provide resistance against tensile loads. The stiffness of a compression only or tension only spring without any preloads is shown below. Stiffness Behavior of a Tension Only Spring: Stiffness Behavior of a Compression Only Spring: 478 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Force Deflection Curve for a Tension Only Spring: Force Deflection Curve for a Compression Only Spring: If you are familiar with Mechanical APDL elements, Workbench uses COMBIN14 elements when Spring Behavior is set to Both (Linear), and uses LINK180 elements when Spring Behavior is set to either Compression Only or Tension Only. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 479 Features Preloading Workbench also provides you with the option to preload a spring and create an initial “loaded” state. The Preload property in the Details view allows you to define a preload as a length using Free Length or to specify a specific Load. The actual length is calculated using spring end points from the Reference and Mobile scoping. For rigid dynamics analyses, the spring will be under tension or compression depending upon whether you specified the free length as smaller or greater than the spring length, respectively. If preload is specified in terms of Load, a positive value creates tension and a negative value creates compression. Spring Length (applicable only to rigid dynamics analyses) The read-only property Spring Length displays the actual length of the spring which is calculated using the end points from the Reference and Mobile scoping. Scoping You can scope a spring to single or multiple faces, single or multiple edges, or to a single vertex. The scoping can either be from body-to-body or body-to-ground. For body-to-body scoping, there is a reference and mobile side. For body-to-ground scoping, the reference side is assumed to be grounded (fixed); scoping is only available on the mobile side. In addition to setting the scoping (where the spring attaches to the body), you can set the spring location on both the mobile and reference side. Since this is a unidirectional spring, these 2 locations determines the spring’s line of action. As such the spring reference and mobile location cannot be the same as this would result in a spring with zero length. Advanced Features Springs include Pinball Region and Behavior as advanced properties. Use the Pinball Region to define where the spring attaches to face(s), edge(s), or a single vertex if the default location is not desirable. By default, the entire face/edge/vertex is tied to the spring element. This may not be desirable, warranting the input of a Pinball Region setting, for the following reasons: • If the scoping is to a topology with a large number of nodes, this can lead to an inefficient solution in terms of memory and speed. • Overlap between the spring scoped faces and other displacement type boundary conditions can lead to over constraint and thus solver failures. Use the Behavior property to specify scoped geometry as either Rigid or Deformable. Refer to the Geometry Behavior (p. 629) section for more information. Note The Pinball Region and Behavior settings are applicable to underlying bodies that are flexible. A Spring is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 628) section for a listing of all remote boundary conditions and their characteristics. 480 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Output Several outputs are available via a spring probe. Applying Springs To add a spring: 1. After importing the model, highlight the Model object in the tree and choose the Connections button from the toolbar. 2. Highlight the new Connections object and choose either Body-Ground> Spring or Body-Body> Spring from the toolbar, as applicable. 3. Highlight the new Spring object and enter information in the Details view. Note that Longitudinal Damping is applicable only to transient analyses. Note The length of the spring connection must be greater than 0.0 with a tolerance of 1e-8 mm. Example: Longitudinal Spring with Damping This example shows the effect of a longitudinal spring connecting a rectangular bar to ground to represent a damper. A Transient Structural analysis was performed in the environment shown: The following are the Details view settings of the Spring object: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 481 Features Presented below is the Total Deformation result: The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the help. Interface names and other components shown in the demo may differ from those in the released product. 482 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Spring Incompatibility (applicable only to rigid dynamics analyses) If the preload for a longitudinal spring is a tensile load, then the spring cannot be defined as compression only. Alternatively, if the preload is a compressive load, then the spring cannot be defined as tension only. Should this case occur, the spring will be marked as underdefined and if you attempt to solve such a case, the following error message is displayed: “The preload for a spring is incompatible with its behavior being tension only spring or compression only spring.” Beam Connections A beam is a structural element that carries load primarily in bending (flexure). Using beams, you can establish a body to body or a body to ground connection. You can use beams for structural analyses. To add a beam: 1. In the Project tree, select Model to make the Model toolbar available. 2. On the Model toolbar, click Connections . 3. On the Connections toolbar, click Body-Ground or Body-Body, and then click Beam to add a circular beam under connections. 4. In the Details View, under Definition, click the Material fly-out menu, and then select a material for the beam. 5. Type the beam radius. 6. Under Reference, type the X, Y, and Z coordinate to define the reference point, or select a face, edge, or vertex, and then click Apply. This step is not required if you chose Body-Ground above. 7. Under Mobile, type the X, Y, and Z coordinate to define the reference point, or select a face, edge, or vertex, and then click Apply. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 483 Features Note • For Body-Ground beam connections, the reference side is fixed. For Body-Body beam connections, you must define the reference point for each body. • The length of the beam connection must be greater than 0.0 with a tolerance of 1e-8 mm. The Beam Probe results provide you the forces and moments in the beam from your analysis. Spot Welds Spot welds are used to connect individual surface body parts together to form surface body model assemblies, just as a Contact Region is used for solid body part assemblies. Structural loads are transferred from one surface body part to another via the spot weld connection points, allowing for simulation of surface body model assemblies. Spot Weld Details Spot welds are usually defined in the CAD system and automatically generated upon import, although you can define them manually in the Mechanical application after the model is imported. Spot welds then become hard points in the geometric model. Hard points are vertices in the geometry that are linked together using beam elements during the meshing process. Spot weld objects are located in a Connection Group folder. When selected in the tree, they appear in the graphical window highlighted by a black square around a white dot on the underlying vertices, with an annotation. If a surface body model contains spot weld features in the CAD system and the Auto Detect Contact On Attach is turned on in Workbench Tools>Options>Mechanical, then Spot Weld objects are generated when the model is read into the Mechanical application. Spot weld objects will also get generated during geometry refresh if the Generate Automatic Connection On Refresh is set to Yes in the Details view of the Connections folder. This is similar to the way in which the Mechanical application automatically constructs contacts when reading in assemblies models and refreshing the geometry. You can manually generate spot welds as you would insert any new object into the Outline tree. Either insert a spot weld object from the context menu and then pick two appropriate vertices in the model, or pick two appropriate vertices and then insert the spot weld object. You can define spot welds for CAD models that do not have a spot weld feature in the CAD system, as long as the model contains vertices at the desired locations. You must define spot welds manually in these cases. Spot Weld Application Spot welds do not act to prevent penetration of the connected surface body in areas other than at the spot weld location. Penetration of the joined surface body is possible in areas where spot welds do not exist. Spot welds transfer structural loads and thermal loads as well as structural effects between solid, surface, and line body parts. Therefore they are appropriate for displacement, stress, elastic strain, thermal, and frequency solutions. 484 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections DesignModeler generates spot welds. The only CAD system whose spot welds can be fully realized in ANSYS Workbench at this time is NX. The APIs of the remaining CAD systems either do not handle spot welds, or the ANSYS Workbench software does not read spot welds from these other CAD systems. Spot Welds in Explicit Dynamics Analyses Spot welds provide a mechanism to rigidly connect two discrete points in a model and can be used to represent welds, rivets, bolts etc. The points usually belong to two different surfaces and are defined on the geometry (see DesignModeler help). During the solver initialization process, the two points defining each spot weld will be connected by a rigid beam element. Additionally, rigid beam elements will be generated on each surface to enable transfer of rotations at the spot weld location (see figure below). If the point of the spot weld lies on a shell body, both translational and rotational degrees of freedom will be linked at the connecting point. If the point of the spot weld lies on a the surface of a solid body, additional rigid beam elements will be generated to enable transfer of rotations at the spot weld location. Spot welds can be released during a simulation using the Breakable Stress or Force option. If the stress criteria is selected the user will be asked to define an effective cross sectional area. This is used to convert the defined stress limits into equivalent force limits. A spot weld will break (release) if the following criteria is exceeded Where: fn and fs are normal and shear interface forces Sn and Ssare the maximum allowed normal and shear force limits n and s are user defined exponential coefficients Not that the normal interface force fn is non-zero for tensile values only. After failure of the spot weld the rigid body connecting the points is removed from the simulation. Spot welds of zero length are permitted. However, if such spot welds are defined as breakable the above failure criteria is modified since local normal and shear directions cannot be defined. A modified criteria is used with global forces Where, are the force differences across the spot weld in the global coordinate system. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 485 Features Note A spot weld is equivalent to a rigid body and as such multiple nodal boundary conditions cannot be applied to spot welds. End Releases This feature allows you to release certain degrees of freedoms at a vertex shared by two or more edges of one or more line bodies, by using an End Release object. You can only apply one end release at the vertex and the edge must be connected to another edge at this vertex. To add an end release: 1. Add a Connections folder if one is not already in the tree, by highlighting the Model object and choosing Connections from the Model Context Toolbar (p. 288) or by choosing Insert >Connections from the context menu (right-click). 2. Add an End Release object by highlighting the Connections folder and choosing End Release from the Connections Context Toolbar (p. 290) or by choosing Insert >End Release from the context menu (right-click). 3. Set the following in the Details view: 486 a. Scoping Method as Geometry Selection (default) or Named Selection. b. Edge Geometry and Vertex Geometry, respectively. The vertex should be one of the two end vertices of the edge. c. Coordinate System as the Global Coordinate System or a local coordinate system that you may have defined previously. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections d. Release any of the translational and/or rotational degrees of freedoms in X, Y and Z directions by changing the individual settings from Fixed to Free. e. Connection Behavior as either Coupled (default) or Joint, using a coupling or a general joint, respectively. Notes • The end release feature is only applicable in structural analyses that use the ANSYS solver. The environment folder of other solvers will become underdefined when one or more End Release objects are present. • An end release object requires that the vertex must be on an edge and it should be shared with one or more other edges or one or more surface bodies. • A vertex cannot be scoped to more than one end release object. • The following boundary conditions are not allowed to be applied to a vertex or an edge that is already scoped to an end release The object will become underdefined with an error message: Fixed Support, Displacement, Simply Supported, Fixed Rotation, Velocity. • The following remote boundary conditions are not allowed to be applied to a vertex scoped to an end release The object will become underdefined with an error message: Remote Displacement, Remote Force, Moment, Point Mass, Thermal Point Mass, Spring, Joint. Body Interactions in Explicit Dynamics Analyses Within an explicit dynamics analysis, the body interaction feature represents contact between bodies and includes settings that allow you to control these interactions. If the geometry you use has two or more bodies in contact, a Body Interactions object folder appears by default under Connections in the tree. Included in a Body Interactions folder are one or more Body Interaction objects, with each object representing a contact pair. You can also manually add these two objects: • To add a Body Interactions folder, highlight the Connections folder and choose Body Interactions from the toolbar. A Body Interactions folder is added and includes one Body Interaction object. • To add a Body Interaction object to an existing Body Interactions folder, highlight the Connections folder, the Body Interactions folder, or an existing Body Interaction object, and choose Body Interaction from the toolbar. General Notes Each Body Interaction object activates an interaction for the bodies scoped in the object. With body interactions, contact detection is completely automated in the solver. At any time point during the analysis any node of the bodies scoped in the interaction may interact with any face of the bodies scoped in the interaction. The interactions are automatically detected during the solution. The default frictionless interaction type that is scoped to all bodies activates frictionless contact between any external node and face that may come into contact in the model during the analysis. To improve the efficiency of analyses involving large number of bodies, you are advised to suppress the default frictionless interaction that is scoped to all bodies, and instead insert additional Body Interaction objects which limit interactions to specific bodies. The union of all frictional/frictionless body interactions defines the matrix of possible body interactions during the analysis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 487 Features For example, in the model shown below: • Body A is traveling towards body B and we require frictional contact to occur. A frictional body interaction type scoped only to bodies A and B will achieve this. Body A will not come close to body C during the analysis so it does not need to be included in the interaction. • Body B is bonded to body C. A bonded body Interaction type, scoped to bodies B and C will achieve this. • If the bond between bodies B and C breaks during the analysis, we want frictional contact to take place between bodies B and C. A frictional body interaction type scoped only to bodies B and C will achieve this. A bonded body interaction type can be applied in addition to a frictional/frictionless body interaction. A reinforcement body interaction type be can be applied in addition to a frictional/frictionless body interaction. Object property settings are included in the Details view for both the Body Interactions folder and the individual Body Interaction objects. Refer to the following sections for descriptions of these properties. Properties for Body Interactions Folder Interaction Type Properties for Body Interaction Object Properties for Body Interactions Folder All properties for the Body Interactions folder are included in an Advanced category and define the global properties of the contact algorithm for the analysis. These properties are applied to all Body Interaction objects and to all frictional and frictionless manual contact regions. This section includes descriptions of the following properties for the Body Interactions folder: Contact Detection Formulation Shell Thickness Factor Body Self Contact Element Self Contact Tolerance Pinball Factor 488 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Time Step Safety Factor Limiting Time Step Velocity Edge on Edge Contact Contact Detection The available choices are described below. Trajectory The trajectory of nodes and faces included in frictional or frictionless contact are tracked during the computation cycle. If the trajectory of a node and a face intersects during the cycle a contact event is detected. The trajectory contact algorithm is the default and recommended option in most cases for contact in Explicit Dynamics analyses. Contacting nodes/faces can be initially separated or coincident at the start of the analysis. Trajectory based contact detection does not impose any constraint on the analysis time step and therefore often provides the most efficient solution. Note Trajectory Contact Detection is not supported for a distributed solve. If you would like to use Trajectory Contact Detection for a distributed solve, please contact ANSYS Technical Support. Note that nodes which penetrate into another element at the start of the simulation will be ignored for the purposes of contact and thus should be avoided. To generate duplicate conforming nodes across a contact interface: 1. Use the multibody part option in DesignModeler and set Shared Topology to Imprint. 2. For meshing, use Contact Sizing, the Arbitrary match control or the Match mesh Where Possible option of the Patch Independent mesh method. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 489 Features Proximity Based The external faces, edges and nodes of a mesh are encapsulated by a contact detection zone. If during the analysis a node enters this detection zone, it will be repelled using a penalty based force. Note 490 • An additional constraint is applied to the analysis time step when this contact detection algorithm is selected. The time step is constrained such that a node cannot travel through a fraction of the contact detection zone size in one cycle. The fraction is defined by the Time Step Safety Factor (p. 493) described below. For analyses involving high velocities, the time step used in the analysis is often controlled by the contact algorithm. • The initial geometry/mesh must be defined such that there is a physical gap/separation of at least the contact detection zone size between nodes and faces in the model. The solver will give error messages if this criteria is not satisfied. This constraint means this option may not be practical for very complex assemblies. • Proximity Based Contact is not supported in 2D explicit dynamics analyses. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Formulation This property is available if Contact Detection is set to Trajectory. The available choices are described below. Penalty If contact is detected, a local penalty force is calculated to push the node involved in the contact event back to the face. Equal and opposite forces are calculated on the nodes of the face in order to conserve linear and angular momentum. Trajectory based penalty force, Proximity based penalty force, Where: D is the depth of penetration M is the effective mass of the node (N) and face (F) ∆t is the simulation time step Note • Kinetic energy is not necessarily conserved. You can track conservation of energy in contact using the Solution Information object, the Solution Output, or one of the energy summary result trackers. • The applied penalty force will push the nodes back towards the true contact position during the cycle. However, it will usually take several cycles to satisfy the contact condition. Decomposition Response All contacts that take place at the same point in time are first detected. The response of the system to these contact events is then calculated to conserve momentum and energy. During this process, forces are calculated to ensure that the resulting position of nodes and faces does not result in further penetration at that time point. Note • The decomposition response algorithm cannot be used in combination with bonded contact regions. The formulation will be automatically switch to penalty if bonded regions are present in the model. • The decomposition response algorithm is more impulsive (in a given cycle) than the penalty method. This can give rise to large hourglass energies and energy errors. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 491 Features Shell Thickness Factor This property is available if the geometry includes one or more surface bodies and if Contact Detection is set to Trajectory. The Shell Thickness Factor allows you to control the effective thickness of surface bodies used in the contact. You can specify a value between 0.0 and 1.0. • A value of 0.0 means that contact will ignore the physical thickness of the surface body and the contact surface will be coincident with the mid-plane of the shell • A value of 1.0 means that the contact shell thickness will be equal to the physical shell thickness. The contact surface will be offset from the mid-plane of the shell by half the shell thickness (on both sides of the shell) Note Only node to surface contact is currently supported. For shell to shell contact, this means that contact takes place when the shell node impacts the shell contact surface as described above. Body Self Contact When set to Yes, the contact detection algorithm will check for external nodes of a body contacting with faces of the same body in addition to other bodies. This is the most robust option since all possible external contacts should be detected. When set to No, the contact detection algorithm will only check for external nodes of a body contacting with external faces of other bodies. This setting reduces the number of possible contact events and can therefore improve efficiency of the analysis. This option should not be used if a body is likely to fold onto itself during the analysis, as it would during plastic buckling for example. Presented below is an example of a model that includes self impact. Element Self Contact When set to Yes, automatic erosion (removal of elements) is enabled when an element deforms such that one of its nodes comes within a specified distance of one of its faces. In this situation, elements are removed before they become degenerated. Element self contact is very useful for impact penetration examples where removal of elements is essential to allow generation of a hole in a structure. 492 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Tolerance This property is available if Contact Detection is set to Trajectory and Element Self Contact is set to Yes. Tolerance defines the size of the detection zone for element self contact when the trajectory contact option is used. (see Element Self Contact (p. 492)). The value input is a factor in the range 0.1 to 0.5. This factor is multiplied by the smallest characteristic dimension of the elements in the mesh to give a physical dimension. A setting of 0.5 effectively equates to 50% of the smallest element dimension in the model. Note The smaller the fraction the more accurate the solution. Pinball Factor This property is available if Contact Detection is set to Proximity Based. The pinball factor defines the size of the detection zone for proximity based contact. The value input is a factor in the range 0.1 to 0.5. This factor is multiplied by the smallest characteristic dimension of the elements in the mesh to give a physical dimension. A setting of 0.5 effectively equates to 50% of the smallest element dimension in the model. Note The smaller the fraction the more accurate the solution. The time step in the analysis could be reduced significantly if small values are used (see Time Step Safety Factor (p. 493)). Time Step Safety Factor This property is available if Contact Detection is set to Proximity Based. For proximity based contact, the time step used in the analysis is additionally constrained by contact such that in one cycle, a node in the model cannot travel more than the detection zone size, multiplied by a safety factor. The safety factor is defined with this property and the recommended default is 0.2. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 493 Features Increasing the factor may increase the time step and hence reduce runtimes, but may also lead to missed contacts. The maximum value you can specify is 0.5. Limiting Time Step Velocity This property is available if Contact Detection is set to Proximity Based. For proximity based contact, this setting limits the maximum velocity that will be used to compute the proximity based contact time step calculation. Edge on Edge Contact This property is available if Contact Detection is set to Proximity Based. By default, contact events in explicit dynamics are detected by discrete nodes impacting surface events. Use this option to extend the contact detection to include discrete edges impacting other edges in the model. Note this option is numerically intensive and can significantly increase runtimes. It is recommended that you compare results with and without edge contact to make sure this feature is required. Interaction Type Properties for Body Interaction Object This section includes descriptions of the interaction types for the Body Interaction object: Frictionless Type Frictional Type Bonded Type Reinforcement Type Frictionless Type Setting Type to Frictionless activates frictionless sliding contact between any exterior node and any exterior face of the scoped bodies. Individual contact events are detected and tracked during the analysis. The contact is symmetric between bodies (that is, each node will belong to a master face impacted by adjacent slave nodes; each node will also act as a slave impacting a master face). Supported Connections Explicit Dynamics Connection Geometry Volume Shell Line Volume Yes Yes Yes Shell Yes Yes Yes Line Yes Yes *Yes *Only for Contact Detection = Proximity Based and Edge on Edge Contact = Yes (This option switches on contact between ALL lines / bodies / edges, that is, there is no dependence on the scoping selection of body interactions.) Explicit Dynamics (LS-DYNA Export) 494 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections Connection Geometry Volume Shell Line Volume Yes Yes No Shell Yes Yes No Line No No No Frictional Type Descriptions of the following properties are also addressed in this section: • Friction Coefficient • Dynamic Coefficient • Decay Constant Setting Type to Frictional activates frictional sliding contact between any exterior node and any exterior face of the scoped bodies. Individual contact events are detected and tracked during the simulation. The contact is symmetric between bodies (that is, each node will belong to a master face impacted by adjacent slave nodes, each node will also act as a slave impacting a master face). Friction Coefficient: A non-zero value will activate Coulomb type friction between bodies (F = µR). The relative velocity (ν) of sliding interfaces can influence frictional forces. A dynamic frictional formulation for the coefficient of friction can be used. µ = µd + (µs – µd) e-βν where µs = friction coefficient µd = dynamic coefficient of friction β = exponential decay coefficient ν = relative sliding velocity at point of contact Non-zero values of the Dynamic Coefficient and Decay Constant should be used to apply dynamic friction. Supported Connections Explicit Dynamics Connection Geometry Volume Shell Line Volume Yes Yes Yes Shell Yes Yes Yes Line Yes Yes *Yes *Only for Contact Detection = Proximity Based and Edge on Edge Contact = Yes (This option switches on contact between ALL lines / bodies / edges, that is, there is no dependence on the scoping selection of body interactions.) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 495 Features Explicit Dynamics (LS-DYNA Export) Connection Geometry Volume Shell Line Volume Yes Yes No Shell Yes Yes No Line No No No Bonded Type Descriptions of the following properties are also addressed in this section: • Maximum Offset • Breakable – Stress Criteria → Normal Stress Limit → Normal Stress Exponent → Shear Stress Limit → Shear Stress Exponent External nodes of bodies included in bonded interactions will be tied to faces of bodies included in the interaction if the distance between the external node and the face is less than the value (tolerance) defined by the user in Maximum Offset. The solver automatically detects the bonded nodes/faces during the initialization phase of the analysis. Note that it is important to select an appropriate value for the Maximum Offset (tolerance). The automatic search will bond everything together which is found within this value (tolerance). Use the custom variable BOND_STATUS to check bonded connections in Explicit Dynamics. The variable records the number of nodes bonded to the faces on an element during the analysis. This can be used not only to verify that initial bonds are generated appropriately, but also to identify bonds that break during the simulation. Maximum Offset defines the tolerance used at initialization to determine whether a node is bonded to a face. Breakable = No implies that the bond will remain throughout the analysis. Breakable = Stress Criteria implies that the bond may break (or be released) during the analysis. The criteria for breaking a bond is defined as . (σn/σnlim it)n + (|σs|/σslim it)m > or equal to 1 where σnlim it = Normal Stress Limit n = Normal Stress Exponent σslim it = Shear Stress Limit 496 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connections m = Shear Stress Exponent The options in the Advanced section are all currently ignored by the Explicit solver, including the Advanced > Pinball region option. The tolerance must be defined via the Maximum Offset value and is only used at initialization. Supported Connections Explicit Dynamics Connection Geometry Volume Shell Line Volume Yes Yes Yes Shell Yes Yes Yes Line Yes Yes Yes Note Bonded body interactions and contact are not supported for 2D Explicit Dynamics analyses. Explicit Dynamics (LS-DYNA Export)* Connection Geometry Volume Shell Line Volume Yes Yes No Shell Yes Yes No Line Yes Yes No *The above matrix is valid only for Contact Regions. Bonded body interactions are not supported at all. Reinforcement Type This body interaction type is used to apply discrete reinforcement to solid bodies. All line bodies scoped to the object will be flagged as potential discrete reinforcing bodies in the solver. On initialization of the solver, all elements of the line bodies scoped to the object which are contained within any solid body in the model will be converted to discrete reinforcement. Elements which lie outside all volume bodies will remain as standard line body elements. The reinforcing beam nodes will be constrained to stay at the same initial parametric location within the volume element they reside during element deformation. Typical applications involve reinforced concrete or reinforced rubber structures likes tires and hoses. If the volume element to which a reinforcing node is tied is eroded, the beam node bonding constraint is removed and becomes a free beam node. On erosion of a reinforcing beam element node, if inertia is retained, the node will remain tied to the parametric location of the volume element. If inertia is not retained, the node will also be eroded Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 497 Features Note Volume elements that are intersected by reinforcement beams, but do not contain a beam node, will not be experiencing any reinforced beam forces. Good modeling practice is therefore to have the element size of the beams similar or less than that of the volume elements. Table 1 Example: Drop test onto reinforced concrete beam Note that the target solid bodies do not need to be scoped to this object – these will be identified automatically by the solver on initialization. Supported Connections Explicit Dynamics Connection Geometry Volume Shell Line Volume No No *Yes Shell No No No Line *Yes No No *Only the line body needs to be included in the scope. The ANSYS AUTODYN solver automatically detects which volume bodies that the line body passes through. Note Reinforcement body interactions are not supported for 2D Explicit Dynamics analyses. Explicit Dynamics (LS-DYNA Export) Connection Geometry Volume Shell Line Volume No No No Shell No No No Line No No No 498 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Analysis Settings The following topics are covered in this section. Analysis Settings for Most Analysis Types Analysis Settings for Explicit Dynamics Analyses Steps and Step Controls for Static and Transient Analyses Solver Controls Restart Analysis Restart Controls Creep Controls Cyclic Controls Radiosity Controls Options for Modal, Harmonic, Linear Buckling, Random Vibration, and Response Spectrum Analyses Damping Controls Nonlinear Controls Output Controls Analysis Data Management Rotordynamics Controls Visibility Analysis Settings for Most Analysis Types When you define an analysis type, an Analysis Settings object is automatically inserted in the Mechanical application tree. With this object selected, you can define various solution options in the Details view that are customized to the specific analysis type, such as enabling large deflection for a stress analysis. The available control groups as well as the control settings within each group vary depending on the analysis type you have chosen. The sections that follow include tables that show the availability of the control settings for each of these control groups. Follow the links in the control group sections for more detailed information on specific controls. Step Controls Solver Controls Restart Analysis Restart Controls Creep Controls Cyclic Controls Radiosity Controls Nonlinear Controls Output Controls Options Damping Controls Visibility Analysis Data Management Analysis Settings Notes Rotordynamics Controls A separate main section includes a table for the Explicit Dynamics settings. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 499 Features Step Controls The following table includes Details view settings in the Step Controls group for the Analysis Settings object. Analysis Type Details View Setting SS TS 9 9 TT 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 2 Initial Time / Substeps 2 2 2 2 Minimum Time / Substeps 2 2 2 2 Maximum Time / Substeps 2 2 2 2 Time Step Number of Substeps Current Step Number Step End Time Auto Time Stepping Define By Time Integration HR M 2 2 LB RV / RS SST Number of Steps RD 2 Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric 500 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. MS E TE Analysis Settings • TE = Thermal Electric Solver Controls The following table includes Details view settings in the Solver Controls group for the Analysis Settings object. Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT MS E TE Solver Type Weak Springs Large Deflection Inertia Relief Time Integration and Constraint Stabilization Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Restart Analysis The following table includes Details view settings in the Restart Analysis group for the Analysis Settings object. Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT MS E TE Restart Type Current Restart Point Load Step Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 501 Features Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT MS E TE Substep Time Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Restart Controls The following table includes Details view settings in the Restart Controls group for the Analysis Settings object. Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT Restart Controls Save at Load Step Save at Substep Save Maximum Files Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum 502 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. MS E TE Analysis Settings • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Creep Controls The following table includes Details view settings in the Creep Controls group for the Analysis Settings object. Analysis Type Details View Setting SS TS 2 2 2 2 Creep Behavior Creep Limit Ratio RD HR M LB RV / RS SST TT MS E TE Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Cyclic Controls The following table includes Details view settings in the Cyclic Controls group for the Analysis Settings object. Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT MS E TE Harmonic Index Range Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 503 Features Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT MS E TE - - - Minimum - - - Maximum - - - Interval Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Radiosity Controls The following table includes Details view settings in the Radiosity Controls group for the Analysis Settings object. Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT Flux Convergence Maximum Iteration Solver Tolerance Over Relaxation Hemicube Resolution Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic 504 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. MS E TE Analysis Settings • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Nonlinear Controls The following table includes Details view settings in the Nonlinear Controls group for the Analysis Settings object. Analysis Type Details View Setting SS TS 2 2 Moment Convergence 2 2 Displacement Convergence 2 2 Rotation Convergence 2 2 Force Convergence Heat Convergence Temperature Convergence RD HR M LB RV / RS SST TT 2 2 2 2 2 2 MS E TE CSG Convergence AMPS Convergence Line Search 2 2 Stabilization Nonlinear Formulation Relative Assembly Tolerance Energy Accuracy Tolerance Voltage Convergence Current Convergence Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 505 Features Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Output Controls The following table includes Details view settings in the Output Controls group for the Analysis Settings object. Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT Stress Strain Nodal Forces Contact Miscellaneous 8 General Miscellaneous Calculate Reactions 7 Store Modal Results Expand Results From 7 7 Calculate Thermal Flux Calculate Velocity 6 Calculate Acceleration 6 Max Number of Result Sets 506 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. MS E TE Analysis Settings Analysis Type Details View Setting SS TS Calculate Results At 2 Value 2 RD HR M LB RV / RS SST TT 2 2 2 2 2 2 MS E TE Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Options The following table includes Details view settings in the Options group for the Analysis Settings object. Analysis Type Details View Setting SS TS RD Various HR M LB RV / RS 1 1 1 1 SST TT MS E TE Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 507 Features • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Damping Controls The following table includes Details view settings in the Damping Controls group for the Analysis Settings object. Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT MS E TE Constant Damping Ratio Beta Damping Defined By Beta Damping Frequency Beta Damping Measure Beta Damping Value Numerical Damping Numerical Damping Value Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Visibility The following table includes Details view settings in the Visibility group for the Analysis Settings object. 508 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT MS E TE (Load) Results Tracker Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Analysis Data Management The following table includes Details view settings in the Analysis Data Management group for the Analysis Settings object. Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT MS E TE 4 5 5 Solver Files Directory Future Analysis Scratch Solver Files Directory Save MAPDL db Delete Unneeded File Nonlinear Solution Solver Units Solver Unit System3 Analysis type abbreviations used in the table: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 509 Features • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Analysis Settings Notes 1 - Refer to the following links for specific control settings in the Options control group: • Modal Analysis • Harmonic Analysis • Linear Buckling Analysis • Random Vibration Analysis • Response Spectrum Analysis 2 - Indicates control setting is ”step aware” meaning that the setting can be different for each step. 3 - Read-only display if Solver Units is set to Active System. 4 - Read-only display of mks, regardless of whether Solver Units is set to Active System or Manual. A Magnetostatic analysis can only be solved in the mks unit system. 5 - mks and µmks are the only unit system choices available when solving an Electric or Thermal Electric analysis. 6 - Available for response spectrum analyses only. 7 - Applicable only when linked to a Modal analysis. 8 - Not Available when linked to a Modal analysis. 9- Number of steps is restricted to 1 if Fluid Solid Interface load exists in the analysis. Rotordynamics Controls The following table includes Details view settings in the Rotordynamics Controls group for the Analysis Settings object. 510 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Analysis Type Details View Setting SS TS RD HR M LB RV / RS SST TT MS E TE Coriolis Effect Reference Frame Rotating Damping Effect Campbell Diagram Number of Points Analysis type abbreviations used in the table: • SS = Static Structural • TS = Transient Structural • RD = Rigid Dynamics • HR = Harmonic • M = Modal • LB = Linear Buckling • RV / RS = Random Vibration / Response Spectrum • SST = Steady - State Thermal • TT = Transient Thermal • MS = Magnetostatic • E = Electric • TE = Thermal Electric Analysis Settings for Explicit Dynamics Analyses The following sections describe the various analysis settings available for an Explicit Dynamics analysis. In addition to describing each setting, it is noted whether the setting is available for 2D analyses, and whether it is available on restart (applies to 2D and 3D analyses). Explicit Dynamics Step Controls Explicit Dynamics Solver Controls Explicit Dynamics Euler Domain Controls Explicit Dynamics Damping Controls Explicit Dynamics Erosion Controls Explicit Dynamics Output Controls Explicit Dynamics Data Management Settings Explicit Dynamics Analysis Settings Notes Explicit Dynamics Step Controls Field Resume From Cycle Options Description 2D Restart Allows you to select the cycle (time increment for explicit integration) from Yes Yes Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 511 Features Field Options Description 2D Restart which to start the solution upon selecting Solve. A cycle of zero (default) indicates the solution will clear any previous progress and start from time zero. A non-zero cycle, on the other hand, allows you to revisit a previous solution and extend it further in time. A solution obtained from a non-zero cycle is considered to have been "resumed" or "restarted". Note that the list will only contain nonzero selections if a solve was previously executed and restart files have been generated. When resuming an analysis, changes to analysis settings will be respected where possible. For example, you may wish to resume an analysis with an extended termination time. Changes to any other features in the model (geometry suppression, connections, loads, and so on) will prevent restarts from taking place. See Resume Capability for Explicit Dynamics Analyses (p. 855) for more information. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Maximum Number of Cycles The maximum number of cycles allowed during the analysis.The analysis will stop once the specified value is reached. Enter a large number to have the analysis run to the defined End Time. Yes Yes End Time (Required input) The maximum length of time (starting from zero seconds) to be simulated by the explicit analysis.You should enter a reasonable estimate to cover the phenomena of interest. Yes Yes Maximum Energy Error Energy conservation is a measure of the quality of an explicit dynamics analysis. Large deviations from energy conservation usually imply a less than optimal model definition. This parameter allows you to automatically stop the solution if the deviation from energy conservation becomes unacceptable. Enter a fraction of the total system energy (measured Yes Yes 512 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Field Options Description 2D Restart Yes Yes Yes Yes Yes Yes at the Reference Energy Cycle) for which you want the analysis to stop. For example, the default value of 0.1 will cause the analysis to stop if the energy error exceeds 10% of the energy at the reference cycle. For Explicit Dynamics (LS-DYNA Export) systems this field requires a percentage to be entered. Thus the field name changes to Maximum Energy Error (%). Reference Energy Cycle The cycle at which you want the solver to calculate the reference energy, against which it will calculate the energy error. Usually this will be the start cycle (cycle = 0).You may need to increase this value if the model has zero energy at cycle = 0 (for example if you have no initial velocity defined). This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Initial Time Step Enter an initial time step you want to use, or use the Program Controlled default. If left on Program Controlled, the time step will be automatically set to ½ the computed element stability time step.The Program Controlled setting is recommended. For Explicit Dynamics (LS-DYNA Export) systems if this field is left on Program Controlled, the initial time step will be determined by the solver. Minimum Time Step Enter the minimum time step allowed in the analysis, or use the Program Controlled default. If the time drops below this value the analysis will stop. If set to Program Controlled, the value will be chosen as 1/10th the initial time step. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Maximum Time Step Enter the maximum time step allowed in the analysis, or use the Program Controlled default.The solver will use the minimum of this value or the computed stability time step during the solve.The Program Controlled setting is recommended. Yes Yes Time Step Safety Factor It is not wise to run at the stability limit, so a safety factor is applied to the computed stabil- Yes Yes Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 513 Features Field Options Description 2D Restart Yes No ity time step.The default value of 0.9 should work for most analyses. Characteristic Dimension Diagonals (default) The characteristic dimension used to determine the time-step for hex elements will be calculated as the volume of the element divided by the square of the longest element diagonal and then scaled by sqrt(2/3). This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Opposing Face The characteristic dimension used to determine the time-step for hex elements will be based on the minimum distance between opposing faces. Select this option to obtain the optimal time step for hex solid elements. Experience to date has shown that this option can significantly improve the efficiency of 3D Lagrange simulations. However, in certain circumstances when cells become highly distorted, instabilities have been observed causing the calculation to terminate with high energy errors. The correct choice of erosion strain can reduce these problems. It is therefore recommended that users only utilize this option if efficiency is critical. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Nearest Face The characteristic dimension used to determine the time-step for hex elements will be based on the minimum distance between neighboring faces. Experience to date has shown that this option can significantly improve the efficiency of 3D Lagrange simulations. However, in certain circumstances when cells become highly distorted, instabilities have been observed causing the calculation to terminate with high energy errors. The correct choice of erosion strain can reduce these problems. It is therefore recommended that 514 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Field Options Description 2D Restart If set to Yes, activates automatic mass scaling and exposes the following options. Yes Yes The CFL time step that you want to achieve in the analysis. Yes Yes Yes Yes Yes Yes Yes Yes users only utilize this option if efficiency is critical. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Automatic Mass Scaling Minimum CFL Time Step Caution Mass scaling introduces additional mass into the system to increase the CFL time step. Introducing too much mass can lead to non-physical results. Note Employ User Defined Results (p. 702) MASS_SCALE (ratio of scaled mass/physical mass) and TIMESTEP to review the effects of automatic mass scaling on the model. Maximum Element Scaling This value limits the ratio of scaled mass/physical mass that can be applied to each element in the model. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Maximum Part Scaling This value provides a check on the total ratio of scaled mass/physical mass that can be applied to an individual body. If this value is exceeded, the analysis will stop and an error message is displayed. For Explicit Dynamics (LS-DYNA Export) systems this field requires a percentage to be entered. Thus the field name changes to Maximum Part Scaling (%). Update Frequency Allows you to control the frequency at which the mass scaling will be calculated during the solve.The frequency equates to the increment Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 515 Features Field Options Description 2D Restart in cycles at which the mass scale factor will be recomputed, based on the current shape of the elements.The default of 0 is recommended and means that the mass scale factor is only calculated once, at the start of the solve. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Explicit Dynamics Solver Controls Field Options Description 2D Restart Precision Single Solves the model using the Single Precision solver. Real values are stored with 32-bit floating point precision.This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Yes No Double (Default) Solves the model using the Double Precision solver to give more accurate results. Real values are stored with 64-bit floating point precision, and will therefore increase memory usage and the size of restart files.The double precision option is recommended when breakable bonded connections are used or an implicit pre-stress condition is used as an initial condition.This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Yes No No No Solve Units All model inputs will be converted to this set of units during the solve. Results from the analysis will be converted back to the user units system in the GUI. For Explicit Dynamics systems, this setting is always mm, mg, ms. For Explicit Dynamics (LS-DYNA Export) systems this field is termed Unit System and four systems are available for selection: m, kg, s, mm, ton, s, mm, mg, ms, in, lbf, s. Beam Solution Type 516 Bending Any line bodies will be represented as beam elements including a full bending moment calculation. Truss Any line bodies will be represented as truss elements. No bending moments are calculated. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Field Options Description 2D Restart An additional safety factor you may apply to the stability time step calculated for beam elements.The default value ensures stability for most cases. No No Exact Provides an accurate calculation of element volume, even for warped elements. No No 1pt Gauss Approximates the volume calculation and is less accurate for elements featuring warped faces.This option is more efficient. Beam Time Step Safety Factor Hex Integration Type Shell Sublayers The number of integration points through the thickness of an isotropic shell.The default of 3 is suitable for many applications however this number can be increased to achieve better resolution of through thickness plastic deformation and/or flow. No No Shell Shear Correction Factor The transverse shear in the element formulation is assumed constant over the thickness. This correction factor accounts for the replacement of the true parabolic variation through the thickness in response to a uniform transverse shear stress. Using a value other than the default is not recommended. No No Shell BWC Warp Correction The Belytschko-Lin-TSy element formulation becomes inaccurate if the elements are warped.To overcome this, the element formulation has an optional correction to include warping. Setting this correction to Yes is recommended. No No Changes in shell thickness are calculated at the nodes of shell elements. No No N/A N/A No No Shell Thickness Update Nodal This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Elemental Changes in shell thickness are calculated at the element integration points. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Available only for Explicit Dynamics (LS-DYNA Export) systems. Full Shell Integration Provides a very fast and accurate shell element formulation. Tet Integration Average Nodal Pressure The tetrahedral element formulation includes an average nodal pressure integration.This formulation does not exhibit volumetric locking, and can be used for large deformation, Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 517 Features Field Options Description 2D Restart No No Yes No and nearly incompressible behavior such as plastic flow or hyperelasticity.This formulation is recommended for the majority of tetrahedral meshes. Constant Pressure Uses the constant pressure integrated tetrahedral formulation.This formulation is more efficient than Average Nodal, however it suffers from volumetric locking under constant bulk deformation. Nodal Strain When Tet Integration is set to Nodal Strain the Puso Stability Coefficient, field is shown. For NBS models exhibiting zero energy modes, the Puso coefficient can be set to a non-zero value. A value of 0.1 is recommended. See Solver Controls (p. 1276) for more information. Shell Inertia Update Recompute The principal axes of rotary inertia are by default recalculated each cycle. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Rotate Rotates the axes, rather than recomputing each cycle.This option is more efficient, however it can lead to numerical instabilities due to floating point round-off for long running simulations. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Density Update Program Controlled The solver decides whether an incremental update is necessary based on the rate and extent of element deformation. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Incremental Forces the solver to always use the incremental update. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Total Forces the solver to always recalculate the density from element-volume and mass. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. 518 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Field Options Minimum Velocity Description 2D Restart The minimum velocity you want to allow in the analysis. If any model velocity drops below this Minimum Velocity, it will be set to zero. The default is recommended for most analyses. Yes Yes Yes Yes Yes Yes This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Maximum Velocity The maximum velocity you want to allow in the analysis. If any model velocity rises above the Maximum Velocity, it will be capped.This can improve the stability/robustness of the analysis in some instances.The default is recommended for most analyses. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Radius Cutoff At the start of your calculation, if a node is within the specified radius of a symmetry plane, it will be placed on the symmetry plane. If a node is outside the specified radius from a symmetry plane at the start of your calculation, it will not be allowed to come closer than this radius to the symmetry plane as your calculation proceeds. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Explicit Dynamics Euler Domain Controls Field Options Description 2D Restart Domain Size Definition Program Controlled Set Domain Size Definition to automatic No No Manual Set Domain Size Definition to manual Toggles visibility of the annotation of the Euler domain in the graphics window No No All Bodies Euler domain is sized to include all bodies No No Eulerian Bodies Only Euler domain is sized to include Euler bodies only Display Euler Domain Scope X Scale factor, Y Scale factor, Z Scale Factor User defined scaling factors for the automatically determined X,Y, and Z sizes No No Minimum X Coordinate, Minimum Y Coordinate, X,Y, Z coordinates for the Euler domain origin for the Manual option No No Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 519 Features Field Options Description 2D Restart Euler domain X,Y, Z dimensions for the Manual option No No Total Cells Set Domain Resolution Definition by specifying the total number of cells in the Euler domain No No Cell Size Set Domain Resolution Definition by specifying the size of the cells in the Euler domain Cells per Component Set Domain Resolution Definition by specifying the number of cells in each dimension in the Euler domain Minimum Z Coordinate X Dimension,Y Dimension,Z Dimension Domain Resolution Definition Total Cells Total number of cells that the Euler domain should contain if Domain Resolution Definition is Total Number of Cells No No Cell Size Dimension of the cell in each of the X,Y, and Z directions if Domain Resolution Definition is Cell Size No No Number of Cells in X,Number of Cells in Y, Number of Cells in Z Number of cells required in the X,Y, and Z directions if Domain Resolution Definition is Number of Cells by Component No No Flow Out (default) Specify the boundary condition of the selected Euler domain face to be Flow Out No No No No Description 2D Restart Linear Artificial Viscosity A linear coefficient of artificial viscosity.This coefficient smooths out shock discontinuities over the mesh. Using a value other than the default is not recommended. Yes Yes Quadratic Artificial Viscosity A quadratic coefficient of artificial viscosity. This coefficient damps out post shock discontinuity oscillations. Using a value other than the default is not recommended. Yes Yes Linear Viscosity in Expansion Artificial viscosity is normally applied to materials in compression only.This option allows Yes Yes Lower X Face, Lower Y Face, Lower Z Face, Upper X Face, Upper Y Face, Upper Z Face Impedance Specify the boundary condition of the selected Euler domain face to be Impedance Rigid Specify the boundary condition of the selected Euler domain face to be Rigid Euler Tracking By Body Results may be scoped to Eulerian bodies in the same way as for Lagrangian bodies Explicit Dynamics Damping Controls Field 520 Options Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Field Options Description 2D Restart The method of hourglass damping to be used with solid hexahedral elements. No Yes Stiffness Coefficient The stiffness coefficient for Flanagan Belytschko hourglass damping in solid hexahedral elements. No Yes Viscous Coefficient The viscous coefficient for hourglass damping used in hexahedral solid elements and quadrilateral shell elements. No Yes Static Damping A static damping constant may be specified which changes the solution from a dynamic solution to a relaxation iteration converging to a state of stress equilibrium. For optimal convergence, the value chosen for the damping constant, R, may be defined by: R = 2*timestep/T where timestep is the expected average value of the timestep and T is longest period of vibration for the system being analyzed. Yes Yes Description 2D Restart If set to Yes, elements will automatically erode if the geometric strain in the element exceeds the specified limit. Yes Yes Yes Yes Yes Yes you to apply the viscosity for materials in compression and expansion. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Hourglass Damping AUTODYN Standard Flanagan Belytschko Explicit Dynamics Erosion Controls Field On Geometric Strain Limit Options This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Geometric Strain Limit The geometric strain limit for erosion. Recommended values are in the range from 0.75 to 3.0.The default value is 1.5. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. On Material Failure If set to Yes, elements will automatically erode if a material failure property is defined in the material used in the elements, and the failure criteria has been reached. Elements with ma- Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 521 Features Field Options Description 2D Restart terials including a damage model will also erode if damage reaches a value of 1.0. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. On Minimum Element Time Step If set to Yes, elements will automatically erode if their calculated time step falls below the specified value. Yes Yes Minimum Element Time Step The minimum controlling time step that an element can have. If the element time step drops below the specified value, the element will be eroded. Yes Yes Yes No Description 2D Restart During the solve of an explicit dynamics system, results are saved to disk at a frequency defined through this control.The following settings are available. Yes Yes Save results files after a specified increment in the number of cycles. Exposes a Cycles field where you enter the increment in cycles. Yes Yes This field is not displayed for Explicit Dynamics (LS-DYNA Export) systems when On Minimum Element Time Step is set to No. Retain Inertia of Eroded Material If all elements that are connected to a node in the mesh erode, the inertia of the resulting free node can be retained if this option is set to Yes. The mass and momentum of the free node is retained and can be involved in subsequent impact events to transfer momentum in the system. If set to No, all free nodes will be automatically removed from the analysis. This field is not displayed for Explicit Dynamics (LS-DYNA Export) systems when On Minimum Element Time Step is set to No. Explicit Dynamics Output Controls Field Options Save Results on Cycles This setting is not available for Explicit Dynamics (LS-DYNA Export) systems. 522 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Field Options Description 2D Restart Time Save results file after a specified increment in time. Exposes a Time field where you enter a time increment. Yes Yes Equally Spaced Points (Default) Save a specified number of result files during the analysis.The frequency is defined by the termination time / number of points. Exposes a Number of Points field where you enter the number of results files required. Yes Yes During the solve of an explicit dynamics system, restart files are saved to disk at a frequency defined through this control.The following settings are available. Yes Yes Cycles Save restart files after a specified increment in the number of cycles. Exposes a Cycles field where you enter the increment in cycles. Yes Yes Time Save restart files after a specified increments in time. Exposes a Time field where you enter a time increment. Yes Yes (Default) Save a specified number of restart files during the analysis.The frequency is defined by the termination time / number of points. Exposes a Number of Points field where you enter the number of restart files required. Yes Yes Use this control to define the frequency at which result tracker data and solution output is saved to disk. Yes Yes Yes Yes Save Restart Files on This setting is not available for Explicit Dynamics (LS-DYNA Export) systems. Equally Spaced Points Save Result Tracker Data on Result tracker data objects are scoped to specific regions in a model. Solution output provides a summary of the state of the solution as the solve proceeds. This is shown when Solution Information is highlighted in the project tree. This setting applies to all the selectable views in the Solution Output drop down list located in the Solution Information Details view. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. Cycles (Default) Save results tracker and solution output data after a specified increment in the number of cycles. Exposes a Cycles field where Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 523 Features Field Options Description 2D Restart Yes Yes you enter the increment in cycles.The default value is 1.The value entered here will be divided by 10 to calculate the actual frequency that the Solver Output view in the Solution Output category will be updated. The following solution output plots will be updated at the entered frequency: • Time Increment • Energy Conservation • Momentum Summary • Energy Summary Cycle zero and the final cycle will always be displayed even if it is not a multiple of the frequency entered. Time Save result tracker and solution output data after a specified increment in time. Exposes a Time field where you enter a time increment. This setting will cause the Solver Output view in the Solution Output category to be updated every cycle. The following solution output plots will be updated at the entered frequency: • Time Increment • Energy Conservation • Momentum Summary • Energy Summary Explicit Dynamics Data Management Settings Note that these settings cannot be changed from the Details panel. Field Description Solver Files Directory The permanent location for all the files generated during a solve.This is a read-only field provided for information. Scratch Solver Files Directory A temporary location for all files generated during a solve.These files are then moved to the Solver Files Directory for completed solves. This is a read-only field provided for information. See Analysis Data Management for more information. This field is not available for Explicit Dynamics (LS-DYNA Export) systems. 524 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Explicit Dynamics Analysis Settings Notes If any bodies are defined as Eulerian (Virtual), when Analysis Settings is selected in the outline view the Euler domain bounding box is displayed in the graphics window, as shown below. The Euler domain resolution is indicated by black node markers along each edge line of the Euler domain. The visibility of this can be controlled by the Display Euler Domain option in the Analysis Settings. Steps and Step Controls for Static and Transient Analyses The following topics are covered in this section: Role of Time in Tracking Steps, Substeps, and Equilibrium Iterations Automatic Time Stepping Guidelines for Integration Step Size Step Controls Role of Time in Tracking Time is used as a tracking parameter in all static and transient analyses, whether or not the analysis is truly time-dependent. The advantage of this is that you can use one consistent "counter" or "tracker" in all cases, eliminating the need for analysis-dependent terminology. Moreover, time always increases monotonically, and most things in nature happen over a period of time, however brief the period may be. Obviously, in a transient analysis time represents actual, chronological time in seconds, minutes, or hours. In a static analysis, however, time simply becomes a counter that identifies steps and substeps. By default, the program automatically assigns time = 1.0 at the end of step 1, time = 2.0 at the end of step 2, and so on. Any substeps within a step will be assigned the appropriate, linearly interpolated time value. By assigning your own time values in such analyses, you can establish your own tracking parameter. For example, if a load of 100 units is to be applied incrementally over one step, you can specify time at the end of that step to be 100, so that the load and time values are synchronous. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 525 Features Steps, Substeps, and Equilibrium Iterations What is a step? A step corresponds to a set of loads for which you want to obtain a solution and review results. In this way every static or transient dynamic analysis has at least one step. However there are several scenarios where you may want to consider using multiple steps within a single analysis, that is, multiple solutions and result sets within a single analysis. A static or transient analysis starts at time = 0 and proceeds until a step end time that you specify. This time span can be further subdivided into multiple steps where each step spans a different time range. As mentioned in the Role of Time in Tracking (p. 525) section, each step spans a ‘time’ even in a static analysis. When do you need Steps? Steps are required if you want to change the analysis settings for a specific time period. For example in an impact analysis you may want to manually change the allowable minimum and maximum time step sizes during impact. In this case you can introduce a step that spans a time period shortly before and shortly after impact and change the analysis settings for that step. Steps are also useful generally to delineate different portions of an analysis. For example, in a linear static structural analysis you can apply a wind load in the first step, a gravity load in the second step, both loads and a different support condition in the third step, and so on. As another example, a transient analysis of an engine might include load conditions corresponding to gravity, idle speed, maximum power, back to idle speed. The analysis may require repetition of these conditions over various time spans. It is convenient to track these conditions as separate steps within the time history. In addition steps are also required for deleting loads or adding new loads such as specified displacements or to set up a pretension bolt load sequence. Steps are also useful in setting up initial conditions for a transient analysis. How do you define steps? See the procedure, ”Specifying Analysis Settings for Multiple Steps” located in the Establish Analysis Settings (p. 9) section. What are substeps and equilibrium iterations? Solving an analysis with nonlinearities requires convergence of an iterative solution procedure. Convergence of this solution procedure requires the load to be applied gradually with solutions carried out at intermediate load values. These intermediate solution points within a step are referred to as substeps. Essentially a substep is an increment of load within a step at which a solution is carried out. The iterations carried out at each substep to arrive at a converged solution are referred to as equilibrium iterations. 526 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Load Substep Load step Final load value 1 2 Equilibrium iterations Substeps Automatic Time Stepping Auto time stepping, also known as time step optimization, aims to reduce the solution time especially for nonlinear and/or transient dynamic problems by adjusting the amount of load increment. If nonlinearities are present, automatic time stepping gives the added advantage of incrementing the loads appropriately and retreating to the previous converged solution (bisection) if convergence is not obtained. The amount of load increment is based on several criteria including the response frequency of the structure and the degree of nonlinearities in the analysis. The load increment within a step is controlled by the auto time stepping procedure within limits set by you. You have the option to specify the maximum, minimum and initial load increments. The solution will start with the “initial” increment but then the automatic procedure can vary further increments within the range prescribed by the minimum and maximum values. You can specify these limits on load increment by specifying the initial, minimum, and maximum number of substeps that are allowed. Alternatively, since a step always has a time span (start time and end time), you can also equivalently specify the initial, minimum and maximum time step sizes. Although it seems like a good idea to activate automatic time stepping for all analyses, there are some cases where it may not be beneficial (and may even be harmful): • Problems that have only localized dynamic behavior (for example, turbine blade and hub assemblies), where the low-frequency energy content of part of the system may dominate the high-frequency areas. • Problems that are constantly excited (for example, seismic loading), where the time step tends to change continually as different frequencies are excited. • Kinematics (rigid-body motion) problems, where the rigid-body contribution to the response frequency term may dominate. Guidelines for Integration Step Size The accuracy of the transient dynamic solution depends on the integration time step: the smaller the time step, the higher the accuracy. A time step that is too large introduces an error that affects the response of the higher modes (and hence the overall response). On the other hand too small a time step size wastes computer resources. An optimum time step size can depend on several factors: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 527 Features 1. Response frequency: The time step should be small enough to resolve the motion (response) of the structure. Since the dynamic response of a structure can be thought of as a combination of modes, the time step should be able to resolve the highest mode that contributes to the response. The solver calculates an aggregate response frequency at every time point. A general rule of thumb it to use approximately twenty points per cycle at the response frequency. That is, if f is the frequency (in cycles/time), the integration time step (ITS) is given by: ITS = 1/(20f ) Smaller ITS values will be required if accurate velocity or acceleration results are needed. The following figure shows the effect of ITS on the period elongation of a single-DOF spring-mass system. Notice that 20 or more points per cycle result in a period elongation of less than 1 percent. Period Elongation (%) 2. 528 10 9 8 7 6 5 4 3 2 1 0 recommended 0 10 20 30 40 50 60 70 80 90 100 Number of Time Steps Per Cycle Resolve the applied load-versus-time curve(s). The time step should be small enough to “follow” the loading function. For example, stepped loads require a small ITS at the time of the step change so that the step change can be closely followed. ITS values as small as 1/180f may be needed to follow stepped loads. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings ü ü Inpu Response t 3. t Resolve the contact frequency. In problems involving contact (impact), the time step should be small enough to capture the momentum transfer between the two contacting faces. Otherwise, an apparent energy loss will occur and the impact will not be perfectly elastic. The integration time step can be determined from the contact frequency (fc) as: c c = π where k is the gap stiffness, m is the effective mass acting at the gap, and N is the number of points per cycle. To minimize the energy loss, at least thirty points per cycle of (N = 30) are needed. Larger values of N may be required if velocity or acceleration results are needed. See the description of the Predict for Impact option within the Time Step Controls contact Advanced settings for more information. You can use fewer than thirty points per cycle during impact if the contact period and contact mass are much less than the overall transient time and system mass, because the effect of any energy loss on the total response would be small. 4. Resolve the nonlinearities. For most nonlinear problems, a time step that satisfies the preceding guidelines is sufficient to resolve the nonlinearities. There are a few exceptions, however: if the structure tends to stiffen under the loading (for example, large deflection problems that change from bending to membrane load-carrying behavior), the higher frequency modes that are excited will have to be resolved. After calculating the time step sizes using the above guidelines, you need to use the minimum value for your analysis. However using this minimum time step size throughout a transient analysis can be very inefficient. For example in an impact problem you may need small time step sizes calculated as above only during and for a short duration after the impact. At other parts of the time history you may be able to get accurate results with larger time steps sizes. Use of the Automatic Time Stepping (p. 527) procedure lets the solver decide when to increase or decrease the time step during the solution. Step Controls Step Controls play an important role in static and transient dynamic analyses. Step controls are used to perform two distinct functions: 1) Defining Steps, and 2) Specifying analysis settings for each step. Defining Steps See the procedure, ”Specifying Analysis Settings for Multiple Steps” located in the Establish Analysis Settings (p. 9) section. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 529 Features Specifying Analysis Settings for Each Step The following items can be changed on a per step basis: Step Controls, Nonlinear Controls, and Output Controls. Nonlinear Controls and Output Controls are discussed in their own sections. Details of Step Controls: Current Step Number shows the step ID for which the settings in Step Controls, Nonlinear Controls, and Output Controls are applicable. The currently selected step is also highlighted in the bar at the bottom of the Graph window. You can select multiple steps by selecting rows in the data grid or the bars at the bottom of the Graph window. In this case the Current Step Number will be set to multistep. In this case any settings modified will affect all selected steps. Step End Time shows the end time of the current step number. When multiple steps are selected this will indicate multi-step. Auto Time Stepping is discussed in detail in the Automatic Time Stepping (p. 527) section. Automatic time stepping is available for static and transient analyses, and is especially useful for nonlinear solutions. Settings for controlling automatic time stepping are included in a drop down menu under Auto Time Stepping in the Details view. The following options are available: • Program Controlled (default): The Mechanical application automatically switches time stepping on and off as needed. A check is performed on nonconvergent patterns. The physics of the simulation is also taken into account. The Program Controlled settings are presented in the following table: Auto Time Stepping Program Controlled Settings Analysis Type Initial Substeps Minimum Substeps Maximum Substeps Linear Static Structural 1 1 1 Nonlinear Static Structural 1 1 10 Linear Steady-State Thermal 1 1 10 Nonlinear Steady-State Thermal 1 1 10 100 10 1000 Transient Thermal 530 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings • • On: You control time stepping by completing the following fields that only appear if you choose this option. No checks are performed on nonconvergent patterns and the physics of the simulation is not taken into account. – Initial Substeps: Specifies the size of the first substep. The default is 1. – Minimum Substeps: Specifies the minimum number of substeps to be taken (that is, the maximum time step size). The default is 1. – Maximum Substeps: Specifies the maximum number of substeps to be taken (that is, the minimum time step size). The default is 10. Off: No time stepping is enabled. You are prompted to enter the Number Of Substeps. The default is 1. Define By allows you to set the limits on load increment in one of two ways. You can specify the Initial, Minimum and Maximum number of substeps for a step or equivalently specify the Initial, Minimum and Maximum time step size. Carry Over Time Step is an option available when you have multiple steps. This is useful when you do not want any abrupt changes in the load increments between steps. When this is set the Initial time step size of a step will be equal to the last time step size of the previous step. Time Integration is valid only for a Transient Structural or Transient Thermal analysis. This field indicates whether a step should include transient effects (for example, structural inertia, thermal capacitance) or whether it is a static (steady-state) step. This field can be used to set up the Initial Conditions for a transient analysis. • On: Default for transient analyses. • Off: Do not include structural inertia or thermal capacitance in solving this step. Note With Time Integration set to Off in Transient Structural analyses, Workbench does not compute velocity results. Therefore spring damping forces, which are derived from velocity will equal zero. This is not the case for Rigid Dynamics analyses. Activation/Deactivation of Loads You can activate (include) or deactivate (delete) a load from being used in the analysis within the time span of a step. For most loads (for example, pressure or force) deleting the load is the same as setting the load value to zero. But for certain loads such as specified displacement this is not the case. Note Changing the method of how a multiple-step load value is specified (such as Tabular to Constant), the Activation/Deactivation state of all steps resets to the default, Active. To activate or deactivate a load in a stepped analysis: 1. Highlight the load within a step in the Graph or a specific step in the Tabular Data window. 2. Click the right mouse button and choose Activate/Deactivate at this step!. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 531 Features Note For displacements and remote displacements, it is possible to deactivate only one degree of freedom within a step. For Temperature, Thermal Condition, Heat Generation, Voltage, and Current loads, the following rules apply when multiple load objects of the same type exist on common geometry selections: • A load can assume any one of the following states during each load step: – Active: Load is active during the first step. – Reactivated: Load is active during the current step, but was deactivated during the previous step. A change in step status exists. – Deactivated: Load is deactivated at the current step, but was active during the previous step. A change in step status exists. – Unchanged: No change in step status exists. • During the first step, an active load will overwrite other active loads that exist higher (previously added) in the tree. • During any other subsequent step, commands are sent to the solver only if a change in step status exists for a load. Hence, any unchanged loads will get overwritten by other reactivated or deactivated loads irrespective of their location in the tree. A reactivated/deactivated load will overwrite other reactivated and deactivated loads that exist higher (previously added) in the tree. Note For each load step, if both Imported Loads and user-specified loads are applied on common geometry selections, the Imported Loads take precedence. For Imported loads commands are sent to the solver at a load step if the Imported Load: • Is active and has data specified for the current step • Has been reactivated and has data for the current step or at a previous step • Has been deactivated and data was applied at the previous step. Some scenarios where load deactivation is useful are: • Springback of a cantilever beam after a plasticity analysis (see example below). • Bolt pretension sequence (Deactivation is possible by setting Define By to Open for the load step of interest). • Specifying different initial velocities for different parts in a transient analysis. Example: Springback of a cantilever beam after a plasticity analysis In this case a Y displacement of -2.00 inch is applied in the first Step. In the second step this load is deactivated (deleted). Deactivated portions of a load are shown in gray in the Graph and also have a red stop bars indicating the deactivation. The corresponding cells in the data grid are also shown in gray. 532 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings In this example the second step has a displacement value of -1.5. However since the load is deactivated this will not have any effect until the third step. In the third step a displacement of -1.5 will be step applied from the sprung-back location. Solver Controls Damped - Modal Analyses Only Set this control to Yes to enable a damped modal system where the natural frequencies and mode shapes become complex. Solver Type If you want to specify a Solver type for the Mechanical application to use, select the Solver Type field. You can choose between Program Controlled, Direct, or Iterative solvers, or, for modal analyses, the additional choices are Unsymmetric, Supernode, Full Damped, or Reduced Damped. A direct solver works better with thin flexible models. An iterative solver works better for bulky models. In most cases, the program controlled option does select the optimal solver. Note Note that for modal analyses, if Damped is Yes, the available solver types are Program Controlled, Full Damped, and Reduced Damped. If Damped is No, the available solver types are Program Controlled, Direct, Iterative, Unsymmetric, and Supernode. Store Complex Solution - Modal Analyses Only This control is only available when a damped Solver Type of Reduced Damped is selected. It allows you to solve and store a damped modal system as an undamped modal system. Weak Springs For stress or shape simulations, the addition of weak springs can facilitate a solution by preventing numerical instability, while not having an effect on real world engineering loads. The following Weak Springs settings are available in the Details view: • Program Controlled (default): Workbench determines if weak springs will facilitate the solution, then adds a standard weak springs stiffness value accordingly. • On: Workbench always adds a weak spring stiffness. Choosing On causes a Spring Stiffness option to appear that allows you to control the amount of weak spring stiffness. Your choices are to use the standard stiffness mentioned above for the Program Controlled setting of Weak Springs or to enter a customized value. The following situations may prompt you to choose a customized stiffness value: a. The standard weak spring stiffness value may produce springs that are too weak such that the solution does not occur, or that too much rigid body motion occurs. b. You may judge that the standard weak spring stiffness value is too high (rare case). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 533 Features c. You many want to vary the weak spring stiffness value to determine the impact on the simulation. The following Spring Stiffness settings are available: • – Program Controlled (default): Adds a standard weak spring stiffness (same as the value added for the Program Controlled setting of Weak Springs). – Factor: Adds a customized weak spring stiffness whose value equals the Program Controlled standard value times the value you enter in the Spring Stiffness Factor field (appears only if you choose Factor). For example, setting Spring Stiffness Factor equal to 20 means that the weak springs will be 20 times stronger than the Program Controlled standard value. – Manual: Adds a customized weak spring stiffness whose value you enter (in units of force/length) in the Spring Stiffness Value field (appears only if you choose Manual). Off: Weak springs are not added. Use this setting if you are confident that weak springs are not necessary for a solution. Large Deflection This field, applicable to static structural and Transient Structural analyses, determines whether the solver should take into account large deformation effects such as large deflection, large rotation, and large strain. Set Large Deflection to On if you expect large deflections (as in the case of a long, slender bar under bending) or large strains (as in a metal-forming problem). When using hyperelastic material models, you must set Large Deflection On. Inertia Relief - Linear Static Structural Analyses Only Calculates accelerations to counterbalance the applied loads. Displacement constraints on the structure should only be those necessary to prevent rigid-body motions (6 for a 3-D structure). The sum of the reaction forces at the constraint points will be zero. Accelerations are calculated from the element mass matrices and the applied forces. Data needed to calculate the mass (such as density) must be input. Both translational and rotational accelerations may be calculated. This option applies only to the linear static structural analyses. Displacements and stresses are calculated as usual. Time Integration Type - Transient Analysis of Multiple Rigid Bodies Only This feature is applicable to a Rigid Dynamics analysis. The Time Integration Type feature employs the fourth and fifth order polynomial approximation of the Runge-Kutta algorithm to enable the Mechanical application to integrate the equations of motion during analyses. This feature allows you to choose time integration algorithms and specify whether to use constraint stabilization. The fifth order approximation usually allows for larger time steps and can therefore reduce the total simulation time. The Details view Solver Controls options for the Time Integration Type include: • • 534 Time Integration Type field. Available time integration algorithms include: – Runge-Kutta 4 (Default) - Fourth Order Runge-Kutta – Runge-Kutta 5 - Fifth Order Runge-Kutta Use Stabilization field. When specified, this option provides the numerical equivalent for spring and damping effects and is proportional to the constraint violation and its time derivative. If there is no Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings constraint violation, the spring and damping has no effect. The addition of artificial spring and damping does not change the dynamic properties of the model. Stabilization options include: – Off (Default) - constraint stabilization is ignored. – On - Because constraint stabilization has a minimal impact on calculation time, its use is recommended. When specified, the Stabilization Parameters field also displays. Stabilization Parameters options include: – Program Controlled - valid for most applications. – User Defined - manual entry of spring stiffness (Alpha) and damping ratio (Beta) required. Note Based on your application, it may be necessary to enter customized settings for Alpha and Beta. In this case, start with small values and use the same value in both fields. Alpha and Beta values that are too small have little effect and values that are too large cause the time step to be too small. The valid values for Alpha and Beta are Alpha >=0 and Beta >=0. If Both Alpha and Beta are zero, the stabilization will have no effect. Restart Analysis Note This group is displayed in the Details view only if restart points are available. Restart points can be generated by adjusting the settings in the Restart Controls group. You will also need to set Delete Unneeded Files, under the Analysis Data Management group to No so that restart point files are retained after a solve. These control whether to use restart points in subsequent solution restarts. If restart points should be used, Load Step, Substep and Time help reveal the point's identity in the calculation sequence. The Restart Analysis controls are as follows: • Restart Type: By default, Mechanical tracks the state of restart points and selects the most appropriate point when set to Program Controlled. You may choose different restart points by setting this to Manual, however. To disable solution restarts altogether, set it to Off. • Current Restart Point: This option lets you choose which restart point to use. This option is displayed only if Restart Type set to Manual. • Load Step: Displays the Load Step of the restart point to use. If no restart points are available (or all are invalid for a Restart Type of Program Controlled) the display is Initial. • Substep: Displays the Substep of the restart point to use. If no restart points are available (or all are invalid for a Restart Type of Program Controlled) the display is Initial. • Time: Displays the time of the restart point to use. Restart Controls These control the creation of Restart Points. Because each Restart Point consists of special files written by the solver, restart controls can help you manage the compromise between flexibility in conducting Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 535 Features your analyses and disk space usage. Please see the Solution Restarts section for more information about the restart capability and how it relates to Restart Points. The Restart Controls are as follows: • Generate Restart Controls: Enables the creation of restart points. – Program Controlled: Instructs the program to select restart point generation settings for you The setting is equivalent to Load Step = Last and Substep = Last. – Manual: Allows you access to the detailed settings for restart point generation. – Off: Restricts any new restart points from being created. • Load Step: Specifies what load steps are to create restart points. Set to All to obtain restart points in all load steps, or to Last to obtain a restart point in the last load step only. • Substep: Specifies how often the restart points are created within a load step. Set to one of the following: • – Last to write the files for the last substep of the load step only. – All to write the files for all substeps of the load step. – Specified Recurrence Rate and enter a number N, in the Value field, to generate restart points for a specified number of substeps per load step. – Equally Spaced Points and enter a number N, in the Value field, to generate restart points at equally spaced time intervals within a load step. Maximum Points to Save Per Step: Specifies the maximum number of files to save for the load step. Choose one of the following options: – Enter 0 to not overwrite any existing files. The maximum number of files for one run is 999. If this number is reached before the analysis is complete, the analysis will continue but will no longer write any files. After 0 is entered, the field will show All. – Enter a positive number to specify the maximum number of files to keep for each load step. When the maximum number has been written for each load step, the first file of that load step will be overwritten for subsequent substeps. Note If you want to interrupt the solution in a linear transient analysis, by default, the interrupt will be at load step boundaries only (as opposed to nonlinear analyses where interrupts occur at substeps). However, if you want to interrupt a solution to a linear transient analysis on a substep basis, set the following: Generate Restart Controls = Manual, Load Step = All, Substep = All, and Maximum Points to Save Per Step = 1. These settings allow you to accomplish the interrupt on a substep basis without filling up your disk with restart files. • 536 Retain Files After Full Solve: When restart points are requested, the necessary restart files are always retained for an incomplete solve due to a convergence failure or user request. However, when the solve completes successfully, you have the option to request to either keep the restart points by setting this field to Yes, or to delete them by setting this field to No. You can control this setting here in the Details view of the Analysis Settings object, or under Tools> Options in the Analysis Settings and Solution preferences list. The setting in the Details view overrides the preference setting. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Note Retain Files After Full Solve has interactions with other controls. Under the Analysis Data Management (p. 549) category, setting Future Analysis to Prestressed forces the restart files to be retained. Similarly, setting Delete Unneeded Files to No implies that restart files are to be retained. Creep Controls Creep is a rate-dependent material nonlinearity in which the material continues to deform under a constant load. You can perform an implicit creep analysis for a static or transient structural analysis. Creep Controls are available in the Details view of the analysis settings for these two environments only after you have selected a creep material for at least one prototype in the analysis. Creep controls are step-aware, meaning that you are allowed to set different creep controls for different load steps in a multistep analysis. If there were multiple load steps in the analysis before you chose the creep material, then choosing the creep material will set the Creep Controls properties to their default value. The Creep Controls group includes the following properties: • Creep Behavior - The default value is Off for the first load step and On for all the subsequent load steps. You may change it according to your analysis. • Creep Limit Ratio (available only if Creep Behavior is set to On) - This property issues the Mechanical APDL CUTCONTROL command with your input value of creep limit ratio. (Refer to the CUTCONTROL command description for details). The default value of Creep Limit Ratio is 1. You are allowed to pick any non-negative value. Cyclic Controls The Harmonic Index Range setting within the Cyclic Controls category is used in a modal analysis that involves cyclic symmetry to specify the solution ranges for the harmonic index . The setting appears if you have defined a Cyclic Region for this analysis. • The Program Controlled option solves all applicable harmonic indices. • The Manual option exposes additional fields that allow you to specify a range of harmonic indices for solution from the Minimum value to the Maximum value in steps of the Interval value. Note Static structural cyclic symmetry solutions always use all harmonic indices required for the applied loads. Radiosity Controls The following settings within the Radiosity Controls category are used in conjunction with the Radiation (p. 586) load when defining surface to surface radiation for thermal related analyses that use the ANSYS solver. These settings are based on the RADOPT command in Mechanical APDL: • Flux Convergence Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 537 Features • Maximum Iteration • Solver Tolerance • Over Relaxation View Factors for 3-D Geometry For 3-D geometry, the Hemicube Resolution setting is also available based on the HEMIOPT command in Mechanical APDL. See the View Factor Calculation - Hemicube Method section in the Mechanical APDL Theory Reference for further information. View Factors for 2-D Geometry For 2–D geometry, the following settings are available and are based on the V2DOPT command in Mechanical APDL: • View Factor Method • Number of Zones • Axisymmetric Divisions See the following sections of the Mechanical APDL help for further information on these settings: • Using the Radiosity Solver Method in the Thermal Analysis Guide. • Mechanical APDL Theory Reference sections: – Non-Hidden Method – Hidden Method – View Factors of Axisymmetric Bodies Options for Modal, Harmonic, Linear Buckling, Random Vibration, and Response Spectrum Analyses An Options control group is included in the Analysis Settings Details view for the following analysis types: • Modal • Harmonic • Linear Buckling • Random Vibration • Response Spectrum Modal Analysis - Options Control Settings Max Modes to Find specifies the number of natural frequencies to solve for in a modal analysis. Limit Search Range allows you to specify a frequency range within which to find the natural frequencies. The default is set to No. If you set this to Yes, you can enter a minimum and maximum frequency value. If you specify a range the solver will strive to extract as many frequencies as possible within the specified range subject to a maximum specified in the Max Modes to Find field. 538 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Harmonic Analysis - Options Control Settings Frequency Sweep Range This is set by defining the Range Minimum and Range Maximum values under Options in the Details view. Solution Intervals This sets the number of the solution points between the Frequency Sweep Range. You can request any number of harmonic solutions to be calculated. The solutions are evenly spaced within the specified frequency range, as long as clustering is not active. For example, if you specify 10 solutions in the range 30 to 40 Hz, the program will calculate the response at 31, 32, 33, ..., 39, and 40 Hz. No response is calculated at the lower end of the frequency range. Two solution methods are available to perform harmonic analysis: Mode Superposition method and Direct Integration (Full) method. Below are some details regarding each of these methods. Mode Superposition Method Specific Options: Mode Superposition is the default method, and generally provides results faster than the Full method. In the Mode Superposition method a modal analysis is first performed to compute the natural frequencies and mode shapes. Then the mode superposition solution is carried out where these mode shapes are combined to arrive at a solution. Modal Frequency Range Specifies the range of frequencies over which mode shapes will be computed in the modal analysis: • Program Controlled: The modal sweep range is automatically set to 200% of the upper harmonic limit and 50% of the lower harmonic limit. This setting is adequate for most simulations. • Manual: Allows you to manually set the modal sweep range. Choosing Manual displays the Modal Range Minimum and Modal Range Maximum fields where you can specify these values. Cluster Results and Cluster Number (Mode Superposition only) This option allows the solver to automatically cluster solution points near the structure’s natural frequencies ensuring capture of behavior near the peak responses. This results in a smoother, more accurate response curves. Cluster Number specifies the number of solutions on each side of a natural frequency. The default is to calculate four solutions, but you may specify any number from 2 to 20. Options: • Solution Method = Mode Superposition • Cluster Number = Yes Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 539 Features Solution Intervals = 15: Here 15 solutions are evenly spaced within the frequency range. Note how the peak can be missed altogether. Cluster = 5: Here 5 solutions are performed automatically on either side of each natural frequency capturing the behavior near the peaks. Store Results At All Frequencies Upon solution, harmonic environments store data specified in the Output Controls for all intervals in the frequency range. Consequently, seeking additional results at new frequencies will no longer force a solved harmonic environment to be resolved. This choice will lead to a better compromise between storage space (results are now stored in binary form in the RST file) and speed (by reducing the need to resort to the solver to supply new results). Should storage become an issue, you can set Store Results At All Frequencies to No to request that only minimal data be retained to supply just the harmonic results requested at the time of solution. This option is especially useful for Mode Superposition harmonic analyses with frequency clustering. It is unavailable for harmonic analyses solved with the Full method. Note With this option set to No, the addition of new frequency or phase responses to a solved environment will require a new solution. The addition of new contour results does not share this requirement; data from the closest available frequency will be displayed (the reported frequency is noted on each result). However, data at an even closer frequency may be obtained with a new solution as needed. Note that the values of frequency and type of contour results (displacement, stress or strain) at the moment of the solve determine the contents of the result file and the subsequent availability of data. Forethought on these choices can significantly reduce the need to re-solve an analysis. Full Method Specific Options: 540 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings There are no special options for Full method. Linear Buckling - Options Control Settings Max Modes to Find: You need to specify the number of buckling load factors and corresponding buckling mode shapes of interest. Typically only the first (lowest) buckling load factor is of interest. Random Vibration - Options Control Settings Number of Modes to Use Specifies the number of modes to use from the modal analysis. A conservative rule of thumb is to include modes that cover 1.5 times the maximum frequency in the PSD excitation table. Exclude Insignificant Modes When set to Yes, allows you to not include modes for the mode combination as determined by the threshold value you set in the Mode Significant Level field. The default value of 0 means all modes are selected (same as setting Exclude Insignificant Modes to No) while a value of 1 means that no modes are selected. The higher the threshold is set, the fewer modes are selected for mode combination. Response Spectrum - Options Control Settings Number of Modes to Use Specify the number of modes to use from the modal analysis. It is suggested to have modes that span 1.5 times the maximum frequency defined in input excitation spectrum. Spectrum Type Specify either Single Point or Multiple Points. If two or more input excitation spectrums are defined on the same fixed degree of freedoms, use Single Point, otherwise use Multiple Points. Modes Combination Type Specify a method to be used for response spectrum calculation. Choices are SRSS, CQC, and ROSE. In general, the SRSS method is more conservative than the other methods. The SRSS method assumes that all maximum modal values are uncorrelated. For a complex structural component in three dimensions, it is not uncommon to have modes that are coupled. In this case, the assumption overestimates the responses overall. On the other hand, the CQC and the ROSE methods accommodate the deficiency of the SRSS by providing a means of evaluating modal correlation for the response spectrum analysis. Mathematically, the approach is built upon random vibration theory assuming a finite duration of white noise excitation. The ability to account for the modes coupling makes the response estimate from the CQC and ROSE methods more realistic and closer to the exact time history solution. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 541 Features Damping Controls Damping is present in most systems and should be specified in a Rigid Dynamics, Transient Structural, harmonic response, random vibration, or response spectrum analysis. The following forms of damping are available in the program: • Beta Damping, β. Beta damping defines the stiffness matrix multiplier for damping. You can input the value of beta damping directly or the value can be computed from a damping ratio at a specified frequency. You define beta damping in the Details view of the Analysis Settings object. The value of β is not generally known directly, but is calculated from the modal damping ratio, ξi. ξi is the ratio of actual damping to critical damping for a particular mode of vibration, i. If ωi is the natural circular frequency, then the beta damping is related to the damping ratio as β = 2 ξi/ωi . Only one value of β can be input in a step, so choose the most dominant frequency active in that step to calculate β. • Material-Dependent Damping. You define material-dependent damping as a material property in Engineering Data. • Constant Material Damping Coefficient - only applicable for harmonic response analyses. You define the constant material damping coefficient as a material property in Engineering Data. • Constant Damping Ratio - only applicable for harmonic response, random vibration, and response spectrum analyses. This specifies the amount of damping in the structure as a percentage of critical damping. If you set this in conjunction with beta damping, the effects are cumulative. You define the constant damping ratio in the Details view of the Analysis Settings object. • Element Damping from Spring elements – only applicable for rigid dynamics, transient structural, and harmonic analyses. You define the element damping from spring elements in the Details view of the Spring object. • Numerical damping, also referred to as amplitude decay factor (γ), controls numerical noise produced by the higher frequencies of a structure. Usually the contributions of these high frequency modes are not accurate and some numerical damping is preferable. A default value of 0.1 is used for Transient Structural analysis and a default value of 0.005 is used for Transient Structural analysis using a linked Modal analysis system. To change the default, change the Numerical Damping field in the Details view of the Analysis Settings object to Manual from Program Controlled, which allows you to enter a custom value in the Numerical Damping Value field. You can specify more than one form of damping in a model. The program will formulate the damping matrix as the sum of all the specified forms of damping. Nonlinear Controls Various controls are available under the Nonlinear Controls category for the following: • Static and Transient Structural • Transient Thermal Analyses • Rigid Dynamics Analyses Nonlinear Controls for Static and Transient Convergence Criterion 542 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings When solving nonlinear static or transient analyses an iterative procedure (equilibrium iterations) is carried out at each substep. Successful solution is indicated when the out-of-balance loads are less than the specified convergence criteria. Criteria appropriate for the analysis type and physics are displayed in this grouping. The following criteria are available: Force, Moment, Displacement, Rotation, Heat, Temperature, CSG, and AMP. The following convergence controls are available for each of these criteria: • Program Controlled (default): The Mechanical application sets the convergence criteria. • On: You specifically would like for this convergence criterion to be activated. – Value: This is the reference value that the solver uses to establish convergence. It may be program controlled (recommended) in which case the solver automatically calculates the value based on external forces including reactions, or you can input a constant value. When Temperature Convergence is set to On, the Value field includes a drop down option list where you can choose either ANSYS Calculated or User Input. Choosing User Input displays an Input Value field where you can add a value. When any other convergence is set to On, simply clicking on ANSYS Calculated allows you to add a value that will replace the ANSYS Calculated display. • – Tolerance times Value determines the convergence criterion – Minimum Reference: This is useful for analyses where the external forces tend to zero. This can happen, for example, with free thermal expansion where rigid body motion is prevented. In these cases the larger of Value or Minimum Reference will be used as the reference value. Remove: Indicates that an attempt will be made to remove this criterion during solution. Note You may activate Displacement/Rotation convergence by the Mechanical APDL solver arbitrarily for highly nonlinear problems, even though you explicitly removed this option by choosing Remove from the drop-down menu. If for some reasons, you want to override this default behavior, it is important to turn on Force/Moment convergence and then try choosing Remove on Displacement/Rotation convergence. If you do not want any convergence options to be turned on, then you may try setting the solution controls to off, using a Commands Objects (p. 856) object. Line Search Line search can be useful for enhancing convergence, but it can be expensive (especially with plasticity). You might consider setting Line Search on in the following cases: • When your structure is force-loaded (as opposed to displacement-controlled). • If you are analyzing a "flimsy" structure which exhibits increasing stiffness (such as a fishing pole). • If you notice (from the program output messages) oscillatory convergence patterns. Stabilization Convergence difficulty due to an unstable problem is usually the result of a large displacement for small load increments. Nonlinear stabilization technique can help achieve convergence. Nonlinear stabilization can be thought of as adding artificial dampers to all of the nodes in the system. Any degree of freedom Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 543 Features that tends to be unstable has a large displacement causing a large damping/stabilization force. This force reduces displacements at the degree of freedom so stabilization can be achieved. There are three Keys for controlling nonlinear stabilization: • Off - Deactivate stabilization (Default). • Constant - Activate stabilization. The energy dissipation ratio or damping factor remains constant during the load step. • Reduce - Activate stabilization. The energy dissipation ratio or damping factor is reduced linearly to zero at the end of the load step from the specified or calculated value. There are two Methods for stabilization control: • Energy - Use the energy dissipation ratio as the control (Default). • Damping - Use the damping factor as the control. For the Energy method, the Energy Dissipation Ratio needs to be specified. The energy dissipation ratio is the ratio of work done by stabilization forces to element potential energy. This value is usually a number between 0 and 1. The default value is 1.0e-4. For the Damping method, the Damping Factor needs to be specified. The damping factor is the value that ANSYS uses to calculate stabilization forces for all subsequent substeps. This value is greater than 0. There are three options for Activation For First Substep control: • No - Stabilization is not activated for the first substep even when it does not converge after the minimal allowed time increment is reached (Default). • On Non-convergence - Stabilization is activated for the first substep if it still does not converge after the minimal allowed time increment is reached. Use this option for the first load step only. • Yes - Stabilization is activated for the first substep. Use this option if stabilization was active for the previous load step Key = Constant. For Stabilization Force Limit, a number between 0 and 1 should be specified. The default value is 0.2. To omit a stabilization force check, set this value to 0. Refer to Unstable Structures in the Mechanical APDL Structural Analysis Guide for assistance with using the stabilization options listed above. Nonlinear Controls for Transient Thermal Analyses Nonlinear Formulation Nonlinear Formulation controls how nonlinearities are to be handled for the solution. The following options are available: • Program Controlled (default) - Workbench automatically chooses between the Full or Quasi setting as described below. The Quasi setting is based on a default Reformulation Tolerance of 5%. The Quasi option is used by default, but the Full option is used in cases when a Radiation load is present or when a distributed solver is used during the solution. • Full - Manually sets formulation for a full Newton-Raphson solution. 544 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings • Quasi - Manually sets formulation based on a tolerance you enter in the Reformulation Tolerance field that appears if Quasi is chosen. Nonlinear Controls for Rigid Dynamics Analyses Relative Assembly Tolerance Allows you to specify the criterion for determining if two parts are connected. Setting the tolerance can be useful in cases where initially, parts are far enough away from one another that, by default, the program will not detect that they are connected. You could then increase the tolerance as needed. Energy Accuracy Tolerance This is the main driver to the automatic time stepping. The automatic time stepping algorithm measures the portion of potential and kinetic energy that is contained in the highest order terms of the time integration scheme, and computes the ratio of the energy to the energy variations over the previous time steps. Comparing the ratio to the Energy Accuracy Tolerance, Workbench will decide to increase or decrease the time step. See the Rigid Dynamics Analysis (p. 102) section for more information. Output Controls Output Controls give you the ability to specify which type of quantities are written to the result file for use during post-processing. As a result, you can control the size of the results file which can be beneficial when performing a large analysis. The following Output Controls are available in the Details view to be activated (Yes) or not (No) and included or not included in the results file. • Stress. Writes element nodal stresses to the results file. The default value is Yes. Available for Static Structural, Transient Structural, Modal, and Linear Buckling analysis types. • Strain. Writes element elastic strains to the results file. The default value is Yes. Available for Static Structural, Transient Structural, Modal, and Linear Buckling analysis types. • Nodal Forces. Writes elemental nodal force to the results file. This output control must be set to Yes if you want to use the MAPDL Command NFOR, FSUM in Mechanical (via command snippets) because those MAPDL commands will access nodal force records in the result file as well as to obtain Reactions on the underlying source or target element. The default value is No. Available for Static Structural, Transient Structural, Harmonic and Modal analysis types. • Calculate Reactions. Turn On for Nodal Forces on constraints. Available for Modal, Harmonic, and Transient analysis types. • Calculate Thermal Flux. Available for Steady-State Thermal and Transient Thermal analysis types. • Calculate Velocity. Writes Velocity to the results file. The default value is No. Available for Response Spectrum analysis types. • Calculate Acceleration. Writes Acceleration to the results file. The default value is No. Available for Response Spectrum analysis types. • Contact Miscellaneous. Turn On if Contact Based Forced Reactions are desired. The default value is No. Available for Static and Transient Structural analysis types. • General Miscellaneous. Used to access element miscellaneous records via SMISC/NMISC expressions for user defined results. The default value is No. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 545 Features Note To ensure that Membrane and Bending Stress results are not under-defined, set this option to Yes. • Max Number of Result Sets. Zero (0) is the default value for this option and displays as Program Controlled (uses the default value defined in MAPDL) . Available for Static Structural, Transient Structural, Steady-State Thermal, and Transient Thermal analysis types. • Store Modal Results. Available for Modal analyses only. This field is displayed only when Stress and/or Strain are set to Yes, implying that stress and strain results are to be expanded and saved to file.mode, in addition to displacement results (mode shapes). Depending on the downstream linked analysis, you may want to save these modal stress and/or modal strain results, which are linearly superimposed to get the stress and/or strain results of the downstream linked analysis. This reduces computation time significantly in the downstream linked analysis because no modal stress and/or modal strain results are expanded again. The following options are available: • – Program Controlled (Default): Let the program choose whether or not the modal results are saved for possible downstream analysis. – No: Stress and strain results are not saved to file.mode for later use in the downstream linked analyses. This option is recommended for the linked harmonic analysis due to load generation, which requires that stresses and/or strains are expanded again as a result of the addition of elemental loads in the linked harmonic analysis. – For Future Analysis: Stress and strain results are saved to file.mode for later use in the downstream linked analyses. This option is recommended for a linked random vibration analysis. Choosing this option improves the performance and efficiency of the linked random vibration analysis because, with no load, there is no need for stress and strain expansion. Expand Results From. – Linked Harmonic analyses. This field is displayed only when Stress and/or Strain and/or Calculate Reactions are set to Yes, implying that stress, strain, and reaction results are to be expanded and saved to file.mode after the load generation. Depending on the number of modes and number of frequency steps, you may want to save these modal stresses and/or strains after the load generation, which can be linearly superimposed to obtain harmonic stresses and/or strains at each frequency step. The following options are available: → Program Controlled (Default): Let the program choose whether or not the stress, strain, and reaction results are expanded and saved for possible downstream analysis. When the Program Controlled option is chosen, one more read-only Details view entry (Expansion) will be shown. This indicates whether the stress, strain and reaction results are expanded from the modal solution or harmonic solution. → Harmonic Solution: Stress, strain, and reaction results are not expanded nor saved to file.mode after the load generation in the linked harmonic system. This option is recommended when the number of frequency steps is far less than the number of modes. In this option, the stress, strain, and/or reaction results are expanded from harmonic displacement at each frequency step. In this case, stress, strain, and/or reaction expansion is performed as many times as the number of frequency steps. → Modal Solution: Stress, strain, and reaction results are expanded and saved to file.mode after the load generation in the linked harmonic system. This option is recommended when the number of frequency steps is far more than the number of modes. In this option, the stress, strain, and/or reaction results are calculated by linearly combining the modal stresses, modal 546 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings strains, and/or modal reactions expanded after the load generation. In this case, stress, strain, and/or reaction expansion are performed as many times as the number of modes. Refer to Recommended Settings for Modal and Linked Analysis Systems (p. 548) for further details. – Linked Transient analyses. This field is displayed only when Calculate Stress and/or Calculate Strain are set to Yes, implying that stress, strain and reaction results are to be expanded and saved to file.mode after the load generation. Depending on the number of modes and total number of sub steps/ time steps, you may want to save these modal stresses and/or strains after the load generation, which can be linearly superimposed to obtain transient stresses and/or strains at each time step. The following options are available: → Program Controlled (Default): Let the program choose whether or not the stress and strain results are expanded and saved for possible downstream analysis. When the program controlled option is chosen, one more read only details view entry - - Expansion will be shown. This indicates whether the stress and strain results are expanded from modal solution or transient solution. → Transient Solution: Stress and strain results are not expanded nor saved to file.mode after the load generation in the linked transient analysis system. This option is recommended when the number of time steps accumulated over all the load steps is far less than the number of modes. In this option, the stress and/or strain results are expanded from transient displacement at each time step. In this case, stress and/or strain expansion is performed as many times as the number of time steps. → Modal Solution: Stress and strain results are expanded and saved to file.mode after the load generation in the linked transient system. This option is recommended when the number of time steps accumulated over all the load steps is far more than the number of modes. In this option, the stress and/or strain results are calculated by linearly combining the modal stresses and/or modal strains expanded after the load generation. In this case, stress and/or strain expansion are performed as many times as the number of modes. Refer to Recommended Settings for Modal and Linked Analysis Systems (p. 548) for further details. Note • It is recommended that you not change Output Controls settings during a Solution Restart. Modifying Output Controls settings change the availability of the respective result type in the results file. Consequently, result calculations cannot be guaranteed for the entire solution. In addition, Result file values may not correspond to GUI settings in this scenario. Settings turned off during a restart generate results equal to zero and may affect post processing of results and are therefore unreliable. • Modification of Stress, Strain, Nodal Force, Contact Miscellaneous, and General Miscellaneous will not invalidate the solution. If you want these output controls setting modification to be incorporated to your solution, please clean the solution first. The above output controls are not step-aware, meaning that the settings are constant across multiple steps. In addition, the following settings allow you to define when data is calculated and written to the result file for static structural, transient structural, rigid dynamics, steady-state thermal, and transient thermal analyses: • Calculate Results At. Specify this time to be All Time Points (default), Last Time Point, Equally Spaced Points or Specified Recurrence Rate. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 547 Features • Value. Displayed only if Calculate Results At is set to Equally Spaced Points or Specified Recurrence Rate. The controls that define when data is calculated are step aware, meaning that the settings can vary across multiple steps. Recommended Settings for Modal and Linked Analysis Systems The following table provides a summary of recommended settings for Store Modal Results and Expand Results From based on the analysis type. Analysis Type Recommended Store Modal Results Settings Recommended Expand Results From Settings Modal with no downstream linked analysis No Not available. Modal with downstream linked Harmonic analysis Stress and strain results not needed to be saved to file.mode because there is no downstream analysis. No Harmonic Solution Stress and strain results from modal analysis are overwritten by stresses and strains which are expanded again in the linked harmonic analysis due to any loads added in the downstream analysis. Use when number of frequency steps are far less than the number of modes. This option is not available when the modal analysis is pre-stress. Modal Solution Use when number of frequency steps are far more than the number of modes. This is the only option available when the modal analysis is pre-stress. Modal with downstream linked Random Vibration analysis Modal with downstream linked Response Spectrum analysis 548 For Future Analysis Not available. Stress and strain results from modal analysis are expanded and used in the linked random vibration analysis. No stress or strain expansion is needed again because there is no load. No Not available. Stress and strain results are always combined in response spectrum analysis using file.rst and file.mcom. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Analysis Type Recommended Store Modal Results Settings Recommended Expand Results From Settings Note To evaluate summation of element nodal forces using FSUM in Command Snippet, it is required to save element nodal forces in modal to file.mode. Modal with downstream linked transient analysis No Transient Solution Stress and strain results from modal analysis are overwritten by stresses and strains which are expanded again in the linked transient analysis due to any loads added in the downstream analysis. Use when number of time steps accumulated over all the load steps is far less than the number of modes. Modal Solution Use when number of time steps accumulated over all the load steps is far more than the number of modes. Limitations When Using the Mechanical APDL Solver • The Mechanical application cannot post process split result files produced by the ANSYS solver. Try either of the following workarounds should this be an issue: – Use Output Controls to limit the result file size. Also, the size can more fully be controlled (if needed) by inserting a Commands object for the OUTRES command. – Increase the threshold for the files to be split by inserting a Commands object for the /CONFIG,FSPLIT command. Analysis Data Management This grouping describes the options and specifications associated with the solution files. • Solver Files Directory: Indicates the location of the solution files for this analysis. The directory location is automatically determined by the program as detailed in File Management in the Mechanical Application (p. 792). For Windows users, the solution file folder can be displayed using the Open Solver Files Directory feature. – Open Solver Files Directory Feature → This right-click context menu option is available when you have an analysis Environment or a Solution object selected. → Once executed, this option opens the operating system's (Windows Only) file manager and displays the directory that contains the solution files for your analysis. → The directory path is shown in the Details View. If a solution is in progress, the directory is shown in the Solver Files Directory field. When a solution is in progress, the directory displays in the Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 549 Features Scratch Solver Files Directory. For a remote solve, it will open the scratch directory until the results download is complete. → This option is available on the Windows platform only. • Future Analysis: Indicates if the results of this analysis will be used as a load or an initial condition in a subsequent analysis. Below are possible future analysis options for each analysis type. Refer to Define Initial Conditions (p. 12) for further details. – Static Structural analysis → Pre-Stressed Modal analysis → Linear Buckling analysis – Modal analysis → Prerequisite for a random vibration (PSD) or response spectrum analysis. • Scratch Solver Files Directory: This is a read-only indication of the directory where a solve “in progress” occurs. All files generated after the solution is done (including but not limited to result files) are then moved to the Solver Files Directory. The files generated during solves on My Computer or files requested from RSM for postprocessing during a solve remain in the scratch directory. For example, an early result file could be brought to the scratch folder from a remote machine through RSM during postprocessing while solving. With the RSM method, the solve may even be computed in this folder (for example, using the My Computer, Background SolveProcess Settings). The Mechanical application maintains the Scratch Solver Files Directory on the same disk as the Solver Files Directory. The scratch directory is only set for the duration of the solve (with either My Computer or My Computer, Background). After the solve is complete, this directory is set to blank. The use of the Scratch Solver Files Directory prevents the Solver Files Directory from ever getting an early result file. • Save MAPDL db: No (default) / Yes. Some Future Analysis settings will require the db file to be written. In these cases this field will be set to Yes automatically. • Delete Unneeded File: Yes (default) / No. If you prefer to save all the solution files for some other use you may do so by setting this field to No. • Nonlinear Solutions: Read only indication of Yes / No depending on presence of nonlinearities in the analysis. • Solver Units: You can select one of two options from this field: • 550 – Active System - This instructs the solver to use the currently active unit system (determined via the toolbar Units menu) for the very next solve. – Manual - This allows the you to choose the unit system for the solver to use by allowing them access to the second field, "Solver Unit System". Solver Units System: – If Active System is chosen for the Solver Units field, then this field is read only and displays the active system. – If Manual is chosen for the Solver Units field, this field is a selectable drop down menu. – If a Magnetostatic analysis is being performed, the field is read only because the only system available to solve the analysis is the mks system. – If a Thermoelectric or Electric analysis is being performed, only mks and µmks systems can be selected because they are the only systems currently allowed for these analyses. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Rotordynamics Controls The following settings control the items that apply to a rotating structure in a Modal Analysis. • Coriolis Effect - Set to On if Coriolis effects should be applied. On is a valid choice only if the Damped Solver Control is Yes. The default is Off. • Campbell Diagram - Set to On if Campbell diagram is to be plotted. The default is Off. On is a valid choice only if Coriolis Effect is turned on. • Number of Points - Indicates the number of solve points for the Campbell diagram. The default is 2. A minimum of 2 solve points is necessary. Displayed only when Campbell Diagram is set to On. • Mode Reuse - Only applicable for the Reduced Damped solver. Mode Reuse allows the solver to compute complex eigensolutions efficiently during subsequent solve points by reusing undamped eigensolution calculated in the first solve point. The default setting is Program Controlled. Visibility Allows you to selectively display loads in the Graph window by choosing Display or Omit for each load. Applying Boundary Conditions All loads and supports are applicable to a 2-D or 3-D simulation except where noted in the description of the specific load or support. To insert a boundary condition for an analysis, right click on the analysis system object in the tree and select Insert > {boundary condition name}. Alternatively, click on the analysis system object, click on Loads, Supports, Conditions, or Direct FE and choose the boundary condition from the drop-down menu. The following topics are addressed in this section: Types of Supports Types of Loads Conditions Direct FE Spatial Varying Loads and Displacements Specifying Load Values Remote Boundary Conditions Imported Loads Direction Scope Types of Supports Fixed Supports Fixed Face Fixed Edge Fixed Vertex Displacements Displacements: Faces, Edges, and Vertices Remote Displacement Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 551 Features Velocity Velocity Explicit Dynamics Impedance Boundary Frictionless Frictionless Face Compression Compression Only Support Cylindrical Cylindrical Support Simply Supported Simply Supported Edge Simply Supported Vertex Fixed Rotation Fixed Rotation Elastic Elastic Support Fixed Supports Fixed Face Prevents one or more flat or curved faces from moving or deforming. Immobilized face Fixed Edge Prevents one or more straight or curved edges from moving or deforming. 552 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Immobilized edge (e.g., of a bolt hole) A fixed edge is not realistic and leads to singular stresses (that is, stresses that approach infinity near the fixed edge). You should disregard stress and elastic strain values in the vicinity of the fixed edge. Fixed Vertex Prevents one or more vertices from moving. Immobilized vertex A fixed vertex fixes both translations and rotations on faces or line bodies. A fixed vertex is not realistic and leads to singular stresses (that is, stresses that approach infinity near the fixed vertex). You should disregard stress and elastic strain values in the vicinity of the fixed vertex. If you are using a surface body model, see Simply Supported Vertex (p. 561). Note This boundary condition cannot be applied to a vertex scoped to an end release. Displacements These boundary conditions are applied at the geometry level and require that one or more flat or curved faces or edges or one or more vertices to displace relative to their original location by one or more components of a displacement vector in the world coordinate system or local coordinate system, if applied. Note In a cylindrical coordinate system X, Y, and Z are used for R, Θ, and Z directions. When using a cylindrical coordinate system, non-zero Y displacements are interpreted as translational displacement quantities, ∆Y = R∆Θ. Since they are treated as linear displacements it is a reasonable approximation only, for small values of angular motion ∆Θ. For Explicit Dynamics analyses, when using a cylindrical coordinate system, the Y the component (that is, Θ direction) of a displacement constraint is defined as a rotation. Solution Restarts are only supported for Tabular data modifications. This boundary condition cannot be applied to a vertex scoped to an End Release. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 553 Features The behavior of the Displacement boundary condition is illustrated below. Table 2 Surface Non-zero X-, Y-, and Z-components. The face retains its original shape but moves relative to its original location by the specified displacement vector. The enforced displacement of the face causes a model to deform. Zero Y-component. No part of the face can move, rotate, or deform in the Y-direction. Blank (undefined) X- and Z-components. The surface is free to move, rotate, and deform in the XZ plane. Table 3 Edge Non-zero X-, Y-, and Z-components . The edge retains its original shape but moves relative to its original location by the specified displacement vector. The enforced displacement of the edge causes a model to deform. Zero Y-component . No part of the edge can move, rotate, or deform in the Y-direction . Blank (undefined) X- and Z-components. The edge is free to move, rotate, and deform in the XZ plane. Table 4 Vertex Non-zero X-, Y-, and Z-components. The vertex moves relative to its original location by the specified displacement vector. The enforced displacement of the vertex causes a model to deform. Zero Y-component. The vertex cannot move in the Y-direction. Blank (undefined) X- and Z-components. The vertex is free to move in the XZ plane. Multiple surfaces, edges, or vertices can be selected. 554 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Define the vector in terms of either: • the displacement constraint acting normal to the surface to which it is attached (essentially a frictionless support with a non-zero displacement) [Define By: Normal To] • components (in the world coordinate system or local coordinate system, if applied) [Define By: Components] Note • Entering a zero for a component prevents deformation in that direction. • Entering a blank for a component allows free deformation in that direction. • Avoid using multiple Displacements on the same face/edge/vertex and on faces/edges/vertices having shared faces/edges/vertices . Enforced displacement of an edge is not realistic and leads to singular stresses (that is, stresses that approach infinity near the loaded edge). You should disregard stress and elastic strain values in the vicinity of the loaded edge. Remote Displacement A Remote Displacement allows you to apply both displacements and rotations at an arbitrary remote location in space. You specify the origin of the remote location under Scope in the Details view by picking, or by entering the XYZ coordinates directly. The default location is at the centroid of the geometry. You specify the displacement and rotation under Definition. The location and the direction of a Remote Displacement can be defined in the global coordinate system or in a local Cartesian coordinate system. A common application is to apply a rotation on a model at a local coordinate system. An example is shown below along with a plot of the resulting Total Deformation. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 555 Features Note This boundary condition cannot be applied to a vertex scoped to an end release. A Remote Displacement is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 628) section for a listing of all remote boundary conditions and their characteristics. Note Solution Restarts are only supported for Tabular data modifications. For a modal analysis, only zero magnitude Remote Displacement values are valid. These function as supports. If non-zero magnitude remote displacements are needed for a PreStress Modal analysis, apply the Remote Displacement in the static structural environment. Velocity Apply a Velocity support to faces, edges, vertices, or bodies. Once geometry specifications are complete, define the vector for this support in terms of either: • components (in the world coordinate system or local coordinate system, if applied) [Define By: Components]. When defined by components, the following options are available for the component values. – Constant – Tabular – Function – Free (default) See the Specifying Load Values (p. 621) section of the Mechanical Help for additional information. • the velocity constraint acting normal to the surface to which it is attached [Define By: Normal To], and is defined in the following forms: – Constant (Free) – Tabular – Function Note that: • Entering a zero for a component sets the velocity to zero. • Entering a blank for a component allows free velocity in that direction. 556 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions • Avoid using multiple velocities on the same vertex. • For Explicit Dynamics analyses, the Y Component (that is, Θ direction) of a velocity constraint defined with a cylindrical coordinate system has units of angular velocity. • This boundary condition cannot be applied to a vertex scoped to an end release. Impedance Boundary You can use the impedance boundary condition to transmit waves through cell faces. The boundary condition predicts the pressure P in the dummy cell from the impedance, particle velocity and a reference pressure (P0). Only the perpendicular component is transmitted, as the pressure is spherical. Therefore, the Impedance boundary condition is only approximate, and should be placed as far as possible from region of interest. Details Category Fields Description Scope Scoping Method Geometry Selection Named Selection Definition Geometry Displays the number of selected faces. Named Selection Displays a list of named geometry elements. Type Material Impedance Program Controlled or value Reference Velocity Program Controlled or value Reference Pressure Program Controlled or value Suppressed Includes or excludes the boundary condition in the analysis. Theory In order to economize on problem size it is sometimes advantageous for problems which have only outward traveling solutions (e.g. an expanding high pressure source) to limit the size of the grid by a boundary condition which allows outward traveling waves to pass through it without reflecting energy back into the computational grid. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 557 Features In practice it proves impossible to include a simple boundary condition which is accurate for all wave strengths but the algorithm used here give a reasonable approximation over a wide spectrum. However it should always be borne in mind that the condition is only approximate and some reflected wave, however small, will be created and care must be taken that such a wave does not have a significant effect on the later solution. Note that the following analysis deals only with the normal component of velocity of the wave and the velocity component parallel to the boundary is assumed to be unaffected by the boundary. For a one-dimensional wave traveling in the direction of increasing x, the conditions on the rearward facing characteristic are where ρc is the acoustic impedance (ρ is the local density and c is the local sound speed) and dp and du are the changes of pressure and velocity normal to the wave along the characteristic. Since it is assumed that no wave energy is being propagated back in the direction of decreasing x the error in applying the above condition on a non-characteristic direction is in general small and it is applied on the transmitting boundary in the form Where: uN is the component of mean velocity normal to the boundary [ρc]boundary is the assumed Material Impedance for the boundary pref is the user defined reference pressure uref is the user defined reference velocity at the boundary For an initially stationary structure at zero pressure, the reference values (pref and uref) are normally set to zero. In this case we have which is exact for a plane elastic longitudinal wave propagating in an infinite elastic medium. Note The default Material Impedance (Program Controlled) is zero. In this case the impedance at the boundary is taken to be the impedance at time t of the element to which the boundary is applied. This represents the case of perfect transmission of plane normal elastic waves. Frictionless Face Prevents one or more flat or curved faces from moving or deforming in the normal direction. 558 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Normal direction relative to the face. No portion of the surface body can move, rotate, or deform normal to the face. Tangential directions. The surface body is free to move, rotate, and deform tangential to the face. For a flat surface body, the frictionless support is equivalent to a symmetry condition. Compression Only Support Applies a compression only constraint normal to one or more faces. Consider the following model with a bearing load and supports as shown. Note the effect of the compression only support in the animation of total deformation. The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the help. Interface names and other components shown in the demo may differ from those in the released product. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 559 Features Since the region of the face in compression is not initially known, a nonlinear solution is required and may involve a substantial increase in solution time. Cylindrical Support For 3-D simulations, prevents one or more cylindrical faces from moving or deforming in combinations of radial, axial, or tangential directions. Any combination of fixed and free radial, axial, and tangential settings are allowed. Radial directions relative to the cylinder (Fixed). Such cylindrical faces cannot move or deform radially to the cylinder. Axial directions relative to the cylinder (Fixed). Such cylindrical faces cannot move or deform axially to the cylinder. Tangential direction relative to the cylinder (Fixed). Such cylindrical faces cannot move or deform tangentially to the cylinder. Axial and tangential directions (Free). The cylinder is free to move, rotate, and deform axially and tangentially. Radial and tangential directions (Free). The cylinder is free to move, rotate, and deform radially and tangentially. Radial and axial directions (Free). The cylinder is free to move, rotate, and deform radially and axially. For 2-D simulations, cylindrical supports can only be applied to circular edges. Simply Supported Edge Available for 3-D simulations only. Edge is fixed in all directions. Rotation, however, is permitted about the edge. Applicable for surface body models or line models only. Prevents one or more straight or curved edges from moving or deforming but rotations about the line are allowed. If you want to fix the rotations as well, use Fixed Edge (p. 552). 560 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Note This boundary condition cannot be applied to a vertex scoped to an end release. Simply Supported Vertex Available for 3-D simulations only. Vertex is fixed in all directions. Rotations, however, are permitted. Applicable for surface body models or line models only. Prevents one or more vertices from moving. Rotation about the vertex is allowed. If you want to prevent rotations, use Fixed Vertex (p. 553). A simply supported vertex is not realistic and leads to singular stresses (that is, stresses that approach infinity near the simply supported vertex). You should disregard stress and elastic strain values in the vicinity of the simply supported vertex. Note This boundary condition cannot be applied to a vertex scoped to an End Release. Fixed Rotation You can apply a fixed rotation support to faces, edges, and vertices of a surface body. When you only apply a fixed rotation support to a surface body, the geometry is free in all translational directions. However, the rotation of the geometry is fixed about the axis of the coordinate system that you select. To apply a fixed rotation support: 1. In the Project tree, right-click the Analysis node to display the context menu. 2. On the context menu, point to Insert, and then click Fixed Rotation. 3. Select a face, edge, or vertex, and then click Apply . 4. Select the coordinate system that you want to use to specify the rotation constraint. 5. In the Details view, select Free or Fixed for Rotation X, Rotation Y, and Rotation Z to define the fixed rotation support. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 561 Features Note • A fixed vertex rotation support is not realistic and leads to singular stresses (that is, stresses that approach infinity near the fixed vertex rotation support). You should disregard stress and elastic strain values in the vicinity of the fixed vertex rotation support. • Rotation constraints are combined with other constraints that produce rotational DOF assignments to determine which values to apply. They are combined with all other constraints to determine the Nodal Coordinate System orientation (frictionless supports, cylindrical supports, given displacements, etc.). • There may be circumstances in which the rotational support and other constraints cannot resolve a discrepancy for preference of a particular node’s coordinate system . • This boundary condition cannot be applied to a vertex scoped to an end release. • When parameterizing this boundary condition, a Free axis of rotation is represented by a zero (0) and Fixed with a value of one (1) inside the Parameter Workspace in ANSYS Workbench (outside of Mechanical). Elastic Support Allows one or more faces or edges to move or deform according to a spring behavior. The Elastic Support is based on a Foundation Stiffness that you set in the Details view, which is defined as the pressure required to produce a unit normal deflection of the foundation. Types of Loads Inertial Loads Acceleration Standard Earth Gravity Rotational Velocity Structural Loads Pressure Pipe Pressure Pipe Temperature Hydrostatic Pressure Force Remote Force Bearing Load Bolt Pretension Moment Generalized Plain Strain Line Pressure PSD Base Excitation RS Base Excitation Joint Load Thermal Condition 562 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Thermal Loads Temperature Convection Radiation Heat Flow Perfectly Insulated Heat Flux Internal Heat Generation Electric Loads Voltage Current Thermal Condition Magnetostatic Loads Electromagnetic Boundary Conditions and Excitations Magnetic Flux Boundary Conditions Conductor Imported Loads Imported Body Force Density Imported Body Temperature Imported Convection Coefficient Imported Heat Flux Imported Heat Generation Imported Pressure Imported Surface Force Density Imported Temperature Interaction Loads The following loads involve interactions between the Mechanical application and other products. Motion Load Fluid Solid Interface Explosive Initiation Detonation Point Acceleration Translational acceleration accounts for the structural effects of a constant linear acceleration. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 563 Features Translational acceleration vector The global Acceleration load defines a linear acceleration of a structure in each of the global Cartesian axis directions. If desired, acceleration can be used to simulate gravity (by using inertial effects) by accelerating a structure in the direction opposite of gravity (the natural phenomenon of ). That is, accelerating a structure vertically upwards (+Y) at 9.80665 m/s2 (in metric units), applies a force on the structure in the opposite direction (-Y) inducing gravity (pushing the structure back towards earth). Units are length/time2. Alternatively, you can use the Standard Earth Gravity load to produce the effect of gravity. Gravity and Acceleration are essentially the same type of load except they have opposite sign conventions and gravity has a fixed magnitude. For applied gravity, a body tends to move in the direction of gravity and for applied acceleration, a body tends to move in the direction opposite of the acceleration. The illustrations shown below compare how Acceleration and Gravity can be used to specify a gravitational load with the same result. Acceleration Example Global Acceleration load applied in the +Y direction to simulate gravity. 564 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Resulting deformation. Standard Earth Gravity Example Standard Earth Gravity applied. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 565 Features Resulting deformation. Define the Acceleration vector in terms of either: • a magnitude and direction (based on selected geometry) [Define By: Vector] • components (in the world coordinate system or local coordinate system, if applied) [Define By: Components] Note While loads are associative with geometry changes, load directions are not. This applies to any load that requires a vector input, such as: moment, acceleration, rotational velocity, force, and bearing load. Standard Earth Gravity Applies gravitational effects on a body in the form of an external force. Gravitational vector • Define the vector in terms of any of the following directions in the World Coordinate System or Local Coordinate System, if applied: +x, -x, +y, -y, +z, -z. • Gravity is a specific example of acceleration with an opposite sign convention and a fixed magnitude. Gravity loads cause a body to move in the direction of gravity. Acceleration loads cause a body to move in the direction opposite of acceleration. Refer to the example shown under Acceleration (p. 563) for details. • The magnitude is set: 9.80665 m/s2 (in metric units) • The direction is changeable. • The vector is added to acceleration when it is present. 566 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Rotational Velocity Rotational velocity accounts for the structural effects of a part spinning at a constant rate. You can apply rotational velocity to solid bodies, 3-D surface bodies, 2-D models and line bodies. For assemblies, you can apply rotational velocity to all bodies, or to selected bodies. You select bodies through geometry or named selections. In a modal analysis, rotational velocity is valid only when Coriolis Effect in the Rotordynamics Controls group of the Analysis Settings object is turned on. Geometry Selection To apply rotational velocity to all bodies, in the Details view, accept the default Geometry setting of All Bodies. [Basis: the CGOMGA command in Mechanical APDL, the CMOMEGA command in Mechanical APDL for Modal Analysis.] To apply rotational velocity to selected bodies, in the Details view, set Scoping Method to either Geometry Selection or Named Selection, then either select the bodies in the Geometry window (hold down the Ctrl key to multiple select) or list the named selections in the Details view. [Basis: the CMOMEGA command in Mechanical APDL.] To apply additional rotational velocity loads, you must have applied the original load to selected bodies, per above, not to All Bodies. Note One rotational velocity load can be applied to one or more bodies. However, multiple rotational velocity loads cannot be applied to the same body. Attempting to apply more than one rotational velocity load to the same body will invalidate the loads. Definition Define rotational velocity in terms of either: • a magnitude and an axis of rotation (based on selected geometry) [Define By: Vector] • a point and components (in the world coordinate system or local coordinate system, if applied) [Define By: Components] Note • In a Modal Analysis with multiple solve points (Campbell Diagram turned on), the magnitude or the resultant of the components must be in ascending order. • In a Modal Analysis when specifying by Components, only the Global Coordinate System is available (the option is read-only). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 567 Features Magnitude Axis of rotation Point Vector For 2-D axisymmetric simulations, a Rotational Velocity load can only be applied about the y-axis. Note While loads are associative with geometry changes, load directions are not. This applies to any load that requires a vector input, such as: moment, acceleration, rotational velocity, force, and bearing load. Pressure For 3-D simulations, a pressure load applies a constant pressure or a varying pressure in a single direction (x, y, or z) to one or more flat or curved faces. The following illustration applies to a constant pressure load: Uniform positive pressure Define the vector as one of the following: • the displacement constraint acting normal to the surface to which it is attached (essentially a frictionless support with a non-zero displacement) [Define By: Normal To] During a structural analysis, you can also create a spatially varying load using this vector type option. A spatially varying load allows you to define the pressure in tabular form or as a function. Applying a pressure load normal to faces (3-D) or edges (2-D) could result in a pressure load stiffness contribution that plays a significant role in a linear buckling analysis. This additional effect is computed during a buckling analysis using the pressure value in the static analysis at time = 0. Because of this, if you perform static analysis for a subsequent buckling analysis, you must apply pressure loads as a separate step in the static analysis. • 568 a magnitude and direction (based on selected geometry) [Define By: Vector] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions • components (in the world coordinate system or local coordinate system, if applied) [Define By: Components] Pressure is uniform and acts normal to a face at all locations on the face. A positive value for pressure acts into the face, compressing the solid body. If you select multiple faces when defining the pressure, the same pressure value gets applied to all selected faces. If a constant pressurized face enlarges due to a change in CAD parameters, the total load applied to the face increases, but the pressure (force per unit area) value remains constant. For 2-D simulations, a pressure load applies a pressure to one or more edges. Pipe Pressure For 3-D structural analyses, a pipe pressure load applies a constant, tabular, or functional variation of pressure to one or more line bodies which are set to be pipes. You can select it to be internal pipe pressure or external pipe pressure from the Details view. Internal and external pressures are input on an average basis over the element. By default, when the pipe is subjected to internal and external pressures, the end-cap pressure effect of the pipe is included. This implies that the end caps are always in equilibrium, that is, no net forces are produced. To apply a pipe pressure: 1. Right-click the environment folder and choose Insert> Pipe Pressure. 2. Select a line body, and then click Apply in the Details view. Pipe pressure can only be scoped to line bodies which are set to be pipes. 3. Define Magnitude as a constant, tabular, or functional input just like any other load. 4. Select Loading to be Internal or External according to your problem. Pipe Temperature For 3-D structural analyses, a pipe temperature load applies a constant, tabular, or functional variation of temperature to one or more line bodies which are set to be pipes. You can select it to be internal pipe temperature or external pipe temperature from the Details view. Pipe temperature loads are available only for static, modal, and full transient analyses. To apply a pipe temperature: 1. Right-click the environment folder and choose Insert> Pipe Temperature. 2. Select a line body, and then click Apply in the Details view. Pipe temperature can only be scoped to line bodies which are set to be pipes. 3. Define Magnitude as a constant, tabular, or functional input just like any other load. 4. Select Loading to be Internal or External according to your problem. Hydrostatic Pressure A hydrostatic pressure load simulates pressure that occurs due to fluid weight. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 569 Features Presented below is a typical procedure showing the use of a hydrostatic pressure load: 1. Define a Static Structural analysis system and import the fluid container model. 2. Double-click the Model cell to enter the Mechanical application, then insert a Hydrostatic Pressure load. 3. Scope all faces that will potentially enclose the fluid. 4. Specify the Shell Face, defined as the side of the shell on which to apply the hydrostatic pressure load. (The Shell Face option appears only for surface bodies.) 5. Specify the magnitude and direction of the Hydrostatic Acceleration. This is typically the acceleration due to gravity, but can be other acceleration values depending on the modeling scenario. For example, if you were modeling rocket fuel in a rocket’s fuel tank, the fuel might be undergoing a combination of acceleration due to gravity and acceleration due to the rocket accelerating while flying. 6. Enter the Fluid Density. 7. Specify the Free Fluid Location, defined as the location of the top of the fluid in the container. You can specify this location by using coordinate systems, by entering coordinate values, or by clicking a location on the model. 8. Mesh the model, then highlight the Hydrostatic Pressure load object to display the pressure contours. The following example shows the simulation of a hydrostatic pressure load on the wall of an aquarium. Here the wall is modeled as a single surface body. The load is scoped to the bottom side of the face. A fixed support is applied to the bottom edge. Acceleration due to gravity is used and the fluid density is entered as 1000 kg/m3. Coordinates representing the top of the fluid are also entered. Shown below is a load plot that clearly illustrates the hydrostatic pressure gradient. Force There are three types of forces: Face (p. 571) Edge (p. 571) Vertex (p. 572) 570 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Note Force loads are not supported for 2D axisymmetric Explicit Dynamics analyses. Face Distributes a force vector across one or more flat or curved faces. Force vector Resulting uniform traction across the face Define the vector in terms of either: • a magnitude and direction (based on selected geometry) [Define By: Vector] • components (in the world coordinate system or local coordinate system, if applied) [Define By: Components] The force is applied by converting it to a pressure, based on the total area of all the selected faces. If a face enlarges due to a change in CAD parameters, the total load magnitude applied to the face remains constant. If you try to apply a force to a multiple face selection that spans multiple parts, the face selection is ignored. The geometry property for the load object displays 'No Selection' if the load was just created, or it maintains its previous geometry selection if there was one. Edge Distributes a force vector along one or more straight or curved edges. Force vector Resulting uniform line load along the edge Define the vector in terms of either: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 571 Features • a magnitude and direction (based on selected geometry) [Define By: Vector] • components (in the world coordinate system or local coordinate system, if applied) [Define By: Components] If you select multiple edges when defining the force, the magnitude of the force is distributed evenly across all selected edges. If an edge enlarges due to a change in CAD parameters, the total load applied to the edge remains constant, but the line load (force per unit length) decreases. A force applied to an edge is not realistic and leads to singular stresses (that is, stresses that approach infinity near the loaded edge). You should disregard stress and elastic strain values in the vicinity of the loaded edge. If you try to apply a force to a multiple edge selection that spans multiple parts, the edge selection is ignored. The geometry property for the load object displays 'No Selection' if the load was just created, or it maintains its previous geometry selection if there was one. Vertex Applies a force vector to one or more vertices. Force vector Define the vector in terms of either: • a magnitude and direction (based on selected geometry) [Define By: Vector] • components (in the world coordinate system or local coordinate system, if applied) [Define By: Components] If you select multiple vertices when defining the force, the magnitude of the force is distributed evenly across all selected vertices. A force applied to a vertex is not realistic and leads to singular stresses (that is, stresses that approach infinity near the loaded vertex). You should disregard stress and elastic strain values in the vicinity of the loaded vertex. While loads are associative with geometry changes, load directions are not. This applies to any load that requires a vector input, such as: moment, acceleration, rotational velocity, force, and bearing load. If you try to apply a force to a multiple vertex selection that spans multiple parts, the vertex selection is ignored. The geometry property for the load object displays 'No Selection' if the load was just created, or it maintains its previous geometry selection if there was one. Remote Force A Remote Force is equivalent to a regular force load on a face or a force load on an edge, plus some moment. 572 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions A Remote Force can be used as an alternative to building a rigid part and applying a force load to it. The advantage of using a remote force load is that you can directly specify the location in space from which the force originates. You apply a Remote Force like you apply a force load except that the location of the load origin can be replaced anywhere in space either by picking or by entering the XYZ locations directly. The default location is at the centroid of the geometry. The location and the direction of a remote force can be defined in the global coordinate system or in a local coordinate system. A Remote Force can be applied to a face of a solid model, or to an edge or a face of a surface model. While loads are associative with geometry changes, load directions are not. This applies to any load that requires a vector input, such as: moment, acceleration, rotational velocity, force, and bearing load. A Remote Force is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 628) section for a listing of all remote boundary conditions and their characteristics. Note This boundary condition cannot be applied to a vertex scoped to an end release. Bearing Load Applies a variable distribution of force to one complete right cylinder in a 3-D simulation, or to a circular edge in a 2-D simulation. In a 3-D simulation, a complete right cylinder is capped on both ends by circles normal to the axis of the cylinder. Load direction Radial component distribution Region of loaded cylinder not affected by radial distribution Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 573 Features You must apply a Bearing load in the cylinder's radial direction using local coordinate systems. If the Mechanical application detects a portion of the load to be in the axial direction, the solver will block the solve and issue an appropriate error message. Define the vector in terms of either: • a magnitude and direction (based on selected geometry) [Define By: Vector] • components (in the world coordinate system or local coordinate system, if applied) [Define By: Components] If the loaded face enlarges (e.g., due to a change in parameters), the total load applied to the face remains constant, but the pressure (force per unit area) decreases. Note 574 • While loads are associative with geometry changes, load directions are not. This applies to any load that requires a vector input, such as: moment, acceleration, rotational velocity, force, and bearing load. • If your CAD system split the cylinder into two or more faces, select all of the faces when defining the bearing load. • Use one bearing load per cylinder. Do not use multiple select to apply a bearing load to different cylinders. If you do, the load is divided among the multiple cylindrical faces by area ratio, as shown in the following example of a single bearing load applied to two cylinders. The length of the cylinder on the right is twice the length of the cylinder on the left. Note that the reactions are proportional to each cylinder's area as a fraction of the total load area. • Although loading across multiple steps may appear as an application of tabular loading, you cannot set the magnitude of a bearing load in terms of either tabular or functional data. You must set a constant or ramped magnitude for each step such that one value corresponds to each step. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Bolt Pretension Available for 3-D simulations only. Applies a pretension load to a cylindrical face, to a straight edge of a line body, to a single body, or to multiple bodies, typically to model a bolt under pretension. If you apply the Bolt Pretension load to a body, you will need to have a local Coordinate System object in the tree. The application of the load will be at the origin and along the z-axis of the local coordinate system. You can place the coordinate system anywhere in the body and reorient the z-axis. Another option for applying the load to a line body is to apply it to a single straight edge on the body. The direction of the bolt load is inferred from the direction of the edge. Body scoping of a Bolt Pretension load can be to more than one body. In this case all the scoped bodies will be cut. There is still only a single Bolt Pretension load created but this feature allows you to apply a bolt load to a bolt that has been cut into several bodies. This feature is illustrated in the following figure. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 575 Features This load is applicable to pure structural or thermal-stress analyses. You specify how the Bolt Pretension load is applied by choosing one of the following options under the Define By setting in the Details view. • Load: Applies a force as a preload. A Load field is displayed where you enter the value of the load in force units. • Adjustment: Applies a length as a pre-adjustment (for example, to model x number of threads). An Adjustment field is displayed where you enter the value of the adjustment in length units. • Lock: Fixes all displacements. You can set this state for any step except the first step. • Open: Use this option to leave the Bolt Pretension load open so that the load has no effect on the applied step, effectively suppressing the load for the step. Note that in order to avoid convergence issues from having under-constrained conditions, a small load (0.01% of the maximum load across the steps) will be applied. You can set this state for any step. Presented below is the same model showing a Bolt Pretension load as a preload force and as a preadjustment length: The following animation shows total deformation: The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the help. Interface names and other components shown in the demo may differ from those in the released product. Limitations The following limitations apply to using Bolt Pretension loads: • If you try to apply a preload on the same face more than once, all definitions except the first one are ignored. 576 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions • Be sure that a sufficiently fine mesh exists on a face or body that contains Bolt Pretension loads so that the mesh can be correctly partitioned along the axial direction (that is, at least 2 elements long). • For simulating one Bolt Pretension through multiple split faces, you should apply only one Bolt Pretension load to one of the split faces, as the Bolt Pretension load will slice though the whole cylinder even though only part of the cylinder is selected. • Care should be used when applying a Bolt Pretension load to a cylindrical face that has bonded contact. There is a possibility that if you apply a Bolt Pretension load to a cylinder that had a bonded contact region, the bonded contact will block the ability of the Bolt Pretension to deform properly. • The Bolt Pretension load should be applied to cylindrical faces that contain the model volume (that is, do not try to apply the Bolt Pretension load to a hole). • Use caution when defining bolt loads by bodies and a coordinate system because the entire body is sliced along the local XY plane (Z=0). Moment Distributes a moment about an axis across one or more flat or curved faces, as illustrated below, or about one or more edges or vertices. Face and edge selections for the moment load can span multiple parts, however, multiple vertex selections must be of the same part type (solid, 3D surface or line bodies) or the selection is ignored. When specifying the Scoping Method, faces and edges can be scoped to either the geometry where the load is to be applied (Geometry Selection), to a Named Selection, or to a Remote Point. Vertices cannot be scoped to Remote Point. Load direction Moment load Affected face Define the moment vector in terms of either: • a magnitude and direction (based on selected geometry) [Define By: Vector] • components (in the world coordinate system or local coordinate system, if applied) [Define By: Components] The moment is applied "about" the vector. Use the right-hand rule to determine the sense of the moment. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 577 Features If you select multiple faces when defining the moment, the magnitude is apportioned across all selected faces. If a face enlarges (e.g., due to a change in parameters), the total load applied to the face remains constant, but the load per unit area decreases. Note • This boundary condition cannot be applied to a vertex scoped to an end release. • While loads are associative with geometry changes, load directions are not. This applies to any load that requires a vector input, such as: moment, acceleration, rotational velocity, force, and bearing load. A Moment is classified as a remote boundary condition. Refer to the Remote Boundary Conditions (p. 628) section for a listing of all remote boundary conditions and their characteristics. Generalized Plane Strain Used in 2-D applications involving generalized plane strain behavior. The Details view includes settings for controlling the items listed below. Refer to Using Generalized Plane Strain (p. 333) for detailed information on these settings and on the overall application of this load. • Setting the x and y coordinates of the reference (starting) point. • Establishing the magnitude and boundary conditions of the fiber direction. Choices for the boundary condition are: • – Free – Force – Displacement Establishing the boundary conditions for rotation about the x-axis and the y-axis. Choices for the boundary conditions are: – Free – Moment – Rotation Specific reactions are also reported in the Details view of a Generalized Plane Strain probe after solving. Line Pressure For 3-D simulations, a line pressure load applies a distributed force on one edge only, using force density loading in units of force per length. You can define the force density on the selected edge in various ways. 578 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Define the load in terms of one of the following: • a magnitude and direction (based on selected geometry) [Define By: Vector] • components (in the world coordinate system or local coordinate system, if applied for both Cartesian and cylindrical coordinate systems) [Define By: Components] • a magnitude and tangent. You can also apply time and spatially varying loads. [Define By: Tangential] If a pressurized edge enlarges due to a change in CAD parameters, the total load applied to the edge increases, but the pressure (force per unit length) remains constant. PSD Base Excitation PSD Base Excitation loads are used exclusively in random vibration analyses to provide excitation in terms of spectral value vs. frequency to your choice of the supports that were applied in the prerequisite modal analysis. The Boundary Condition setting in the Details view includes a drop down list where you can specify any of the following supports for excitation that are defined in the modal analysis: Fixed Support, Displacement, Remote Displacement, and Body-to-Ground Spring. If multiple fixed supports or multiple remote displacements are defined in the modal analysis, you can apply the excitation load to all fixed supports or all remote displacements or all of both loads using one of the following options: • All Fixed Supports • All Remote Displacements • All Supports Note Only fixed degrees of freedom of the supports are valid for excitations. You can also specify the excitation direction (X Axis, Y Axis, or Z Axis). The user-defined PSD data table is created in the Tabular Data window. You can create a new PSD table or import one from a library that you have created, via the fly-out of the Load Data option in the Details view. Note Only positive table values can be input when defining this load. When creating PSD loads for a Random Vibration analysis in the Mechanical application, Workbench evaluates your entries by performing a "Goodness of Fit" to ensure that your results will be dependable. Click the fly-out of the Load Data option and choose Improved Fit after entering data points for viewing the graph and updating the table. Interpolated points are displayed if they are available from the goodness of fit approximation. Once load entries are entered, the table provides one of the following color-code indicators per segment: • Green - Values are considered reliable and accurate. • Yellow - This is a warming indicator. Results produced are not considered to be reliable and accurate. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 579 Features • Red - Results produced are not considered trustworthy. If you choose to solve the analysis, the Mechanical APDL application executes the action, however; the results are almost certainly incorrect. It is recommended that you modify your input PSD loads prior to the solution process. Four types of base excitation are supported: • PSD Acceleration • PSD G Acceleration • PSD Velocity • PSD Displacement The direction of the PSD base excitation is defined in the nodal coordinate of the excitation points. Multiple PSD excitations (uncorrelated) can be applied. Typical usage is to apply 3 different PSDs in the X, Y, and Z directions. Correlation between PSD excitations is not supported. RS Base Excitation RS Base Excitation loads are used exclusively in response spectrum analyses to provide excitation in terms of a spectrum. For each spectrum value, there is one corresponding frequency. Use the Boundary Condition setting in the Details view to apply an excitation to all of the fixed supports that were applied in the prerequisite modal analysis. Note Only fixed DOFs of the supports are valid for excitations. You can also specify the excitation in a given direction (X Axis, Y Axis, or Z Axis). The user-defined RS data table is created in the Tabular Data window. You can create a new RS table or import one from a library that you have created, via the fly-out of the Load Data option in the Details view. Note Only positive table values can be used when defining this load. Three types of base excitation are supported: • RS Acceleration • RS Velocity • RS Displacement You should specify the direction of the RS base excitation in the global Cartesian system. Multiple RS excitations (uncorrelated) can be applied. Typical usage is to apply 3 different RS excitations in the X, Y, and Z directions. Correlation between RS excitations is not supported. The following additional settings are included in the Details view of an RS Base Excitation load: 580 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions • Scale Factor: Scales the entire table of input excitation spectrum for a Single Point response spectrum. The factor must be greater than 0.0. The default is 1.0. • Missing Mass Effect: Set to Yes to include the contribution of high frequency modes in the total response calculation. Including these modes is normally required for nuclear power plant design. The responses contributed by frequency modes higher than those of rigid responses, specifically frequency modes beyond Zero Period Acceleration (ZPA) are called residual rigid responses. The frequency modes beyond ZPA are defined as frequency modes at which the spectral acceleration returns to the Zero Period Acceleration. In some applications, especially in the nuclear power plant industry, it is critical and required to include the residual rigid responses to the total responses. Ignoring the residual rigid responses will result in an underestimation of responses in the vicinity of supports. There are two methods available to calculate residual rigid responses: the Missing Mass and Static ZPA methods. The Missing Mass method is named based on the fact that the mass associated with the frequency modes higher than that of ZPA are missing from the analysis. As a result, the residual rigid responses are sometimes referred to missing mass responses. When set to Yes, the Missing Mass Effect is used in a response spectrum analysis. • Rigid Response Effect: Set to Yes to include rigid responses to the total response calculation. Rigid responses normally occur in the frequency range that is lower than that of missing mass responses, but higher than that of periodic responses. In many cases, it is impractical and difficult to accurately calculate all natural frequencies and mode shapes for use in the response spectrum evaluation. For high-frequency modes, rigid responses basically predominate. To compensate for the contribution of higher modes to the responses, the rigid responses are combined algebraically to the periodic responses, which occur in the low-frequency modes that are calculated using one the methods above. The most widely adopted methods to calculate the rigid responses are the Gupta and Lindley-Yow methods. These two methods are available for a response spectrum analysis under Rigid Response Effect Type when Rigid Response Effect is set to Yes. Joint Load When you are using joints in a Transient Structural or Rigid Dynamics analysis, you use a Joint Load object to apply a kinematic driving condition to a single degree of freedom on a Joint object. Joint Load objects are applicable to all joint types except fixed, general, universal, and spherical joints. For translation degrees of freedom, the Joint Load can apply a displacement, velocity, acceleration, or force. For rotation degrees of freedom, the Joint Load can apply a rotation, angular velocity, angular acceleration, or moment. The directions of the degrees of freedom are based on the reference coordinate system of the joint and not on the mobile coordinate system. A positive joint load will tend to cause the mobile body to move in the positive degree of freedom direction with respect to the reference body, assuming the mobile body is free to move. If the mobile body is not free to move then the reference body will tend to move in the negative degree of freedom direction for the Joint Load. One way to learn how the mechanism will behave is to use the Configure feature. For the joint with the applied Joint Load, dragging the mouse will indicate the nature of the reference/mobile definition in terms of positive and negative motion. To apply a Joint Load: 1. Highlight the Transient environment object and insert a Joint Load from the right mouse button context menu or from the Loads drop down menu in the Environment toolbar. 2. From the Joint drop down list in the Details view of the Joint Load, select the particular Joint object that you would like to apply to the Joint Load. You should apply a Joint Load to the mobile bodies Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 581 Features of the joint. It is therefore important to carefully select the reference and mobile bodies while defining the joint. 3. Select the unconstrained degree of freedom for applying the Joint Load, based on the type of joint. You make this selection from the DOF drop down list. For joint types that allow multiple unconstrained degrees of freedom, a separate Joint Load is necessary to drive each one. Further limitations apply as outlined under Joint Load Limitations (p. 582) below. Joint Load objects that include velocity, acceleration, rotational velocity or rotational acceleration are not applicable to static structural analyses. 4. Select the type of Joint Load from the Type drop down list. The list is filtered with choices of Displacement, Velocity, Acceleration, and Force if you selected a translational DOF in step 3. The choices are Rotation, Rotational Velocity, Rotational Acceleration, and Moment if you selected a rotational DOF. 5. Specify the magnitude of the Joint Load type selected in step 4 as a constant, in tabular format, or as a function of time using the same procedure as is done for most loads in the Mechanical application. Refer to Specifying Load Values (p. 621) for further information. On Windows platforms, an alternative and more convenient way to accomplish steps 1 and 2 above is to drag and drop the Joint object of interest from under the Connections object folder to the Transient object folder. When you highlight the new Joint Load object, the Joint field is already completed and you can continue at step 3 with DOF selection. 6. As applicable, specify the load step at which you want to lock the joint load by entering the value of the step in the Lock at Load Step field. The default value for this option is zero (0) and is displayed as Never. This feature immobilizes movement of the joint’s DOFs. For example, this option is beneficial when you want to tighten a bolt to an initial torque value (via a Moment Joint Driver on a Revolute Joint) and then lock that joint during a subsequent load step. Note MAPDL References: This feature makes use of the %_FIX% parameter on the DJ command. When a joint driver with a force or moment load is deactivated, then the lock constraint on the joint is also deleted using the DJDELE command. This happens if the locking occurs before the deactivation. Joint Load Limitations Some joint types have limitations on the unconstrained degrees of freedom that allow the application of joint loads as illustrated in the following table: Joint Type Unconstrained Degrees of Freedom Allowable Degrees of Freedom for Applying Joint Loads Fixed None Not applicable Revolute ROTZ ROTZ Cylindrical UZ, ROTZ UZ, ROTZ Translational UX UX Slot UX, ROTX, ROTY, ROTZ UX Universal ROTX, ROTZ None 582 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Joint Type Unconstrained Degrees of Freedom Allowable Degrees of Freedom for Applying Joint Loads Spherical ROTX, ROTY, ROTZ None Planar UX, UY, ROTZ UX, UY, ROTZ General UX, UY and UZ, Free X, Free Y, Free Z, and Free All All unconstrained degrees of freedom Bushing UX, UY, UZ, ROTX, ROTY, ROTZ All unconstrained degrees of freedom Note Where applicable, you must define all three rotations for a Joint Load before proceeding to a solve. Thermal Condition You can insert a known temperature (not from data transfer) boundary condition in a Structural or Electric analysis by inserting a Thermal Condition object and specifying the value of the temperature in the Details view under the Magnitude property. If the load is applied to a surface body, by default the temperature is applied to both the top and bottom surface body faces. You do have the option to apply different temperatures to the top and bottom faces by adjusting the Shell Face entry in the details view. When you apply a thermal condition load to a solid body, the Shell Face property is not available in the Details view. You can add the thermal condition load as time-dependent or spatially varying. To apply a thermal condition: 1. In the Project tree, right-click the environment folder, point to Insert, and then click Thermal Condition. 2. Select a surface body face, a solid body or a line body, and then click Apply in the Details view. 3. For surface bodies, in the Details view, click the Shell Face list, and then select Top, Bottom, or Both (Default) to apply the thermal condition to the selected face. For bodies that have one or more layered section objects, you need to specify Both for Shell face or the Thermal Condition will be under-defined and an error message will be generated. Note • When you have only one Thermal Condition load and you select only a top or bottom face, Workbench applies the environment temperature value to the opposite face unless it is otherwise specified from another load object. • For an assembly of bodies with different topologies, you must define a separate Thermal Condition load for each topology, that is, you must define one load scoped to line bodies, define a second load scoped to surface bodies, and so on. • For each load step, if an Imported Body temperature load and a Thermal Condition load are applied on common geometry selections, the Imported Body temperature load takes precedence. See Activation/Deactivation of Loads (p. 531) for additional rules when multiple load objects of the same type exist on common geometry selections. • If the Thermal Condition is applied to a shell face that has a Layered Section applied to it, you must set Shell Face to Both in order to solve the analysis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 583 Features Temperature Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only. You can apply a temperature load to one or more faces, edges, or vertices, as well as to an entire body. When scoping a load to a body, you need to specify whether the temperature is applied to Exterior Faces Only or to the Entire Body using the Apply To option. The same temperature value is applied when multiple faces, edges, or vertices are selected. You can also define a temperature load as a spatially varying load during a thermal analysis. A spatially varying load allows you to vary the magnitude of a temperature in a single coordinate direction and as a function of time using the Tabular Data or Function features. Please see the Specifying Load Values (p. 621) section for the specific steps to apply tabular and/or function loads. The following illustrate geometry selection for the temperature load. Curved Surface Edge Vertex Note For each load step, if an Imported Temperature load and a Temperature load are applied on common geometry selections, the Imported Temperature load takes precedence. See Activation/Deactivation of Loads (p. 531) for additional rules when multiple load objects of the same type exist on common geometry selections. Temperature Convection Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only. Causes convective heat transfer to occur through one or more flat or curved faces (in contact with a fluid). Ambient fluid temperature. Film coefficient and Face Temperature. 584 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions The bulk fluid temperature is measured at a distance from the face outside of the thermal boundary layer. The face temperature refers to the temperature at the face of the simulation model. You can define a convection load as a spatially varying load during a thermal analysis. A spatially varying load allows you to vary the magnitude of film coefficient and ambient temperature in a single coordinate direction and as a function of time using the Tabular Data or Function features. Please see the Specifying Load Values (p. 621) section for the specific steps to apply tabular and/or function loads. Note Normalized S and scaling based on time are not supported for convection. Film Coefficient The film coefficient (also called the heat transfer coefficient or unit thermal conductance) is based on the composition of the fluid in contact with the face, the geometry of the face, and the hydrodynamics of the fluid flow past the face. It is possible to have a time, temperature or spatially dependent film coefficient. Refer to heat transfer handbooks or other references to obtain appropriate values for film coefficient. Coefficient Type This field is available when the film coefficient is temperature dependent. Its value can be evaluated at the average film temperature (average of surface and bulk temperatures), the surface temperature, the bulk temperature, or the absolute value of the difference between surface and bulk temperatures. Note If you change the units from Celsius to Fahrenheit, or Fahrenheit to Celsius, when the convection coefficient type Difference between surface and bulk is in use, the displayed temperature values indicate a temperature difference only. The addition or subtraction of 32o for each temperature in the conversion formula offset one another. In addition, switching to or from the Difference between surface and bulk Coefficient Type option from any other option, clears the values in the Convection Coefficient table. This helps to ensure that you enter correct temperature values. Ambient Temperature The ambient temperature is the temperature of the surrounding fluid. It is possible to have a time or spatially dependent ambient temperature. Edit Data For This field allows you to select and edit film coefficient or ambient temperature. The tabular data, details view, graph and graphics view will change based on the selection in the Edit Data For field. For example, when film coefficient is tabular/function and Edit Data For is film coefficient, you will actively edit data for the film coefficient in the appropriate details view and tabular data fields. Convective Heat Transfer Convection is related to heat flux by use of Newton's law of cooling: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 585 Features q/A = h(ts - tf) where • q/A is heat flux out of the face (calculated within the application) • h is the film coefficient (you provide) • ts is the temperature on the face (calculated within the application) • tf is the bulk fluid temperature (you provide) When the fluid temperature exceeds face temperature, energy flows into a part. When the face temperature exceeds the fluid temperature, a part loses energy. If you select multiple faces when defining convection, the same bulk fluid temperature and film coefficient is applied to all selected faces. Radiation Applies thermal radiation to a surface of a model. You can define the exchange of radiation between a body and the ambient temperature, or between two surfaces. Ambient Temperature Radiation With Correlation = To Ambient in the Details view of a Radiation object, the radiation energy is exchanged with the ambient temperature, that is, the Form Factor1 is assumed to be 1.0. You can set the following additional radiation properties in the Details view: • Emissivity: The ratio of the radiation emitted by a surface to the radiation emitted by a black body at the same temperature. • Ambient Temperature: The temperature of the surrounding space. Note 1 Radiation exchange between surfaces is restricted to gray-diffuse surfaces. Gray implies that emissivity and absorptivity of the surface do not depend on wavelength (either can depend on temperature). Diffuse signifies that emissivity and absorptivity do not depend on direction. For a gray-diffuse surface, emissivity = absorptivity; and emissivity + reflectivity = 1. Note that a black body surface has a unit emissivity. Surface to Surface Radiation With Correlation = Surface to Surface in the Details view of a Radiation object, the radiation energy is exchanged between two surfaces. In this context, “surface” refers to a face of a shell or solid body in a 3-D model, or an edge in a 2-D model. You can specify both Emissivity and Ambient Temperature (defined above) in the Details view. Emissivity must be a positive value that is not greater than 1. The capability is also included for entering temperature dependent Emissivity in the Tabular Data window. Additionally, you can specify an Enclosure number. You should assign the same Enclosure number to surfaces radiating to each other.1 You cannot apply a Surface to Surface Radiation load to a geometric entity that is already attached to another Radiation load. 586 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions When using the Surface to Surface correlation with shell bodies, the Details view also includes a Shell Face setting that allows you the choice of applying the load to Both faces, to the Top face only, or to the Bottom face only. For thermal related analyses that use the ANSYS solver, the actual calculation of the radiation exchange between two surfaces is performed using the Radiosity Solver method. The Radiosity Solver method accounts for the heat exchange between radiating bodies by solving for the outgoing radiative flux for each surface, when the surface temperatures for all surfaces are known. The surface fluxes provide boundary conditions to the finite element model for the conduction process analysis in Workbench. When new surface temperatures are computed, due to either a new time step or iteration cycle, new surface flux conditions are found by repeating the process. The surface temperatures used in the computation must be uniform over each surface facet to satisfy the conditions of the radiation model. For models that are entirely symmetrical, you can account for symmetry using Symmetry Regions or Cyclic Regions. The Radiosity Solver method respects plane or cyclic symmetries. Using a model's symmetry can significantly reduce the size of the model. The Radiosity Solver method will take symmetry into account and the Radiation Probe solution results will be valid for the full model. Settings for the Radiosity Solver method are available under the Analysis Settings object in the Radiosity Controls category. Related References See the sections of the Mechanical APDL help listed below for further information related to using the Radiation load in thermal related analyses that employ the ANSYS solver. These help sections mention the underlying commands and elements used for implementation of the feature in the Mechanical APDL application. They are presented for reference only. To implement the feature in the Mechanical application, you do not need to interact directly with these commands and elements. • • Thermal Analysis Guide: – 1 - Definitions – Using the Radiosity Solver Method Mechanical APDL Theory Reference: – Radiation – Radiosity Solution Method Heat Flow Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only. There are three types of Heat Flow Rates: Face Heat Flow Rate (p. 587) Edge Heat Flow Rate (p. 588) Vertex Heat Flow Rate (p. 588) Face Heat Flow Rate Specifies the rate of heat flow through one or more flat or curved faces. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 587 Features Positive heat flow A positive heat flow acts into a face, adding energy to a body. Heat flow is defined as energy per unit time. If you select multiple faces when defining the heat flow rate, the magnitude is apportioned across all selected faces. If a face enlarges due to a change in CAD parameters, the total load applied to the face remains constant, but the heat flux (heat flow rate per unit area) decreases. If you try to apply a heat flow to a multiple face selection that spans multiple bodies, the face selection is ignored. The geometry property for the load object displays No Selection if the load was just created, or it maintains its previous geometry selection if there was one. Edge Heat Flow Rate Specifies the rate of heat flow through one or more straight or curved edges. Positive heat flow A positive heat flow acts into an edge, adding energy to a body. Heat flow is defined as energy per unit time. If you select multiple edges when defining the heat flow rate, the magnitude is apportioned across all selected edges. If an edge enlarges due to a change in CAD parameters, the total load applied to the edge remains constant, but the line load (heat flow rate per unit length) decreases. If you try to apply a heat flow to a multiple edge selection that spans multiple bodies, the edge selection is ignored. The geometry property for the load object displays No Selection if the load was just created, or it maintains its previous geometry selection if there was one. Vertex Heat Flow Rate Specifies the rate of heat flow through one or more vertices. 588 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Positive heat flow A positive heat flow acts into a vertex, adding energy to the body. Heat flow is defined as energy per unit time. If you select multiple vertices when defining the heat flow rate, the magnitude is apportioned among all selected vertices. If you try to apply a heat flow to a multiple vertex selection that spans multiple bodies, the vertex selection is ignored. The geometry property for the load object displays No Selection if the load was just created, or it maintains its previous geometry selection if there was one. Perfectly Insulated Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only. Overrides or applies a "no load" insulated condition to a face. An insulated face is a no load condition meant to override any thermal loads scoped to a body. The heat flow rate is 0 across this face. This load is useful in a case where most of a model is exposed to a given condition (such a free air convection) and only a couple of faces do not share this condition (such as the base of a cup that is grounded). This load will override only thermal loads scoped to a body. See Resolving Thermal Boundary Condition Conflicts for a discussion on thermal load precedence. If you select multiple faces when defining an insulated face, all selected faces will be insulated. Heat Flux Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only. Applies a uniform heat flux to one or more flat or curved faces. Uniform positive heat flux A positive heat flux acts into a face, adding energy to a body. Heat flux is defined as energy per unit time per unit area. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 589 Features If you select multiple faces when defining the heat flux, the same value gets applied to all selected faces. If a face enlarges due to a change in CAD parameters, the total load applied to the face increases, but the heat flux remains constant. Internal Heat Generation Available for 3-D simulations, and 2-D simulations for Plane Stress and Axisymmetric behaviors only. Applies a uniform generation rate internal to a body. A positive heat generation acts into a body, adding energy to it. Heat generation is defined as energy per unit time per unit volume. If you select multiple bodies when defining the heat generation, the same value gets applied to all selected bodies. If a body enlarges due to a change in CAD parameters, the total load applied to the body increases, but the heat generation remains constant. Note For each load step, if an Imported Body temperature load and a Thermal Condition load are applied on common geometry selections, the Imported Body temperature load takes precedence. See Activation/Deactivation of Loads (p. 531) for additional rules when multiple load objects of the same type exist on common geometry selections. Voltage Applies an electric potential to a body during an electric analysis, a thermal-electric analysis, or a magnetostatic analysis. For each analysis type, you define the voltage by magnitude and phase angle in the Details view, according to the following equation. V = Vocos(ωt+φ) Vo is the magnitude of the voltage (input value Voltage), ω is the frequency, and φ is the phase angle. For a static analysis, ωt = 0. The voltage load can be defined as a constant, in tabular form, or as a mathematical function. Electric and Thermal-Electric Analysis Requirements During an Electric / Thermal-Electric Analysis, a voltage is applied to a face, edge, or vertex. To apply a voltage load to a body, select Voltage from the Environment toolbar or right-click the mouse on the environment object in the tree and select Insert>Voltage. 590 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Caution During an Electric / Thermal-Electric Analysis, voltage loads cannot be applied to a face, edge, or vertex that is shared with another voltage or current load or a Coupling. Magnetostatic Analysis Requirements See Voltage Excitation for Solid Source Conductors (p. 596). Current Applies an electric current to a body during an electric analysis, a thermal-electric analysis, or a magnetostatic analysis. For each analysis type, you define the current by magnitude and phase angle in the Details view, according to the following equation. I = Iocos(ωt+φ) Io is the magnitude of the current (input value Current), ω is the frequency, and φ is the phase angle. For a static analysis, ωt = 0. The current load is defined as a constant, or in tabular form, or as a mathematical function. For electric, thermal-electric, and magnetostatic analyses, current loads assume that the scoped entities are equipotential, meaning they behave as electrodes where the voltage degrees of freedom are coupled and solve for a constant potential. Electric and Thermal-Electric Analysis Requirements During an Electric / Thermal Analysis, a current is applied to a face, edge, or vertex of a body. It is assumed that the material properties of the body provide conductance. An applied current assumes that the body surfaces and edges are equipotential. A positive current applied to a face, edge, or vertex flows into the body. A negative current flows out of the body. To apply a current load to a body for an Electric / Thermal Analysis, select Current from the Environment toolbar or right-click the mouse on the environment object in the tree and select Insert> Current. Caution Current loads cannot be applied to a face, edge, or vertex that is shared with another voltage or current load or a Coupling. Magnetostatic Analysis Requirements See Current Excitation for Solid Source Conductors (p. 597). Electromagnetic Boundary Conditions and Excitations You can apply electromagnetic excitations and boundary conditions when performing a Magnetostatic analysis in the Mechanical application. A boundary condition is considered to be a constraint on the field domain. An excitation is considered to be a non-zero boundary condition which causes an electric Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 591 Features or magnetic excitation to the system. Boundary conditions are applied to the field domain at exterior faces. Excitations are applied to conductors. • Magnetic Flux Boundary Conditions (p. 592) • Conductor (p. 593) – Solid Source Conductor Body (p. 594) → Voltage Excitation for Solid Source Conductors (p. 596) → Current Excitation for Solid Source Conductors (p. 597) – Stranded Source Conductor Body (p. 598) → Current Excitation for Stranded Source Conductors (p. 599) Magnetic Flux Boundary Conditions Available for 3-D simulations only. Magnetic flux boundary conditions impose constraints on the direction of the magnetic flux on a model boundary. This boundary condition may only be applied to faces. By default, this feature constrains the flux to be normal to all exterior faces. Selecting Flux Parallel forces the magnetic flux in a model to flow parallel to the selected face. In the figure below, the arrows indicate the direction of the magnetic flux. It can be seen that the flux flows parallel to the xy plane (for any z coordinate). A flux parallel condition is required on at least one face of the simulation model. It is typically applied on the outer faces of the air body to contain the magnetic flux inside the simulation domain or on symmetry plane faces where the flux is known to flow parallel to the face. To set this feature, right-click on the Magnetostatic environment item in the tree and select Magnetic Flux Parallel from the Insert context menu or click on the Magnetic Flux Parallel button in the toolbar. It can only be applied to geometry faces and Named Selections (faces). 592 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Half-symmetry model of a keepered magnet system. Note that the XY-plane is a Flux Parallel boundary. The flux arrows flow parallel to the plane. Half-symmetry model of a keepered magnet system. Note that the YZ-plane is a Flux Normal boundary. The flux arrows flow normal to the plane. This is a natural boundary condition and requires no specification. Note Applying the flux parallel boundary conditions to the exterior faces of the air domain may artificially capture more flux in the simulation domain than what physically occurs. This is because the simulation model truncates the open air domain. To minimize the effect, ensure the air domain extends far enough away from the physical structure. Alternatively, the exterior faces of the air domain may be left with an unspecified face boundary condition. An unspecified exposed exterior face imposes a condition whereby the flux flows normal to the face. Keep in mind that at least one face in the model must have a flux parallel boundary condition. Conductor Available for 3-D simulations only. A conductor body is characterized as a body that can carry current and possible excitation to the system. Solid CAD geometry is used to model both solid source conductors and stranded source conductors. In solid conductors, such as bus bars, rotor cages, etc., the current can distribute non-uniformly due to Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 593 Features geometry changes, hence the program performs a simulation that solves for the currents in the solid conductor prior to computing the magnetic field. Stranded source conductors can be used to represent wound coils. Wound coils are used most often as sources of current excitation for rotating machines, actuators, sensors, etc. You may directly define a current for each stranded source conductor body. • Solid Source Conductor Body (p. 594) • Stranded Source Conductor Body (p. 598) Solid Source Conductor Body This feature allows you to tag a solid body as a solid source conductor for modeling bus bars, rotor cages, etc. When assigned as a solid source conductor, additional options are exposed for applying electrical boundary conditions and excitations to the conductor. These include applying an electrical potential (voltage) or current. To set this condition, right-click the Magnetostatic environment object in the tree and select Source Conductor from the Insert drop-down menu, or click on the Source Conductor button in the toolbar. Select the body you want to designate as a conductor body, then use the Details view to scope the body to the conductor and set Conductor Type to Solid. The default Number of Turns is 1, representing a true solid conductor. A solid source conductor can be used to represent a stranded coil by setting the Number of Turns to > 1. The conductor still computes a current distribution according to the physics of a solid conductor, but in many cases the resulting current density distribution will not significantly effect the computed magnetic field results. This “shortcut” to modeling a stranded conductor allows you to circumvent the geometry restrictions imposed by the stranded conductor bodies and still obtain acceptable results. After defining the conductor body, you may apply voltage and current conditions to arrive at the desired state. 594 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Note Conductors require two material properties: relative permeability and resistivity. They also must not terminate interior to the model with boundary conditions that would allow current to enter or exit the conductor. Termination points of a conductor may only exist on a plane of symmetry. Only bodies can be scoped to a conductor. Solid conductor bodies must have at least one voltage excitation and either a second voltage excitation or a current excitation. Also, two solid conductor bodies may not 'touch' each other, i.e. they must not share vertices, edges, or faces. To establish current in the conductor, you must apply excitation to at least two locations on the conductor, typically at terminals. For example, you could • apply a voltage drop at two terminals of a conductor body residing at symmetry planes. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 595 Features • ground one end of a conductor (set voltage to zero) and apply the net current at the terminal's other end. Voltage Excitation for Solid Source Conductors This feature allows you to apply an electric potential (voltage) to a solid source conductor body. A voltage excitation is required on a conductor body to establish a ground potential. You may also apply one to apply a non-zero voltage excitation at another location to initiate current flow. Voltage excitations may only be applied to faces of the solid source conductor body and can be defined as constant or time-varying. To apply a voltage excitation to a solid source conductor body, right-click on the Conductor object under the Magnetostatic environment object in the tree whose Conductor Type is set to Solid, and select Voltage from the Insert drop-down menu, or click on the Voltage button in the toolbar. You define the voltage by magnitude and phase angle in the Details view, according to the equation below. V = Vocos(ωt+φ) Vo is the magnitude of the voltage (input value Voltage), ω is the frequency, and φ is the phase angle. For a static analysis, ωt = 0. Note Voltage excitations may only be applied to solid source conductor bodies and at symmetry planes. 596 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions An applied voltage drop across the terminals of a conductor body will induce a current. In this simple example, the current in the conductor is related to the applied voltage drop, using the equations shown below. ∆V = applied voltage drop, I = current, ρ = resistivity of the conductor (material property), L = length of the conductor, and Area = cross section area of the conductor. ∆V = IR R = (ρ*L)/Area Current Excitation for Solid Source Conductors This feature allows you to apply a current to a solid source conductor or stranded source conductor body. Use this feature when you know the amount of current in the conductor. To apply a current excitation to a conductor body, right-click on the Conductor object under the Magnetostatic environment object in the tree whose Conductor Type is set to Solid, and select Current from the Insert drop-down menu, or click on the Current button in the toolbar. A positive current applied to a face flows into the conductor body. A negative current applied to a face flows out of the conductor body. For a stranded source conductor, positive current is determined by the y-direction of a local coordinate system assigned to each solid body segment that comprises the conductor. You define the current by magnitude and phase angle in the Details view, according to the equation below. I = Iocos(ωt+φ) Io is the magnitude of the current (input value Current), ω is the frequency, and φ is the phase angle. For a static analysis, ωt = 0. Note Current excitations may only be applied to a face of a solid source conductor body at symmetry planes. An excitation must be accompanied by a ground potential set at another termination point of the conductor body on another symmetry plane. No current may be applied to a conductor body face that is interior to the model domain. The symmetry plane on which the current excitation is applied must also have a magnetic flux-parallel boundary condition. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 597 Features An applied current to a conductor face will calculate and distribute the current within the conductor body. A ground potential (voltage = 0) must be applied to a termination point of the conductor body. Both the applied current and voltage constraints must be applied at a symmetry plane. Stranded Source Conductor Body This feature allows you to tag solid multiple bodies as a stranded source conductor for modeling wound coils. When assigned as a stranded source conductor, additional options are exposed for applying electric boundary conditions and current excitation to the conductor. Model a stranded source conductor using only isotropic materials and multiple solid bodies. Local coordinate systems assigned to these bodies (via the Details view) are the basis for determining the direction of the current that you later apply to a stranded source conductor. The model should include a separate solid body to represent each directional “turn” of the conductor. Assign a local coordinate system to each body with the positive current direction as the y-direction for each of the local coordinate systems. An illustration is shown below. 598 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions After creating the body segments and assigning coordinate systems, right-click the Magnetostatic environment object in the tree and select Source Conductor from the Insert drop-down menu, or click on the Source Conductor button in the toolbar. Select all body segments, then scope the bodies to the conductor and, in the Details view, set Conductor Type to Stranded, then enter the Number of Turns and the Conducting Area (cross section area of conductor). The stranded conductor is now ready for you to apply a current. A step-by-step example is presented in the Current Excitation for Stranded Source Conductors (p. 599) section. Note Conductors require two material properties: relative permeability and resistivity. They also must not terminate interior to the model with boundary conditions that would allow current to enter or exit the conductor. Termination points of a conductor may only exist on a plane of symmetry. Current Excitation for Stranded Source Conductors Stranded source conductor bodies are applicable to any magnetic field problem where the source of excitation comes from a coil. The coil must have a defined number of coil "turns." Stranded source body geometry is limited to straight geometry or circular arc geometry sections with constant cross-section (see below) Source loading for a coil is by a defined current (per turn) and a phase angle according to the equation below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 599 Features = o ω +φ Io is the magnitude of the current (input value Current), ω is the frequency, and φ is the phase angle. For a static analysis, ωt = 0. The direction of the current is determined by the local coordinate systems you assign to each of the solid bodies that comprise the stranded source conductor. A positive or negative assigned value of current will be respective to that orientation. Use the following overall procedure to set up a Stranded Source Conductor and apply a current to the conductor: 1. Define local coordinate systems that have the y-direction point in the direction of positive current flow. • Use Cartesian coordinate systems for straight geometry sections and cylindrical coordinate systems for “arc” geometry sections. 2. Assign a local coordinate system to each stranded source conductor body in the Details view of the body under the Geometry folder. 3. Right-click on the Magnetostatic environment object in the tree and select Source Conductor from the Insert drop down menu, or click on the Source Conductor button in the toolbar. 600 • Scope the Source Conductor to all of the solid bodies. • Set Conductor Type to Stranded. • Enter the Number of Turns and Conducting Area for the conductor. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions For the Conducting Area, select a face that represents the conductor's cross-sectional area and read the surface area that displays in the Status Bar located at the bottom of the screen display. The Source Conductor graphic and Details view listing is shown below. 4. Right-click on the Conductor object in the tree and select Current from the Insert drop down menu, or click on the Current button in the toolbar. • Set Magnitude as constant or time-varying. • Set Phase Angle. The Current automatically is scoped to the same bodies as the Source Conductor. The displayed current arrows give you visual validation that the current direction has been properly defined by the assigned local coordinate systems for each conductor body. Changing either the Type of Source Conductor or any coordinate system will invalidate the setup. Imported Body Force Density When electromagnetic body forces are transferred to a structural environment, an Imported Body Force Density object can be inserted to represent the transfer. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 601 Features Please see the Imported Loads (p. 630) section for applicable transfers or for specific steps to transfer data. Note For a particular load step, an active Imported Body Force Density load will overwrite other Imported Body Force Density loads that exist higher (previously added) in the tree, on common geometry selections. See Activation/Deactivation of Loads (p. 531) for additional rules when multiple load objects of the same type exist on common geometry selections. Note For large-deflection analyses, the loads are applied to the initial size of the element, not the current size. Imported Body Temperature When temperatures are transferred to a structural or electric analysis, an Imported Body Temperature object is automatically inserted to represent the transfer. If the load is applied to one or more surface bodies, the Shell Face option in the details view enables you to apply the temperatures to Both faces, to the Top face(s) only, or to the Bottom face(s) only. By default, the temperatures are applied to both the top and bottom faces of the selection. Please see the Imported Loads (p. 630) section for applicable transfers or for specific steps to transfer data. 602 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Note • Adaptive Convergence objects inserted under an environment that is referenced by an Imported Body Temperature object will invalidate the Imported Body Temperature object, and not allow a solution to progress. • For a particular load step, an active Imported Body Temperature load will overwrite any Thermal Condition loads on common geometry selections. • If the temperatures are only applied to the top or bottom face of a surface body, Workbench applies the environment temperature value to the opposite face, unless it is otherwise specified from another load object. • For an assembly of bodies with different topologies, you must define a separate Imported Body Temperature load for surface bodies. • The values used in the solution are calculated by first converting the imported load values into the solver unit system and then multiplying the scale value. • For each load step, if an Imported Body Temperature load and a Thermal Condition load are applied on common geometry selections, the Imported Body Temperature load takes precedence. An active Imported Body Temperature load will also overwrite other Imported Body Temperature loads that exist higher (previously added) in the tree, on common geometry selections. See Activation/Deactivation of Loads (p. 531) for additional rules when multiple load objects of the same type exist on common geometry selections. • If a scale factor is specified, the values used in the solution are calculated by first converting the imported load values into the solver unit system and then multiplying the scale value. • For surface bodies, the thickness of each target node is ignored when data is mapped. When importing data from an External Data system, the Shell Thickness Factor property enables you to account for the thickness at each target node, and consequently modify the location used for each target node during the mapping process. See External Data Import for additional information. Imported Convection Coefficient When CFD convection coefficients are transferred to a thermal analysis, an Imported Convection Coefficient object can be inserted to represent the transfer. See the Imported Loads (p. 630) section for applicable transfers or for specific steps to transfer data. Note For surface bodies, the thickness of each target node is ignored when data is mapped. When importing data from an External Data system, the Shell Thickness Factor property enables you to account for the thickness at each target node, and consequently modify the location used for each target node during the mapping process. See External Data Import for additional information. Imported Heat Flux When thermal heat is transferred to a thermal environment, an Imported Heat Flux object can be inserted to represent the transfer. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 603 Features See the Imported Loads (p. 630) section for applicable transfers or for specific steps to transfer data. Note For surface bodies, the thickness of each target node is ignored when data is mapped. When importing data from an External Data system, the Shell Thickness Factor property enables you to account for the thickness at each target node, and consequently modify the location used for each target node during the mapping process. See External Data Import for additional information. Imported Heat Generation When thermal heat is transferred to a thermal environment, an Imported Heat Generation object can be inserted to represent the transfer. Imported Heat Generation applies Joule heating from an electric analysis in a thermal analysis. Please see the Imported Loads (p. 630) section for applicable transfers or for specific steps to transfer data. Note • The Joule heating, from an Electric analysis, resulting from limited contact electric conductance is ignored during this data transfer. • For each load step, if an Imported Heat Generation load and an Internal Heat Generation load are applied on common geometry selections, the Imported Heat Generation load takes precedence. An active Imported Heat Generation load will also overwrite other Imported Heat Generation loads that exist higher (previously added) in the tree, on common geometry selections. See Activation/Deactivation of Loads (p. 531) for additional rules when multiple load objects of the same type exist on common geometry selections. • For surface bodies, the thickness of each target node is ignored when data is mapped. When importing data from an External Data system, the Shell Thickness Factor property enables you to account for the thickness at each target node, and consequently modify the location used for each target node during the mapping process. See External Data Import for additional information. Imported Pressure When CFD pressures are transferred to a structural analysis, an Imported Pressure object is automatically inserted to represent the transfer. See the Imported Loads (p. 630) section for applicable transfers or for specific steps to transfer data. Note For surface bodies, the thickness of each target node is ignored when data is mapped. When importing data from an External Data system, the Shell Thickness Factor property enables you to account for the thickness at each target node, and consequently modify the location used for each target node during the mapping process. See External Data Import for additional information. 604 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Imported Surface Force Density When electromagnetic surface forces are transferred to a structural environment, an Imported Surface Force Density object can be inserted to represent the transfer. Please see the Imported Loads (p. 630) section for applicable transfers or for specific steps to transfer data. Imported Temperature When temperatures are transferred to a thermal analysis, an Imported Temperature object can be inserted to represent the transfer. See the Imported Loads (p. 630) section for applicable transfers or for specific steps to transfer data. Note • For each load step, if an Imported Temperature load and Temperature load are applied on common geometry selections, the Imported Temperature load takes precedence. An active Imported Temperature load will also overwrite other Imported Temperature loads that exist higher (previously added) in the tree, on common geometry selections. See Activation/Deactivation of Loads (p. 531) for additional rules when multiple load objects of the same type exist on common geometry selections. • If a scale factor is specified, the values used in the solution are calculated by first converting the imported load values into the solver unit system and then multiplying the scale value. • For surface bodies, the thickness of each target node is ignored when data is mapped. When importing data from an External Data system, the Shell Thickness Factor property enables you to account for the thickness at each target node, and consequently modify the location used for each target node during the mapping process. See External Data Import for additional information. Motion Load The application interacts with motion simulation software such as Dynamic Designer™ from MSC, and MotionWorks from Solid Dynamics. This is not the motion feature that is built into the Mechanical application. See the Rigid Dynamics Analysis (p. 102) and Transient Structural Analysis (p. 91) sections for information on the motion features built into the Mechanical application. Motion simulation software allows you to define and analyze the motion in an assembly of bodies. One set of computed results from the motion simulation is forces and moments at the joints between the bodies in the assembly. See Inserting Motion Loads (p. 607) for the procedure on inserting these loads. These loads are available for static structural analyses. Single Body Capability Insert Motion Loads is intended to work only with a single body from an assembly. If more than one body is unsuppressed in the Model during Import, you will receive an error message stating that only one body should be unsuppressed. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 605 Features Frame Loads File The application reads a text file produced by the motion simulation software. This file contains the load information for a single frame (time step) in the motion simulation. To study multiple frames, create multiple environment objects for the Model and import each frame to a separate environment. The frame loads file includes joint forces and inertial forces which "balance" the joint forces and gravity. Inertial State If the part of interest is a moving part in the assembly, the frame loads file gives the inertial state of the body. This includes gravitational acceleration, translational velocity and acceleration, and rotational velocity and acceleration. Of these inertial "loads" only the rotational velocity is applied in the environment. The remaining loads are accounted for by solving with inertia relief (see below). If the part of interest is grounded (not allowed to move) in the motion simulation, corresponding supports need to be added in the environment before solving. Joint Loads For each joint in the motion simulation, the frame loads file reports the force data - moment, force, and 3D location - for the frame. Features are also identified so that the load can be applied to the appropriate face(s), edge(s) or vertex(ices) within the application. These features are identified by the user in the motion simulation software before exporting the frame loads file. For all non-zero moments and forces, a corresponding "Moment" and "Remote Force" are attached to the face(s), edge(s) or vertex(ices) identified in the frame loads file. The Remote Force takes into account the moment arm of the force applied to the joint. Solving with Inertia Relief Inertia relief is enabled when solving an environment with motion loads. Inertia relief balances the applied forces and moments by computing the equivalent translational and rotational velocities and accelerations. Inertia relief gives a more accurate balance than simply applying the inertia loads computed in the motion simulation. Weak springs are also enabled. The computed reaction forces in the weak springs should be negligible. This option will automatically be turned on if you import any motion loads. Note Material properties have to be manually set to match density used in motion analysis. Modifying Parts with Motion Loads If you modify a part having a motion load, you should rerun the solution in the motion simulator software (e.g., Dynamic Designer) and re-export the loads to the Mechanical application. Then, in the Mechanical application, you must update the geometry, delete the load (from the Environment object) and re-insert the motion load. 606 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Modifying Loads You can modify loads that have been inserted, but you should only do so with great care. Modifying loads in the Mechanical application after importing from the motion simulation software will nullify the original loading conditions sets in the motion simulation software. Therefore, you need to examine your results in the Mechanical application carefully. Inserting Motion Loads You must make sure the files and data are up to date and consistent when analyzing motion loads. Use the following procedure to ensure that the correct loads are applied for a given time frame. To insert motion loads after solving the motion simulation: 1. Advance the motion simulation to the frame of interest. 2. Export the frame loads file from the motion software. 3. Attach the desired geometry. 4. Choose any structural New Analysis type except Rigid Dynamics and Random Vibration. 5. Suppress all bodies except the one of interest. 6. Click the environment object in the tree, then right-click and select Insert> Motion Loads. 7. Select the Frame Load file that you exported from Dynamic Designer. 8. Click Solve. If more than one body is unsuppressed in the Model corresponding to the environment object, you will receive an error message at the time of solution stating that only one body should be unsuppressed. 9. View the results. The exported loads depend on the part geometry, the part material properties, and the part's location relative to the coordinate system in the part document. When any of these factors change, you must solve the motion simulation again by repeating the full procedure. Verify that material properties such as density are consistent in the motion simulation and in the material properties. Insert Motion Loads is intended to work with a single body only. Results with grounded bodies (bodies not in motion in the mechanism) are not currently supported. If an assembly feature (such as a hole) is added after Dynamic Designer generates its Joint attachments for FEA, the attachments may become invalid. These attachments can be verified by opening the Properties dialog box for a Joint and selecting the FEA tab. An invalid attachment will have a red "X" through the icon. To correct this problem, manually redefine the joint attachments using the FEA tab in the Joint Properties dialog. A .log file is created when motion loads are imported. This troubleshooting file has the same name (with an .log extension) and file location as the load file. If the .log file already exists, it is overwritten by the new file. Fluid Solid Interface A Fluid Solid Interface is used to identify the interface where the transfer of loads to and from external fluid solvers CFX or FLUENT will occur. These loads are applicable on faces of solid or surface bodies in Static Structural and Transient Structural analyses. The integer Interface Number, found in the Details Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 607 Features view, is incremented by default each time a new interface is added. This value can be overridden if desired. Mechanical - CFX Once Fluid Solid Interfaces are identified, loads are transferred to and from body faces in the Mechanical APDL model using the MFX variant of the ANSYS Multi-field solver (see “Chapter 4. Multi-field Analysis Using Code Coupling” in the Coupled-Field Analysis Guide for details). This solver is accessed from either the Mechanical APDL Product Launcher or CFX-Solver Manager, and requires both the Mechanical APDL and CFX input files. To generate the Mechanical APDL input file, select the Solution object folder in the Mechanical Outline View, and then select Tools> Write Input File.... To generate the CFX input file, use the CFX preprocessor, CFX-Pre. Run time-monitoring is available in both the Mechanical APDL Product Launcher and CFX-Solver Manager. Postprocessing of the Mechanical APDL results is available in the Mechanical application, and simultaneous postprocessing of both the Mechanical APDL and CFX results is available in the CFX postprocessor, CFD-Post. Mechanical - FLUENT Fluid-solid interfaces define the interfaces between the solid in the Mechanical system and the fluid in the FLUENT system. These interfaces are defined on faces in the Mechanical model. Data is exchanged across these interfaces during the execution of the simulation. The Mechanical application sends displacements to FLUENT and FLUENT sends forces to the Mechanical application. Detonation Point An explosive may be initiated by various methods of delivering energy to it. However whether an explosive is dropped, thermally irradiated, or shocked, either mechanically or through a shock from an initiator (of a more sensitive explosive), initiation of an explosive always goes through a stage in which a shock wave is an important feature. In its ideal form this assumes that, on initiation, a detonation wave travels away from the initiation point with constant detonation velocity, being refracted around any inert obstacles in the explosive without moving the obstacle, maintaining a constant detonation velocity in the refracted zone and detonating each particle of explosive on arrival at that particle. The Detonation Point object is treated as a load, and can be inserted into the tree as a child of an Explicit Dynamics analysis object by choosing Insert > Detonation Point from the context menu, or selecting it from the Loads menu of the Environment toolbar. Multiple detonation points can be added to an analysis. The location of the selected detonation point and the detonation time are displayed in the annotation on the model. Note Detonation Points are not available for Explicit Dynamics (LS-DYNA Export) or for 2D Explicit Dynamics analyses. Details Category 608 Fields Description Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Definition Location Burn Instantaneously When set to Yes, results in initiation of detonation for all elements with an explosive material at the start of the solve. Detonation Time User can enter the time for initiation of detonation. [Only visible if Burn Instantaneously is set to No.] Suppressed Includes or excludes the boundary condition in the analysis. X Coordinate Enter detonation point coordinates. Y Coordinate Z Coordinate Location User can interactively select detonation location using the vertex/edge/face selection tools: • Select Vertex – sets X/Y/Z location to vertex location • Select Edge – sets X/Y/Z location to centre of edge • Select Face – sets X/Y/Z location to centre of face Theory The Detonation analysis method used is Indirect Path detonation. Detonation paths are computed by finding either a direct path through explosive regions or by following straight line segments connecting centers of cells containing explosives. Either: Detonation paths will be computed as the shortest route through cells that contain explosive. or Detonation paths are computed by finding the shortest path obtained by following straight line segments connecting the centers of cells containing explosive. The correct detonation paths will automatically be computed around wave-shapers, obstacles, corners, etc. Detonation points must lie within the grid. Paths cannot be computed through multiple Parts. If a detonation point is placed in one Part, the detonation from this point cannot propagate to another Part. If this is required, you must place one or more detonation points in the second Part with the appropriate initiation times set to achieve the required detonation. The following illustrates the detonation process: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 609 Features • Detonation is initiated at a node or plane (user defined) • Detonation front propagates at the Detonation Velocity, D • Cell begins to burn at time T1 • Burning is complete at time T2 • Chemical energy is released linearly from T1 to T2; burn fraction increases from 0.0 to 1.0 over this time The result DET_INIT_TIME can be used to view the initiation times of the explosive material. For example, in the image below, the body on the left side has a detonation point with instantaneous burn defined, and so the entire material has a detonation initiation time of 1x10-6 ms. The second body has a detonation point defined in the lower X, lower Y, lower Z corner, and the detonation time can be seen to vary from 0 ms (i.e. instantaneous detonation) to a value of 0.19555 ms in the corner of the body furthest away from the detonation point. Once detonation is initiated in an element, a value of zero is shown for DET_INIT_TIME. 610 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions The result ALPHA can be used to view the progress of the detonation wave through the material. This corresponds to the burn fraction, which will be a value between zero (no detonation) and one (detonation complete). For the same example, looking at values of alpha at a later stage in the calculation, the detonation wave can clearly be seen in the body on the right as the spherical band of contours showing the value of alpha changing from zero to one. The body on the left has a value of one for the entire body, as it detonated instantaneously. Conditions The following Conditions are available: Coupling Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 611 Features Constraint Equation Pipe Idealization Coupling While setting up a model for analysis, you can establish relationships among the different degrees of freedom of the model by physically modeling the part or a contact condition. However, sometimes there is a need to be able to model distinctive features of a geometry (for example, models that have equipotential surfaces) which cannot be adequately described with the physical part or contact. In this instance, you can create a set of surfaces/edges/vertices which have a coupled degree of freedom by using the Coupling boundary condition. Coupling the degrees of freedom of a set of geometric entity constrains the results calculated for one member of the set to be the same for all members of the set. Coupling can be used in the Thermal or Electric environments. Restrictions Make sure that you meet the following restrictions when scoping Coupling. • You cannot specify more than one Coupling (the same DOF) on the same geometric entity, such as two edges sharing a common vertex or two faces sharing a common edge. • Coupling should not be applied to a geometric entity that also has a constraint applied to it. To apply a coupled boundary condition with a single degree of freedom: 1. Insert a Coupling load by: a. Selecting Coupling from the Conditions drop-down menu. Or... b. Right-clicking on the environment object and selecting Insert> Coupling. Or... c. 2. Selecting your desired geometric entity (face/edge/vertex), right-clicking the mouse, and then selecting Insert> Coupling. Based on the analysis type, make Details view entries as applicable. • Thermal - Geometry • Electric - Geometry Constraint Equation This feature allows you to relate the motion of different portions of a model through the use of an equation. The equation relates the degrees of freedom (DOF) of one or more remote points for Harmonic, Modal, Modal (SAMCEF), Static Structural, Static Structural (SAMCEF), or Transient Structural systems, or one or more joints for the ANSYS Rigid Dynamics solver. For example, the motion along the X direction of one remote point (Remote Point A) could be made to follow the motion of another remote point (Remote Point B) along the Z direction by: 0 = [1/mm · Remote Point A (X Displacement)] - [1/mm · Remote Point B (Z Displacement)] 612 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions The equation is a linear combination of the DOF values. Thus, each term in the equation is defined by a coefficient followed by a node (Remote Point) and a degree of freedom label. Summation of the linear combination may be set to a non-zero value. For example: 7 = [4.1/mm · Remote Point A (X Displacement)] + [1/rad · Remote Vertex(Rotation Z)] Similarly, for the ANSYS Rigid Dynamics solver, to make the rotational velocity of gear A (Revolute A) to follow the rotational velocity of gear B (Revolute B), in the Z direction, the following constraint equation should be written: 0 = [1/rad · Revolute A (Omega Z)] - [1/rad · Revolute B (Omega Z)] This equation is a linear combination of the Joints DOF values. Thus, each term in the equation is defined by a coefficient followed by a joint and a degree of freedom label. Summation of the linear combination may be set to a non-zero value. For example: 7 = [4.1/mm · Joint A (X Velocity)] + [1/rad · Joint B (Omega Z)] Note that the Joints DOF can be expressed in terms of velocities or accelerations. However, all terms in the equation will be based on the same nature of degrees of freedom, that is, all velocities or all accelerations. To apply a constraint equation support: 1. Insert a Constraint Equation object by: a. Selecting Constraint Equation from the Conditions drop-down menu. Or... b. Right-clicking on the environment object and selecting Insert> Constraint Equation. 2. In the Details view, enter a constant value that will represent one side of the constraint equation. The default constant value is zero. 3. In the Worksheet, right-click in the first row and choose Add, then enter data to represent the opposite side of the equation. For the first term of the equation, enter a value for the Coefficient, then select entries for Remote Point or Joint and DOF Selection. Add a row and enter similar data for each subsequent term of the equation. The resulting equation displays as you enter the data. Using the example presented above, a constant value of 7 is entered into the Details view, and the data shown in the table is entered in the Worksheet. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 613 Features Note For Harmonic, Modal, Static Structural, and Transient Structural systems, the first unique degree of freedom in the equation is eliminated in terms of all other degrees of freedom in the equation. A unique degree of freedom is one which is not specified in any other constraint equation, coupled node set, specified displacement set, or master degree of freedom set. You should make the first term of the equation be the degree of freedom to be eliminated. Although you may, in theory, specify the same degree of freedom in more than one equation, you must be careful to avoid over-specification. Constraint Equation Characteristics • In the Worksheet, you can insert rows, modify an existing row, or delete a row. • A local coordinate system is defined in each remote point that is used. • The constant term is treated as a value with no unit of measure. • Coefficients for X Displacement, Y Displacement, Z Displacement, X Velocity, Y Velocity, Z Velocity, X Acceleration, Y Acceleration, and Z Acceleration have a unit of 1/length. • Coefficients for Rotation X, Rotation Y, Rotation Z, Omega X, Omega Y, Omega Z, Omega Dot X, Omega Dot Y, and Omega Dot Z have a unit of 1/angle. • If you change a DOF such that the unit type of a coefficient also changes (for example, rotation to displacement, or vice versa), then the coefficient resets to 0. • You can parameterize the constant value entered in the Details view. • The state for the Constraint Equation object will be under-defined (? in the tree) under the following circumstances: • – There are no rows with valid selections. – Remote Points being used are underdefined or suppressed. – Joints being used are underdefined or suppressed. – The analysis type does not support this feature. – The selected DOFs are invalid for the analysis (2-D versus 3-D, or remote point versus joints DOFs). The graphic user interface does not check for overconstraint. Pipe Idealization A Pipe Idealization object can be inserted in Static Structural, Transient Structural, Modal, and Harmonic analyses. Pipe Idealizations can be used to model pipes that have cross-section distortion, which can be commonly observed in curved pipe structures under loading. It can only be scoped to edges that have been modeled as pipes. It can be scoped directly to the geometry or to a named selection containing edges that are modeled as pipes. If a pipe idealization is scoped to a pipe, the underneath PIPE289 elements of the pipe are modified to ELBOW290 elements. You can extend the elbow elements to adjacent edges in order to reduce the boundary effects caused by the incompatible section deformation between edges modeled as straight pipes and high deformation pipes (elbows). If you do not want to extend the elements, under the Extend to Adjacent Elements section of the Details panel set Extend to No. To extend the elements, set Extend to Factor. You can then enter a Factor value, which will extend the elements to the adjacent edge up to a length of factor times selected pipe diameter. If the length calculated by factor times pipe diameter is less than the length of one element, it will still be extended by one element. 614 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Pipe pressure and pipe temperature loads are permitted on Pipe Idealizations. To add a Pipe Idealization to your analysis: 1. Right click on the environment object in the tree and select Insert > Pipe Idealization, Or... Select the environment object, then select Pipe Idealization from the Conditions drop down in the Environment toolbar. 2. Verify that in the Details panel for the Mesh object, Element Midside Nodes in the Advanced section is set to Kept. 3. Choose the setting for Extend to Adjacent Elements and enter the Factor, if you are using it. Note • If one or more of the elbow elements has a subtended angle of more than 45 degrees, a warning is reported. The solution can proceed, or you may want to use a finer mesh for better results. Pipe Idealization cannot be use with symmetry. • The scoped body must be meshed with higher order elements (Element Midside Nodes in the Advanced section of the Mesh Details panel must be set to Kept); otherwise the solver will report an error. • Although the solution will account for cross section distortions, the graphics rendering for the results will display the cross sections in their original shape. Direct FE The Direct Finite Element (FE) menu contains options that allow you to apply boundary conditions directly to the nodes on the finite element mesh of a model. These boundary conditions are scoped via nodebased Named Selections. They differ from geometry based boundary conditions in the fact that they are applied directly to the nodes during solution calculations whereas geometry-based boundary conditions are applied through special loading elements such as SURF, CONTAC, or FOLLW201 elements. These boundary conditions are applied in the Nodal Coordinate System (except Nodal Pressure). Direct FE boundary conditions cannot be applied to nodes that are already scoped with geometry-based constraints which may modify the Nodal Coordinate system. The following Direct FE options are available: Nodal Orientation Nodal Force Nodal Pressure FE Displacement FE Rotation Nodal Orientation Nodal Orientation objects are meant to rotate the nodes to a given coordinate system that you select in the GUI. By inserting a Nodal Orientation object and scoping it to a subset of nodes, you can create a Nodal Coordinate System and apply nodal rotations to the scoped nodes. Later, other node based boundary conditions (Nodal Force, FE Displacements, and FE Rotations) can use these Nodal Coordinate Systems. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 615 Features When two or more Nodal Orientations prescribe different Nodal Coordinate Systems at a single node, the object that is added last (in the tree) is applied. To define Nodal Orientation and apply it to nodes: 1. On the Environment context toolbar, click Direct FE > Nodal Orientation. Or, right–click the mouse button while on the Environment object in the tree or in the Geometry window and then select Insert>Nodal Orientation. 2. Click the Named Selection drop-down list and then select the node-based Named Selection to prescribe the scope of the boundary conditions. 3. Select the coordinate system that you want to use to define nodal orientation. The Details View selections are described below. Scope Description Scoping Method Read-only field that displays scoping method – Named Selection. Named Selection Drop-down list of available node-based Named Selections. Coordinate System Drop-down list of available coordinate systems. The selected system is used to orientate the nodes in the Named Selection. Definition Suppressed Includes or excludes the boundary condition in the analysis. Nodal Force Using Nodal Force, you can apply a force to an individual node or a set of nodes. You must create a node based Named Selection before you can apply a Nodal Force. The Nodal Force that you apply in Mechanical is represented as an F Command in the Mechanical APDL application. You can also apply a spatially varying Nodal Force to the scoped nodes. Note A Nodal Force may be added during Solution Restart without losing the restart points. To apply a Nodal Force: 1. On the Environment toolbar, click Direct FE > Nodal Force. Or, right–click the mouse button while on the Environment object in the tree or in the Geometry window and then select Insert>Nodal Force. 2. Click the Named Selection drop-down list and then select the node-based Named Section to prescribe the scope of the Nodal Force. 3. Enter a magnitude for the X, Y, and Z component to define the load. Tip Define a Nodal Orientation for the Named Selection to control the Nodal Coordinate System. The Details View selections are described below. Scope 616 Description Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Scoping Method Read-only field that displays scoping method - Named Selection. Named Selection Drop-down list of available node-based Named Selection. Definition Type Read-only field that describes the node-based object - Force. Coordinate System Read-only field that displays the coordinate system - Nodal Coordinate System. The Nodal Coordinate System can be modified by applying Nodal Orientation objects. X Component Defines force in the X direction Y Component Defines force in the Y direction Z Component Defines force in the Z direction Divide Load by Nodes Yes — (Default) Load value is normalized: it is divided by number of scoped nodes before application. No — Load value applied directly to every scoped node. Suppressed Includes or excludes the boundary condition in the analysis. Note • When Divide Load by Nodes is set to Yes, the forces are evenly distributed across the nodes and do not result in a constant traction. • Two Nodal Force objects that have same scoping do not produce a cumulative loading effect. The Nodal Force that was specified last takes priority and is applied, and as a result, the other Nodal Force is ignored. • A force or constraint applied to a geometric entity and a Nodal Force produce a resultant effect. Nodal Pressure Using Nodal Pressure, you can apply pressure on element faces. You must create a node based named selection before you can apply a FE Displacement. It is applicable for solid and surface bodies only. Specifically, an elemental face pressure is created only if all of the nodes of a given element face (including midside) are included. If all nodes defining a face are shared by an adjacent face of another selected element, the face is not free and will not have a load applied. For more information on the solver representation of this load, reference the SF Command in the Mechanical APDL application. Warning • For application to surface bodies, the MAPDL solver logic for this load is such that if all of the nodes of a shell element are specified, then the load is applied to the whole element face. However, if only some nodes are specified on an element and those nodes constitute a complete external edge, then an edge pressure is created. Therefore, it is critical that you make sure that you have not selected nodes that constitute only a free shell edge. This is because shell edge pressures are input on a per-unit-length basis, and Mechanical treats this load always as a per-unit-area quantity. Please see the SHELL181 Element Description for more information. • Nodal Pressures applied to shell bodies act in the opposite direction of geometry-based pressures. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 617 Features Note A Nodal Pressure may be added during Solution Restart without losing the restart points. To apply a Nodal Pressure: 1. On the Environment toolbar, click Direct FE > Nodal Pressure. Or, right–click the mouse button while on the Environment object in the tree or in the Geometry window and then select Insert>Nodal Pressure. 2. Click the Named Selection drop-down list, and then select the node-based Named Selection to prescribe the scope of the Nodal Pressure. 3. Enter a magnitude for the load. The Details View selections are described below. Scope Description Scoping Method Read-only field that displays scoping method - Named Selection. Named Selection Drop-down list of available node-based Named Selections. Definition Type Read-only field that displays boundary condition type - Pressure. Define By Read-only field that displays that the boundary condition is acting Normal To the surface to which it is attached. Magnitude Input field to define the magnitude of the boundary condition. This value can be defined as a Constant, in Tabular form, or as a Function. Suppressed Includes or excludes the boundary condition in the analysis. Note • To apply Nodal Pressure, the Named Selections that you create must include nodes such that they define an element face. • Two Nodal Pressure objects that have same scoping do not produce a cumulative loading effect. The Nodal Pressure that was specified last takes priority and is applied, and as a result, the other Nodal Pressure is ignored. • A force or constraint applied to a geometric entity and a Nodal Pressure produce a resultant effect. • You can apply a spatially varying Nodal Pressure to scoped nodes. FE Displacement Using FE Displacement, you can apply a displacement to an individual node or a set of nodes. You must create a node based named selection before you can apply a FE Displacement. You can also apply a spatially varying FE Displacement to the scoped nodes. To apply a FE Displacement: 618 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions 1. On the Environment toolbar, click Direct FE>FE Displacement. Or, right–click the mouse button while on the Environment object in the tree or in the Geometry window and then select Insert>FE Displacement. 2. Click the Named Selection drop-down list and then select the node-based Named Section to prescribe the scope of the FE Displacement. 3. Define loads in the X, Y, and/or Z directions. Tip Define a Nodal Orientation for the Named Selection to control the Nodal Coordinate System. The Details View selections are described below. Scope Description Scoping Method Read-only field that displays scoping method - Named Selection. Named Selection Drop-down list of available node-based Named Selections. Definition Type Read-only field that describes the node-based object - Displacement. Coordinate System Read-only field that displays the coordinate system - Nodal Coordinate System X Component Specifies a displacement value in the X direction. The default value is Free (no Displacement constraint applied). This value can also be defined as a Constant, in Tabular form, or as a Function. Y Component Specifies a displacement value in the Y direction. The default value is Free (no Displacement constraint applied). This value can also be defined as a Constant, in Tabular form, or as a Function. Z Component Specifies a displacement value in the Z direction. The default value is Free (no Displacement constraint applied). This value can also be defined as a Constant, in Tabular form, or as a Function. Suppressed Includes or excludes the boundary condition in the analysis. Note • Solution Restarts are only supported for Tabular data modifications. • If a Component is set to Function, all other Components automatically default to the Free setting and become read-only. • Two FE Displacement objects that have same scoping do not produce a cumulative loading effect. The FE Displacement that was specified last takes priority and is applied, and as a result, the other FE Displacement is ignored. • A force or constraint applied to a geometric entity and a FE Displacement produce a resultant effect. FE Rotation Using FE Rotation, you can apply a fixed rotation to an individual node or a set of nodes that have rotational degrees of freedom (DOFs). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 619 Features To apply a FE Rotation: 1. On the Environment toolbar, click Direct FE>FE Rotation. Or, right–click the mouse button while on the Environment object in the tree or in the Geometry window and then select Insert>FE Rotation. 2. Click the Named Selection drop-down list and then select the node-based Named Section to prescribe the scope of the FE Rotation. 3. Define the X, Y, and/or Z axis as Fixed or Free. At least one Component must be defined as Fixed. Tip Define a Nodal Orientation for the Named Selection to control the Nodal Coordinate System. The Details View selections are described below. Scope Description Scoping Method Read-only field that displays scoping method - Named Selection. Named Selection Drop-down list of available node-based Named Selections. Definition Type Read-only field that describes the node-based object - Fixed Rotation. Coordinate System Read-only field that displays the coordinate system - Nodal Coordinate System X Component Define the x-axis of rotation as Fixed (default) or Free. Y Component Define the y-axis of rotation as Fixed (default) or Free. Z Component Define the z-axis of rotation as Fixed (default) or Free. Suppressed Includes or excludes the boundary condition in the analysis. Note When parameterizing this boundary condition, a Free axis of rotation is represented by a zero (1) and Fixed with a value of one (0) inside the Parameter Workspace in ANSYS Workbench (outside of Mechanical). Spatial Varying Loads and Displacements A spatially varying load or displacement has a variable magnitude in a single coordinate direction (x, y, or z). The following load and displacement types qualify as varying loads and varying displacements, and can be a function of time as well. • Pressure - in a Normal direction only during a structural analysis • Line Pressure - in a Tangential direction only during a structural analysis • Pipe Pressure – during a structural analysis • Pipe Temperature – during a structural analysis • Temperature - during a thermal analysis • Convection - during a thermal analysis • Thermal Condition - during a structural analysis 620 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions • Displacement for Faces, Edges, or Vertices- during a structural analysis • FE Displacement • Nodal Force • Nodal Pressure For spatial varying loads and displacements, the spatial independent variable uses the origin of the coordinate system for its calculations and therefore it does not affect the direction of the load or displacement. To apply a spatial varying load or displacement, set the input as either Tabular or Function in the Details view. Specifying Load Values A load value or magnitude can be specified in the following ways: Constant Load Values Constant Load Expressions Tabular Loads Function Loads Note Changing the method of how a multiple-step load value is specified (such as Tabular to Constant), the Activation/Deactivation state of all steps resets to the default, Active. Constant Load Values For entering a static load value, click the flyout arrow in the Magnitude field, choose Constant, then type the value. Constant Load Expressions For entering a static load expression, click the flyout arrow in the Magnitude field and choose Constant. You then type a value in the field as an expression, similar to using a calculator. The Details view evaluates the expression and applies the value. For example, if you enter =2 + (3 * 5) + pow(2,3) in English in the numeric field, the Details view evaluates this expression and applies 25 for the value. You are required to enter an equal sign [=] before the expression. Note If the decimal separator in the current language is a comma (,) as it is in German, then the separator for the list of parameters of a function is a semicolon (;). For example, if an English expression is =2.5 + pow (1.3, 6), the equivalent German expression is =2,5 + pow (1.3; 6). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 621 Features The supported operators are: + - , *, /, ^ (for power) and % (integer Modulus) Sample usage: 2+3 10.5 – 2.5 3.5 * 3.3 10.12 / 1.89 2 ^ 10 10 % 3 2 * (3 + 5) The order of operator precedence is: parentheses intrinsic functions (like sin or cos) power (^) multiplication (*), division (/) and integer modulus (%) addition (+) and subtraction (-) The supported intrinsic functions are: Supported Intrinsic Functions Sample Usage Usage (angles in current Mechanical units setting) sin(x) sin(3.1415926535/2) sinh(x) sinh(3.1415926535/2) cos(x) cos(3.1415926535/2) cosh(x) cosh(3.1415926535/2) tan(x) tan(3.1415926535/4) tanh tanh(1.000000) asin(x) asin(0.326960) Calculates the arcsine. (x - Value whose arcsine is to be calculated) acos(x) acos(0.326960) Calculates the arccosine. (x - Value between –1 and 1 whose arccosine is to be calculated) atan(x) atan(-862.42) atan2(y,x) atan2(862.420000,78.514900) Calculates the arctangent of x (atan) or the arctangent of y/x (atan2). (x,y Any numbers) 622 Calculate sines and hyperbolic sines. Calculate the cosine (cos) or hyperbolic cosine (cosh). Calculate the tangent (tan) or hyperbolic tangent (tanh). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Supported Intrinsic Functions Sample Usage Usage (angles in current Mechanical units setting) pow(x,y) pow(2.0,3.0) Calculates x raised to the power of y. (x – Base y Exponent) sqrt(x) sqrt(45.35) Calculates the square root. ( x should be a Nonnegative value ) exp(x) exp(2.302585093) Calculates the exponential. (x - Floating-point value) log(x) log(9000.00) Calculates the natural logarithm. (x - Value whose logarithm is to be found) log10(x) log10(9000.00) Calculates the common logarithm. (x - Value whose logarithm is to be found) rand() rand() Generates a pseudorandom number. ceil(x) ceil(2.8) Calculates the ceiling of a value. It returns a floating-point value representing the smallest integer that is greater than or equal to x. (x - Floating-point value) ceil(-2.8) floor(x) floor(2.8) floor(-2.8) fmod(x,y) fmod(-10.0, 3.0) Calculates the floor of a value. It returns a floatingpoint value representing the largest integer that is less than or equal to x. (x - Floating-point value) Calculates the floating-point remainder.The fmod function calculates the floating-point remainder f of x / y such that x = i * y + f, where i is an integer, f has the same sign as x, and the absolute value of f is less than the absolute value of y. (x,y - Floatingpoint values). You can also enter hexadecimal (starting with 0x) and octal (starting with &) numbers, for example 0x12 and &12. Tabular Loads For entering a tabular load value, click the flyout arrow in the input field, such as the Magnitude field, choose Tabular (Time), then type the tabular data in the Tabular Data window. The Graph window displays the variation of the load with time. Annotations in the Geometry window display the current time in the Graph window along with the load value at that time. The following tabular load topics are discussed in this section: Importing Load History Exporting Load History Spatial Load Tabular Data Supported Tabular Loads Importing Load History To import a load history from a library: 1. Select the appropriate geometry on the model and do one of the following: • Click on the appropriate icon on the toolbar and choose the load. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 623 Features OR • Click right mouse button, select Insert, and choose the load. 2. Go to the Details view and in the input field, such as the Magnitude field, click on the flyout field and choose Import.... 3. Choose the desired load history if it is listed, then click OK. If it is not listed, click the Add... button, choose a load history or Browse... to one that is stored, then click OK in both dialog boxes. Exporting Load History To export a load history: By default, any load history that you create in the Mechanical application remains in the Mechanical application. To save the load history for future use: 1. Create a load history using the Graph or Tabular Data windows. 2. Go to the Details view and in the input field, such as the Magnitude field, click on the flyout field, choose Export, and save the file to a specific location. Spatial Load Tabular Data When using spatial varying loads, selecting Tabular as the input option displays the Tabular Data and Graph Controls categories in the Details view. The Tabular Data category provides the following options: • Independent Variable - specifies how the load varies, with Time (default), or in the X, Y, or Z spatial direction. For Line Pressure loads in a 3-D analysis or Pressure loads in a 2–D analysis, a Normalized S variable is also available, which allows you to define pressure as a function of the distance along a path whose length is denoted by S. When you select the Normalized S variable, the Tabular Data window accepts input data in the form of normalized values of path length (Normalized S) and corresponding Pressure values. A path length of 0 denotes the start of the path and a 1 denotes the end of the path. Any intermediate values between 0 and 1 are acceptable in the table. Load values are sent to the solver for each element on the defined path based on a first-order approximation. • Coordinate System - choose an existing coordinate system. The Graph Controls category provides the option for the X-Axis. Use this option to change the Graph window’s display to either Time or to the spatial direction specified in the Independent Variable field. When the X-Axis field is defined as Time: • Tabular Data content can be scaled against time. • You can activate and deactivate the load at a solution load step. Note The values used in the solution are calculated by first converting the imported load values into the solver unit system and then multiplying the scale value. 624 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Supported Tabular Loads You can enter the following loads and supports in tabular form: Structural Tabular Loads • Acceleration • Rotational Velocity • Pressure • Pipe Pressure • Pipe Temperature • Force • Remote Force • Moment • Line Pressure • Thermal Condition • Joint Load • Displacement • Remote Displacement • Velocity • Fixed Rotation • RS Base Excitation (RS Acceleration, RS Velocity, RS Displacement) • PSD Base Excitation (PSD G Acceleration, PSD Acceleration, PSD Velocity, PSD Displacement) Thermal Tabular Loads • Temperature • Convection Coefficient • Heat Flow • Heat Flux • Internal Heat Generation Note Tabular thermal loads applied to an edge in a 3D analysis are not supported. Electromagnetic Tabular Loads • Voltage • Current Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 625 Features Function Loads For entering a mathematical function, click the flyout arrow in the input field (for example, Magnitude), choose Function, then type a function such as =1000*sin(10*time). Any time values that you are evaluating can exceed the final time value by as much as one time step. The Graph window displays the variation of the load with time. Annotations in the Geometry window display the current time in the Graph window along with the load value at that time. The following function load topics are discussed in this section: Spatial Load and Displacement Function Data Supported Function Loads Spatial Load and Displacement Function Data When using spatial varying loads or displacements, selecting Function as the input option in the Details view presents an editable function field. Enter a mathematical expression in this field. Expressions have the following requirements: • For a Pressure load, the Define By option must be set to Normal To. • For a Line Pressure load, the Define By option must be set to Tangential. • You can use the spatial variation independent variables x, y, or z, and time (entered in lowercase) in the definition of the function. • For Line Pressure loads in a 3-D analysis or Pressure loads in a 2–D analysis, you can also use the variable s, which allows you to define pressure as a function of the distance along a path whose length is denoted by s. When defining a path length, valid primary variables you can enter are s alone or s combined with time, for example, s*time, or s*sin(time/s). Load values are sent to the solver for each element on the defined path based on a first-order approximation. • Define only one direction, x, y, or z; or path length, s. After entering a direction or path length, the Graph Controls category (see above) displays. When the Details view property Magnitude is set to Function, the following categories automatically display. • • 626 Function - properties include: – Unit System – the active unit system. – Angular Measure – the angular measure that is used to evaluate trigonometric functions. Graph Controls - based of the defined function, properties include: – X-Axis – This provides options to display time or the spatial independent variable in the graph. When set to Time you can activate and deactivate the load at a solution step. – Alternate Value – If the function combines time and a spatial independent variable, one of these values (alternate) must be fixed to evaluate the function for the two dimensional graph. – Range Minimum – If the X-Axis property is set to a spatial independent variable, this is the minimum range of the graph. For time, this value defaults to 0.0 and cannot be modified. – Range Maximum – If the X-Axis property is set to a spatial independent variable, this is the maximum range of the graph. For time this defaults to the analysis end time and can’t be modified. – Number of Segments - The function is graphed with a default value of two hundred line segments. This value may be changed to better visualize the function. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Spatial Varying Displacements You can also apply spatial varying displacements, which have the following additional or unique characteristics: • Edge scoping is available. • Displacements are shown as vectors instead of contours except if you choose Normal To the surface. Vectors are only displayed if the model has been meshed. The vector arrows are color-coded to indicate their value. A contour band is included for interpretation of the values. The contour band is the vector sum of the possible three vector components and therefore will only display positive values. • For one Displacement object, you can select up to three displacement components that can all vary using the same direction. If an additional direction is required, you can use an additional Displacement object. • A constant value and a table cannot be used in different components. A table will be forced in any component having a constant value if another component has a table. Supported Function Loads You can enter the following loads and supports as a mathematical function: Structural Function Loads • Acceleration • Rotational Velocity • Pressure • Pipe Pressure • Pipe Temperature • Force • Remote Force • Moment • Line Pressure • Thermal Condition • Joint Load • Displacement • Remote Displacement • Velocity • Fixed Rotation Note Function loads are not supported for Explicit Dynamics (LS-DYNA) analyses. Thermal Function Loads • Temperature • Convection Coefficient Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 627 Features • Heat Flow • Heat Flux • Internal Heat Generation Note Function thermal loads applied to an edge in a 3D analysis are not supported. Electromagnetic Function Loads • Voltage • Current Remote Boundary Conditions The following are classified as remote boundary conditions. These boundary conditions are considered as ”abstract” entities as opposed to boundary conditions that can be applied directly to the nodes or elements of a solid model. You can scope the remote boundary conditions to a remote point using Promote Remote Point in the RMB menu. • Point Mass • Thermal Point Mass • Springs • Joints • Remote Displacement • Remote Force • Moment Presented below is an example showing a Remote Displacement: Remote boundary conditions have the following characteristics: • 628 All remote boundary conditions make use of MPC contact used in the Mechanical APDL application. See the Surface-Based Constraints section in the Contact Technology Guide - part of the Mechanical APDL Help, for more information. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions • You are advised to check reaction forces to ensure that a remote boundary condition has been fully applied, especially if the boundary condition shares geometry with other remote boundary conditions, any type of constraint, or even MPC contact. • You can set the geometry Behavior as Rigid or Deformable, as described and illustrated below. • All remote boundary conditions are associative, meaning they remember their connection to the geometry. Their location however does not change. If you want the location to be associative, create a coordinate system on the particular face and set the location to 0,0,0 in that local coordinate system. • Remote boundary conditions scoped to a large number of elements can cause the solver to consume excessive amounts of memory. Point masses in an analysis where a mass matrix is required and analyses that contain remote displacements are the most sensitive to this phenomenon. If this situation occurs, consider modifying the Pinball setting to reduce the number of elements included in the solver. Forcing the use of an iterative solver may help as well. Refer to the troubleshooting section for further details. • If a remote boundary condition is scoped to rigid body, the underlying topology on which the load is applied is irrelevant. Since the body is rigid, the loading path through the body will be of no consequence; only the location at which the load acts. Geometry Behavior You can specify the Behavior of the scoped geometry for a remote boundary condition in the Details view as either Rigid or Deformable. This option dictates the behavior of the attached geometry. Rigid behavior will not allow the scoped geometry to deform whereas Deformable behavior will allow it. You must determine which Behavior best represents the actual loading. Note that this option has no effect if the boundary condition is scoped to a rigid body in which case a Rigid behavior is always used. Presented below are examples of the Total Deformation resulting from the same Remote Displacement first using a Rigid formulation, then using a Deformable formulation. Note For remote boundary conditions applied to an edge or edges of a line body that are colinear, the deformable behavior is invalid. As such, the scoped entities exhibit rigid behavior even if a deformable formulation is specified, and a warning is issued in the Message Window. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 629 Features Note To apply a remote boundary condition scoped to a surface more than once (for example, two springs), you must do one of the following: • Set scoped surface Behavior to Deformable. • Change scoping to remove any overlap. • Leverage the Pinball Region option (for Springs). Imported Loads Using this feature, results from one analysis can be applied as loads for a structural, thermal, electric or thermal-electric analysis with data transfer. You can include the loads from a CFD, thermal, electric, thermal-electric and electromagnetic analysis in the structural, thermal, electric, or thermal-electric analysis environments. You can also import data from external files and apply it in a Mechanical application analysis by creating a link with an upstream External data system. The following table shows valid environment interaction to import loads for an analysis with data transfer. Source Analysis/System (Transfer Data Type) Target Analysis CFD (Pressure) Static Structural, Transient Structural1 CFD (Temperature) Steady State Thermal, Transient Thermal, Thermal - Electric, Static Structural, Transient Structural1 CFD (Convection) Steady State Thermal, Transient Thermal, Thermal - Electric Steady-State Thermal, Transient Thermal (Temperature) Static Structural, Transient Structural1, Electric Thermal-Electric (Temperature) Static Structural, Transient Structural1, Electric (Joule Heat) Steady State Thermal, Transient Thermal Electromagnetic (Power Loss Density) Steady State Thermal, Transient Thermal 630 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Source Analysis/System (Transfer Data Type) Target Analysis Electromagnetic (Force Density) Static Structural, Transient Structural 1 External Files (Temperature, Convection, Heat Flux, Heat Generation) Steady State Thermal, Transient Thermal, Thermal – Electric, Static Structural, Transient Structural1 External Files (Pressure) Static Structural, Transient Structural1 POLYFLOW (Temperature) Steady State Thermal, Transient Thermal, Thermal - Electric, Static Structural, Transient Structural1 1 - rigid dynamics solver not supported. You can work with imported loads only when you perform an analysis with data transfer. To import loads for an analysis: 1. In the Project Schematic, add an appropriate analysis with data transfer to create a link between the solution of a previous analysis and the newly added analysis. 2. Attach geometry to the analysis system, and then double-click Setup to open the Mechanical window. An Imported Load folder is added under the environment folder, by default. 3. To add an imported load, click the Imported Load folder to make the Environment toolbar available or right mouse click on the Imported Load folder and select the appropriate load from the context menu. 4. On the Environment toolbar, click Imported Loads, and then select an appropriate load. 5. Select the appropriate geometry, and then click Apply. 6. Set the appropriate options in the Details view. 7. The Data View can be used to control the load data that is imported. Each data transfer incorporates some or all of the column types shown below. • Source Time - Time at which the load will be imported. • Source Time Step - Time Step at which the load will be imported. • Analysis Time - Time at which the load will be applied when the analysis is solved. • Scale - The amount by which the imported load values are scaled before they are sent to the solver. The scale value is applied to the imported load values in the solver unit system. For Imported Temperature and Imported Body Temperature loads: – • The values used in the solution are calculated by first converting the imported load values into the solver unit system and then multiplying the scale value. Offset - An offset that is added to the imported load values before they are sent to the solver. The offset value is applied to the imported load values in the solver unit system. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 631 Features Specific transfer details can be found in the Special Analysis Topics (p. 137) section. 8. In the Project tree, right-click the imported load, and then click Import Load to import the load. When the load has been imported successfully, a contour plot will be displayed in the Geometry window. 9. To preview the imported load contour that applies to a given row in the Data View, use the Active Row option in the Details view. To export data, select the Imported Load object, right-click the mouse, and then select Export. Additional information on Thermal-Stress, Fluid-Structure Interaction (FSI), Ansoft - Mechanical Data Transfer, Icepak to Mechanical Data Transfer, and External Data Import can be found in the Special Analysis Topics (p. 137) section. Note • If you are using the ANSYS solver, the Analysis Time must match the end time of one of the steps. • Convergence is not supported for environments with imported loads. Direction There are four types of Direction: Planar Face (p. 632) Edge (p. 632) Cylindrical Face or Geometric Axis Two Vertices (p. 633) Planar Face Selected planar face. The load is directed normal to the face. Note Not applicable to rotational velocity. Rotational velocity gets aligned along the normal to a planar face and along the axis of a cylindrical face. Edge Straight Colinear to the edge Circular or Elliptical Normal to the plane containing the edge 632 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Applying Boundary Conditions Selected straight edge Cylindrical Face or Geometric Axis Applies to cylinders, cones, tori, and cylindrical or conical fillets Selected cylinder Two Vertices 2 selected vertices Note Hold the CTRL key to select the second vertex. Loads that require you to define an associated direction include the Define By Details view control. Setting Define By to Vector allows you to define the direction graphically, based on the selected geometry. Setting Define By to Components allows you to define the direction by specifying the x, y, and z magnitude components of the load. Note If you switch the load direction setting in the Define By field, the data is lost. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 633 Features Scope Scope refers to geometry over which load/support applies. If you apply a force of 1000N in the X-direction, applied to a vertex, the load is "scoped" to that vertex. You can "scope" that load to some other geometry such as a face. Environment objects in general can be scoped (such as force, pressure, temperature) to geometry that you select, or to a named selection. Some environment objects, such as acceleration, cannot be scoped. Shared faces exist in the case of multibody parts. Contact regions, pressures, surface body forces, surface body moments, compression only supports, bearing loads, remote forces, convections, heat fluxes, and heat flows are not allowed to be applied to shared faces. For most loads, the Details view includes settings for you to specify the Scoping Method to either the geometry where the load is to be applied (Geometry Selection) or to a Named Selection. If you want to move a load from one part of a model to another, click the Geometry field, click on the new model location, then click Apply. Results in the Mechanical Application To insert a result, you must highlight a Solution object in the tree. You can then select the appropriate result item, result probe, or result tool from the available Solution Context Toolbar menus or by using the right-mouse click option to insert an object. In addition, you can scope your results to geometric entities or to meshing entities in some cases. You can also create user defined results using the User Defined Result option. Note The Result, User Defined Result, and Result Probe objects when suppressed will clear the generated data. The following result topics are presented in this section: Structural Results Thermal Results Magnetostatic Results Electric Results Fatigue Results User Defined Results Results Related Topics Structural Results The following structural result topics are addressed in this section: Deformation Stress and Strain Stabilization Energy Strain Energy Linearized Stress Contact Results Reactions Energy (Transient Structural and Rigid Dynamics Analyses) 634 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Frequency Response and Phase Response Stress Tools Fatigue (Fatigue Tool) Contact Tool Beam Tool Structural Probes Beam Results Gasket Results Campbell Diagram Chart Results Stress Tools (p. 658) are used to determine the following results: • Maximum Equivalent Stress Safety Tool (p. 659) • Maximum Shear Stress Safety Tool (p. 661) • Mohr-Coulomb Stress Safety Tool (p. 662) • Maximum Tensile Stress Safety Tool (p. 664) Structural Probes (p. 671) can be used to determine the following results: • Deformation • Strain • Position • Velocity • Angular Velocity • Acceleration • Angular Acceleration • Energy • Force Reaction • Moment Reaction • Joint • Response PSD • Spring • Beam • Bolt Pretension • Generalized Plane Strain Deformation Physical deformations can be calculated on and inside a part or an assembly. Fixed supports prevent deformation; locations without a fixed support usually experience deformation relative to the original location. Deformations are calculated relative to the part or assembly world coordinate system. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 635 Features Component deformations (Directional Deformation) Deformed shape (Total Deformation vector) The three component deformations Ux, Uy, and Uz, and the deformed shape U are available as individual results. Scoping is also possible to both geometric entities and to underlying meshing entities (see example below). Numerical data is for deformation in the global X, Y, and Z directions. These results can be viewed with the model under wireframe display, facilitating their visibility at interior nodes. Example: Scoping Deformation Results to Mesh Nodes The following example illustrates how to obtain deformation results for individual nodes in a model. The nodes are specified using criteria based named selections. 1. Create a named selection by highlighting the Model tree object and clicking the Named Selection toolbar button. 2. Highlight the Selection object and in the Details view, set Scoping Method to Worksheet. 3. In the Worksheet, add a row and set the following items for the row. Refer to Specifying Named Selections using Worksheet Criteria (p. 362) for assistance, if needed. • Entity Type = Mesh Node. • Criterion = Location X. • Operator = Greater Than. • Value = 0.1. 4. Add a second row with Criterion = Location Y, Value = 0.2, and all remaining items set the same as the first row. 5. Add a third row with Criterion = Location Z, Value = 0.3, and all remaining items set the same as the first row. The table displays as shown below 636 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application 6. Click the Generate button. The Geometry field in the Details view displays the number of nodes that meet the criteria defined in the Worksheet. 7. After applying loads and supports to the model, add a Total Deformation result object, highlight the object, set Scoping Method to Named Selection, and set Named Selection to the Selection object defined above that includes the mesh node criteria. Before solving, annotations are displayed at each selected node as shown below. 8. Solve the analysis. Any element containing a selected node will display a contour color at the node. If all nodes on the element are selected, the element will display contour colors on all facets. Element facets that contain unselected nodes will be transparent. An example is shown below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 637 Features Note that all element facets are drawn, not just the facets on the surface or skin of the model. To possibly reduce clutter for complex models, the size of the dots representing the nodes can be changed by choosing View> Large Vertex Contours. Working with Deformations Deformations can be used to • Set Alert objects. • Control accuracy and convergence and to view converged results. • Study deformations in a selected or scoped area of a part or an assembly. Velocity and Acceleration In addition to deformation results, velocity and acceleration results are also available for Transient Structural, Rigid Dynamics, Random Vibration, and Response Spectrum analyses. Both total and directional components are available for the Transient Structural analyses and Response Spectrum analyses but only directional components are available for Random Vibration as described below. Considerations for Random Vibration and Response Spectrum Analyses For Random Vibration and Response Spectrum analyses, only component directional deformations are available because the directional results from the solver are statistical in nature. The X, Y, and Z displacements cannot be combined to get the magnitude of the total displacement. The same holds true for other derived quantities such as principal stresses. Directional Deformation, Directional Velocity, and Directional Acceleration result objects in Random Vibration analyses also include the following additional items in the Details view: • 638 Reference - Read-only reference indication that depends on the directional result. Possible indications are: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application – Relative to base motion for a Directional Deformation result. – Absolute (including base motion) for a Directional Velocity or Directional Acceleration result. • Scale Factor - A multiple of standard deviation values (with zero mean value) that you can enter which determines the probability of the time the response will be less than the standard deviation value. By default, the results output by the solver are 1 Sigma, or one standard deviation value. You can set the Scale Factor to 2 Sigma, 3 Sigma, or to User Input, in which case you can enter a custom scale factor in the Scale Factor Value field. • Probability - Read-only indication of the percentage of the time the response will be less than the standard deviation value as determined by your entry in the Scale Factor field. A Scale Factor of 1 Sigma = a Probability of 68.3 %. 2 Sigma = 95.951 %. 3 Sigma = 99.737 %. Stress and Strain Stress solutions allow you to predict safety factors, stresses, strains, and displacements given the model and material of a part or an entire assembly and for a particular structural loading environment. A general three-dimensional stress state is calculated in terms of three normal and three shear stress components aligned to the part or assembly world coordinate system. The principal stresses and the maximum shear stress are called invariants; that is, their value does not depend on the orientation of the part or assembly with respect to its world coordinate system. The principal stresses and maximum shear stress are available as individual results. The principal strains ε1, ε2, and ε3 and the maximum shear strain γmax are also available. The principal strains are always ordered such that ε1> ε2> ε3. As with principal stresses and the maximum shear stress, the principal strains and maximum shear strain are invariants. You can choose from the following stress/strain results: Equivalent (von Mises) Maximum, Middle, and Minimum Principal Maximum Shear Intensity Vector Principals Error (Structural) Thermal Strain Equivalent Plastic Strain Equivalent Creep Strain Equivalent Total Strain Membrane Stress Bending Stress Normal (X, Y, Z) and Shear (XY, YZ, XZ) stress and strain results are also available. It is assumed that whatever holds true for stress applies to strain as well. However, the relationship between maximum shear stress and stress intensity does not hold true for an equivalent relationship between maximum shear strain and strain intensity. For more information about Stress/Strain, see the Mechanical APDL Theory Reference. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 639 Features Considerations The degree of uncertainty in the numerical calculation of Stress answers depends on your accuracy preference. See Adaptive Convergence (p. 787) for information on available options and their effect on Stress answers. For your convenience and future reference, Report can include stress, strain, and deformations value, convergence histories, and any alerts for these values. Equivalent (von Mises) Equivalent stress is related to the principal stresses by the equation: 1/ 2  σ −σ 2 + σ −σ 2 + σ −σ 2 1 2 2 3 3 1 σe =     Equivalent stress (also called von Mises stress) is often used in design work because it allows any arbitrary three-dimensional stress state to be represented as a single positive stress value. Equivalent stress is part of the maximum equivalent stress failure theory used to predict yielding in a ductile material. The von Mises or equivalent strain εe is computed as:  ε = + ν 
 ε − ε  + ε − ε  + ε − ε      
 
  where: ν' = effective Poisson's ratio, which is defined as follows: • Material Poisson's ratio for elastic and thermal strains computed at the reference temperature of the body. • 0.5 for plastic strains. Maximum, Middle, and Minimum Principal From elasticity theory, an infinitesimal volume of material at an arbitrary point on or inside the solid body can be rotated such that only normal stresses remain and all shear stresses are zero. The three normal stresses that remain are called the principal stresses: σ1 - Maximum σ2 - Middle σ3 - Minimum The principal stresses are always ordered such that σ1 > σ2 > σ3. 640 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Maximum Shear The maximum shear stress τmax, also referred to as the maximum shear stress, is found by plotting Mohr's circles using the principal stresses: or mathematically through: σ − σ3 τmax = 1 For elastic strain, the maximum sheer elastic strain γmax is found through: γmax = ε1 - ε3 since the shear elastic strain reported is an engineering shear elastic strain. Intensity Stress intensity is defined as the largest of the absolute values of σ1 - σ2, σ2 - σ3, or σ3 - σ1: σI = ( σ − σ 2 σ 2 − σ
σ
− σ ) Stress intensity is related to the maximum shear stress: σI = 2τmax Elastic Strain intensity is defined as the largest of the absolute values of ε1 - ε2, ε2 - ε3, or ε3 - ε1: ε = ( ε − ε ε − ε ε − ε ) Elastic Strain intensity is equal to the maximum shear elastic strain: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 641 Features εI = γmax Equivalent Stress (and Equivalent Elastic Strain) and Stress Intensity are available as individual results. Note Computation of Equivalent Elastic Strain uses Poisson’s ratio. If Poisson’s ratio is temperature dependent then the Poisson’s ratio value at the reference temperature of the body is used to compute the Equivalent Elastic Strain. Vector Principals A Vector Principals plot provides a three-dimensional display of the relative size of the principal quantities (stresses or elastic strains), and the directions along which they occur. Positive principals point outwards and negative ones inwards. Plots of Vector Principals help depict the directions that experience the greatest amount of normal stress or elastic strain at any point in the body in response to the loading condition. The locus of directions of maximum principal stresses, for example, suggests paths of maximum load transfer throughout a body. Request a Vector Principals plot in the same way that you would request any other result. Scoping is also possible. Numerical data for these plots can be obtained by exporting the result values to an .XLS file. These files have 6 fields. The first three correspond to the maximum, middle, and minimum principal quantities (stresses or elastic strains). The last three correspond to the Mechanical APDL application Euler angle sequence (CLOCAL command in the ANSYS environment) required to produce a coordinate system whose X, Y and Z-axis are the directions of maximum, middle and minimum principal quantities, respectively. This Euler angle sequence is ThetaXY, ThetaYZ, and ThetaZX and orients the principal coordinate system relative to the global system. These results can be viewed using the Graphics button, so that you can use the Vector Display toolbar. Error (Structural) You can insert an Error result based on stresses to help you identify regions of high error and thus show where the model would benefit from a more refined mesh in order to get a more accurate answer. You can also use the Error result to help determine where Workbench will be refining elements if Convergence is active. The Error result is based on the same errors used in adaptive refinement. Information on how these errors are calculated is included in POST1 - Error Approximation Technique, in the Theory Reference for ANSYS and ANSYS Workbench. Note Scoping is limited to assembly or body scoping (that is, face/edge/vertex scoping is not allowed). The Error result is based on linear stresses and as such may be inaccurate in certain nonlinear analyses (for example, when plasticity is active). Furthermore, the Error result is currently restricted to isotropic materials. You may wish to refer to the Structural Material Properties section of the Engineering Data help for additional information. Presented below are example applications of using the Error result in a Structural simulation. 3-D Model: 642 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application 2-D Model, Base Mesh: 2-D Model, Adaptive Refinement (Convergence Added): 2-D Model, With Mesh Control: Thermal Strain Thermal strain is computed when coefficient of thermal expansion is specified and a temperature load is applied in a structural analysis. To specify the coefficient of thermal expansion, you must set Thermal Strain Effects to Yes in the Details view of the part or body objects before initiating a solve. Each of the components of thermal strain are computed as: Where: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 643 Features - thermal strain in one of the directions x, y, or z. - Secant coefficient of thermal expansion defined as a material property in Engineering Data (see “Chapter 2.4 Linear Material Properties” in the Element Reference of the Mechanical APDL application Help for more information about the secant function). - reference temperature or the "stress-free" temperature. This can be specified globally for the model using the Reference Temperature field of Static Structural or Transient Structural analysis types. Optionally you can also specify the reference temperature as a material property for cases such as the analysis for cooling of a weld or solder joint where each material has a different stress-free temperature. Equivalent Plastic Strain The equivalent plastic strain gives a measure of the amount of permanent strain in an engineering body. The equivalent plastic strain is calculated from the component plastic strain as defined in the Equivalent stress/strain section. Most common engineering materials exhibit a linear stress-strain relationship up to a stress level known as the proportional limit. Beyond this limit, the stress-strain relationship will become nonlinear, but will not necessarily become inelastic. Plastic behavior, characterized by nonrecoverable strain or plastic strain, begins when stresses exceed the material's yield point. Because there is usually little difference between the yield point and the proportional limit, the Mechanical APDL application assumes that these two points are coincident in plasticity analyses. Stress Yield Point Proportional Limit Strain Plastic Strain In order to develop plastic strain, plastic material properties must be defined. You may define plastic material properties by defining either of the following in the Engineering Data: • Bilinear Stress/Strain curve. • Multilinear Stress/Strain curve. Note Yield stresses defined under the Stress Limits section in the Engineering Data are used for the post tools only (that is, Stress Safety Tools and Fatigue tools), and do not imply plastic behavior. 644 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Equivalent Creep Strain Creep is a rate-dependent material nonlinearity in which the material continues to deform under a constant load. The material deforms under an initial applied load and the load diminishes over time with an increase in deformation or creep strain. The equivalent creep strain gives a measure of the amount of the creep strain in an engineering body. The equivalent creep strain is calculated from component creep strains. In order to develop creep strain, creep material properties must be defined. You may define creep material properties by choosing one of the available 13 creep models in Engineering Data. This result type is available in Mechanical only after you have selected a creep material for at least one prototype in the analysis. Equivalent Total Strain The equivalent total strain gives a total value of strain in any engineering body. The total strain components are calculated by addition of components of elastic, plastic, thermal, and creep strains and then equivalent total strain is calculated from total strain components. This result type is available in Mechanical only if at least one of the other three strain results is available for post processing. In Mechanical APDL this strain in called Total Mechanical and Thermal Strain. Membrane Stress Membrane stress calculates the stresses along the thickness of the shell in longitudinal direction, in transverse direction, and in plane shear. The result is available only for shell bodies and solids that are meshed using the thin-solid meshing option. Each element of the body can display individual stress values and give a checkboard appearance to the result contours. The results are calculated in the element coordinate system. Shell membrane stress tensor (s11m, s22m, s12m) is the average of the in-plane stress tensor (s11(z), s22(z), s12(z)) along the shell thickness direction: t ∫σ σ 11m = 11 z dz 0 σ 22 =   σ  = ∫σ 22  
∫σ   Where: t is the total shell thickness, z is the thickness location where the in-plane stress is evaluated. Unlike linearized stress in other elements, a pre-defined path through the shell thickness is not required in order to compute shell membrane stress. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 645 Features Note Make sure that the Output Control, General Miscellaneous is set to Yes or your results may be under-defined. Bending Stress The result is available only for shell bodies and solids that are meshed using the thin-solid meshing option and are calculated in the element coordinate system. Each element of the body can display individual stress values and give a checkboard appearance to the result contours. Shell bending stress tensor (s11b, s22b, s12b) represents the linear variation portion of the in-plane stress tensor (s11(z), s22(z), s12(z)) along the shell thickness direction: t b 11 σ = 2 ∫σ 11 z 0  

σ =  σ =
∫σ

 ∫σ    −z  − − dz   Where: t is the total shell thickness, z is the thickness location where the in-plane stress is evaluated. Note Make sure that the Output Control, General Miscellaneous is set to Yes or your results may be under-defined. Stabilization Energy Stabilization can help with convergence problems, but it can also affect accuracy if the stabilization energy or forces are too large. Although ANSYS automatically reports the stabilization force norms and compares them to internal force norms, it is still very important to check the stabilization energy and forces to determine whether or not they are excessive. If the stabilization energy is much less than the potential energy (for example, within a 1.0 percent tolerance), the result should be acceptable. When stabilization energy is large, check the stabilization forces at each DOF for all substeps. If the stabilization forces are much smaller than the applied loads and reaction forces (for example, within a 0.5 percent tolerance), the results are still acceptable. Such a case could occur when an elastic system is loaded first, then unloaded significantly. It is possible that the final element potential energy is small and stabilization energy is relatively large, but all stabilization forces are small. Currently, stabilization forces are accessible in the .OUT file. 646 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Even when both stabilization energy and forces are too large, the results could still be valid. Such a scenario is possible when a large part of an elastic structure undergoes large rigid body motion (as in a snap-through simulation). In such a case, the stabilization energy could be large as well as the stabilization force for some DOFs at some substeps, but the results could still be acceptably accurate. Nevertheless, consider the results along with other support data and use your own discretion. To insert a Stabilization Energy result, highlight the Solution object in the tree, then select Stabilization Energy from the Solution Context Toolbar (p. 291) or right-mouse click on the object and choose Insert> Energy> Stabilization Energy. The following figure shows an example stabilization energy contour plot: Strain Energy Energy stored in bodies due to deformation. This value is computed from stress and strain results. It includes plastic strain energy as a result of material plasticity. To insert a Stabilization Energy result, highlight the Solution object in the tree, then select Stabilization Energy from the Solution Context Toolbar (p. 291) or right-mouse click on the object and choose Insert> Energy> Strain Energy. Linearized Stress The Linearized Stress results calculate membrane, bending, peak, and total stress along a straight line path in the Mechanical application. To calculate linearized stress, you must first define a straight line path object using Construction Geometry under Model. A path you define for linearized stress can be of type Two Points or of type X axis Intersection and should have at least 47 sample points. The number of points must be an odd number; otherwise the result will not solve and an error message will be issued. The path must be straight and entirely within the model’s elements. The X axis Intersection option is recommend as it ensures that the start and end points are inside the mesh and that the path is straight. Note that the Two Points method obtains the points from the tessellation of the geometric model, and if the geometry faces are curved, the points might not be inside the mesh. For these Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 647 Features situations, you can use the Snap to mesh nodes feature (see Path (Construction Geometry) (p. 376)) to ensure that the two points are contained within the mesh. Linearized stress does not support the Edge path type. To calculate linearized stresses: 1. In the object tree, select Solution to make the Solution toolbar available. 2. On the Solution toolbar, click Linearized Stress, and then click the stress you want to calculate. 3. In the Details view, select the Path you have defined to calculate the linearized stress. 4. Select the coordinate system you have used for the model. 5. Click Solve to calculate linearized stress along the path. Geometry Select bodies that contribute toward stress calculation Path The path you define to calculate the linearized stresses Type Types of linearized stresses available Coordinate System Coordinate systems you can select for stress calculation About Linearized Stress When the result is evaluated, component stress values at the path points are interpolated from the appropriate element's average corner nodal values. Stress components through the section are linearized by a line integral method and are separated into constant membrane stresses, bending stresses varying linearly between end points, and peak stresses (defined as the difference between the actual (total) stress and the membrane plus bending combination). The Details view shows Membrane, Bending, Membrane + Bending, Peak, and Total stresses. The bending stresses are calculated such that the neutral axis is at the midpoint of the path. Principle stresses are recalculated from the component stresses and are invariant with the coordinate system as long as stress is in the same direction at all points along the defined path. It is generally recommended that calculations be performed in a rectangular coordinate system (e.g. global Cartesian). The Details view also includes the following three choices for 2D Behavior: Planar, Axisymmetric Straight, and Axisymmetric Curve. These choices are available to any type of geometry (for example, you can choose Axisymmetric Straight for a 3D model). For Axisymmetric Straight and Axisymmetric Curve, the Details view includes entries for Average Radius of Curvature and Through-Thickness Bending Stress. The Average Radius of Curvature represents the in-plane (X-Y) average radius of curvature of the inside and outside surfaces of an axisymmetric section. If the radius is zero, a plane or 3-D structure is assumed. The curve radius is in the current units. An Axisymmetric Straight analysis always has an infinite radius of curvature (which is denoted by a value of -1). The choices for Through-Thickness Bending Stress are: • Include: Include the thickness-direction bending stresses. • Ignore: Ignore the thickness-direction bending stresses. • Include Using Y Dir. Formula: Include the thickness-direction bending stress using the same formula as the Y (axial direction ) bending stress. Also use the same formula for the shear stress. 648 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application If the Average Radius of Curvature is non-zero, Mechanical reports the linearized stresses in the section coordinates (SX – along the path, SY – normal to the path, and SZ – hoop direction). In this case, the choice of Coordinate System in the Details view is ignored. If the Average Radius of Curvature is zero, Mechanical reports the linearized stresses in the active results coordinate system. Notes on Linearized Stress • The line integral method is the same as that used in the Mechanical APDL command PRSECT, RHO, KBR. • Mechanical does not support the Solution Coordinate System for this result. • The Worksheet reports the linearized component and principal stresses for each stress category at the beginning, mid-length, and end of the section path. Contact Results If your model contains Contact Regions, you can define the following contact results under the Solution object by inserting a Contact Tool: • Gap • Penetration • Pressure • Frictional Stress - available only for evaluating contact conditions after solution. Note – To reflect total contact pressures or frictional stress, you must either set the Behavior option to Asymmetric or Auto Asymmetric, or manually create an asymmetric contact pair. – For node-to-surface contact, Pressure will display zero results. To display the associated contact force, you must insert a user defined result called CONTFORC. • Sliding Distance - available only for evaluating contact conditions after solution. • Status. Status codes are: – 0-open and not near contact – 1-open but near contact – 2-closed and sliding – 3-closed and sticking The labels Far, Near, Sliding, and Sticking are included in the legend for Status. Note Contact that has been deactivated via Auto Asymmetric behavior will be displayed with a status of Far-Open. Results for deactivated pairs can be suppressed in the Contact Tool by changing Both to either Contact or Target as necessary. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 649 Features The scoping method will affect how the results are displayed. If the Contact Tool is scoped using the Geometry Selection method, the contact results will be averaged across the selected geometry. If the Contact Tool is scoped using the Worksheet method, you can select one (or more) contact pair in the worksheet, and the displayed results will correspond specifically to that contact pair (or pairs). The images below illustrate how contact results are affected by the different scoping types. The model consists of two blocks contacting a third block. Using the Worksheet method, one Contact Tool was scoped to the contact pair on the left, and another one was scoped to the contact pair on the right. This allows you to view the contact results for each contact pair individually. The contact status for the contact pair on the left is shown below. The contact status for the contact pair on the right is shown below. 650 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application A third Contact Tool scoped to the surface of the large block (using the Geometry Selection method) allows you view the contact status averaged over that surface, as shown below. Note Be aware of the following restrictions regarding contact results: • When a contact result is scoped to a face of an assembly, a contact result may not be obtained in certain cases, especially if the scoped face is not a part of any contact region. • Contour contact results are not reported for 3-D edge contact. Reactions Forces and Moments You can obtain reaction forces and moments at the following supports using Force Reaction probes or Moment Reaction probes. • Fixed face • Fixed edge • Fixed vertex • Displacement for faces Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 651 Features • Displacement for edges • Displacement for vertices • Remote Displacement • Frictionless face • Compression Only support Note Reactions for Compression Only supports will only display results for a fully solved solution. Results will not be available for partial solutions. • Cylindrical support • Simply supported edge • Simply supported vertex • Fixed face rotation (does not include Force reactions) • Fixed edge rotation (does not include Force reactions) • Fixed vertex rotation (does not include Force reactions) • Weak springs In the Details view of the probes you can specify the coordinate system in which to interpret these results. By default these forces and moments are displayed in global Cartesian coordinate system. When you request a Force Reaction or Moment reaction in a Cartesian coordinate system at a specific time point by setting Display = Single Time Point in the Details view for Static Structural and Transient Structural Analysis, the Force Reaction or Moment reaction is displayed by an arrow in the Geometry window. Force Reaction uses a single arrowhead and moment reaction uses double arrowhead. The arrows are drawn on the deformed mesh. Similar is the case, when the force or moment reaction results are requested based on Frequency or Set Number and Phase Angle for Harmonic analysis and Mode Number for Modal analysis. 652 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Note • Force Reaction probes support Cartesian or cylindrical coordinate systems. Moment Reaction probes support Cartesian coordinate systems only. • A reported reaction may be inappropriate if that support shares a face, edge, or vertex with another support, contact pair, or load. This is because the underlying finite element model will have both loads and supports applied to the same nodes. If a model contains two or more supports that share an edge or vertex, use caution in evaluating the listed reaction forces at those supports. Calculation of reaction forces includes the force acting along bounding edges and vertices. When supports share edges or vertices the global summation of forces may not appear to balance. Reaction forces may be incorrect if they share an edge or face with a contact region. • For a moment reaction scoped to a contact region, the location of the summation point may not be exactly on the contact region itself. • If you set Extraction = Source(Underlying Element) in the Details view of either a force or moment probe, the reaction calculations work from summing the internal forces on the underlying elements under a contact region. Thus, a reported reaction may be inappropriate on a contact face if that face shares topology with another contact face/edge or external load (such as a force or fixed support), which would contribute to the underlying elements' internal force balance. In addition, during a transient analysis, inertial and damping forces are also included. Another possible scenario could arise for MPC contact of solid surfaces. In this case, if a gap is detected, the solver may build constraints on an additional layer into the solid mesh from the TARGET elements. This produces a more accurate response but will invalidate any reactions from the underlying solid elements of the TARGET elements. If symmetric contact is chosen be careful to verify which side becomes active for the TARGET elements so that the correct reaction can be determined. Contact Based Force Reactions For a force reaction scoped to a contact region, if you set Extraction = Source(Contact Element), the reaction calculations come directly from the contact elements themselves. This results in accurate force reactions even when the contact region overlaps with other boundary conditions, such as other contact regions, supports, etc. Characteristics of the Source(Contact Element) setting are that MPC contact is not supported, nor are reactions from the Target(Underlying Element) side. This feature should only be used with Asymmetric contact and requires that Calculate Miscellaneous be set to Yes in the Output Controls. A limitation of the Source(Contact Element) setting is when you use linear contact (that is, either Bonded or No Separation contact types) with loads that are unrealistically very high or very low in magnitude. These situations can produce inaccurate force reactions. Reactions to Bolt Pretension Load When a Bolt Pretension load is applied, the Mechanical application reports the following reactions: Adjustment: This represents the displacement that occurs from the pretension. In Mechanical APDL terms, this is the displacement reported from the pretension node. This result is also available for reporting regardless of how the bolt is defined. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 653 Features Working Load: This represents a constrained force reaction from the pretension load. In Mechanical APDL terms, this is the constrained reaction reported from the pretension node. This is essentially the sum of all the forces acting through the pretension cut. This result is applicable for load steps when the load is defined by either Locked or Adjustment. Reactions to Generalized Plane Strain Load When a Generalized Plane Strain load is applied (2-D application), the Mechanical application reports the following reactions: • Fiber Length Change: Fiber length change at ending point. • Rotation X Component: Rotation angle of end plane about x-axis. • Rotation Y Component: Rotation angle of end plane about y-axis. • Force: Reaction force at end point. • Moment X Component: Reaction moment on end plane about x-axis. • Moment Y Component: Reaction moment on end plane about y-axis. Reactions in Modal Analysis • This feature requires Calculate Reactions to be set to Yes in the Output Controls. • Reaction results in damped modal analysis provides By field option in the result definition to compute results based on Mode Number, Phase of Maximum, and Maximum Over Phase. Reactions in Harmonic Analysis • This feature requires Calculate Reactions to be set to Yes in the Output Controls. • Reaction results support all options of the result definition available for other harmonic results. • Reaction results are reported based on the nearest frequency results available and no interpolation is done. Reactions in Random Vibration and Response Spectrum Analyses • This feature requires Calculate Reactions to be set to Yes in the Output Controls of Modal system. • Reaction results can only be scoped to a Remote Displacement boundary condition. Note Animation of reaction results is not supported for modal and harmonic analysis. Energy (Transient Structural and Rigid Dynamics Analyses) A Transient Structural analysis supports the following energy outputs: Strain Energy: Energy stored in bodies due to deformation. This value is computed from stress and strain results. It includes plastic strain energy as a result of material plasticity. Kinetic Energy: Kinetic energy due to the motion of parts in a transient analysis. A Rigid Dynamics analysis supports the following energy outputs: 654 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Kinetic Energy: Kinetic energy due to the motion of parts in a transient analysis is calculated as ½ *mass* velocity2 for translations and ½ *omegaT*Inertia*omega for rotations. Potential Energy: This energy is the sum of the potential energy due to gravity and the elastic energy stored in springs. The potential energy due to gravity is proportional to the height of the body with respect to a reference ground. The reference used in a Rigid Dynamics analysis is the origin of the global coordinate system. Because of this, it is possible to have a negative potential energy (and negative total energy) depending on your model coordinates. The elastic energy includes only energy due to deformation of spring(s) in a rigid body dynamic analysis and is calculated as ½ * Stiffness * elongation2. External Energy: This is all the energy the loads and joints bring to a system. Total Energy: This is the sum of potential, kinetic and external energies in a Rigid Dynamics analysis. Frequency Response and Phase Response Graphs can be either Frequency Response graphs that display how the response varies with frequency or Phase Response plots that show how much a response lags behind the applied loads. Frequency Response Results displayed on a graph can be scoped to specific geometric entity (vertex, face, or edge) and can be viewed as a value graphed along a specified frequency range. These include the frequency results for stress, elastic strain, deformation, or acceleration (frequency only) plotted as a graph. The plot will include all the frequency points at which a solution was obtained. When you generate frequency response results, the default plot (Bode) shows the amplitude and phase angle. Optionally, you can plot the following results values for graphs: • Real • Imaginary • Real and Imaginary • Amplitude • Phase Angle You can select any of these from a drop-down list in the Details view for the results. For edges, faces, surface bodies, and multiple vertex selections (which contain multiple nodes), the results can be scoped as minimum, maximum, or average. This is also available for frequency and phase response results scoped on a single vertex. The Use Minimum and Use Maximum settings are based on the amplitude and thus are reported from the location with either the largest or smallest amplitude. The Use Average setting calculates the average by calculating the real and imaginary components separately. Note You cannot use the Mechanical application convergence capabilities for any results item under a harmonic analysis. Instead, you can first do a convergence study on a modal analysis and reuse the mesh from that analysis. Presented below is an example of a Frequency Response plot: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 655 Features The average, minimum, or maximum value can be chosen for selected entities. Stress, Strain, Deformation, and Acceleration components vary sinusoidally, so these are the only result types that can be reviewed in this manner. (Note that items such as Principal Stress or Equivalent Stress do not behave in a sinusoidal manner since these are derived quantities.) Phase Response Similarly, Phase Response plots show the minimum, average, or maximum Stress, Strain, or Deformation for selected entities. An example of a Phase Response plot is illustrated below. However, unlike Frequency Response plots that show a response amplitude over a frequency range, Phase Response plots show a response over a range of phase angles, so you can determine how much a response lags behind the applied load. General approach to harmonic analysis postprocessing Generally speaking, you would look at Frequency Response plots at critical regions to ascertain what the frequency of interest may be. In conjunction with Phase Response plots, the phase of interest is 656 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application also determined. Then, you can request Stress, Strain, or Deformation contour plots to evaluate the response of the entire structure at that frequency and phase of interest. Creating Contour Result from Frequency Response Results You can use Frequency Response result types (not Acceleration) to generate new result objects of the same type, orientation, frequency, and phase angle. To create a Contour Result in a Harmonic Analysis: 1. Select and right-click on the desired Harmonic result in the solution tree. 2. Choose Create Contour Result From Result. As illustrated here, you can see how the feature automatically scopes the type, orientation, frequency, and phase angle. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 657 Features The Reported Frequency in the Information category is the frequency at which contour results were found and plotted. This frequency can be potentially different from the frequency you requested. Stress Tools You can insert any of the following stress tools in a Solution object by choosing Stress Tool under Tools in the Solution context toolbar, or by using a right mouse button click on a Solution object and choosing Stress Tool: Maximum Equivalent Stress Safety Tool (p. 659) Maximum Shear Stress Safety Tool (p. 661) Mohr-Coulomb Stress Safety Tool (p. 662) Maximum Tensile Stress Safety Tool (p. 664) After adding a Stress Tool object to the tree, you can change the specific stress tool under Theory in the Details view. The Stress Tools make use of the following material properties: • Tensile Yield Strength • Compressive Yield Strength • Tensile Ultimate Strength 658 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application • Compressive Ultimate Strength Safety Tools in the ANSYS Workbench Product The ANSYS Workbench product uses safety tools that are based on four different stress quantities: 1. Equivalent stress (σe). 2. Maximum tensile stress (σ1). 3. Maximum shear stress (τMAX) This uses Mohr's circle: σ − σ3 τMAX = 1 where: σ1 and σ3 = principal stresses. 4. Mohr-Coulomb stress This theory uses a stress limit based on σ σ +
f σt σcf where: σ = inpu ensile sress limi σ =  o o     Maximum Equivalent Stress Safety Tool The Maximum Equivalent Stress Safety tool is based on the maximum equivalent stress failure theory for ductile materials, also referred to as the von Mises-Hencky theory, octahedral shear stress theory, or maximum distortion (or shear) energy theory. Of the four failure theories supported by the Mechanical application, this theory is generally considered as the most appropriate for ductile materials such as aluminum, brass and steel. The theory states that a particular combination of principal stresses causes failure if the maximum equivalent stress in a structure equals or exceeds a specific stress limit: σ ≥   Expressing the theory as a design goal: σ   < If failure is defined by material yielding, it follows that the design goal is to limit the maximum equivalent stress to be less than the yield strength of the material: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 659 Features σe y < An alternate but less common definition states that fracturing occurs when the maximum equivalent stress reaches or exceeds the ultimate strength of the material: σ u < Options Define the stress limit in the Details view under Stress Limit Type. Use either Tensile Yield Per Material, or Tensile Ultimate Per Material, or enter a Custom Value. By default, Stress Limit Type equals Tensile Yield Per Material. Choose a specific result from the Stress Tool context toolbar or by inserting a stress tool result using a right mouse button click on Stress Tool: Safety Factor lim it s= σ
Safety Margin = − =   − σ Stress Ratio σ* = σ Notes • The reliability of this failure theory depends on the accuracy of calculated results and the representation of stress risers (peak stresses). Stress risers play an important role if, for example, yielding at local discontinuities (e.g., notches, holes, fillets) and fatigue loading are of concern. If calculated results are suspect, consider the calculated stresses to be nominal stresses, and amplify the nominal stresses by an appropriate stress concentration factor Kt. Values for Kt are available in many strength of materials handbooks. • If fatigue is not a concern, localized yielding will lead to a slight redistribution of stress, and no real failure will occur. According to J. E. Shigley (Mechanical Engineering Design, McGraw-Hill, 1973), "We conclude, then, that yielding in the vicinity of a stress riser is beneficial in improving the strength of a part and that stress-concentration factors need not be employed when the material is ductile and the loads are static." • Alternatively, localized yielding is potentially important if the material is marginally ductile, or if low temperatures or other environmental conditions induce brittle behavior. 660 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application • Yielding of ductile materials may also be important if the yielding is widespread. For example, failure is most often declared if yielding occurs across a complete section. • The proper selection and use of a failure theory relies on your engineering judgment. Refer to engineering texts such as Engineering Considerations of Stress, Strain, and Strength by R. C. Juvinall (McGraw-Hill) and Mechanical Engineering Design by J. E. Shigley (McGraw-Hill) for in-depth discussions on the applied theories. Maximum Shear Stress Safety Tool The Maximum Shear Stress Safety tool is based on the maximum shear stress failure theory for ductile materials. The theory states that a particular combination of principal stresses causes failure if the Maximum Shear (p. 641) equals or exceeds a specific shear limit: τ max ≥ lim it where the limit strength is generally the yield or ultimate strength of the material. In other words, the shear strength of the material is typically defined as a fraction (f < 1) of the yield or ultimate strength: s = s − =  
τ −  In a strict application of the theory, f = 0.5. Expressing the theory as a design goal: τ <   If failure is defined by material yielding, it follows that the design goal is to limit the shear stress to be less than a fraction of the yield strength of the material: τ  < y An alternate but less common definition states that fracturing occurs when the shear stress reaches or exceeds a fraction of the ultimate strength of the material: τ  < u Options Define the stress limit in the Details view under Stress Limit Type. Use either Tensile Yield Per Material, or Tensile Ultimate Per Material, or enter a Custom Value. By default, Stress Limit Type equals Tensile Yield Per Material. Define coefficient f under Factor in the Details view. By default, the coefficient f equals 0.5. Choose a specific result from the Stress Tool context toolbar or by inserting a stress tool result using a right mouse button click on Stress Tool: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 661 Features Safety Factor s lim it = τmax Safety Margin = − = 

 τ − Stress Ratio * τ = τ  Notes • The reliability of this failure theory depends on the accuracy of calculated results and the representation of stress risers (peak stresses). Stress risers play an important role if, for example, yielding at local discontinuities (e.g., notches, holes, fillets) and fatigue loading are of concern. If calculated results are suspect, consider the calculated stresses to be nominal stresses, and amplify the nominal stresses by an appropriate stress concentration factor Kt. Values for Kt are available in many strength of materials handbooks. • If fatigue is not a concern, localized yielding will lead to a slight redistribution of stress, and no real failure will occur. According to J. E. Shigley (Mechanical Engineering Design, McGraw-Hill, 1973), "We conclude, then, that yielding in the vicinity of a stress riser is beneficial in improving the strength of the part and that stress-concentration factors need not be employed when the material is ductile and the loads are static." • Alternatively, localized yielding is potentially important if the material is marginally ductile, or if low temperatures or other environmental conditions induce brittle behavior. • Yielding of ductile materials may also be important if the yielding is widespread. For example, failure is most often declared if yielding occurs across a complete section. • The proper selection and use of a failure theory relies on your engineering judgment. Refer to engineering texts such as Engineering Considerations of Stress, Strain, and Strength by R. C. Juvinall (McGraw-Hill) and Mechanical Engineering Design by J. E. Shigley (McGraw-Hill) for in-depth discussions on the applied theories. Mohr-Coulomb Stress Safety Tool The Mohr-Coulomb Stress Safety Tool is based on the Mohr-Coulomb theory for brittle materials, also known as the internal friction theory. The theory states that failure occurs when the combination of the Maximum, Middle, and Minimum Principal (p. 640) equal or exceed their respective stress limits. The theory compares the maximum tensile stress to the material's tensile limit and the minimum compressive stress to the material's compressive limit. Expressing the theory as a design goal: σ1 ene   662 + σ3 < copreve   Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application where σ1 > σ2 > σ3; σ3 and the compressive strength limit assume negative values even though you must actually enter positive values for these quantities. Also, a given term is only used if it includes the correct sign. For example, σ1 must be positive and σ3 must be negative. Otherwise, the invalid term is assumed to be negligible. Note that the Mohr-Coulomb Stress Safety tool evaluates maximum and minimum principal stresses at the same locations. In other words, this tool does not base its calculations on the absolute maximum principal stress and the absolute minimum principal stress occurring (most likely) at two different locations in the body. The tool bases its calculations on the independent distributions of maximum and minimum principal stress. Consequently, this tool provides a distribution of factor or margin of safety throughout the part or assembly. The minimum factor or margin of safety is the minimum value found in this distribution. For common brittle materials such as glass, cast iron, concrete and certain types of hardened steels, the compressive strength is usually much greater than the tensile strength, of which this theory takes direct account. The design goal is to limit the maximum and minimum principal stresses to their ultimate strength values by means of the brittle failure relationship: σ1 ut + σ3 uc < An alternative but less common definition compares the greatest principal stresses to the yield strengths of the material: σ y + σ
y < The theory is known to be more accurate than the maximum tensile stress failure theory used in the Maximum Tensile Stress Safety tool, and when properly applied with a reasonable factor of safety the theory is often considered to be conservative. Options Define the tensile stress limit in the Details view under Tensile Limit Type. Use either Tensile Yield Per Material, or Tensile Ultimate Per Material, or enter a Custom Value. By default, Tensile Limit Type equals Tensile Yield Per Material. Define the compressive stress limit in the Details view under Compressive Limit Type. Use either Comp. Yield Per Material, or Comp. Ultimate Per Material, or enter a Custom Value. By default, Compressive Limit Type equals Comp. Yield Per Material. Choose a specific result from the Stress Tool context toolbar or by inserting a stress tool result using a right mouse button click on Stress Tool: Safety Factor   σ σ +  s =  ensile lim i ompressive lim i  − Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 663 Features Safety Margin = s s  − =  σ + 1 tensile lim it σ 3 compressive lim it    −1 − Stress Ratio σ σ = *  


 σ +   


 Notes • The use of a yield strength limit with brittle materials is not recommended since most brittle materials do not exhibit a well-defined yield strength. • For ductile and some other types of materials, experiments have shown that brittle failure theories may be inaccurate and unsafe to use. The brittle failure theories may also be inaccurate for certain brittle materials. Potential inaccuracies are of particular concern if the accuracy of calculated answers is suspect. • The reliability of this failure criterion is directly related to treatment of stress risers (peak stresses). For brittle homogeneous materials such as glass, stress risers are very important, and it follows that the calculated stresses should have the highest possible accuracy or significant factors of safety should be expected or employed. If the calculated results are suspect, consider the calculated stresses to be nominal stresses, and amplify the nominal stresses by an appropriate stress concentration factor Kt. Values for Kt are available in many strength of materials handbooks. For brittle nonhomogeneous materials such as gray cast iron, stress risers may be of minimal importance. • If a part or structure is known or suspected to contain cracks, flaws, or is designed with sharp notches or re-entrant corners, a more advanced analysis may be required to confirm its structural integrity. Such discontinuities are known to produce singular (i.e., infinite) elastic stresses; if the possibility exists that the material might behave in a brittle manner, a more rigorous fracture mechanics evaluation needs to be performed. An analyst skilled in fracture analysis can use the Mechanical APDL application to determine fracture mechanics information. • The proper selection and use of a failure theory relies on your engineering judgment. Refer to engineering texts such as Engineering Considerations of Stress, Strain, and Strength by R. C. Juvinall (McGraw-Hill) and Mechanical Engineering Design by J. E. Shigley (McGraw-Hill) for in-depth discussions on the applied theories. Maximum Tensile Stress Safety Tool The Maximum Tensile Stress Safety tool is based on the maximum tensile stress failure theory for brittle materials. The theory states that failure occurs when the maximum principal stress equals or exceeds a tensile stress limit. Expressing the theory as a design goal: σ  <   The maximum tensile stress failure theory is typically used to predict fracture in brittle materials with static loads. Brittle materials include glass, cast iron, concrete, porcelain and certain hardened steels. 664 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application The design goal is to limit the greatest principal stress to be less than the material's ultimate strength in tension: σ1 < ut An alternate definition compares the greatest principal stress to the yield strength of the material: σ < y
For many materials (usually ductile materials), strength in compression and in tension are roughly equal. For brittle materials, the compressive strength is usually much greater than the tensile strength. The Mohr-Coulomb theory used in the Mohr-Coulomb Stress Safety tool is generally regarded as more reliable for a broader range of brittle materials. However, as pointed out by R. C. Juvinall (Engineering Considerations of Stress, Strain, and Strength, McGraw-Hill, 1967), "There is some evidence to support its use with porcelain and concrete. Also, it has been used in the design of guns, as some test results on thick-walled cylinders tend to agree with this theory." Options Define the stress limit in the Details view under Stress Limit Type. Use either Tensile Yield Per Material, or Tensile Ultimate Per Material, or enter a Custom Value. By default, Stress Limit Type equals Tensile Yield Per Material. Choose a specific result from the Stress Tool context toolbar or by inserting a stress tool result using a right mouse button click on Stress Tool: Safety Factor lim i s= σ Safety Margin = − =   − σ Stress Ratio σ* = σ  Notes • The use of a yield strength limit with brittle materials is not recommended since most brittle materials do not exhibit a well-defined yield strength. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 665 Features • For ductile and some other types of materials, experiments have shown that brittle failure theories may be inaccurate and unsafe to use. The brittle failure theories may also be inaccurate for certain brittle materials. Potential inaccuracies are of particular concern if the accuracy of calculated answers is suspect. • The reliability of this failure criterion is directly related to treatment of stress risers (peak stresses). For brittle homogeneous materials such as glass, stress risers are very important, and it follows that the calculated stresses should have the highest possible accuracy or significant factors of safety should be expected or employed. If the calculated results are suspect, consider the calculated stresses to be nominal stresses, and amplify the nominal stresses by an appropriate stress concentration factor Kt. Values for Kt are available in many strength of materials handbooks. For brittle nonhomogeneous materials such as gray cast iron, stress risers may be of minimal importance. • If a part or structure is known or suspected to contain cracks, flaws, or is designed with sharp notches or re-entrant corners, a more advanced analysis may be required to confirm its structural integrity. Such discontinuities are known to produce singular (i.e., infinite) elastic stresses; if the possibility exists that the material might behave in a brittle manner, a more rigorous fracture mechanics evaluation needs to be performed. An analyst skilled in fracture analysis can use the Mechanical APDL application program to determine fracture mechanics information. • The proper selection and use of a failure theory relies on your engineering judgment. Refer to engineering texts such as Engineering Considerations of Stress, Strain, and Strength by R. C. Juvinall (McGraw-Hill) and Mechanical Engineering Design by J. E. Shigley (McGraw-Hill) for in-depth discussions on the applied theories. Fatigue (Fatigue Tool) See Fatigue Overview. Contact Tool The Contact Tool allows you to examine contact conditions on an assembly both before loading, and as part of the final solution to verify the transfer of loads (forces and moments) across the various contact regions. The Contact Tool is an object you can insert under a Connections branch object for examining initial contact conditions, or under a Solution or Solution Combination branch object for examining the effects of contact as part of the solution. The Contact Tool allows you to conveniently scope contact results to a common selection of geometry or contact regions. In this way, all applicable contact results can be investigated at once for a given scoping. A Contact Tool is scoped to a given topology, and there exist two methods for achieving this: the Worksheet method and the Geometry Selection method. Under the Worksheet method, the Contact Tool is scoped to one or more contact regions. Under the Geometry Selection method, the Contact Tool can be scoped to any geometry on the model. Regardless of the method, the scoping on the tool is applied to all results grouped under it. To use a Contact Tool, prepare a structural analysis for an assembly with contacts. You then use either the Geometry Selection or Worksheet scoping method for results. Evaluating Initial Contact Conditions To evaluate initial contact conditions using the Worksheet method: 1. 666 Insert a Contact Tool in the Connections folder (Contact Tool from the Connections context toolbar, or right mouse button click on Connections, then Insert> Contact Tool). You will see a Contact Tool inserted that includes a default Initial Information object. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application 2. In the Details view of the Contact Tool, ensure that Worksheet (the default) is selected in the Scoping Method field. The Worksheet appears. Scoped contact regions are those that are checked in the table. 3. You can modify your selection of contact regions in the Worksheet using the following procedures: • To add or remove pre-selected groups of contact regions (All Contacts, Nonlinear Contacts, or Linear Contacts), use the drop-down menu and the corresponding buttons. • To add any number of contact regions, you can also drag-drop or copy-paste any number of contact regions from the Connections folder into the Contact Tool in the Tree View. Also, one or more contact regions can be deleted from the Contact Tool worksheet by selecting them in the table and pressing the Delete key. • To change the Contact Side of all contact regions, choose the option in the drop-down menu (Both, Contact, or Target from the drop-down menu and click the Apply button). • To change an individual Contact Side, click in the particular cell and choose Both, Contact, or Target from the drop-down menu. 4. Add contact result objects of interest under the Contact Tool folder (Contact> Penetration or Gap or Status from the Contact Tool context toolbar, or right mouse button click on Contact Tool, then Insert> Penetration or Gap or Status). The specific contact result objects are inserted. 5. Obtain the initial contact results using a right mouse button click on the Contact object, or Contact Tool object, or any object under the Contact Tool object, then choosing Generate Initial Contact Results from the context menu. Results are displayed as follows: • When you highlight the Initial Information object, a table appears in the Worksheet that includes initial contact information for the contact regions that you specified in step 2 above. You can display or hide the various columns in the table. The table rows display in various colors that indicate the detected contact conditions. A brief explanation of each color is provided in the legend that is displayed beneath the table. Copies of the legend explanations are presented below in quotes, followed by more detailed explanations. – Red: "The contact status is open but the type of contact is meant to be closed. This applies to bonded and no separation contact types." Workbench has detected an open contact Status condition, which is invalid based on the definitions of Bonded and No Separation contact types. It is very likely that the model will not be held together as expected. The geometry of the contact may be too far apart for the closed condition to be satisfied. Review of the Contact Region definition is strongly recommended. – Yellow: "The contact status is open. This may be acceptable." Workbench has detected an open contact Status condition on a nonlinear contact type, Frictionless, Rough, or Frictional, which is probably acceptable under certain conditions as stated in their descriptions. If the Status is Far Open, the Penetration and the Gap will be set to zero even though the Resulting Pinball is non-zero. Note Currently, contact results are not saved to results (.rst) file for all contact elements that are outside the pinball region to optimize the file size. Results for far field contact elements were reported as zero in prior releases. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 667 Features – Orange: "The contact status is closed but has a large amount of gap or penetration. Check penetration and gap compared to pinball and depth.” Workbench has detected that any of the following contact results are greater than 1/2 of the Resulting Pinball, or greater than 1/2 of the Contact Depth: Gap, Penetration, maximum closed Gap, maximum closed Penetration. This could lead to poor results in terms of stiffness of the contacting interface. It is recommended that you alter the geometry to reduce the gap or penetration. – Gray: "Contact is inactive. This can occur for MPC and Normal Lagrange formulations. It can also occur for auto asymmetric behavior." Refer to the individual descriptions for the MPC and Normal Lagrange formulations, and the description for Auto Asymmetric behavior. Note The “not applicable” designation, N/A appears in the following locations and situations: • • All result columns when the contact pair is inactive (row is gray, or Inactive appears under the Status column). • The Geometric Gap column for Frictionless, Rough, or Frictional contact Types and an Interface Treatment set to Add Offset. When you highlight any of the contact result objects, the Geometry tab appears and displays the graphical result for the contact regions that you specified in step 2 above. To evaluate initial contact conditions using the Geometry Selection method: 1. Select one or more bodies that are in contact. 2. Insert a Contact Tool in the Connections folder (Contact Tool from the Connections context toolbar, or right mouse button click on Connections, then Insert> Contact Tool). You will see a Contact Tool inserted that includes a default Initial Information object. Note The scoping of the Initial Information object is only available using the Worksheet method. Selecting bodies as in step 1 above has no effect on Initial Information results. 3. In the Details view of the Contact Tool, select Geometry Selection in the Scoping Method field. The bodies that you selected in step 1 are highlighted in the Geometry tab. 4. Add contact result objects of interest under the Contact Tool folder (Contact> Penetration or Gap or Status from the Contact Tool context toolbar, or right mouse button click on Contact Tool, then Insert> Penetration or Gap or Status). The specific contact result objects are inserted. 5. Obtain the initial contact results using a right mouse button click on the Contact object, or Contact Tool object, or any object under the Contact Tool object, then choosing Generate Initial Contact Results from the context menu. When you highlight any of the contact result objects, the Geometry tab appears and displays the graphical result for the bodies that you selected in step 1. 668 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Evaluating Contact Conditions After Solution Note The default method will be the last one that you manually chose in the Scoping Method drop down menu. If you have already selected geometry, the Scoping Method field automatically changes to Geometry Selection. The default however will not change until you manually change the Scoping Method entry. To evaluate contact conditions after solution using the Worksheet method: 1. Insert a Contact Tool in the Solution folder (Tools> Contact Tool from the Solution context toolbar, or right mouse button click on Solution, then Insert> Contact Tool> Contact Tool). You will see a Contact Tool inserted with a default contact result. 2. In the Details view, select Worksheet in the Scoping Method field. The Worksheet appears. Scoped contact regions are those that are checked in the table. 3. You can modify your selection of contact regions in the Worksheet using the following procedures: • To add or remove pre-selected groups of contact regions (All Contacts, Nonlinear Contacts, or Linear Contacts), use the drop-down menu and the corresponding buttons. • To add any number of contact regions, you can also drag-drop or copy-paste any number of contact regions from the Contact folder into the Contact Tool in the Tree View. Also, one or more contact regions can be deleted from the Contact Tool worksheet by selecting them in the table and pressing the Delete key. • To change the Contact Side of all contact regions, choose the option in the drop-down menu (Both, Contact, or Target from the drop-down menu and click the Apply button). • To change an individual Contact Side, click in the particular cell and choose Both, Contact, or Target from the drop-down menu. 4. Add more contact results as needed in the Contact Tool folder (Contact> [Contact Result, for example, Pressure] from the Contact Tool context toolbar, or right mouse button click on Contact Tool, then Insert> [Contact Result, for example, Pressure]). 5. Solve database. Upon completion, you will see contact results with the common scoping of the Contact Tool. To evaluate contact conditions after solution using the Geometry Selection method: 1. Select one or more bodies that are in contact. 2. Insert a Contact Tool in the Solution folder (Tools> Contact Tool from the Solution context toolbar, or right mouse button click on Solution, then Insert> Contact Tool> Contact Tool). You will see a Contact Tool inserted with a default contact result. Because you have already selected one or more bodies, Geometry Selection is automatically set in the Scoping Method field within the Details view. 3. Add more contact results as needed in the Contact Tool folder (Contact> [Contact Result, for example, Pressure] from the Contact Tool context toolbar, or right mouse button click on Contact Tool, then Insert> [Contact Result, for example, Pressure]). 4. Solve database. Upon completion, you will see contact results with the common scoping of the Contact Tool. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 669 Features The configuration of the Contact Tool, in particular the location (Solution vs Solution Combination) and the scoping method, affects the availability of results. A Contact Tool in the Solution Combination folder has the limitation that it supports only pressure, frictional stress, penetration and distance. Contact Tool Initial Information When a Contact Tool is inserted under the Connections object, it includes a default object, Initial Information. This object provides the following information from the Worksheet. • Name: Contact Region name. • Contact Side: Selected contact side, either Contact or Target. • Type: contact type, Bonded, No Separation, Frictionless, Rough, Frictional. • Status: the status of the contact, Open, Closed, Far Open. • Number Contacting: the number of contact or target elements in contact. • Penetration: the resulting penetration. • Gap: the resulting gap. • Geometric Gap: the gap that initially exists between the Contact and Target surfaces. For Frictional or Frictionless contact, this is the minimum gap. For Bonded or No Separation contact, this is the maximum closed gap detected. • Geometric Penetration: the penetration that initially exists between the Contact and Target surfaces. • Resulting Pinball: user specified or the Mechanical APDL application calculated pinball radius. • Contact Depth: average contact depth of elements. • Normal Stiffness: the calculated maximum normal stiffness value. • Tangential Stiffness: the calculated maximum tangential stiffness value. • Real Constant: the contact Real Constant number. Beam Tool You can apply a Beam Tool to any assembly in order to view the linearized stresses on beam bodies. It is customary in beam design to employ components of axial stress that contribute to axial loads and bending in each direction separately. Therefore, the stress outputs (which are linearized stresses) associated with beam bodies have been focused toward that design goal. The Beam Tool is similar to the Contact Tool in that the tool, not the results themselves control the scoping. By default, the scoping is to all beam bodies. You can change the scoping in the Details view, if desired. To insert a Beam Tool, highlight the Solution object then choose Tools> Beam Tool from the Solution context toolbar. Three beam stress results are included under the Beam Tool object: Direct Stress, Minimum Combined Stress, and Maximum Combined Stress. You can add additional beam stress results or deformation results by highlighting the Beam Tool object and choosing the particular result from the Beam Tool context toolbar. As an alternative, you can right mouse button click on the Beam Tool object and, from the context menu, choose Insert> Beam Tool> Stress or Deformation. Presented below are definitions of the beam stress results that are available: • 670 Direct Stress: The stress component due to the axial load encountered in a beam element. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application • Minimum Bending Stress: From any bending loads a bending moment in both the local Y and Z directions will arise. This leads to the following four bending stresses: Y bending stress on top/bottom and Z bending stress the top/bottom. Minimum Bending Stress is the minimum of these four bending stresses. • Maximum Bending Stress: The maximum of the four bending stresses described under Minimum Bending Stress. • Minimum Combined Stress: The linear combination of the Direct Stress and the Minimum Bending Stress. • Maximum Combined Stress: The linear combination of the Direct Stress and the Maximum Bending Stress. Structural Probes The following structural probe types are available. Probe Type Deformation Applicable Analysis Types Output Static Structural, Transient Structural, Rigid Dynamics, Explicit Dynamics Deformation: X axis, Y axis, Z axis, Total Characteristics Scope to: flexible or rigid body. Scope by: bodies (single body only if rigid), location only, vertex, edge, face. Orientation coordinate system: any; defaults to Global Cartesian. Strain Stress Static Structural, Transient Structural, Explicit Dynamics Static Structural, Transient Structural, Explicit Dynamics Strain: Components, Principals, Normal X, Normal Y, Normal Z, XY Shear,YZ Shear, XZ Shear, Minimum Principal, Middle Principal, Maximum Principal, Intensity, Equivalent (vonMises) Scope to: flexible body only. Stress: Components, Principals, Normal X, Normal Y, Normal Z, XY Shear,YZ Shear, XZ Shear, Minimum Scope to: flexible body only. Scope by: bodies, location only, vertex, edge, face. Orientation coordinate system: any; defaults to Global Cartesian. Scope by: bodies, location Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 671 Features Probe Type Position Applicable Analysis Types Static Structural, Transient Structural, Rigid Dynamics, Explicit Dynamics Output Characteristics Principal, Middle Principal, Maximum Principal, Intensity, Equivalent (vonMises) only, vertex, edge, face. Position: X axis,Y axis , Z axis Scope to: rigid body only. Orientation coordinate system: any; defaults to Global Cartesian. Scope by: bodies, coordinate system. Orientation coordinate system: any; defaults to Global Cartesian. Velocity Transient Structural, Rigid Dynamics, Explicit Dynamics Velocity: X axis,Y axis, Z axis Scope to: flexible or rigid body. Scope by: bodies (single body only if rigid), coordinate system (rigid bodies only), location only, vertex, edge, face. Orientation coordinate system: any; defaults to Global Cartesian. Angular Velocity Transient Structural, Rigid Dynamics, Angular Velocity: X axis,Y axis, Z axis Scope to: rigid body only. Scope by: bodies. Orientation coordinate system: any; defaults to Global Cartesian. 672 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Probe Type Acceleration Applicable Analysis Types Output Transient Structural, Rigid Dynamics, Explicit Dynamics Acceleration: X axis, Y axis, Z axis Characteristics Scope to: flexible or rigid body. Scope by: bodies (single body only if rigid), coordinate system (rigid bodies only), location only, vertex, edge, face. Orientation coordinate system: any; defaults to Global Cartesian. Angular Acceleration Transient Structural, Rigid Dynamics Angular Acceleration: X axis,Y axis, Z axis Scope to: rigid body only. Scope by: bodies. Orientation coordinate system: any; defaults to Global Cartesian. Energy Force Reaction2 Static Structural, Transient Structural, Rigid Dynamics Static Structural, Transient Structural, Modal, Harmonic, Random Vibration, Response Spectrum For Static Structural and Transient Structural analyses: Kinetic, Strain. Scope to: flexible or rigid body. Scope by: For Rigid Dynamics analyses: Kinetic, Potential, External, Total. • System or per body for Kinetic, Potential, Strain. • System only for External and Total. Force Reaction: X axis,Y axis, Z axis Scope to: flexible body only. Scope by: boundary condition, contact region. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 673 Features Probe Type Applicable Analysis Types Output Characteristics Orientation coordinate system: any Cartesian; defaults to Global Cartesian. Only Solution Coordinate System is valid for Random Vibration and Response Spectrum. Moment Reaction2 Static Structural, Transient Structural, Modal, Harmonic, Random Vibration, Response Spectrum Moment Reaction: X axis,Y axis, Z axis Scope to: flexible body only. Scope by: boundary condition, contact region. Orientation coordinate system: any Cartesian; defaults to Global Cartesian. Only Solution Coordinate System is valid for Random Vibration and Response Spectrum. Summation point: centroid or orientation coordinate system. Joint Transient Structural, Rigid Dynamics See Joint Probes. Scope to: joint only. Orientation coordinate system: joint reference only for all outputs except Force and Moment. Use 674 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Probe Type Applicable Analysis Types Output Characteristics any coordinate system for these. Only Cartesian coordinate systems are valid for all Joint probes. Summation point: always at joint for Moment. Response PSD1 Random Vibration X axis,Y axis, and Z axis. Scope to: flexible body only. Displacement, Stress, Strain, Acceleration, Velocity Scope by: location only and vertex. Orientation Coordinate System: Only Solution Coordinate System is valid for Random Vibration. Spring Static Structural, Transient Structural, Rigid Dynamics Elastic Force, Damping Force, Elongation, Velocity. Scope to: spring only. Orientation coordinate system: spring axis only. Beam Static Structural, Transient Structural, Rigid Dynamics Axial Force, Torque, Shear Force at I, Shear Force at J, Moment at I, and Moment at J. Boundary Condition: Select beam. Bolt Pretension Static Structural, Transient Structural Adjustment, Tensile Force Scope by: boundary condition (Y pretension bolt condition). Orientation coordinate system: along pre- Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 675 Features Probe Type Applicable Analysis Types Output Characteristics tension direction only. Generalized Plane Strain 2-D: Static Structural, Transient Structural Rotation: X,Y; Moment: X,Y; Fiber Length Change; Force Orientation coordinate system: any; defaults to Global Cartesian. 1 - The Response PSD Probe provides an excitation response plot across the frequency domain of an input PSD load. It also evaluates the root mean square (RMS) of a response PSD. It is assumed that the excitations are stationary random processes from the input PSD values. 2 - The contact region based force and moment reactions are not supported for Modal and Harmonic analysis. Differences in Probes Applied to Rigid Bodies The following table describes the differences between probes applied to rigid bodies in an Explicit Dynamics analysis, compared to probes applied to rigid bodies in a Static Structural or Transient Structural analysis. Characteristic Explicit Dynamics Analysis Static Structural or Transient Structural Analysis How rigid part is meshed Meshed with solid element containing multiple nodes. Meshed as a single element containing a single node. Centroid of the rigid part Need not be represented by any node in the mesh.The Mechanical application computes the part centroid by averaging the element centroids. Each element centroid is the average of the element's nodes. Results at the single node represent the displacement, velocity, etc. at the centroid of the part. Display of minimum and maximum results Probe applied to rigid body displays both the minimum and maximum results at a given time because there are multiple elements and nodes reporting results. Probe applied to rigid body does not display both the minimum and maximum results at a given time because there is only one element and one node reporting results. The position probe represents the sum of the minimum (or maximum) displacement with the average nodal coordinate. More Information on Probes See the Probes (p. 737) section for further information. In addition, see the following sections for details on these probe types: Joint Probes Response PSD Probe Spring Probes 676 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Beam Probes Joint Probes The joint type determines which results will be available for that joint. Please refer to the Types of Joints (p. 436) section for a discussion of joint types and the free degrees of freedom. The following table presents each of the joint probe results available through the Result Type drop down menu in the Details view. Joint Probe Result Type Applicable Joint Type(s) Total Force All Total Moment All except Slot and Spherical Relative Displacement All except Revolute, Universal, and Spherical Relative Velocity All except Revolute, Universal, and Spherical Relative Acceleration All except Revolute, Universal, and Spherical Relative Rotation All except Translational Relative Angular Velocity All except Translational Relative Angular Acceleration All except Translational Damping Force Bushing Damping Moment Revolute, Cylindrical, and Bushing Constraint Force Revolute, Cylindrical, and Bushing Constraint Moment Revolute, Cylindrical, and Bushing Elastic Moment Revolute, Cylindrical, and Bushing Elastic Force Bushing Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 677 Features Note 678 • A joint defines the interface between two bodies. One of the bodies is referred to as a reference body and the other as the mobile body. The results from the joint measure the relative motion of the mobile body with respect to the reference body. • A joint definition also includes specification of a local “reference” coordinate system for that joint. All results from the joint are output in this reference coordinate system. • The reference coordinate system moves with the reference body. Depending on the motion of the reference body it might be difficult to interpret the joint results. • All of these results have X, Y, and Z components in the reference coordinate system. • Relative rotation is expressed in Euler angles. When all three rotations are free, the general joint cannot report an angle that accounts for the number of turns. A typical behavior will be to switch from +π radians to -π radians for increasing angles passing the π limit, as illustrated below. • For spherical and general joints the output of relative rotations is characterized by the Cardan (or Bryant) angles; the rotation around the joint Y axis is limited to between -90 degrees to +90 degrees. When this rotation magnitude value reaches 90 degrees, the output may “jump” to the opposite sign. • The convention for the deformations differs for joints in a Rigid Dynamics analysis vs. those in a Transient Structural analysis. For the Rigid Dynamics type, the reference of zero deformation is taken after the model has been assembled, and the initial conditions have been applied. For the Transient Structural analysis type, the initial location of bodies is used as reference, before applying initial conditions. • When you request a force or moment at a specific time point by setting Display time = time value in the Details view of a Joint probe, the force or moment will be displayed by an arrow in the Geometry window. Force will use a single arrowhead and moment will use double arrowhead. • Joints compute no reactions forces or moments for the free degrees of freedom of the joint. However, Displacement, Velocity, Acceleration, Rotation, Rotational Velocity and Rotational Acceleration conditions - generate forces and moments, that are reported in the constraint force and moment. • Joint forces and moment conditions are not reported in the joint force and moment probe. • Joint force and moment are by definition the action of the moving body on the reference body. For the ANSYS solver, the joint constraint forces and moments are reported in the joint reference coordinate system. The elastic forces/moments and damping forces/moments in the joints are reported in the reference and mobile axes of the joint which follow the displacements and rotations of the underlying nodes of the joint element. When using the ANSYS Rigid Dynamics solver, the joint forces and moments components are always reported in the joint reference coordinate system. • Joint force and moment probes are not supported for Body-Body fixed joints between 2 rigid bodies in a Transient Structural analysis, which uses the ANSYS solver. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Response PSD Probe The Response PSD Probe provides a spectrum response of a structural component subjected to a random excitation. Response PSD is plotted as square of spectrum response over excitation frequency range. The plot provides an information as to where the average power is distributed as a function of frequency. The square root of the area under the response PSD is the so-called root-mean-square (RMS) value. It is a one-sigma, or one-standard-deviation, value in a statistical term. The Details View properties and selections for the Response PSD object are described below. Property Control Description Definition Type Read-only control - only Response PSD is allowed for this result. Location Method The response PSD is a point based result.The location of the point can be provided using geometry selection or coordinate system. For the geometry selection, only vertex is allowed for the selection. For the coordinate system, a local/customized coordinate system defining a certain location can be used for evaluation of the response PSD. It can also be scoped to a Remote Point if there is one defined in geometry. Geometry Appears if Scoping Method is set to Geometry Selection. Orientation Read-only control - only Solution Coordinate System is allowed for this result. Location Appears if Location Method is set to Coordinate System. X Coordinate Read-only field that displays coordinate that is based on the Location property of the coordinate system. Y Coordinate Read-only field that displays coordinate that is based on the Location property of the coordinate system. Z Coordinate Read-only field that displays coordinate that is based on the Location property of the coordinate system. Reference Two options are available for the response PSD result evaluation; Relative to base motion (or relative motion) and Absolute (including base motion). For the Relative to base motion, the response of any location in a structural component is calculated in term of a relative motion between the base and the structural component, and vice versa. Remote Points Appears if Location Method is set to Remote Points. Suppressed Include (No) or exclude (Yes) the result in the analysis. Result Type Result Type: The result types include three basic motion characteristics (Displacement, Velocity and Acceleration), Stress (including normal and shear) and Strain (including normal and shear). Result Selection Defines the direction, in Solution Coordinate System, in which response specified in the result type is calculated. RMS Value Read-only field that displays value calculated during solution. Options Results Spring Probes You can use a probe to display the following longitudinal result items from a spring. Elastic Force: The force is calculated as (Spring Stiffness * Elongation). The force acts along the length of the spring. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 679 Features Damping Force: Damping force is calculated as (Damping Factor * velocity) and acts to resist motion. Elongation: The elongation is the relative displacement between the two ends of the springs. The elongation could be positive (stretching the spring) or negative (compressing the spring). Velocity: Velocity is the rate of stretch (or compression) of the spring. This quantity is only calculated in a Transient Structural or Rigid Dynamics analysis. Beam Probes The Beam Probe results provide you the forces and moments in the beam from your analysis. Using the Beam Probe you can determine the Axial Force, Torque, Shear Force at I, Shear Force at J, Moment at I, Moment at J. You can also add the Force reaction and Moment Reaction probes to view reaction force moment for the beam. To add beam probes: 1. In the Project Tree, click Solution to make the Solution toolbar available. 2. On the Solution toolbar, click Probe, and then click Beam to add the Beam Probe under Solution. 3. In the Details view, under Definition, click the Boundary Condition list and click the beam you want to analyze. 4. Under Options, in the Result Selection list, click the result you want to calculate. Beam Results Beam results can be applied only to line body edges and are defined as follows in reference to the solution coordinate system of each beam or pipe element: • Axial Force: the force along a beam element axis (X component). • Bending Moment: the moment in the plane perpendicular to the beam element axis (Y and Z components). • Torsional Moment: the moment about the beam element axis (X component). • Shear Force: the force perpendicular to the beam element axis (Y and Z components). • Shear-Moment Diagram: simultaneously illustrates the distribution of shear forces, bending moments and displacements, as a function of arc length along a path consisting of line bodies. To apply a beam result, define a path by using edges, on the line body edges as described in “Defining a Path using an Edge” in Path (Construction Geometry) (p. 376). For Shear-Moment Diagrams, the defined line body edges must be contiguous. Note 680 • User Defined Result equivalents of the above results are BEAM_AXIAL_F, BEAM_BENDING_M, BEAM_TORSION_M, and BEAM_SHEAR_F. • An Axial Force display will not include an arrow (that is, a vector). The force consists of only the X component. A positive force denotes tension; a negative force denotes compression. • If a path is coincident with an edge, beam results from scoping to the path may not match beam results from scoping to the edge. The path for beams only allows contributions from beam elements with both endpoints in the path. An edge can allow contributions from elements that have only one node on the edge. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Shear-Moment Diagram A shear-moment diagram is a beam result that you can apply only to paths, which simultaneously illustrates the distribution of shear forces, bending moments and displacements, as a function of arc length along the path consisting of line bodies. These three quantities are included in a shear-moment diagram because they are so closely related. For example, the derivative of the moment is the shear: dM/dx = V(x) You can pre-define the path by selecting a contiguous set of line body edges, then inserting a ShearMoment Diagram object in the tree. Insert from the Beam Results drop down menu on the Solution context toolbar, or by a right-click on the Solution folder and choosing Insert> Beam Results from the context menu. With the Shear-Moment Diagram object highlighted, the Path, Type and Graphics Display settings in the Details view control the curves you can display in the Worksheet or the Graph window. Descriptions are presented below. When the X, Y, or Z component is indicated, they are in the local coordinate system whose X axis is directed instantaneously along the beam. The Y and Z axes can be inspected using an Element Triad result. All Type and Graphics Display directions are referenced to this axis. • Path: The specific path to which the shear-moment diagram is to apply. For ease of use, before inserting the Shear-Moment Diagram object, you can define the path by selecting a contiguous set of line body edges. You can choose to use this path or any other pre-defined paths that you have created for other path results. • Type: The shear-moment diagram to display. Choices are: • – Total Shear-Moment Diagram – Directional Shear-Moment Diagram (VY-MZ-UY) – Directional Shear-Moment Diagram (VZ-MZ-UZ) Graphics Display: Controls which quantity is plotted in the Graph window and reported as Minimum and Maximum values in the Details view. Example in Worksheet: You can toggle the display of all the Max and Min annotation labels by right-clicking anywhere in the top diagram and choosing Hide/Show Annotation Labels. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 681 Features Example in Graph and Tabular Data Windows: Example of Tracking Graph with Path Position: When you click anywhere along the Length axis, the vertical bar and length that display corresponds to the position of the + annotation on the path as shown below. Gasket Results Gasket results are structural results associated with ANSYS interface elements. When used with ANSYS structural elements, interface elements simulate an interface between two materials. The behavior at these interfaces is highly nonlinear. 682 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application To mesh a body using interface elements, highlight the Body object in the tree and set Stiffness Behavior to Gasket. The following gasket results are available in the Mechanical Application: • Normal Gasket Pressure - corresponding to Mechanical APDL command PLNSOL,GKS,X • Shear Gasket Pressure - corresponding to Mechanical APDL commands PLNSOL,GKS,XY and PLNSOL,GKS,XZ • Normal Gasket Total Closure - corresponding to Mechanical APDL command PLNSOL,GKD,X • Shear Gasket Total Closure - corresponding to Mechanical APDL commands PLNSOL,GKD,XY and PLNSOL,GKD,XZ These results are only available in the solution coordinate system. Campbell Diagram Chart Results A Campbell diagram chart result is only valid in modal analyses. The Campbell diagram chart result is mainly used in rotor dynamics for rotating structural component design. When a structural component is rotating, an inertial force is introduced into the system. The dynamic characteristics of the structural component change as a result of the inertia effect, namely, gyroscopic effect. To study changes in dynamic characteristics of a rotating structure, more than one solve point in Rotational Velocity is required. To insert a Campbell diagram chart result, highlight the Solution object in the tree, then select Campbell Diagram from the Solution Context Toolbar, or right click on the object and choose Insert > Campbell Diagram. The following is an example of a Campbell diagram result chart: In this chart, each line represents a frequency evolution of a whirl mode with respect to increased rotational velocities. The whirl frequency value of an eigenmode at each rotational velocity is also listed in Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 683 Features the table. For each whirl mode, it is either labeled as forward (FW) or backward (BW) whirl direction. In some cases, when there is no evident whirl direction, the whirl frequency is labeled as UNDETERMINED. If a whirl mode is identified as FW, the rotating structural component whirls the same direction as the rotation direction, and vice versa. If a whirl mode is evaluated to be unstable (marked as UNSTABLE), the whirl orbit will evolve into a divergent trajectory, instead of an elliptical trajectory. In addition to whirl modes, a line (black color) of any ratio between whirl frequency and rotational velocity is plotted. The intersection between this line and each whirl mode is indicated with a red triangular marker. The rotational velocity corresponding to this intersection is called critical speed. At critical speed, the rotating structural component will experience a peak as the rotating frequency resonates with the natural whirl frequency. The Campbell diagram chart result can be customized in Details of Campbell Diagram as follows: Scope • Rotational Velocity Selection: It is a drop-down menu allows users to select a rotational velocity for which the Campbell diagram chart result is evaluated. The default is None. Campbell Diagram Controls • Y Axis Data: There are three data types available for selection; Frequency, Stability and Logarithmic Decrement. The default is Frequency. • Critical Speed: Option for users to display critical speeds. The default is No. When it is set to Yes, users are prompted to provide a value in the Ratio field below. The option is only valid for frequency. • Ratio: Value used to evaluate critical speeds. The default value is 1.0. • Sorting: Option to display data in a sorted mode manner when some modes are crossing/intercepting each other. The default is Yes. Note Any change made in these fields requires a result re-evaluation. Axis Note Two different unit types, rad/s and RPM, are available to define rotational velocity in the chart. The selection can be made in Units toolbar. 684 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application • X Axis Label: Allows users to provide a customized label for rotational velocity. • X Axis Range: There are two options to display the rotational velocity data range; Program Controlled and Specified. The default is Program Controlled, which uses minimum and maximum determined by the system. The option of Specified allows users to provide a customized range to be used in the chart. The minimum and maximum values are displayed in the X Axis Minimum and X Axis Maximum fields below after result evaluation is done. • X Axis Minimum: Minimum rotational velocity value is displayed according to the selection made in X Axis Range. • X Axis Maximum: Maximum rotational velocity value is displayed according to the selection made in X Axis Range. • Y Axis Label: Allows users to provide a customized label for frequency, stability or logarithmic decrement depending on the selection made in Y Axis Data. • Y Axis Range: There are two options, Program Controlled and Specified, to display the frequency, stability or logarithmic value range depending on the selection made in Y Axis Data. The default is Program Controlled, which uses minimum and maximum determined by the system. The option of Specified allows users to provide a customized range to be used in the chart. The minimum and maximum values are displayed in the Y Axis Minimum and Y Axis Maximum fields below after result evaluation is done. • Y Axis Minimum: Minimum frequency, stability or logarithmic decrement value is displayed according to the selection made in Y Axis Range. • Y Axis Maximum: Maximum frequency, stability or logarithmic decrement value is displayed according to the selection made in Y Axis Range. Thermal Results The following thermal result topics are addressed in this section: Temperature Heat Flux Heat Reaction Error (Thermal) Thermal Probes Thermal Probes (p. 687) can be used to determine the following results: • Temperature • Heat Flux • Heat Reaction Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 685 Features Temperature In a steady-state or transient thermal analysis, temperature distribution throughout the structure is calculated. This is a scalar quantity. Scoping allows you to limit the temperature display to particular geometric entities. Similarly scoping allows you to get reactions at specific boundary condition objects. Temperature results can be displayed as a contour plot. You can also capture the variation of these results with time by using a probe. Heat Flux The Mechanical application calculates the heat flux (q/A, energy per unit time per unit area) throughout the body. Heat flux can be output as individual vector components X, Y or Z. You can display the X, Y, and Z components of heat flux in different coordinate systems. Scoping allows you to limit the heat flux display to particular geometric entities. Similarly scoping allows you to get reactions at specific boundary condition objects. Heat flux results can be displayed as a contour plot. You can also capture the variation of these results with time by using a probe. Plots of Vector Heat Flux A Vector Heat Flux plot provides the direction of heat flux (relative magnitude and direction of flow) at each point in the body. The following graphic illustrates an example showing a high temperature area at the top and a low temperature area at the bottom. Note the direction of the heat flow as indicated by the arrows. Request Vector Heat Flux plots in the same way that you would request any other result. After inserting the result object in the tree and solving, click the Graphics button in the Result context toolbar. 686 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Heat Reaction You can obtain heat reaction (q, energy per unit time) at locations where a temperature, convection or radiation boundary condition is specified. Heat reaction is a scalar. To obtain a heat reaction result, insert a Reaction probe and specify an existing Boundary Condition. See Thermal Probes (p. 687) for more information. Error (Thermal) The description of this result is the same as Error (Structural) except that heat flux is the basis for the errors instead of stresses. Thermal Probes The following thermal probe types are available. Probe Type Temperature Applicable Analysis Types Output Steady-state thermal, transient thermal Temperature: overall Characteristics Scope to: body. Scope by: bodies, location only, vertex, edge, face. Heat Flux Steady-state thermal, transient thermal Heat Flux: X axis,Y axis, Z axis Scope to: body. Scope by: bodies, location only, vertex, edge, face. Orientation coordinate system: any; defaults to Global Cartesian. Heat Reaction Steady-state thermal, transient thermal Heat: overall Scope to: body. Scope by: boundary condition. Radiation1 Steady-state thermal, transient thermal Net Radiation, Emitted Radiation, Reflected Radiation, Incident Radiation Scope to: face. Scope by: boundary condition (Radiation loads with Sur- Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 687 Features Probe Type Applicable Analysis Types Output Characteristics face-to-Surface correlation). 1 - For 2-D plane stress models the Radiosity Solver method assumes an infinite third dimension so the Radiation Probe results will be proportional to the Workbench model thickness. See the Probes (p. 737) section for further information. Magnetostatic Results A magnetostatic analysis offers several results items for viewing. Results may be scoped to bodies and, by default, all bodies will compute results for display. You can use the Details view to view vector results in several ways. Magnetic Flux Density, Magnetic Field Intensity, and Force represent the magnitude of the results vector and can be viewed as a contour or as a directional vector. Any directional solution represents direction vector components (X, Y, Z) of the vector. They may be displayed as a contour. The following electromagnetic result topics are addressed in this section: Electric Potential Total Magnetic Flux Density Directional Magnetic Flux Density Total Magnetic Field Intensity Directional Magnetic Field Intensity Total Force Directional Force Current Density Inductance Flux Linkage Error (Magnetic) Magnetostatic Probes Magnetostatic Probes (p. 691) can be used to determine the following results: • Flux Density • Field Intensity • Force Summation • Torque • Energy • Magnetic Flux Electric Potential Electric potential represents contours of constant electric potential (voltage) in conductor bodies. This is a scalar quantity. Total Magnetic Flux Density Magnetic Flux Density is computed throughout the simulation domain and is a vector quantity. Selecting this option allows you to view the magnitude of the vector as a contour or as a directional vector. 688 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Directional Magnetic Flux Density Magnetic Flux Density vector components are computed throughout the simulation domain. Selecting this option allows you to view individual vector components (X, Y, Z) as a contour. Total Magnetic Field Intensity Magnetic Field Intensity is computed throughout the simulation domain and is a vector quantity. Selecting this option allows you to view the magnitude of the vector as a contour or as a directional vector. Directional Magnetic Field Intensity Magnetic Field Intensity vector components are computed throughout the simulation domain. Selecting this option allows you to view individual vector components (X, Y, Z) as a contour. Total Force Total Force results represent electromagnetic forces on bodies. This is a vector quantity. Selecting this option allows you to view the magnitude of the vector as a contour or as a directional vector. Directional Force Vector components of force and torque are computed throughout the simulation domain. They are meaningful only on non-air bodies. Selecting this option allows you to view individual vector force components (X, Y, Z) as a contour. The total summed forces and torque are available in the Details view. For example, requesting the z component of directional force/torque will report the net force acting in the z direction and the net torque acting about the z axis of the specified coordinate system. Current Density Current density can be computed for any solid conductor body. It is displayed as a vector and is best viewed in wireframe mode. You can use the Vector toolbar to adjust the vector arrow viewing options. You can use the element-aligned option in the Vector toolbar for current density vectors, but not the grid-aligned option. Inductance Inductance can be computed for conductor bodies. It is defined as a measure of the differential change in flux linkage to the differential change in current. This is represented by the equation below, where dψ is the differential change in flux linking conductor j produced by a differential change in current for conductor i. Note that this is valid for linear and nonlinear systems, the inductance will be a function of current. ψ = ij ij i Inductance is often used as a parameter in electric machine design and in circuit simulators. A conductor body must have a current load to be considered in inductance calculations. Inductance results are presented in the Worksheet View. The results are presented in table form. The example below shows inductance results for a two-conductor system. The diagonal terms represent self-inductance, while the off-diagonal terms represent mutual inductance. In this case, L11 = 1e - 4, L22 = 8e - 4, L12 = L21 = 4e - 4 Henries. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 689 Features Cond1 (H) Cond2 (H) Cond1 -4 1e 4e-4 Cond2 4e-4 8e-4 The Details view for inductance allows you to define a Symmetry Multiplier. Use this if your simulation model represents only a fraction of the full geometry. The multiplier should be set to compensate for the symmetry model. For example, if you create a half-symmetry model of the geometry for simulation, set the Multiplier to '2.' Changing the multiplier will update the Worksheet results. Note • Computing inductance can be time-consuming and should only be used if needed. • Loads (Voltage, and Current) must be constant when Inductance is specified. Tabular and function loads are not supported. • Inductance can only be used with a single step, single substep solution. User settings to the contrary will be overridden. • Inductance requires the Direct solver setting (default) for the Solver Type property of Analysis Settings. User settings to the contrary will be overridden. Flux Linkage Flux linkage can be computed for any system incorporating a conductor. Solving for flux linkage calculates the flux, ψ, linking a conductor. This is commonly referred to as the "flux linkage." For nonlinear systems, the flux linkage will be a function of current. Flux linkage is also a function of stroke (e.g., displacement of an armature). Flux linkage is often used to compute the emf (electromotive force) in a conductor, defined using the equation below, where V is the electromotive force, typically expressed in volts. =− ψ Conductor bodies must have defined current loads to be considered in flux linkage calculations. Flux linkage results are presented in the Worksheet View. The results are presented in table form. The example below shows flux linkage results for a two-conductor system. Flux Linkages (Wb) Cond1 5e-4 Cond2 10e-4 The Details view for flux linkage allows you to define a Symmetry Multiplier. Use this if your simulation model represents only a fraction of the full geometry. The multiplier should be set to compensate for the symmetry model. For example, if you create a half-symmetry model of the geometry for simulation, set the Multiplier to '2.' Changing the multiplier will update the Worksheet results. 690 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Note • Computing flux linkage can be time-consuming and should only be used if needed. • Loads (Voltage, and Current) must be constant when flux linkage is specified. Tabular and function loads are not supported. • Flux linkage can only be used with a single step, single substep solution. User settings to the contrary will be overridden. • Flux linkage requires the Direct solver setting (default) for the Solver Type property of Analysis Settings. User settings to the contrary will be overridden. Error (Magnetic) The description of this result is similar to Error (Structural) except that flux density is the basis for the errors instead of stresses. When all materials are linear, Workbench uses relative permeability (MURX, MURY, MURZ) values which are available in the material properties. When nonlinear materials are present, Workbench does not extract relative permeability from the material properties. Instead, for a given element, Workbench first sums the flux density vectors of the result nodes to form a vector called B. Workbench next sums the field intensity vectors of the result nodes to form a vector called H. MURX, MURY, and MURZ are all assigned the value ( |B|/|H| ) / MUZERO, where: • |B| is the length of the B vector, • |H| is the length of the H vector, • MUZERO is free space permeability. If the H vector has a zero length, the contribution of this element to the energy error will be set to 0. Magnetostatic Probes The following magnetostatic probe types are available. Probe Type Flux Density Applicable Analysis Types Magnetostatic Output Flux Density: X axis, Y axis, Z axis Characteristics Scope to: body. Scope by: bodies, location only, vertex, edge, face. Orientation coordinate system: any; defaults to Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 691 Features Probe Type Applicable Analysis Types Output Characteristics Global Cartesian. Field Intensity Magnetostatic Flux Intensity: X axis, Y axis, Z axis Scope to: body. Scope by: bodies, location only, vertex, edge, face. Orientation coordinate system: any; defaults to Global Cartesian. Force Summation Magnetostatic Force Sum: X axis,Y axis, or Z axis; Symmetry Multiplier Scope to: body. Scope by: bodies. Orientation coordinate system: any; defaults to Global Cartesian. Torque Magnetostatic Torque:1 X axis,Y axis, or Z axis; Symmetry Multiplier Scope to: body. Scope by: bodies. Orientation coordinate system: any; defaults to Global Cartesian. Summation: Orientation coordinate system. Energy 692 Magnetostatic Magnetic Co-energy Scope to: body. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Probe Type Applicable Analysis Types Output Characteristics Scope by: System or per body. Magnetic Flux Magnetostatic Magnetic Flux2 Scope to: body. Scope by: edge. 1 - Torque results represent the torque on a body due to electromagnetic forces. Torque is specified about the origin of a coordinate system. By default, the global coordinate system is used. To change the specification point, create a local coordinate system and specify the results about the new origin. The torque result is listed in the Details view. 2 - Magnetic Flux is computed along the edge scoping. The scoping should produce a single continuous path along a model edge. Flux is reported as magnitude only. See the Probes (p. 737) section for further information. Electric Results The following electric result types are available: Result Type Description Electric Voltage Represents contours of constant electric potential (voltage) in conductor bodies.This is a scalar quantity. Total Electric Field Intensity Is computed throughout the simulation domain and is a vector sum quantity. Selecting this option allows you to view the total magnitude of the vectors as a contour. Directional Electric Field Intensity Its vector components are computed throughout the simulation domain.This option allows you to view individual vector components (X,Y, Z) as contours. Total Current Density Can be computed for any solid conductor body. It is displayed as a vector and is best viewed in wireframe mode.You can use the Vector toolbar to adjust the vector arrow viewing options. You can use the element-aligned option in the Vector toolbar for current density vectors, but not the grid-aligned option. Directional Current Density Its vector components are computed throughout the simulation domain.This option allows you to view individual current density vector components (X,Y, Z) as contours. Joule Heat Occurs in a conductor carrying an electric current. Joule heat is proportional to the square of the current, and is independent of the current direction. Note This result when generated by non-zero contact resistance is not supported. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 693 Features Electric Probes (p. 694) can be used to determine the following results: • Electric Voltage • Field Intensity • Current Density • Reaction Electric Probes The following electric probe types are available. Probe Type Electric Voltage Applicable Analysis Types Electric Output Voltage Characteristics Scope to: body. Scope by: bodies, location only, vertex, edge, face. Field Intensity Electric X axis,Y axis, Z axis, Total Scope to: body. Scope by: bodies, location only, vertex, edge, face. Orientation coordinate system: any; defaults to Global Cartesian. Current Density Electric X axis,Y axis, Z axis, Total Scope to: body. Scope by: bodies, location only, vertex, edge, face. Orientation coordinate system: any; defaults to Global Cartesian. Reaction Electric Current: overall Scope to: body. Scope by: boundary condition. See the Probes (p. 737) section for further information. 694 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Fatigue Results Fatigue provides life, damage, and factor of safety information and uses a stress-life or strain-life approach, with several options for handling mean stress and specifying loading conditions. Common uses for the strain-life approach are in notched areas where, although the nominal response is elastic, the local response may become plastic. The three components to a fatigue analysis are: Fatigue Material Properties (p. 695) Fatigue Analysis and Loading Options (p. 696) Reviewing Fatigue Results (p. 699) For detailed information on how these components are handled, go to the ANSYS web site. Fatigue Material Properties Engineering Data contains example materials which may include fatigue curves populated with data from engineering handbooks. You can also add your own fatigue curves. The Fatigue Tool will use the information from these curves for each material in the model when calculating life, damage, safety factors, etc. If Young's Modulus is temperature dependent, then the fatigue calculations are carried out using the Young's Modulus computed at the reference temperature of the body. For the strain-life approach, the materials must have Strain-Life Parameters defined. For the Stress-Life approach, the materials must have Alternating Stress defined. To add this data to a material follow the Add Material Properties procedure (see Perform Material Tasks in Engineering Data). • Alternating Stress The alternating stress, or stress-life (SN), mean curve data can be defined for a mean stress or rratio. The Interpolation method (Log-Log, Semi-Log, or Linear) can be defined. The curve data must be defined to be greater than zero. – Mean Stress Use this definition if experimental SN data was collected at constant mean stress for individual SN curves. – R-Ratio Use this definition if multiple SN curves were collected at a constant r-ratio. The r-ratio is defined as the ratio of the second loading to the first: r = L2 / L1. Typical experimental r-ratios are -1 (fully reversed), 0 (zero-based), and .1 (to ensure that a tensile stress always exists in the part). It is possible to define multiple SN curves to account for different mean stress or r-ratio values. The values of mean stress/r-ratio are only important if multiple curves are defined and the SN-Mean Stress Curves correction using experimental data option is chosen in the Fatigue Tool • Strain-Life Parameters The following four strain-life parameter properties and the two cyclic stress-strain parameters must have data defined: – Strength Coefficient – Strength Exponent – Ductility Coefficient – Ductility Exponent Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 695 Features – Cyclic Strength Coefficient – Cyclic Strain Hardening Exponent Note that in Engineering Data, in the Display Curve Type drop down menu, you can plot either a Strain-Life or Cyclic Stress-Strain curve. Fatigue Analysis and Loading Options After you have defined the stress-life or strain-life curves for all materials in your model, you can choose your fatigue options and run the fatigue analysis. To select the fatigue analysis and loading options, you must select the Fatigue Tool Solution object from the Solution Context Toolbar, or via a right-mouse click. In the Details View (p. 274) you may specify the following options: • Fatigue Strength Factor (Kf ) • Loading Type • Scale Factor • Analysis Type • Mean Stress Theory • Stress Component • Units Name • 1 “Unit” is Equal To • Bin Size • Use Quick Rainflow Counting • Infinite Life • Maximum Data Points To Plot The Worksheet includes theoretical graphic information that reflects settings in the Details view. Fatigue Strength Factor (Kf ) This is the fatigue strength reduction factor. The stress-life or strain-life curve(s) are adjusted by this factor when the fatigue analysis is run. This setting is used to account for a "real world" environment that may be harsher than a rigidly-controlled laboratory environment in which the data was collected. Common fatigue strength reduction factors to account for such things as surface finish can be found in design handbooks. Loading Type Choose from the following: • Zero-Based (r=0) • Fully Reversed (r=-1) • Ratio • History Data • Non-proportional Loading (available only for stress-life applications) 696 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application The first three are all constant amplitude, proportional loading types and are illustrated with a graph in the Geometry window. The fourth type, history data, allows you to navigate to a file containing the data points. This option is a non-constant amplitude proportional loading type. This data is depicted in a graph on the Worksheet. You can specify the number of data points this graph will display in the Maximum Data Points To Plot field located in the Details view of the Fatigue Tool. The fifth option is a non-proportional constant amplitude loading type for models that alternate between two completely different stress states (for example, between bending and torsional loading). Problems such as an alternating stress imposed on a static stress can be modeled with this feature. Non-proportional loading is applicable on fatigue tools under Solution Combination where exactly two environments are selected. Scale Factor This setting scales the load magnitude. For example, if you set this to 3, the amplitude (and mean) of a zero-based loading will be 1.5 times the stress in the body. The graph in the Worksheet window will update to reflect this setting. This option is useful to see the effects of different finite element loading magnitudes without having to run the complete structural analysis repeatedly. Note that this scale factor is applied after the stresses have been collapsed from a tensor into a scalar. Thus any multiaxial stress collapse methods that are sensitive to the sign (Von-Mises, Maximum Shear, Maximum Principal) may not give the same answer had the scale factor been applied to the environment load itself. Analysis Type Choose either Stress Life or Strain Life. Mean Stress Theory This setting specifies how the mean stress effects should be handled. • If Analysis Type is set to Stress Life, choose from None, Goodman, Soderberg, Gerber, and Mean Stress Curves. The Goodman, Soderberg, and Gerber options use static material properties along with S-N data to account for any mean stress while Mean Stress Curves use experimental fatigue data to account for mean stress. The default mean stress theory can be defined through the Mechanical application Fatigue settings in the Options dialog box. • If Analysis Type is set to Strain Life, choose from None, Morrow, and SWT (Smith-Watson-Topper). Note A sample plot of each of these theories is shown at the bottom of the Worksheet view. This plot does not use live data, but is rather a generic representation of each theory. For more information on these theories, see "Metal Fatigue In Engineering" by Ralph I. Stephens, et. al. Stress Component Because stresses are multiaxial but experimental fatigue data is usually uniaxial, the stress must be converted from a multiaxial stress state to a uniaxial one. A value of 2 times the maximum shear stress is used. You can choose from several types, including component stresses, von Mises, and a signed von Mises, which takes the sign of the absolute maximum principal stress. The signed von Mises is useful for accounting for any compressive mean stresses. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 697 Features Units Name This field allows you to specify the name for the Life Units. The unit options include: • cycles • hours • blocks • days • seconds • months • minutes • User Defined User Defined Selecting the User Defined option displays the Custom Units Name field. Enter the name for your customized unit name in this field. The specified unit is reflected in the Details view for all applicable fatigue settings. 1 “Unit” is Equal To Where "unit" is either cycle or block based on the Units Name selection. Modify the field’s value based on the desired number of cycles or blocks for the units. Bin Size This option appears only if Type is set to History Data (non-constant amplitude loading). This setting defines how many divisions the cycle counting history should be organized into for the history data loading type. Strictly speaking, this is number specifies the dimensions of the rainflow matrix. A larger bin size has greater precision but will take longer to solve and use more memory. Use Quick Rainflow Counting This option appears only if Type is set to History Data (non-constant amplitude loading). Since rainflow counting is used, using a “quick counting” technique substantially reduces runtime and memory, especially for long time histories. In quick counting, alternating and mean stresses are sorted into bins before partial damage is calculated. This means that with quick counting active, calculations will be performed for maximum of binsize. Thus the accuracy will be dictated by the number of bins. Without quick counting, the data is not sorted into bins until after partial damages are found and thus the number of bins will not affect the results. The accuracy of quick counting is usually very good if a proper number of bins are used when counting. To see the effects of using quick counting, compare the results of constant amplitude loading to simulated constant amplitude loading from a load history file. With quick counting off, the result should match exactly but with quick counting on, there will be some error depending on the bin size and alternating stress value in relation to the midpoint of the bin the count is sorted into. Infinite Life Stress Life Analysis This option appears only if Type is set to History Data (non-constant amplitude loading) and defines what life will be used if the stress amplitude is lower than the lowest stress on the SN curve. It may be important in how damaging small stress amplitudes from the rainflow matrix are. Strain Life Analysis 698 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Since the strain-life method is equation based it has no built-in limit, unlike stress-life for which the Fatigue Tool uses a maximum life equal to the last point on the SN curve. Thus to avoid skewed contour plots showing very high lives, you can specify Infinite Life in a strain-life analysis. For example, if you set a value of 1e9 cycles as the Infinite Life, the maximum life reported is 1e9. Maximum Data Points To Plot This option is only applicable for History Data loading and allows you to specify the number of data points to display in the corresponding graph that appears in the Worksheet. The default value is 5000 points. The graph displays the full range of points and all points are used in the analysis. However, depending on the value you set, every second or third point may not be displayed in the interest of avoiding clutter and making the graph more readable. Reviewing Fatigue Results After you have included the Fatigue Tool in your analysis, you can then choose from among several results options. Any of these results can be scoped to individual parts or faces if desired. To select the fatigue solution items, you must be under a Solution object. Click Fatigue Tool either on the toolbar or via a right-mouse click and select any of the following options: • Life (p. 699) • Damage (p. 699) • Safety Factor (p. 700) • Biaxiality Indication (p. 700) • Equivalent Alternating Stress • Rainflow Matrix (history data only) (p. 700) • Damage Matrix (history data only) (p. 700) • Fatigue Sensitivity (p. 701) • Hysteresis (p. 702) Life This result contour plot shows the available life for the given fatigue analysis. If loading is of constant amplitude, this represents the number of cycles until the part will fail due to fatigue. If loading is nonconstant, this represents the number of loading blocks until failure. Thus if the given load history represents one month of loading and the life was found to be 120, the expected model life would be 120 months. In a constant amplitude analysis, if the alternating stress is lower than the lowest alternating stress defined in the S-N curve, the life at that point will be used. Damage Fatigue damage is defined as the design life divided by the available life. The default design life may be set through the Options dialog box. A damage of greater than 1 indicates the part will fail from fatigue before the design life is reached. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 699 Features Safety Factor This result is a contour plot of the factor of safety (FS) with respect to a fatigue failure at a given design life. The maximum FS reported is 15. Biaxiality Indication This result is a stress biaxiality contour plot over the model that gives a qualitative measure of the stress state throughout the body. A biaxiality of 0 corresponds to uniaxial stress, a value of -1 corresponds to pure shear, and a value of 1 corresponds to a pure biaxial state. For Non-proportional loading, you can choose between average biaxiality and standard deviation of biaxiality in the Details view. Equivalent Alternating Stress The Equivalent Alternating Stress contour is the stress used to query the S-N curve. This result is not valid if the loading has non-constant amplitude (Loading Type = history data). The result is useful for cases where the design criteria is based on an equivalent alternating stress as specified by the fatigue analyst. Rainflow Matrix (history data only) This graph depicts how many cycle counts each bin contains. This is reported at the point in the specified scope with the greatest damage. The Navigational Control at the bottom right-hand corner of the graph can be used to zoom and pan the graph. You can use the double-sided arrow at any corner of the control to zoom in or out. When you place the mouse in the center of the Navigational Control, you can drag the four-sided arrow to move the chart points within the chart. Damage Matrix (history data only) Similar to the rainflow matrix, this graph depicts how much relative damage each bin has caused. This result can give you information related to the accumulation of the total damage (such as if the damage occurred though many small stress reversals or several large ones). 700 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application The Navigational Control at the bottom right hand corner of the graph can be used to zoom and pan the graph. You can use the double-sided arrow at any corner of the control to zoom in or out. When you place the mouse in the center of the Navigational Control, you can drag the four-sided arrow to move the chart points within the chart. Fatigue Sensitivity This plot shows how the fatigue results change as a function of the loading at the critical location on the scoped region. Sensitivity may be found for life, damage, or factory of safety. For instance, if you set the lower and upper fatigue sensitivity limits to 50% and 150% respectively, and your scale factor to 3, this result will plot the data points along a scale ranging from a 1.5 to a 4.5 scale factor. You can specify the number of fill points in the curve, as well as choose from several chart viewing options (such as linear or log-log). The Navigational Control at the bottom right hand corner of the graph can be used to zoom and pan the graph. You can use the double-sided arrow at any corner of the control to zoom in or out. When you place the mouse in the center of the Navigational Control, you can drag the four-sided arrow to move the chart points within the chart. To specify a result item, you must be under a Solution object. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 701 Features Hysteresis In a strain-life fatigue analysis, although the finite element response may be linear, the local elastic/plastic response may not be linear. The Neuber correction is used to determine the local elastic/plastic response given a linear elastic input. Repeated loading will form close hysteresis loops as a result of this nonlinear local response. In a constant amplitude analysis a single hysteresis loop is created although numerous loops may be created via rainflow counting in a non-constant amplitude analysis. The Hysteresis result plots the local elastic-plastic response at the critical location of the scoped result (the Hysteresis result can be scoped, similar to all result items). Hysteresis is a good result to help you understand the true local response that may not be easy to infer. Notice in the example below, that although the loading/elastic result is tensile, the local response does venture into the compressive region. Loading/Elastic Response: Corresponding Local Elastic Plastic Response at Critical Location: User Defined Results This section examines the purpose, operation, and use of the User Defined Result feature of Workbench. Overview Characteristics Application Nodal Scoping User Defined Result Expressions User Defined Result Identifier Unit Description 702 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application User Defined Results for the Mechanical APDL Solver User Defined Results for Explicit Dynamics Analyses Overview The User Defined Result feature allows you to derive user defined result values by performing mathematical operations on results obtained following a solution. Workbench generates user defined results, based on the analysis type. These results display on the Solution Worksheet. Using this feature, many results stored in the result file can be displayed. The following illustration displays a sample of the worksheet. Refer to the following sections for descriptions of user defined result entries in the worksheet: • User Defined Results for the Mechanical APDL Solver (p. 711) • User Defined Results for Explicit Dynamics Analyses (p. 714) Characteristics General: • All analysis types and solver targets can produce User Defined Results. A User Defined Result may be unique to a particular solver and analysis. After clicking on the Solution object, you must click on the Worksheet to produce the complete listing of the results that are applicable to the analysis type and solver being used. • All result types can be combined except for results which have different dimensions. For example, displacement vectors, which contain 3 items, cannot be added to stress tensors, which contain 6 items. • User Defined Results which are elemental (such as stress or strain results) can be displayed as averaged or unaveraged results. It takes Workbench longer to display a result which is not averaged. Like most result types that display using contours, user defined results: • Are scoped to a geometry (vertex, edge, face, body), named selection, path, or surface. However, you cannot scope user defined results based on Contacts to a path or surface. • Require a set, time, and frequency/phase, to be fully specified (depending on the analysis type). • Display minimum/maximum values and a Graph. • Display nodal averaged data. • Can be added to a Chart • Can be examined using probe annotations, slice planes, isosurface, etc. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 703 Features • Can be cleared. • Can be duplicated. Unlike other contour results, user defined results: • Can be duplicated or copy/pasted except for identifiers. • Can have a variable unit category assigned to its contour. • Become obsolete if a user defined result is dependent upon another user defined result that has been modified, cleared, or deleted. In this instance, the graphic of the geometry displays without results. • User defined results cannot employ Probes. • User defined results cannot link to multiple environments and cannot employ the Solution Combination feature. Application Apply a User Defined Result using one of the following methods: • Select the User Defined Result toolbar button. • Right-click the Solution object and the select the User Defined Result option. • Display the Solution Worksheet following a Solve, right-click the mouse on the desired row of the table, and then select Create User Defined Result. Until you become familiar with this feature, it is recommended that you insert user defined results using the worksheet. This makes sure that results are valid and applicable for the particular analysis type and solver being used. As illustrated below, right-clicking the mouse on a row of the worksheet displays an option to create a user defined result. Note NMISCxxx and SMISCxxx results are not displayed in the worksheet and can only be accessed by typing in the keyword directly. See User Defined Results for the Mechanical APDL Solver (p. 711) for details. Selecting this option places a User Defined Result object for the specified result in the tree as a child of the Solution object, as shown in the example below. Compared to the other two methods for inserting a User Defined Result, this technique automatically completes field data in the Details view. Note that the new result object’s name appears in the Expression field of the Details view. Except for an Identifier, all remaining details are also automatically generated based on the information provided by the result type, such as Input Unit System (U.S. Custom) and Output Unit (Displacement). 704 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application If you create a user defined result and do not use the worksheet as the origin, you need to manually enter an Expression and also define the Output Unit. These fields display with a yellow highlight to indicate the required entries. See the User Defined Result Expressions and Unit Description sections for more information. Once a user defined result is created, the advantage of the feature is your ability to further define expressions using mathematical operators. For example, you can enter the mathematical combination UX+UY in the Expression field and then retrieve a new result. Nodal Scoping In regard to usage, suppose two user defined results (with identifiers A and B, respectively) are scoped to ScopeA and ScopeB . The algorithm to draw the contours for C = A + B (scoped to ScopeC) proceeds as follows: • The results A and B are combined on all common bodies (determined from ScopeA and ScopeB and referred to as CommonBodies). • The scope (ScopeC) of the newly defined result C is then employed: the contours of C are drawn on the intersection of ScopeC and CommonBodies. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 705 Features Note, each of ScopeA, ScopeB, and ScopeC can be any set of geometric entities: vertices, edges, faces, bodies, or named selections (consisting of geometric entities or even nodes in the mesh). Example 2 Nodal Scoping Assumptions: A is scoped to bodies 1 and 2 and B is scoped to two faces , one in body 2 and one in body 3. The combination C = A+B is scoped to two vertices, one in body 2, and the other in body 3. Result: A+B will be computed on nodes common to the underlying bodies of A and B; these nodes will exist only in body 2. Then the combination C = A + B will be displayed only on the vertex belonging to body 2 (the one belonging to body 3 is not in the intersection of the two original scoping bodies). User Defined Result Expressions The term “expression” has more than one use when defining user defined results. An expression is: • Primarily, the combination of mathematical values, based on syntax rules and the available math operations. • A column displayed on the Solution Worksheet that indicates the result type. • An entry field in the Details view of a user defined result where you enter mathematical values, such as UX+UY+UZ. Note You can use user defined result expressions across multiple combinations of environments with limited functionality by using a Design Assessment system. However, you can not use it within standard Solution Combinations. The example of the Solution Worksheet shown below highlights the Expression column. When a User Defined Result is applied, the content of the above column populates the Expression field of the user defined result's Detail View. In this case, UX. 706 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application The content of the Expression field can be modified using mathematical operators to further define the expression. As shown below, you can combine the X, Y, and Z components and then retrieve a new customized result. Expression Syntax Expressions support the following syntax: • Operands: ( ‘+’, ‘-‘,’*’, ‘/’, ‘^’) • Functions: (sqrt(), min()…) - always use lower case • Numbers: (scalar quantities such as 1.0, 25, -314.23, or 2.5e12) • Identifiers: unique user defined names Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 707 Features Supported Mathematical Operations The following is a list of the mathematical operations currently supported for user defined results. The shorthand notation "s" defines a scalar quantity and "a" defines an array. An array is distinguished by its dimension which includes the length, based on the number of rows (that is, number of nodes or elements), and the width, consisting of 1, 3, or 6 columns depending on the type of result stored. • Addition (+): s1+s2, a1+a2, a+s (s+a is not supported) • Subtraction (-): s1-s2, a1-a2, a-s (s-a is not supported) • Multiplication (*): s1*s2, a1*a2, a*s, s*a • Division (/): s1/s2, a1/a2, a/s (s/a is not supported) • Power (^): s1^s2, a^s, (undefined if s1 = 0 and s2 < 0) • Log base ten (log10): log10(s), log10(a), (s and a > 0.0) • Square root (sqrt): sqrt(s), sqrt(a), (s and a should be >= 0.0) • Dot product (dot): dot(a1,a2) (results in a single-column array consisting of the inner products, one for each row of a1 and a2; thus, a1, a2 should have the same dimensions) • Cross product (cross): cross(a1,a2) (a1, a2 must have 3 columns) • Add Comp (addcomp): addcomp(uvectors) = ux + uy + uz (If the argument uvectors has 3 columns, they are added to produce a single-column array. If the argument is a single-column array, the result will be a scalar summing all the array entries.) • Maximum (max): s = max(s1,s2), a = max(a1,a2) • Minimum (min): s = min(s1,s2), a = min(a1,a2) • Absolute Value (abs): s = abs(s1), a=abs(a1) • Trigonometric Functions (sin, cos, tan): sin(s), cos(s), tan(s), sin(a), cos(a), tan(a) (s and a are both in radians) • Inverse Trigonometric Functions (asin, acos, atan): asin(s), acos(s), atan(s), asin(a), acos(a), atan(a) (return values are in radians; where -1 <= s <= 1 and -1 <= a <=1 for asin and acos) • atan2: atan2(s1,s2), atan2(a1,a2) (return values are in radians; calculates the arctangent of s1/s2 or a1/a2 and uses the sign of the arguments to determine the quadrant of the returned angle) Note • The current expression list does not allow input parameters from the Parameter Workspace. Only output parameters are allowed for Min and Max values of a user defined result. • All operations involving two vector arrays must have the same dimensionality. • Any result whose expression contains the addcomp function needs to be scoped to exactly one body. • You cannot perform mathematical operations directly within the Design Assessment system. However, the Design Assessment system provides the ability to use python scripts to combine results from various environment using highly complex, user defined mathematical functions. User Defined Result Identifier Each user defined result you create can be assigned a unique name using the Identifier field in the Details view as illustrated below. 708 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application User defined identifiers: • Can begin with a letter or an underscore character. • Can contain any number of letters, digits, or underscores. • Are not case insensitive - however, functions should always use lowercase (sqrt, max, min, etc.). • Are not affected by the order in which they are entered. For example, for Identifiers A and B, the expression for: – User defined Result 1 can equal: B = 2*A, and: – User Defined Result 2 can equal: A = UX It is recommend that you use the proper order and try to define dependents first. For example, define A, B, C and then D = A^2+B^2+C^2 • • Cyclic dependencies are blocked, such as the following: – User Defined Result 1: A = UX + C – User Defined Result 2: C = 2 * A - 1 Correspond to an array over all nodes (or all elements): – Length = number of nodes (or elements) – Width = 1, 3, or 6 columns An Identifier, together with Expression content (UX, UY, etc.), can be used in combination with other user defined results. For example, using the Identifier MyResult, you could create the Expression: sqrt(MyResult+UX+UY). In addition, if an Identifier is used in an expression, it must be scoped to the same geometry. It is recommended that when you assign an identifier to the expression of a user defined result, that you rename the tree object with the same name/identifier. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 709 Features Limitations of the User Defined Result Identifier There are several problematic scenarios that can arise when you use the Identifier of an existing user defined result to create a new user defined result. For each scenario, changing an item in the Details view of the new result causes the new result to be unreliable. For example, the Display Time of a User Defined Result is only relevant when the expression consists of built-in identifiers. Unlike user defined identifiers, built-in identifiers retain their time dependence through the evaluation of the expression. To reveal the built-in identifiers for a given solver, examine the Worksheet view on the Solution folder. Please note that Workbench may not necessarily issue a warning or error message for these situations. Suppose the Identifier of the original result is "Original". Further, suppose that the Expression of the new result is "2 * Original". Consider the following scenarios: • Different choices of By Time or By Result Set • Different choices of the value of Display Time or Set • Different choices of Coordinate System • Different choices of Yes/No for Calculate Time History • Different choices for Use Average Unit Description The units of a user defined result are defined by the following Detail view settings: • Input Unit System: A read-only field that displays the active Mechanical application unit system. To evaluate an expression, a user defined result's units must be converted to the Input Unit System. As a result, the expression is most easily verified when the intervening data is viewed in the Input Unit System. • Output Unit: The physical dimension assigned to a user defined result. It determines which factors are used to convert the result from its Input Unit System to the current unit system selection. Units are defined in a two step process. 1. Before you evaluate an expression, the units are converted to the Input Unit System. 2. Once evaluated, values are converted from the input system to the active Mechanical application unit system using the appropriate factor. For example, given the following user defined result expressions with MKS (m, kg, N, ºC, s, V, A) units: • FORCE_MKS=FSUM • STRESS_MKS=SEQV • DISP_MKS=USUM If you change the unit system to CGS (cm, g, dyne, ºC, s, V, A) and create a new user defined result with Expression=FSUM+SEQV+USUM and volume as the output unit, you'll produce the following user defined results: Custom Identifier Expression Input Unit System Output Units FORCE_MKS FSUM Metric (m, kg, N, s, V, A) Force STRESS_MKS SEQV Metric (m, kg, N, s, V, A) Stress 710 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application DISPL_MKS USUM Metric (m, kg, N, s, V, A) Displacement VOLUME_CGS FSUM+SEQV+USUM Metric (cm, g, dyne, s, V, A) Volume The expression VOLUME_CGS is easy to verify for its Input Unit System, CGS. If FSUM=3 dyne, SEQV=17 dyne/cm² and USUM=2 cm, (as seen in when CGS is selected in the Mechanical application), VOLUME_CGS produces the value 22 cm³. Any subsequent changes to the unit system in the Mechanical application cause each of the user defined results to convert based on their required factors. In this manner, VOLUME_CGS will use a factor of 1000 to convert from Metric CGS to Metric mm, because it represents a Volume. FORCE_MKS, STRESS_MKS and DISPL_MKS will convert differently, based on the selected Output Units. User Defined Results for the Mechanical APDL Solver Refer to the PRNSOL and PRESOL command pages in the Mechanical APDL application Commands Reference for descriptions of most Component and Expression entries in the table. Some other entries are self-explanatory (SUM for example). VECTORS refer to vector plot results that include arrows in the display. The following tables include descriptions of other user defined result names not included in the PRESOL/PRNSOL listings. Nodal Results Nodal results are most often associated with degree of freedom solutions (like nodal reactions). Name Description R Nodal rotations in a structural analysis (analogous to PRNS,ROT) OMG Nodal rotational velocities in a structural transient dynamic analysis (analogous to PRNS,OMG) DOMG Nodal rotational accelerations in a structural transient dynamic analysis (analogous to PRNS,DMG) MVP_AZ Nodal Z magnetic vector potential in an axisymmetric electromagnetic analysis (analogous to PRNS,A) LOC Nodal locations (x,y,z) LOC_DEF Deformed nodal locations (x+ux,y+uy,z+uz) F Nodal structural forces (reaction)1 M Nodal structural moments (reaction)1 CSG Nodal magnetic current segments (reaction) HEAT Nodal thermal heat flow (reaction) AMPS Nodal electric current (reaction) NDIR Nodal THXY, THYZ, and THZX values.The NDIRVECTORS display consists of triads. 1 - When user defined results FX, FY, FZ, FSUM, and FVECTORS (and MX, MY, MZ, MSUM, and MVECTORS) are scoped to a path, then it is possible that no contours will be displayed. The reason is that these types of forces/moments are solved only at constrained nodes. The result value at a path point is interpolated from the nodal values of the elements that contain the path point. If a path point touches an element in which some nodes have undefined reactions, then Mechanical cannot properly interpolate the nodal values for the path point. No contour color is displayed at such a path point. Elemental Results Elemental results can exist at the nodes (like stress and strain) or can exist at the centroid (like volume). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 711 Features Name Description SPSD Element nodal equivalent stress as calculated by the solver. EPELEQV_RST Element nodal equivalent elastic strain as calculated by the solver. EPPLEQV_RST Element nodal equivalent plastic strain as calculated by the solver. EPCREQV_RST Element nodal equivalent creep strain as calculated by the solver. EPTOEQV_RST Element nodal equivalent total strain as calculated by the solver, that is, EPTOEQV_RST is total mechanical strain: EPTOEQV_RST = EPELEQV_RST + EPPLEQV_RST + EPCREQV_RST. EPTTEQV_RST Element nodal equivalent total strain (plus thermal strain) as calculated by the solver, that is, EPTTEQV_RST is total mechanical and thermal strain: EPTTEQV_RST = EPELEQV_RST + EPPLEQV_RST + EPCREQV_RST + EPTHEQV_RST. ETOP Element nodal densities used for topological optimization (same as TOPO). BEAM Element nodal beam stresses: direct, minimum bending, maximum bending, minimum combined, maximum combined. SVAR Element nodal state variable data. CONTJHEA Element nodal Joule heat for CONTA174. CONTFORC Element nodal contact normal forces for CONTA175. BEAM_AXIAL_F Element nodal axial force vectors for BEAM188/189. BEAM_BENDING_M Element nodal bending moment vectors for BEAM188/189. BEAM_TORSION_M Element nodal torsion moment vectors for BEAM188/189. BEAM_SHEAR_F Element nodal shear force vectors for BEAM188/189. ENFO Element nodal reaction forces for structural analyses. EHEAT Element nodal heat values for thermal analyses. CURRENTSEG Element nodal magnetic current segments. VOLUME Element volumes. ENERGY Element potential and kinetic energies. RIGID_ANG Element Euler angles for MASS21 elements (rotation about x-axis, rotation about y-axis, rotation about z-axis). CONTSMISC Element summable miscellaneous data for contact elements. CONTSMISC is completely analogous in implementation to SMISC (see “User Defined Results Not Displayed in Worksheet” below). CONTNMISC Element non-summable miscellaneous data for contact elements. CONTNMISC is completely analogous in implementation to NMISC (see “User Defined Results Not Displayed in Worksheet” below). EDIR Elemental THXY,THYZ, and THZX values: (1) currently only angles of first node in solution record are employed; (2) the EDIRVECTORS display consists of triads. PNUMTYPE Element type reference numbers. PNUMREAL Real constant set numbers. 712 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Name Description PNUMMAT Material set numbers. PNUMSEC Section numbers. PNUMESYS Element coordinate system numbers (note: a 0 value corresponds to the global Cartesian system). PNUMELEM MAPDL element ID. SMISC Element summable miscellaneous data. NMISC Element non-summable miscellaneous data. Using this data, you can explicitly define your user defined result, such as total deformation by using the component deformations across all of the nodes in the model, identified by UX, UY, and UZ. You can use these component values to mathematically produce a user defined result for total deformation: SQRT(UX^2+UY^2+UZ^2). Notes If the Display Option is set to Averaged, then for the results ENFO, EHEAT, and CURRENTSEG, the result at each node represents the sum (or contributions) of all the elements that contain the node. If the Display Option is set to Unveraged, the ENFO result is analogous to PLES,FORCE. SPSD is a User Defined Result that is unique to the Mechanical APDL result file. For any element that supports stresses, the SPSD result represents the equivalent stress, for each corner node in the element, as stored on the result file. Hence, SPSD is the equivalent stress as calculated by the Mechanical APDL solver for the corner nodes. For this result, SPSD is the expression displayed in the Type column and Stress is displayed in the Output Unit column. Prior to release 13.0, SPSD represented the equivalent stress as calculated from component stresses during postprocessing, that is, it was not calculated by the Mechanical APDL solver. Displays of PNUM results are analogous to EPLOTs with the following commands in MAPDL: • /PNUM,TYPE,1 • /PNUM,REAL,1 • /PNUM,MAT,1 • /PNUM,SEC,1 • /PNUM,ESYS,1 • /PNUM,ELEM,1 For example, the range of the values of the PNUMTYPE result vary from the smallest element type to the largest element type, as created by ANSYS ET commands. Note PNUM results are available for all analyses supported by MAPDL. For non-linear analyses, user defined results corresponding to MAPDL PLES commands with NL as an Item are available with the following components: SEPL, SRAT, HPRE, EPEQ, PSV, PLWK, CRWK, ELWK, SGYT, and PEQT Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 713 Features Although there are no user defined results with SEND in Mechanical, you can use the following: Use This For This NLPLWK PLES,SEND,PLASTIC NLCRWK PLES,SEND,CREEP NLELWK PLES,SEND,ELASTIC User Defined Results Not Displayed in Worksheet For the Mechanical APDL solver, there are User Defined Results associated with summable miscellaneous data (SMISC) and non-summable miscellaneous data (NMISC) on the result file. These results are not listed in the Solution Worksheet. Because this data can be voluminous, by default, Mechanical does not write it to the result file for all types of models. Examples of models which cause SMISC and NMISC data to be written are beam models and certain contact models. Activate miscellaneous output for all elements or just contact elements using the Output Controls available in the Details of the Analysis Settings object. Mechanical has adopted a convention that miscellaneous data for contact elements be called CONTSMISC and CONTNMISC. This means that SMISC and NMISC data will only display on noncontact elements and that CONTSMISC and CONTNMISC data will only display on contact elements. To display these results: 1. Click on the User Defined Result toolbar button. 2. In the Details view Expression field, type the string SMISC or NMISC followed by the sequence number which indicates the desired datum. For example, to display the 2nd sequence number for SMISC, enter SMISC2 for the Expression. The graphics contour display will be similar to the Mechanical APDL display for the command PLES,SMISC,2. When you evaluate this result, the Details view will show no units and no coordinate system for this data. That is, no unit conversions and no coordinate transformations are performed. If you enter a data expression that does not exist on the result file, the result will not be evaluated. To display the 2nd sequence number for summable miscellaneous data on scoped contact elements, enter CONTSMISC2 for the Expression. User Defined Results for Explicit Dynamics Analyses Presented below are the user defined results that are specific to an explicit dynamics analysis using the AUTODYN solver. Variable Description Type BEAM_LEN Beam length Element Nodal BOND_STATUS The number of nodes bonded to the faces on an element during the analysis. A value of -1 is shown where all the bonds for the face have broken. Elemental C_S_AREA Beam cross section area Element Nodal COMPRESS Material compression Element Nodal Compression, µ = ρ/ρ0 CROSS_SECTION Beam cross section number Elemental DAMAGE Material Damage Element Nodal 714 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Variable Description Type 0– intact material 1- fully fractured DENSITY Material Density Element Nodal EFF_STN Effective Geometric Strain of a cell Element Nodal EFF_PL_STN Effective Plastic Strain. Note: This is calculated incrementally, unlike the equivalent plastic strain (EPPLEQV), which is calculated as an instantaneous value. Element Nodal ENERGY_DAM Energy resulting from fracture for the Johnson-Holmquist brittle strength model Element Nodal EROSION Erosion Status Elemental 0 - no erosion >0 - eroded. (will not be displayed) EPS_RATE Effective Plastic Strain Rate Element Nodal F_AXIAL Beam axial force Element Nodal INT_ENERGY Internal energy of the material Element Nodal MASS Mass of material in an element Element Nodal MATERIAL Material index. The material index as defined in the Explicit solver. There is not always a direct one-to-one correlation with materials defined in Engineering Data and the those used in the Explicit solver. Elemental For layered section shells, the MATERIAL for individual layers can be shown by using the Layer property in the results details view. MOM_TOR Beam rotation inertia Element Nodal POROSITY Material porosity Elemental Porosity, α = ρSolid/ρ PRESSURE Pressure Element Nodal PRES_BULK Dilation pressure for the Johnson-Holmquist brittle strength model Elemental SOUNDSPEED Material soundspeed Element Nodal STATUS Material Status Elemental 1 – elastic 2 – undergoing plastic flow 3 – failed due to effective criteria 4 – failed due to effective criteria 5 – failed due to stress/strain in principal direction 1 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 715 Features Variable Description Type 6 – failed due to stress/strain in principal direction 2 7 – failed due to stress/strain in principal direction 3 For layered section shells, the STATUS for individual layers can be shown by selecting the Layer number in the results details view. STOCH_FACT Stochastic factor applied when the stochastic property as defined in the material failure model Elemental STRAIN_XX Total strain XX Element Nodal STRAIN_YY Total strain YY Element Nodal STRAIN_ZZ Total strain ZZ Element Nodal STRAIN_XY Total strain XY.These are tensor shear strains, and not engineering shear strains. Element Nodal STRAIN_YZ Total strain YZ.These are tensor shear strains, and not engineering shear strains. Element Nodal STRAIN_ZX Total strain ZX.These are tensor shear strains, and not engineering shear strains. Element Nodal SUB_STN_X_SHELL_LAYER__# Shell total strain XX, sub-layer #.These are tensor shear strains, and not engineering shear strains. Element Nodal SUB_STN_Y_SHELL_LAYER__# Shell total strain YY, sub-layer #.These are tensor shear strains, and not engineering shear strains. Element Nodal SUB_STN_Z_SHELL_LAYER__# Shell total strain ZZ, sub-layer #.These are tensor shear strains, and not engineering shear strains. Element Nodal SUB_STN_XY_SHELL_LAYER__# Shell total strain XY, sub-layer #.These are tensor shear strains, and not engineering shear strains. Element Nodal SUB_STN_YZ_SHELL_LAYER__# Shell total strain YZ, sub-layer #.These are tensor shear strains, and not engineering shear strains. Element Nodal SUB_STN_ZX_SHELL_LAYER__# Shell total strain ZX, sub-layer #.These are tensor shear strains, and not engineering shear strains. Element Nodal SUBL_EPS_SHELL_LAYER_# Effective plastic strain, sub-layer # Element Nodal TEMPERATURE Material Temperature Element Nodal THICKNESS Shell Thickness Element Nodal TYPE Element category (element number returned) Elemental HEX: 100-101 PENTA: 102 TET: 103-104,106 PYRAMID: 105 QUAD: 107 TRI: 108 716 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Variable Description Type SHL: 200-202, 204 BEAM: 203 VISC_PRES Viscous pressure due to artificial viscosity Element Nodal VTXX Viscoelastic stress XX Element Nodal VTYY Viscoelastic stress YY Element Nodal VTZZ Viscoelastic stress ZZ Element Nodal VTXY Viscoelastic stress XY Element Nodal VTYZ Viscoelastic stress YZ Element Nodal VTZX Viscoelastic stress ZX Element Nodal For Euler (Virtual) Analyses The following results are multi-material variables in the AUTODYN solver. • EFF_PL_STN • INT_ENERGY • MASS • COMPRESS • DET_INIT_TIME • ALPHA • DAMAGE • TEMPERATURE For each Eulerian (Virtual) body in the analysis, a separate component will be available, which will allow the user to plot the result for the particular material associated with that body. The component name will be derived from the body name. There will also be an “ALL” component, which will displays results for all materials. Results for Lagrangian bodies can be viewed by selecting this “ALL” component. For a purely Lagrangian analysis, only the “ALL” component will be available to the user. For example, an analysis has two Eulerian (Virtual) bodies (Solid, Solid) and a Lagrangian Body (Surface Body), as shown in the image of the Outline View below. In the User Defined Result Expression Worksheet, there are three components available for the multimaterial results, named SOLID, SOLID_2, and ALL. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 717 Features Note It may be necessary to delete and reinsert multi-material results in order to view result for databases created prior to Release 13.0 For NBS Tetrahedral Elements The element variables listed below can be used to visualize the variable values at the nodes. The variable values presented in the element are a volume weighted average of those at the nodes. • TEMPERATURE • SOUNDSPEED • DENSITY • COMPRESS • STRAINS (NORMAL AND SHEAR) • EFF_PL_STN • TIMESTEP • INT_ENERGY The following variables are available as calculated directly from the solver in the element: • EFF_STN Results Related Topics The following topics are covered in this section. Result Definitions Result Outputs Result Utilities Result Definitions The following topics related to result definitions are covered in this section. Applying Results Based on Geometry Averaged vs. Unaveraged Contour Results Clearing Results Data Peak Composite Results Material Properties Used in Postprocessing Scoping Results 718 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Solution Coordinate System Surface Body Results Unconverged Results Applying Results Based on Geometry The available result objects are based on the given geometry and the analysis type. The following tables outline which bodies can be represented by the various choices available in the drop-down menus and buttons of the Solution toolbar. Static Structural Analysis Geometry Solution Toolbar Options Deformation Strain Stress Tools User Defined Result Solid Body Total, Directional All choices All choices Stress, Fatigue,Contact1 Yes Surface Body Total, Directional All choices All choices Stress, Fatigue,Contact1 Yes Line Body Total, Directional None None Contact1, Beam Yes Transient Analysis Geometry Solution Toolbar Options Deformation Strain Stress Tools User Defined Result Solid Body All choices All choices All choices Stress, Fatigue,Contact1 Yes Surface Body All choices All choices All choices Stress, Fatigue, Contact Yes All None None Contact1, Beam Yes Line Body Modal and Linear Buckling Analyses Geometry Solution Toolbar Options Deformation Strain Stress Tools User Defined Result Solid Body Total, Directional All applicable choices, except Energy All choices None Yes Surface Body Total, Directional All applicable choices, except Energy All choices None Yes Line Body Total, Directional None None None Yes Random Vibration Analysis and Response Spectrum Analysis Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 719 Features Geometry Solution Toolbar Options Deformation Strain Stress Tools User Defined Result Solid Body Directional, Directional Velocity, Directional Acceleration Normal, Shear Equivalent (von-Mises), Normal, Shear None No Surface Body Directional, Directional Velocity, Directional Acceleration Normal, Shear Equivalent (von-Mises), Normal, Shear None No Line Body Directional, Directional Velocity, Directional Acceleration None None None No Steady-State Thermal and Transient Thermal Analyses Geometry Solution Toolbar Options Thermal User Defined Result Solid Body All choices Yes Surface Body All choices Yes Temperature Yes Line Body Magnetostatic Analysis Geometry Solution Toolbar Options Electromagnetic Solid Body Surface Body Line Body All choices User Defined Result 2 Yes Not Applicable Yes None Yes Electric Analysis Geometry Solution Toolbar Options Electric User Defined Result All choices Yes Surface Body Yes Yes Line Body Yes Yes Solid Body Harmonic Analysis (Deformation, Strain, Stress) Geometry Solution Toolbar Options Deformation 720 Strain Stress Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Solid Body All choices3 All choices, except Energy,Thermal,Equivalent Plastic All choices Surface Body All choices3 All choices, except Energy,Thermal,Equivalent Plastic All choices Line Body All choices None None Harmonic Analysis (Frequency Response, Phase Response, User Defined Result) Geometry Solution Toolbar Options Frequency Response 3 Phase Response3 User Defined Result Solid Body All choices All choices No Surface Body All choices All choices No Line Body All choices All choices No 1 - Contact results are not reported, and are not applicable to the following: • Edges. • MPC contact. • Target side of asymmetric contact. 2 - Electric Potential can only be scoped to conductor bodies. 3 - See Harmonic Analysis section. Averaged vs. Unaveraged Contour Results Normally, contour results in the Mechanical application are displayed as averaged results. Some results can also display as unaveraged contours. Averaged contours will average elemental nodal results across element and geometric discontinuities but will never average results across bodies. Using the Mechanical APDL application terminology, unaveraged contour results display as element nodal contours that vary discontinuously even across element boundaries. These contours are determined by linear interpolation within each element and are unaffected by surrounding elements (that is, no nodal averaging is performed). The discontinuity between contours of adjacent elements is an indication of the gradient across elements. Results that include the unaveraged contour display option are most elemental quantities such as stress or strain. This option is not available for degree of freedom results such as displacements. Nodal averaging of element quantities involves direct averaging of values at corner nodes. For higherorder elements, midside node results are then taken as the average of the corner nodes. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 721 Features Note If an elemental result is scoped to a surface body, then there may be two sets of results at each node (Top and Bottom) and sometimes a third set of results (Middle). At release 12.0, if the solver writes Middle results to the result file, then Mechanical displays these results if the Shell Face setting in the Details view equals Middle (Membrane). If the solver did not write Middle results to the result file, then Mechanical displays the average of Top and Bottom if the Shell Face setting in the Details View is Middle (Membrane). For a given node on the shell, the Mechanical application will average Top results, separately average Bottom results, and separately average Middle results. When you export a result in the Mechanical application that is set to Top/Bottom, you may note that a node number is repeated in the Excel file. This is because both the Top and Bottom stresses are listed. To determine if a particular result item includes the option for displaying unaveraged contours, highlight a Solution object in the tree and insert the result item from the toolbar or through a right mouse button click. Then, with the result object selected, check the Details view under the Integration Point Results group. The result item includes the option for displaying unaveraged results if a Display Option field exists. You can display contour results by setting the Display Option field to one of the following: • Unaveraged: Displays unaveraged results. • Averaged: Displays averaged results. • Nodal Difference: Computes the maximum difference between the unaveraged computed result (for example, total heat flux, equivalent stress) for all elements that share a particular node. • Nodal Fraction: Computes the ratio of the nodal difference and the nodal average. • Elemental Difference: Computes the maximum difference between the unaveraged computed result (for example, total heat flux, equivalent stress) for all nodes in an element, including midside nodes. • Elemental Fraction: Computes the ratio of the elemental difference and the elemental average. • Elemental Mean: Computes the elemental average from the averaged component results. Characteristics of unaveraged contour displays: • Because of the added data involved in the processing of unaveraged contour results, these results take a longer time to display than averaged results. • Occasionally, unaveraged contour result displays tend to resemble a checkerboard pattern. • Capped Isosurface displays can have missing facets. Clearing Results Data You can clear results and meshing data from the database using the Clear Generated Data command from the File menu, or from a right-mouse click menu item. This reduces the size of the database file, which can be useful for archiving. To clear all results data, simply select the Solution object and choose the Clear Generated Data menu item from the File menu or from a right-mouse click menu. You can clear individual results by selecting a result object before choosing the Clear Generated Data menu item. 722 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Note Anytime the geometry or mesh has been changed, you should clear all results data. If meshes become obsolete, the solution and results are totally cleared. Peak Composite Results With this feature you can view the result contours over an independent variable such as time in a static or transient structural analysis, or frequency/phase in a harmonic analysis, or cyclic phase in a cyclic modal analysis. Using time as an example, the color in the contour represents one of the following: the results at the specified time, the results for the specified set, the maximum result over time or the time when the maximum result occurred for the node, element, or sample point. To view peak composite results: 1. Insert a result under solution. 2. In the Details view, under Definition, click the By list and select the result view. Choices are the following: • Maximum Over Time or Time of Maximum: Each node/element/sample point is swept through the result sets to find its maximum result. Either the result itself is reported (sometimes referred to as a "peak hold") or the time at which the peak occurred is reported. This result is applicable in static and transient analyses. • Maximum Over Frequency or Frequency of Maximum: With these options chosen, phase angle is held constant and each node/element/sample point is swept through frequency range to find its maximum result. This result is applicable in harmonic analyses only. • Maximum Over Phase or Phase of Maximum: With these options chosen, frequency is held constant and each node/element/sample point is swept through a phase angle of 0 to 360 in 10 degree increments find its maximum result. This result is applicable in harmonic analyses only. • Maximum Over Cyclic Phase or Cyclic Phase of Maximum: Each node/element/sample point is swept through a phase angle of 0 to 360 in 10 degree increments find its maximum result. This result is applicable in cyclic modal analyses only and for harmonic indices greater than zero. Note There is no affiliation between composite results and composite elements. Material Properties Used in Postprocessing The material properties listed below are used in postprocessing calculations to produce the displays of probe and contour results. For reference, the corresponding labels (Lab argument) for the MP command in Mechanical APDL are included in parentheses. • Elasticity modulus (EX, EY, EZ) • Shear modulus (GXY, GYZ, GXZ) • Poisson's ratio (NUXY, NUYZ, NUXZ) • Thermal conductivities (KXX, KYY, KZZ) • Magnetic permeability (MURX, MURY, MURZ) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 723 Features The following results, together with their identifiers (see User Defined Results (p. 702)), are directly affected by the material property values: • Equivalent Strain - uses only NUXY Poisson's ratio 1. Plastic (EPPL) and Creep (EPCR) strain always use NUXY = 0.5. 2. Elastic (EPEL), Thermal (EPTH) and Total (EPTO) default to 0.0. • Structural Error - uses elasticity modulus, shear modulus and Poisson's ratio. • Thermal Error - uses thermal conductivities • Magnetic Error - uses magnetic permeability An error message is generated if an associated material property is not defined when evaluating Structural, Thermal or Magnetic Error result. If Poisson's ratio is not defined when evaluating Equivalent Strain, the Poisson's ratio will assume a zero value. Other results affected by material property values include Stress Tool and Fatigue Tool results. Note If a material property is temperature dependent, it is evaluated at the reference temperature of the body to be used in the computation for the result. Scoping Results All result objects can be scoped to named selections that are based on geometric entities. In addition, some results can be scoped to named selections that are based on underlying meshing entities as well. This is known as “nodal scoping”. Results that support nodal scoping are listed below Once a solution is computed, the scope of the result object cannot change. You must either add a new result object with the desired scope, or you can right mouse click on that result item, and choose Clear Generated Data to change its scope. Result scoping has an impact on convergence. Refinement doesn't happen outside the scope for a given convergence control. Multiple convergence controls are possible, however. Geometric Scoping Most result objects (such as stress, stress tool, fatigue life, temperature) can be scoped to edges, a single vertex, faces, parts, bodies, or the entire assembly. Shape results can be scoped only to the assembly, parts, or bodies. Harmonic results can be scoped only on vertices, or edges, or faces. Nodal Scoping The following results can be scoped to named selections that are based on underlying meshing entities: • Equivalent, Principal, Intensity, Maximum Shear, Shear, and Normal Stresses • Equivalent, Principal, Intensity, Maximum Shear, Shear, and Normal Strains • Thermal, Equivalent Plastic, Equivalent Creep, Equivalent Total Strains 724 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application • Stress Tool Results • Fatigue Tool Results • Gasket Pressures • Gasket Closures • Deformations • Velocities • Accelerations • Pressures • Densities • Beam Axial Forces • Beam Bending Moments • Beam Torsional Moments • Beam Shear Forces • Velocities (PSD) • Accelerations (PSD) • Equivalent Stress (PSD) • Velocities (RS) • Accelerations (RS) • Equivalent Stress (RS) • Angular Displacements • Angular Velocities • Angular Accelerations • Temperature • Heat Flux • Magnetic Flux Density • Magnetic Field Intensity • Magnetic Forces • Electric Voltages • Electric Flux Density • Electric Field Intensity • Electric Current Density Notes The following are known characteristics related to nodal scoping: • If all nodes of an element face are scoped, then Mechanical will draw contour bands on the entire face. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 725 Features • If some nodes of an element face are not scoped, then Mechanical will draw the face as transparent and draw the scoped nodes in contour colors. • As is the case with other scoping that occurs within a body (such as vertex or edge), any applicable averaging will be done considering all the nodes on a body. Solution Coordinate System Solution Coordinate System is available as a Coordinate System option in the Details view for most result objects. If you are familiar with the Mechanical APDL application commands, Solution Coordinate System is an implementation of the RSYS,SOLU command, where for element results, such as stress, a coordinate system is produced for each element. If these individual element coordinate systems are aligned randomly, you can re-align them to a local coordinate system to obtain a uniform alignment. Viewing results in the element solution coordinate system has value since results in a local coordinate system aligned with a certain shell direction are typically more meaningful than results in a global coordinate system. For example, seeing bending and in-plane stresses have meaning in a local coordinate system, but have no meaning in a global coordinate system. Application The following are typical applications for viewing results in a solution coordinate system: • Viewing results in a particular direction for surface bodies or “solid shell” bodies, that is, solids meshed with the Solid Shell element option (see the Meshing Help: Sweep description in the Method Control section). • Viewing results in a random vibration, spectrum, or surface bodies in an explicit dynamics analysis. Results for these analysis types only have meaning in a solution coordinate system. Background The meshing of surface bodies and solid shell bodies result in coordinate systems whose alignment is on a per element basis, in contrast to solid body element types whose coordinate systems are aligned with the global coordinate system by default. Surface body alignment on a per element basis can lead to results with totally random alignment directions as shown below. To produce meaningful results for surface body and solid shell bodies, you can re-align the random direction of each element's solution coordinate systems to a uniform direction of a local coordinate system. An example is shown below. 726 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Procedure To correct for random coordinate system alignments in surface bodies and solid shell bodies, and to ensure a consistent alignment: 1. For each part, create a local coordinate system to specify the alignment of the elements of the part. 2. Choose the Solution Coordinate System option for the result. Note • The Coordinate System setting for result objects in a random vibration, spectrum, or explicit dynamics analysis is set to Solution Coordinate System by default and cannot be changed because the results only have meaning when viewed in the solution coordinate system. • The solution coordinate system is not supported by explicit dynamics analyses for results. Surface Body Results For surface bodies, stress and strain results at the top and bottom faces are displayed simultaneously, by default. (See Surface Body Shell Offsets (p. 321) for information on identifying the top and bottom faces.) The contours vary linearly through the thickness from the top face to the bottom face. However you can choose to display only the Top, Middle, or Bottom stress/strains in the Details view of the result item. Selecting Top, Middle, or Bottom will display the result at the selected location as a uniform contour through the thickness. Middle Stresses • Normal and Shear results The middle stresses are calculated at the shell mid-surface or at each layer mid-surface if layers are present. The Middle option for Shell gives the actual result values at the mid-surface if the solver was directed to calculate these results. In Mechanical APDL terminology, the solver computes results at mid-surface if KEYOPT(8) for the shell element is set to 2 at the time of element creation. Otherwise, the Middle results are computed as the average of the Top and Bottom results, that is, (Top + Bottom) / 2. Note that these results are valid only for linear analyses. • Equivalent and Principal results Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 727 Features These results are derived from the Normal and Shear results. Hence the Normal and Shear component results for Middle are computed first, and then the Equivalent and Principal results are derived. Element Nodal results (like stress/strain), as well as EDIR- and PNUM-type Elemental results, can be plotted on a specific layer by entering the desired Layer number in the Details view of the result object. Elemental results outputting volume or energy are calculated for the entire element, regardless of the requested layer. If the Layer specified does not exist for a particular surface body, the display of the result will be translucent with zero values for minimums and maximums on that body. If you enter 0 for Layer, it defaults to the Entire Section. Note • A Layer number must be specified to calculate the Middle stresses and strains. If you set Layer to 0 (Entire Section) while Shell is Middle, the Shell option will become invalid. Similarly, if you have Layer set to Entire Section and you try to set Shell to Middle, Shell will become invalid. • If there is a Layered Section in the model, convergence is not supported for results. • If Layer is Entire Section, Top stresses and strains are for the top surface of the topmost layer and the Bottom stresses and strains are for the outer surface of the bottom layer. • If a Layered Section is present in the model and you enter a number larger than the maximum number of layers that exists in the model, the Layer field will become invalid. • All stress tool results and all fatigue tool results are unsupported if Layered Sections are present in the model. For Explicit Dynamics Layer Results Normal/shear stresses and strains are available in global and solution coordinate systems. Stress and strain results for individual layers may be selected by using the Layer property in the result’s Details view. Only a single result is available per layer. Unconverged Results A nonlinear analysis may fail to converge due to a number of reasons. Some examples may be initially open contact surfaces causing rigid body motion, large load increments, material instabilities, or large deformations that distort the mesh resulting in element shape errors. In the Mechanical application, you can review this unconverged result as well as any converged results at previous time points. These results are marked in the legend of contour/vector plots as ‘Unconverged’ indicating that these results must be used only for debugging purposes. Note that a plot of NewtonRaphson residuals is a very useful tool to identify regions of your structure that led to the convergence difficulty. 728 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Note • Results in Solution Combination objects that use partial solutions will not be solved. You can view partial results but cannot use them in further post/solution work. • Newton-Raphson residuals is a very useful tool to identify regions of your structure that led to the convergence difficulty. • The handling of unconverged solutions is the same for both probes and results. Result Outputs The following topics related to result outputs are covered in this section. Chart and Table Contour Results Coordinate Systems Results Eroded Nodes in Explicit Dynamics Analyses The Euler Domain in Explicit Dynamics Analyses Path Results Probes Surface Results Vector Plots Chart and Table Selecting the Chart and Table icon button allows you to create charts of loads and/or results against time. In addition you can also chart result quantities against a load or another results quantity. You can also chart loads or results from across different analyses; for example, to compare the displacement response from two different transient runs with different damping characteristics. Use the Chart and Table feature to: • Chart load(s) and result(s) vs time. • Chart multiple harmonic response plots vs. frequency. • Change x-axis to plot a result against a load or another result. • Compare results across analyses. • Visualize and compress data into an easy-to-understand report. Select Loads and Results from Tree Press the Control or Shift key to select multiple objects of interest. In doing so, note that: • You can choose objects in the tree that belong to different analyses of a model. However all objects must belong to the same Model. • Only loads, probes and results that can be contoured are added to the chart. • For result items the variation of minimum and maximum values is plotted as a function of time Select Chart icon from Standard Toolbar This adds a new chart object to the tree structure. You can add as many charts as needed. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 729 Features Determining Data Points You can choose a mixture of loads and results that may even span different analyses. In these cases there can be a mismatch between the time points at which the loads are defined and the time points at which results are available. For example in case of a nonlinear transient stress analysis under constant load, the load has a single value but there can be many time points where results are available. The below interpolation scheme is used to create charts when such mismatch occurs. • Loads are interpolated or extrapolated to the time points at which result values or other load values. • Results are not interpolated or extrapolated Details View Content The main categories are: • Definition: – • Outline Selection: Lists how many objects are used in the chart. Clicking on the number of objects highlights the objects in the tree allowing you to modify the selection if needed. Chart Controls: – X-Axis: By default the data of the selected objects are plotted against time. You may choose a different load or result quantity for the x-axis. For example you can plot a Force – Deflection curve by choosing the deflection to be the X-axis. – Plot Style: display as Lines, Points, or Both (default). – Scale: → Linear (default) - plot as linear graph. → Semi-Log (X) - X-Axis is plotted logarithmically. If negative axis values exist, this option has no effect. → Semi-Log (Y) - Y-Axis is plotted logarithmically. If negative axis values exist, this option has no effect. → Log-Log - X-Axis and Y-Axis are plotted logarithmically. If negative axis values exist, this option has no effect. • Axis Labels: – X-Axis and Y-Axis: You can enter appropriate labels for the X and Y axes. In doing so, note that: → The X and Y axes always show the units of the item(s) being charted. These units are appended to any label that you enter. → When multiple items are plotted on the Y-axis the units are determined as follows: If all the items plotted on the Y-axis have the same units then the unit is displayed. For example, if all items are of type deformation and the active unit system is British Inch unit system then the unit is displayed as Inch. If the items plotted on the Y-axis are of different types for example, stress and strain then Normalized is displayed for unit. → When determining pairs of points to plot on the chart when X-axis is not time be aware that time is still used to determine the pairs of points to plot when an item other than time is used for the x-axis. Both the X-axis quantity and the Y-axis quantity must share a common time point to be considered a valid pair. • 730 Report: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application – Content: By default both the chart as well as the data listing of the objects gets added to reports. Instead you may choose to only add the chart or only add the data listing or exclude the chart from report. Note that only tabular data or chart data with two or more points is displayed in the report. – • Caption: You may enter a caption for the chart. The caption will be included in the report. Input Quantities: – Input Quantities: Any valid load object added to the chart gets displayed under Input Quantities. If a load has multiple components then each component will get a line in this details group. – Output Quantities: Any valid result object added to the chart gets displayed under Output Quantities. If a result has multiple components then each component will get a line in this details group. In using Input and Output Quantities, note that: – Naming and legend: Each object added to a chart is assigned a name and a legend label. The name is simply the object name in the tree if there are no components associated with the object. An example would be a Y displacement probe. For objects that have multiple components the component direction or name will get added to the object name. For example adding ‘Equivalent Stress’ result item to a chart will result in two items getting added – ‘Equivalent Stress (min)’ and ‘Equivalent Stress (max)’. – Each name is preceded by a one letter label such as [A] or [B]. This label is also displayed on the corresponding curve in the chart and is used to associate the object name with the curve. – The default setting is to display the item in the chart and data grid. You can exclude an item by setting this field to Omit. Omitting an item removes the corresponding data from both data grid and chart. Be aware that an item chosen for X-axis cannot be omitted and this field will be reset to Display for that item. Chart Display • • Legend: You can use Show Legend /Hide Legend option via the right mouse button context menu to display or hide legends in the charts, the following limitations withstanding. – A maximum of 10 items will get displayed due to space limitations. – If more than 10 items are displayed in a chart then the curves will show all the prefixes even though the legend is limited to 10 items. You can refer to the details of the chart for the description of the items that corresponds to a prefix. Normalization: Scaling of Y-axis is determined as follows. – Single item on Y-axis : Scaling is based on the minimum and maximum values of the item plotted – Multiple items on Y-axis that have same unit type: Scaling is based on the minimum and maximum values of the items plotted. For example, plot applied pressure load and a stress result against time. – Multiple items on Y-axis that have different unit types: In this case each curve is normalized to lie between 0 and 1, that is the minimum value is treated as zero and the maximum value as one. The label of the Y-axis reflects this by appending Normalized to any user specified label. Note that the data grid displays the actual values always. Datagrid Display It is read-only. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 731 Features Contour Results Most result types can be displayed using contours or vectors. The Result context toolbar applies to Solution level objects that display contour or vector results. Coordinate Systems Results The following topics are addressed in this section: Nodal Coordinate Systems Results Elemental Coordinate Systems Results Rotational Order of Coordinate System Results Nodal Coordinate Systems Results Every node in a model is associated with a coordinate system that, by default, is aligned with the global Cartesian coordinate system. If any of the X, Y, or Z axes of an individual node is rotated, the resulting coordinate system will typically not be aligned with the global Cartesian coordinate system. Using this feature, you can display nodal result rotations either as Euler rotated triads at each node location, or as contours that represent an Euler rotation angle about an individual nodal axis. Boundary conditions are highly dependent upon Euler angles. To display nodal coordinate systems results: Highlight the Solution object, and choose one of the following options from the Coordinate Systems drop down menu in the toolbar. A corresponding object will be inserted in the tree. • Nodal Triads: Displays an XYZ triad at each node representing the resulting rotation of the node's coordinate system compared to the global Cartesian coordinate system. See Rotational Order of Coordinate System Results (p. 733) for details. • Nodal Euler XY Angle: Displays a contour plot representing the magnitude of the resulting Euler angle rotation at each node about the Z axis. • Nodal Euler YZ Angle: Displays a contour plot representing the magnitude of the resulting Euler angle rotation at each node about the X axis. • Nodal Euler XZ Angle: Displays a contour plot representing the magnitude of the resulting Euler angle rotation at each node about the Y axis. Note For the ANSYS solver, nodal coordinate systems will not vary from time step to time step. Elemental Coordinate Systems Results Every element in a model is associated with a coordinate system that, by default, is aligned with the global Cartesian coordinate system. If any of the X, Y, or Z axes of an individual element is rotated, the resulting coordinate system will typically not be aligned with the global Cartesian coordinate system. Using this feature, you can display elemental result rotations either as Euler rotated triads at each element's centroid, or as contours that represent an Euler rotation angle about an individual elemental axis. Shell stresses are highly dependent upon Euler angles. To display elemental coordinate systems results: 732 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Highlight the Solution object, and choose one of the following options from the Coordinate Systems drop down menu in the toolbar. A corresponding object will be inserted in the tree. • Elemental Triads: Displays an XYZ triad at each element centroid representing the resulting rotation of the element's coordinate system compared to the global Cartesian coordinate system. See Rotational Order of Coordinate System Results (p. 733) for details. Note You may need to use the Wireframe viewing mode to see a particular triad in an element. • Elemental Euler XY Angle: Displays a contour plot representing the magnitude of the resulting Euler angle rotation at each element centroid about the Z axis. • Elemental Euler YZ Angle: Displays a contour plot representing the magnitude of the resulting Euler angle rotation at each element centroid about the X axis. • Elemental Euler XZ Angle: Displays a contour plot representing the magnitude of the resulting Euler angle rotation at each element centroid about the Y axis. Note For the ANSYS solver, it is possible for elemental coordinate systems to vary from time step to time step. Rotational Order of Coordinate System Results The following rotational convention is used for both Nodal Coordinate Systems Results (p. 732) and Elemental Coordinate Systems Results (p. 732): 1. The first rotation is called ... Euler XY and is in the X-Y plane (X towards Y, about Z). 2. The second rotation is called ... Euler YZ and is in Y1-Z1 plane (Y1 towards Z1, about X1). 3. The third rotation is called ... Euler XZ and is in X2-Z2 plane (Z2 towards X2, about Y2). X1, Y1, and Z1 refer to the coordinate system axes after the initial rotation about the global Z axis. X2, Y2, and Z2 refer to the coordinate system axes after the initial rotation about the global Z axis and subsequent rotation about X1. See Figure 3.2: "Euler Rotation Angles" from the Modeling and Meshing Guide for a pictorial representation of this convention. Eroded Nodes in Explicit Dynamics Analyses During explicit dynamics analyses, highly distorted elements may be automatically removed (eroded) from the model. As elements erode, nodes may become free (not connected to any element). These nodes have mass and inertia and can impact other structures. By default, eroded nodes are plotted as red dots (see below). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 733 Features The View> Eroded Nodes toggle from the Main Menu allows you to remove the eroded nodes from the display, as shown below. 734 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application The Euler Domain in Explicit Dynamics Analyses In an Explicit Dynamics Analysis, if any bodies have a reference frame set to Eulerian (Virtual), an Euler domain is created that encloses all bodies in the model. The Euler domain is a structured hexahedral mesh. The exact size and resolution of the Eulerian domain can be controlled in the Euler Domain Controls section of the Analysis Settings Details view. Bodies with a reference frame set to Eulerian (Virtual) are used to initialize material into the Euler domain. The surfaces of the Eulerian bodies are not tracked exactly; the original mesh created by the mesher is discarded and the location of materials in the Euler domain is stored as a material (volume) fraction for each of the Euler cells. A representation of the material surface can be displayed as an isosurface for a material fraction value of 50%. A comparison of Lagrangian (left) and Eulerian (right) representations of the same body is shown below. When plotting results on Eulerian bodies, the results calculated in the Eulerian domain are then interpolated onto this isosurface. If the Euler Tracking By Body option is selected in the Analysis Settings Details view, results may be scoped to Eulerian bodies in the same way as for Lagrangian bodies, and body trackers are available for Eulerian parts. Additional considerations: • Displacement, strain, and BOND_STATUS results are not available for scoped results. • Probes and path plots are not supported for Eulerian bodies. • External Force and Contact Force trackers will return zero for Eulerian bodies. • Point trackers for Strain are not supported. • Deformation scaling (i.e. Undeformed, .5 Auto, AutoScaling, 2x Auto, 5x Auto ) is not available for Eulerian bodies. • Show undeformed wireframe is not available for Eulerian bodies. • Show undeformed model is not available for Eulerian bodies. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 735 Features • Although it is not possible to view the Eulerian domain directly within the Mechanical application, the size and resolution of the domain are indicated in the graphics window when Analysis Settings are selected in the outline view; if required, the model may be transferred to an AUTODYN component system where the Euler mesh can be displayed. • There may be issues with solver efficiency for analyses containing more than ten Eulerian bodies. Further discussion of the Eulerian solver used by Explicit Dynamics Analyses, including a description of the theory, can be found in Key Concepts of Euler (Virtual) Solutions in the ANSYS Mechanical Application User's Guide. Path Results If you have already defined a path, you can view the path results by highlighting the result object, and in the Details view, setting Scoping Method to Path, then choosing the name of the particular path that you defined. An example path result plot is shown below. In this example, the Number of Sampling Points for the Path object was set to 47. Results were calculated for each of these 47 points as shown in the Graph below. 736 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Probes This section examines the general function of the probe tool in Workbench as well as the specific probe types that are available in the Mechanical application. It also describes the Details view options associated with the Probe object. Overview and Probe Types Probe Details View The following table shows the limitations of the Probe results. If you make incorrect selections in the Details view for any of the probes, all the probes under solution remain unsolved. Probe Scope Deformation Vertices, Edges, Faces, or Volume Stress Strain Thermal Flux Flux Density 1 1 Flux Intensity Must be Scoped to a rigid part Components and Principals Result Selection invalid All Result Selection invalid X X X X X X X 1 X Velocity X Acceleration X Position Angular Velocity X 1 X 1 Angular Acceleration X 1 - Not supported in explicit dynamics analyses. Overview and Probe Types Probes allow you to find results at a point on the model, or minimum or maximum results on a body, face, edge, or vertex. The following probe types are available: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 737 Features • Structural Probes (p. 671) • Thermal Probes (p. 687) • Magnetostatic Probes (p. 691) • Electric Probes (p. 694) You insert a Probe object under Solution in the tree, from the toolbar or from a right mouse button click. You can adjust options in the Details view or add results for specific points/geometry. When you solve the probe, the display of the result probe reveals the displaced mesh for the specified time. The probe shows values over time and for a specified time. The Details view shows either the maximum or minimum value over time. Note You cannot turn off the time history for result probe. Scoping: Since probes are customized for the particular result type, different probes allow different scoping mechanisms. For example a reaction probe allows scoping to a boundary condition while a stress probe will allow scoping to an x, y, z location on the geometry. Please refer to the “Characteristics” column of the tables in the linked sections above for scoping. Use Location Method in the Details view of the probe to scope to the desired entity. When you create a probe by clicking on a location or by assigning a coordinate system, Workbench associates a small subset of nodes which reside near the probe. The value of this probe is interpolated from the values at these neighboring (undeformed) nodes. The interpolation is based on the original node locations and not a function of the displaced position of the probe or of the nodes. When picking a specific x, y, z location, you can obtain the probe result directly at the closest corner node, without extra interpolation, by right-clicking on the probe object in the tree and choosing Snap to mesh nodes from the context menu. The identification number of the closest corner node is displayed as the Node ID in the Details view of the probe in the Results category . Note For surface bodies with expanded thickness, because the snapping location is located on the expanded mesh, while other items such as the original x, y, z location and the node ID are on the non-expanded mesh, you are advised to turn the visual expansion off in order to best view these items. When you create a probe by scoping a vertex, edge, face, or volume, the results reported for the probe are for the undisplaced nodes and elements. The displaced location of the probe (if any) is not used in any way to calculate results. If the probe is scoped to any suppressed parts, then the probe will not solve or evaluate results. This strategy exists to prevent numeric contributions from elements and nodes that are not scoped. Results output coordinate system: Some probes such as the Directional Deformation probe allow the results to be calculated and displayed in a coordinate system of your choice. Some other probes such as a Spring probe allow results to be output only in a specific coordinate system. Please refer to Orientation Coordinate System: entry under the “Characteristics” column in the probe tables (see links above) regarding what coordinate systems are allowed and what the default coordinate system is. You can use Orientation in the Details view of the probe to change the output coordinate system. 738 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Note When the Orientation Coordinate System is Global Cartesian, the triad symbol is not displayed. The exception is for Torque probes in magnetostatic analyses, where the global triad is displayed and the direction vector is placed at the global origin. Probe Details View Presented below is an overview of the Details view properties for all probe types. Every probe type displays the same categories but the fields and options vary depending on the application of the particular probe. All fields and options are included in the table below. Category Definition Fields Options Type: Read-only - Displays the probe name. Location Method: Sets the probe location. Geometry Selection: Use to select an x,y,z point, edges, vertices, faces or bodies using toolbar filter buttons. After making your selection, click in the Geometry field, then click the Apply button. If you select a point using the x,y,z picking method, the X,Y,Z Coordinates of the location will be shown. For the other geometries, a Spatial Resolution option is displayed in the Options category.This allows you to Use Maximum or Use Minimum result values across the given selection. Coordinate System: Use to set the location according to a coordinate system that you defined previously under the Model object.This choice displays a Location drop-down list where you pick the particular coordinate system.The X,Y,Z Coordinates of the location are also displayed. Remote Points: Use to scope the probe to an existing remote point that you pick from a Remote Points drop down list. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 739 Features Category Fields Options Boundary Condition: Use to scope the probe to an existing boundary condition that you pick from a Boundary Condition drop down list. Contact Region: Use to scope Force Reaction and Moment Reaction probes to an existing contact region that you pick from a Contact Region drop down list. Beam: Use to scope the probe to an existing boundary condition that you pick from a Beam drop down list. Geometry: See Location Method set to Geometry Selection above. Select a geometry. Orientation: Sets the direction of the coordinate system specified under Location. See Location Method set to Coordinate System above. Available coordinate systems X coordinate: Read-only. See Location Method set to Geometry Selection or Coordinate System above. Y coordinate: Read-only. See Location Method set to Geometry Selection or Coordinate System above. Z coordinate: Read-only. See Location Method set to Geometry Selection or Coordinate System above. 740 Summation: Displayed only for Moment Reaction probes when Orientation is also displayed. Allows you to specify the summation point where the moment reaction is reported. Centroid or Orientation System (that is, the coordinate system you specified with the Orientation setting. Extraction: Displayed only for Force Reaction and Moment Reaction probes Source(Underlying Element) or Target(Underlying Element). For Force Reaction probes, a Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Category Options Fields Options when Location Method is set to Contact Region. Source(Contact Element) option is also available. Orientation Method: Displayed only for Joint Probe. Joint Reference System or User Specified Result Selection List of available results Display Time End time or Time step Spatial Resolution: See Location Method set to Geometry Selection above. Use Minimum or Use Maximum Result Type List of available results for a Joint Probe. Results Read-only - Values of result you select in the Result Selection or Result Type list. The Node ID is displayed if you used the Snap to mesh nodes feature. Maximum Value Over Time Read-only - Maximum value of the results you select over time in stepped analysis. Minimum Value Over Time Read-only - Minimum value of the results you select over time in stepped analysis. Information Read-only - Time, Load Step, Substep, and Iteration Number information associated with the result. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 741 Features Note • When you set Location Method to Coordinate System, the probe traverses the primary axes to determine where the hits occur on the model. The hit closest to the origin of the coordinate system is used. This behavior is similar to placing a laser at the origin of the system and then shooting the laser sequentially along positive and negative direction of x, y, z axis. • Probe objects scoped to x, y, z picking locations are achieved in such a way that a projection of the picked location in screen coordinates occurs onto the model based on the current view orientation, in other words, normal to the display screen onto the model at the picked location on the screen. If the geometry is updated, the update of the projection will follow the original vector that was established “behind the scenes” when the x, y, z pick was first made. Therefore the update of Probe objects scoped to x, y, z picking locations may not appear to be logical since it follows a vector that was established dependent on a view orientation when the original pick was made. • Probe animation for joints is only supported if there is at least one rigid body. • Probes are designed to work with geometry entities only. They are not intended to probe displacements on remote locations. • The details view of the probe shows either the maximum or the minimum result values but not both. • If you attempt to intersect such probes with a line body, Workbench will issue a warning message. No results (such as stresses or displacements) will appear in the details view of the probe. Surface Results If you have already defined a surface, you can view the surface results by first adding a standard result or user defined result, and in the Details view of the result object, setting Scoping Method to Surface, then choosing the name of the particular surface that you defined. The Details view for a surface result contains an additional item called Average, which can be parametrized. For example, average stress over the surface is given by: { ∫ Stress(X, Y, Z) dAREA} / {TOTAL_AREA} For some results, the Details view will also contain a Total quantity, such as Total Force, which also can be parametrized. The Total quantities are presented in the following table. Currently, if you desire a Total quantity for Heat Flux, Magnetic Flux Density, Current Density, or Electric Flux Density, you must choose a vector user defined result. Total Force (as integrated from principal stress vectors) is available to both standard and user defined results. Identifier Result Surface Integral TFVECTORS Heat Flux Heat Rate BVECTORS Magnetic Flux Density Magnetic Flux DVECTORS Electric Flux Density Charge 742 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Identifier Result Surface Integral JTVECTORS, JCVECTORS Current Density Current SVECTORS (also see Vector Principals) Stress Tensor Force Vector Plots Certain result items can be displayed using vectors such as the vector principal stresses or vector principal strain results. Similarly total deformation, total velocity and total acceleration can also be displayed using vectors. Using the Graphics button, you can display results as vectors with various options for controlling the display. See the Vector Display Context Toolbar (p. 295) section for more information. Result Utilities The following topics related to result utilities are covered in this section. Adaptive Convergence Animation Capped Isosurfaces Dynamic Legend Generating Reports Renaming Results Based on Definition Results Legend Results Toolbar Solution Combinations Adaptive Convergence Refer to the Adaptive Convergence (p. 787) section. Animation The Animation feature displays in the Graph window when you select a result object in the Mechanical application. Here is an example of the Graph window with a result object selected. The specific Animation functions are presented below. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 743 Features Control Description Play: Initiates a new animation. (same toolbar location as Play) Pause: Pauses an existing animation. Choosing Play after Pause does not generate new animation frames. When the animation is paused, as you move the cursor across the graph, the cursor's appearance changes to a double horizontal arrow when you hover over the current frame indicator. With the cursor in this state, you can drag the frame indicator to define a new current frame.The result graphic will update accordingly. Stop: Halts a result animation. Choosing Play after Stop generates new animation frames. Distributed: For static analyses, frames display linearly interpolated results. Frame 1 represents the initial state of the model and the final frame represents the final results calculated by the solver. For stepped and transient analyses, the frames in Distributed mode are distributed over a time range selected in the graph.1 Result Sets: (available only for stepped and transient simulations) Frames represent the actual result sets that were generated by the solver.1 Frame Markers: display what time points are being used in the animation by placing a vertical line at the time points. Select the number of frames in the animation. Select the desired amount of time for the entire animation. Export Video File: Saves animation as an AVI file. Note When exporting an AVI file, make sure that you keep the Workbench module window in front of other windows until the exporting is complete. Opening other windows in front of the module window before the exporting is complete may cause those windows to be included in the AVI file capture. Damped Modal Animation:Turns on time decay animation of complex modes in a Modal Analysis that has damping applied.This button is not available (grayed out) for any of the following: • 744 Any analysis type other than modal. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Control Description • Any modal analysis whose Damped setting (under Solver Controls) is set to No. • Any modal analysis whose Damped setting is set to Yes, and whose Solver Type is set to Reduced Damped, and Store Complex Solution is set to No. 1 - For stepped and transient simulations, as you move the cursor across the graph, the cursor's appearance changes to a scope icon for solved solution points. Animation Behavior Depending upon the type of simulation that you perform, the behavior of the resulting animation varies. For a static simulation, the progression of an animation occurs in a linear forward/backward manner. The color contours begin with the initial condition, advance to the solution state, and then “rewinds” to the initial conditions. For transient and stepped simulations that have an associated time or step range, the animation begins at the initial time or step value, progresses to the final set, and then stops and starts at zero again. It does not traverse backward as it does for static simulations. As illustrated below, you may also select a specific time period to animate that is a subset of the total time. To do so, drag the mouse through the time period in the graph. The selected time period turns blue. Press the Play button to animate only through that period. While that specific period is playing, you can right-click the mouse to receive the options to Pause, Stop, or to Zoom To Range, which expands the defined period across the entire graph. The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the help. Interface names and other components shown in the demo may differ from those in the released product. Note In a dynamic analysis, probe animation for joints is only supported if there is at least one rigid body. See Probes. Capped Isosurfaces Capped Isosurface mode displays surface bodies through the geometry that correspond to a given value within the calculated range for a selected result. To view a capped isosurface, display the Capped Isosurface toolbar from the Mechanical application. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 745 Features The value for the isosurface is set by the slider or textbox in the toolbar. The slider represents the range from min to max for the selected result. The three radio buttons control if any solid geometry remains visible on either side of the isosurface. The leftmost button displays the isosurface only, the center button displays the surface body and geometry with values below the surface body, the right button displays the surface body and values above. Dynamic Legend The dynamic legend feature helps you display the result range and contour colors associated with the visible elements. You can use the dynamic legend feature when you slice a body or hide bodies in an assembly. When you apply the dynamic legend feature to a sliced body, Workbench repositions the Min and Max annotations to the lowest and highest result values in the sliced body. For models that include multiple bodies the maximum and minimum result values can occur at the joined surfaces even if these surfaces are not visible. To update the legend and view the result range for the visible elements: • 746 Right-click the legend, and then click Adjust to Visible Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application Note The dynamic legend behavior is not applicable for Probe annotation. Adjusting the legend to visible elements updates the legend colors, values, and adds a Custom tag to the legend information. To restore the legend display for the entire body after you disable the slice or hide command: • Right-click the legend, and then click Reset All to view the result range for the entire body Note If you do not reset the legend to show result range for the entire body after disabling the slice or hide command, Workbench displays the out of range values with colors not included in the legend. Generating Reports See the Report Preview (p. 864) section. Renaming Results Based on Definition The option Rename Based on Definition is available when you right mouse click on any result (under Solution objects), or any Result Tracker (under Solution Information objects). When you choose this option, the Mechanical application automatically renames the result or Result Tracker based on the selected parts (for example, Temperature can be renamed to Temperature - Tube, or Directional Deformation can be renamed to Directional Deformation - All Bodies). Results Legend By default the results legend displays the following information: • Object Title: Name of the selected tree object. Right mouse button click on the object title to display: – Named Legends – Date and Time Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 747 Features – Max, Min on Color Bar – Logarithmic Scale – All Scientific Notation – Digits – Independent Bands – Color Scheme • Type: Type of the selected tree object. • Units: Current unit system. • Time: Current solution time for the result. • Time stamp: Current real world time. Maximum/Minimum Contour Range If the context menu is displayed from a color band instead of the title bar, the following items appear at the top of the menu, followed by a separator: • Custom Color: A pop-up color appears when you right click a color band. The same color can be used for more than one band. • Automatic Color: The default color is restored. By hovering your mouse over the contour values in the maximum/minimum contour range, you edit the highlighted information. Two items appear at the top of the context menu: • Edit: You can enter a custom value in the field at the top of the contour provided it is greater than the default value calculated by the program. • Automatic Value: The value calculated by the program. You can set the number of bands between the bottom and top of the contour using the + or – buttons. The number of bands can range from 4 to 14. Note When the distance between adjacent bands is very small (thousandth of the entire range), the contour colors may not correctly reflect the ranges in the legend. Named Legends A name can represent the following data: • Number of contours • Color scheme • Color overrides per band • Value break per break, either automatic or numeric Use the Named Legends option to create new named legends or to manage existing ones that can be edited independently. 748 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results in the Mechanical Application New Named Legends By selecting New, an input dialog box displays to specify a name. Future edits use this new name. You can create an independent variation of a named legend by choosing Unnamed or New. The option Unnamed is the default. The Unnamed option indicates that the legend can be edited independently. Managing Named Legends The Named Legends dialog box allows you to manage styles. Options included: • Import • Export • Rename • Delete Checked named legends appear in the legend context menu by default for new databases only. Date and Time Toggles line in Object Title. Max, Min on Color Bar If checked, extremes are shown . If unchecked, they appear in the title book. Logarithmic Scale Displays result values. All Scientific Notation Displays result values. Digits Contains 2 through 8. The default is 3. Independent Bands Use to set the alarm color representing the maximum/minimum contour range. The following choices are available: • None (default) • Top • Bottom • Top and Bottom Color Scheme Use to change the color spectrum. The choices available are: • Rainbow (default) • Reverse Rainbow Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 749 Features • Gray scale • Reverse Gray scale • Reset Colors Results Toolbar Refer to the Result Context Toolbar (p. 291) section under Context Toolbar (p. 287). Solution Combinations You can create solutions that are calculated from other solutions. These are derived from the addition of results coming from one or more environments, each of which can include a multiplication coefficient that you supply. Included are nonlinear results, which are a simple addition of values. The calculated values cannot be parameterized. The Design Assessment system provides a more powerful Solution Selection capability, allowing you to combine results from a greater variety of upstream analysis systems and perform additional post processing functions using external scripts. Note Choosing Update Project from the Project Schematic will not solve a Solution Combination in the Mechanical application. To Create a Solution Combination Object You can insert one or more Solution Combination objects under the Model object. Under the Solution Combination object, you can add the following results types: • Stress Tool • Fatigue Tool • Contact Tool (for the following contact results: Frictional Stress, Penetration, Pressure, and Sliding Distance) • Beam Tool • Beam Results • Stresses • Elastic Strains • Deformations Each solution object contains its own configuration spreadsheet, available through the Worksheet View. 750 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview When setting up a Solution Combination, you select the Environment Objects you wish to add together from a drop-down list of all available environments. At least one environment must be checked. Enter the multiplication coefficient you wish for each environment. The results values shown for these objects are derived from the same results objects in the referenced environments, including any defined multiplication coefficients. The basic formula for calculating the results is: (multiplication coefficient 1 X value from environment 1) + (multiplication coefficient 2 X value from environment 2) + etc. Note You can specify a coordinate system in the Details view of the Solution item for which you request a solution combination. The default is the Global Cartesian Coordinate system. • The solution item at each result set identified in the Worksheet view is calculated in the specified coordinate system and then solution combination is carried out. If you request solution combination for derived quantities such as equivalent/principal stresses and strains as well as total displacement, the following two step procedure is used: 1. Solution combination is carried out to compute component results first. 2. The requested result items are then derived from the components. Solving Overview The overall procedure for obtaining a solution in the Mechanical application is as follows: 1. Specify the solver type and other settings as applicable in the Details view of the Analysis Settings object. 2. For background solving capabilities other than My Computer, Background, use RSM Administration to configure servers and queue. This step may be done for you by a person designated as the RSM administrator. 3. For solving capabilities other than standard My Computer options, create solve process settings to utilize the queue created in step 2. The appropriate solve process settings (for example Solve Manager and Queue) for your computing environment may be provided by your RSM administrator. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 751 Features 4. Initiate the solve. You can simply click on the Solve button to use the default solve process settings or display the drop down menu to select specific solve process settings. • To solve all analyses, highlight the Project object, then choose Solve. • To solve all analyses for a model, highlight the Model object, then choose Solve. • To solve a particular analysis, highlight any of the following objects, then choose Solve: – The particular analysis object (for example, Static Structural). – The Solution object. – Child objects of the Solution object. If you initiate a background solve, and the project has not been initially saved, you will be prompted to save the project first. Note For a background solve process setting, you still see the Meshing dialog box because meshing will first be run locally and in synchronous mode before the solve is sent to the queue. Meshing locally allows the same mesh to be used in each solve if multiple Solutions are being solved simultaneously under a single Model, rather than re-meshing for each solve. For both synchronous and background solves, you can check your mesh before solving through a right mouse click on the Mesh object and selecting Preview Mesh in the context menu. A Solution Status window in the Mechanical application monitors solution progress for synchronous solutions. Conventional progress bars are displayed in this window along with a Stop Solution button and an Interrupt Solution button. You have two choices when halting the progress of the Mechanical APDL solver in the Solution Status window. If you would like the solver to halt immediately and forego writing any outstanding restart points, press the Stop Solution button. If, instead, you would like to allow the solver to complete its current iteration and record outstanding restart points, press the Interrupt Solution button (available for static structural and transient structural analyses). Neither case affects previous restart points. Note If you are familiar with Mechanical APDL functionality, clicking the Interrupt Solution button places a file named file.abt in the working directory. Any error messages are displayed in the Messages window immediately after attempting the solution. If you interrupt the solution, a confirmation message is displayed in the Messages window. When a solution is in progress in the Mechanical application, you can freely access the Engineering Data workspace and review data. The engineering data used in the solution will be in read-only mode as indicated by a lock icon. The following characteristics apply to background configurations where the RSM user interface is used to monitor solutions: 752 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview • While a background solution is in progress for a branch, that branch will be in a read-only state with the exception that result objects can be deleted during this time. Other branches can be edited freely. • You can cancel a running job and reset the state of the tree by selecting Solution in the tree and choosing Stop Solution in the context menu (right mouse button click). Note that this will immediately kill the job and not attempt to bring back any solver files (if solving on a compute server). Use Evaluate Results or Retrieve first if you wish to bring back any files from the server. • An alternative to canceling a job is to choose Interrupt Solution in the context menu. As in a synchronous solution, this will allow the solver to complete its current iteration and record outstanding restart points. • A green down arrow status symbol indicates that a solution is ready for download and/or loading into the Mechanical application. This does not indicate the success or failure of a solve. • When the green down arrow is displayed to indicate results are ready for download, choose Get Results from the context menu to perform the download, if necessary, and load results into the Mechanical application. Note When using a Local solve process setting and a solve is in progress, do not reboot or log off of the Windows client machine. If you reboot or log off, the connection to the Linux job will be lost and results will not be retrievable. If the Linux job has completed, then rebooting or logging off is safe. The mathematical model is applied and the results are evaluated. When the compute server is a remote machine, the model is applied and results are evaluated on that machine. You can rename Solution or Solution Information objects and items under these objects using a right mouse button click and choosing Rename. You then type a new name for the object (similar to renaming a file in Windows Explorer). If you are using a The Mechanical Wizard (p. 230), you must be sure that all the tasks in the wizard are complete ( ) before you try to solve. To view your solution, select View Results from the The Mechanical Wizard (p. 230). Or, click the result and the solution appears in the Geometry (p. 240) window. You can use the postprocessing features during solve when the solve process is on a remote computer or as a background process. Related Solving Topics Solve Modes and Recommended Usage Using Solve Process Settings Solution Restarts Solving Scenarios Solution Information Object Postprocessing During Solve Result Trackers Adaptive Convergence File Management in the Mechanical Application Solving Units Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 753 Features Saving your Results in the Mechanical Application Writing and Reading the Mechanical APDL Application Files Converting Boundary Conditions to Nodal DOF Constraints (Mechanical APDL Solver) Resolving Thermal Boundary Condition Conflicts Resume Capability for Explicit Dynamics Analyses Solve Modes and Recommended Usage Workbench includes capabilities for efficiently solving various kinds of analyses taking CPU usage and solving time into consideration. The following table defines the various solve “modes” available and includes references to recommended usages and associated solve process settings. Further details are discussed in the various other sections under Solving Overview (p. 751). Solve Start Mode Solve Monitor Mode Recommended Usage Solve Process Settings In Process - The solve starts and finishes on your computer in the directory where your project resides. Synchronous The solve runs and finalizes within the same Workbench session. Analyses that are not expected to be extremely CPU intensive. My Computer No[1] Out of Process The solve starts and finishes either on another computer, or on your computer but in a directory that is separate from the one where your project resides. Asynchronous The solve is not restricted to run and finalize during any particular Workbench session.[2] Analyses involving large models or a large amount of processing time and machine resources, excluding linked analyses and analyses that involve multiple convergence loops.[3] My Computer, Background Yes Synchronous The solve runs and finalizes within the same Workbench session. Analyses involving large models or a large amount of processing time and machine resources,including linked analyses and analyses that involve multiple convergence loops. My Computer, Background, then click Advanced... button and check Solve in synchronous mode (ANSYS only). Yes Remote Solve Manager (RSM) Involvement [1] - Exceptions are the Rigid dynamics and Explicit Dynamics solvers. Both solvers user RSM for the In Process mode. [2] - When solving in asynchronous mode, you are free to continue working independently of the solve job, or close the Workbench session and retrieve the solution results at a later time. You can even shut down your computer when using a Solve Manager located on another computer (See RSM Administration 754 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview and Using Solve Process Settings (p. 755)). An asynchronous solution is queued with other solutions and can run either on your local machine or on a more powerful remote machine. Background solutions are recommended for large models or simulations that require a large amount of processing time and machine resources. Sending the Solve to a remote computer can increase productivity when a highend server is available on your network. [3] - Though not recommended for a linked analysis using this solve mode combination, you can solve a linked analysis or an analysis involving multiple convergence loops provided you solve each analysis separately, that is, you must obtain the first solution, then choose Get Results from the context menu in the first analysis before obtaining the solution in the second analysis. The Out of Process and Synchronous mode combination is recommended for these types of analyses because the solve can occur from a single user action. Also, asynchronous solutions involving linked analyses that are initiated from the Project Schematic by choosing Update will automatically achieve the same effect as choosing Get Results, thus providing another method for solving linked analyses from a single user action. Using Solve Process Settings Solve process settings are individual solving configurations that you set up prior to initiating solves. Settings include specifying a synchronous or background solve, as well as solve manager machine and queue designations for background configurations. Using the Solve Process Settings dialog box, you can: • Add a local solve process • Add a remote solve process • Specify a default solve process • Modify existing solve process settings • Delete an existing solve process • Rename a solve process To access solve process settings, choose Tools> Solve Process Settings... in the Mechanical application window. The solve process in red indicates that the process is selected as the default solve process and persists across Workbench sessions. The built-in solve processes include: My Computer — Solves and finalizes the solution on the local computer in the current Workbench session. My Computer, Background — Solves on the local machine but is not restricted to finalizing in a particular Workbench session. You need more than one solver license to use this setting. However, Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 755 Features you can perform Rigid Dynamics and Explicit Dynamics analyses with one solver license by selecting the Use Shared License, if possible option on the Advanced Properties dialog box. Solve Process options Add Local Adds a new local Solve process. The solve manager for this type of solve process is My Computer and cannot be changed. Add Remote Adds a new process, where you can specify the remote computer you want to use. Set As Default Specifies the solve process as Default across workbench sessions. Rename Renames the selected solve process. Delete Deletes the selected solve process. Note Each Solve process you add must have a unique name. Solve Process Settings Computer Settings Solve Manager Specifies the name of the Solution Manager machine. The manager machine is configured with queues and compute servers. Note For local configurations, Solve Manager is automatically set to My Computer and cannot be modified. Queue Specifies the name of the queue configured using RSM Administration. If this list does not contain any queues, check that RSM is installed for the computer specified in the Solve Manager field. License Specifies the name of a valid ANSYS product license (ANSYS Professional or higher) to be used for the solution on the server. Note 756 • You must specify a valid ANSYS product license (ANSYS Professional or higher) because a separate instance of an ANSYS application is being used. • The license from your current ANSYS Workbench client session cannot be accessed from the remote ANSYS application executable. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Note • Computer Settings are not available when you select the built-in My Computer solve process. • Solve Manager and Queue fields are required for all local and remote background configurations. Advanced Properties Distribute Solution (if possible) Enables a distributed solution. Note Supported only for static, buckling, transient, modal, full harmonic, and explicit dynamic analyses. Use GPU Acceleration (if possible) Provides access to the Graphics Processing Unit (GPU) acceleration capability offered by Mechanical APDL, including support for the NVIDIA acceleration card. To enable this feature, you must select NVIDIA from the drop down menu. Max number of utilized processors Sets the number of processors to use during solution. The default is 2. Entering 0 does not send any request to the Mechanical APDL solver related to the number of processors to use. If you specify a number greater than the number of processors in the computer, the highest available number of processors is used. This setting is applicable for both shared-memory and Distributed ANSYS solutions. See this section from the Mechanical APDL help for more information: HPC License in the Parallel Processing Guide. For Explicit Dynamics analyses, this setting is used to determine the number of processors unless this has been specified in the Additional Command Line Arguments. Note Manually specify Mechanical APDL solver memory settings • Available only for Mechanical APDL and Explicit Dynamics solver. • You need an ANSYS Mechanical HPC license for each processor after the first two. • For Explicit Dynamics analyses, this setting is used to determine the number of processors unless this has been specified in the Additional Command Line Arguments. Helps you specify the amount of system memory, in MB, used for the ANSYS application workspace and database. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 757 Features Note Applicable to Mechanical APDL solver only. Additional Command Line Arguments Specifies arguments that you would normally enter into a command line input, for example, -machine option for a distributed solution. Custom Executable Name (with path) Specifies a custom ANSYS application solver executable name and path. This executable will be used for the ANSYS application solve rather than using the default. Manually specify Linux settings Enter a valid User Name and Working Folder to override the RSM compute server proxy settings. Note Use Shared License, if possible • You must have write access to this folder on all potential compute proxies in the queue. • To use the RSM settings, leave this field blank. Enables the use of a Shared License Note • This option works only for Explicit Dynamics and Rigid Dynamics analysis. For more information, see Shared Licensing • License sharing is only possible within a single Workbench session with the solver running on the same machine. A remote solve on another machine via RSM will require a license for the Workbench session and a license for the remote solve. License Queuing: Wait for Available License Instruct the MAPDL solver to wait for an available license when solving remotely via RSM. Solve in synchronous mode (Mechanical APDL solver only) Select to mimic the default My Computer behavior while leveraging the computation power of a remote machine. See this section from the Mechanical APDL help for more information: HPC Licensing in the Parallel Processing Guide. For Explicit Dynamics analyses, this setting is used to determine the number of processors unless this has been specified in the Additional Command Line Arguments. Note 758 • Applicable only for Mechanical APDL solver. • Requires an additional license. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Clear the check box to deliberately download results from a remote machine (by issuing Get Results on a right-mouse click on the Solution object). This precludes the solution of linked analyses or multiple convergence loops automatically on a single click of the Solve button. This is the default and allows the user to close the Mechanical editor or solve an unrelated analysis. OK — Commits all changes in the Solve Process Settings dialog box and closes the dialog box. You must choose OK for the Solve Process Setting configurations to be used when you initiate the solve Cancel — Closes the dialog box and ignores all changes. Note In order to run a distributed Explicit Dynamics solution on Linux, you must add the MPI_ROOT environment variable and set it to the location of the MPI software installation. It should be of the form: {ANSYS installation}/commonfiles/MPI/Platform/{version}/{platform} For example: usr/ansys_inc/v140/commonfiles/MPI/Platform/8.1/linx64 Solution Restarts Note Solution Restarts are supported in Static Structural and Transient Structural analyses only. The solution process is composed of a sequence of calculations that predict a structure’s response when applied to a specific analysis type and loading condition. Restarts provide the ability to continue an initial or existing solution which can save time during the solve phase. This feature facilitates a variety of workflows, which include: 1. Pausing or stopping a job to review results and then restarting the job. 2. Review and correction of a non-converging solution. Solution parameters in the analysis settings could be fine-tuned or adjusted allowing the solution to proceed while retaining prior solution progress. Similarly a load history can be modified to aid in the convergence. 3. Extending a solution that has already completed, for example, to allow system transients to progress further into time. 4. Submitting post processing instructions into Mechanical APDL after the model has been fully solved (see below). The following topics are covered in this section: • Restart Points (p. 760) • Generating Restart Points (p. 760) • Retaining Restart Points (p. 760) • Viewing Restart Points (p. 760) • Using Restart Points (p. 761) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 759 Features • Deleting Restart Points (p. 762) • Modifications Affecting Restart Points (p. 762) • Loads Supported for Restarts (p. 765) • Solution Information Files During Restart (p. 766) Restart Points Solution restarts are based on the concept of a restart point. Each restart point can be considered as a snapshot of the system solution state at a discrete point along the sequence of calculations. The solver stores this state of the solution in a restart file on disk. Every restart file on disk will have a corresponding restart point in the Mechanical GUI. See Viewing Restart Points (p. 760) below. A solution can only be restarted from an available restart point. It is thus important to understand how to work with these restart points. Generating Restart Points Restart points are automatically created by Mechanical depending on the analysis type. The program controlled option will create one restart point at the last successful solve point for a nonlinear analysis. However, you may directly control their frequency to alter the balance between flexibility and disk usage with the Restart Controls (p. 535) group of the Analysis Settings object. Restart points could be generated at all substeps or specific substep intervals in the analysis or at none at all. Note • You can manually interrupt a solution and preserve any restart points that may have been produced from a converged iteration by clicking the Interrupt Solution button on the Solution Status window. • A stand-alone linear analysis will not produce any restart points with the program controlled option. It has to be explicitly turned on using the manual setting. However, if the analysis is linked to a follow on modal analysis, it will generate restart points by default. Retaining Restart Points An incomplete solution (for example, a convergence failure) will always retain the restart points. However, for a complete solution, this is controlled by Retain Files After Full Solve property located in the Details view of Analysis Settings under Restart Controls. This property is set to No by default and hence will delete all restart points after the solution is completed. It can be set to YES which will retain the restart files for the current project. Alternatively, there is a global option to control the restart points after a successful solve Tools> Options> Mechanical> Analysis Settings and Solution> Restart Controls and it applies to all projects. Viewing Restart Points Once restart points are generated, they will be visible in several forms. For an overview, select the Analysis Settings object and refer to the Graph window where restart points are symbolized by triangular markers atop the timeline. The Tabular Data window lists the restart points within each load step. 760 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview A restart point is color coded to distinguish between replayable and a non-replayable. A replayable solution is one which will produce the exact solution when run from start to finish or completed incrementally using intermediate restart points. A blue triangle indicates a replayable restart point. A red triangle indicates a potentially non-replayable restart point and can only be used in manual mode. Note The Initial Restart Point does not represent a restart file on disk. It is only a place holder to facilitate selection to run the solution from the beginning even when other restart points are available. Using Restart Points You can manually choose the restart point to be used in a solution. Alternatively, you can configure Mechanical to suggest one for you. To allow Mechanical to automatically select a restart point, set Restart Type to Program Controlled. If you prefer a different point, you may specify it directly by setting Restart Type to Manual and by: • Choosing Current Restart Point in the Details view of the Analysis Settings object. • Selecting the desired marker on the Graph window and choosing Set Current Restart Point in the context menu. • Selecting the desired cell in the Tabular Data window and choosing Set Current Restart Point in the context menu. The Current Restart Point in the Restart Analysis group of the Analysis Settings object will indicate which restart point will be used the next time a solution is attempted. The current restart point in the graph/timeline window will be denoted with a double triangle in the timeline. The program controlled setting takes a conservative approach to guarantee a replayable solution and will always select the last replayable restart point. In manual mode, the software will not automatically change the current restart point and has to be selected explicitly. Picking a non-replayable restart point Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 761 Features in manual mode is only recommended for experienced users who understand the implications of the results produced. Mechanical automatically tracks how restart points are affected as you work and modify your model. So they may get flagged as non-replayable (red triangle) or be removed altogether depending on the operation. See Modifications Affecting Restart Points (p. 762) for details. Also see Restart Analysis (p. 535) under Analysis Settings (p. 499). Note An analysis should use the same units (set at the beginning of a solve) throughout the solve including all restarts. If the units are changed at any restart point, the solve is aborted and an error message is displayed. Deleting Restart Points In order to delete existing restart points, you may use the Delete All Restart Points in the context menu at the Environment and Solution folders. For more granularity, one or more restart points may also be deleted by selecting them on either the Graph or Tabular Data windows and issuing Delete Restart Points. Note The Clear Generated Data option in the context menu from either the Solution, Environment, Model or Project objects also deletes all restart points. Modifications Affecting Restart Points The following table summarizes the effects of making changes to the controls of the Analysis Settings object and the impacts on restart points. If a change is made to one of the following Controls… Then... All Restart Points are Deleted Step Controls Current Restart Point set to the Beginning of the Modified Load Step Non-replayable Restart Points may be Available2 Step End Time3 X Auto Time Stepping X X Define By X X Carry Over Time Step X X Time Integration X X Solver Controls X Rotordynamics Controls X 762 Current Restart Point is Set to Initial Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Restart Points are Unaffected Solving Overview If a change is made to one of the following Controls… Then... All Restart Points are Deleted Current Restart Point is Set to Initial Non-replayable Restart Points may be Available2 Current Restart Point set to the Beginning of the Modified Load Step Restart Points are Unaffected Restart Controls X Restart Analysis X Non Linear Controls Output Controls X 4 X Stress X Strain X Nodal Force X Contact Miscellaneous X General Miscellaneous X Calculate Results At X Max Number of Result Sets Damping Controls X X X X Analysis Data Management Save MAPDL dB X Delete Unneeded Files X Solver Units X The following table summarizes the effects of step modifications on restart points. If a change is made to one of the following Controls… Then... All Restart Points are Deleted Current Restart Point is set to the Beginning of the Modified Load Step Non-replayable Restart Points may be Available2 Activate/Deactivate X X Add Step/Insert Step X Delete Step X A solution can be restarted after modification to the load history. However, any other changes to the definition delete all of the Restart Points. Note that Displacements, Remote Displacements, and FE Displacements only support Tabular data modifications. See the Loads Supported for Restarts (p. 765) topic for a detailed list. If a change is made to one of the following Controls… Then... Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 763 Features Current Restart Point is Set to Initial1 Modify Load History Constant Current Restart Point is set to the Beginning of the Modified Load Step Non-replayable Restart Points may be Available2 X X Tabular X Function Change Load Type (Constant, Tabular, Function) X X X X X The following table summarizes the effects of adding/modifying/deleting a Commands object. When Restart Points are available, adding a new Commands object defaults to the last step so as to preserve the Restart Points. Adding a Commands object without Restart Points defaults to first step. If a change is made to one of the following Controls… Then… All Restart Points are Deleted Add/Modify/Delete Command Snippets Under Environment Current Restart Point is set to the Beginning of the Modified Load Step Non-replayable Restart Points may be Available2 X X Under Solution/Results Under Model/Trunk Objects Restart Points are Unaffected X X Modifications such as adding or changing boundary conditions (for example, scoping changes), constraints, initial conditions, or editing model level objects (Geometry, Contact Region, Joint, Mesh) invalidates and deletes existing Restart Points. The exception is Direct FE loads with a zero magnitude Restart Points are retained. If a change is made to one of the following Controls… Then… All Restart Points are Deleted Add/Delete Boundary Condition 764 Restart Points are Unaffected X Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview If a change is made to one of the following Controls… Then… All Restart Points are Deleted Add/Delete Direct Boundary Condition Restart Points are Unaffected Force (zero) X Force (non zero) X Displacement X Model Level Changes X 1 Restart Type specified as Program Controlled. 2 It can only be selected when Restart Type is specified as Manual. 3 When the Step End Time option in the Step Controls category is changed, the restart point is deleted as well as all the steps after this modified restart points are deleted and are not available, not even for manual restarts. Exception is the case when Fluid Solid Interface load exists and all the restart points are retained. 4 It is recommended that you not change Output Controls settings during a solution restart. Modifying Output Controls settings changes the availability of the respective result type in the results file. Consequently, result calculations cannot be guaranteed for the entire solution. In addition, result file values may not correspond to GUI settings in this scenario. Settings turned off during a restart generate results equal to zero and may affect post processing of results and are therefore unreliable. Note Restart is not supported for an analysis with Adaptive Convergence. So the presence of an adaptive convergence will not retain any restart points. Loads Supported for Restarts The following table outlines which loads may be modified for a solution restart. Load Type Load Specified As... Constant Tabular Function Pressure X X X Line Pressure X X X Force X X X Remote Force X X X Moment X X X Displacement X X N/A Remote Displacement X X N/A Rotational Velocity X X X Bolt Pretension X X N/A Acceleration X X X Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 765 Features Earth Gravity N/A N/A N/A Hydrostatic Pressure X N/A N/A Bearing Load X X N/A Joint Load X X X Pipe Temperature X X X Pipe Pressure X X X Thermal Condition X X X Imported Load N/A N//A N/A Nodal Force X X X Nodal Pressure X X X FE Displacement X X N/A Solution Information Files During Restart During a restart, solution information files (input file ds.dat and output file solve.out) from the previous solve are retained for reference by renaming it just before the restart solve is initiated. The naming convention is filename_loadstep_substep.ext. For example, if the previous solve occurred at loadstep = 2 and substep = 5, the file name would be ds_2_5.dat and solve_2_5.out. Files from the initial solve will be named ds_0_0.dat and solve_0_0.dat. Based on the restart point, Mechanical will ensure that obsolete and invalid solution files are cleaned up. Solving Scenarios This section describes the various configuration steps involved for the following solving scenarios: • Solve on the Local Machine within the Workbench process (synchronous) (p. 766) • Solve on My Computer in the Background (asynchronous) (p. 766) • Solve Directly from My Computer to a Remote Windows Computer (p. 766) • Solve Directly from My Computer to a Remote Linux Computer (p. 767) • Solve to a Windows Compute Server via a Solve Manager Running on Another Computer (p. 767) • Solve to a Linux Compute Server via a Solve Manager Running on Another Computer (p. 768) • Solve to LSF Cluster with Remote Solve Manager (p. 768) • Solve to Microsoft HPC Cluster with Remote Solve Manager (p. 768) Solve on the Local Machine within the Workbench process (synchronous) • Use the built-in My Computer solve process setting. Solve on My Computer in the Background (asynchronous) • Use the built-in My Computer, Background solve process setting. The option is only functional if Remote Solve Manager (RSM) was installed along with Workbench. RSM has a built-in “Local” queue and server for running jobs on the client computer. Solve Directly from My Computer to a Remote Windows Computer This step requires the following configuration steps: 766 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview 1. The Mechanical application and RSM must also be installed on both your local computer and the remote Windows Computer. 2. For the (My Computer) Solve Manager on your local machine: • Create a remote Compute Server. (This is the remote Windows machine). For details, see Adding a Compute Server in the RSM documentation. Create a Queue and add the remote Compute Server to the Queue. For details, see Creating a Queue in the RSM documentation. The job will run under the currently logged in user account on the remote computer. • 3. Create a Local solve process setting (see Using Solve Process Settings (p. 755)). After creating the solve process setting, select the local queue created in step 2. 4. Use the Solve Process Setting created in step 3 using the Solve drop down button on the toolbar. Solve Directly from My Computer to a Remote Linux Computer This step requires the following configuration steps: 1. Configure a Linux machine for native mode communications. (In native mode, RSM is installed and running locally on the remote Linux machine that serves as the remote Compute Server Proxy, so a separate protocol isn’t required for Windows-to-Linux communications.) See Configuring RSM to Use a Remote Computing Mode and Configuring Native Cross-Platform Communications for details. 2. For (My Computer) Solve Manager on your local machine: • Create a remote Compute Server. (This is the remote Linux machine). For details, see Adding a Compute Server in the RSM documentation. • Create a Queue and add the remote Linux Compute Server to the Queue. For details, see Creating a Queue in the RSM documentation. 3. Create a Local solve process setting (see Using Solve Process Settings (p. 755)). After creating the solve process setting, select the queue created in step 2. 4. Use the Solve Process Setting created in step 3 using the Solve drop down button on the toolbar. Solve to a Windows Compute Server via a Solve Manager Running on Another Computer This scenario requires the following configuration: 1. Open the RSM user interface window from the Start menu or double-click on the tray icon ( ) if it is already running. Under Tools> Options add the Solve Manager machine (that is, the remote machine that was configured with Servers and Queues). The Solve Manager will appear in the tree view. This step will allow you to monitor jobs sent to that Solve Manager. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 767 Features 2. Create a Remote solve process setting (see Using Solve Process Settings (p. 755)). You will enter the same machine name that you used in step 1. You will then be able to select the appropriate queue from the drop down list. 3. Select the Solve Process Setting created in step 2 on the Solve drop down button on the Mechanical application toolbar. Solve to a Linux Compute Server via a Solve Manager Running on Another Computer This scenario requires the following configuration: 1. Open the RSM user interface window from the Start menu or double-click on the tray icon ( ) if it is already running. Under Tools> Options add the Solve Manager machine (that is, the machine that was configured with Servers and Queues). The Solve Manager will appear in the tree view. This step will allow you to monitor jobs sent to that Solve Manager. 2. A Queue with a Server pointing to the target Linux machine must be configured in the Solve Manager (See RSM Administration). Remember, in this case the Linux machine is a proxy for a Windows-based computer. As far as RSM knows, the job is running on the Windows machine. 3. Create a Remote solve process setting (see Using Solve Process Settings (p. 755)). You will enter the same machine name that you used in step 1. You will then be able to select the appropriate queue from the drop down list. 4. Select the solve process setting created in step 3 from the Solve drop down button on the Mechanical application toolbar. Solve to LSF Cluster with Remote Solve Manager The configuration from a Mechanical application user perspective is the same as above. A Solve Process Setting is required that specifies a local or remote RSM Solve Manager and Queue where the Solve is submitted. See Integrating Windows with a Platform LSF cluster in the RSM documentation for configuration details. Solve to Microsoft HPC Cluster with Remote Solve Manager The configuration from a Mechanical application user perspective is the same as above. A Solve Process Setting is required that specifies a local or remote RSM Solve Manager and Queue where the Solve is submitted. See Integrating with Mircosoft HPC in the RSM documentation for specific configuration details. 768 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Solution Information Object You can track, monitor, or diagnose problems that arise during any solution as well as view certain finite element aspects of the engineering model, using a Solution Information object, which is inserted automatically under a Solution object of a new environment or an environment included in a database from a previous release. You can also manually insert a Solution Information object under a Connections object for solver feedback. When you select a Solution Information object in the tree, the following controls are available in the Details view under the Solution Information category: • Solution Output: [not applicable to Connections object] Determines how you want solution response results displayed. All of the options are displayed in real time as the solution progresses: – Solver Output (default): Displays the solution output file (text) from the appropriate solver (for example, the Mechanical APDL application, AUTODYN). This option is valuable to users who are accustomed to reviewing this type of output for diagnostics on the execution of their solver of choice. – Solve Script Output: (Design Assessment system only) Displays the log file from the python Solve script specified for the current Design Assessment system. – Evaluate Script Output: (Design Assessment system only) Displays the log file from the python Evaluate script specified for the current Design Assessment system. Choosing any of the following options displays a graph of that option as a function of Cumulative Iteration/Cycle (availability depends on the solver). – Force Convergence1 – Displacement Convergence1 – Rotation Convergence1 – Moment Convergence1 – Max DOF Increment – Line Search – Time – Time Increment – CSG Convergence1 (magnetic current segments) – Heat Convergence1 – Energy Conservation – shows plots of total energy, reference energy, work done, and energy error. – Momentum Summary – shows plots of X, Y and Z momentum and X, Y and Z impulse for the model. – Energy summary – shows plots of internal energy, kinetic energy, hourglass energy and contact energy. Note The frequency at which data is written can be specified as a time step frequency or a physical time frequency. By default information is displayed for every 100 time steps. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 769 Features 1 - All convergence plots include designations where any bisections, converged substeps, or converged steps occur. These designations are the red, green, and blue dotted lines shown in the example below of a Force Convergence plot. Note For ease of viewing solutions with many substeps/iterations, the Substep Converged and Load Step Converged lines are not displayed when the number of lines exceeds 1000. Also, graphs are shown as lines only, rather than lines and points, when the number of points exceeds 1000. • Newton-Raphson Residuals: [applicable only to Structural environments solved with the Mechanical APDL application] Specifies the maximum number of Newton-Raphson residual forces to return. The default is 0 (no residuals returned). You can request that the Newton-Raphson residual restoring forces be brought back for nonlinear solutions that either do not converge or that you aborted during the solution. The Newton-Raphson force is calculated at each Newton-Raphson iteration and can give you an idea where the model is not satisfying equilibrium. If you select 10 residual forces and the solution doesn't converge, those last 10 residual forces will be brought back. The following information is available in the Details view of a returned Newton-Raphson Residual Force object: – Results - Minimum and Maximum residual forces across the model – Convergence - Global convergence Criterion and convergence Value – Information - Time based information These results cannot be scoped and will automatically be deleted if another solution is run that either succeeds or creates a new set of residual forces. • Update Interval: (appears only for synchronous solutions) Specifies how often any of the result tracking items under a Solution Information object get updated while a solution is in progress. The default is 2.5 seconds. • Display Points: [not applicable to Connections object] Specifies the number of points to plot for a graphical display determined by the Solution Output setting (described above). • Display Filter During Solve: [applicable only when using Result Tracker filtering in Explicit Dynamics analyses] When set to Yes, displays filtered data from Result Trackers in the Worksheet at each refresh interval of the Result Tracker. As shown below, a legend is included in the Worksheet to help distinguish the filtered data from the non-filtered data. Typically there are two curves, non-filtered data is displayed in red, and filtered data is displayed in green. 770 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Note If an error occurs during a solve when using the ANSYS solver, the Solution Information worksheet may point you to files (for example, file.err) in temporary scratch folders whose purpose is for solving only (this is the folder where ANSYS actually ran). After the solution, these files are moved back to the project structure, so you may not find them in the scratch folders (or sub-folders). Viewing and Exporting Finite Element Connections During the solution, the Mechanical application will sometimes create additional elements or Constrain Equations (CE) for certain objects such as a remote boundary condition, spot weld, joint, MPC based contact, or weak spring. So that you might better understand how the boundary conditions are applied, the Mechanical application allows you to “view” these connections after a solution is completed. The following controls are available in the Details view under the FE Connection Visibility category: • Activate Visibility: Allows control on whether or not the Finite Element Connection data is stored during the solution. If visualization of the finite element connections will never be desired or to maximize performance on extreme models in which many constraint equations exist, this feature can be deactivated by setting the value to No before solving the model. Note that in the case of a multiple step analysis, if constraint equations are present, they will be reported from the first load step. • Display: Allows control over which finite element connections are to be viewed. The options include: – All FE Connectors (Default) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 771 Features – 772 CE Based (As illustrated below, outlined or hollow nodes indicate use for calculation purposes only.) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview – Beam Based – Weak Springs – None This control is especially useful to separate the constraint equation connections from the beam connections. The None choice is available to assist in avoiding potential performance issues from this feature. • Draw Connections Attached To: provides a drop-down list with the option All Nodes (Default) and it will also list any existing node-based Named Selections. • Line Color: Assigns colors to allow you to differentiate connections. The options include: – Connection Type (Default): Displays a color legend that presents one color for constraint equation connections and another color for beam connections. – Manual: Displays a color that you choose. – Color: Appears if Line Color is set to Manual. By clicking in this field, you can choose a color from the color palette. • Visible on Results: When set to Yes (Default), the finite element connections are displayed with any result plot (with the exception of a base mesh). When set to No, the connections are displayed only when the Solution Information object is selected. • Line Thickness: Displays the thickness of finite element connection lines in your choice of Single (default), Double, or Triple. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 773 Features • Display Type: allows you to view FE connections as Lines (Default) or as Points. If you wish to view the Points of a specified Named Selection, the nodes belonging to the Named Selection display as solid colors. Any other associated nodes not belonging to the Named Selection, display with an outline only. You can export the finite element connection information described above by right-clicking on the Solution Information object and choosing Export FE Connections from the context menu. The Display control governs what information is exported. Information for constraint equation connections is exported in terms of Mechanical APDL CE commands, while for beam and weak spring connections, a list of material numbers is exported and written as a block of Mechanical APDL ESEL commands. Tracking Background Solutions When running background solutions, you can check the status of the solution by using the Retrieve feature, which is available in a context menu when you click the right mouse button on the Solution Information object. In rare instances, the Retrieve feature could fail if the necessary retrieve files do not become available at a particular time. Simply choosing Retrieve again will likely solve the issue. Postprocessing During Solve Postprocessing during a solve allows you to use postprocessing tools while an analysis is still in progress. This feature is useful for analyses that produce partial results (that is, analyses that produce intermediate results files that are readable but incomplete) such as all Static and Transient Structural, all Static and Transient Thermal, and Explicit Dynamics analyses. This feature is available only when you solve an analysis on a remote computer or as a background process. When you run the solution as a background process, you can add new results under the Solution object or use postprocessing features such as viewing results contours, animation, min and max labels, and so on. To postprocess results during a solve: 1. Set up the Remote Solve Manager (RSM) and run a solution. Request results for a specific time by entering the time in the Display Time field within the Details view of the Solution object. 2. Right-click on the Solution object and choose Evaluate All Results. If you chose a specific time point that is not yet solved, the result of the most recent solved point will be displayed in the output fields within the Details view. Note When using this feature, it is important that you allow adequate time after the solve for the results files to be created and present before any postprocessing can be successful. Requesting a postprocessing function too prematurely could generate an error message stating that the result file could not be opened. Result Trackers In addition to the real time solution response graphs you can view from the Solution Information object, you can also view graphs of specific displacement and contact results as a function of time using 774 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Result Tracker objects. These objects are inserted as branch objects under a Solution Information object. To insert a Result Tracker object, select a Solution Information object in the tree and either choose an option under the Result Tracker drop-down menu in the Solution Information context toolbar, or perform a RMB click on the Result Tracker object, then insert a Result Tracker object. The following topics are addressed in this section: Structural Result Trackers Thermal Result Trackers Explicit Dynamics Result Trackers Result Tracker Features Structural Result Trackers Result trackers for structural analyses are presented in the main bulleted items below. The Details view settings for each are presented as sub-bulleted items. • Deformation: for displacement scoped to a vertex. – Scope → Geometry: Specifies vertex. – Definition → Type: Read-only field that displays the type of Results Tracker. → Orientation: Specifies X-Axis, Y-Axis, or Z-Axis. → Suppressed: Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Results → Minimum: Read-only indication of the minimum value of the result tracker type. → Maximum: Read-only indication of the maximum value of the result tracker type. • Contact: for contact outputs scoped to a given contact pair. – Definition → Type: Specifies the particular contact output. For each of these options, the result tracking is performed on the Contact side of the pair. If you want to perform the result tracking on the Target side, you should flip the source and target sides. If this occurs you can change the contact region to Asymmetric and flip the source and target faces in order to specify the side of interest that is to be the contact side. If Auto Asymmetric contact is active (either by the Behavior contact region setting equaling Auto Asymmetric or by the Formulation setting equaling Augmented Lagrange or MPC) and the contact side is chosen by the program to be disabled, the Results Tracker will not contain any results (as signified by a value of -2 for Number Contacting output). Contact results will be valid depending on the type of contact (for example, edge-edge) and the contact formulation. • Pressure: Maximum pressure • Penetration: Maximum penetration • Gap: Minimum gap. The values will be reported as negative numbers to signify a gap. A value of zero is reported if the contact region is in contact (and thus has a penetration). Also, if the region is in far-field contact (contact faces are outside the pinball radius), then the gap will be equal to the resulting pinball size for the region. • Frictional Stress: Maximum frictional stress Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 775 Features • Sliding Distance: Maximum sliding distance • Number Sticking: Number of elements that are sticking • Number Contacting (default): Number of elements in contact. A value of -1 means the contact pair is in far field contact (meaning the faces lie outside the contact pinball region). • Chattering: Maximum chattering level • Elastic Slip: Maximum elastic slip • Normal Stiffness: Maximum normal stiffness • Max Tangential Stiffness: Maximum tangential stiffness • Min Tangential Stiffness: Minimum tangential stiffness • Contacting Area: The total area of the elements that are in contact. • Max Damping Pressure: Maximum contact damping pressure. → Suppressed: Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Scope → Contact Region: Specifies the particular contact region in the pair. Default names are Contact Region and Contact Region 2. – Results → Minimum: Read-only indication of the minimum value of the result tracker type. → Maximum: Read-only indication of the maximum value of the result tracker type. • Kinetic energy and Stiffness Energy – Definition → Type: Read-only field that displays the type of Results Tracker. → Suppressed: Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Results → Minimum: Read-only indication of the minimum value of the result tracker type. → Maximum: Read-only indication of the maximum value of the result tracker type. Thermal Result Trackers The result tracker for thermal analyses is presented in the main bulleted item below. The Details view settings are presented as sub-bulleted items. • Temperature: scoped to a vertex. – Definition → Type: Read-only field that displays the type of Results Tracker. → Suppressed: Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Scope → Scoping Method: Specifies Geometry Selection, Global Minimum, or Global Maximum at a solution point. 776 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview → Geometry: Specifies vertex. – Results → Minimum: Read-only indication of the minimum value of the result tracker type. → Maximum: Read-only indication of the maximum value of the result tracker type. Explicit Dynamics Result Trackers The following topics are related specifically to result trackers in explicit dynamics analyses: Point Scoped Result Trackers for Explicit Dynamics Body Scoped Result Trackers for Explicit Dynamics Force Reaction Result Trackers for Explicit Dynamics Viewing and Filtering Result Tracker Graphs for Explicit Dynamics Point Scoped Result Trackers for Explicit Dynamics A point scoped result tracker is used to create a Gauge point in the ANSYS AUTODYN solver. These are either associated with a node or element center, depending on the variable selected. If the location specified in the Mechanical application interface does not correspond to a node or element center then the nearest node or element is used. Note The point scoped trackers are only available for an explicit dynamics analysis. Point scoped trackers may only be inserted prior to the analysis being solved. You can specify the location of point scoped Explicit Dynamics result trackers in three ways: • • • Selecting a vertex on the geometry. 1. Set Location Method to Geometry Selection. 2. Select a vertex, click in the Geometry field, then click Apply. Selecting a point using the Coordinate toolbar button. 1. Set Location Method to User Defined Location. 2. Choose Click to Change in the Location field. 3. Depress the Coordinate toolbar button. 4. Move the cursor across the model and notice that the coordinates display and update as you reposition the cursor. 5. Click at the desired location. A small cross hair appears at this location. You can click again at another location, which changes the cross hair location. 6. Click Apply in the Location field. The location coordinates display in the X, Y, Z Coordinate fields. You can change the location by repositioning the cursor, clicking at the new location, then clicking Click to Change and Apply, or by editing the X, Y, Z Coordinate fields in the Details view. Selecting a point by entering coordinates directly in the Details view. 1. Set Location Method to User Defined Location. 2. Type the coordinates in the X, Y, Z Coordinate fields in the Details view. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 777 Features Point scoped result trackers for explicit dynamics analyses are presented in the main bulleted items below. The Details view settings for each are presented as sub-bulleted items. Included in the Details view of all Explicit Dynamics result trackers is a low-pass filter option, not listed below. • • • • 778 Deformation (Scoping: flexible bodies only) – Location Method – Select geometry or a user defined location. – Coordinate System – Assigned to user defined location. – X, Y, Z Coordinate – Position of the user defined location. – Location – Select user defined location. – Type – Select deformation type. – Orientation – Deformation along X, Y, or Z axis. – Geometry – Select vertex. – Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Position (Scoping: flexible bodies only) – Type – Read only. – Location Method – Select geometry or a user defined location. – Coordinate System – Assigned to user defined location. – X, Y, Z Coordinate – Position of the user defined location. – Location – Select user defined location. – Orientation – Position along X, Y, or Z axis. – Geometry – Select vertex. – Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Velocity (Scoping: flexible bodies only) – Location Method – Select geometry or a user defined location. – Coordinate System – Assigned to user defined location. – X, Y, Z Coordinate – Position of the user defined location. – Location – Select user defined location. – Type – Select velocity type. – Orientation – Velocity along X, Y, or Z axis. – Geometry – Select vertex. – Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Acceleration (Scoping: flexible bodies only) – Location Method – Select geometry or a user defined location. – Coordinate System – Assigned to user defined location. – X, Y, Z Coordinate – Position of the user defined location. – Location – Select user defined location. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview • • • • – Type – Select acceleration type. – Orientation – Acceleration along X, Y, or Z axis. – Geometry – Select vertex. – Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Internal Energy (Scoping: flexible bodies only) – Type – Read only. – Location Method – Select geometry or a user defined location. – Coordinate System – Assigned to user defined location. – X, Y, Z Coordinate – Position of the user defined location. – Location – Select user defined location. – Geometry – Select vertex. – Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Stress (Scoping: flexible bodies only) – Location Method – Select geometry or a user defined location. – Coordinate System – Assigned to user defined location. – X, Y, Z Coordinate – Position of the user defined location. – Location – Select user defined location. – Type – Select stress type. – Geometry – Select vertex. – Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Strain (Scoping: flexible bodies only; not available for Euler bodies) – Location Method – Select geometry or a user defined location. – Coordinate System – Assigned to user defined location. – X, Y, Z Coordinate – Position of the user defined location. – Location – Select user defined location. – Type – Select strain type. – Geometry – Select vertex. – Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Temperature (Scoping: flexible bodies only) – Type – Read only. – Location Method – Select geometry or a user defined location. – Coordinate System – Assigned to user defined location. – X, Y, Z Coordinate – Position of the user defined location. – Location – Select user defined location. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 779 Features • • – Type – Read only. – Geometry – Select vertex. – Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Pressure (Scoping: flexible bodies only) – Type – Read only. – Location Method – Select geometry or a user defined location. – Coordinate System – Assigned to user defined location. – X, Y, Z Coordinate – Position of the user defined location. – Location – Select user defined location. – Geometry – Select vertex. – Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Density (Scoping: flexible bodies only) – Type – Read only. – Location Method – Select geometry or a user defined location. – Coordinate System – Assigned to user defined location. – X, Y, Z Coordinate – Position of the user defined location. – Location – Select user defined location. – Geometry – Select vertex. – Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Note Density is not calculated for shell and beam elements. Importing Point Scoped Result Trackers From a File Choosing Result Trackers From File from the Result Tracker drop down menu in the toolbar enables you to import point scoped result trackers from a file. The format of the file should be as in the following example: cm 1;2;3;velx;velocity;x 1.4;2.5;3.745;My Deformation;Deformation;Total 10;20;30;prin max strain;strain;principal1 10;20;30;middle strain;strain;principal2 The first line, "cm" represents the units of the values in the file. Acceptable inputs for this are: "m", "cm", "mm", "in", "ft", or "um". The subsequent lines contain the data for each tracker to be inserted. The first three numbers are the x,y,z location values. The fourth entry is the user given name - the one that will be seen in the tree. The 5th and 6th entries are type and subtype. 780 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Acceptable entries for type and subtype are: type = "velocity", "acceleration" or "deformation" with subtypes of "x","y","z" or "total" type = "position", "temperature", "pressure", "energy" or "density" (no subtype used) type = "stress" or "strain" with subtypes of "xx", "yy", "zz", "xy", "yz", "zx", "principal1", "principal2", "principal3", "equivalent" All values in each line should be separated by a semicolon. Any lines that are not properly formatted will be skipped - no tracker will be inserted for them. Body Scoped Result Trackers for Explicit Dynamics Body scoped result trackers for explicit dynamics analyses are presented in the main bulleted items below. The Details view settings for each are presented as sub-bulleted items. • Momentum (Scoping: flexible or rigid bodies) – Definition → Type – Read only. → Orientation – Select X, Y, or Z axis. → Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Scope → Geometry – Select bodies. – Results → Minimum – Read-only indication of the minimum value of the result. tracker type. → Maximum – Read-only indication of the maximum value of the result. tracker type. – Filter → Type – Specify low-pass filtering option. • Total Mass Average Velocity (Scoping: flexible or rigid bodies) – Definition → Type – Read only. → Orientation – Select X, Y, or Z axis. → Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Scope → Geometry – Select bodies. – Results → Minimum – Read-only indication of the minimum value of the result. tracker type. → Maximum – Read-only indication of the maximum value of the result. tracker type. – Filter → Type – Specify low-pass filtering option. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 781 Features • Contact Force (Scoping: flexible or rigid bodies; not available for Euler bodies) – Definition → Type – Read only. → Orientation – Select X, Y, or Z axis. → Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Scope → Geometry – Select bodies. – Results → Minimum – Read-only indication of the minimum value of the result. tracker type. → Maximum – Read-only indication of the maximum value of the result. tracker type. – Filter → Type – Specify low-pass filtering option. • External Force (Scoping: flexible or rigid bodies; not available for Euler bodies) – Definition → Type – Read only. → Orientation – Select X, Y, or Z axis. → Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Scope → Geometry – Select bodies. – Results → Minimum – Read-only indication of the minimum value of the result. tracker type. → Maximum – Read-only indication of the maximum value of the result. tracker type. – Filter → Type – Specify low-pass filtering option. • Kinetic Energy (Scoping: flexible or rigid bodies) – Definition → Type – Read only. → Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Scope → Geometry – Select bodies. – Results → Minimum – Read-only indication of the minimum value of the result. tracker type. → Maximum – Read-only indication of the maximum value of the result. tracker type. – 782 Filter Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview → Type – Specify low-pass filtering option. • Total Energy (Scoping: flexible or rigid bodies) – Definition → Type – Read only. → Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Scope → Geometry – Select bodies. – Results → Minimum – Read-only indication of the minimum value of the result. tracker type. → Maximum – Read-only indication of the maximum value of the result. tracker type. – Filter → Type – Specify low-pass filtering option. • Internal Energy (Scoping: flexible bodies only) – Definition → Type – Read only. → Location Method – Select geometry or a user defined location. → Coordinate System – Assigned to user defined location. → X, Y, Z Coordinate – Position of the user defined location. → Location – Select user defined location. → Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Scope → Geometry – Select bodies for Location Method of Geometry Selection. – Results → Minimum – Read-only indication of the minimum value of the result. tracker type. → Maximum – Read-only indication of the maximum value of the result. tracker type. – Filter → Type – Specify low-pass filtering option. • Plastic Work (Scoping: flexible bodies only) – Definition → Type – Read only. → Suppressed – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. – Scope → Geometry – Select bodies. – Results Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 783 Features → Minimum – Read-only indication of the minimum value of the result. tracker type. → Maximum – Read-only indication of the maximum value of the result. tracker type. – Filter → Type – Specify low-pass filtering option. Force Reaction Result Trackers for Explicit Dynamics Result trackers that can be scoped to boundary conditions and geometry are available for explicit dynamics analyses. The Details view settings are presented as sub-bulleted items under the tracker bullet. • Force Reaction tracker – Location Method – Select the scoping method for this tracker. Options are Boundary Condition and Geometry Selection. – Boundary Condition – When Boundary Condition is selected as the Location Method, select the defined boundary condition that is to be used for scoping. At this time, the boundary conditions that are available are: Velocity and Displacement. – Geometry – When Geometry Selection is selected as the Location Method, select the vertex, edge, face, or body where the tracker will be located. – Force Component – When Geometry Selection is selected as the Location Method, select the Force Component (Support, Euler/Lagrange Coupling, Contact, All) for which reaction force results will be shown. Euler/Lagrange Coupling specifies that the tracker show results for the forces exerted by any material in bodies assigned with an Eulerian reference frame that interact with the scoped region. These trackers can only be scoped to geometry that has a Lagrangian reference frame. See Explicit Fluid Structure Interaction (Euler-Lagrange Coupling) (p. 1268) for more information about Euler Lagrange interactions. Support specifies that the tracker show results for the forces that will be generated due to supports that are acting on the scoped area. Contact specifies that the tracker show results for the total force resulting from the contact forces acting on the scoped area. All specifies that the tracker show results for the sum of all three components. – • Orientation – Select X, Y, or Z axis, or Total, which is the resultant force of its X, Y, and Z components. The Filter option in the Details view is defined in the same manner as any other result tracker (see Viewing and Filtering Result Tracker Graphs for Explicit Dynamics (p. 785)). The reaction force will be shown varying over time in the Graph window, and a table is displayed that shows the data. The magnitude of the reaction force is calculated by summing the reaction forces on each of the nodes selected by the scoping. For example, if you have scoped the tracker by Geometry Selection to a face using the Contact Force Component, the magnitude of the reaction force is the sum of all reaction forces due to contact at the nodes on the selected face. If you scope by Boundary Condition, the magnitude will be the sum of all of the reaction forces due to Support on the nodes scoped to the selected boundary condition. 784 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Note • The Force Reaction trackers are only available for an explicit dynamics analysis. • If you right click on a Force Reaction tracker and select Rename Based on Definition, the tracker is renamed based on its type, the direction it shows results for, and the object it is scoped to. For example, if a Force Reaction tracker is selected to show results in the Y direction and is scoped to a Velocity constraint boundary condition named "Velocity Fix", by selecting Name Based on Definition it will be renamed to "Y Force Reaction at Velocity Fix". See Renaming Result Trackers (p. 787) for more information on this renaming behavior. Viewing and Filtering Result Tracker Graphs for Explicit Dynamics Explicit dynamics analyses typically involve a large number of time history samples, sometimes in the order of hundreds of thousands, and the results tend to include high frequency noise that can obscure slow rate phenomena. A low-pass filtering option is available that allows you to separate slow-rate trends from high frequency noise in signals. This feature can be controlled from the Details view of a Result Tracker object. The filtered results are displayed by default in the Timeline window after the solve. By setting Display Filter During Solve to Yes in the Details view of the Solution Information object, the filtered results can also be displayed in the Worksheet at each refresh interval of the Result Tracker. To configure the low-pass filter for the sampled data: • Under Filter, set the following controls: – Type: Set to one of the following: → None: (Default) No filtering is applied to the data. → Butterworth: Applies a four-channel low-pass Butterworth filter to the data. Two channels are passed twice, once in the forward direction and once in the reverse direction, to prevent phase shifts. – Cut Frequency (displayed if Type is set to Butterworth): Set to the desired cut frequency in Hz or MHz depending on the current unit system. The default is 0, which implies no filtering. Notes A time history data is composed of a limited number of frequency signals that bound the range of meaningful cut frequencies to use for filtering. If the cut frequency is too low, most signals will be lost. On the other hand, if the cut frequency is too high, the signal may remain unaltered. In determining a good cut frequency, sampling frequency plays a role. The sampling frequency can be obtained by dividing the number of samples by the sampling duration. The cut frequency should not exceed a quarter of this value. For example, if 15,000 samples occur in 0.015 seconds, the sampling frequency will be 15,000/(0.015 s) = 1,000,000 Hz = 1 MHz. Consequently, the cut frequency should not exceed 0.25 MHz. The process of filtering pads the original signal with extrapolated data. This may produce unexpected shapes in the filtered signal near the margins. The data away from the margins should reflect, however, the proper trends and slow rate phenomena. The signal is not filtered at all if it has less than 11 samples. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 785 Features Under Filter, if Type is set to Butterworth, there are also read only indications for the Minimum and Maximum values of the filtered data. Result Tracker Features The following topics describe features related to all types of result trackers: Result Tracker Plot Features Renaming Result Trackers Exporting Result Trackers Result Tracker Plot Features Any of the graphs created by either the Result Tracker or nonlinear convergence items have the following features: • Multiple Result Tracker objects may be selected at the same time to create a combined chart assuming they share the same X and Y output types (such as pressure for Y and time for X). An example is shown here: • The graph can be zoomed by using the ALT key + left mouse button. Moving down and to the right zooms in, and moving up and to the left zooms out. • A plot can be saved by using the Image Capture toolbar button. • If a new Result Tracker is added to an otherwise up to date solution, a new solution will not be invoked automatically. In order for the new result to be solved, you must Clear at the Solution level and then resolve (which will force a complete resolve and thus fill the result tracker). 786 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Caution Because nodes may be rotated in solutions obtained with the Mechanical APDL application, deformation Result Trackers may not record the expected component of the deformation. Should this occur, a warning message alerting you to this will appear after the solve in the Details view of the Solution object, in the Solver Messages field. This situation can occur when Result Trackers are adjacent to supported faces, lines, or vertices. One possible approach to avoid this situation is to add 3 deformation Result Trackers, one for each of the x, y, and z directions. This will ensure that the tracker is showing all deformation of that vertex of the model. Renaming Result Trackers The Result Tracker has an option for renaming the object based on the result and the scoping. You choose the option in the context menu (RMB click). This option is useful in having the program create meaningful names of the result trackers. An example would be Result Tracker 5 being renamed to Pressure on Contact Region 2. Exporting Result Trackers Result Tracker objects can be exported to an Excel file by selecting Export in the context menu using a right-mouse button click on the Result Tracker object. This option appears in the menu after the solution is obtained. Note You must right-mouse click on the selected object in the tree to use this Export feature. On Windows platforms, if you have the Microsoft Office 2002 (or later) installed, you may see an Export to Excel option if you right-mouse click in the Worksheet window. This is not the Mechanical application Export feature but rather an option generated by Microsoft Internet Explorer. Adaptive Convergence You can control the relative accuracy of a solution in two ways. You can use the meshing tools to refine the mesh before solving, or you can use convergence tools as part of the solution process to refine solution results on a particular area of the model. This section discusses the latter. Through its convergence capabilities, the application can fully automate the solution process, internally controlling the level of accuracy for selected results. You can seek approximate results or adapted/converged results. This section explains how to interpret accuracy controls. Converged Results Control You can control convergence to a predefined level of error for selected results. In the calculation of stresses, displacements, mode shapes, temperatures, and heat fluxes, the application employs an adaptive solver engine to identify and refine the model in areas that benefit from adaptive refinement. The criteria for convergence is a prescribed percent change in results. The default is 20%. You can change this default using the Convergence setting in the Options dialog box. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 787 Features Adaptivity (Refinement of meshes based on solutions) You can continue to refine the mesh based on a specific solution result. When you pick a result (Equivalent Stress, Deformation, Total Flux Density, etc.), indicate that you want to converge on this solution. You pick a value and the solution is refined such that the solution value does not change by more than that value. To add convergence, click the result you added to your solution; for example, Equivalent Stress , Total Deformation, or Total Flux Density. If you want to converge on deformation, right-click on Total Deformation and select Insert> Convergence. In the Details View (p. 274), you can specify convergence on either the Minimum or Maximum value. Additionally, you can specify the Allowable Change between convergence iterations. Note • Convergence objects inserted under an environment that is referenced by an Initial Condition object or a Thermal Condition load object, will invalidate either of these objects, and not allow a solution to progress. • Results cannot be converged when you have a Mesh Connection object or a Pinch control with Pinch Behavior set to Post. • To use Convergence, you must set Calculate Stress to Yes under Output Controls in the Analysis Settings details panel. However, you can perform Modal and Buckling Analysis without specifying this option. • You cannot use Convergence if you have an upstream or a downstream analysis link. • Convergence is not available when you import loads into the analysis. • Convergence is not supported for a model with Layered Sections. For an adaptive solution, a solution is first performed on the base mesh, and then the elements are queried for their solution information (such as deflection, X-stress, Y-stress, etc.). If the element's results have a high Zienkiewicz-Zhu, or ZZ error (see the Mechanical APDL Theory Reference for more information on adaptivity theory), the element is placed in the queue to be refined. The application then continues to refine the mesh and perform additional solutions. Adaptivity will be more robust if your initial mesh is with tetrahedrons. Adaptive refinement starting from a hex-dominant mesh will automatically result in a re-meshing of the structure with tetrahedrons. The face mesh given to the tet mesher is the initial quad mesh split into triangles. That face mesh is then filled with tetrahedrons so it is recommended that you insert an all tetrahedron mesh method before you start an adaptive solution. You can control the aggressiveness of the adaptive refinement by adjusting the Refinement Depth setting under Adaptive Mesh Refinement in the Details view of a Solution object. The default value is 2 for structural analyses, and 0 for magnetostatic analyses. The range is from 0 to 3. By default, when adaptive convergence occurs, the program will refine to a depth of 2 elements to help ensure smooth transitions and avoid excessive element distortion for repeated refinement. However, you can adjust this refinement depth to a value of 0 or 1 if for a particular problem, the deep refinement is not required and problem size is a major concern. In general, for mechanical analyses, the default value of 2 is highly recommended. However, you can lower the value if too much refinement is occurring and is overwhelming the solution in terms of size of solution time. If you use a value less than 2, be aware of the following: • 788 Verify that false convergence is not occurring because of too little refinement. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview • More refinements may be required to achieve the desired tolerance, which may increase the total solution time. The following pictures show the effects of various settings of Refinement Depth on plots of Total Deformation. Base Mesh: No Refinement Refinement Depth = 1 Refinement Depth = 0 Refinement Depth = 2 For magnetostatic analyses, there are additional settings that allow you to change the percentage of the element selected for adaptive refinement during solution. These settings use an Energy Based percentage and an Error Based percentage. The internal selection process first uses the Energy Based percentage to select the number of elements in the full model that have the highest values of magnetic energy. From this number, it uses the Error Based percentage to select the number of elements with the highest error in the particular body. Magnetic Error results are also available to display on the geometry for verification. These adaptive refinement settings for magnetostatic analyses are in the Refinement Controls group, located in the Details view of the Solution object, provided you have a Convergence object inserted under any magnetostatic result. An Element Selection setting in this group has the following options: • Program Controlled (default): The percentage of elements selected for adaptive refinement equals the default values of 10% for the Energy Based percentage and 20% for the Error Based percentage. • Manual: The percentage of elements selected for adaptive refinement equals the values you enter in the Energy Based and Error Based fields that appear only when you choose Manual. Adaptive Convergence in Multiple Result Sets You can apply adaptive convergence on multiple result sets that may include different loadings or time points. To do so, create a result for each loading or time point and insert a Convergence object under each result. The following example shows Total Deformation results at two time points where a Convergence object was inserted under each result. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 789 Features ANSYS Workbench Product Adaptive Solutions Nearly every ANSYS Workbench product result can be calculated to a user-specified accuracy. The specified accuracy is achieved by means of adaptive and iterative analysis, whereby h-adaptive methodology is employed. The h-adaptive method begins with an initial finite element model that is refined over various iterations by replacing coarse elements with finer elements in selected regions of the model. This is effectively a selective remeshing procedure. The criterion for which elements are selected for adaptive refinement depends on geometry and on what ANSYS Workbench product results quantities are requested. The result quantity φ, the expected accuracy E (expressed as a percentage), and the region R on the geometry that is being subjected to adaptive analysis may be selected. The user-specified accuracy is achieved when convergence is satisfied as follows: 790 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview where i denotes the iteration number. It should be clear that results are compared from iteration i to iteration i+1. Iteration in this context includes a full analysis in which h-adaptive meshing and solving are performed. The ANSYS Workbench product uses two different criteria for its adaptive procedures. The first criterion merely identifies the largest elements (LE), which are deleted and replaced with a finer finite element representation. The second employs a Zienkiewicz-Zhu (ZZ) norm for stress in structural analysis and heat flux in thermal analysis. Table 5 ANSYS Workbench Product Adaptivity Methods Result Adaptive Criterion Stresses and strains ZZ norm Structural margins and factors of safety ZZ norm Fatigue damage and life ZZ norm Heat flows ZZ norm Temperatures ZZ norm Deformations ZZ norm Mode frequencies LE As mentioned above, geometry plays a role in the ANSYS Workbench product adaptive method. In general, accurate results and solutions can be devised for the entire assembly, a part or a collection of parts, or a surface or a collection of surfaces. The user makes the decision as to which region of the geometry applies. If accurate results on a certain surface are desired, the ANSYS Workbench product ignores the aforementioned criterion and simply refines all elements on the surfaces that comprise the defined region. The reasoning here is that the user restricts the region where accurate results are desired. In addition, there is nothing limiting the user from having multiple accuracy specification. In other words, specified accuracy in a selected region and results with specified accuracy over the entire model can be achieved. General Notes Adaptive convergence is not supported for orthotropic materials. Adaptive convergence is not supported for solid shell elements (the SOLSH190 series elements). Adaptive convergence is not valid for linked environments where the result of one analysis is used as input to another analysis. See the Define Initial Conditions (p. 12) section for details. Low levels of accuracy are acceptable for demonstrations, training, and test runs. Allow for a significant level of uncertainty in interpreting answers. Very low accuracy is never recommended for use in the final validation of any critical design. Moderate levels of accuracy are acceptable for many noncritical design applications. Moderate levels of accuracy should not be used in a final validation of any critical part. High levels of accuracy are appropriate for solutions contributing to critical design decisions. When convergence is not sought, studies of problems with known answers yield the following behaviors and approximated errors: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 791 Features At maximum accuracy, less than 20% error for peak stresses and strains, and minimum margins and factors of safety. At maximum accuracy, between 5% and 10% error for average (nominal) stresses and elastic strains, and average heat flows. At maximum accuracy, between 1% and 5% error for average stress-related displacements and average calculated temperatures. At maximum accuracy, 5% or less error for mode frequencies for a wide range of parts. When seeking highly accurate, Converged Results, more computer time and resources will be required than Manual control, except in some cases where the manual preference approaches highest accuracy. Given the flexible nature of the solver engine, it is impossible to explicitly quantify the effect of a particular accuracy selection on the calculation of results for an arbitrary problem. Accuracy is related only to the representation of geometry. Increasing the accuracy preference will not make the material definition or environmental conditions more accurate. However, specified converged results are nearly as accurate as the percentage criteria. Critical components should always be analyzed by an experienced engineer or analyst prior to final acceptance. For magnetostatic analyses, Directional Force results allow seeking convergence based on Force Summation or Torque as opposed to other results converging on Maximum or Minimum values. Adaptive convergence is not valid if a Periodic Region or Cyclic Region symmetry object exists in the model. Adaptive convergence is not valid if an imported load object exists in the environment. File Management in the Mechanical Application During the solution, several files are created. Some of these can be deleted after the solution but some need to be retained for postprocessing or for feeding other subsequent analyses. Since you can perform several different analyses on a single model or even have several models in the same Mechanical application project, you must manage the solution files in a consistent and predictable manner. Consistent Directory Structure for Mechanical Application Analyses ANSYS Workbench's file management system keeps multiple databases under a single project. See Project File Management for a description of the file management system. Note The Analysis Settings Details view has an Analysis Data Management grouping that shows the solution directory location for each analysis. Solution Files Default behavior: By default an analysis in the Mechanical application saves only the minimal files required for postprocessing. Typically these include results files (file.rst, file.rth, file.rmg, file.psd, file.mcom), input file (ds.dat), output file (solve.out), and some other files that 792 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview have valuable information about the solution ( file.BCS, file.nlh, file.gst). Of these only the results file is generally of significant size. For Windows users, the solution files folder can be displayed using the Open Solver Files Directory feature. Future Analysis: If the results of this analysis are to be used as a load or an initial condition in a subsequent analysis then additional files may need to be saved. Declaring your intent to use this in the future will automatically save the required files and reuse them in the subsequent analysis. Refer to Define Initial Conditions (p. 12) for details of these analyses. Delete Unneeded Files: The solution process creates other files that are typically not needed for postprocessing or are not used in subsequent analyses. By default, the Mechanical application deletes these files at the end of solution. However, if for any reason, you want to keep all the files you could choose to do so. You can use the Output Controls on the analysis settings page to limit only desired types of results be written to the rst file. (For example, if strains are not needed, you can turn them off which would create a smaller result file). In addition, for advanced Mechanical APDL application users, Command objects can be used to further limit output via the OUTRES command. An external result file is needed to post results. The following behavior will occur: • If you save a simulation, any simulation files (result and other required files) will be saved to the new location. • If you use the Duplicate Without Results option (Environment and Model objects only), all subordinate objects are reproduced with the exception of the data for all result objects. This is based on the intention that loading changes are performed and the solution process is repeated. • If you attempt to resolve a previously solved and saved database, the corresponding saved result files are backed up automatically in case the current solve is not saved. • The /post1 XML transfer of result files used in previous releases is no longer used so any existing solution Command objects which were modifying the Mechanical APDL application results to be brought back into the Mechanical application no longer function. Solving Units There are eight possible unit systems for a Mechanical application solution. The following tables show the unit systems for the various quantities. For a given Mechanical application run, one of the eight systems is selected and all quantities are converted into that system. This guarantees that all quantities, inputs and outputs to the Mechanical APDL application, can be interpreted correctly in terms of the units in the system. User units shown anywhere in the GUI may differ from those shown below although they will convert properly when they are sent to the solver. All magnetostatic analyses solve in the mks system regardless of the system selected. Acceleration Energy Density by Mass Magnetic Flux Density PSD Velocity Thermal Capacitance Angle Film Coefficient Mass Relative Permeability Thermal Conductance Angular Acceleration Force Material Impedance Relative Permittivity Thermal Expansion Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 793 Features Angular Velocity Force Intensity Moment Rotational Damping Temperature Area Force Per Angular Unit Moment of Inertia of Area Rotational Stiffness Temperature Difference Capacitance Fracture Energy Moment of Inertia of Mass RS Acceleration Time Charge Frequency Normalized Value RS Displacement Translational Damping Charge Density Gasket Stiffness Permeability RS Strain Velocity Conductivity Heat Flux Permittivity RS Stress Voltage Current Heat Generation Poisson's Ratio RS Velocity Volume Current Density Heat Rate Power Seebeck Coefficient Decay Constant Impulse Pressure Section Modulus Density Impulse Per Angular Unit PSD Acceleration Shear Elastic Strain Displacement Inductance PSD Acceleration (G) Shock Velocity Electric Conductance Per Unit Area Inverse Angle PSD Displacement Specific Heat Electric Conductivity Inverse Length PSD Force Specific Weight Electric Field Inverse Stress PSD Moment Stiffness Electric Flux Density Length PSD Pressure Strain Electric Resistivity Magnetic Field Intensity PSD Strain Stress Energy Magnetic Flux PSD Stress Strength Table 6 Acceleration and RS Acceleration Unit System Measured in . . . o meters/second2 [m/s2] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A centimeters/second2 [cm/s2] (cgs) mm, kg, N, oC, s, mV, mA millimeters/second2 [mm/s2] (nmm) mm, t, N, oC, s, mV, mA millimeters/second2 [mm/s2] (nmmton) mm, dat, N, oC, s, mV, mA millimeters/second2 [mm/s2] (nmmdat) 794 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . o µm, kg, µN, C, s, V, mA micrometers/second2 [µm/s2] (µmks) ft, lbm, lbf, oF, s, V, A feet/second2 [ft/s2] (Bft) in, lbm, lbf, oF, s, V, A inches/second2 [in/s2] (Bin) millimeters/millisecond2 [mm/ms2] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] meters/second2 [m/s2] m, kg, s [ LS-DYNA solver] millimeters/second2 [mm/s2] mm, t, s [ LS-DYNA solver] inches/second2 [in/s2] in,lbf, s [ LS-DYNA solver] Table 7 Angle Unit System Measured in . . . o m, kg, N, C, s, V, A radians [rad] (mks) cm, g, dyne, oC, s, V, A radians [rad] (cgs) mm, kg, N, oC, s, mV, mA radians [rad] (nmm) mm, t, N, oC, s, mV, mA radians [rad] (nmmton) mm, dat, N, oC, s, mV, mA radians [rad] (nmmdat) µm, kg, µN, oC, s, V, mA radians [rad] (µmks) ft, lbm, lbf, oF, s, V, A radians [rad] (Bft) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 795 Features Unit System Measured in . . . o in, lbm, lbf, F, s, V, A radians [rad] (Bin) Table 8 Angular Acceleration Unit System Measured in . . . o radians/second2 [rad/s2] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A radians/second2 [rad/s2] (cgs) mm, kg, N, oC, s, mV, mA radians/second2 [rad/s2] (nmm) mm, t, N, oC, s, mV, mA radians/second2 [rad/s2] (nmmton) mm, dat, N, oC, s, mV, mA radians/second2 [rad/s2] (nmmdat) µm, kg, µN, oC, s, V, mA radians/second2 [rad/s2] (µmks) ft, lbm, lbf, oF, s, V, A radians/second2 [rad/s2] (Bft) in, lbm, lbf, oF, s, V, A radians/second2 [rad/s2] (Bin) Table 9 Angular Velocity Unit System Measured in . . . o m, kg, N, C, s, V, A radians/second [rad/s] (mks) cm, g, dyne, oC, s, V, A radians/second [rad/s] (cgs) mm, kg, N, oC, s, mV, mA radians/second [rad/s] (nmm) mm, t, N, oC, s, mV, mA radians/second [rad/s] (nmmton) mm, dat, N, oC, s, mV, mA 796 radians/second [rad/s] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (nmmdat) µm, kg, µN, oC, s, V, mA radians/second [rad/s] (µmks) ft, lbm, lbf, oF, s, V, A radians/second [rad/s] (Bft) in, lbm, lbf, oF, s, V, A radians/second [rad/s] (Bin) mm, mg, ms radians/millisecond [rad/ms] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s radians/second [rad/s] [ LS-DYNA solver] mm, t, s radians/second [rad/s] [ LS-DYNA solver] in,lbf, s radians/second [rad/s] [ LS-DYNA solver] Table 10 Area Unit System Measured in . . . o meters2 [m2] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A centimeters2 [cm2] (cgs) mm, kg, N, oC, s, mV, mA millimeters2 [mm2] (nmm) mm, t, N, oC, s, mV, mA millimeters2 [mm2] (nmmton) mm, dat, N, oC, s, mV, mA millimeters2 [mm2] (nmmdat) µm, kg, µN, oC, s, V, mA micrometers2 [µm2] (µmks) ft, lbm, lbf, oF, s, V, A feet2 [ft2] (Bft) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 797 Features Unit System Measured in . . . o inches2 [in2] in, lbm, lbf, F, s, V, A (Bin) millimeters2 [mm2] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] meters2 [m2] m, kg, s [ LS-DYNA solver] millimeters2 [mm2] mm, t, s [ LS-DYNA solver] inches2 [in2] in,lbf, s [ LS-DYNA solver] Table 11 Capacitance Unit System Measured in . . . m, kg, N, oC, s, V, A Farads [F] (mks) cm, g, dyne, oC, s, V, A Farads [F] (cgs) mm, kg, N, oC, s, mV, mA microFarads [µF] (nmm) mm, t, N, oC, s, mV, mA microFarads [µF] (nmmton) mm, dat, N, oC, s, mV, mA microFarads [µF] (nmmdat) µm, kg, µN, oC, s, V, mA picoFarads [pF] (µmks) ft, lbm, lbf, oF, s, V, A Farads [F] (Bft) in, lbm, lbf, oF, s, V, A Farads [F] (Bin) Table 12 Charge Unit System o m, kg, N, C, s, V, A 798 Measured in . . . Coulombs [C] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (mks) cm, g, dyne, oC, s, V, A Coulombs [C] (cgs) mm, kg, N, oC, s, mV, mA milliCoulombs [mC] (nmm) mm, t, N, oC, s, mV, mA milliCoulombs [mC] (nmmton) mm, dat, N, oC, s, mV, mA milliCoulombs [mC] (nmmdat) µm, kg, µN, oC, s, V, mA picoCoulombs [pC] (µmks) ft, lbm, lbf, oF, s, V, A Coulombs [C] (Bft) in, lbm, lbf, oF, s, V, A Coulombs [C] (Bin) Table 13 Charge Density Unit System Measured in . . . o Coulombs/meter2 [C/m2] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A Coulombs/centimeter2 [C/cm2] (cgs) mm, kg, N, oC, s, mV, mA milliCoulombs/millimeter2 [mC/mm2] (nmm) mm, t, N, oC, s, mV, mA milliCoulombs/millimeter2 [mC/mm2] (nmmton) mm, dat, N, oC, s, mV, mA milliCoulombs/millimeter2 [mC/mm2] (nmmdat) µm, kg, µN, oC, s, V, mA picoCoulombs/micrometer2 [pC/µm2] (µmks) ft, lbm, lbf, oF, s, V, A Coulombs/foot2 [C/ft2] (Bft) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 799 Features Unit System Measured in . . . o Coulombs/inch2 [C/in2] in, lbm, lbf, F, s, V, A (Bin) Table 14 Conductivity Unit System Measured in . . .1 m, kg, N, oC, s, V, A Watts/meter.degree Celsius [W/m.oC] (mks) cm, g, dyne, oC, s, V, A dynes/second.degree Celsius [dyne/s.oC] (cgs) mm, kg, N, oC, s, mV, mA (nmm) mm, t, N, oC, s, mV, mA (nmmton) mm, dat, N, oC, s, mV, mA (nmmdat) µm, kg, µN, oC, s, V, mA (µmks) ft, lbm, lbf, oF, s, V, A ton.millimeters/second3.degree Celsius [t.mm/s3.oC] ton.millimeters/second3.degree Celsius [t.mm/s3.oC] ton.millimeters/second3.degree Celsius [t.mm/s3.oC] picoWatts/micrometers.degree Celsius [pW/µm.oC] (Slug) feet/second3.degree Fahrenheit [(lbm/32.2)ft/s3.oF] (Bft) in, lbm, lbf, oF, s, V, A (slinch) inches/second3.degree Fahrenheit [(lbm/386.4)in/s3.oF] (Bin) Table 15 Current Unit System Measured in . . . o m, kg, N, C, s, V, A Amperes [A] (mks) cm, g, dyne, oC, s, V, A Amperes [A] (cgs) mm, kg, N, oC, s, mV, mA milliAmperes [mA] (nmm) mm, t, N, oC, s, mV, mA milliAmperes [mA] (nmmton) mm, dat, N, oC, s, mV, mA 800 milliAmperes [mA] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (nmmdat) µm, kg, µN, oC, s, V, mA picoAmperes [pA] (µmks) ft, lbm, lbf, oF, s, V, A Amperes [A] (Bft) in, lbm, lbf, oF, s, V, A Amperes [A] (Bin) Table 16 Current Density Unit System Measured in . . . o Amperes/meter2 [A/m2] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A Amperes/centimeter2 [A/cm2] (cgs) mm, kg, N, oC, s, mV, mA milliAmperes/millimeter2 [mA/mm2] (nmm) mm, t, N, oC, s, mV, mA milliAmperes/millimeter2 [mA/mm2] (nmmton) mm, dat, N, oC, s, mV, mA milliAmperes/millimeter2 [mA/mm2] (nmmdat) µm, kg, µN, oC, s, V, mA picoAmperes/micrometer2 [pA/µm2] (µmks) ft, lbm, lbf, oF, s, V, A Amperes/foot2 [A/ft2] (Bft) in, lbm, lbf, oF, s, V, A Amperes/inch2 [A/in2] (Bin) Table 17 Decay Constant Unit System Measured in . . . o m, kg, N, C, s, V, A 1/seconds [1/s] (mks) cm, g, dyne, oC, s, V, A 1/seconds [1/s] (cgs) mm, kg, N, oC, s, mV, mA 1/seconds [1/s] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 801 Features Unit System Measured in . . . (nmm) mm, t, N, oC, s, mV, mA 1/seconds [1/s] (nmmton) mm, dat, N, oC, s, mV, mA 1/seconds [1/s] (nmmdat) µm, kg, µN, oC, s, V, mA 1/seconds [1/s] (µmks) ft, lbm, lbf, oF, s, V, A 1/seconds [1/s] (Bft) in, lbm, lbf, oF, s, V, A 1/seconds [1/s] (Bin) Table 18 Density Unit System Measured in . . . o kilograms/meter3 [kg/m3] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A grams/cm3 [g/cm3] (cgs) mm, kg, N, oC, s, mV, mA tons/millimeter3 [t/mm3] (nmm) mm, t, N, oC, s, mV, mA tons/millimeter3 [t/mm3] (nmmton) mm, dat, N, oC, s, mV, mA tons/millimeter3 [t/mm3] (nmmdat) µm, kg, µN, oC, s, V, mA kilograms/micrometer3 [kg/µm3] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)1/foot3 [(lbm/32.2)1/ft3] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)1/inch3 [(lbm/386.4)1/in3] (Bin) grams/cm3 [g/cm3] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] 802 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . m, kg, s kilograms/meter3 [kg/m3] [ LS-DYNA solver] tons/millimeter3 [t/mm3] mm, t, s [ LS-DYNA solver] (Slinch)1/inch3 [(lbm/386.4)1/in3] in,lbf, s [ LS-DYNA solver] Table 19 Displacement and RS Displacement Unit System Measured in . . . o m, kg, N, C, s, V, A meters [m] (mks) cm, g, dyne, oC, s, V, A centimeters [cm] (cgs) mm, kg, N, oC, s, mV, mA millimeters [mm] (nmm) mm, t, N, oC, s, mV, mA millimeters [mm] (nmmton) mm, dat, N, oC, s, mV, mA millimeters [mm] (nmmdat) µm, kg, µN, oC, s, V, mA micrometers [µm] (µmks) ft, lbm, lbf, oF, s, V, A feet [ft] (Bft) in, lbm, lbf, oF, s, V, A inches [in] (Bin) mm, mg, ms millimeters [mm] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s meters [m] [ LS-DYNA solver] mm, t, s millimeters [mm] [ LS-DYNA solver] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 803 Features Unit System Measured in . . . in,lbf, s inches [in] [ LS-DYNA solver] Table 20 Electric Conductance Per Unit Area Unit System Measured in . . . o m, kg, N, C, s, V, A S/m^2 (mks) cm, g, dyne, oC, s, V, A S/cm^2 (cgs) mm, kg, N, oC, s, mV, mA S/mm^2 (nmm) mm, t, N, oC, s, mV, mA S/mm^2 (nmmton) mm, dat, N, oC, s, mV, mA S/mm^2 (nmmdat) µm, kg, µN, oC, s, V, mA pS/um^2 (µmks) ft, lbm, lbf, oF, s, V, A S/ft^2 (Bft) in, lbm, lbf, oF, s, V, A S/in^2 (Bin) Table 21 Electric Conductivity Unit System Measured in . . . o m, kg, N, C, s, V, A Siemens/meter [S/m] (mks) cm, g, dyne, oC, s, V, A Siemens/centimeter [S/cm] (cgs) mm, kg, N, oC, s, mV, mA Siemens/millimeter [S/mm] (nmm) mm, t, N, oC, s, mV, mA Siemens/millimeter [S/mm] (nmmton) mm, dat, N, oC, s, mV, mA 804 Siemens/millimeter [S/mm] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (nmmdat) µm, kg, µN, oC, s, V, mA picoSiemens/micrometer [pS/µm] (µmks) ft, lbm, lbf, oF, s, V, A Siemens/foot [S/ft] (Bft) in, lbm, lbf, oF, s, V, A Siemens/inch [S/in] (Bin) Table 22 Electric Field Unit System Measured in . . . o m, kg, N, C, s, V, A Volts/meter [V/m] (mks) cm, g, dyne, oC, s, V, A Volts/centimeter [V/cm] (cgs) mm, kg, N, oC, s, mV, mA milliVolts/millimeter [mV/mm] (nmm) mm, t, N, oC, s, mV, mA milliVolts/millimeter [mV/mm] (nmmton) mm, dat, N, oC, s, mV, mA milliVolts/millimeter [mV/mm] (nmmdat) µm, kg, µN, oC, s, V, mA Volts/micrometer [V/µm] (µmks) ft, lbm, lbf, oF, s, V, A Volts/foot [V/ft] (Bft) in, lbm, lbf, oF, s, V, A Volts/inch [V/in] (Bin) Table 23 Electric Flux Density Unit System Measured in . . . o Coulombs/meter2 [C/m2] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A Coulombs/centimeter2 [C/cm2] (cgs) mm, kg, N, oC, s, mV, mA milliCoulombs/millimeter2 [mC/mm2] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 805 Features Unit System Measured in . . . (nmm) mm, t, N, oC, s, mV, mA milliCoulombs/millimeter2 [mC/mm2] (nmmton) mm, dat, N, oC, s, mV, mA milliCoulombs/millimeter2 [mC/mm2] (nmmdat) µm, kg, µN, oC, s, V, mA picoCoulombs/micrometer2 [pC/µm2] (µmks) ft, lbm, lbf, oF, s, V, A Coulombs/foot2 [C/ft2] (Bft) in, lbm, lbf, oF, s, V, A Coulombs/inch2 [C/in2] (Bin) Table 24 Electric Resistivity Unit System Measured in . . . o Ohm.meters [Ohm.m] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A Ohm.centimeters [Ohm.cm] (cgs) mm, kg, N, oC, s, mV, mA Ohm.millimeters [Ohm.mm] (nmm) mm, t, N, oC, s, mV, mA Ohm.millimeters [Ohm.mm] (nmmton) mm, dat, N, oC, s, mV, mA Ohm.millimeters [Ohm.mm] (nmmdat) µm, kg, µN, oC, s, V, mA teraOhm.micrometers [Tohm.µm] (µmks) ft, lbm, lbf, oF, s, V, A Ohm.Cir-mils/foot [Ohm.Cir-mil/ft] (Bft) in, lbm, lbf, oF, s, V, A Ohm.Cir-mils/inch [Ohm.Cir-mil/in] (Bin) Table 25 Energy Unit System o m, kg, N, C, s, V, A 806 Measured in . . . Joules [J] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (mks) cm, g, dyne, oC, s, V, A Ergs [erg] (cgs) mm, kg, N, oC, s, mV, mA milliJoules [mJ] (nmm) mm, t, N, oC, s, mV, mA milliJoules [mJ] (nmmton) mm, dat, N, oC, s, mV, mA milliJoules [mJ] (nmmdat) µm, kg, µN, oC, s, V, mA picoJoules [pJ] (µmks) ft, lbm, lbf, oF, s, V, A (slug) feet2/second2 [(lbm/32.2)ft2/s2] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)inches2/second2 [(lbm/386.4)in2/s2] (Bin) mm, mg, ms microJoules [µJ] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Joules [J] [ LS-DYNA solver] mm, t, s milliJoules [mJ] [ LS-DYNA solver] (Slinch)inches2/second2 [(lbm/386.4)in2/s2] in,lbf, s [ LS-DYNA solver] Table 26 Energy Density by Mass Unit System Measured in . . . o m, kg, N, C, s, V, A Joules/kilograms [J/kg] (mks) cm, g, dyne, oC, s, V, A dynes.centimeters/grams [dyne cm /g] (cgs) mm, kg, N, oC, s, mV, mA milliJoules/tons [mJ/t] (nmm) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 807 Features Unit System Measured in . . . o mm, t, N, C, s, mV, mA milliJoules/tons [mJ/t] (nmmton) mm, dat, N, oC, s, mV, mA milliJoules/tons [mJ/t] (nmmdat) µm, kg, µN, oC, s, V, mA picoJoules/kilograms [pJ/kg] (µmks) ft, lbm, lbf, oF, s, V, A feet² /seconds² [ft²/s²] (Bft) in, lbm, lbf, oF, s, V, A inches²/seconds² [in²/sec ²] (Bin) mm, mg, ms Joules/kilograms [J/kg] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Joules/kilograms [J/kg] [ LS-DYNA solver] mm, t, s milliJoules/tons [mJ/t] [ LS-DYNA solver] in,lbf, s inches²/seconds² [in²/sec ²] [ LS-DYNA solver] Table 27 Film Coefficient Unit System Measured in . . .1 m, kg, N, oC, s, V, A Watts/meter2.degree Celsius [W/m2.oC] (mks) cm, g, dyne, oC, s, V, A (cgs) mm, kg, N, oC, s, mV, mA dynes/second.centimeter.degree Celsius [dyne/s.cm.oC] tons/second3.degree Celsius [t/s3.oC] (nmm) mm, t, N, oC, s, mV, mA tons/second3.degree Celsius [t/s3.oC] (nmmton) mm, dat, N, oC, s, mV, mA tons/second3.degree Celsius [t/s3.oC] (nmmdat) µm, kg, µN, oC, s, V, mA 808 picoWatts/micrometer2.degree Celsius [pW/µm2.oC] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Measured in . . .1 Unit System (µmks) ft, lbm, lbf, oF, s, V, A (Slug)1/second3.degree Fahrenheit [(lbm/32.2)1/s3.oF] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)1/second3.degree Fahrenheit [(lbm/386.4)1/s3.oF] (Bin) Table 28 Force Unit System Measured in . . . o m, kg, N, C, s, V, A Newtons [N] (mks) cm, g, dyne, oC, s, V, A dynes [dyne] (cgs) mm, kg, N, oC, s, mV, mA ton.millimeters/second2 [t.mm/s2] (nmm) mm, t, N, oC, s, mV, mA ton.millimeters/second2 [t.mm/s2] (nmmton) mm, dat, N, oC, s, mV, mA ton.millimeters/second2 [t.mm/s2] (nmmdat) µm, kg, µN, oC, s, V, mA microNewtons [µN] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)feet/second2 [(lbm/32.2)ft/s2] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)inches/second2 [(lbm/386.4)in/s2] (Bin) mm, mg, ms milliNewtons [mN] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Newtons [N] [ LS-DYNA solver] mm, t, s Newtons [N] [ LS-DYNA solver] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 809 Features Unit System Measured in . . . in,lbf, s pound force (lbf ) [ LS-DYNA solver] Table 29 Force Intensity Unit System Measured in . . . o m, kg, N, C, s, V, A Newtons/meter [N/m] (mks) cm, g, dyne, oC, s, V, A dynes/centimeter [dyne/cm] (cgs) mm, kg, N, oC, s, mV, mA tons/second2 [t/s2] (nmm) mm, t, N, oC, s, mV, mA tons/second2 [t/s2] (nmmton) mm, dat, N, oC, s, mV, mA tons/second2 [t/s2] (nmmdat) µm, kg, µN, oC, s, V, mA microNewtons/micrometer [µN/µm] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)1/second2 [(lbm/32.2)1/s2] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)1/second2 [(lbm/386.4)1/s2] (Bin) mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Newtons/meter [N/m] or milliNewtons/millimeter [mN/mm] Newtons/meter [N/m] [ LS-DYNA solver] mm, t, s Newtons/millimeter [N/mm] [ LS-DYNA solver] in,lbf, s pound force/inch (lbf/in) [ LS-DYNA solver] Table 30 Force Per Angular Unit Unit System o m, kg, N, C, s, V, A 810 Measured in . . . Newtons/radian [N/rad] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (mks) cm, g, dyne, oC, s, V, A dynes/radian [dyne/rad] (cgs) mm, kg, N, oC, s, mV, mA Newtons/radian [N/rad] (nmm) mm, t, N, oC, s, mV, mA Newtons/radian [N/rad] (nmmton) mm, dat, N, oC, s, mV, mA Newtons/radian [N/rad] (nmmdat) µm, kg, µN, oC, s, V, mA microNewtons/radian [µN/rad] (µmks) ft, lbm, lbf, oF, s, V, A pounds mass/radian [lbf/rad] (Bft) in, lbm, lbf, oF, s, V, A pounds mass/radian [lbf/rad] (Bin) Table 31 Fracture Energy Unit System Measured in . . . o m, kg, N, C, s, V, A Joules/meters² [J /m²] (mks) cm, g, dyne, oC, s, V, A dynes/centimeters [dyne/cm] (cgs) mm, kg, N, oC, s, mV, mA milliJoules/millimeters² [mJ/mm²] (nmm) mm, t, N, oC, s, mV, mA milliJoules/millimeters² [mJ/mm²] (nmmton) mm, dat, N, oC, s, mV, mA milliJoules/millimeters² [mJ/mm²] (nmmdat) µm, kg, µN, oC, s, V, mA picoJoules /micrometers² [pJ/µm²] (µmks) ft, lbm, lbf, oF, s, V, A slug/seconds² [slug/s²] (Bft) in, lbm, lbf, oF, s, V, A slinch/seconds² [slinch/s²] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 811 Features Unit System Measured in . . . (Bin) microJoules/millimeter2 [µJ/mm2] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Joules/meters² [J /m²] [ LS-DYNA solver] mm, t, s milliJoules/millimeters² [mJ/mm²] [ LS-DYNA solver] in,lbf, s slinch/seconds² [slinch/s²] [ LS-DYNA solver] Table 32 Frequency Unit System Measured in . . . o m, kg, N, C, s, V, A Hertz[Hz] (mks) cm, g, dyne, oC, s, V, A Hertz[Hz] (cgs) mm, kg, N, oC, s, mV, mA Hertz[Hz] (nmm) mm, t, N, oC, s, mV, mA Hertz[Hz] (nmmton) mm, dat, N, oC, s, mV, mA Hertz[Hz] (nmmdat) µm, kg, µN, oC, s, V, mA Hertz[Hz] (µmks) ft, lbm, lbf, oF, s, V, A Hertz[Hz] (Bft) in, lbm, lbf, oF, s, V, A Hertz[Hz] (Bin) Table 33 Gasket Stiffness Unit System o m, kg, N, C, s, V, A Measured in . . . Pascals/meter [Pa/m] (mks) 812 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . o cm, g, dyne, C, s, V, A dynes/centimeter3 (cgs) mm, kg, N, oC, s, mV, mA tons/second2.millimeter2 [t/s2.mm2] (nmm) mm, t, N, oC, s, mV, mA tons/second2.millimeter2 [t/s2.mm2] (nmmton) mm, dat, N, oC, s, mV, mA tons/second2.millimeter2 [t/s2.mm2] (nmmdat) µm, kg, µN, oC, s, V, mA megaPascals/micrometer [MPa/µm] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)/second2.foot2 [(lbm/32.2)/s2.ft2] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)/second2.inch2 [(lbm/386.4)/s2.in2] (Bin) Table 34 Heat Flux Unit System Measured in . . . o Watts/meter2 [W/m2] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A dynes/second.centimeter [dyne/s.cm] (cgs) mm, kg, N, oC, s, mV, mA tons/second3 [t/s3] (nmm) mm, t, N, oC, s, mV, mA tons/second3 [t/s3] (nmmton) mm, dat, N, oC, s, mV, mA tons/second3 [t/s3] (nmmdat) µm, kg, µN, oC, s, V, mA picoWatts/micrometer2 [pW/µm2] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)1/second3 [(lbm/32.2)1/s3] (Bft) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 813 Features Unit System Measured in . . . o (Slinch)1/second3 [(lbm/386.4)1/s3] in, lbm, lbf, F, s, V, A (Bin) Table 35 Heat Generation Unit System Measured in . . . o Watts/meter3 [W/m3] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A dynes/second.centimeter2 [dyne/s.cm2] (cgs) mm, kg, N, oC, s, mV, mA tons/second3.millimeter [t/s3.mm] (nmm) mm, t, N, oC, s, mV, mA tons/second3.millimeter [t/s3.mm] (nmmton) mm, dat, N, oC, s, mV, mA tons/second3.millimeter [t/s3.mm] (nmmdat) µm, kg, µN, oC, s, V, mA picoWatts/micrometer3 [pW/µm3] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)1/second3.foot [(lbm/32.2)1/s3.ft] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)1/second3.inch [(lbm/386.4)1/s3.in] (Bin) Table 36 Heat Rate Unit System Measured in . . . o m, kg, N, C, s, V, A Watts [W] (mks) cm, g, dyne, oC, s, V, A dyne.centimeters/second [dyne.cm/s] (cgs) mm, kg, N, oC, s, mV, mA ton.millimeters2/second3 [t.mm2/s3] (nmm) mm, t, N, oC, s, mV, mA ton.millimeters2/second3 [t.mm2/s3] (nmmton) mm, dat, N, oC, s, mV, mA 814 ton.millimeters2/second3 [t.mm2/s3] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (nmmdat) µm, kg, µN, oC, s, V, mA picoWatts [pW] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)feet2/second3 [(lbm/32.2)ft2/s3] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)inches2/second3 [(lbm/386.4)in2/s3] (Bin) Table 37 Impulse Unit System Measured in . . . o Newton . second [N . s] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A Dyne . second [dyne . s] (cgs) mm, kg, N, oC, s, mV, mA Newton . second [N . s] (nmm) mm, t, N, oC, s, mV, mA Newton . second [N . s] (nmmton) mm, dat, N, oC, s, mV, mA Newton . second [N . s] (nmmdat) µm, kg, µN, oC, s, V, mA microNewton . second [µN . s] (µmks) ft, lbm, lbf, oF, s, V, A pounds mass . second [lbf . s] (Bft) in, lbm, lbf, oF, s, V, A pounds mass . second [lbf . s] (Bin) microNewton . second [µN . s] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Newton . second [N . s] [ LS-DYNA solver] mm, t, s Newton . second [N . s] [ LS-DYNA solver] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 815 Features Unit System Measured in . . . in,lbf, s pound force. second (lbf. second) [ LS-DYNA solver] Table 38 Impulse Per Angular Unit Unit System Measured in . . . o Newton . second/rad [N . s/rad] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A Dyne . second/radian [dyne . s/rad] (cgs) mm, kg, N, oC, s, mV, mA Newton . second/rad [N . s/rad] (nmm) mm, t, N, oC, s, mV, mA Newton . second/rad [N . s/rad] (nmmton) mm, dat, N, oC, s, mV, mA Newton . second/rad [N . s/rad] (nmmdat) µm, kg, µN, oC, s, V, mA microNewton . second/radian [µN . s/rad] (µmks) ft, lbm, lbf, oF, s, V, A pounds mass . second/radian [lbf . s/rad] (Bft) in, lbm, lbf, oF, s, V, A pounds mass . second/radian [lbf . s/rad] (Bin) Table 39 Inductance Unit System Measured in . . . o m, kg, N, C, s, V, A Henries [H] (mks) cm, g, dyne, oC, s, V, A Henries [H] (cgs) mm, kg, N, oC, s, mV, mA milliHenries [mH] (nmm) mm, t, N, oC, s, mV, mA milliHenries [mH] (nmmton) mm, dat, N, oC, s, mV, mA 816 milliHenries [mH] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (nmmdat) µm, kg, µN, oC, s, V, mA teraHenries [TH] (µmks) ft, lbm, lbf, oF, s, V, A Henries [H] (Bft) in, lbm, lbf, oF, s, V, A Henries [H] (Bin) Table 40 Inverse Angle Unit System Measured in . . . o m, kg, N, C, s, V, A 1/radians [1/rad] (mks) cm, g, dyne, oC, s, V, A 1/radians [1/rad] (cgs) mm, kg, N, oC, s, mV, mA 1/radians [1/rad] (nmm) mm, t, N, oC, s, mV, mA 1/radians [1/rad] (nmmton) mm, dat, N, oC, s, mV, mA 1/radians [1/rad] (nmmdat) µm, kg, µN, oC, s, V, mA 1/radians [1/rad] (µmks) ft, lbm, lbf, oF, s, V, A 1/radians [1/rad] (Bft) in, lbm, lbf, oF, s, V, A 1/radians [1/rad] (Bin) Note The units presented above are applicable when the Units menu is set to Radians. The applicable units are 1/degree [1/o] when the Units menu is set to Degrees. Table 41 Inverse Length Unit System o m, kg, N, C, s, V, A Measured in . . . 1/meter [1/m] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 817 Features Unit System Measured in . . . (mks) cm, g, dyne, oC, s, V, A 1/centimeter [1/cm] (cgs) mm, kg, N, oC, s, mV, mA 1/millimeter [1/mm] (nmm) mm, t, N, oC, s, mV, mA 1/millimeter [1/mm] (nmmton) mm, dat, N, oC, s, mV, mA 1/millimeter [1/mm] (nmmdat) µm, kg, µN, oC, s, V, mA 1/micrometer [1/µm] (µmks) ft, lbm, lbf, oF, s, V, A 1/foot [1/ft] (Bft) in, lbm, lbf, oF, s, V, A 1/inch [1/in] (Bin) Table 42 Inverse Stress Unit System Measured in . . . o m, kg, N, C, s, V, A 1/Pascal [1/Pa] (mks) cm, g, dyne, oC, s, V, A centimeters2/dyne [cm2/dyne] (cgs) mm, kg, N, oC, s, mV, mA second2.millimeters/ton [s2.mm/t] (nmm) mm, t, N, oC, s, mV, mA second2.millimeters/ton [s2.mm/t] (nmmton) mm, dat, N, oC, s, mV, mA second2.millimeters/ton [s2.mm/t] (nmmdat) µm, kg, µN, oC, s, V, mA 1/megaPascal [1/MPa] (µmks) ft, lbm, lbf, oF, s, V, A second2.feet/(Slug) [s2.ft/(lbm/32.2)] (Bft) 818 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . o second2.inch/(Slinch) [s2.in/(lbm/386.4)] in, lbm, lbf, F, s, V, A (Bin) Table 43 Length Unit System Measured in . . . o m, kg, N, C, s, V, A meters [m] (mks) cm, g, dyne, oC, s, V, A centimeters [cm] (cgs) mm, kg, N, oC, s, mV, mA millimeters [mm] (nmm) mm, t, N, oC, s, mV, mA millimeters [mm] (nmmton) mm, dat, N, oC, s, mV, mA millimeters [mm] (nmmdat) µm, kg, µN, oC, s, V, mA micrometers [µm] (µmks) ft, lbm, lbf, oF, s, V, A feet [ft] (Bft) in, lbm, lbf, oF, s, V, A inches [in] (Bin) mm, mg, ms millimeters [mm] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s meters [m] [ LS-DYNA solver] mm, t, s millimeters [mm] [ LS-DYNA solver] in,lbf, s inches [in] [ LS-DYNA solver] Table 44 Magnetic Field Intensity Unit System o m, kg, N, C, s, V, A Measured in . . . Amperes/meter [A/m] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 819 Features Unit System Measured in . . . (mks) cm, g, dyne, oC, s, V, A Oersteds [Oe] (cgs) mm, kg, N, oC, s, mV, mA milliAmperes/millimeter [mA/mm] (nmm) mm, t, N, oC, s, mV, mA milliAmperes/millimeter [mA/mm] (nmmton) mm, dat, N, oC, s, mV, mA milliAmperes/millimeter [mA/mm] (nmmdat) µm, kg, µN, oC, s, V, mA picoAmperes/micrometer [pA/µm] (µmks) ft, lbm, lbf, oF, s, V, A Amperes/foot [A/ft] (Bft) in, lbm, lbf, oF, s, V, A Amperes/inch [A/in] (Bin) Table 45 Magnetic Flux Unit System Measured in . . . o m, kg, N, C, s, V, A Webers [Wb] (mks) cm, g, dyne, oC, s, V, A Maxwells [Mx] (cgs) mm, kg, N, oC, s, mV, mA milliWebers [mWb] (nmm) mm, t, N, oC, s, mV, mA milliWebers [mWb] (nmmton) mm, dat, N, oC, s, mV, mA milliWebers [mWb] (nmmdat) µm, kg, µN, oC, s, V, mA Webers [Wb] (µmks) ft, lbm, lbf, oF, s, V, A Lines (Bft) 820 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . o in, lbm, lbf, F, s, V, A Lines (Bin) Table 46 Magnetic Flux Density Unit System Measured in . . . o m, kg, N, C, s, V, A Teslas [T] (mks) cm, g, dyne, oC, s, V, A Gauss [G] (cgs) mm, kg, N, oC, s, mV, mA milliTeslas [mT] (nmm) mm, t, N, oC, s, mV, mA milliTeslas [mT] (nmmton) mm, dat, N, oC, s, mV, mA milliTeslas [mT] (nmmdat) µm, kg, µN, oC, s, V, mA teraTeslas [TT] (µmks) ft, lbm, lbf, oF, s, V, A Lines/ft2 (Bft) in, lbm, lbf, oF, s, V, A Lines/in2 (Bin) Table 47 Mass Unit System Measured in . . . o m, kg, N, C, s, V, A kilograms [kg] (mks) cm, g, dyne, oC, s, V, A grams [g] (cgs) mm, kg, N, oC, s, mV, mA tons [t] (nmm) mm, t, N, oC, s, mV, mA tons [t] (nmmton) mm, dat, N, oC, s, mV, mA tons [t] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 821 Features Unit System Measured in . . . (nmmdat) µm, kg, µN, oC, s, V, mA kilograms [kg] (µmks) ft, lbm, lbf, oF, s, V, A (Slug) [(lbm/32.2)] (Bft) in, lbm, lbf, oF, s, V, A (Slinch) [(lbm/386.4)] (Bin) mm, mg, ms milligrams [mg] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s kilograms [kg] [ LS-DYNA solver] mm, t, s tons [t] [ LS-DYNA solver] in,lbf, s Slinch [ LS-DYNA solver] Table 48 Material Impedance Unit System Measured in . . . mm, mg, ms milligrams/millimeter2/second [mg/mm2/s] [ANSYS (AUTODYN) and LS-DYNA solvers] kilograms/meter2/second [kg/m2/s] m, kg, s [ LS-DYNA solver] tons/millimeter2/second [t/mm2/s] mm, t, s [ LS-DYNA solver] Slinch/inch2/second [Slinch/in2/s] in,lbf, s [ LS-DYNA solver] Table 49 Moment Unit System Measured in . . . o Newton.meters [N.m] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A 822 dyne.centimeters [dyne.cm] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (cgs) mm, kg, N, oC, s, mV, mA ton.millimeters2/second2 [t.mm2/s2] (nmm) mm, t, N, oC, s, mV, mA ton.millimeters2/second2 [t.mm2/s2] (nmmton) mm, dat, N, oC, s, mV, mA ton.millimeters2/second2 [t.mm2/s2] (nmmdat) µm, kg, µN, oC, s, V, mA microNewton.micrometers [µN.µm] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)feet2/second2 [(lbm/32.2)ft2/s2] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)inches2/second2 [(lbm/386.4)in2/s2] (Bin) microNewton.meters [µN.m] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] Newton.meters [N.m] m, kg, s [ LS-DYNA solver] Newton.millimeters [N.mm] mm, t, s [ LS-DYNA solver] pound force.inch [lbf.in] in,lbf, s [ LS-DYNA solver] Table 50 Moment of Inertia of Area Unit System Measured in . . . o meters4 [m4] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A centimeters4 [cm4] (cgs) mm, kg, N, oC, s, mV, mA millimeters4 [mm4] (nmm) mm, t, N, oC, s, mV, mA millimeters4 [mm4] (nmmton) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 823 Features Unit System Measured in . . . o mm, dat, N, C, s, mV, mA millimeters4 [mm4] (nmmdat) µm, kg, µN, oC, s, V, mA micrometers4 [µm4] (µmks) ft, lbm, lbf, oF, s, V, A feet4 [ft4] (Bft) in, lbm, lbf, oF, s, V, A inches4 [in4] (Bin) millimeters4 [mm4] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] meters4 [m4] m, kg, s [ LS-DYNA solver] millimeters4 [mm4] mm, t, s [ LS-DYNA solver] inches4 [in4] in,lbf, s [ LS-DYNA solver] Table 51 Moment of Inertia of Mass Unit System Measured in . . . o kilogram.meter2 [kg.m2] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A gram.centimeter2 [g.cm2] (cgs) mm, kg, N, oC, s, mV, mA kilogram .millimeter2 [kg.mm2] (nmm) mm, t, N, oC, s, mV, mA kilogram .millimeter2 [kg.mm2] (nmmton) mm, dat, N, oC, s, mV, mA kilogram .millimeter2 [kg.mm2] (nmmdat) µm, kg, µN, oC, s, V, mA kilogram.micrometer2 [kg.µm2] (µmks) ft, lbm, lbf, oF, s, V, A 824 (Slug)feet2 [(lbm/32.2)ft2] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (Bft) in, lbm, lbf, oF, s, V, A (Slinch)inch2 [(lbm/386.4)in2] (Bin) milligram .millimeter2 [mg.mm2] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] kilogram.meter2 [kg.m2] m, kg, s [ LS-DYNA solver] ton.millimeter2 [t.mm2] mm, t, s [ LS-DYNA solver] (Slinch)inch2 [(Slinch)in2] in,lbf, s [ LS-DYNA solver] Table 52 Normalized Value Unit System Measured in . . . o m, kg, N, C, s, V, A unitless (mks) cm, g, dyne, oC, s, V, A unitless (cgs) mm, kg, N, oC, s, mV, mA unitless (nmm) mm, t, N, oC, s, mV, mA unitless (nmmton) mm, dat, N, oC, s, mV, mA unitless (nmmdat) µm, kg, µN, oC, s, V, mA unitless (µmks) ft, lbm, lbf, oF, s, V, A unitless (Bft) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 825 Features Unit System Measured in . . . o in, lbm, lbf, F, s, V, A unitless (Bin) Table 53 Permeability Unit System Measured in . . . o m, kg, N, C, s, V, A Henries/meter [H/m] (mks) cm, g, dyne, oC, s, V, A Henries/centimeter [H/cm] (cgs) mm, kg, N, oC, s, mV, mA milliHenries/millimeter [mH/mm] (nmm) mm, t, N, oC, s, mV, mA milliHenries/millimeter [mH/mm] (nmmton) mm, dat, N, oC, s, mV, mA milliHenries/millimeter [mH/mm] (nmmdat) µm, kg, µN, oC, s, V, mA teraHenries/micrometer [TH/µm] (µmks) ft, lbm, lbf, oF, s, V, A Henries/foot [H/ft] (Bft) in, lbm, lbf, oF, s, V, A Henries/inch [H/in] (Bin) Table 54 Permittivity Unit System Measured in . . . o m, kg, N, C, s, V, A Farads/meter [F/m] (mks) cm, g, dyne, oC, s, V, A Farads/centimeter [F/cm] (cgs) mm, kg, N, oC, s, mV, mA microFarads/millimeter [µF/mm] (nmm) mm, t, N, oC, s, mV, mA microFarads/millimeter [µF/mm] (nmmton) mm, dat, N, oC, s, mV, mA 826 microFarads/millimeter [µF/mm] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (nmmdat) µm, kg, µN, oC, s, V, mA picoFarads/micrometer [pF/µm] (µmks) ft, lbm, lbf, oF, s, V, A Farads/foot [F/ft] (Bft) in, lbm, lbf, oF, s, V, A Farads/inch [F/in] (Bin) Table 55 Poisson's Ratio Unit System Measured in . . . o m, kg, N, C, s, V, A unitless (mks) cm, g, dyne, oC, s, V, A unitless (cgs) mm, kg, N, oC, s, mV, mA unitless (nmm) mm, t, N, oC, s, mV, mA unitless (nmmton) mm, dat, N, oC, s, mV, mA unitless (nmmdat) µm, kg, µN, oC, s, V, mA unitless (µmks) ft, lbm, lbf, oF, s, V, A unitless (Bft) in, lbm, lbf, oF, s, V, A unitless (Bin) mm, mg, ms unitless [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s unitless [ LS-DYNA solver] mm, t, s unitless [ LS-DYNA solver] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 827 Features Unit System Measured in . . . in,lbf, s unitless [ LS-DYNA solver] Table 56 Power Unit System Measured in . . . o m, kg, N, C, s, V, A Watts [W] (mks) cm, g, dyne, oC, s, V, A dyne.centimeters/second [dyne.cm/s] (cgs) mm, kg, N, oC, s, mV, mA ton.millimeters2/second3 [t.mm2/s3] (nmm) mm, t, N, oC, s, mV, mA ton.millimeters2/second3 [t.mm2/s3] (nmmton) mm, dat, N, oC, s, mV, mA ton.millimeters2/second3 [t.mm2/s3] (nmmdat) µm, kg, µN, oC, s, V, mA picoWatts [pW] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)feet2/second3 [(lbm/32.2)ft2/s3] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)inches2/second3 [(lbm/386.4)in2/s3] (Bin) mm, mg, ms milliWatts [mW] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Watts [W] [ LS-DYNA solver] Newton.millimeters/second [N.mm/s] mm, t, s [ LS-DYNA solver] pound force.inch/second [lbf.in/s] in,lbf, s [ LS-DYNA solver] Table 57 Pressure Unit System o m, kg, N, C, s, V, A 828 Measured in . . . Pascals [Pa] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (mks) cm, g, dyne, oC, s, V, A dynes/centimeter2 [dyne/cm2] (cgs) mm, kg, N, oC, s, mV, mA ton/second2.millimeters [t/s2.mm] (nmm) mm, t, N, oC, s, mV, mA ton/second2.millimeters [t/s2.mm] (nmmton) mm, dat, N, oC, s, mV, mA ton/second2.millimeters [t/s2.mm] (nmmdat) µm, kg, µN, oC, s, V, mA megaPascals [MPa] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)1/second2.foot [(lbm/32.2)1/s2.ft] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)1/second2.inch [(lbm/386.4)1/s2.in] (Bin) mm, mg, ms kiloPascals [kPa] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Pascals [Pa] [ LS-DYNA solver] mm, t, s megaPascals [MPa] [ LS-DYNA solver] pounds/inch2 [lb/in2] in,lbf, s [ LS-DYNA solver] Table 58 PSD Acceleration Unit System Measured in . . . o (meters/second2)2/Hertz [(m/s2)2/Hz] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A (centimeters/second2)2/Hertz [(cm/s2)2/Hz] (cgs) mm, kg, N, oC, s, mV, mA (millimeters/second2)2/Hertz [(mm/s2)2/Hz] (nmm) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 829 Features Unit System Measured in . . . o mm, t, N, C, s, mV, mA (millimeters/second2)2/Hertz [(mm/s2)2/Hz] (nmmton) mm, dat, N, oC, s, mV, mA (millimeters/second2)2/Hertz [(mm/s2)2/Hz] (nmmdat) µm, kg, µN, oC, s, V, mA (µmks) ft, lbm, lbf, oF, s, V, A (micrometers/second2)2/Megahertz [(µm/s2)2/MHz] (feet/second2)2/Hertz [(ft/s2)2/Hz] (Bft) in, lbm, lbf, oF, s, V, A (inch/second2)2/Hertz [(in/s2)2/Hz] (Bin) Table 59 PSD Acceleration (G) Unit System Measured in . . . o G2/Hertz [G2/Hz] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A G2/Hertz [G2/Hz] (cgs) mm, kg, N, oC, s, mV, mA G2/Hertz [G2/Hz] (nmm) mm, t, N, oC, s, mV, mA G2/Hertz [G2/Hz] (nmmton) mm, dat, N, oC, s, mV, mA G2/Hertz [G2/Hz] (nmmdat) µm, kg, µN, oC, s, V, mA G2/Hertz [G2/Hz] (µmks) ft, lbm, lbf, oF, s, V, A G2/Hertz [G2/Hz] (Bft) in, lbm, lbf, oF, s, V, A G2/Hertz [G2/Hz] (Bin) Table 60 PSD Displacement Unit System o m, kg, N, C, s, V, A 830 Measured in . . . meters2/Hertz [m2/Hz] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (mks) cm, g, dyne, oC, s, V, A centimeters2/Hertz [cm2/Hz] (cgs) mm, kg, N, oC, s, mV, mA millimeters2/Hertz [mm2/Hz] (nmm) mm, t, N, oC, s, mV, mA millimeters2/Hertz [mm2/Hz] (nmmton) mm, dat, N, oC, s, mV, mA millimeters2/Hertz [mm2/Hz] (nmmdat) µm, kg, µN, oC, s, V, mA micrometers2/Megahertz [µm2/MHz] (µmks) ft, lbm, lbf, oF, s, V, A feet2/Hertz [ft2/Hz] (Bft) in, lbm, lbf, oF, s, V, A inches2/Hertz [in2/Hz] (Bin) Table 61 PSD Force Unit System Measured in . . . o Newtons2/Hertz [N2/Hz] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A Dynes2/Hertz [dyne2/Hz] (cgs) mm, kg, N, oC, s, mV, mA (nmm) mm, t, N, oC, s, mV, mA (nmmton) mm, dat, N, oC, s, mV, mA (nmmdat) µm, kg, µN, oC, s, V, mA ((kiloGrams.milliMeters)/Second2)2/Hertz [((kg.mm)/s2)2/Hz] ((Tons.milliMeters)/Second2)2/Hertz [((t.mm)/s2)2s/Hz] ((Tons.milliMeters)/Second2)2/Hertz [((t.mm)/s2)2s/Hz] microNewtons2/Hertz [µN2/Hz] (µmks) ft, lbm, lbf, oF, s, V, A (Bft) ((Pounds.Mass/32.2).Feet)/Second2))2/Hertz [((lb.m/32.2).ft/s2))2/Hz] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 831 Features Unit System Measured in . . . o ((Pounds.Mass/32.2).Inches)/Second2))2/Hertz [((lb.m/32.2).in/s2))2/Hz] in, lbm, lbf, F, s, V, A (Bin) Table 62 PSD Moment Unit System Measured in . . . o (Newtons.Meters)2/Hertz [(N.m)2/Hz] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A (Dynes.centiMeters)2/Hertz [(dyne.cm)2/Hz] (cgs) mm, kg, N, oC, s, mV, mA (nmm) mm, t, N, oC, s, mV, mA (nmmton) mm, dat, N, oC, s, mV, mA (nmmdat) µm, kg, µN, oC, s, V, mA (µmks) ft, lbm, lbf, oF, s, V, A ((kiloGrams.milliMeters2)/Second2)2/Hertz [((kg.mm2)/s2)2/Hz] ((Tons.milliMeters2)/Second2)2/Hertz [((t.mm2)/s2)2/Hz] ((Tons.milliMeters2)/Second2)2/Hertz [((t.mm2)/s2)2/Hz] (microNewtons.microMeters)2/Hertz [(µN.µm)2/Hz] ((Pounds.Mass/32.2).Feet2)/Second2) 2/Hertz [((lb.m/32.2).ft2)/s2)2/Hz] (Bft) in, lbm, lbf, oF, s, V, A ((Pounds.Mass/386.4).Inches2)/Second2)2/Hertz [((lb.m/386.4).in2)/s2)2/Hz] (Bin) Table 63 PSD Pressure Unit System Measured in . . . o Pascals2/Hertz [Pa2/Hz] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A (Dynes/centiMeter2)2/Hertz [(Dyne/cm2)2/Hz] (cgs) mm, kg, N, oC, s, mV, mA (nmm) mm, t, N, oC, s, mV, mA (nmmton) mm, dat, N, oC, s, mV, mA 832 (kiloGrams/(milliMeter.Second2))2/Hertz [(kg/(mm.s2))2/Hz] (Tons/(milliMeter.Second2))2/Hertz [(t/(mm.s2))2/Hz] (Tons/(milliMeter.Second2))2/Hertz [(t/(mm.s2))2/Hz] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (nmmdat) µm, kg, µN, oC, s, V, mA megaNewtons2/Hertz [MPa2/Hz] (µmks) ft, lbm, lbf, oF, s, V, A ((Slug)/(Foot.Second2))2/Hertz [((lbm/32.2)/(ft.s2))2/Hz] (Bft) in, lbm, lbf, oF, s, V, A ((Slinch)/(Inch.Second2))2/Hertz [((lbm/386.4)/(in.s2))2/Hz] (Bin) Table 64 PSD Strain Unit System Measured in . . . o (Meters/Meter)2/Hertz [(m/m)2/Hz] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A (cgs) mm, kg, N, oC, s, mV, mA (nmm) mm, t, N, oC, s, mV, mA (nmmton) mm, dat, N, oC, s, mV, mA (nmmdat) µm, kg, µN, oC, s, V, mA (µmks) ft, lbm, lbf, oF, s, V, A (centiMeters/centiMeter)2/Hertz [(cm/cm)2/Hz] (milliMeters/milliMeter)2/Hertz [(mm/mm)2/Hz] (milliMeters/milliMeter)2/Hertz [(mm/mm)2/Hz] (milliMeters/milliMeter)2/Hertz [(mm/mm)2/Hz] (microMeters/microMeter)2/Hertz [(µm/µm)2/Hz] (Feet/Foot)2/Hertz [(ft/ft)2/Hz] (Bft) in, lbm, lbf, oF, s, V, A (Inches/Inch)2/Hertz [(in/in)2/Hz] (Bin) Table 65 PSD Stress Unit System Measured in . . . o Pascals2/Hertz [Pa2/Hz] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A (Dynes/centiMeter2)2/Hertz [(Dyne/cm2)2/Hz] (cgs) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 833 Features Unit System Measured in . . . o mm, kg, N, C, s, mV, mA (nmm) mm, t, N, oC, s, mV, mA (nmmton) mm, dat, N, oC, s, mV, mA (nmmdat) µm, kg, µN, oC, s, V, mA (kiloGrams/(millimeter.Second2))2/Hertz [(kg/(mm.s2))2/Hz] (Tons/(milliMeter.Second2))2/Hertz [(t/(mm.s2))2/Hz] (Tons/(milliMeter.Second2))2/Hertz [(t/(mm.s2))2/Hz] megaNewtons2/Hertz [MPa2/Hz] (µmks) ft, lbm, lbf, oF, s, V, A ((Slug)/(Foot.Second2))2/Hertz [((lbm/32.2)/(ft.s2))2/Hz] (Bft) in, lbm, lbf, oF, s, V, A ((Slinch)/(Inch.Second2))2/Hertz [((lbm/386.4)/(in.s2))2/Hz] (Bin) Table 66 PSD Velocity Unit System Measured in . . . o (meters/second)2/Hertz [(m/s)2/Hz] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A (centimeters/second)2/Hertz [(cm/s)2/Hz] (cgs) mm, kg, N, oC, s, mV, mA (millimeters/second)2/Hertz [(mm/s)2/Hz] (nmm) mm, t, N, oC, s, mV, mA (millimeters/second)2/Hertz [(mm/s)2/Hz] (nmmton) mm, dat, N, oC, s, mV, mA (millimeters/second)2/Hertz [(mm/s)2/Hz] (nmmdat) µm, kg, µN, oC, s, V, mA (µmks) ft, lbm, lbf, oF, s, V, A (micrometers/second)2/Megahertz [(µm/s)2/MHz] (feet/second)2/Hertz [(ft/s)2/Hz] (Bft) 834 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . o (inches/second)2/Hertz [(in/s)2/Hz] in, lbm, lbf, F, s, V, A (Bin) Table 67 Relative Permeability Unit System Measured in . . . o m, kg, N, C, s, V, A unitless (mks) cm, g, dyne, oC, s, V, A unitless (cgs) mm, kg, N, oC, s, mV, mA unitless (nmm) mm, t, N, oC, s, mV, mA unitless (nmmton) mm, dat, N, oC, s, mV, mA unitless (nmmdat) µm, kg, µN, oC, s, V, mA unitless (µmks) ft, lbm, lbf, oF, s, V, A unitless (Bft) in, lbm, lbf, oF, s, V, A unitless (Bin) Table 68 Relative Permittivity Unit System Measured in . . . o m, kg, N, C, s, V, A unitless (mks) cm, g, dyne, oC, s, V, A unitless (cgs) mm, kg, N, oC, s, mV, mA unitless (nmm) mm, t, N, oC, s, mV, mA unitless (nmmton) mm, dat, N, oC, s, mV, mA unitless Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 835 Features Unit System Measured in . . . (nmmdat) µm, kg, µN, oC, s, V, mA unitless (µmks) ft, lbm, lbf, oF, s, V, A unitless (Bft) in, lbm, lbf, oF, s, V, A unitless (Bin) Table 69 Rotational Damping Unit System Measured in . . . o Newton.meter.seconds/radian [N.m.s/rad] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A (cgs) mm, kg, N, oC, s, mV, mA (nmm) mm, t, N, oC, s, mV, mA (nmmton) mm, dat, N, oC, s, mV, mA (nmmdat) µm, kg, µN, oC, s, V, mA (µmks) ft, lbm, lbf, oF, s, V, A dyne.centimeter.seconds/radian [dyne.cm.s/rad] ton.millimeter2.seconds/second2.radian [t.mm2.s/s2.rad] ton.millimeter2.seconds/second2.radian [t.mm2.s/s2.rad] ton.millimeter2.seconds/second2.radian [t.mm2.s/s2.rad] microNewton.micrometer.seconds/radian [µN.µm.s/rad] (Slug)foot2.seconds/second2.radian [(lbm/32.2)ft2.s/s2.rad] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)inch2.seconds/second2.radian [(lbm/386.4)in2.s/s2.rad] (Bin) Table 70 Rotational Stiffness Unit System Measured in . . . o Newton.meters/radian [N.m/rad] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A dynes.centimeters/radian [dyne.cm/rad] (cgs) 836 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . o ton.millimeters2/second2.radian [t.mm2/s2.rad] mm, t, N, oC, s, mV, mA ton.millimeters2/second2.radian [t.mm2/s2.rad] mm, kg, N, C, s, mV, mA (nmm) (nmmton) mm, dat, N, oC, s, mV, mA (nmmdat) µm, kg, µN, oC, s, V, mA (µmks) ft, lbm, lbf, oF, s, V, A ton.millimeters2/second2.radian [t.mm2/s2.rad] microNewton.micrometers/radian [µN.µm/rad] (Slug)feet2/second2.radian [(lbm/32.2)ft2/s2.rad] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)inches2/second2.radian [(lbm/386.4)in2/s2.rad] (Bin) Table 71 Seebeck Coefficient Unit System Measured in . . .1 m, kg, N, oC, s, V, A Volts/degree Celsius [V/oC] (mks) cm, g, dyne, oC, s, V, A Volts/degree Celsius [V/oC] (cgs) mm, kg, N, oC, s, mV, mA milliVolts/degree Celsius [mV/oC] (nmm) mm, t, N, oC, s, mV, mA milliVolts/degree Celsius [mV/oC] (nmmton) mm, dat, N, oC, s, mV, mA milliVolts/degree Celsius [mV/oC] (nmmdat) µm, kg, µN, oC, s, V, mA Volts/degree Celsius [V/oC] (µmks) ft, lbm, lbf, oF, s, V, A Volts/degree Fahrenheit [V/oF] (Bft) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 837 Features Unit System Measured in . . .1 in, lbm, lbf, oF, s, V, A Volts/degree Fahrenheit [V/oF] (Bin) Table 72 Section Modulus Unit System Measured in . . . o meters3 [m3] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A centimeters3 [cm3] (cgs) mm, kg, N, oC, s, mV, mA millimeters3 [mm3] (nmm) mm, t, N, oC, s, mV, mA millimeters3 [mm3] (nmmton) mm, dat, N, oC, s, mV, mA millimeters3 [mm3] (nmmdat) µm, kg, µN, oC, s, V, mA micrometers3 [µm3] (µmks) ft, lbm, lbf, oF, s, V, A feet3 [ft3] (Bft) in, lbm, lbf, oF, s, V, A inches3 [in3] (Bin) millimeters3 [mm3] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] meters3 [m3] m, kg, s [ LS-DYNA solver] millimeters3 [mm3] mm, t, s [ LS-DYNA solver] inch3 [in3] in,lbf, s [ LS-DYNA solver] Table 73 Shear Elastic Strain Unit System o m, kg, N, C, s, V, A 838 Measured in . . . radians [rad] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (mks) cm, g, dyne, oC, s, V, A radians [rad] (cgs) mm, kg, N, oC, s, mV, mA radians [rad] (nmm) mm, t, N, oC, s, mV, mA radians [rad] (nmmton) mm, dat, N, oC, s, mV, mA radians [rad] (nmmdat) µm, kg, µN, oC, s, V, mA radians [rad] (µmks) ft, lbm, lbf, oF, s, V, A radians [rad] (Bft) in, lbm, lbf, oF, s, V, A radians [rad] (Bin) Table 74 Shock Velocity Unit System Measured in . . . o m, kg, N, C, s, V, A seconds/meters [s/m] (mks) cm, g, dyne, oC, s, V, A seconds/centimeters [s/cm] (cgs) mm, kg, N, oC, s, mV, mA seconds/millimeters [s/mm] (nmm) mm, t, N, oC, s, mV, mA seconds/millimeters [s/mm] (nmmton) mm, dat, N, oC, s, mV, mA seconds/millimeters [s/mm] (nmmdat) µm, kg, µN, oC, s, V, mA seconds/micrometers [s/µm] (µmks) ft, lbm, lbf, oF, s, V, A seconds/feet [s/ft] (Bft) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 839 Features Unit System Measured in . . . o in, lbm, lbf, F, s, V, A seconds/inches [s/in] (Bin) Table 75 Specific Heat Unit System Measured in . . .1 m, kg, N, oC, s, V, A Joules/kilogram.degree Celsius [J/kg.oC] (mks) cm, g, dyne, oC, s, V, A (cgs) mm, kg, N, oC, s, mV, mA (nmm) mm, t, N, oC, s, mV, mA (nmmton) mm, dat, N, oC, s, mV, mA (nmmdat) µm, kg, µN, oC, s, V, mA dyne.centimeters/gram.degree Celsius [dyne.cm/g.oC] millimeters2/second2.degree Celsius [mm2/s2.oC] millimeters2/second2.degree Celsius [mm2/s2.oC] millimeters2/second2.degree Celsius [mm2/s2.oC] picoJoules/kilogram.degree Celsius [pJ/kg.oC] (µmks) ft, lbm, lbf, oF, s, V, A feet2/second2.degree Fahrenheit [ft2/s2.oF] (Bft) in, lbm, lbf, oF, s, V, A inches2/second2.degree Fahrenheit [in2/s2.oF] (Bin) Joules/kilogram.degree Kelvin [J/kg.oK] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] Joules/kilogram/degree Kelvin [J/kg/oK] m, kg, s [ LS-DYNA solver] milliJoules/ton/degree Kelvin [mJ/t/oK] mm, t, s [ LS-DYNA solver] inch2/second2/oF [in2/s2/oF] in,lbf, s [ LS-DYNA solver] Table 76 Specific Weight Unit System o m, kg, N, C, s, V, A 840 Measured in . . . Newtons/meter3 [N/m3] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (mks) cm, g, dyne, oC, s, V, A dynes/centimeter3 [dyne/cm3] (cgs) mm, kg, N, oC, s, mV, mA tons/second2.millimeters2 [t/s2.mm2] (nmm) mm, t, N, oC, s, mV, mA tons/second2.millimeters2 [t/s2.mm2] (nmmton) mm, dat, N, oC, s, mV, mA tons/second2.millimeters2 [t/s2.mm2] (nmmdat) µm, kg, µN, oC, s, V, mA microNewtons/micrometer3 [µN/µm3] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)1/second2.feet2 [(lbm/32.2)1/s2.ft2] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)1/second2.inch2 [(lbm/386.4)1/s2.in2] (Bin) MegaNewtons/meter3 [MN/m3] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] Newtons/meter3 [N/m3] m, kg, s [ LS-DYNA solver] Newtons/millimeter3 [N/mm3] mm, t, s [ LS-DYNA solver] pound force/inch3 [lbf/in3] in,lbf, s [ LS-DYNA solver] Table 77 Stiffness Unit System Measured in . . . o m, kg, N, C, s, V, A Newtons/meter [N/m] (mks) cm, g, dyne, oC, s, V, A dynes/centimeter [dyne/cm] (cgs) mm, kg, N, oC, s, mV, mA Newtons/millimeter [N/mm] (nmm) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 841 Features Unit System Measured in . . . o mm, t, N, C, s, mV, mA Newtons/millimeter [N/mm] (nmmton) mm, dat, N, oC, s, mV, mA Newtons/millimeter [N/mm] (nmmdat) µm, kg, µN, oC, s, V, mA microNewtons/micrometer [µN/µm] (µmks) ft, lbm, lbf, oF, s, V, A pound force/foot [lbf/ft] (Bft) in, lbm, lbf, oF, s, V, A pound force/inch [lbf/in] (Bin) mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Newtons/meter [N/m] or milliNewtons/millimeter [mN/mm] Newtons/meter [N/m] [ LS-DYNA solver] mm, t, s Newtons/millimeter [N/m] [ LS-DYNA solver] in,lbf, s pound force/inch [lbf/in] [ LS-DYNA solver] Table 78 Strain and RS Strain Unit System Measured in . . . o m, kg, N, C, s, V, A meter/meter [m/m] (mks) cm, g, dyne, oC, s, V, A centimeter/centimeter [cm/cm] (cgs) mm, kg, N, oC, s, mV, mA millimeter/millimeter [mm/mm] (nmm) mm, t, N, oC, s, mV, mA millimeter/millimeter [mm/mm] (nmmton) mm, dat, N, oC, s, mV, mA millimeter/millimeter [mm/mm] (nmmdat) µm, kg, µN, oC, s, V, mA 842 micrometer/micrometer [µm/µm] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (µmks) ft, lbm, lbf, oF, s, V, A feet/foot [ft/ft] (Bft) in, lbm, lbf, oF, s, V, A inch/inch [in/in] (Bin) mm, mg, ms millimeter/millimeter [mm/mm] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s meter/meter [m/m] [ LS-DYNA solver] mm, t, s millimeter/millimeter [mm/mm] [ LS-DYNA solver] in,lbf, s inch/inch [in/in] [ LS-DYNA solver] Table 79 Stress and RS Stress Unit System Measured in . . . o m, kg, N, C, s, V, A Pascals [Pa] (mks) cm, g, dyne, oC, s, V, A dynes/centimeter2 [dyne/cm2] (cgs) mm, kg, N, oC, s, mV, mA ton/second2.millimeters [t/s2.mm] (nmm) mm, t, N, oC, s, mV, mA ton/second2.millimeters [t/s2.mm] (nmmton) mm, dat, N, oC, s, mV, mA ton/second2.millimeters [t/s2.mm] (nmmdat) µm, kg, µN, oC, s, V, mA megaPascals [MPa] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)/second2.foot [(lbm/32.2)/s2.ft] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)/second2.inch [(lbm/386.4)/s2.in] (Bin) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 843 Features Unit System Measured in . . . mm, mg, ms kiloPascals [kPa] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Pascals [Pa] [ LS-DYNA solver] mm, t, s megaPascals [MPa] [ LS-DYNA solver] pounds/inch2 [lb/in2] in,lbf, s [ LS-DYNA solver] Table 80 Strength Unit System Measured in . . . o m, kg, N, C, s, V, A Pascals [Pa] (mks) cm, g, dyne, oC, s, V, A dynes/centimeter2 [dyne/cm2] (cgs) mm, kg, N, oC, s, mV, mA ton/second2.millimeters [t/s2.mm] (nmm) mm, t, N, oC, s, mV, mA ton/second2.millimeters [t/s2.mm] (nmmton) mm, dat, N, oC, s, mV, mA ton/second2.millimeters [t/s2.mm] (nmmdat) µm, kg, µN, oC, s, V, mA megaPascals [MPa] (µmks) ft, lbm, lbf, oF, s, V, A (Slug)1/second2.foot [(lbm/32.2)1/s2.ft] (Bft) in, lbm, lbf, oF, s, V, A (Slinch)1/second2.inch [(lbm/386.4)1/s2.in] (Bin) mm, mg, ms kiloPascals [kPa] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s Pascals [Pa] [ LS-DYNA solver] mm, t, s 844 megaPascals [MPa] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . [ LS-DYNA solver] pounds/inch2 [lb/in2] in,lbf, s [ LS-DYNA solver] Table 81 Thermal Capacitance Unit System Measured in . . .1 m, kg, N, oC, s, V, A Joules/degree Celsius [J/oC] (mks) cm, g, dyne, oC, s, V, A Ergs/degree Celsius [Erg/oC] (cgs) mm, kg, N, oC, s, mV, mA milliJoules/degree Celsius [mJ/oC] (nmm) mm, t, N, oC, s, mV, mA milliJoules/degree Celsius [mJ/oC] (nmmton) mm, dat, N, oC, s, mV, mA milliJoules/degree Celsius [mJ/oC] (nmmdat) µm, kg, µN, oC, s, V, mA picoJoules/degree Celsius [pJ/oC] (µmks) ft, lbm, lbf, oF, s, V, A BTU/degree Fahrenheit [BTU/oF] (Bft) in, lbm, lbf, oF, s, V, A BTU/degree Fahrenheit [BTU/oF] (Bin) Table 82 Thermal Conductance Unit System Measured in . . .1 m, kg, N, oC, s, V, A Watts/degree Celsius [W/oC] (mks) cm, g, dyne, oC, s, V, A Watts/degree Celsius [W/oC] (cgs) mm, kg, N, oC, s, mV, mA Watts/degree Celsius [W/oC] (nmm) mm, t, N, oC, s, mV, mA Watts/degree Celsius [W/oC] (nmmton) mm, dat, N, oC, s, mV, mA Watts/degree Celsius [W/oC] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 845 Features Measured in . . .1 Unit System (nmmdat) µm, kg, µN, oC, s, V, mA picoWatts/degree Celsius [pW/oC] (µmks) ft, lbm, lbf, oF, s, V, A BTU/second.degree Fahrenheit [BTU/s.oF] (Bft) in, lbm, lbf, oF, s, V, A BTU/second.degree Fahrenheit [BTU/s.oF] (Bin) Table 83 Thermal Expansion Unit System Measured in . . .1 m, kg, N, oC, s, V, A 1/degree Celsius [1/oC] (mks) cm, g, dyne, oC, s, V, A 1/degree Celsius [1/oC] (cgs) mm, kg, N, oC, s, mV, mA 1/degree Celsius [1/oC] (nmm) mm, t, N, oC, s, mV, mA 1/degree Celsius [1/oC] (nmmton) mm, dat, N, oC, s, mV, mA 1/degree Celsius [1/oC] (nmmdat) µm, kg, µN, oC, s, V, mA 1/degree Celsius [1/oC] (µmks) ft, lbm, lbf, oF, s, V, A 1/degree Fahrenheit [1/oF] (Bft) in, lbm, lbf, oF, s, V, A 1/degree Fahrenheit [1/oF] (Bin) microJoules/degree Kelvin [µJ/oK] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s 1/degree Kelvin [1/oK] [ LS-DYNA solver] mm, t, s 1/degree Kelvin [1/oK] [ LS-DYNA solver] 846 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . .1 in,lbf, s 1/degree Fahrenheit [1/oF] [ LS-DYNA solver] Table 84 Temperature Unit System Measured in . . .1 m, kg, N, oC, s, V, A degrees Celsius [oC] (mks) cm, g, dyne, oC, s, V, A degrees Celsius [oC] (cgs) mm, kg, N, oC, s, mV, mA degrees Celsius [oC] (nmm) mm, t, N, oC, s, mV, mA degrees Celsius [oC] (nmmton) mm, dat, N, oC, s, mV, mA degrees Celsius [oC] (nmmdat) µm, kg, µN, oC, s, V, mA degrees Celsius [oC] (µmks) ft, lbm, lbf, oF, s, V, A degrees Fahrenheit [oF] (Bft) in, lbm, lbf, oF, s, V, A degrees Fahrenheit [oF] (Bin) degrees Kelvin [oK] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] degrees Kelvin [oK] m, kg, s [ LS-DYNA solver] degrees Kelvin [oK] mm, t, s [ LS-DYNA solver] degrees Fahrenheit [oF] in,lbf, s [ LS-DYNA solver] Table 85 Temperature Difference Unit System Measured in . . .1 m, kg, N, oC, s, V, A degrees Celsius [oC] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 847 Features Measured in . . .1 Unit System (mks) cm, g, dyne, oC, s, V, A degrees Celsius [oC] (cgs) mm, kg, N, oC, s, mV, mA degrees Celsius [oC] (nmm) mm, t, N, oC, s, mV, mA degrees Celsius [oC] (nmmton) mm, dat, N, oC, s, mV, mA degrees Celsius [oC] (nmmdat) µm, kg, µN, oC, s, V, mA degrees Celsius [oC] (µmks) ft, lbm, lbf, oF, s, V, A degrees Fahrenheit [oF] (Bft) in, lbm, lbf, oF, s, V, A degrees Fahrenheit [oF] (Bin) degrees Kelvin [oK] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] Table 86 Time Unit System Measured in . . . o m, kg, N, C, s, V, A seconds [s] (mks) cm, g, dyne, oC, s, V, A seconds [s] (cgs) mm, kg, N, oC, s, mV, mA seconds [s] (nmm) mm, t, N, oC, s, mV, mA seconds [s] (nmmton) mm, dat, N, oC, s, mV, mA seconds [s] (nmmdat) µm, kg, µN, oC, s, V, mA seconds [s] (µmks) 848 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . o ft, lbm, lbf, F, s, V, A seconds [s] (Bft) in, lbm, lbf, oF, s, V, A seconds [s] (Bin) mm, mg, ms milliseconds [ms] [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s seconds [s] [ LS-DYNA solver] mm, t, s seconds [s] [ LS-DYNA solver] in,lbf, s seconds [s] [ LS-DYNA solver] Table 87 Translational Damping Unit System Measured in . . . o Newton.seconds/meter [N.s/m] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A dyne.seconds/centimeter [dyne.s/cm] (cgs) mm, kg, N, oC, s, mV, mA (nmm) mm, t, N, oC, s, mV, mA (nmmton) mm, dat, N, oC, s, mV, mA (nmmdat) µm, kg, µN, oC, s, V, mA ton.millimeter.seconds/second2.millimeter [t.mm.s/s2.mm] ton.millimeter.seconds/second2.millimeter [t.mm.s/s2.mm] ton.millimeter.seconds/second2.millimeter [t.mm.s/s2.mm] microNewton.seconds/micrometer [µN.s/µm] (µmks) ft, lbm, lbf, oF, s, V, A (Bft) (Slug)foot.seconds/second2.foot [(lbm/32.2)ft.s/s2.ft] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 849 Features Unit System Measured in . . . o (Slinch)inch.seconds/second2.inch [(lbm/386.4)in.s/s2.in] in, lbm, lbf, F, s, V, A (Bin) Table 88 Velocity and RS Velocity Unit System Measured in . . . o m, kg, N, C, s, V, A meters/second [m/s] (mks) cm, g, dyne, oC, s, V, A centimeters/second [cm/s] (cgs) mm, kg, N, oC, s, mV, mA millimeters/second [mm/s] (nmm) mm, t, N, oC, s, mV, mA millimeters/second [mm/s] (nmmton) mm, dat, N, oC, s, mV, mA millimeters/second [mm/s] (nmmdat) µm, kg, µN, oC, s, V, mA micrometers/second [µm/s] (µmks) ft, lbm, lbf, oF, s, V, A feet/second [ft/s] (Bft) in, lbm, lbf, oF, s, V, A inches/second [in/s] (Bin) mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] m, kg, s meters/second [m/s] or millimeters/millisecond [mm/ms] meters/second [m/s] [ LS-DYNA solver] mm, t, s millimeters/second [mm/s] [ LS-DYNA solver] in,lbf, s inches/second [in/s] [ LS-DYNA solver] Table 89 Voltage Unit System o m, kg, N, C, s, V, A 850 Measured in . . . Volts [V] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview Unit System Measured in . . . (mks) cm, g, dyne, oC, s, V, A Volts [V] (cgs) mm, kg, N, oC, s, mV, mA milliVolts [mV] (nmm) mm, t, N, oC, s, mV, mA milliVolts [mV] (nmmton) mm, dat, N, oC, s, mV, mA milliVolts [mV] (nmmdat) µm, kg, µN, oC, s, V, mA Volts [V] (µmks) ft, lbm, lbf, oF, s, V, A Volts [V] (Bft) in, lbm, lbf, oF, s, V, A Volts [V] (Bin) Table 90 Volume Unit System Measured in . . . o meters3 [m3] m, kg, N, C, s, V, A (mks) cm, g, dyne, oC, s, V, A centimeters3 [cm3] (cgs) mm, kg, N, oC, s, mV, mA millimeters3 [mm3] (nmm) mm, t, N, oC, s, mV, mA millimeters3 [mm3] (nmmton) mm, dat, N, oC, s, mV, mA millimeters3 [mm3] (nmmdat) µm, kg, µN, oC, s, V, mA micrometers3 [µm3] (µmks) ft, lbm, lbf, oF, s, V, A feet3 [ft3] (Bft) in, lbm, lbf, oF, s, V, A inches3 [in3] Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 851 Features Unit System Measured in . . . (Bin) millimeters3 [mm3] mm, mg, ms [ANSYS (AUTODYN) and LS-DYNA solvers] meters3 [m3] m, kg, s [ LS-DYNA solver] millimeters3 [mm3] mm, t, s [ LS-DYNA solver] inches3 [in3] in,lbf, s [ LS-DYNA solver] All “ton” designations in the table mean metric ton. 1 — Selecting Kelvin as the unit for temperature updates the default temperature values to Kelvin unit system. Workbench uses temperature values in Celsius for the metric system, by default. To change the units from Celsius to Kelvin: • On the Units menu, click Kelvin. Conversion Factors • Degree Celsius to Kelvin — C + 273.15. • Kelvin to degree Celsius — K-273.15. • Kelvin to degrees Fahrenheit — ((K-273.15)*9/5)-32. Saving your Results in the Mechanical Application There are three ways to save your results in the Mechanical application: • As a Mechanical APDL application database file. To save the Mechanical application results in a Mechanical APDL application database file, click Analysis Settings on the Tree Outline (p. 235) and in its Details, click Yes next to Save ANSYS db under Analysis Data Management (p. 549). • As an input file for the Mechanical APDL application. See Writing and Reading the Mechanical APDL Application Files (p. 852). • As a Mechanical application database file. To save your solution as a Mechanical application database file, select File> Export. Select File> Save As in the Project Schematic to save the project. The Save As dialog box appears, allowing you to type the name of the file and specify its location. Writing and Reading the Mechanical APDL Application Files The Tools menu includes options for writing the Mechanical APDL application input files and for reading the Mechanical APDL application results files. 852 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview To write the Mechanical APDL application input file: 1. Highlight the Solution object folder in the tree. 2. From the Main Menu (p. 280), choose Tools> Write Input File.... 3. In the Save As dialog box, specify a location and name for the input file. To read the Mechanical APDL application result files: 1. Highlight the Solution object folder in the tree. 2. From the Main Menu (p. 280), choose Tools> Read Result Files.... 3. Browse to the folder that contains the Mechanical APDL application result files and click Open. 4. In the dialog box that follows, select the unit system, then click OK. Note • Errors will occur if the Mechanical APDL application result files are from a version of the Mechanical application that is older than the version currently running. • Referring to step 3 in the above procedure, the directory to which you browse should only contain files pertinent to that solution. Otherwise failure of Mechanical to identify the proper files could occur if extraneous files exist in the directory. In addition, if the folder that you browse to contains multiple result files or jobname runs, files identified as solver generated files will be copied from this folder and those that match the jobname you select in the file browse window will be renamed to the “file” jobname during the copy. Files already with the jobname of “file” will be copied as well. It is for this reason that you should avoid browsing to a folder that contains a mix of files with the base name “file” combined with files without this base name. Mechanical APDL Application Analysis from a Mechanical Application Mesh The option for writing the Mechanical APDL application file can be used to perform analyses in the Mechanical APDL application while taking advantage of the meshing capabilities within the Mechanical application. The procedure is as follows: 1. Attach the model into the Mechanical application. 2. Mesh the model. 3. Select the Solution folder in the tree. 4. Tools> Write Input File... and specify a location and name for the input file. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 853 Features 5. Use this input file to complete your analysis in the Mechanical APDL application. The meshed model will contain generic elements encoding only shape and connectivity information. Such elements can then be replaced by others that are appropriate to your desired analysis. Note Any named selection group from the Mechanical application is transferred to the Mechanical APDL application as a component according to specific naming rules and conventions. Using Writing and Reading Files Together The writing and reading options are useful when used together. You can use the write option, then solve at your leisure on the machine of your choice. When the solution is done, you can use the read option to browse to the directory that contains the Mechanical APDL application output files (for example, result file, file.err, solve.out, file.gst, file.nlh). Workbench will then copy all files into your solution directory and proceed to use those files for postprocessing. The reading option requires that the directory include the result and file.err files at a minimum. Note You must ensure that the mesh in the result file matches the mesh in Workbench. The reading Mechanical APDL application file option is available for all analysis types except rigid dynamic analyses and shape analyses. The writing Mechanical APDL application file option is available for all analysis types except rigid dynamic analyses. System units must be specified in the Mechanical APDL application result files being read for Result Tracker graphs to display properly. Result Tracker graphs will display in the Mechanical APDL application result file units if the units specified when reading the files are inconsistent with those in the files. Converting Boundary Conditions to Nodal DOF Constraints (Mechanical APDL Solver) This section discusses converting structural boundary conditions on the geometry to constraints on the mesh for analyses targeting the ANSYS solver. In the Mechanical APDL application, structural degree-of-freedom constraints can be defined at individual nodes. Specifically, you can choose to constrain each node along any of the three axis directions (x, y, z) of its local coordinate system to simulate the kinds of supports your model requires. In the Mechanical application, however, you specify boundary conditions on the geometry, so the program must automatically convert them into nodal constraints prior to solution. Ordinarily, this process is straightforward and the boundary conditions can be transcribed directly onto the nodes. In certain cases, however, the Mechanical application may be confronted with combinations of boundary conditions that require negotiation to produce an equivalent rendition of the effective constraints acting on the nodes. A common case occurs in structural analyses where two or more boundary conditions are applied to neighboring topologies, for example, Frictionless Supports applied to neighboring faces that meet at an angle: the nodes on the edge are subject to two separate combinations of DOF constraints, one from each Frictionless Support. The Mechanical application attempts to identify a suitable orientation to the nodal coordinate system that accommodates both frictionless supports and, if successful, constrain 854 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solving Overview its axes accordingly. Should this attempt ever fail, the solution will be prevented and an error will be issued to the Message Window (See The Solver Has Found Conflicting DOF Constraints (p. 1088) in the Troubleshooting section.) Among the boundary conditions that participate in this conversion, there are: Fixed Supports (Fixed Face, Fixed Edge, Fixed Vertex) Simply Supported (Simply Supported Edge, Simply Supported Vertex) Fixed Rotation Displacements (Displacements for Faces, Displacement for Edges, Displacements For Vertices) Frictionless Support Cylindrical Support Symmetry Regions The calculations that convert the boundary conditions into nodal constraints involve: • the identification of the linear span contributed by each of the boundary conditions • the combination of the individual spans into a final nodal constraint choice. Angular tolerances are involved in distinguishing and combining the spans; a program controlled tolerance of 0.01 degrees will be used. Note The calculations have a built in preference for producing nodal coordinate systems that are closest in orientation to the global coordinate system. Resolving Thermal Boundary Condition Conflicts Conflicts between boundary conditions scoped to parts and individual faces Boundary conditions applied to individual geometry faces always override those that are scoped to a part(s). For conflicts associated with various boundary conditions, the order of precedence is as follows: 1. Applied temperatures (Highest). 2. Convection, heat fluxes, and flows (Cumulative, but overridden by applied temperatures). 3. Insulated (Lowest. Overridden by all of the above). Resume Capability for Explicit Dynamics Analyses If an Explicit Dynamics analysis has partially or totally completed, then it is possible to resume the analysis from a non-zero time step (cycle). These are some examples of why this would be desirable: • To extend an analysis that has successfully completed beyond its current end time or cycle. • To complete an analysis that has been interrupted. For example you may wish to interrupt an analysis in order to review results part way through a longer simulation. • To continue an analysis that has stopped part way through. For example, if an analysis has terminated prematurely due to the time-step size being too small, you can make adjustments to mass scaling, and restart the calculation. • To adjust the frequency of restart file, result file or other output information. For example, you may wish to re-solve part of an analysis that is of interest with more frequent results. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 855 Features • To adjust damping or erosion controls. An analysis may be resumed from any cycle that has a restart file by first selecting the cycle in the Resume From Cycle field located in the Step Controls section of the Analysis Settings, then making any other required analysis changes, and selecting Solve. The frequency of restart file output is controlled in the Analysis Settings Output Controls. There is no limit to the number of times an analysis may be resumed. The following restrictions apply: • Changes made to any feature of the model outside of the Analysis Settings will prevent a resume from taking place. • Changes made to any of the (Analysis Settings) Solver Controls, except for Minimum Velocity, Maximum Velocity and Radius Cutoff, will prevent a resume from taking place. • Changes made to the Retain Inertia of Eroded Material field will prevent a resume from taking place. • Changes to all other Erosion Controls, Damping Controls, and Output Controls are valid and will not prevent a resume from taking place. • To use Automatic Mass Scaling under (Analysis Settings, Step Controls), it must be enabled from the start of the calculation. You cannot change the Automatic Mass Scaling property for a restart calculation. If Automatic Mass Scaling is active, the other Mass Scaling properties may be changed part way through a calculation. • Analyses with non-zero Displacement constraints defined may not be resumed. Commands Objects You can input commands such as Mechanical APDL commands, directly in the Mechanical application using a Commands object. Refer to the Commands objects reference page for information on valid objects under which you can insert single or multiple Commands objects. Upon inserting a Commands object, the Worksheet appears and displays information or special instructions tailored to the specific parent object. For example, the following information appears if you insert a Commands object under a Contact Region object: *********contact region default statement********* ! Commands inserted into this file will be executed just after the contact region definition. ! The type number for the contact type is equal to the parameter "cid". ! The type number for the target type is equal to the parameter "tid". ! The real and mat number for the asymmetric contact pair is equal to the parameter "cid". ! The real and mat number for the symmetric contact pair(if it exists) is equal to the parameter "tid". Note For the Transient Structural (Rigid Dynamics) systems, commands are expressed in Python. The following topics are covered in this section: Commands Object Features Using Commands Objects with the MAPDL Solver 856 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Commands Objects Commands Object Features Solver Target The Target property in the Details view of a Commands object allows you to associate the object with a solver target. All text that displays for a new Commands object can vary and is dependent on the associated solver target. When displayed, the Target property is set according to the following situations: • If all the environments in the tree have the same solver target then the Commands object is tied to that solver target. • If there is a mix of solver targets in the tree, the Target property is left empty and you must assign a solver target. The commands inserted into the Commands object will only be sent to the solver if the solver target of the environment being solved matches that of the Commands object. Post Processing Command Specifications The Commands object can perform post processing actions when inserted under the Solution object. For solved analyses, you can specify a command and choose whether the MAPDL Solver processes the specified commands only or whether the solver processes the entire solution (including the new command) all over again using the Invalidate Solution control. This control is, by default, set to No - do not invalidate the results. If the solver is not specified as MAPDL, then the Invalidate Solution control defaults to Yes and is read-only. An example of the Commands object and its Details is illustrated below. As shown on the status/progress dialog box, the Solver processes only the newly specified commands. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 857 Features Post Output File The post command entries generate a new and independent solution output file, post.dat. The post.dat file contains only the content of unsuppressed command objects. The output file can be viewed in the Worksheet for the Solution Information object by setting the Solution Output control to Post Output, as shown below. 858 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Commands Objects Note • This post processing solution only happens if changes or additions are made to the Commands of a Solution object for an otherwise solved environment. If the solution is unsolved or obsolete for some other reason, then the commands are executed as part of the normal solving process. • Existing and post processed results are available for use with any subsequent linked analyses. • When using this mode, MAPDL runs all commands including the ones that may have existed as a part of the regular solve. Some commands may require certain variables or parameters to be active for execution or to produce correct results. As a result, it may be necessary to resume MAPDL db file by making sure that the Analysis Settings>Analysis Data Management>Save MAPDL db option is set to Yes prior to restarting the entire solution. • The solve mode is always In Process. • If the command snippet is inserted or edited with the Invalidate Solution setting set to Yes, then you can issue post-processing commands using the last restart point of a completed solution. The solution executes without incurring the cost of a full solve, as it sends only the post commands and will generate solve.out as a solution output file. Note that the generated Output files are written to the Solver Files Directory and are named accordingly. An example of the directory is shown below. Input Arguments (Not applicable to the LS-DYNA solver) Input arguments are available on all Commands objects. There are nine arguments that you can pass to the Mechanical APDL application macros. Numerical values only are supported. Input Arguments are editable on the Details view of a Commands object under Input Arguments and listed as ARG1 through ARG9. If you enter a numerical value, including zero, for an argument, that value is passed along to the Mechanical APDL application. If you leave the argument value field empty, no argument value is passed for that specific argument. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 859 Features Note If you are calling a user defined macro from within a Commands object, be aware of the macro's location on the disk to make sure the macro is able to be located during the solution. Refer to the /PSEARCH command description located in the Mechanical APDL application Command Reference within the Mechanical APDL Help for more information. Commands Object Controls The following controls are also available with Commands objects. Each control is available from the toolbar or from the context menu that appears from a right mouse button click on a Commands object: • Export...: Exports the text in the Worksheet to an ASCII text file. Note You must right-mouse click on the selected object in the tree to use this Export feature. On Windows platforms, if you have the Microsoft Office 2002 (or later) installed, you may see an Export to Excel option if you right-mouse click in the Worksheet. This is not the Mechanical application Export feature but rather an option generated by Microsoft Internet Explorer. • Import...: Imports the text from an ASCII text file to the Worksheet. You can rename the Commands object to the name of an imported or exported file by choosing Rename Based on Definition from the context menu available through a right mouse button click. The Commands object is renamed to the name appearing in the File Name field under the Details view. • Refresh: Synchronizes the text in the Worksheet to that of the currently used ASCII text file. Refresh can be used to discard changes made to commands text and revert to a previously imported or exported version. • Suppress (available in context menu only): Suppressed commands will not propagate to the Mechanical APDL application input file. Note Preprocessing Commands objects or Postprocessing Commands objects, available in past releases are no longer supported. If you open a database that includes these objects, the objects are automatically converted to Commands objects. • Search Parameters (available only at the Solution level): Scans the text output and updates the list of detected parameters. Matched the Mechanical APDL application parameters can be parameterized just as other values in Workbench can be parameterized. Refer to the next section for details. Using Commands Objects with the MAPDL Solver The following information applies to Commands objects used with the MAPDL solver. Their use with other solvers may exhibit different behavior. 860 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Commands Objects Text and Units Commands text cannot contain characters outside of the standard US ASCII character set due to the fact that this text will propagate into the Mechanical APDL application input files and must follow the rules set aside for the Mechanical APDL application commands and input files. Use of languages other than English for the command text may cause erratic behavior. The Mechanical APDL application commands should not be translated. Make sure that you use consistent units throughout a simulation. Commands objects whose inputs are units-dependent will not update if you change unit systems for solving. Commands object input for magnetostatic analyses must be in MKS units (m, Kg, N, V, A). Step Selection Mode For stepped analyses, the Step Selection Mode control is also available in the Details view of a Commands object when you insert the object under an Environment. This control allows you to specify which sequence steps are to process the Commands object. The choices are: First, Last, All, and By Number. If you choose By Number, a Sequence Number control appears that allows you to scroll through and select a specific numbered step that will process the Commands object. User Convenience Parameters When a project is saved in workbench, the application’s project file management creates a directory/folder structure. The generated folders house a variety of files, such as input or result files. As a part of this structure, there is a folder created that is named user_files. The MAPDL solver input file, ds.dat, includes the following parameter (variable): _wb_userfiles_dir(1) The value of this parameter equals the path to the user_files directory. You can use this parameter with the Commands Object and perform file operations in the MAPDL language. For example, by specifying this parameter, you can copy result files to the user_files directory. For a more specific example, accessing external user macros located in this directory might be done using the following MAPDL command: /INPUT, '%_wb_userfiles_dir(1)%file_aqld1001.dat' For additional information on the MAPDL Command language, see the Mechanical APDL Command Reference. Output Parameters: Using Parameters Defined in Solution Command Objects For Commands objects at the Solution level, an output search prefix can be used to scan the text from a resulting solution run. After you choose Search Parameters, values for the Mechanical APDL application parameter assignments are returned that match the output search prefix. The default output search prefix is my_. Changing the prefix at any time causes a rescan of the text for a matching list. After a SOLVE, the Mechanical APDL application parameters that are found to match the prefix are listed in the Details view for the Commands object with their values. This procedure is illustrated in the demonstration below. Parameters created using Commands objects can be used in Design Exploration. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 861 Features Note If you have parameterized an output parameter in the Commands object, you cannot edit the command text. You need to remove the parameters to edit the text The following demo is presented as an animated GIF. Please view online if you are reading the PDF version of the help. Interface names and other components shown in the demo may differ from those in the released product. Viewing Mechanical APDL Application Plots in Workbench You can view Mechanical APDL application plots in Workbench that result from using Commands objects. The Mechanical APDL application plots are returned from Mechanical APDL to display in the Worksheet. This feature is useful if you want to review result plots that are available in the Mechanical APDL application but not in Workbench, such as unaveraged stress results or contact results only on a particular region. To View the Mechanical APDL Application Plots in Workbench: 1. Create one or more Commands objects. 2. Direct plot(s) to PNG format. 3. Request plots in the Commands objects. 4. Make sure that there is at least one Commands object under Solution in the tree. 5. Solve. Requested plots for all Commands objects are displayed as objects under the first unsuppressed Commands object that appears below Solution. Note The Mechanical APDL application PowerGraphics mode for displaying results is not compatible with Commands objects. No results will be produced in this mode. If your command list includes the PowerGraphics mode (/GRAPH,POWER), you must switch to the Full mode by including /GRAPH,FULL at the end of the list. Presented below is an example of a Commands object used to create two plots, one for unaveraged stress, and one for element error. ! ! 862 Commands inserted into this file will be executed immediately after the ANSYS /POST1 command. If a SET command is issued, results from that load step will be used as the basis of all Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Commands Objects ! result objects appearing in the Solution folder. /show,png ! output to png format /gfile,650 ! adjust size of file /edge,1,1 /view,,1,1,1 ! turn on element outlines ! adjust view angle ples,s,eqv ples,serr ! plot unaverage seqv ! plot element error The Mechanical APDL application plots are shown below. Unaveraged Stress Result: Element Error Result: Suggestions on Using Commands Objects with Materials 1. When using Commands objects, do not change the material IDs for elements. This will cause the results retrieval form the Mechanical APDL application to Workbench to malfunction. 2. Instead of adding one large Commands object to change all of the materials, add individual Commands objects under each part. That way you will be able to reference the “matid” in the Commands object for the material ID of the elements that make up the part. You will also only need to enter the adjusted coefficient of thermal expansion and not the other materials. 3. Use the Worksheet view of the Geometry object to determine which materials are assigned to specific parts. 4. Click the right mouse button on a selected item in the Worksheet view, then choose Go To Selected Items in Tree to add Commands objects. 5. Copy and paste Commands objects from one part to another that have the same material assignment. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 863 Features Possible Conflicts Between the Mechanical and Mechanical APDL Applications Commands objects can be used to access the Mechanical APDL application commands from within Workbench. The commands issued by the Commands objects affect the solution. However they do not alter settings within Workbench. The Mechanical APDL application commands used in Commands objects may conflict with internal settings in Workbench. One example where a possible conflict between the Mechanical APDL application and Workbench can occur is when Commands objects are used to define material models. The user may have defined only linear elastic properties in Engineering Data. However, it is possible to use the Mechanical APDL application commands in a Commands object to override the material properties defined in Engineering Data or even change the linear elastic material model to a nonlinear material model, such as adding a bilinear kinematic hardening (BKIN) model. In that case, the solution will use the BKIN model defined in the Commands object. However, since the Mechanical application is unaware of the nonlinear material specified by the Commands object, nonlinear solution quantities such as plastic strain will not be available for postprocessing. Another example where a possible conflict between the Mechanical APDL application and Workbench can occur is when Commands objects are used to define boundary conditions. The Mechanical APDL application nodal boundary conditions are applied in the nodal coordinate system. For consistency, Workbench sometimes must internally rotate nodes. The boundary conditions specified by the commands in the Commands object will be applied in the rotated nodal coordinate system. Other situations can occur where the Mechanical APDL application commands issued in Commands objects are inconsistent with Workbench. It is the user’s responsibility to confirm that any the Mechanical APDL application commands issued in a Commands object do not conflict with Workbench. Commands support the definition of Mechanical APDL arguments via the settings of the properties ARG1 through ARG9. Once a value for one of these arguments is set, it will be retained for the remainder of the MAPDL solve run unless explicitly set to zero in the Commands text. Report Preview Click the Report Preview tab to create a report that covers all analyses in the Outline. The process starts immediately. Unlike prior report generators, this system works by extracting information from the user interface. It first selects each item in the Outline, then examines worksheets in a second pass, and finally appends any material data used in the analysis. The material data will be expressed in the Workbench standard unit system which most closely matches the Mechanical application unit system. Once started the report generation process must run to completion. Avoid clicking anywhere else in Workbench during the run because this will stop the report process and may cause an error. This approach to reporting ensures consistency, completeness, and accuracy. This section examines the following Report Preview topics: Tables Figures and Images Publishing Sending Comparing Databases Customize Report Content 864 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Report Preview Tables Most tables in the report directly correspond to the Details of an object or set of related objects. Object names appear across the top of the tables. By default, tables contain no more than six columns. This limit increases the likelihood that tables will fit on the screen and on printed pages. In the Report Options dialog you can increase or decrease the limit. For example, you may allow more columns if object names take up little space, if you have a high resolution screen, or print in landscape layout. The minimum is two columns, in which case no grouping of objects occurs and the Contents is equivalent to the Outline. The system merges identical table cells by default. This reduces clutter and helps to reveal patterns. You can disable this feature in the Report Options dialog. Figures and Images Figures and Images appear in the report as specified in the Outline. The system automatically inserts charts as needed. The system creates all bitmap files in PNG format. You may change the size of charts and figures in the Report Options dialog. For example, you may specify smaller charts due to few data points or bigger figures if you plan to print on large paper. For best print quality, increase the Graphics Resolution in the Report Options dialog. Publishing Click the Publish toolbar button to save your report as a single HTML file that includes the picture files in a given folder, or as an HTML file with a folder containing picture files. The first option produces a single MHT file containing the HTML and pictures. MHT is the same format used by Internet Explorer when a page is saved as a “Web Archive”. Only Internet Explorer 5.5 or later on Windows supports MHT. For the other two options, the HTML file is valid XHTML 1.0 Transitional. Full support for MHT file format by any other browser cannot be guaranteed. Sending Click the Send To button to send the report as an E-mail attachment, or to open the report in Microsoft Word or import the figures into Microsoft PowerPoint. When emailing, a single MHT file is automatically attached. Note that some email systems may strip or filter MHT files from incoming messages. If this occurs, email a ZIP archive of a published report or email the report from Microsoft Word. Sending a report to Word is equivalent to opening a published HTML file in the application. Sending a report to PowerPoint creates a presentation where one figure or image appears per slide. No other data is imported. Comparing Databases Because the report content directly corresponds to the user interface, it is easy to determine exactly how two databases differ. Generate a report for the first database, open it in Word, save and exit. Open the report for the second database in Word and choose Tools>Compare Documents. In the dialog, uncheck the Find Formatting box and select the first file. Word highlights the differences, as illustrated here: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 865 Features Customize Report Content Report customization falls into two categories: preferences in the Report Options dialog and the ability to run a modified report generator from a local or network location. This ability to externalize the system is shared by the Mechanical Wizard. It allows for modifications outside of the installation folder and reuse of a customized system by multiple users. To run report externally: 1. Copy the following folder to a different location: Program Files\ANSYS Inc\v140\AISOL\DesignSpace\DSPages\Language\en-us\Report2006. 2. Specify the location under Custom Report Generator Folder in the Report Options (for example: \\server\copied_Report2006_folder). The easiest customization is to simply replace Logo.png. The system uses that image on the wait screen and on the report cover page. The file Template.xml provides the report skeleton. Editing this file allows: • Reformatting of the report by changing the CSS style rules. • Addition of standard content at specific points inside the report body. This includes anything supported by XHTML, including images and tables. The file Rules.xml contains editable configuration information: • Standard files to include and publish with reports. The first is always the logo; other files could be listed as the images used for custom XHTML content. • Rules for excluding or bolding objects in the Contents. • Rules for applying headings when objects are encountered. • Selective exclusion of an object’s details. For example, part Color (extracted as a single number) isn’t meaningful in a report. • Exclusion of Graph figures for certain objects. This overrides the other four criteria used to decide if a Graph figure is meaningful. • Rules against comparing certain types of objects. • Object states that are acceptable in a “finalized” report. • Search and replace of Details text. For example, the report switches "Click to Change" to "Defined". This capability allows for the use of custom terminology. 866 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Parameters • Insertion of custom XHTML content based on object, analysis and physics types, and whether the content applies to the details table, the chart or the tabular data. For example, report includes a paragraph describing the modal analysis bar chart. All files in the Report2006 folder contain comments detailing customization techniques. Meshing in the Mechanical Application All meshing operations in the Mechanical application are described in the Meshing Overview section of the Meshing Help. Parameters The term Parameters in the Mechanical application includes CAD parameters and engineering parameters (pressure magnitude, maximum stress, fatigue life, dimension of a part, material property type, Young's modulus, and others). While engineering parameters are indicated simply by clicking the parameter box in the Details View (p. 274), CAD Parameters (p. 869) must be given some extra attention, both in the CAD package and in the Mechanical application. The Parameter Workspace collects all specified parameters and lists them in the Parameter Workspace grids for later use and/or modification. Related topics: • Specifying Parameters (p. 867) Specifying Parameters The Details View (p. 274) in the application window provides check boxes for items that may be parameterized. The following Details View images illustrate parameter definition for typical objects in the Mechanical application: Part Object (p. 867) Force Object (p. 868) Stress Object (p. 868) Part Object The details of a part object: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 867 Features A P defines the Volume as parameterized. Force Object The details for a Force object: The Magnitude of the force is parameterized. Other details, such as the Geometry, Define By and Direction cannot be parameterized. Stress Object The details for a Stress object. 868 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Parameters A P appears next to the selected output parameters. The Minimum is selected as an output parameter. The Maximum is not selected as an output parameter. Parameter Restrictions If an object has a parameterized field, and that object definition is changed in a way that makes that parameterization non-meaningful, the parameterization will be removed by the program. Some examples include: • A material in Engineering Data has a parameterized density, and then the user suppresses the material. • A result in the Mechanical application is scoped to a face and has a parameterized maximum value, and then the user re-scopes the result to a different topology. Note If you suppresses an object, no parameter boxes will be shown for any property on that object. If you parameterize the Suppressed property on an object, no parameter boxes will be shown for any other property on that object, regardless of whether or not the object is suppressed. CAD Parameters CAD parameters are a subset of the application parameters. As the name implies, CAD parameters come from a CAD system and are used to define the geometry in the CAD system. Although each CAD system assigns its parameters differently, the Mechanical application identifies them via a key (ds or DS). This identifier can appear either at the beginning or the end of the parameter name and does not need to be separated from the name with an underscore or any other character. By identifying the parameters of interest you can effectively filter CAD parameter exposure. Any of the following examples are valid CAD parameter names using DS or ds as the key: • DSlength • widthds • dsradius DS is the default key for importing CAD parameters into the application. You can change this default via the Personal Parameter Key option on the Geometry Preferences. Note If you change the key phrase to nothing all parameters are exposed. CAD parameters must be assigned correctly in the CAD system in order to be imported. Refer to your CAD system instructions for detailed information on assigning these parameters. Some system specific notes are included here for your convenience. Remember that these are all actions that must be performed in the CAD system before importing the model. CAD systems: • Autodesk Inventor (p. 870) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 869 Features • CATIA V5 (p. 870) • Creo Parametric (formerly Pro/ENGINEER) (p. 870) • NX (p. 870) • Solid Edge (p. 870) • SolidWorks (p. 871) Autodesk Inventor After a part is open in Inventor, click Tools> Parameters. In the Parameters dialog box, click a parameter name under the Parameter Name column, modify the parameter name to include ds at either the beginning or end of the name and click Enter. Click Done to close the Parameters dialog box. For detailed information, see CAD Integration. CATIA V5 After a part is open in CATIA V5, click Tools> Formula. In the Formulas dialog box, select the desired parameter in the scrolling list. In the "Edit name or value of the current parameter" field, modify the parameter name to include ds at either the beginning or end of the name, then click OK or Apply. For detailed information, see CATIA V5 Associative Geometry Interface (*.CATPart, *.CATProduct) in the CAD Integration section of the product help. Creo Parametric (formerly Pro/ENGINEER) In Creo Parametric, modify the parameter name by selecting the feature it belongs to, right click on Edit. Creo Parametric will then display all dimensions (parameters) for the selected feature. If the model shows numeric values, then select Info> SwitchDims so that the names are text based instead of numeric. Next, select the dimension/parameter you wish to rename, it will turn red when selected. Then hold down right click until a menu appears and there select Properties. The Dimension Properties dialog box will appear, select the Dimension Text tab. Here you can give the dimension a new name, also be sure to change the @D to @S (case sensitive) before completing the modification by clicking OK. For detailed information, see Creo Parametric (formerly Pro/ENGINEER) Associative Geometry Interface (*.prt, *.asm) in the CAD Integration section of the product help. NX After a model is opened in NX, click Application> Modeling and the Tools> Expression In the Edit Expressions dialog box, select the expression with the variable name that you want to rename and click Rename. Change the expression name in the Rename Variable dialog box to include ds at either the beginning or end of the name and click OK. Click OK/Apply to close the Edit Expressions dialog box. For detailed information, see NX in the CAD Integration section of the product help. Solid Edge After a model is opened in Solid Edge, click Tools> Variables... If the dimensions (type Dim) are not shown in the Variable Table dialog box, click the Filter button for the Filter dialog box. Highlight both Dimensions and User Variables under the Type column; select Both under the Named By 870 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment column and select File under the Graphics in column. Then click OK. Click the name of a dimension (under the Name column), modify the dimension name to include ds at either the beginning or end of the name and click Enter. Close the Variable Table dialog box. For detailed information, see Solid Edge in the CAD Integration section of the product help. SolidWorks In SolidWorks, open the part and then click on the part or on the feature in the tree. Then right-click the dimension on the model, open the Properties dialog box, and edit the name of the dimension. For detailed information, see SolidWorks in the CAD Integration section of the product help. Design Assessment The Design Assessment system provides further options to quantitatively examine the results from other Mechanical systems by supporting built-in operations, as well as facilities to perform custom computations on the data. For example, a Design Assessment system could be used to obtain solution combinations, to verify a design in relation to a particular standard (e.g. for BEAMCHECK and FATJACK), or to perform custom calculation processes (e.g. fragmentation analyses, calling a third-party program to process results data, or running a Mechanical APDL post processing session). User Workflow It is useful to understand the user workflow in a Design Assessment system in order to customize its calculation process. A key step in the workflow is to select the Mechanical system whose results will be examined. This is accomplished using the Solution Selection object. Once specified, there are three considerations that affect the outcome of the calculation process (and can thus be customized): • what inputs are required • what scripts should run • how results should be displayed The user feeds inputs into the Design Assessment system via one or more Attribute Group objects. The scripts are the workhorse for computation. They are programmed in the Python scripting language and have access, at runtime, to all relevant data in the model, including any inputs collected from the user, along with the mesh and upstream results, through an Application Programmable Interface (API). The user defines result requests using the DA Result object to prescribe what quantities to plot and where on the model. Customization With the exception of Solution Combinations, predefined assessment types such as FATJACK and BEAMST feature Attribute Groups, Scripts, and Result Objects, and can be used as the basis for customization. These three components of the calculation process must be described in the XML Definition File before they can be featured in a Design Assessment system. Collectively, the inputs for the process are described in the AttributeGroups section of the Definition File. Each input is controlled by an individual Attribute indicating the type of data to gather from the user, its scope of application on the model, and its validation, among other details. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 871 Features The scripts are prescribed in the DAScripts section of the XML Definition File and are the workhorse for computation. Distinct scripts for "Solve" and for "Evaluating Results" are possible to respond to the respective user operations in the Mechanical editor. Example snippets are provided for each class in the scripting API, along with full worked examples in this documentation. There is a section on Developing and Debugging Scripts for more operation details. The display of results is configured in the Results section of the XML Definition File. Individual Attributes are also used here to collect inputs from the user that can be accessed in the script to control what is to be plotted. Once configured, the XML Definition File is imported into Design Assessment as a User Defined type, distinct from all the predefined ones mentioned, and is ready to be used as a custom calculation process. For details, please see the section below on configuring the assessment type. Design Assessment Types Design Assessment systems offer three predefined types and a user define type (for customization). The predefined types are: • Solution Combination • BEAMCHECK • FATJACK To configure a particular Design Assessment system, you may: • Setup cell Right Mouse Button Menu Right click on the Setup cell for the system in the Project Schematic and select Assessment Type. Here you can select one of the pre-defined types, or a user defined type. For user defined types, you could provide the XML Definition File from an Open File dialog or a listing of recent files (if available). To identify the selected assessment type, look for a checkmark next to the pre-defined type on the menu. Absence of a checkmark means a user defined type is in effect. or • Setup Cell Properties Panel Select View > Properties from the Main Menu in the Project Schematic. This will display the Properties Panel in the workspace. Now click on the Setup cell of the Design Assessment system and the Properties Panel will be updated to show the available options for the cell. From here you can change the Assessment Type using the drop-down list in the Design Assessment Settings section. You can choose between the predefined types or select User Defined. For user defined types, you can provide the XML Definition File from an Open File dialog or a listing of recent files (if available). The name of this file will then be displayed in the properties panel. For User Defined assessment types, the XML Definition File will automatically be copied to your project folder upon selection, to keep as a reference. If you subsequently edit your XML Definition File and want the changes to be used in a project, it will need to be re-selected. At this stage the differences 872 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment between the original and the revised XML Definition File will be detected and any defined objects will be updated as detailed in Changing the Assessment Type or XML Definition File Contents (p. 910) Note If you Import a Mechanical database (e.g., a .mechdat file) containing a Design Assessment system you must reselect the Assessment Type (and associated XML definition file for the User Defined type) before opening the project in the Mechanical application. Otherwise, your assessment type will revert to Solution Combination Only and any Design Assessment objects will be lost. The following sections describe the use of the Design Assessment system. Predefined Assessment Types Changing the Assessment Type or XML Definition File Contents Solution Selection Using the Attribute Group Object Developing and Debugging Design Assessment Scripts Using the DA Result Object The Design Assessment XML Definition File Design Assessment API Reference Examples of Design Assessment Usage Predefined Assessment Types The following predefined Assessment Types can be selected as described previously after you add a Design Assessment system to the Project Schematic. Solution Combination Only Enables solution combinations of upstream results using the Solution Selection object. Mechanical results can be added to the system but no DA Results objects will be available. BEAMCHECK (Beam and Joint Strength) Enables solution combinations of upstream results and post processing with BEAMST. BEAMST performs various regulatory authority based code of practice checks for the ultimate limit state assessment of Beam or Tubular elements. Mechanical results and DA Results objects are available. FATJACK (Beam Joint Fatigue) Enables solution selection of upstream results and post processing with FATJACK. FATJACK (FATigue calculations for offshore JACKets) performs fatigue analysis at the joints of Beam / Tubular based elements for fatigue/service limit state assessment. No Mechanical results are available but DA Results objects can be added to the system. The following sections describe the use of the predefined Assessment Types in the Design Assessment system. Modifying the Predefined Assessment Types Menu Using BEAMST and FATJACK with Design Assessment Using BEAMST with the Design Assessment System Using FATJACK with the Design Assessment System Modifying the Predefined Assessment Types Menu The menu of predefined assessment types can be controlled by editing the AttributeTemplate.xml file in the {ANSYS Installation}\v140\Addins\Simulation folder. This file defines what entries appear in the menu when it is selected, along with the order of the entries and the default entry. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 873 Features The User Defined entry is always shown on the Assessment Type menu in addition to the predefined assessment types. An Example Menu Definition File The following example defines the standard entries on the Assessment Type menu: <?xml version="1.0" encoding="utf-8" standalone="no"?> <AttributeTemplates> <AttributeList> <Attribute> <Name>FATJACK (Beam Joint Fatigue)</Name> <File>DA_FATJACK.xml</File> <Priority>1.1</Priority> <ValidOn>Windows</ValidOn> </Attribute> <Attribute> <Name>BEAMCHECK (Beam and Joint Strength)</Name> <File>DA_BEAMST.xml</File> <Priority>1.2</Priority> <ValidOn>Windows</ValidOn> </Attribute> <Attribute> <Default>true</Default> <Name>Solution Combination Only</Name> <File>DA_SolutionCombinations.xml</File> <Priority>1.5</Priority> <ValidOn>Windows,Linux</ValidOn> </Attribute> </AttributeList> </AttributeTemplates> Defining the Menu Entries Each menu entry is defined using an Attribute XML block. The following tags can be defined in the <Attribute></Attribute> block. Name: The name that the user will see in the menu. File: The XML definition file that is passed to Mechanical. If the full path to the file is omitted, the location is assumed to be in the {ANSYS Installation}\v140\aisol\DesignSpace\DSPages\xml folder. Priority: The position in the menu, entered as 1.1 - 1.xxx. Default: Specifies which entry is the default. Include this tag with a value of true for the entry that is to be the default option (omit it for other entries). ValidOn: Specifies which platforms are supported for the entry. Available options are Windows and Linux. To specify both platforms, separate entries with a comma (Windows,Linux). Using BEAMST and FATJACK with Design Assessment The Design Assessment system provides for the selection of Attribute Group objects to define the input data to FATJACK and BEAMST. In addition, DA Result objects can be added to the Solution to define which results to obtain and display. Workbench and Design Assessment are geometry based, which means that areas of the geometry are selected rather than individual elements. With the Mechanical solver, a member ought to be meshed and formed of a number of elements. Results can be added to the Solution in the Design Assessment system and displayed in Workbench; these will contour the maximum value that occurs for each element. Results can be added either before 874 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment or after the analysis. If additional results are added after the analysis has been performed, then evaluating the results will obtain the values from the existing database, if the result type exists. Elements that do not have results will be shown as semi transparent. Using BEAMST with the Design Assessment System The ability to perform code checking has been incorporated into Workbench using the Design Assessment System. This system can be connected to both Static Structural and Transient Structural systems. The structural analysis needs to be performed using the Mechanical solver. The following sections describe how to setup a BEAMST analysis in the Design Assessment system. Introduction Information for Existing ASAS Users Attribute Group Types Available Results Introduction The Design Assessment system enables the input of Attribute Group objects to define the input data to BEAMST and DA Result objects to define which results to obtain and present. Workbench and Design Assessment are geometry based, which means that areas of the geometry are selected rather than individual elements. With the Mechanical solver, a member ought to be meshed and formed of a number of elements, the Design Assessment, BEAMST implementation automatically sets the unbraced lengths as the distance between the end vertices of the member to account for this. Results can be added to the Solution in the Design Assessment system and displayed in Workbench; these will contour the maximum value that occurs for each element. Results can be added either before or after the analysis, if further results are added after the analysis has been performed then evaluating the results will obtain the values from the existing database, if the result type exists. Elements that do not have results will be semi transparent. Reports can be produced of the input data and the results can be parameterized and exposed for use with other systems. Information for Existing ASAS Users BEAMST Command Attribute Group Type Attribute Group Subtype Requirement ABNO Load Dependant Factors Load Classification API LRFD Only AISC Code of Practise Selection AISC WSD Checks * AISC LRFD Checks API Code of Practise Selection API WSD Checks * API LRFD Checks BRIG Ocean Environment Buoyancy Calculation Method BS59 Code of Practise Selection BS5950 Checks CASE Not supported, Load case selection is via the Solution Selection Object CB Load Dependant Factors Bending Coefficient CHOR Geometry Definition Manually Define Chords Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. * 875 Features BEAMST Command Attribute Group Type Attribute Group Subtype Requirement Define Chord Thickening at Joint Automatic Joint Identification CMBV Not Supported, only linear static combinations are permitted. CMY Load Dependant Factors Amplification Reduction Factor CMY CMZ Load Dependant Factors Amplification Reduction Factor CMZ COMB Automatically determined from the Solution Selection Object DESI Automatically determined from the geometry. DENT Geometry Definition Dented Member Profile ISO Only DS44 Code of Practise Selection DS449 / DS412 Checks * EFFE Geometry Definition Effective Lengths ELEM Code of Practise Selection As selected for the appropriate code of practice ELEV Ocean Environment Water Details EXTR Load Dependant Factors Safety Factor Definition GAPD Geometry Definition Default Gap/Eccentricity GRAV Automatic from units, assumed water surface is in global XY plane. GROU Not Supported HYDR Load Dependant Factors Safety Factor Definition ISO Code of Practise Selection ISO Checks JOIN Code of Practise Selection As selected for the appropriate code of practice LIMI Not Supported MCOF Material Definition Partial Material Coefficient (NPD, NORSOK, DS449 only) MFAC Load Dependant Factors Moment Reduction Factors MLTF Load Dependant Factors LTB Moment Reduction Factor MOVE Not Supported NORS Code of Practise Selection NORSOK Checks * NPD Code of Practise Selection NPD Checks * PHI Load Dependant Factors PHI Coefficient POST Not Supported PRIN Not Supported PROF Not Supported QuAK Load Dependant Factors RENU Not Supported SAFE Load Dependant Factors SEAR Not Supported 876 Safety Factor Definition Safety Factor Definition Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment BEAMST Command Attribute Group Type Attribute Group Subtype SECO Code of Practise Selection As selected for the appropriate code of practice SECT Not Supported SELE Not Supported SIMP Code of Practise Selection SPEC Not Supported STUB Not Supported TITL Not Supported TYPE Geometry Definition Requirement BS5950 Checks Joint Types Default Joint Types ULCF Geometry Definition Unbraced Compression Flange Length Unbraced Compression Flange Length (Factor) UNBR Geometry Definition Unbraced Length Unbraced Length (Factor) UNIT Automatically determined from analysis, selections for N mm, pdl ft, pdl in and N m are supported. WAVE Ocean Environment Wave Definition YIEL YIEL Material Definition Yield Definition Compulsory * At least one of these entries is required. Attribute Group Types Attribute Groups enable the entry of the data that is associated with the BEAMST analysis. The following sections describe the available Attribute Group Types and their subtypes. Code of Practise Selection General Text Geometry Definition Load Dependant Factors Material Definition Ocean Environment Note If units are changed when defining data for Attributes, then the resulting data sent to the processing script may be incorrect. It is recommended that units are not modified from those used in creating the geometry. Code of Practise Selection All groups that have this type enable the selection of a particular code of practice. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 877 Features Note If a specific code check version is set to Not Checked for a given code of practice, it is still necessary to make a geometry selection for that Attribute. • API WSD Checks Enables the selection of the API WSD code of practice and the appropriate edition. Use this to select the joints and members to be included in the check. Any members that are not selected will be excluded from the checks. Allowable Stress, Hydrostatic Checks and Joint check clauses will be included as appropriate for the edition chosen. • API LRFD Checks Enables the selection of the API LRFD code of practice and the appropriate edition. Use this to select the joints and members to be included in the check. Any members that are not selected will be excluded from the checks. Allowable Stress Checks, Hydrostatic Checks and Joint check clauses will be included as appropriate for the edition chosen. • AISC WSD Checks Enables the selection of the AISC WSD code of practice and the appropriate edition. Use this to select the members to be included in the check. Any members that are not selected will be excluded from the checks. Allowable Stress Checks clauses will be included as appropriate for the edition chosen. • AISC LRFD Checks Enables the selection of the AISC LRFD code of practice and the appropriate edition. Use this to select the members to be included in the check. Any members that are not selected will be excluded from the checks. Member Checks clauses will be included as appropriate for the edition chosen. • BS5950 Checks Enables the selection of the BS5950 code of practice and the appropriate edition. Use this to select the members to be included in the check. Any members that are not selected will be excluded from the checks. Member Checks clauses will be included as appropriate for the edition chosen. Members that only need the simplified checks can also be selected • DS449 / DS412 Checks Enables the selection of the DS code of practice and the appropriate edition. Use this to select the joints and members to be included in the check. Any members that are not selected will be excluded from the checks. Allowable Stress and Joint check clauses will be included as appropriate for the edition chosen. • 878 ISO Checks Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Enables the selection of the ISO code of practice and the appropriate edition. Use this to select the joints and members to be included in the check. Any members that are not selected will be excluded from the checks. Member, Hydrostatic Checks and Joint check clauses will be included as appropriate for the edition chosen. • NORSOK Checks Enables the selection of the NORSOK code of practice and the appropriate edition. Use this to select the joints and members to be included in the check. Any members that are not selected will be excluded from the checks. Member, Hydrostatic Checks and Joint check clauses will be included as appropriate for the edition chosen. • NPD Checks Enables the selection of the NPD code of practice and the appropriate edition. Use this to select the joints and members to be included in the check. Any members that are not selected will be excluded from the checks. Member and Joint check clauses will be included as appropriate for the edition chosen. General Text This can be used to supply additional and non-supported commands. This will always override data set by other tree objects. • Geometry Independent Enables additional commands to be entered, these will be appended to the end of all code checks. Geometry Definition All groups that have this type enable the selection of a particular code of practice. • Manually Define Chords The chord member(s) and the central vertex can be chosen to define which members at a joint form the chords. Without this definition, chords are automatically determined. Chords for each Joint needs to be defined separately. Only applicable to joint checks. • Automatic Joint Identification Enables the identification of joints formed of more than one node by the ratio of the distance between nodes to the diameter of the member. All joints can be selected at once. Only applicable to joint checks. • Define Chord Thickening at Joint Enables the entry of chord thickening at the selected joints. Only applicable to joint checks. • Effective Lengths Enables the definition of effective length factor k for the selected members to be entered for both the local y and z directions. Applicable for member strength based checks only. • Unbraced Compression Flange Length Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 879 Features Enables the definition of the unbraced compression flange length. If this and the factor version are omitted then the direct distance between vertices which do not have 2 lines joining is taken. • Unbraced Length Enables the definition of the unbraced length. If this and the factor version are omitted then the direct distance between vertices which do not have 2 lines joining is taken. • Joint Types Enables default joint type to be over-ridden. • Default Gap/Eccentricity Enables default gap or eccentricity to be overridden. • Dented Member Profile Enables the definition of dents and imperfections in the straightness of the member to be defined for the ISO code of practice • Unbraced Compression Flange Length (Factor) Enables the definition of the compression flange length. The factor is applied to the distance between vertices which do not have 2 lines joining is taken and is converted to a length. If undefined (and not over-ridden by the direct entry), a factor of 1 is applied to all elements forming the line • Unbraced Length (Factor) Enables the definition of the unbraced length. The factor is applied to the distance between vertices which do not have 2 lines joining is taken and is converted to a length. If undefined (and not overridden by the direct entry), a factor of 1 is applied to all elements forming the line Load Dependant Factors All groups that have this type enable the entry of values that are dependent on. • Safety Factor Definition Use this to define if the loading scenario is considered to be an earthQuake/seismic or extreme load, for which the safety factors can be reduced, alternatively, custom values can be added. Additionally the Hydrostatic pressure load factor can be defined for hydrostatic checks. • Load Classification Enables the identification of abnormal load scenarios. Only applies to the API LRFD code of practice. • Bending Coefficient Enables the definition of the pure coefficient of bending, Cb and selection of the members to which it applies. In absence of application of a user value it is calculated automatically. Only applies to the AISC and API allowable stress checks. • PHI Coefficient Enables the specification of the parameter Φ, used in the determination of the lateral buckling strength of beams for NS3472E, this value can either be automatically determined or manually over-ridden. Only applied to the NPD checks. • 880 LTB Moment Reduction Factor Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Enables the definition and application of MLTB, the moment reduction factor for lateral torsional buckling. Only applicable to BS5950 • Amplification Reduction Factor CMY Enables the definition and application of the factor Cmy, the amplification reduction factor. Only applies to AISC & API Allowable stress checks. • Amplification Reduction Factor CMZ Enables the definition and application of the factor Cmz, the amplification reduction factor. Only applies to AISC & API Allowable stress checks • Moment Reduction Factors Enables the definition and application of the My and Mz factors, the moment reduction factors. Only applies to BS5950 checks. Material Definition All groups that have this type enable the selection of a particular code of practice. • Partial Material Coefficients Enables the definition of the partial material coefficients utilised in the NPD, NORSOK and DS449 codes • Yield Definition Definition of the yield stress, must have a value applied for each member in the analysis. Required for all code checks Ocean Environment All groups that have this type enable the selection of a particular code of practice. • Water Details Enables the elevation of the mean water level, sea bed to be defined in global Z. Water density and tide/surge heights can also be entered. Required for all code checks involving hydrostatic analysis. Note The global X/Y plane is coincident with the horizontal mean sea level, with global Z vertically upwards (away from the mudline). • Buoyancy Calculation Method By default rigorous buoyancy is enabled for compatibility with the Mechanical analysis methods. If necessary, this methodology can be disabled for the code check. • Wave Definition Used to specify the wave height and period for the calculation for wave induced hydrostatic pressure head calculations. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 881 Features Available Results The following results are available for the Code of Practice types as indicated below. Results are added using the DA Results tree object. AISC LRFD Results AISC WSD Results API LRFD Results API WSD Results BS5950 Results DS449 High Results DS449 Normal Results ISO Results NORSOK Results NPD Results As each result object presents a number of types of results, units are not employed in the output. Hence all values will be reported in the solver units used for the BEAMST analysis. AISC LRFD Results Two Results subtypes are available for this code of practice. The results available for those subtypes are shown below. Member Unity Checks • Axial • Y Shear • Z Shear • Y Bending • Z Bending • Buckling CSR • Yield Member General Results • Y Amplification Reduction Factor • Z Amplification Reduction Factor • Allowable Axial Stress • Critical Stress • Allowable Y Euler Buckling Stress • Allowable Z Euler Buckling Stress • Allowable Y Shear Stress • Allowable Z Shear Stress • Allowable Y Bending Stress • Allowable Z Bending Stress 882 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment AISC WSD Results Two Results subtypes are available for this code of practice. The results available for those subtypes are shown below. Member Unity Check • Axial • Y Shear • Z Shear • Y Bending • Z Bending • Maximum Shear • Buckling • Buckling CSR • Yield Member General Results • Y Amplification Reduction Factor • Z Amplification Reduction Factor • Allowable Axial Stress • Allowable Shear Stress • Allowable Y Bending Stress • Allowable Z Bending Stress API LRFD Results Six Results subtypes are available for this code of practice. The results available for those subtypes are shown below. Member Unity Checks • Axial • Shear • Torsion • Y Bending • Z Bending • Resultant Bending • Buckling • Buckling CSR • Yield 1 • Yield 2 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 883 Features Hydrostatic Unity Checks • Axial • Hoop • Yield • Buckling • Combined Joint Unity Check • Axial • In-Plane Bending • Out-of-Plane Bending • Bending • Combined Axial + Bending • Joint Strength Hydrostatic General Results • Hydrostatic Depth • Hydrostatic Pressure Load Factor • Geometry Parameter • Hoop Buckling Coefficient • Hoop Stress • Allowable Axial Stress • Allowable Bending Stress • Allowable Elastic Axial Stress • Allowable Elastic Hoop Stress • Allowable Inelastic Axial Stress • Allowable Inelastic Hoop Stress Joint General Results • Proportion of Joint 1 • Proportion of Joint 2 • Gap • Beta Ratio • Tau Ratio • Theta Angle • Chord Stress • Chord Yield Stress • Brace Yield Stress 884 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment • Brace Axial Stress • In-Plane Brace Bending Stress • Out-of-Plane Brace Bending Stress • Axial Qf Factor • In-Plane Qf Factor • Out-of-Plane Qf Factor • Axial Qu Factor Brace 1 • In-Plane Bending Qu Factor Brace 1 • Out-of-Plane Bending Qu Factor Brace 1 • Axial Qu Factor Brace 2 • In-Plane Bending Qu Factor Brace 2 • Out-of-Plane Bending Qu Factor Brace 2 • Axial Force • In-Plane Bending Force • Out-of-Plane Bending Force • Allowable Axial Force Brace 1 • Allowable In-Plane Bending Force Brace 1 • Allowable Out-of-Plane Bending Force Brace 1 • Allowable Axial Force Brace 2 • Allowable In-Plane Bending Force Brace 2 • Allowable Out-of-Plane Bending Force Brace 2 • Allowable Cross Chord Force Member General Results • Y Amplification Reduction Factor • Z Amplification Reduction Factor • Column Slenderness Parameter • Allowable Axial Stress • Allowable Shear Stress • Allowable Torsion Stress • Allowable Bending Stress • Allowable Y Euler Buckling Stress • Allowable Z Euler Buckling Stress • Yield Stress • Buckling Stress Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 885 Features API WSD Results Eleven Results subtypes are available for this code of practice. The results available for those subtypes are shown below. Member Unity Checks • Axial • Y Shear (not TUBE - Ed17+) • Z Shear (not TUBE - Ed17+) • Y Bending • Z Bending • Buckling • Buckling CSR • Yield • Maximum Shear (TUBE - Ed13 Only) • Flexural Shear (TUBE - Ed17+) • Torsional Shear (TUBE - Ed17+) • Resultant Bending (TUBE - Ed17+) Hydrostatic Unity Checks • Axial Tension • Hoop • Combined 1 • Combined 2 • Combined T Joint (Punching) Unity Checks • Axial • In-Plane Bending • Out-of-Plane Bending • Bending • Combined Axial + Bending • Joint Strength Joint (Nominal) Unity Checks • Axial • In-Plane Bending • Out-of-Plane Bending • Bending • Combined Axial + Bending 886 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment • Joint Strength Joint Unity Checks • Axial • In-Plane Bending • Out-of-Plane Bending • Combined Axial + Bending Hydrostatic General Results • Hydrostatic Depth • Hoop Stress • Allowable Axial Tension Stress • Allowable Elastic Axial Stress • Allowable Elastic Hoop Stress • Allowable Inelastic Axial Stress • Allowable Inelastic Hoop Stress Joint (Nominal) General Results • Gap • Beta Ratio • Tau Ratio • Theta Angle • Chord Stress • Chord Yield • AISC Allowable Punching Shear Stress • Brace Axial Stress • In-Plane Brace Bending Stress • Out-of-Plane Brace Bending Stress • Axial Qf Factor • In-Plane Qf Factor • Out-of-Plane Qf Factor • Axial Qu Factor Brace 1 • In-Plane Bending Qu Factor Brace 1 • Out-of-Plane Bending Qu Factor Brace 1 • Axial Qu Factor Brace 2 • In-Plane Bending Qu Factor Brace 2 • Out-of-Plane Bending Qu Factor Brace 2 • Axial Force Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 887 Features • In-Plane Bending Force • Out-of-Plane Bending Force • Allowable Axial Force Brace 1 • Allowable In-Plane Bending Force Brace 1 • Allowable Out-of-Plane Bending Force Brace 1 • Allowable Axial Force Brace 2 • Allowable In-Plane Bending Force Brace 2 • Allowable Out-of-Plane Bending Force Brace 2 Joint General Results • Allowable Pa • Allowable Ma In-Plane • Allowable Ma Out-of-Plane • Beta Ratio • Gamma Ratio • Tau Ratio • Theta Angle • 1st Chord Member • Chord Axial Force • Chord Moment In-Plane • Chord Moment Out-of-Plane • Chord Capacity • Chord Strength • Brace Axial Force • Brace Moment In-Plane • Brace Moment Out-of-Plane • Joint Proportion (%) 1 • Joint Proportion (%) 2 • Joint Proportion (%) 3 • Joint Proportion (%) 4 • Joint Proportion (%) 5 • Axial Qu Factor 1 • Axial Qu Factor 2 • Axial Qu Factor 3 • Axial Qu Factor 4 • Axial Qu Factor 5 • Axial Qf Factor 1 • Axial Qf Factor 2 888 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment • Axial Qf Factor 3 • Axial Qf Factor 4 • Axial Qf Factor 5 • Gap Factor 1 • Gap Factor 2 • Gap Factor 3 • Gap Factor 4 • Gap Factor 5 • Qu Factor - In-Plane • Qu Factor - Out-of-Plane • Qf Factor Joint (Punching) Results • Proportion of Joint 1 • Proportion of Joint 2 • Gap • Beta Ratio • Tau Ratio • Theta Angle • Chord Stress • Chord Yeild • AISC Allowable Punching Shear Stress • Brace Axial Stress • In-Plane Brace Bending Stress • Out-of-Plane Brace Bending Stress • Axial Qf Factor • In-Plane Qf Factor • Out-of-Plane Qf Factor • Axial Qq Factor Brace 1 • In-Plane Bending Qq Factor Brace 1 • Out-of-Plane Bending Qq Factor Brace 1 • Axial Qq Factor Brace 2 • In-Plane Bending Qq Factor Brace 2 • Out-of-Plane Bending Qq Factor Brace 2 • Axial Stress • In-Plane Bending Stress • Out-of-Plane Bending Stress • Allowable Axial Stress Brace 1 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 889 Features • Allowable In-Plane Bending Stress Brace 1 • Allowable Out-of-Plane Bending Stress Brace 1 • Allowable Axial Stress Brace 2 • Allowable In-Plane Bending Stress Brace 2 • Allowable Out-of-Plane Bending Stress Brace 2 Member General Results • Y Amplification Reduction Factor • Z Amplification Reduction Factor • Critical Buckling (Bending) • Allowable Axial Stress • Allowable Shear Stress • Allowable Y Bending Stress (Not TUBE Ed17 On) • Allowable Z Bending Stress (Not TUBE Ed17 On) • Allowable Torsion Stress (TUBE Ed17 On) • Allowable Bending Stress (TUBE Ed17 On) Spectral Results • Y Amplification Reduction Factor • Z Amplification Reduction Factor • Allowable Axial Stress • Allowable Y Bending Stress (Not TUBE Ed16 On) • Allowable Z Bending Stress (Not TUBE Ed16 On) • Allowable Euler Buckling Stress Y • Allowable Euler Buckling Stress Z • Maximum Axial Stress • Maximum Y Bending Stress • Maximum Z Bending Stress BS5950 Results Two Results subtypes are available for this code of practice. The results available for those subtypes are shown below. Member Unity Checks • Major Axis Bending • Minor Axis Bending • Major Axis Shear • Minor Axis Shear • Axial Tension 890 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment • Combined Axial + Moment • Minor Axis Buckling • Major Axis Buckling • Lateral Torsional Buckling • Overall Buckling Member General Results • Axial Force Capacity • Major Axis Shear Force Capacity • Minor Axis Shear Force Capacity • Major Axis Bending Moment Capacity • Minor Axis Bending Moment Capacity • Reduced Moment Capacity - Major Axis • Reduced Moment Capacity - Minor Axis • Member Compressive Capacity - Minor Axis Buckling • Member Compressive Capacity - Major Axis Buckling • Member Moment Capacity - Lateral Torsional Buckling DS449 High Results Four Results subtypes are available for this code of practice. The results available for those subtypes are shown below. Member Unity Checks • Von Mises • Shear • Local Buckling • Y Total Buckling • Z Total Buckling • Hydrostatic Overpressure • Combined Local + Hydrostatic Joint (Nominal) Unity Check • Axial • In-Plane Bending • Out-of-Plane Bending • Bending • Combined Axial + Bending Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 891 Features Member General Results • Von Mises Stress • Hoop Stress (H) • Hydrostatic Pressure (H) • Relative Slenderness Ratio For Local Buckling • Critical Stress For Local Buckling • Critical Stress For Hydrostatic Overpressure (H) • Critical Stress For Combined Case (H) • Critical Pressure (H) • Maximum Axial Force • Y Equivalent Design Moment • Z Equivalent Design Moment • Y Euler Buckling Force • Z Euler Buckling Force • Y Relative Slenderness Ratio • Z Relative Slenderness Ratio • Y Equivalent Geometric/Material Imperfections • Z Equivalent Geometric/Material Imperfections • Critical Stress Joint General Results • Proportion of Joint 1 • Proportion of Joint 2 • Gap • Beta Ratio • Tau Ratio • Theta Angle • Gamma Ratio • Chord Stress • Chord Yield Stress • Chord Wall Shear Limit • Brace Axial Stress • Brace In-Plane Bending Stress • Brace Out-of-Plane Bending Stress • Axial UU Factor • In-Plane UU Factor • Out-of-Plane UU Factor 892 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment • Axial Ten/Comp CC Factor For Brace 1 • In-Plane Bending CC Factor For Brace 1 • Out-of-Plane Bending CC Factor For Brace 1 • Axial Ten/Comp CC Factor For Brace 2 • In-Plane Bending CC Factor For Brace 2 • Out-of-Plane CC Factor For Bending Brace 2 • Axial Nominal Load • In-Plane Bending Moment • Out-of-Plane Bending Moment • Axial Capacity Brace 1 • In-Plane Bending Capacity Brace 1 • Out-of-Plane Bending Capacity Brace 1 • Axial Capacity Brace 2 • In-Plane Bending Capacity Brace 2 • Out-of-Plane Bending Capacity Brace 2 DS449 Normal Results Two Results subtypes are available for this code of practice. The results available for those subtypes are shown below. Member Unity Checks • Von Mises • Shear • Local Buckling • Y Total Buckling • Z Total Buckling • Hydrostatic Overpressure • Combined Local + Hydrostatic Member General Results • Von Mises Stress • Hoop Stress (H) • Hydrostatic Pressure (H) • Relative Slenderness Ratio For Local Buckling • Critical Stress For Local Buckling • Critical Stress For Hydrostatic Overpressure (H) • Critical Stress For Combined Case (H) • Critical Pressure (H) • Maximum Axial Force Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 893 Features • Y Equivalent Design Moment • Z Equivalent Design Moment • Y Euler Buckling Force • Z Euler Buckling Force • Y Relative Slenderness Ratio • Z Relative Slenderness Ratio • Y Equivalent Geometric/Material Imperfections • Z Equivalent Geometric/Material Imperfections • Critical Stress ISO Results Six Results subtypes are available for this code of practice. The results available for those subtypes are shown below. Member Unity Checks • Axial • Shear • Torsion • Y Bending • Z Bending • Resultant Bending • Yield 1 • Yield 2 Hydrostatic Unity Checks • Hoop Compressive • Combined Hoop + Axial • Combined Hoop Bending + Axial 1 • Combined Hoop Bending + Axial 2 • Combined Joint Unity Check • Axial • In-Plane Bending • Out-of-Plane Bending • Combined Axial + Bending Member General Results • 894 Y Moment Amplification Reduction Factor Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment • Z Moment Amplification Reduction Factor • Column Slenderness Parameter • Allowable Axial Stress • Allowable Shear Stress • Allowable Torsion Stress • Allowable Y Bending Stress • Allowable Z Bending Stress • Allowable Y Euler Buckling Stress • Allowable Z Euler Buckling Stress • Allowable Local Buckling Stress Hydrostatic General Results • Section Position • Hydrostatic Depth • Hydrostatic Load Factor • Geometry Parameter • Hoop Buckling Coefficient • Hoop Stress • Allowable Axial Stress • Allowable Bending Stress • Allowable Elastic Axial Stress • Allowable Inelastic Axial Stress • Allowable Elastic Hoop Stress • Allowable Inelastic Hoop Stress Joint General Results • Allowable Pa • Allowable Ma In-Plane • Allowable Ma Out-of-Plane • Beta Ratio • Gamma Ratio • Tau Ratio • Theta Angle • Chord Axial Force • Chord Moment In-Plane • Chord Moment Out-of-Plane • Chord Capacity • Chord Strength Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 895 Features • Brace Axial Force • Brace Moment In-Plane • Brace Moment Out-of-Plane • Joint Proportion (%) 1 • Joint Proportion (%) 2 • Joint Proportion (%) 3 • Joint Proportion (%) 4 • Joint Proportion (%) 5 • Axial Qu Factor 1 • Axial Qu Factor 2 • Axial Qu Factor 3 • Axial Qu Factor 4 • Axial Qu Factor 5 • Axial Qf Factor 1 • Axial Qf Factor 2 • Axial Qf Factor 3 • Axial Qf Factor 4 • Axial Qf Factor 5 • Gap Factor 1 • Gap Factor 2 • Gap Factor 3 • Gap Factor 4 • Gap Factor 5 • Qu Factor - In Plane • Qu Factor - Out Of Plane • Qf Factor - In Plane • Qf Factor - Out Of Plane NORSOK Results Six Results subtypes are available for this code of practice. The results available for those subtypes are shown below. Member Unity Checks • Axial • Shear • Torsion • Y Bending • Z Bending 896 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment • Resultant Bending • Bending + Shear • Shear + Bending + Torsion • Yield 1 • Yield 2 Hydrostatic Unity Checks • Hoop Compressive • Combined Hoop + Axial • Combined Hoop Bending + Axial 1 • Combined Hoop Bending + Axial 2 • Combined Joint Unity Check • Axial • In-Plane Bending • Out-of-Plane Bending • Combined Axial + Bending Member General Results • Y Moment Amplification Reduction Factor • Z Moment Amplification Reduction Factor • Chord Diameter • Chord Thickness • Column Slenderness Parameter • Allowable Axial Stress • Allowable Shear Stress • Allowable Torsion Stress • Allowable Bending Stress • Allowable Y Euler Buckling Stress • Allowable Z Euler Buckling Stress • Allowable Yield Hydrostatic General Results • Hydrostatic Depth • Geometry Parameter • Hoop Buckling Coefficient • Hoop Stress • Allowable Axial Stress Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 897 Features • Allowable Bending Stress • Allowable Elastic Axial Stress • Allowable Inelastic Axial Stress • Allowable Elastic Hoop Stress • Allowable Inelastic Hoop Stress Joint (Nominal) General Results • Gap • Beta Ratio • Tau Ratio • Theta Angle • Chord Stress • Chord Yield Stress • Brace Yield Stress • Brace Axial Stress • In-Plane Brace Bending Stress • Out-of-Plane Brace Bending Stress • Axial Qf Factor • In-Plane Bending Qf Factor • Out-of-Plane Bending Qf Factor • Axial Qu Factor Brace 1 • In-Plane Bending Qu Factor Brace 1 • Out-of-Plane Bending Qu Factor Brace 1 • Axial Qu Factor Brace 2 • In-Plane Bending Qu Factor Brace 2 • Out-of-Plane Bending Qu Factor Brace 2 • Axial Force • In-Plane Bending Force • Out-of-Plane Bending Force • Allowable Axial Force Brace 1 • Allowable In-Plane Bending Moment Brace 1 • Allowable Out-of-Plane Bending Moment Brace 1 • Allowable Axial Force Brace 2 • Allowable In-Plane Bending Moment Brace 2 • Allowable Out-of-Plane Bending Moment Brace 2 • Chord Effective Length 898 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment NPD Results Nine Results subtypes are available for this code of practice. The results available for those subtypes are shown below. Member Unity Checks (1984) • Axial • Bending (TUBE) • Lateral Pressure (TUBE) • Torsional Shear (TUBE) • Bending Shear (TUBE) • Von Mises • Axial + Bending Combined (TUBE) • Axial + Lateral Pressure (TUBE) • Axial + Torsion (TUBE) • Axial + Bending Shear (TUBE) • Y Shear (BEAM) • Z Shear (BEAM) • Y Total (Overall) • Z Total (Overall) Joint (Punching) Unity Checks (1984) • Punching • Yield Member Unity Checks (1992) • Von Mises (Yield) • Y Total (Overall) • Z Total (Overall) Joint Unity Checks (1992) • Axial • In-Plane Bending • Out-of-Plane Bending • Combined Axial + Bending Member Local General Results (1984) • Section Position • Axial Stress • Bending Stress (TUBE) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 899 Features • Hoop Stress (TUBE) • Von Mises Stress • Shear Stress Due To Torsion (TUBE) • Shear Stress Due To Bending (TUBE) • Relative Slenderness Ratio (Axial) (TUBE) • Relative Slenderness Ratio (Bending) (TUBE) • Relative Slenderness Ratio (Lateral Pressure) (TUBE) • Relative Slenderness Ratio (Shear) (TUBE) • Critical Buckling Stress (Axial) (TUBE) • Critical Buckling Stress (Bending) (TUBE) • Critical Buckling Stress (Lateral Pressure) (TUBE) • Critical Buckling Stress (Shear) (TUBE) • Maximum Y Shear Stress (BEAM) • Maximum Z Shear Stress (BEAM) Member Overall General Results (1984) • Y Equivalent Moment • Z Equivalent Moment • Y Relative Slenderness Ratio • Z Relative Slenderness Ratio • FKY To Yield Stress Ratio • FKZ To Yield Stress Ratio • Y Theoretical Buckling Load • Z Theoretical Buckling Load • Y Euler Buckling Load • Z Euler Buckling Load • Y Ultimate Bending Capacity • Z Ultimate Bending Capacity • Critical Torsional Axial Stress • Revised Buckling Strength Member General Results (1992) • Axial Stress • Bending Stress • Hoop Stress • Von Mises Stress • Torsional Stress • Maximum Bending Shear Stress 900 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment • Y Equivalent Moment • Z Equivalent Moment Joint General Results (1984) • Theta Angle • Beta Ratio • Tau Ratio • Gamma Ratio • Joint Geometry Factor • Chord Stress Factor • Brace Axial Stress • In-Plane Brace Bending Stress • Out-of-Plane Brace Bending Stress • Chord Axial Stress • Chord Bending Stress • Chord Shear Yield Stress • Acting Punching Shear • Critical Joint Punching Shear Stress Joint General Results (1992) • Theta Angle • Beta Ratio • Gamma Ratio • Brace Axial Stress • Brace In-Plane Stress • Brace Out-of-Plane Stress • Chord Axial Stress • Chord Y Bending Stress • Chord Z Bending Stress Using FATJACK with the Design Assessment System The ability to perform joint fatigue assessment has been incorporated into Workbench using the Design Assessment System. This system can be connected to Static Structural, Transient Structural, and Harmonic Response systems as required. See Analysis Type Selection (p. 905) for more details of the appropriate upstream systems. The structural analysis needs to be performed using the Mechanical solver. The following sections describe how to setup a FATJACK analysis in the Design Assessment system. Introduction Information for Existing ASAS Users Solution Selection Customization Attribute Group Types Available Results Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 901 Features Introduction Attribute Group objects are added to the Design Assessment system to define the input data to FATJACK. DA Result objects are added to the Design Assessment system to define which results to obtain and display. Workbench and Design Assessment are geometry based, which means that areas of the geometry are selected rather than individual elements. With the Mechanical solver, a member ought to be meshed and formed of a number of elements. Some data associated to the upstream solutions is entered in the solution selection table. Results can be added to the Solution in the Design Assessment system and displayed in Workbench; these will contour the maximum value that occurs for each element. Results can be added either before or after the analysis. If additional results are added after the analysis has been performed, then evaluating the results will obtain the values from the existing database, if the result type exists. Elements that do not have results will be semi transparent. Results are for the end of the brace and are shown on the brace element. Reports can be produced of the input data and the results can be parameterized and exposed for use with other systems. Information for Existing ASAS Users FATJACK Command Attribute Group Type Attribute Group Subtype Requirement ANALYSIS Analysis Type Selection Time History, Spectral, Stress History, and Deterministic Compulsory ACCE Automatically defined based on units, Analysis type Spectral only. ALLO Analysis Type Selection Stress History CHOR Geometry Definition Chord Definition CURV Material Definitions S-N Curve Definition Compulsory CYCL Analysis Type Selection Time History Compulsory for Time History analysis types DESI Automatically determined from the geometry DETE Data is entered via Structure Selection table for analysis type Time History. For Deterministic and Stress History analysis types, the information should be provided in a separate file. Compulsory for Deterministic and Stress History Analysis Types FREQ Supply in a separate file with SPEC and TRAN data, referenced in Analysis Type for Spectral analyses. Compulsory for Spectral analysis types GAP Geometry Definition Gap Definition GAPD Geometry Definition Default Gap HIST Data is entered via Structure Selection table INSE Geometry Definition Inset INSP Joint Inspection Points Tubular Members, By Number Compulsory for Time History analyses Tubular Members, By List of Angles 902 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment FATJACK Command Attribute Group Type Attribute Group Subtype Requirement Non-Tubular Members, By Symmetric Positions Non-Tubular Members, By Individual Positions JOIN Analysis Type Selection Time History, Spectral, Stress History, and Deterministic Compulsory LIMI Not Supported, can be added using General Text input PARA Not Supported, can be added using General Text input PRIN Automatically defined as PRIN FULL DETA USAG XCHE SCFE SCFP DAMW, plus OCUR, OCRW or OCRT for Spectral Analyses or plus RNGE or PEAK for Stress History Analyses, both depending upon the option entered in the Analysis definition. If different text output is required, then it can be added using General Text input. REDU SCF Definitions Marshall Reduction SCF SCF Definitions Default Values SCF ANGLE SCF Definitions Joint Values, Tubular (Inspection Point by Angle) SCF AUTO DEFAULT SCF Definitions Default Empirical Formulation by Joint Type SCF AUTO JOINT SCF Definitions Empirical Formulation by Joint SCFBRACE SCF Definitions Joint Values, Non-Tubular (All Inspection Points) SCFJOINT SCF Definitions Brace Side Joint Values, Tubular (Crown + Saddle) Compulsory Chord Side Joint Values, Tubular (Crown + Saddle) SCFMINIMUM SCF Definitions Minimum Value SCFPOINT SCF Definitions Joint Values, Non-Tubular (Inspection Point by Position) SECO Geometry Definition Excluded Members SIGM Not Supported Analysis Type for Spectral analyses Compulsory for Spectral analysis S-N Material Definitions S-N Curve Application Compulsory SPEC Supply in a separate file with FREQ and TRAN data Analysis Type for Spectral analyses Compulsory for Spectral analysis SPRE Not Supported Analysis Type for Spectral analyses Compulsory for Spectral analysis THIC Material Definitions S-N Thickness Modification TRAN Supply in a separate file with FREQ and SPEC data Analysis Type for Spectral analyses Compulsory for Spectral analysis Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 903 Features FATJACK Command Attribute Group Type Attribute Group Subtype TYPE Geometry Definition Joint Type (Single Brace) Requirement Joint Type (Multiple Braces) UNIT Automatically determined from analysis, selections for N mm, pdl ft, pdl in and N m are supported. WAVE WAVE AUTO Automatically included for Spectral, Deterministic and Stress History analysis types, use General Text entry to override if specific control is required. YEAR Analysis Type Selection Time History, Spectral, Stress History, and Deterministic Compulsory Solution Selection Customization The Solution Selection object for FATJACK has additional columns for the entry of the range of steps to use for rainflow counting (start step, end step, and interval between steps). Also, the occurrence data for each environment can be defined either by number of cycles per year and an amplification factor, or by probability. If a probability is entered this will be used instead of cycles per year. A consistent method needs to be used throughout all solution environments. This data is only applicable for Time History based analyses. For Stress History and Deterministic methods the occurrence data is defined externally, referenced in the analysis type. Attribute Group Types Attribute Groups enable the entry of the data that is associated with the FATJACK analysis. The following sections describe the available Attribute Group Types and their subtypes. Analysis Type Selection General Text Geometry Definition Joint Inspection Points SCF Definitions Material Definition Ocean Environment Some attribute groups are compulsory, indicated by superscript letters as follows: TH – compulsory for Time History based analyses SH – compulsory for Stress History based analyses SP – compulsory for Spectral based analyses DT – compulsory for Deterministic based analyses C – compulsory for all analyses Note If units are changed when defining data for Attributes, then the resulting data sent to the processing script may be incorrect. It is recommended that units are not modified from those used in creating the geometry. 904 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Analysis Type Selection All types of fatigue analysis supported with this interface. • Time HistoryTH Enables the selection of which joints are to be included, along with definition of the number of cycles for rainflow counting and target year life of the analysis. Upstream systems should be Structual Transient, normally each including randomized ocean loading with different wave directions. • Stress HistorySH Enables the selection of which joints are to be included, along with definition of the target year life of the analysis. Wave conditions (heights, periods, directions) are automatically determined from the ocean loading provided in upstream system(s) in the order that they are defined. Wave occurrence data can be provided by addition of attribute groups of the Ocean Environment type. Upstream systems can be either static structural or transient structural. If loading is not applied using the ocean loading, then General Text can be used to define the WAVE commands. If the value for Allowable Stress is left blank, then actual stresses will be output; if a value is entered, then utilization factors will be output. These values will either be the Peak or Full Range values as specified. • SpectralSP Enables the selection of which joints are to be included, along with definition of the peak stress, wave spreading and target year life of the analysis. Wave transfer function, spectrum,and additional frequency data should be provided in a text file containing the FATJACK commands. Wave load cases are automatically determined using the harmonic ocean wave procedure provided in upstream system(s) in the order that they are defined. Upstream systems should be of the Harmonic Response type; both the Static and Harmonic options of the HROCEAN command can be used when performing Spectral analysis. • DeterministicDT Enables the selection of which joints are to be included, along with definition of the target year life of the analysis. Wave load cases are automatically determined using the harmonic ocean wave procedure provided in upstream system(s) in the order that they are defined. Upstream systems should be of harmonic response type; only the Static option of the HROCEAN command is appropriate for Deterministic analysis. Note References to ocean loading assume the input of MAPDL commands using Commands objects in upstream Mechanical systems. General Text This can be used to supply additional and non-supported commands. This will always override data set by other tree objects. • Geometry Independent Enables additional commands to be entered that will be appended to the end of all code checks. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 905 Features Geometry Definition All groups that have this type enable the selection of a particular code of practice. • Chord Definition The chord member(s) and the central vertex can be chosen along with the length of the chord and fixity parameters to define which members at a joint form the chords. Without this definition, chords are automatically determined. Chords for each Joint need to be defined separately. Only applicable to joint checks. • Gap Definition Enables specific gap information to be defined between the pairs of braces forming KT or K joints, and to determine which member is the through member. • Default Gap Enables the entry of the default gap size to use for the given equations. • Inset Enables a distance to be entered to allow for moment backoff. • Joint Type (Single Brace) Enables the manual definition of joint type when only a single brace is connected. • Joint Type (Multiple Braces) Enables the manual definition of joint type when more than one brace is connected. • Excluded Members Enables members that are to be excluded from the joint checks to be selected. Joint Inspection Points Inspection points are the positions to check for fatigue around the brace where it connects to the chord. • Tubular Members, By Number Use this to define the number of inspection points equally spaced around tubular members. • Tubular Members, By List of Angle Use this to define a list of space separated angles that define the inspection points spaced around tubular members at an individual joint. • Non-Tubular Members, By Symmetric Positions Use this to define inspection points for selected non-tubular members by defining Z and Y offset distances from the centre of the member to generate 4 points for the positive and negative combinations. • Non-Tubular Members, By Individual Positions Use this to define specific inspection points on an individual joint, by a list of y z pairs, space separated. 906 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment SCF Definitions All groups that have this type enable the entry of values that define the stress concentration factors. • Marshall Reduction Use this to define the Marshall Reduction factor for the brace side SCF values when using the Kuang equations. • Default ValuesC Use this to specify the default SCF values for a given section type. • Chord Side Joint Values, Tubular (Crown + Saddle) Use this to specify user defined crown and saddle SCF values for the chord side of tubular braces at specific joints. • Brace Side Joint Values, Tubular (Crown + Saddle) Use this to specify user defined crown and saddle SCF values for the brace side of tubular braces at specific joints. • Joint Values, Non-Tubular (All Inspection Points) Use this to specify the SCF values at all inspection points on non tubular braces. • Joint Values, Tubular (Inspection Point by Angle) Use this to specify the SCF values at specific inspection points on tubular braces. • Joint Values, Non-Tubular (Inspection Point by Position) Use this to specify the SCF values at specific inspection points on non tubular braces. • Empirical Formulation by Joint Use this to specify that the empirical equations to be utilized for the SCF generation for the given joint selection. • Default Empirical Formulation by Joint Type Use this to specify the default empirical equations to be utilized for the SCF generation for the given joint type. • Minimum Value Use this to set the minimum SCF value in the analysis. Material Definition All groups that have this type enable the selection of a particular code of practice. • S-N Curve ApplicationC Use this to define which S-N Curve applies to selected area of the model. Enter the same name as used in the S-N Curve Definition. • S-N Thickness Modification Use this to request the modification of the S-N curves to account for varying plate thickness. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 907 Features • S-N Curve DefinitionC Use this to define an S-N curve for use in the analysis; the name is limited to 4 characters in length. Ocean Environment All groups that have this type define wave occurrence data in the ocean environment, if a large number of occurrence data needs to be entered, then general entry can be used to reference an external file containing the data. • Additional Wave Occurrence Data Use this to define a single line of additional wave occurrence data; i.e., additional wave height, direction, and number of cycle definitions. Only applicable to Deterministic and Stress History analysis types. Available Results The following results are available as indicated below. Results are added using the DA Results tree object. • Damage Values* • Fatigue Assessment*# • SCF Values# • Stress Histogram Results • Stress Range Results * Note, to obtain these results for Spectral Analyses, Stress Histogram Results Output needs to be set to Disabled. # Note, to obtain these results for Stress History Analyses, Stress Range Output needs to be set to Disabled. Damage Values • Per Wave (Solution) The damage per wave for each joint (worst case for each inspection point, shown on the brace and chord elements) can be displayed. The Spectrum or Wave Case number needs to be entered as additional input. Fatigue Assessment • Usage Factor • Life The Usage Factor or Life for each joint (worst case for each inspection point, shown on the brace and chord elements) can be displayed. SCF Values • Brace Side • Chord Side 908 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment The SCF factors for each joint for the chord and brace sides (worst case for each inspection point, shown on the brace and chord elements) can be displayed for the required component (Axial, In-Plane Bending, Out-of-Plane Bending). Stress Histogram Results These results are only applicable to Spectral analysis and Time History analysis results, unless noted otherwise. • Brace Side Occurrence • Chord Side Occurrence • Brace Side Stress • Chord Side Stress The stress data for each joint (worst case for each inspection point, shown on the brace and chord elements) can be displayed. The Wave Case number is the Upstream System Number and Interval needs to be entered. In the case of Spectral analyses, the Wave Case number is not required and is ignored. In the case of Time History analyses, this is equivalent to the row of the upstream solution in the Solution Selection. For Spectral Analyses, Stress Histogram Results Output needs to be enabled. • Brace Side Occurrence by Transfer Function • Chord Side Occurrence by Transfer Function The occurrence data for each joint (worst case for each inspection point, shown on the brace and chord elements) can be displayed for a given Transfer function. Spectral analyses only, when Stress Histogram Results Output is set to “By Transfer Function”. • Brace Side Occurrence by Spectrum • Chord Side Occurrence by Spectrum The occurrence data for each joint (worst case for each inspection point, shown on the brace and chord elements) can be displayed for a given Spectrum. Spectral analyses only, when Stress Histogram Results Output is set to “By Spectrum”. Stress Range Results These results are only applicable to Stress History results; in addition, Stress Range Output must be set to either Peak Stress or Stress Range appropriately. • Signed Peak Stress • Peak Stress Utilization • Stress Range • Stress Range Utilization The stress data for each joint (worst case for each inspection point, shown on the brace and chord elements) can be displayed. The Wave Case number is the case entered in the Deterministic analysis data. Utilization results are only available if an allowable stress has been entered. Non-utilization results are only available if a zero allowable stress has been entered. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 909 Features Changing the Assessment Type or XML Definition File Contents If you change the Assessment Type of your Design Assessment system, or if you change the location or contents of the XML definition file, the Mechanical application will evaluate the existing Design Assessment objects in your project and modify those objects as indicated below. If no content changes are found in the XML definition file (even if the file location changes), or if only the Solve or Evaluate script locations change, no changes are made in the Design Assessment objects in the tree. If you change the Assessment Type of the Design Assessment system: From Solution Combination Only to BEAMCHECK No changes are made to the existing objects in the project. From Solution Combination Only to FATJACK All Mechanical results inserted under the Solution object will be deleted. From FATJACK to BEAMCHECK All existing Attribute Group and DA Result objects will be refreshed based on certain criteria. From FATJACK to Solution Combination Only All DA Result and Attribute Group objects will be deleted. From BEAMCHECK to FATJACK All Mechanical results will be deleted and Attribute Group and DA Result objects will be refreshed based on certain criteria. From BEAMCHECK to Solution Combination Only All Attribute Group and DA Result objects will be deleted. Note The behavior described above also corresponds to the settings of the DAData and CombResults properties in the DAScripts section of the XML definition file. For BEAMCHECK, DAData=1 and CombResults=1; for FATJACK, DAData=1 and CombResults=0; for Solution Combination Only, DaData=0 and CombResults=1. So, for example, if you have the DAData and CombResults properties both set to 1 in a user defined XML file, and you change the DAData property to 0, the behavior would be that described in the From BEAMCHECK to Solution Combination Only entry above. If the contents of any Design Assessment XML definition file change, the Mechanical application refreshes the existing Design Assessment objects as follows: When the Group Type in use is not present in the file The affected Attribute Group or DA Result is initialized to default values. Default values are the values which you get when an Attribute Group or DA Result is inserted in the tree. When the Group Sub Type in use is not present in the file The affected Attribute Group or DA Result is initialized to default values. Default values are the values which you get when an Attribute Group or DA Result is inserted in the tree. When the Attribute IDs present for a Group Type and Sub Type combination in use are changed (IDs added or removed) The affected Attribute Group or DA Result is initialized to default values. Default values are the values which you get when an Attribute Group or DA Result is inserted in the tree. Group Type not in use is changed/added/removed No existing Design Assessment objects are affected. 910 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Group Sub Type not in use is changed/added/removed No existing Design Assessment objects are affected. Attribute IDs are changed/added/removed for a Group Type and Sub Type combination which is not in use No existing Design Assessment objects are affected. Validation/Default Value/Attribute Name/Geometry Application/Property type is changed Design Assessment object is modified as indicated. Note For any above mentioned change, the state of the system becomes obsolete, forcing the user to solve again. Solution Selection A Solution Selection object is automatically included as part of the Design Assessment environment. This object allows you to select upstream solutions to be used in a way similar to the standard Solution Combination object available in the Mechanical application. To use the Solution Selection object, the individual analysis systems should be connected in sequence on the Project Schematic (sharing the Engineering Data, Geometry and Model cells), with the Design Assessment system at the end of the chain. Depending upon the type of Assessment Type various different types of upstream systems are valid as shown in the below table. Assessment Type Valid systems Solution Combination Only Static Structural, Modal, Harmonic Response, Response Spectrum or Transient Structural BEAMCHECK Transient Structural or Static Structural FATJACK Transient Structural, Static Structural or Harmonic Response User Defined Static Structural, Modal, Harmonic Response, Random Vibration, Response Spectrum, Explicit Dynamics or Transient Structural The Results Availability field in the Details panel for the Design Assessment system Solution object allows you to specify which Mechanical results will be available to the Design Assessment system. If Results Availability is set to Filter Combination Results and different upstream system types are selected, only results that are valid for all selected systems can be inserted under the Solution object. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 911 Features However, if you set the Results Availability field to Allow all Available Results, you can add any results valid for any of the selected systems to the Solution object. In this case, results that are inserted will be combined for those systems for which they are valid. You can set the default value for the Results Availability field in the Mechanical Options. If Results Availability is set to Filter Combination Results, and additional upstream systems are selected which cause a result type to be invalid, then its state will change accordingly and a solution will not be possible. Note • When used in a solution combination based result, it may not be correct to combine the results. Any combined results are formed by linear combination only. • The available systems in the drop down list are not constrained depending upon the Assessment Type. • The Results Availability setting will only appear under the Design Assessment Solution object in the tree if the <CombResults> tag within the XML that is being used by the Design Assessment system is set to 1. Otherwise it has no function. • User defined results containing complex expressions are not supported for Solution Combination results within Design Assessment. However, you can access results from various environments, using python scripts to combine results with highly complex, user defined mathematical functions (see CreateSolutionResult in the Solution class). The Solution Selection object differs in several ways from a standard Solution Combination object: • There is an ability to add extra columns to the worksheet using the XML configuration file. Each row in the table can be used to enter additional data that can be passed out to the processing script. These values can be obtained using the Design Assessment API. • Results are added to the Solution object in the Design Assessment system, not directly under the Solution Selection object. • The Solution Selection object can be configured such that select results from multiple upstream systems are available for use in post processing scripts, but the display of combined results is suppressed. For the FATJACK Assessment Type, or when CombResults = 0 in a user defined XML file, Solution Selection will make the results of the selected solutions available for external processing, but no solution combination is done, and no Mechanical results are available. • Appropriate columns are enabled to access appropriate result sets defined by time, step, frequency, phase and mode, based on the upstream system. • Upstream results systems can be accessed via the python scripts using the Selection class. Using the Attribute Group Object Attribute Group objects allow the Mechanical application to collect inputs. They are available in Predefined Assessment Types such as BEAMST and FATJACK, or can also be configured in the XML definition file of a User Defined Type. After you have opened the project in the Mechanical application, insert an Attribute Group by one of the following methods: 1. Right click on the Design Assessment object and select Insert > Attribute Group or 912 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Click on the Design Assessment object, then click on the Attribute Group button in the toolbar. An Attribute Group object will be added to the analysis. 2. Click on the Attribute Group and then set it up by selecting the appropriate AttributeGroupType and AttributeGroupSubtype. This will display the attributes for that group subtype. 3. Enter the attribute values that you wish to pass out to the postprocessing script defined in the XML definition file, along with any associated geometry information. Note Numerical attributes within an attribute group can be parameterized. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 913 Features Developing and Debugging Design Assessment Scripts The scripting environment used in Design Assessment is the same as that used in the Workbench and is based on IronPython, which is well integrated into the rest of the .NET Framework (on Windows) and Mono CLR (on Linux). For more details see the Workbench Scripting documentation. With the help of a development environment, such as Microsoft® Visual Studio®, Python scripts can be developed and “debugged”. To debug a script, open its text file in your development environment and attach the debugger to the AnsysWBU.exe process of interest. Be sure to specify managed code mode. You will then be able to control the execution of your script, stepping along and reviewing the values obtained. Using the DA Result Object DA Results Objects allow the end user to specify what results to calculate and how to display them. You can add DA Result objects to the analysis system for the BEAMCHECK or FATJACK assessment types, or if DAData=1 in a user defined XML definition file. After you have opened the project in the Mechanical application, insert a DA Result object using one of the following methods: 1. Right click on the Solution object under Design Assessment and select Insert > DA Result. or Click on the Solution object, then click on the DA Result button in the toolbar. A DA Result object will be added to the analysis. 2. Click on the Result Group and then set it up by selecting the appropriate ResultType and ResultSubtype. This will display the attributes for that group subtype. 3. Set the Entry Value for each attribute in the DA Result object to return the Results of interest to you. 4. Right click on the DA Result object and select Solve. The results of the post processing script are displayed in the Results section of the Details panel. Entry Value cells are only shown for Global or Geometry Display Types, and then only if there is one time step; otherwise, the values will be shown in a graph plotted against solve position with an accompanying table of the values. 914 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment The Design Assessment XML Definition File The Design Assessment system is driven in part by an XML definition file (referred to as the XML definition file) . This file can be user defined or provided by ANSYS or a third party. This section defines the format of the XML definition file. The XML definition file is split into four parts to define the following: • Available Attributes • Attribute Groups • Scripts • Result Availability Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 915 Features For each Design Assessment system, a copy will be made of the selected XML definition file and associated with that Design Assessment system to define the visibility of the tree objects. The entries in the tree objects will be saved with the Mechanical project database file; this includes the actual script used for the assessment. The overview of the file format is shown below. <?xml version="1.0"?> <Attributes> definition of attributes for re-use throughout the attribute groups. </Attributes> <AttributeGroups> grouping of attributes; used to define the available options in the attribute groups objects </AttributeGroups> <DAScripts> analysis script language & contents; used to define a script covering how the design assessment will be performed and a script used to obtain results </DAScripts> <DAResults> definition of the available results and the available options in the results object. </DAResults> Note For all sections of the XML definition file, all values entered as part of a list in a tag must be separated by commas only (no spaces); for example in the following tag, <Validation PropType="vector&lt;string>">0.5,10</Validation>, there should not be any space between the values 0.5 and 10. Attributes Format Within the Attributes section there are a number of options to define the name and type of attribute (for example, whether it’s a double, integer, drop-down list, text, etc.), and what it applies to (for example, can it be applied to selectable geometry or loadcases, and if geometry, is it vertex, lines, surfaces or solids). Depending upon the type, default values and validation ranges can be set. Attributes of int and double types can be parameterized. <Attributes ObjId="2" Type="CAERepBase" Ver="2"></Attributes> <DAAttribute ObjId="100" Type="DAAttribute" Ver="2"> <AttributeName PropType="string">attr name</name> <AttributeType PropType="string">type keyword</type> <Application PropType="string">selection keyword</application> <Validation PropType="string">validation data</validation> <Default PropType="string">default value</default> <DisplayUnits PropType="string">display units keyword</DisplayUnits> </DAAttribute> </Attribute> The attribute is defined in the Details panel with 4 rows: If Scoping Method is set to Named Selection, the fourth row will contain a drop-down of all defined named selections that contain geometric entities of the type specified in the attribute definition. 916 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment The Attributes tag properties should be set as follows: Property Value Meaning ObjId enter an integer Number identifying this attribute collection Type CAERepBase Specifies that the file is in ANSYS intermediate file format Ver enter an integer Version of the Attributes object definition; this should be set to 2 The DAAttribute tag properties should be set as follows: Property Value Meaning ObjId enter an integer Unique number identifying this DAAttribute, suggest starting at a fixed number (e.g. 100) to avoid conflict with other objects Type DAAttribute Signifies that the contents of the DAAttribute tag define an attribute Ver enter an integer Version of the DAAtribute object definition; this should be set to 2 The following tags can be included as children of a DAAttribute tag (note that each tag must have a property PropType=”string” or PropType=”vector&lt;string>” (the latter if entering more than a single value in the tag contents). Property Value Meaning AttributeName enter a string Displayed name of the attribute AttributeType, with following values of type keyword allowed: Int Integer entry only Double Double precision entry only Text Text entry only DropDown Drop down list selection Browse Text based, but includes browse to a file button None Only Geometry Selection required, hides Value Cell Vertices Enables Geometric selection of vertices only Lines Enables Geometric selection of line bodies only Surfaces Enables Geometric selection of surface bodies only Solids Enables Geometric selection of solid bodies only Geometry Enables Geometric selection of lines, surfaces and solids All Hides Geometry Selection cell, applies to the whole analysis Two comma separated numbers defining a min and max For Int or Double type keywords Multiple comma separated strings defining the available entries For DropDown type keywords Application, with following values of selection keyword allowed: Validation, with following values of validation data allowed: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 917 Features Property Default, with following values of default value allowed: DisplayUnits, with following values of display units keywords allowed: (Only used if version number of DAAttribute > 2 and AttributeType is Double) When a display unit is defined the value will automatically scale depending on the defined unit system for the Analysis and for the unit system used to view 918 Value Meaning A single number to define the maximum length of the string For the Text or Browse type keywords Default value in SI units; if default is within the valid range, when it’s created the object state will be checked, otherwise “?” For Int or Double type keywords String; used to set the default entry in the drop-down For DropDown type keywords Default text string For the Text or Browse type keywords No Units No units are associated with the value (default if field is not defined) Stress Values are treated as stress Distance Values are treated as distance Strain Values are treated as strain Force Values are treated as force Moment Values are treated as moment, i.e. force x distance Rotation Values are treated as rotation Angular Acceleration Values are treated as angular acceleration, i.e. rotation / time2 Angular Velocity Values are treated as angular velocity, i.e. rotation / time Velocity Values are treated as velocity, i.e. distance / time Acceleration Values are treated as acceleration, i.e. distance / time2 Temperature Values are treated as temperature Pressure Values are treated as pressure, i.e. force / distance2 Voltage Values are treated as voltage Energy Values are treated as energy Volume Values are treated as volume, i.e. distance3 Area Values are treated as area, i.e. distance2 Current Values are treated as current Heat Rate Values are treated as heat rate Current Density Values are treated as current density Power Values are treated as power Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Property Value Meaning Heat Generation Values are treated as heat generation Magnetic Flux Values are treated as magnetic flux Attribute Groups Format The AttributeGroups tag contains DAAttributeGroup tags that provide a means for the user to select the groups of attributes shown in the Details panel when an Attributes Group tree object is selected. A maximum of 10 attributes can be grouped per attribute group object. Attribute group objects automatically sort themselves by drop downs of available types and subtypes. <AttributeGroups ObjId="3" Type="CAERepBase" Ver="2"> <DAAttributeGroup ObjId ="100001" Type="DAAttributeGroup" Ver="2"> <GroupType PropType="string">Group Type</GroupType> <GroupSubtype PropType="string">Group Subtype</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">list of attribute numbers</AttributeIDs> </DAAttributeGroup> </AttributeGroups> The group is defined in the Details panel with 3 standard rows and then up to 10 attributes: The AttributeGroups tag properties should be set as follows: Property Value Meaning ObjId enter an integer Number identifying this attribute group collection Type CAERepBase Specifies that the file is in ANSYS intermediate file format Ver enter an integer Version of the AttributeGroups object definition; this should be set to 2 The DAAttributeGroup tag properties should be set as follows: Property Value Meaning ObjId enter an integer Unique number identifying this DAAttributeGroup, suggest starting at fixed number (e.g. 500) to avoid conflict with other objects Type DAAttributeGroup Signifies that the contents of the DAAttributeGroup tag define an attribute group Ver enter an integer Version of the DAAttributeGroup object definition; this should be set to 2 The following tags can be included as children of a DAAttributeGroup tag: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 919 Features Property Value Meaning GroupType enter a string Type of this attribute group GroupSubtype enter a string Subtype of this attribute group AttributeIDs enter a comma separated list of attribute ID numbers Attributes that will be displayed for this attribute group The PropType property of the GroupType and GroupSubtype tags must be set to string, and the PropType property of the AttributeIDs tags must be set to vector&lt;unsigned int>. Script Format This section defines the location for the Design Assessment post processing scripts and also defines what values can be accessed in this Design Assessment system. The scripts are to be written using the Python scripting language. There are three Design Assessment specific system environment variables that can be used when specifying script paths: DAPROGFILES Default: C:\Program Files DANSYSDIR Default: C:\Program Files\ANSYS Inc\v140 DAUSERFILES The Workbench project user_files subfolder The Solve tag defines the location of the script that will be run upon pressing the solve button within the Mechanical application. The Evaluate tag defines the location of the script that will be run when evaluting the DAResult objects. The Evaluate script will be run by default after the solve script when solve has been selected. This separation enables the ability for any intensive processing to be performed and saved to files during the solve stage and then results extraction and presentation to be scripted during the evaluation stage. Alternatively, you may want all the processing performed during the evaluate script and enter None in the Solve Script section. Additional tags allow you to: • permit or prevent the inclusion of Design Assessment Attribute Groups and Results in the tree for the associated Design Assessment system • permit or prevent the availability of solution combination results in the associated Design Assessment system • add additional columns to the Solution Selection Worksheet • define which upstream solution types are permitted in the Solution Selection Worksheet <DAScripts ObjId="4" Type="DAScripts" Ver="2"/> <!--analysis script language & contents; used to define a script covering how the design assessment will be performed and a script used to obtain results--> <Solve PropType="string">"c:\mysolve.py"</Solve> <Evaluate PropType="string">"c:\myevaluate.py"</Evaluate> <DAData PropType="int">1</DAData> <CombResults PropType="int">1</CombResults> <CombExtra PropType="vector&lt;string>">Extra 1,Extra 2,Extra 3</CombExtra> <CombTypes PropType="vector&lt;unsigned int>">1,2,3,4,5,6,7</CombTypes> lt;/DAScripts> The DAScripts tag properties should be set as follows: 920 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Property Value Meaning ObjId enter an integer Number identifying this script set Type DAScripts Signifies that the contents of the DAScripts tag define solve and evaluate postprocessing scripts Ver enter an integer Version of the DAScripts tag; this should be set to 2 The following tags can be included as children of a DAScripts tag: Property Value Meaning Solve enter a string Path to the file called during the solution; a relative path can be entered. A relative path will be relative to {install}\aisol\bin\{platform}, so for example, ..\..\..\My_Solve.py would need to be located in the same folder as the installation. Standard environment variables or one of the Design Assessment specific environment variables may be used in the path (enclosed in percent signs). For example: %TEMP%\My_solve.py %DAPROGFILES%\My_solve.py If no solve script is required, the keyword None can be entered. Evaluate enter a string Path to the file called during the evaluate. As per the Solve string, this can be relative or use standard environment variables or the Design Assessment specific environment variables. DAData enter either 1 or 0 Set to 0 to prevent any DA Data (Attribute Groups or DA Results) from being added to the project, or 1 to allow them CombResults enter either 1 or 0 Set to 0 to prevent Mechanical Results objects from being added to the Design Assessment Solution, or 1 to allow them Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 921 Features Property Value Meaning CombExtra enter a comma separated list of strings Enter a string for each extra column heading that you want to appear in the Solution Selection Worksheet. CombTypes enter a comma separated list of positive numbers between 1 and 7 Each of the numbers represents a system type. Only system types in this list will be permitted to be selected in the Solution Selections table. The numbers correspond to the systems as follows: 1: Static Structural 2: Transient Structural 3: Explicit Dynamics 4: Modal 5: Harmonic Response 6: Random Vibration 7: Response Spectrum If CombTypes is not defined, there will be no restrictions applied. The PropType property of the Solve and Evaluate tags must be set to string, The PropType property of the DAData and CombResults tags must be set to int, and the PropType property of the CombExtra tag must be set to vector&lt;string> and the PropType property of the CombTypes tag must be set to vector&lt;unsigned int>. Results Format The DA Results format defines the available DA Results tree objects. A maximum of 10 attributes can be included per DA Result object; for example to define direction components. For attributes applied to results objects, the application entry is ignored. DA Result objects automatically sort themselves by drop downs of available types and subtypes. Each DA Result object also contains information on how it should display results; this can either be set in this XML definition file or programmatically in the python solve or evaluate scripts. Minimum and maximum values are also reported and can be parametrized. Probe labels can be added to the graphic to identify specific results, or the minimum and maximum locations. <Results ObjId="3" Type="CAERepBase" Ver="2"> <DAResult ObjId ="100001" Type="DAResult" Ver="2"> <GroupType PropType="string">Group Type</GroupType> <GroupSubtype PropType="string">Group Subtype</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">list of attribute numbers</AttributeIDs> <DisplayType PropType="string">display type keyword</DisplayType> 922 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment <DisplayStyle PropType="string">display style keyword</DisplayStyle> <DisplayUnits PropType="string">display units keyword</DisplayUnits> </DAResult> </Results> The result is defined in the Details panel with standard rows and then up to 10 attributes: Note that if the Display Style of a result is anything other than scalar, a "Components" field is shown in the Definitions section. The Results tag properties should be set as follows: Property Value Meaning ObjId enter an integer Number identifying this attribute group collection Type CAERepBase Specifies that the file is in ANSYS intermediate file format Ver enter an integer Version of the Results definition section; this should be set to 2 The DAResult tag properties should be set as follows: Property Value Meaning ObjId enter an integer Unique number identifying this DA Result; suggest starting at a fixed number (e.g. 1000) to avoid conflict with other objects Type DAResult Signifies that the contents of the DAResult tag defines a result group Ver enter an integer Version of the DA Result object definition; this should be set to 3 The following tags can be included as children of a DAResult tag: Property Value Meaning GroupType enter a string Type of this DA Result object GroupSubtype enter a string Subtype of this DA Result object AttributeIDs enter a comma separated list of attribute ID numbers Attributes that will be displayed for this DA Result object DisplayType, with following values of display type keywords allowed: Element Values per element are expected Nodal Values per node are expected. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 923 Features Property DisplayStyle, with following values of display style keywords allowed: (Only used if version number of DAResult > 2) Value Meaning ElementNodal Values per node of each element are expected Scalar A single number is expected for each element / node depending upon the DisplayType set (default if field is not defined) Vector X, Y and Z component values are expected for each element / node depending upon the DisplayType An additional drop down will be provided to choose between X, Y, Z, Resultant and Vector Display The Resultant, R, is determined by = √ Tensor
 +   +  X, Y, Z, XY, YZ and XZ component values are expected for each element / node depending upon the DisplayType An additional drop down will be provided to choose between X, Y, Z, XY, YZ and XZ, Maximum Principal, Middle Principal, Minimum Principal, Intensity, Equivalent, Vector Principal, and Maximum Shear DisplayUnits, with following values of display units keywords allowed: (Only used if version number of DAResult > 2) When a display unit is defined the result will automatically scale depending on the given unit system 924 StrainTensor As Tensor, but without the Maximum Shear option No Units No units are associated with the result (default if field is not defined) Stress Results are treated as stress Distance Results are treated as distance Strain Results are treated as strain Force Results are treated as force Moment Results are treated as moment, i.e. force x distance Rotation Results are treated as rotation Angular Acceleration Results are treated as angular acceleration, i.e. rotation / time2 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Property Value Meaning Angular Velocity Results are treated as angular velocity, i.e. rotation / time Velocity Results are treated as velocity, i.e. distance / time Acceleration Results are treated as acceleration, i.e. distance / time2 Temperature Results are treated as temperature Pressure Results are treated as pressure, i.e. force / distance2 Voltage Results are treated as voltage Energy Results are treated as energy Volume Results are treated as volume, i.e. distance3 Area Results are treated as area, i.e. distance2 Current Results are treated as current Heat Rate Results are treated as heat rate Current Density Results are treated as current density Power Results are treated as power Heat Generation Results are treated as heat generation Magnetic Flux Results are treated as magnetic flux The DisplayType, DisplayStyle and Display unit can all be over-ridden or set within the python script if desired. However, DisplayStyle needs to be set here to enable the addition of the drop-down to choose the component and automatic calculation of additional results (e.g. Resultant, Maximum Principal, etc.) in the cases of vector or tensor display. See the DAResult class in the API for details on how to set these programmatically. The PropType property of the GroupType, GroupSubtype, and DisplayType tags must be set to string, and the PropType property of the AttributeIDs tags must be set to vector&lt;unsigned int>. Design Assessment API Reference These guidelines describe the Design Assessment API. Included with the standard ANSYS Workbench installation is the IronPython scripting environment that allows a Python script to be run. Within Design Assessment scripts can be run upon Solve and Evaluate. These Python based scripts have a DesignAssessment object defined as an entry point to access to the API functions to enable data to be processed either directly in python, or externally by calling 3rd party programs. The following API classes are available: DesignAssessment class Helper class MeshData class DAElement class Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 925 Features DANode class SectionData class AttributeGroup class Attribute class SolutionSelection class Solution class SolutionResult class DAResult class DAResultSet class The API is structured as shown in this diagram: Every effort is made to ensure compatibility of the API across versions. However, there are occasions where functions or properties need to be modified. In these scenarios, the existing function will be deprecated, i.e. it will become undocumented. Any data output via the print command will be added to the appropriate script output file which can be reviewed via the Solution Information object. If a deprecated function is called a message will be added to the appropriate script output file with a suggested alternative methodology. These can be viewed via the Solution Information object. This inclusion of the message in the file can be controlled by the OutputDeprecatedWarnings function in the DesignAssessment class. Additional text output from your script can be included in a file that is displayed using the Solver Output option (see Helper class, ReplaceSolverOutputFile). Undocumented functions (including those recently deprecated) may be removed or altered in subsequent releases if it becomes impractical to maintain a backwards compatible interface, so effort should be made to update any calls to deprecated functions. Functions may not work on previous releases; therefore, all users should use the same release of Workbench to ensure compatibility. 926 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment API Change Log for R14.0 Release 14 represents the first release after the initial version. In response to feedback, we have made a number of changes of functions to properties where appropriate, hence there are an unusually high number of deprecated functions. These changes are tabulated below, grouped by class name. The tables do not include newly added functions. Design Assessment Class: Method/Property Description of Change getHelper() Changed to property Helper, old code: DesignAssessment.getHelper(), new code DesignAssessment.Helper GeometryMeshData() Changed to property MeshData, old code: DesignAssessment.GeometryMeshData(), new code DesignAssessment.MeshData Selections() Changed name to SolutionSelections() to be consistent with the Mechanical application Selection(int Index) Duplication of python functionality. Old code DesignAssessment.SolutionSelection(0), new code MyArray = DesignAssessment.SolutionSelections() then MyArray[0] (NB, using the shortcut DesignAssessment.SolutionSelections()[index] in a loop is less efficient than assigning it to an array within python) ResultGroups() Changed name to DAResults() to be consistent with the Mechanical application ResultGroup(int Index) Duplication of python functionality. Old code DesignAssessment.DAResult(0), new code MyArray = DesignAssessment.DAResults() then MyArray[0] (NB, using the shortcut DesignAssessment.DAResults()[index] in a loop is less efficient than assigning it to an array within python) NoOfAttributeGroups() Changed to property AttributeGroupCount, old code: DesignAssessment.NoOfAttributeGroups(), new code DesignAssessment.AttributeGroupCount NoOfSelections() Changed to property SolutionSelectionCount, old code: DesignAssessment.NoOfSelections(), new code DesignAssessment.SolutionSelectionCount NoOfResultGroups() Changed to property DAResultCount, old code: DesignAssessment. NoOfResultGroups(), new code DesignAssessment.DAResultCount ProjectName() Changed to property ProjectTitle, old code: DesignAssessment. ProjectName(), new code DesignAssessment.ProjectTitle AttributeGroup(int Index) Duplication of python functionality. Old code DesignAssessment.AttributeGroup(0), new code MyArray = DesignAssessment.AttributeGroups() then MyArray[0] (NB, using the shortcut DesignAssessment.AttributeGroups()[index] in a loop is less efficient than assigning it to an array within python) Helper Class: A number of functions related to an internal file, the CAERep, were previously documented in error. These have been removed from the documentation; it is not recommended that these are used as the file structure is subject to change. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 927 Features Function/Property Description of Change getUnits() Replaced by property Units in the DesignAssessment class, for the units set for the Design Assessment System and also the property Units in the Solution class for the units system used in upstream solution. getSolverOut() Changed to property SolverOutputFilePath, old code: Helper.getSolverOut(), new code Helper.SolverOutputFilePath getOutputFile() Changed to property SystemDirectory, old code: Helper.getOutputFile(), new code Helper.SystemDirectory getGeometryPath () Changed to property GeometryPath, old code: Helper. getGeometryPath (), new code Helper.GeometryPath getResultPath () Changed to property ResultPath, old code: Helper.getResultPath(), new code Helper.ResultPath getSystemDirectory () Changed to property SystemDirectory, old code: Helper.getSystemDirectory(), new code Helper.SystemDirectory getLogFile() Removed as the log file can be displayed via Solution Information and its contents can be added to via the standard python print function WriteToLog () Removed as the log file contents can be added to via the standard python print function MeshData Class (previously named GeometryMeshData): A number of functions related to an internal reference, the TopologyID, were previously documented in error. These have been removed from the documentation. Method/Property Description of Change NoOfNodes() Changed to property NodeCount, old code: MeshData. NoOfNodes(), new code MeshData.NodeCount NoOfElements() Changed to property ElementCount, old code: MeshData.NoOfElements(), new code MeshData.ElementCount ElementbyID(int ID) Corrected capitalization, old code: MeshData.ElementbyID(Id), new code MeshData.ElementById(Id) NodebyID(int ID) Corrected capitalization, old code: MeshData.NodebyID(Id), new code MeshData.NodeById(Id) getConnectedElementIDs (int ID) Removed as incorrectly located and duplicated functionality; the method should be the responsibility of the Node object, old code: MeshData.getConnectedElementIDs(Id), new code MeshData.NodeById(Id).ConnectedElementIds() getConnectedElements (int ID) Removed as incorrectly located and duplicated functionality; the method should be the responsibility of the Node object, old code: MeshData.getConnectedElementIDs(ID), new code MeshData.NodeById(Id).ConnectedElements() getElementsByID(int[] ID) Consistency issue, old code: MeshData.getElementsByID (ID[]), new code MeshData.ElementsByIds(ID[]) Element(int Index) Duplication of python functionality. Old code MeshData.Element(0), new code MyArray = MeshData.Elements() then MyArray[0] (NB, using the shortcut MeshData.Elements()[index] in a loop is less efficient than assigning it to an array within python) Node(int Index) Duplication of python functionality. Old code MeshData.Node(0), new code MyArray = MeshData.Nodes() then MyArray[0] (NB, using the shortcut Mesh- 928 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Method/Property Description of Change Data.Nodes()[index] in a loop is less efficient than assigning it to an array within python) DAElement Class: The function TopologyID() related to an internal reference was previously documented in error. This has been removed from the documentation. Method/Property Description of Change Type() Replaced with property Description, this provides a text description of the element, rather than an internal number which was subject to change, old code: DAElement.Type(), new code DAElement.Description SectionData() Changed to property CrossSectionData, old code: DAElement.SectionData(), new code DAElement.CrossSectionData getNodeIDs() Consistency issue, old code: DAElement.getNodeIDs(), new code DAElement.NodeIds() ID() Changed to property Id, old code: DAElement.ID(), new code DAElement.Id NoOfConnectedNodes() Changed to property NodeCount, old code: DAElement.NoOfConnectedNodes(), new code DAElement.NodeCount DANode Class: Method/Property Description of Change ID() Changed to property Id, old code: DANode.ID(), new code DANode.Id x() Changed to property X, old code: DANode.x(), new code DANode.X y() Changed to property Y, old code: DANode.y(), new code DANode.Y z() Changed to property Z, old code: DANode.z(), new code DANode.Z NoOfConnectedElements() Changed to property ConnectedElementCount, old code: DANode.NoOfConnectedElements(), new code DANode.ConnectedElementCount ConnectedElementIDs() Corrected capitalization, old code: DANode.ConnectedElementIDs(Id), new code DANode.ConnectedElementIds(Id) SectionData Class: Method/Property Description of Change Type() Replaced with property Description, this provides a text description of the element, rather than an internal number which was subject to change, old code: SectionData.Type(), new code SectionData.Description Diameter() Changed to property TubeDiameter, old code: SectionData.Diameter(), new code SectionData.TubeDiameter Thickness() Changed to property TubeThickness, old code: SectionData.Thickness(), new code SectionData.TubeThickness WebThickness() Changed to property BeamWebThickness, old code: SectionData.WebThickness(), new code SectionData.BeamWebThickness Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 929 Features Method/Property Description of Change FlangeThickness() Changed to property BeamFlangeThickness, old code: SectionData.FlangeThickness(), new code SectionData.BeamFlangeThickness FilletRadii() Changed to property BeamFilletRadii, old code: SectionData.FilletRadii(), new code SectionData.BeamFilletRadii Height() Changed to property BeamHeight, old code: SectionData.Height(), new code SectionData.BeamHeight Width() Changed to property BeamWidth, old code: SectionData.Width(), new code SectionData.BeamWidth AttributeGroup Class: Method/Property Description of Change NoOfAttributes() Changed to property AttributeCount, old code: AttributeGroup.NoOfAttributes(), new code AttributeGroup.AttributeCount Name() Changed to property TreeName, old code: AttributeGroup.Name(), new code AttributeGroup.TreeName Type() Changed to property XmlType, old code: AttributeGroup.Type(), new code AttributeGroup.XmlType SubType() Changed to property XmlSubType, old code: AttributeGroup.SubType(), new code AttributeGroup.XmlSubType Attribute Class: Method/Property Description of Change Name() Changed to property AttributeName, old code: Attribute.Name(), new code Attribute.AttributeName Value() Replaced with the properties ValueAsInt, ValueAsDouble, ValueAsString in order to simplify the interface, old code: ValueObj = Attribute.Value() then ValueObj.GetAsInt(), new code: Attribute.ValueAsInt getNoOfSelectedElements() Changed to property SelectedElementCount, old code: Attribute.getNoOfSelectedElements(), new code Attribute.SelectedElementCount getSelectedElements() Consistency issue, old code: Attribute.getSelectedElements(), new code Attribute.SelectedElements() getNoOfSelectedNodes() Changed to property SelectedNodeCount, old code: Attribute.getNoOfSelectedNodes(), new code Attribute.SelectedNodeCount getSelectedNodes() Consistency issue, old code: Attribute.getSelectedNodes(), new code Attribute.SelectedNodes() SolutionSelection Class (previously named Selection): Method/Property Description of Change NoOfSolutions() Changed to property SolutionCount, old code: Selection.NoOfSolutions(), new code SolutionSelection.SolutionCount Solution(int index) Replaced with method SolutionByRow(int Row), Row is 1 based. Old code: Selection.Solution(0), new code SolutionSelection.SolutionByRow(1) 930 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Solution Class: Method/Property Description of Change NoOfAdditionalSolutionData() Changed to property AdditionalSolutionDataCount, old code: Solution.NoOfAdditionalSolutionData(), new code Solution.AdditionalSolutionDataCount EnvironmentName() Changed to property Id, old code: Solution.EnvironmentName(), new code Solution.Id getResult() This method and the object it returned have been removed and the objects functions replaced with properties within the Solution Class. Old code: Solution.getResult().ResultFilePath(), new code: Solution.ResultFilePath AdditionalSolutionData(int Index) Replaced with method AdditionalSolutionDataByColumn (int Col), Col is 1 based. Old code: Solution. AdditionalSolutionData(0), new code Solution.AdditionalSolutionDataByColumn(1) SolutionResult Class: Method/Property Description of Change ResultFilePath() Function moved to SolutionClass. Old code: Solution.getResult().ResultFilePath(), new code: Solution.ResultFilePath DAResult Class (previously named ResultGroup): Method/Property Description of Change Name() Changed to property TreeName, old code: ResultGroup.Name(), new code DAResult.TreeName Type() Changed to property XmlType, old code: ResultGroup.Type(), new code DAResult.XmlType AddStepResult() Renamed to AddDAResultSet, old code: ResultGroup.AddStepResult(), new code DAResult.AddDAResultSet() AddStepResult(Result myResult) Function has been removed, use AddDAResultSet to create the DAResultSet object then define values within that object. StepResult() Renamed to DAResultSets(), old code: ResultGroup.StepResult(), new code DAResult.DAResultSets() StepResult(int index) Renamed to DAResultSet(), old code: ResultGroup.StepResult(index), new code DAResult.DAResultSet(SetNumber). Note: SetNumber is 1 based. NoOfAttributes() Changed to property AttributeCount, old code: ResultGroup.NoOfAttributes(), new code DAResult. AttributeCount DAResultSet Class (previously named Result): Method/Property Description of Change AddElementResultValue(ValueStructureClass newElementResultValue) Modified so that it’s easier to create sets of result values. Now element result values can be directly defined using SetElementalValue. Old code Result.AddElementValue(ValueStructure), new code: DAResultSet.SetElementalValue(ElementID, Component, Value) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 931 Features Method/Property Description of Change ValueStructureClass AddElementResultValue() The ValueStructure class has been deprecated as the result values can be accessed directly. Values are also now added with a given ElementID, so numerous entries need not be made. Old code ValueStructure = Result.AddElementValue() then ValueStructure.setValue(Value), new code: DAResultSet.SetElementalValue(ElementID, Component, Value) ValueStructureClass[] ElementResultValues() The ValueStructure class has been deprecated as the result values can be accessed directly for the given element. It is no longer possible to get all the values out as an Array, but values can be obtained via GetElementalValue(ElementID, Component) instead. ValueStructureClass ElementResultValue(int index) The ValueStructure class has been deprecated as the result values can be accessed directly for the given element. Values are also now added with a given ElementID. Old code ValueStructure = Result. ElementResultValue(Index) then Value = ValueStructure.GetAsDouble(), new code: Value = DAResultSet.GetElementalValue(ElementID, Component) ValueStructure Class: This class has been deprecated; all functionality is now redundant as the values can either be obtained or set directly. DesignAssessment class This class is the parent class of all Design Assessment API objects that can be called from the python scripts. It is a global variable that can be accessed from anywhere in your script. Table 91 Members Name Type Description Helper Helper class See Helper class description for available properties and methods Units string Returns the solver units defined by the user in the analysis settings, represented as a string: MKS: i.e. Metric (m, Kg, N, s, V, A) UMKS: i.e. Metric (µm, Kg, µN, s, mV, mA) CGS: i.e. Metric (cm, g, dyne, s, V, A) NMM: i.e. Metric (mm, Kg, N, s, mV, mA) LBFT: i.e. US Customary (ft, lbm, lbf, s, V, A) LBIN: i.e. US Customary (in, lbm, lbf, s, V, A) MeshData MeshData class See MeshData class description for available properties and methods AttributeGroups() AttributeGroup[] class Array of AttributeGroup objects 932 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Name Type Description AttributeGroups(string TreeName) AttributeGroup[] class Array of AttributeGroup objects with the given TreeName filtered from the available AttributeGroups AttributeGroups(string Type, string SubType) AttributeGroup[] class Array of AttributeGroup objects with the given Type and SubType filtered from the available AttributeGroups SolutionSelections() SolutionSelection[] class Array of SolutionSelection class objects DAResults() DAResult[] class Array of DAResult objects DAResults(string TreeName) DAResult[] class Array of DAResult objects with the given TreeName filtered from the available DAResults DAResults(string Type, string SubType) DAResult[] class Array of DAResult objects with the given Type and SubType filtered from the available DAResults AttributeGroupCount int A count of the number of AttributeGroup objects SolutionSelectionCount int A count of the number of SolutionSelection objects DAResultCount int A count of the number of DAResult objects ProjectTitle string The title of the project OutputDeprecatedWarnings(bool ShowWarnings) void Sets the verbosity of the warnings related to deprecated properties/methods: False – for no output True – for full output for each call Warnings are presented as text output to the solve or evaluate debug logs. By default only a summary is shown; the user can then decide to add this function to their script to display them all, or display none. Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_DesignAssessment(): DA = DesignAssessment #just to save typing. #To know full details of deprecated functions. DA.OutputDeprecatedWarnings(True) #Get the helper object HelperObject = DA.Helper #Output units string, e.g. MKS print DA.Units # Get the MeshData object MeshDataObject = DA.MeshData print DA.ProjectTitle Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 933 Features #Attribute Groups: #Obtain an array of all attribute group objects. AllAttributeGroupsObjects = DA.AttributeGroups() #Filter for an array of attribute group objects called Bob NameFilterAttributeGroupsObject = DA.AttributeGroups("Bob") #Filter for an array of attribute groups with type Sam, subtype Phil TypeFilterAttributeGroupsObject = DA.AttributeGroups("Sam", "Phil") #Returns the total number of attribute groups print str(DA.AttributeGroupCount) #Solution Selection: #Obtain all solution selection objects AllSolutionSelections = DA.SolutionSelections() #DA Results: #Obtain an array of all DA Result objects. AllDAResultsObjects = DA.DAResults() #Filter for an array of DA Result objects called John NameFilterDAResultsObject = DA.DAResults("John") #Filter for an array of DA Result with with type Paul, subtype Mike TypeFilterDAResultsObject = DA.DAResults("Paul", "Mike") #Returns the total number of DA Result objects print str(DA.DAResultCount) #Access first object in NameFilterAttributeGroupsObject array if (NameFilterAttributeGroupsObject != None): AGObjectA = NameFilterAttributeGroupsObject[0] #Example Loop around Array AllAttributeGroupsObjects for AGObject in AllAttributeGroupsObjects: #Now AGObject is a representation of each Attribute Group. print AGObject.TreeName runClassDemo_DesignAssessment() Typical Evaluate (or Solve) Script Output The output will depend upon the number of Attribute Group and DA Result objects defined and used in the model. MKS HelpFileExample--Design Assessment (B5) 1 1 Attribute Group Helper class This class provides some general functions to assist the user writing scripts. Table 92 Members Name Type Description GeometryPath string Returns the directory where the Geometry file is saved. ResultPath string Returns the directory where the Result files should be written. During the solving process this can be an intermediate directory, not the project system directory. SystemDirectory string Returns the project system directory. UserFilesDirectory string Returns the user_files directory for the current project. 934 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Name Type Description RunMAPDL(string input, string output, string CommandLineParams) void Runs an instance of the Mechanical APDL solver. You must provide file names which may include the full path or may be in the application or current directory for input and output. Specify any additional MAPDL command line parameters for CommandLineParams, or a blank string if none are required. SetLastError(string errorString) void Sets the text message to show in the output messages of the editor. This can be used to present a message to the user of the script for a reason for failure, ReplaceSolverOutputFile(string FileLoc) void Specifies a text file produced during output to replace the default solve.out log file. The solve.out log file will be shown in the Solution Information Worksheet view if selected from the drop down. SolverOutputFilePath string Gets the file name and path of the file that is displayed when the Solution Output displays the Solver Output data. AppendToSolverOutputFile(string AdditionalText) void Appends a line of text to the Solver Output display. ClearSolverOutputFile() void Deletes contents of the Solver Output File. Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_Helper(): HelperObject = DesignAssessment.Helper #Get the helper object #Obtain some Helper based properties and print them to the debug file. print "GeometryPath = " + HelperObject.GeometryPath print "ResultPath = " + HelperObject.ResultPath print "SystemDirectory = " + HelperObject.SystemDirectory print "SolverOutputFilePath = " + HelperObject.SolverOutputFilePath #Use some Helper based design assessment methods #Create a text file with write access in the result path location NewSolverFilePathAndName = HelperObject.ResultPath+"\\MySolverFile.txt" MySolverFile = open(NewSolverFilePathAndName, "w") MySolverFile.write("This is a solver output file\n") MySolverFile.write("The backslash n indicates the end of a line\n") MySolverFile.close() #Make the solver output file text to be that contained in the MySolverFile HelperObject.ReplaceSolverOutputFile(NewSolverFilePathAndName) #uncomment out the below line to clear the previously entered text #HelperObject.ClearSolverOutputFile() #Append some more text, note this automatically includes the new line code. HelperObject.AppendToSolverOutputFile("My First Additional Line") HelperObject.AppendToSolverOutputFile("My Second Additional Line") runClassDemo_Helper() Typical Evaluate (or Solve) Script Output GeometryPath = D:\Data\Documents\HelpFileExample_files\dp0\SYS\DM\SYS.agdb ResultPath = D:\Data\Documents\HelpFileExample_files\dp0\SYS-1\MECH\ SystemDirectory = D:\Data\Documents\HelpFileExample_files\dp0\SYS-1\MECH\ SolverOutputFilePath = D:\Data\Documents\HelpFileExample_files\dp0\SYS-1\MECH\solve.out Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 935 Features Typical Solver Output This is a solver output file The backslash n indicates the end of a line My First Additional Line My Second Additional Line MeshData class This class provides access to the mesh created for the analysis, including all elements and nodes, which can be filtered or obtained as required. Table 93 Members Name Type Description NodeCount int Total of number of nodes in this mesh ElementCount int Total of number of elements in this mesh ElementById(int Id) DAElement class Obtains the DAElement class object with the given Id. Represents a single element in the Mesh. Elements() DAElement[] class Array of all DAElement class objects. representing all the elements in the mesh NodeById(int Id) DANode class Obtains the DANode class object with the given Id. Represents a single node in the Mesh Nodes() DANode[] class Array of all DANode class objects representing all the nodes in the mesh NodesByIds (int[] Ids) DANode[] class Array of DANode class objects that belong to any of the array of element Ids specified in ids. ElementsByIds(int[] Ids) DAElement[] class Array of DAElement class objects that belong to any of the array of element Ids specified in Ids. Example Usage The following example can be used as a basis of either the solve or evaluate script. #we need to use arrays for the ElementsByIds and NodesByIds methods from System import Array def runClassDemo_MeshData(): MeshDataObject = DesignAssessment.MeshData #Get the MeshData object #Output some data to the debug log file. print "Number of Nodes = " + str(MeshDataObject.NodeCount) print "Number of Elements = " + str(MeshDataObject.ElementCount) #Loop around all element objects. for ElementIterator in MeshDataObject.Elements(): print "ElementId = " + str(ElementIterator.Id) #Three ways of getting elements. #It can not be assumed that Element Ids start at 1 and are contiguous Elements = MeshDataObject.Elements() FirstElementId = Elements[0].Id ByIdMethodElement = MeshDataObject.ElementById(FirstElementId) # print true if they are the same Id. print str(FirstElementId == ByIdMethodElement.Id) # Create an Array so we can iterface with the .NET code ElementIdArray = Array[int]([FirstElementId,MeshDataObject.Elements()[1].Id]) print ElementIdArray #Pass the array into the ElementsById method. 936 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment ByIdArrayMethodElement = MeshDataObject.ElementsByIds(ElementIdArray) # print true if they are the same Id. print str(FirstElementId == ByIdArrayMethodElement[0].Id) #Three ways of getting nodes. #It can not be assumed that Node Ids start at 1 and are contiguous Nodes = MeshDataObject.Nodes() FirstNodeId = Nodes[0].Id ByIdMethodNode = MeshDataObject.NodeById(FirstNodeId) # print true if they are the same Id. print str(FirstNodeId == ByIdMethodNode.Id) # Create an Array so we can iterface with the .NET code NodeIdArray = Array[int]([FirstNodeId,MeshDataObject.Nodes()[1].Id]) print NodeIdArray #Pass the array into the NodesById method. ByIdArrayMethodNode = MeshDataObject.NodesByIds(NodeIdArray) # print true if they are the same Id. print str(FirstNodeId == ByIdArrayMethodNode[0].Id) runClassDemo_MeshData() Typical Evaluate (or Solve) Script Output The output will depend upon the mesh used in the model. Number of Nodes = 457 Number of Elements = 236 ElementId = 237 ElementId = 238 .... ElementId = 470 ElementId = 471 ElementId = 472 True Array[int]((237, 238)) True True Array[int]((1, 3)) True DAElement class This class represents an element on the mesh for this model, providing access to the element, its connectivity and, if it is a beam or tube, the associated section data. Table 94 Members Name Type Description Description string A description of the element: Tetrahedral Hexagonal Wedge Pyramid Triangle Triangle,Shell Quadrilateral Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 937 Features Name Type Description Quadrilateral,Shell Line Point EMagLine EMagArc EMagCircle Surface Edge Beam Special CrossSectionData SectionData class Section data for this element, describes beam cross sections for beam types; Only elements that have a Circular Hollow Section, Rectangular Hollow Section or I Section are supported, all other elements will return NULL NodeIds() int[] Array of integer values representing Ids of the Element’s Nodes Nodes() DANode[] class Array of DANode class objects for each node of this Element Id int Returns the unique Id number of this Element NodeCount int Returns the number of Nodes for this Element ElementThickness double The shell thickness of the element. If the element is not a shell, the value returned will be zero. Where shell thickness can be applied via geometry or by a Shell Thickness object, that defined by the Shell Thickness will take precedence. ElementThicknessAtNode(NodeId) double The shell thickness of the element at position of Node with NodeId. If the element is not a shell, the value returned will be zero. Where shell thickness can be applied via geometry or by a Shell Thickness object, that defined by the Shell Thickness 938 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Name Type Description will take precedence. If shell thickness varies across the element then it is determined by the average thickness of the element nodes. Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_DAElement(): #Loop around all element objects. for ElementIterator in DesignAssessment.MeshData.Elements(): #General info: print "Element Description = " + ElementIterator.Description print "Element Id = " + str(ElementIterator.Id) # Information about the nodes of the element print "Number of connected Nodes = " + str(ElementIterator.NodeCount) NodeIdArray = ElementIterator.NodeIds() print NodeIdArray ConnectedNodeObjects = ElementIterator.Nodes() #Cross Section Data is only available for beams. #First test to see if it's a beam as they support it. if 'Beam' in ElementIterator.Description: XSectionDataObj = ElementIterator.CrossSectionData #Element Thickness only applies to some elements, returns 0.0 if not supported. print "Element Thickness = " + str(ElementIterator.ElementThickness) ThicknessAtNode = ElementIterator.ElementThicknessAtNode(NodeIdArray[0]) print "Thickness at Node Id " + str(NodeIdArray[0]) + " = " + str(ThicknessAtNode) runClassDemo_DAElement() Typical Evaluate (or Solve) Script Output The output will depend upon the elements used in the model; this output is for beams. Element Description = Beam Element Id = 237 Number of connected Nodes = 3 Array[int]((1, 3, 222)) Element Thickness = 0.0 Thickness at Node Id 1 = 0.0 DANode class This class represents a node on the mesh for this analysis. It can be used to find the coordinates of the node and the elements that it is connected to. Table 95 Members Name Type Description Id int Returns the unique Id number of this Node X double Returns the x coordinate of this Node in solver units as set in Analysis settings Y double Returns the y coordinate of this Node in solver units as set in Analysis settings Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 939 Features Name Type Description Z double Returns the z coordinate of this Node in solver units as set in Analysis settings ConnectedElementIds() int[] Array of integer values representing Ids of the connected Elements ConnectedElements() DAElement[] class Array of DAElement class objects that represent the elements that this Node is connected to ConnectedElementCount int Returns the number of Elements this node is connected to IsOrientationNode bool Some beam nodes are created to orient the local axis system for the section; if this node is used for orientation this function will return true Note: results cannot be displayed on orientation nodes Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_DANode(): #Loop around all nodes. for NodeIterator in DesignAssessment.MeshData.Nodes(): #General info: print "Node Id = " + str(NodeIterator.Id) print "Node X = " + str(NodeIterator.X) print "Node Y = " + str(NodeIterator.Y) print "Node Z = " + str(NodeIterator.Z) print "Node only used for beam orientation? " + str(NodeIterator.IsOrientationNode) # Information about the elements that connect to this node print "Number of connected Elements = " + str(NodeIterator.ConnectedElementCount) ElementIdArray = NodeIterator.ConnectedElementIds() print "Connected Element Ids = " + str(ElementIdArray) ConnectedElementObjects = NodeIterator.ConnectedElements() runClassDemo_DANode() Typical Evaluate (or Solve) Script Output The output will depend upon the nodes used in the model. Node Id = 1 Node X = -2.0 Node Y = 4.4408920985e-16 Node Z = 5.0 Is the node only used for beam orientation? False Number of connected Elements = 4 Connected Element Ids = Array[int]((408, 400, 245, 237)) SectionData class This class provides Section Data properties for a beam based element in solver units as set in Analysis settings. It can be accessed via DAElement. Table 96 Members Name Type Description Description string Returns a description of the type of cross section: 940 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Name Type Description CHS,Tube I,Beam RHS,Beam TubeDiameter double Returns the Diameter as double, only applicable to sections that are tubular TubeThickness double Returns the Thickness as double, only applicable to sections that are tubular BeamWebThickness double Returns the WebThickness as double, only applicable to sections that are beam based BeamFlangeThickness double Returns the FlangeThickness as double, only applicable to sections that are beam based BeamFilletRadii double Returns the FilletRadii as double, only applicable to sections that are beam based BeamHeight double Returns the Height as double, only applicable to sections that are beam based BeamWidth double Returns the Width as double, only applicable to sections that are beam based Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_SectionData(): #Loop around all element data objects. for ElementIterator in DesignAssessment.MeshData.Elements(): #Cross Section Data is only available for beams. #First test to see if it's a beam as they support it. if 'Beam' in ElementIterator.Description: XSectionData = ElementIterator.CrossSectionData print XSectionData.Description if 'Tube' in XSectionData.Description: print "Diameter = " + str(XSectionData.TubeDiameter) print "Thickness = " + str(XSectionData.TubeThickness) if 'Beam' in XSectionData.Description: print "Web Thickness = " + str(XSectionData.BeamWebThickness) print "Flange Thickness = " + str(XSectionData.BeamFlangeThickness) print "Fillet Radii = " + str(XSectionData.BeamFilletRadii) print "Height = " + str(XSectionData.BeamHeight) print "Width = " + str(XSectionData.BeamWidth) runClassDemo_SectionData() Typical Evaluate (or Solve) Script Output The output will depend upon the elements used in the model; this output is for a tube and a beam. CHS,Tube Diameter = 0.5 Thickness = 0.01 I,Beam Web Thickness = 0.01 Flange Thickness = 0.01 Fillet Radii = 0.03 Height = 0.65 Width = 0.5 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 941 Features AttributeGroup class This class represents the Attribute Group entries in the tree view and provides access to the data entered. This tree object is defined in the AttributeGroups section of the XML definition file. Table 97 Members Name Type Description Attributes() Attribute[] class Array of all the Attribute class objects held under this AttributeGroup Attribute(int index) Attribute class An Attribute class object at the index as defined in the AttributeIDs field in the XML definition file. Index is zero based. Attribute(string XMLName) Attribute class An Attribute class object of the name defined in the XML definition file, from the Attribute array AttributeCount int The number of Attribute class objects in the Attribute array TreeName string The name of this AttributeGroup as defined by the user in the user interface XmlType string The Type of this AttributeGroup as defined in the XML definition file XmlSubType string The Sub Type of this AttributeGroup as defined in the XML definition file Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_AttributeGroups(): #Loop around all attribute group objects. for AGIterator in DesignAssessment.AttributeGroups(): #Attribute Group info print "Name = " + AGIterator.TreeName print "Type = " + AGIterator.XmlType print "Subtype = " + AGIterator.XmlSubType #Obtaining contained attributes print "No of Attributes = " + str(AGIterator.AttributeCount) Index = 0 for AttributeIterator in AGIterator.Attributes(): #Get the name of this attribute AName = AttributeIterator.AttributeName #Get the attribute, based on the index AttributeMethod1 = AGIterator.Attribute(Index) #Get the attribute, based on the Name, it's easier to look up by name. AttributeMethod2 = AGIterator.Attribute(AName) print "Attribute Name: " + AName print "Check names are the same: " + str(AName == AttributeMethod1.AttributeName) print "Are attrib. objects the same: " + str(AttributeMethod1 == AttributeMethod2) #Add to the index (there are more concise ways of doing this in a loop) Index = Index + 1 runClassDemo_AttributeGroups() Typical Evaluate (or Solve) Script Output The output will depend upon the XML definition file used in the model and the attribute groups used. 942 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Name = Attribute Group Type = Geometry Factor Subtype = My Factors No of Attributes = 1 Attribute Name: Factor Check names are the same: True Are attrib. objects the same: True Attribute class This class provides access to the input provided for each attribute in the attribute group. The attributes are defined in the Attributes section of the XML definition file. Table 98 Members Name Type Description AttributeName int The name of this Attribute ValueAsInt int Returns the value entered as an integer; double values will be truncated. Accepted input is determined by the XML definition file. ValueAsDouble double Returns the value entered as a double. Accepted input is determined by the XML definition file. ValueAsString string Returns the value entered as text; if the value is numerical, it will automatically be converted to text. Accepted input is determined by the XML definition file. SelectedElementCount int Returns the number of elements included in the selected geometry SelectedElements() DAElement[] class Returns an array of DAElements included in the selected geometry SelectedNodeCount int Returns the number of nodes included in the selected geometry SelectedNodes() DANode[] class Returns an array of DANodes included in the selected geometry Note The functions SelectedNodes and SelectedElements will return None if no geometry is specified. These functions, plus the SelectedNodeCount and SelectedElementCount are only valid if the <Application> field in the attributes section of the XML definition file is used to enable geometry selection. Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_Attributes(): #Loop around all attribute group objects for AGIterator in DesignAssessment.AttributeGroups(): for AttributeIterator in AGIterator.Attributes(): #Get info about the attribute print "Attribute Name = " + AttributeIterator.AttributeName print "Value via ValueAsInt = " + str(AttributeIterator.ValueAsInt) print "Value via ValueAsDouble = " + str(AttributeIterator.ValueAsDouble) print "Value via ValueAsString = " + AttributeIterator.ValueAsString Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 943 Features print "No Elements in Selection = " + str(AttributeIterator.SelectedElementCount) print "1st Element in Selection = " + str(AttributeIterator.SelectedElements()[0]) print "No of Nodes in Selection = " + str(AttributeIterator.SelectedNodeCount) print "First Node in Selection = " + str(AttributeIterator.SelectedNodes()[0]) runClassDemo_Attributes() Typical Evaluate (or Solve) Script Output The output will depend upon the XML definition file used in the model and the attributes and attribute groups used. Attribute Name = Factor Value via ValueAsInt = 1 Value via ValueAsDouble = 1.0 Value via ValueAsString = 1 No Elements in Selection = 236 1st Element in Selection = <Ans.Simulation.DesignAssessmentAssembly.DAElementClass object at 0x000000000000002B [Ans.Simulation.DesignAssessmentAssembly.DAElementClass]> No of Nodes in Selection = 221 First Node in Selection = <Ans.Simulation.DesignAssessmentAssembly.DANodeClass object at 0x000000000000002C [Ans.Simulation.DesignAssessmentAssembly.DANodeClass]> SolutionSelection class This class represents the Solution Selection object in the tree view and provides access to the Solutions entered in the Worksheet view. Each solution represents an upstream analysis. Table 99 Members Name Type Description Solutions() Solution[] class Array of all the Solution class objects held under this Solution Selection, each being a row of the table. SolutionByRow(int row) Solution class A Solution class object at the given row in the SolutionSelections worksheet, a one based value, so to obtain the Solution class object for the first row, enter 1 SolutionCount int The number of Solution class objects in the Solutions array Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_SolutionSelection(): #Loop around all solution selection objects (NB only 1 currently supported) for SolutionSelectionIterator in DesignAssessment.SolutionSelections(): print "No of Solutions in selection = " + str(SolutionSelectionIterator.SolutionCount) print "1st row in Solseln = " + str(SolutionSelectionIterator.SolutionByRow(1).Id) for SolutionIterator in SolutionSelectionIterator.Solutions(): print "Id for solution = " + str(SolutionIterator.Id) runClassDemo_SolutionSelection() Typical Evaluate (or Solve) Script Output The output will depend upon the XML definition file used in the model and the attributes and attribute groups used. No of Solutions in selection = 1 1st row in Solseln = 23 Id for solution = 23 944 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Solution class This class represents a row in the Worksheet of the Solution Selection tree object. Table 100 Members Name Type Description AdditionalSolutionData() string[] Array of strings representing all the additional data entered in to the Solution Selection table additional data columns AdditionalSolutionDataByColumn(int Column) string The string object at the Column of the AdditionalSolutionData AdditionalSolutionDataCount int The number of AdditionalSolutionData text files in the AdditionalSolutionData array Id int The unique Id number for the solution. Solution Id’s do not change once the solution is created. Type string The type of solution as defined by the description: Static Structural Transient Structural Explicit Dynamics Modal Harmonic Response Random Vibration Response Spectrum CreateSolutionResult() SolutionResult class Create a new result based on this analysis system. Returns the created object. CreateSolutionResult(string Name) SolutionResult class Create a new result of the given Name based on this analysis system. Returns the created object. CreateSolutionResult(string Name, string Expression, string ResultType) SolutionResult class Create a new result of the given Name, Expression and ResultType based on this analysis system. Returns the created object. ResultType string should be set to one of the values listed for DisplayUnits keyword in the DAResult section of the XML definition file. SolutionResults() SolutionResult[] class Array of results containing all the result objects. SolutionResults(string Name) SolutionResult[] class Array of results containing specific results filtered on the given Name. Units string Returns the Units used in this solution, represented as a string: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 945 Features Name Type Description CGS NMM LBFT LBIN UMKS MKS No Units System ResultFilePath string String representing the solution combination result file path (rst file) for the loadcase. Time double Gets the value of time that has been entered by the user in the table, if applicable. Freq double Gets the value of frequency that has been entered by the user in the table, if applicable. Coefficient double Gets the Coefficient entered by the user. Phase double Gets the value of Phase Angle that has been entered by the user in the table, if applicable. Mode int Gets the value of Mode that has been entered by the user in the table, if applicable. Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_Solution2(): #Get all results called bob and set the expression to SX. AllBobs = DesignAssessment.SolutionSelections()[0].SolutionByRow(1).SolutionResults("Bob") for BobResultIter in AllBobs: print "Bob found at " + str(BobResultIter) BobResultIter.Expression = "SX" def runClassDemo_Solution(): #Get the first entered upstream solution. UpstreamSoln = DesignAssessment.SolutionSelections()[0].SolutionByRow(1) #Get properties that identify this solution. print "Id = " + str(UpstreamSoln.Id) print "Type = " + str(UpstreamSoln.Type) #Get properties defined for this entry in the solution selection worksheet print "Time = " + str(UpstreamSoln.Time) print "Frequency = " + str(UpstreamSoln.Frequency) print "Phase = " + str(UpstreamSoln.Phase) print "Mode = " + str(UpstreamSoln.Mode) print "Coefficient = " + str(UpstreamSoln.Coefficient) print "Result File Path = " + str(UpstreamSoln.ResultFilePath) print "Units system used = " + str(UpstreamSoln.Units) #XML defined properties in the solution selection worksheet print "Number of Additional strings = " + str(UpstreamSoln.AdditionalSolutionDataCount) print "Additional strings = " + str(UpstreamSoln.AdditionalSolutionData()) print "Additional string, col 1 = " + str(UpstreamSoln. AdditionalSolutionDataByColumn(1)) #Create a new result object for this solution 946 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment #this object can then be used directly to set expressions, etc. MyResult = UpstreamSoln.CreateSolutionResult() #Use the Name for identification, #useful to obtain the results in another subroutine in python. MyBobResult = UpstreamSoln.CreateSolutionResult("Bob") MyFredResult = UpstreamSoln.CreateSolutionResult("Fred") My2ndBobResult = UpstreamSoln.CreateSolutionResult("Bob") #Define expression at same time as creating the result. MySXDefinedResult = UpstreamSoln.CreateSolutionResult("FredSX","sx") runClassDemo_Solution() Typical Evaluate (or Solve) Script Output The output will depend upon the XML definition file used in the model and the attributes and attribute groups used. Id = 23 Type = Static Structural Time = 1.0 Frequency = 0.0 Phase = 0.0 Mode = 0 Coefficient = 1.0 Result File Path = D:\Data\Documents\HelpFileExample_files\dp0\SYS\MECH\file.rst Units system used = MKS Number of Additional strings = 1 Additional strings = Array[str](('')) Additional string, col 1 = Bob found at <Ans.Simulation.DesignAssessmentAssembly.SolutionResultClass object at 0x000000000000002D [Ans.Simulation.DesignAssessmentAssembly.SolutionResultClass]> Bob found at <Ans.Simulation.DesignAssessmentAssembly.SolutionResultClass object at 0x000000000000002E [Ans.Simulation.DesignAssessmentAssembly.SolutionResultClass]> SolutionResult class This class holds the solution result data that can be accessed, directly related to the solution. The solution result class will be initialized with the unit system specified for the Design Assessment analysis. Only when a valid unit system and type are set will results obtained be converted correctly to the expected result units. Results are organized in sets; each set contains the results at a given time, frequency, etc. depending upon the analysis type. It is more efficient to get all the required results at a given set, before changing sets. For convenience the set can be identified automatically by defining a time or frequency. If the value is not exact then the results will be interpolated from the adjacent values. If the value cannot be obtained (for example, requesting elemental values for a nodal result), the maximum value for a double type is returned (1.79769e+308). Note DefineCoordinateSystem and CoordinateSystem are mutually exclusive; if both are used, the last one defined takes precedence. Table 101 Members Name Type Description Name string Gets or sets the name of the result, so that it can be found from the solution class. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 947 Features Name Type Description ElementNodalValues(int ElementId, int NodeId) double[] Array of values of an element nodal result at the given ElementId and NodeId. The size of the returned array will depend upon the number of result components. If required, this can be determined using ComponentCount or the python len() function. ElementalValues(int ElementId) double[] Array of values of an element result at the given ElementId. The size of the returned array will depend upon the number of result components. If required, this can be determined using ComponentCount or the python len() function. NodalValues(int NodeId) double[] Array of values of a nodal result at the given NodeId. The size of the returned array will depend upon the number of result components. If required, this can be determined using ComponentCount or the python len() function. DisplayStyle string Returns the DisplayStyle: i.e. if it’s a Vector, Tensor, Scalar, etc. The returned string can be used to programmatically set the ResultGroup’s DisplayStyle. Note: the returned value is dependent on provided Expression and IntegrationMethod, so these should be called beforehand. DisplayType string Returns the DisplayType: i.e. if it’s a Nodal, Elemental or ElementNodal result. The returned string can be used to programmatically set the ResultGroup’s DisplayType. Note: the returned value is dependent on provided Expression and IntegrationMethod, so these should be called beforehand. ComponentCount int Returns the number of components for this result, typically 1, 3, or 6. Note: the returned value is dependent on provided Expression and IntegrationMethod, so these should be called beforehand. ResultSetCount int Returns the total number of results sets for this system. The Result Set count is read directly from the underlying file containing the results.. Expression string Set the expression by assigning a string. Valid expressions are the same as those used for user defined results and can include mathematical modifiers. CoordinateSystem string Sets the coordinate system type by assigning a string. Valid inputs are either the name of a user coordinate system in the 948 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Name Type Description Mechanical application or one of the following: Global (default) Solution The solution coordinate system is generally associated with beam based results. DefineCoordinateSystem(string Axes, double Axis1X, double Axis1Y, double Axis1Z, double Axis2X, double Axis2Y, double Axis2Z, double OriginX, double OriginY, double OriginZ) void Defines a custom coordinate system orientation matrix to obtain results in. Use as an alternative to CoordinateSystem to enable an axis to be defined directly in the python code. Axes is one of the following strings used to define what two axes of the orientation matrix are being entered, the third axis is calculated automatically. XY YZ ZX SetUnitsSystem(string UnitsSystem, string RotationUnit, string TemperatureUnit) void Defines the units system that the results are to be obtained in. If a string is blank, then the default is assumed. Options for UnitsSystem are: MKS: i.e. Metric (m, Kg, N, s, V, A), (Default) UMKS: i.e. Metric (µm, Kg, µN, s, mV, mA) CGS: i.e. Metric (cm, g, dyne, s, V, A) NMM: i.e. Metric (mm, Kg, N, s, mV, mA) LBFT: i.e. US Customary (ft, lbm, lbf, s, V, A) LBIN: i.e. US Customary (in, lbm, lbf, s, V, A) Options for RotationUnit are: Degrees Radians (Default) Options for TemperatureUnit are: Kelvin Celsius (Default for metric systems) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 949 Features Name Type Description For US Customary, Fahrenheit is always used and the entered value is ignored. ResultType string Gets or Sets the ResultType. ResultType string should be set to one of the values listed for DisplayUnits keyword in the DAResult section of the XML definition file. No Units is the default value. If not set or left as default No Units, any results obtained will not be unit converted to the appropriate units for the Design Assessment system. IntegrationMethod string Defines the integration method used when obtaining results by assigning a string. Valid options are: UnAveraged Averaged (default) Nodal Difference Nodal Fraction Elemental Mean Elemental Difference Elemental Fraction Different Integration options can affect the DisplayType. ResultSet int Defines the set that data is obtained from by assigning an integer value. It is recommended that this method is used to specify which results are to be obtained for Modal, Spectrum, and Response Spectrum analyses. Assigning 0 will obtain data from the last result set in the analysis. Default is based on the entry in the Solution Selection table. ResultTimeFrequency double Defines the time or frequency that data is obtained from by assigning a real number to indicate the time or frequency. Whether it is defining Time or Frequency1 is determined automatically from the analysis type. 950 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Name Type Description Assigning 0.0 will obtain data from the last time or frequency in the analysis. If the analysis is time or frequency independent then the ResultSet property can be used instead. Default is based on the entry in the Solution Selection table. ShellLayer int Define the layer for which to obtain results. In the case of composite sections, assigning ShellLayer to a positive integer can be used to define the layer number. Alternatively, assign 0 for the whole section; this is default behavior. See also ShellFaceResultDisplay. Only applicable to shell elements. ShellFaceResultDisplay string Define what results are displayed on the faces of shell elements by assigning a string. Valid entries are: Top (i.e. results calculated for the top face on both faces) Bottom (i.e. results calculated for the bottom face on both faces) Middle (i.e. calculated middle values on both faces - see Surface Body Results (p. 727) for details) Only applicable to shell elements. 1 - Obtaining frequency based results is not presently supported. Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_SolutionResult(): #Create a scripted, user defined, result MyRes = DesignAssessment.SolutionSelections()[0].SolutionByRow(1).CreateSolutionResult() #Define what result we're obtaining. MyRes.Expression = "UX" #You can specify the solution or Global system.. MyRes.CoordinateSystem = "Solution" #Alternatively, define a coordinate system directly. #The last CS defined takes precidence. #MyRes.DefineCoordinateSystem("ZX",1,0,0,0,1,0,0,0,0) #Define the units sytem and the units type to convert the results. #MyRes.SetUnitsSystem("UMKS","Radians","Celsius","Distance") #Define the method of integrating the results, this can affect the result type. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 951 Features #MyRes.IntegrationMethod = "UnAveraged" #Set the time or set for the results that we want to obtain, #last one defined takes precidence. MyRes.ResultSet = 0 MyRes.ResultTimeFrequency = 0 #Get some info about this result DS = MyRes.DisplayStyle print DS DT = MyRes.DisplayType print DT NC = MyRes.ComponentCount print NC NRS = MyRes.ResultSetCount print NRS #Loop around all elements objects. for ElementIter in DesignAssessment.MeshData.Elements(): print "Element Values = " + str(MyRes.ElementalValues(ElementIter.Id)) for NodeIter in ElementIter.Nodes(): Values = str(MyRes.ElementNodalValues(ElementIter.Id,NodeIter.Id)) print "Element Nodal Result Values = " + Values #Loop around all node objects. for NodeIterator in DesignAssessment.MeshData.Nodes(): print "Node Result Values = " + str(MyRes.NodalValues(NodeIterator.Id)) runClassDemo_Solution() Typical Evaluate (or Solve) Script Output The output will depend upon the model. Scalar Nodal 1 1 Element Value = Array[float](( 1.7976931348623157e+308)) Element Nodal Result Values = Array[float]((-2.5374282230927747e-08)) Element Nodal Result Values = Array[float]((-1.6870160379767185e-08)) Element Nodal Result Values = Array[float]((-9.8640562384844088e-09)) .... Node Result Values = Array[float]((-4.6618247040441929e-08)) Node Result Values = Array[float]((-3.7071398395482902e-08)) Node Result Values = Array[float]((-2.8261506912485856e-08)) .... DAResult class This class provides access to the results objects, and enables the user to set the results that are to be displayed when the result object is selected. The DAResult is defined in the DAResults section of the XML definition file. Table 102 Members Name Type Description TreeName string Returns the user defined name of this result instance XmlType string Returns the text string of the Type of this result instance; the Type is set in the user interface by a drop down list (as defined in the XML definition file) XmlSubType string Returns the text string of the Sub Type of this result instance; the Sub Type is set in the user interface by a drop down list (as defined in the XML definition file) 952 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Name Type Description DAResultSetCount int Total number of sets that are available for this result; at present only one set is supported CreateDAResultSet() DAResultSet class Creates a new result set and returns it so that values can be defined within it DisplayStyle and DisplayType will be read from values in the XML definition file, or if multiple DAResultSets are created, they’ll be read from the first set. CreateDAResultSet(string DAResultSet class DisplayStyle, string DisplayType) Creates a new result set and returns it so that values can be defined within it overrides the DisplayStyle entered in the XML definition file for this result group. However, unlike the XML definition file setting, defining it here does not enable the option to choose the component in the user interface of the DA Result object. However, this option can be used to force the display to show either a Vector or Tensor result; 3 or 6 component values should be defined accordingly. DisplayStyle strings should be set to one of the values listed for the DisplayStyle keyword in the DAResult section of the XML definition file. DisplayType overrides the DisplayType entered in the XML definition file, and should be a valid DisplayType keyword in the DAResult section of the XML definition file. DAResultSets() DAResultSet[] class Returns an array of DAResultSets classes from the DAResultSet collection for this DAResult; at present only the first set is used in result display DAResultSet(int SetNumber) DAResultSet class Returns a single DAResultSet object for the given SetNumber . SetNumber is 1 based and incremented automatically with each set that is added. AttributeCount() int Total number of Attributes objects defined Attributes() Attribute[] class Array of Attribute class objects; the Attribute collection for this DAResult as Attribute class type Attribute(string XMLName) Attribute class An Attribute class object of the name defined in the XML definition file, from the Attribute array Attribute(int index) Attribute class An Attribute class object at the index as defined in the AttributeIDs field in the XML definition file. Index is zero based. DisplayStyle string Gets the type of display, as defined in the XML definition file, or as defined when creating a result set; Scalar, Vector, Tensor, or StrainTensor. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 953 Features Name Type Description DisplayType string Gets the type of display, as defined in the XML definition file or as defined when creating a result set; Elemental, Nodal, or ElementNodal. DisplayUnits string Gets or sets the DisplayUnits set programmatically. By default it’s obtained from the display units set via the XML definition file for this DAResult. If setting it, the string should be set to one of the values listed for DisplayUnits keyword in the DAResult section of the XML definition file. IsUpToDate bool This will return true if the DAResult is currently Up To Date, otherwise it will return false. Note A DAResult that is currently Up To Date is in a read-only state, and therefore its properties and results can not be modified. In order to modify the DAResult, you will need to clear it via the User Interface before solving or evaluating. Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_DAResult(): for DAResultIter in DesignAssessment.DAResults(): #General info: print "Name = " + DAResultIter.TreeName print "XmlType = " + DAResultIter.XmlType print "XmlSubType = " + DAResultIter.XmlSubType #Show and modify display options. print "Initial DisplayType = " + DAResultIter.DisplayType print "Initial DisplayStyle = " + DAResultIter.DisplayStyle print "Initial DisplayUnits = " + DAResultIter.DisplayUnits DAResultIter.DisplayUnits = "Stress" print "New DisplayUnits = " + DAResultIter.DisplayUnits #Attribute access: print "Number of Attributes = " + str(DAResultIter.AttributeCount) myAttribute = DAResultIter.Attribute(0) myAttributeByName = DAResultIter.Attribute("Mathematical Operator") print "Are they the same? = " + str(myAttribute == myAttributeByName) print "All attributes = " + str(DAResultIter.Attributes()) NewSet = DAResultIter.CreateDAResultSet() GetSet = DAResultIter.DAResultSet(1) print "Are they the same object? = " + str(NewSet == GetSet) print "Number of Result Sets = " + str(DAResultIter.DAResultSetCount) print "Result Sets = " + str(DAResultIter.DAResultSets()) runClassDemo_DAResult() Typical Evaluate (or Solve) Script Output The output will depend upon the XML definition file used in the model and the attributes and attribute groups used. Name = DA Result XmlType = My Custom Result XmlSubType = Element 954 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Initial DisplayType = Elemental Initial DisplayStyle = Scalar Initial DisplayUnits = No Units New DisplayUnits = Stress Number of Attributes = 1 Are they the same? = True All attributes = Array[AttributeClass]((<Ans.Simulation.DesignAssessmentAssembly.AttributeClass object at 0x000000000000002F [Ans.Simulation.DesignAssessmentAssembly.AttributeClass]>)) Are they the same object? = True Number of Result Sets = 1 Result Sets = Array[DAResultSetClass]((<Ans.Simulation.DesignAssessmentAssembly.DAResultSetClass object at 0x0000000000000030 [Ans.Simulation.DesignAssessmentAssembly.DAResultSetClass]>)) DAResultSet class This class provides the ability to set result values ready for displaying at the appropriate solution step. The object stores 3 types of result values: • Elemental results are for when only a single value is to be displayed for each element. • ElementNodal results are for when an element has different results at each node, but the result belongs to the element, hence there can be multiple results at a given node. • Nodal results have a value at each node. Only results that are appropriate for the display type set in the XML definition file should be added to the object; otherwise an exception will be generated. Depending upon the display style set in the XML definition file the result can have a 1, 3 or 6 components, i.e. scalar, vector or tensor. The component input required is 1 based, i.e. use 1 in the case of scalar. Setting any value to the capacity of a double (1.79769e+308) will result in the element being displayed in a translucent manner. This is the default if a value is not defined for a particular element. Table 103 Members Name Type Description SetElementalValue(int ElementId, int Compon- void ent, double Value) Sets an element result for a given component to the specified Value GetElementalValue(int ElementID, int Compon- double ent) Returns the result value SetElementalValues(int ElementId, double[] Values) void Sets an element result for all components to the specified Value array GetElementalValues(int ElementId) double [] Returns the result values for all components as an array SetElementNodalValue(int ElementId, int NodeId, int Component, double Value) void Sets a node result at the NodeId of an element defined by the provided ElementId, for the specified Component. If the NodeId doesn’t exist on the given ElementId an exception will be generated. GetElementNodalValue(int ElementId, int NodeId, int Component) double Returns the result for a given NodeId, ElementId, and Component. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 955 Features Name Type Description If the NodeId doesn’t exist on the given ElementId an exception will be generated. SetElementNodalValues(int ElementId, int NodeId, double[] Values) void Sets a node result at the NodeId of an element defined by the provided ElementId for all components. If the NodeId doesn’t exist on the given ElementId an exception will be generated. GetElementNodalValues(int ElementId, int NodeId) double[] Returns the result for a given NodeId and ElementId for all components as an array. If the NodeId doesn’t exist on the given ElementId an exception will be generated. SetNodalValue(int NodeId, int Component, double Value) void Sets a node result value for the given NodeId and Component GetNodalValue(int NodeId, int Component) double Returns the value for the given NodeId and Component SetNodalValues(int NodeId, double[] Values) void Sets a node result values for the given NodeId for all Components GetNodalValues(int NodeId) double[] Returns the value for the given NodeId as an array for all Components Example Usage The following example can be used as a basis of either the solve or evaluate script. def runClassDemo_DAResultSet(): for DAResultIter in DesignAssessment.DAResults(): #Create Result Set: Res = DesignAssessment.SolutionSelections()[0].SolutionByRow(1).CreateSolutionResult() #Set the expression and integration method, result info is dependant on these Res.Expression = "UX" Res.IntegrationMethod = "Unaveraged" #Create a result based on the upstream results type and style. DT = Res.DisplayType DS = Res.DisplayStyle NewDAResultSet = DAResultIter.CreateDAResultSet(DS, DT) print DT print DS if (DT == "Elemental"): #Loop around all elements objects. for ElementIter in DesignAssessment.MeshData.Elements(): ElemId = ElementIter.Id NewDAResultSet.SetElementalValues(Id, Res.ElementalValues(Id)) elif (DT == "ElementNodal"): #Loop around all elements objects. for ElementIter in DesignAssessment.MeshData.Elements(): 956 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment ElemId = ElementIter.Id #Loop around all node objects attached to the element. for NodeIter in ElementIter.Nodes(): NodeId = NodeIter.Id ResultValues = Res.ElementNodalValues(ElemId, NodeId) NewDAResultSet.SetElementNodalValues(ElemId, NodeId, ResultValues) elif (DT == "Nodal"): #Loop around all node objects. for NodeIterator in DesignAssessment.MeshData.Nodes(): NodeId = NodeIterator.Id ResultValues = Res.NodalValues(NodeId) print NodeId + " : " + str(ResultValues) NewDAResultSet.SetNodalValues(NodeId, ResultValues) runClassDemo_DAResultSet() Typical Evaluate (or Solve) Script Output The output will depend upon the XML definition file used in the model and the attributes and attribute groups used. Nodal Scalar 1 : 9.5726960580577725e-08 2 : -8.2783643051698164e-08 3 : -7.0038652211223962e-08 4 : -1.0865198873943882e-07 Examples of Design Assessment Usage The following examples show how the Design Assessment system can be used to provide external processing during an analysis. Using Design Assessment to Obtain Results from Mechanical APDL Using Design Assessment to Calculate Complex Results, such as Those Required by ASME Using Design Assessment to Perform Further Results Analysis for an Explicit Dynamics Analysis Using Design Assessment to Obtain Composite Results Using Mechanical APDL Using Design Assessment to Obtain Results from Mechanical APDL The purpose of this example is to illustrate how to run Mechanical APDL in batch mode using Design Assessment, and how to display the results within the Workbench environment; see the Mechanical APDL Command Reference for further information. An example Mechanical APDL data file is shown below. This surf154.dat file is written to obtain surface 154 results that are not supported natively in the Mechanical application and to output them to a CSV file called data.csv. In this scenario, results are element based. Two arguments are to be passed in: • ARG1 = Result file path (without file extension) • ARG2 = Time point to obtain results The surf154.dat file /batch /post1 FILE,ARG1 set,NEAR,,1.0,,ARG2 esel,s,ename,,154 ETABLE,my_press,smisc,13 *get,ecount,elem,0,count *dim,output,arra,ecount,10 curre = 0 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 957 Features *do,i,1,ecount curre = ELNEXT(curre) output(i,1) = curre *get,output(i,2),etab,1,elem,curre *enddo *cfopen,data,csv *vwrite,output(1,1), output(1,2) (2(F16.7,',')) *cfclose fini /exit It is recommended that the files for this example are to be placed in a folder called “DA MAPDL Example” within your ANSYS Inc folder. If you choose not to use this folder, the paths used in the XML Definition File to locate the python scripts will need to be modified. Creating the XML Definition File The XML definition file is set up to create an Attribute Group object for the user to browse to the macro, and a DA Result object to indicate which column from the CSV file to present results for. It will run two scripts. Upon solve, the macro file defined by the user in the Attribute Group will be run by Mechanical APDL and the CSV file created. Upon evaluate, values will be read from the appropriate column in the CSV file and displayed in the Details view of the Design Assessment system. MAPDL.xml <?xml version="1.0" encoding="utf-8"?> <DARoot ObjId ="1" Type="CAERep" Ver="2"> <Attributes ObjId="2" Type="CAERepBase" Ver="2"> <DAAttribute ObjId="100" Type="DAAttribute" Ver="2"> <AttributeName PropType="string">MAPDL Macro File</AttributeName> <AttributeType PropType="string">Browse</AttributeType> <Application PropType="string">All</Application> <Validation PropType="vector&lt;string>">256</Validation> <Default PropType="string"></Default> </DAAttribute> <DAAttribute ObjId="101" Type="DAAttribute" Ver="2"> <AttributeName PropType="string">Column</AttributeName> <AttributeType PropType="string">Int</AttributeType> <Application PropType="string">All</Application> <Validation PropType="vector&lt;string>">1,100</Validation> <Default PropType="string">1</Default> </DAAttribute> </Attributes> <AttributeGroups ObjId ="3" Type="CAERepBase" Ver="2"> <DAAttributeGroup ObjId ="110000" Type="DAAttributeGroup" Ver="2"> <GroupType PropType="string">Select MAPDL File</GroupType> <GroupSubtype PropType="string">By Browsing</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">100</AttributeIDs> </DAAttributeGroup> </AttributeGroups> <DAScripts ObjId="4" Type="DAScripts" Ver="2"> <Solve PropType="string">%DAPROGFILES%\Ansys Inc\DA MAPDL Example\MADPL_S.py</Solve> <Evaluate PropType="string">%DAPROGFILES%\Ansys Inc\DA MAPDL Example\MAPDL_E.py</Evaluate> <DAData PropType="int">1</DAData> <CombResults PropType="int">0</CombResults> </DAScripts> <Results ObjId="5" Type="CAERepBase" Ver="2"> <DAResult ObjId ="120000" Type="DAResult" Ver="2"> <GroupType PropType="string">Select Result Column</GroupType> <GroupSubtype PropType="string">Number Input</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101</AttributeIDs> <DisplayType PropType="string">Elemental</DisplayType> <DisplayStyle PropType="string">Scalar</DisplayStyle> 958 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment <DisplayUnits PropType="string">No Units</DisplayUnits> </DAResult> </Results> </DARoot> The Attributes section defines two DAAttributes: 1st Attribute: Enables the users to browse to the Macro file, Attribute Id = 100: • Named “MAPDL Macro File” • Browse control type • Applies to all geometry • Validates for a maximum length of 256 characters • No default entry 2nd Attribute: Enables the users to select a column in the CSV file, Attribute Id = 101: • Named “Column” • Integer entry type • Applies to all geometry • Validates to check the value is between 1 and 100 (inclusive) • Defaults to a value of 1 In the AttributeGroups section, we define a single Attribute Group object. As we have only one, the GroupType and GroupSubtype fields are effectively redundant, but ought to be entered. • Allow the users to browse to the Macro file, Attribute Id = 110000: – Type = Select MAPDL File – SubType = By Browsing – Include Attribute with Id = 100 This becomes the following object in the Mechanical application: In the DAScripts section we set the path to the scripts to be run on Solve and on Evaluate. In this case we use the %DAPROGFILES% option to direct the program to the Program Files folder, wherever it’s defined locally. The scripts in this case are called MAPDL_S.py and MAPDL_E.py. We want to permit Design Assessment results and prevent combination results In the Results section, we define a single DAResult object. As we have only one, the GroupType and GroupSubtype fields are effectively redundant, but ought to be entered. • Allow the users to browse to the Macro file, Attribute Id = 110000: – Type = Select Result Column Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 959 Features – SubType = Number Input – Include Attribute with Id = 101 – DisplayType is set to show results per element – DisplayStyle is set to show a single, scalar, result – There are no units associated to this result, we’ll set this in the python script This becomes the following object in the Mechanical application: Creating the Script to be Run on Solve, MAPDL_S.py When the user selects “solve” the python script will: 1. Find out what macro file has been selected a. 2. Obtain selected upstream solution data a. 3. Display a message to the Solver Script Output if more than one attribute group is defined Display a message to the Solver Script Output if more than one upstream system is entered Run the macro with Mechanical APDL a. It is assumed that the macro will write data out to a CSV file so it can be read at the evaluate stage b. Display the output from running the macro as the Solver Output import os DA = DesignAssessment def runDADemoSolve(): #1.a - display message if DA.AttributeGroupCount != 1: print "Only one Attribute Group should be entered" #2.a - Display message if DA.SolutionSelections()[0].SolutionCount != 1: print "Only one upstream solution should be entered" #1 - Get the macro path MAPDLMacro = DA.AttributeGroups()[0].Attribute("MAPDL Macro File").ValueAsString SolPath = DA.SolutionSelections()[0].SolutionByRow(1).ResultFilePath #2 - Form the command line strings 960 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment SolPath_Output = "Macro.out" SolTime_ARG2 = str(DA.SolutionSelections()[0].SolutionByRow(1).Time) BatchArgs = " -par1 file -par2 " + SolTime_ARG2 #2 - Run the solve with MAPDL #Change to the path where the results are kept os.chdir(SolPath.rstrip('file.rst')) #Run MAPDL DA.Helper.RunMAPDL(MAPDLMacro,SolPath_Output,BatchArgs) #2.b - Display the output DA.Helper.ReplaceSolverOutputFile(SolPath_Output) runDADemoSolve() Creating the Script to be Run on Evaluate All Results, MAPDL_E.py When the user selects “evaluate” the python script will: 1. 2. Read the CSV file a. Identify the location of the CSV file; this is stored in the upstream result path b. Convert it to a dictionary based on the element ID; each entry of the dictionary is a list of values for each column in the file i. Read each line of the file ii. Split using the commas as the delimiter iii. Convert the text into numeric values iv. Store the values in an array v. Add the array into the dictionary based on the ID For each DAResult create a DAResultSet. Each DAResultSet will display a value for each element a. Find the column to use based on the users entry b. Create the DAResultSet c. The value is found by looking it up in the dictionary with the given element ID #import System DA = DesignAssessment #1.b.iii - Define a rountine to convert text to either a real or integer number. def convertStr(s): #remove the comma s = s.translate(None,',') #If a value exists if len(s) > 0: #Try to convert to an integer try: ret = int(s) except ValueError: #couldn't convert to an integer, try a real number try: ret = float(s) except ValueError: #couldn't convert to a number, set to large value #(makes Mechanical display translucent) ret = 1.7976931348623157e+308 return ret #1.b - Define seperate routine to convert CSV to a dictionary for in-memory access. def CSVToDictionary(PathAndFile): #Define a dictionary IDToDataDict = {}; Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 961 Features #Open the file CSVFile = open(PathAndFile,"r") #1.b.i - step through the file, line by line. for line in CSVFile: #1.b.ii - Split into an array of words. words = line.split(",") #Get the first column, this is the identifier (e.g. Element or Node ID) ID = convertStr(words[0]) #1.b.iv - All other data becomes a list of numbers Data = [] for i in range(len(words)-1): Data.append(convertStr(words[i+1])) #1.b.v - Assign the list to the identifier in the dictionary IDToDataDict[ID] = Data #Close the file and return the dictionary. CSVFile.close() return IDToDataDict def runDADemo(): #1.a - Find where the CSV fle is stored. SolPath = DA.SolutionSelections()[0].SolutionByRow(1).ResultFilePath CSVPath = SolPath.rstrip('file.rst') + "data.csv" #1.b - Call the function to convert the CSV file into a dictionary IDToDataDict = CSVToDictionary(CSVPath) #2 - access each DA Result object in the available results for DAResult in DA.DAResults(): #2.a - Find the column to look up in the CSV data ColIndex = DAResult.Attribute("Column").ValueAsInt - 1 #2.b - Create a result set to display the results using. #We know that in this case it's scalar and element based. DAResultSet = DAResult.CreateDAResultSet("Scalar","Elemental") #2.c - For each element set the value. for Element in DA.MeshData.Elements(): DAResultSet.SetElementalValue(Element.Id,1,IDToDataDict[Element.Id][ColIndex]) runDADemo() Expanding the Example The example given was for a scalar, elemental result. However, if the result required was say a nodal, vector based result, then this example could easily modified by changing a few lines in the evaluate script. Assume that the CSV file contains a first column for the node Id, then 3 columns for X, Y, Z components of the vector. Then, these lines where it previously used SetElementValue: DAResultSet = DAResult.CreateDAResultSet("Scalar","Elemental") #2a - For each element set the value. for Element in DA.MeshData.Elements(): DAResultSet.SetElementalValue(Element.Id,1,IDToDataDict[Element.Id][ColIndex]) Would change to the following, using the SetNodalValue function: DAResultSet = DAResult.CreateDAResultSet("Vector","Nodal") #2a - For each element set the value. for Node in DA.MeshData.Nodes(): 962 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment DAResultSet.SetNodalValue(Node.Id,1,IDToDataDict[Node.Id][0]) DAResultSet.SetNodalValue(Node.Id,2,IDToDataDict[Node.Id][1]) DAResultSet.SetNodalValue(Node.Id,3,IDToDataDict[Node.Id][2]) Alternatively, if the CSV file was always of this NodeId, X, Y, Z format, and given that this is converted into a dictionary of arrays using the Node Id as the key, then the SetNodalValues function could be used instead: DAResultSet = DAResult.CreateDAResultSet("Vector","Nodal") #2a - For each element set the value. for Node in DA.MeshData.Nodes(): DAResultSet.SetNodalValues(Node.Id,IDToDataDict[Node.Id]) Using Design Assessment to Calculate Complex Results, such as Those Required by ASME The purpose of this example is to illustrate how to Design Assessment can be used to calculate results that are beyond the capabilities of the standard user defined result; for example those given in codes of practice such as those from ASME. Creating the XML Definition File The XML definition file defines 4 attributes; 3 are material constants and are to be grouped under a single Attribute Group. The final one is the result set, used to obtaining intermediary results at a given time. The attribute section of the XML definition file is defined as: <Attributes ObjId="2" Type="CAERepBase" Ver="2"> <DAAttribute ObjId="101" Type="DAAttribute" Ver="2"> <AttributeName PropType="string">Const 1</AttributeName> <AttributeType PropType="string">Double</AttributeType> <Application PropType="string">All</Application> <Validation PropType="vector&lt;string>">-100,100</Validation> <Default PropType="string">0.247</Default> </DAAttribute> <DAAttribute ObjId="102" Type="DAAttribute" Ver="2"> <AttributeName PropType="string">Const 2</AttributeName> <AttributeType PropType="string">Double</AttributeType> <Application PropType="string">All</Application> <Validation PropType="vector&lt;string>">-100,100</Validation> <Default PropType="string">2.2</Default> </DAAttribute> <DAAttribute ObjId="103" Type="DAAttribute" Ver="2"> <AttributeName PropType="string">Const 3</AttributeName> <AttributeType PropType="string">Double</AttributeType> <Application PropType="string">All</Application> <Validation PropType="vector&lt;string>">-100,100</Validation> <Default PropType="string">0.25</Default> </DAAttribute> <DAAttribute ObjId="110" Type="DAAttribute" Ver="2"> <AttributeName PropType="string">Set Number</AttributeName> <AttributeType PropType="string">Int</AttributeType> <Application PropType="string">All</Application> <Validation PropType="vector&lt;string>">1,100</Validation> <Default PropType="string">1</Default> </DAAttribute> </Attributes> And to group the 3 material constants together we have an Attribute Group. Defining these in the Attribute Group means that the values can be parameterized if required. This enables a range of coefficients and associative results obtained by running Design Explorer. <AttributeGroups ObjId ="3" Type="CAERepBase" Ver="2"> <DAAttributeGroup ObjId="100000" Type="DAAttributeGroup" Ver="2"> <GroupType PropType="string">ASME VIII Division 3 High Pressure Vessels</GroupType> Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 963 Features <GroupSubtype PropType="string">Material Constants</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,102,103</AttributeIDs> </DAAttributeGroup> </AttributeGroups> The solve and evaluate files are to reside in the user files folder so that they can be easily distributed with the project. All of the processing is to be performed during the evaluate script, so no intermediary files are created to pass data from the solve process to the evaluate process. Combination results are not required and we have no additional system based selection data to define. <DAScripts ObjId="4" Type="DAScripts" Ver="2"> <Solve PropType="string">%DAUSERFILES%\DA-AFT-012_m1-S_empty.py</Solve> <Evaluate PropType="string">%DAUSERFILES%\DA-AFT-012_m1-E_v3_ST.py</Evaluate> <DAData PropType="int">1</DAData> <CombResults PropType="int">0</CombResults> </DAScripts> In the final section, 3 types of DAResults are defined based on the following equations: X - Based on 3 entered constants, plus principal and Von Mises stress =
       +         +   +   −           Damage - The damage value: change in plastic strain divided by X  −  =  , !"#$%&'  , !"#$%&' , !()&*+$  Damage Sum - Accumulative damage; i.e. sum of current and previous Damage values for each result set. The results section of the XML definition file appears as follows: <Results ObjId="5" Type="CAERepBase" Ver="2"> <DAResult ObjId="100001" Type="DAResult" Ver="3"> <GroupType PropType="string">ASME VIII Division 3 High Pressure Vessels</GroupType> <GroupSubtype PropType="string">Value X</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">110</AttributeIDs> <DisplayType PropType="string">ElementNodal</DisplayType> <DisplayStyle PropType="string">Scalar</DisplayStyle> <DisplayUnits PropType="string">Stress</DisplayUnits> </DAResult> <DAResult ObjId="100002" Type="DAResult" Ver="3"> <GroupType PropType="string">ASME VIII Division 3 High Pressure Vessels</GroupType> <GroupSubtype PropType="string">Damage</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">110</AttributeIDs> <DisplayType PropType="string">ElementNodal</DisplayType> <DisplayStyle PropType="string">Scalar</DisplayStyle> <DisplayUnits PropType="string">No Units</DisplayUnits> </DAResult> <DAResult ObjId="100003" Type="DAResult" Ver="3"> <GroupType PropType="string">ASME VIII Division 3 High Pressure Vessels</GroupType> <GroupSubtype PropType="string">Culmative Damage</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>"></AttributeIDs> <DisplayType PropType="string">ElementNodal</DisplayType> <DisplayStyle PropType="string">Scalar</DisplayStyle> <DisplayUnits PropType="string">No Units</DisplayUnits> </DAResult> </Results> 964 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Creating the Script to be Run on Evaluate The script first imports the python math function and defines some constants. import math DA = DesignAssessment DA.OutputDeprecatedWarnings(True) UpstreamSolution = DesignAssessment.SolutionSelections()[0].Solutions()[0] Three routines “EvaluateValueX”, “EvaluateDamage”, and “EvaluateCulmativeDamage”, are defined for performing the calculations for each equation. These are followed with definitions for two additional routines, “Plot” to plot the results and “EvaluateAllResults” to control the evaluate process. The following sections look at each of these routines, starting from the “EvaluateAllResults” entry point. EvaluateAllResults EvaluateDamage EvaluateCulmativeDamage Plot EvaluateAllResults After defining a dictionary to store the element nodal based results, this function creates a new result with part of the required equation and then defines which set to obtain the results from. Then, looping through each element and its nodes, it calculates the part of the equation that is not possible with the standard Mechanical equations and assigns it into the dictionary for the given node and element Id. def EvaluateValueX(Set, Const1, Const2, Const3): XValues = {} #key = element node id tuple, #data = values array. SolRes = UpstreamSolution.CreateSolutionResult("",str(Const2/(1+Const3))+"*((((s1+s2+s3)/(3*seqv))-(1/3)))", SolRes.ResultSet = Set for Element in DA.MeshData.Elements(): for Node in Element.Nodes(): SolResValue = SolRes.ElementNodalValues(Element.Id,Node.Id) XValue = Const1 * math.exp(SolResValue[0]) XValues[Element.Id,Node.Id] = XValue return XValues EvaluateDamage This routine calls the “EvaluateValueX” function to obtain the X Values then creates 2 solution results for the plastic strain results for this and, if one exists, the previous set. A dictionary is created for the element nodal results being generated and this is populated by performing the required calculation. def EvaluateDamage(Set, Const1, Const2, Const3): XValues = EvaluateValueX(Set, Const1, Const2, Const3) StrainRes = UpstreamSolution.CreateSolutionResult("","EPPLEQV","Strain") StrainRes.ResultSet = Set PrevStrainRes = UpstreamSolution.CreateSolutionResult("","EPPLEQV","Strain") if (Set >= 2): PrevStrainRes.ResultSet = Set - 1 DamageValues = {} #key = element node id tuple, #data = values array. for Element in DA.MeshData.Elements(): for Node in Element.Nodes(): S1 = StrainRes.ElementNodalValues(Element.Id,Node.Id)[0] S2 = 0 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 965 Features if (Set >= 2): S2 = PrevStrainRes.ElementNodalValues(Element.Id,Node.Id)[0] XValue = XValues[Element.Id,Node.Id] DamageValues[Element.Id,Node.Id] = (S1 - S2) / XValue return DamageValues EvaluateCulmativeDamage This routine creates a dummy result to obtain the number of result sets. Then, for each set, calls the “EvaluateDamage” function summing the results into a dictionary of element nodal results called CulmativeDamage. def EvaluateCulmativeDamage(Const1, Const2, Const3): DummyRes = UpstreamSolution.CreateSolutionResult("","EPPLEQV","Strain") CulmativeDamage = {} for Set in range(DummyRes.ResultSetCount): DamageValues = EvaluateDamage(Set,Const1, Const2, Const3) if (Set > 1): for Element in DA.MeshData.Elements(): for Node in Element.Nodes(): CulmativeDamage[Element.Id,Node.Id] = CulmativeDamage[Element.Id,Node.Id] + DamageValues[Element.Id else: CulmativeDamage = DamageValues return CulmativeDamage Plot This routine creates a new result for this DAResult object and then loops over each element and node setting the value obtained from the passed in dictionary. def Plot(DAResult, ValuesDictionary): ResultSet = DAResult.CreateDAResultSet() for Element in DA.MeshData.Elements(): for Node in Element.Nodes(): Value = ValuesDictionary[Element.Id,Node.Id] ResultSet.SetElementNodalValue(Element.Id,Node.Id,1,Value) When the script is run, a contour plot is generated for each DA Result. 966 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment Using Design Assessment to Perform Further Results Analysis for an Explicit Dynamics Analysis The purpose of this example is to illustrate how Design Assessment can be used to perform further processing, presenting results in a text file and graphically. In this example, algorithms are written in python to identify which elements form fragments of the geometry following an Explicit Dynmaics analysis. Creating the XML Definition File The XML definition file defines a number of DA Results. All of the processing is to be performed during the evaluate script. This approach means that different levels of damage can be used for the fragment identification within one analysis. This would not be the case if the fragments were determined at the solve stage, but determining fragments at solve stage could be more efficient. Six different results are set up as follows: • • Element Results: – Hide Damaged Elements – Show User Defined Result Fragment Results: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 967 Features – Number of Elements in Fragment – Volume of Fragment – Mass of Fragment – Average Damage in Fragment Each can have failure based upon Failure Threshold or Status, with a numeric limit, and all but the Show User Defined Result can optionally output text to the solver output file. These are attributes 90, 91, and 92 respectively. The Show User Defined Result also has additional input to enable the user to choose the result to display. The results section of the XML definition file is as follows: <Results ObjId="5" Type="CAERepBase" Ver="2"> <DAResult ObjId ="120000" Type="DAResult" Ver="2"> <GroupType PropType="string">Element</GroupType> <GroupSubtype PropType="string">Hide Damaged Elements</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">90,91,92</AttributeIDs> </DAResult> <DAResult ObjId ="120001" Type="DAResult" Ver="2"> <GroupType PropType="string">Element</GroupType> <GroupSubtype PropType="string">Show User Defined Result</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">90,91,103,105,106</AttributeIDs> </DAResult> <DAResult ObjId ="130000" Type="DAResult" Ver="2"> <GroupType PropType="string">Fragment</GroupType> <GroupSubtype PropType="string">Number of Elements in Fragment</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">90,91,92</AttributeIDs> </DAResult> <DAResult ObjId ="130001" Type="DAResult" Ver="2"> <GroupType PropType="string">Fragment</GroupType> <GroupSubtype PropType="string">Volume of Fragment</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">90,91,92</AttributeIDs> </DAResult> <DAResult ObjId ="130002" Type="DAResult" Ver="2"> <GroupType PropType="string">Fragment</GroupType> <GroupSubtype PropType="string">Mass of Fragment</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">90,91,92</AttributeIDs> </DAResult> <DAResult ObjId ="130003" Type="DAResult" Ver="2"> <GroupType PropType="string">Fragment</GroupType> <GroupSubtype PropType="string">Average Damage in Fragment</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">90,91,92</AttributeIDs> </DAResult> </Results> Creating the Script to be Run on Evaluate The script first calls the function runDADemo. This loops over each result and, based on the type and subtype it calls an appropriate sub function to perform the calculation. In the case of fragmentation results, it first calls a function, IdentifyFragments, to create a dictionary of fragments. The fragment dictionary created is a data collection that contains the fragment number for each Element Id. This dictionary is passed to each function so it can be used for the fragment result calculation. An example of this fragment result calculation is VolumeOfFragment: def VolumeOfFragment(DAResult, FragmentDict): #UpstreamSolution has been defined as the upstream solution object #Now we can programmatically create the mass and density results for this solution UpstrResMass = UpstreamSolution.CreateSolutionResult("","MASSALL","Mass") UpstrResDensity = UpstreamSolution.CreateSolutionResult("","DENSITY","Density") 968 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment #Explicit sets each node to have the value of mass or density. #Setting the integration method to average preserves these values #otherwise they are averaged based on the adjacent elements. UpstrResMass.IntegrationMethod = "Unaveraged" UpstrResDensity.IntegrationMethod = "Unaveraged" #Calculate the volume per fragment. FragmentDataDict = {} #key = elementid, data = fragment volume for ElementID in FragmentDict.keys(): FirstNode = DA.MeshData.ElementById(ElementID).NodeIds()[0] Mass = UpstrResMass.ElementNodalValues(ElementID, FirstNode) Density = UpstrResDensity.ElementNodalValues(ElementID, FirstNode) Volume = Mass[0] / Density[0] Fragment = FragmentDict[ElementID] if FragmentDataDict.has_key(Fragment): FragmentDataDict[Fragment] = FragmentDataDict[Fragment] + Volume else: FragmentDataDict[Fragment] = Volume #Output to text for Index, Data in enumerate(FragmentDataDict): Text = "Fragment :" + str(Index + 1) + ", volume = " + str(FragmentDataDict[Data]) print Text if DAResult.Attribute("Output Text Summary").ValueAsString == "Yes": DA.Helper.AppendToSolverOutputFile(Text) #Create a graphical result NewResultData = DAResult.CreateDAResultSet("Scalar","Elemental") DAResult.DisplayUnits = "Volume" for ElemId in FragmentDict: NewResultData.SetElementalValue(ElemId, 1, FragmentDataDict[FragmentDict[ElemId]]) The result can then be displayed: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 969 Features Expanding the Example Additional results could be obtained on a per fragment basis. Using Design Assessment to Obtain Composite Results Using Mechanical APDL Along with the example Using Design Assessment to Obtain Results from Mechanical APDL (p. 957), the purpose of this example is to illustrate how to run Mechanical APDL in batch mode using Design Assessment, and how to present the results within the Workbench environment - see MAPDL command reference for further information. Unlike Using Design Assessment to Obtain Results from Mechanical APDL (p. 957) which is more generic, this example is set up to run a specific script and obtain specific results; therefore the interface can be more targeted and offer better guidance to the end user. In this example the input file for Mechanical APDL is dynamically generated by the python script. This in turn calls a fix macro with various given parameters as determined from the DA Result objects added to the model. The macro file that is run, named LayerMultiPly.mac, is as follows: ! INPUT: ! Input arguments relate to the failure criteria for one material ! ARG1 Type of result, e.g. 'fail' 970 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment ! ARG2 Subtype of the result, e.g. 'emax' ! ARG3 1 for nodal or 0 for elemental based results ! ARG4 1 based layer number ! ! OUTPUT: critical layer and Strength Ratio will be written to defined CSV file ! /post1 /delete,CSVFile_Directory(1),csv /cwd,Current_Directory(1) Type = ARG1 SubType = ARG2 DisplayType = ARG3 LayerNum = ARG4 file,SYS_Directory(1),rst set,last rsys,solu ! set the last set into memory ! set the failure criteria FCTYP,add,all tblist,,1 ! set the layer layer,LayerNum *if,DisplayType,eq,0,then ! select the elements esel,s,ename,,181 ! get the number of elements that we need to loop over *get,ecount,elem,0,count ! make sure some elements are selection *if,ecount,lt,1,then *MSG,ERROR THERE ARE NO ELEMENTS SELECTED FOR FAILURE CHECKING *endif ! dimension the output arrays *dim,output,arra,ecount,2 etab,bob,Type,SubType !get elemental results curre = 0 *do,i,1,ecount curre = ELNEXT(curre) ! get the element number output(i,1) = curre *get,output(i,2),etab,1,elem,curre *enddo *cfopen,CSVFileScratch_Directory(1),csv *vwrite,output(1,1),output(1,2) (F10.0,',',F16.3) *cfclose *elseif,DisplayType,eq,1,then ! select the elements esel,s,ename,,181 nsle ! get the number of nodes that we need to loop over *get,ncount,node,0,count ! make sure some nodes are selection *if,ncount,lt,1,then *MSG,ERROR Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 971 Features THERE ARE NO NODES SELECTED FOR FAILURE CHECKING *endif *dim,output2,arra,ncount,2 curre = 0 *do,i,1,ncount curre = NDNEXT(curre) output2(i,1) = curre *get,output2(i,2),node,i,Type,SubType *enddo *cfopen,CSVFileScratch_Directory(1),csv *vwrite,output2(1,1),output2(1,2) (F10.0,',',F16.3) *cfclose *endif It is recommended that the files for this example are to be placed in your user_files folder. Creating the XML Definition File The XML definition file is set up so that there are no attribute groups, and where appropriate the layer number, display types, and an option to invert the value attributes are included in the DA Result definitions. The failure.xml file <?xml version="1.0" encoding="UTF-8" standalone="no"?> <DARoot ObjId="1" Type="CAERep" Ver="2"> <Attributes ObjId="2" Type="CAERepBase" Ver="2"> <DAAttribute ObjId="100" Type="DAAttribute" Ver="2"> <AttributeName PropType="string">Layer</AttributeName> <AttributeType PropType="string">Int</AttributeType> <Application PropType="string">All</Application> <Validation PropType="vector&lt;string>">1,1000000</Validation> <Default PropType="string">1</Default> </DAAttribute> <DAAttribute ObjId="101" Type="DAAttribute" Ver="2"> <AttributeName PropType="string">Display</AttributeName> <AttributeType PropType="string">DropDown</AttributeType> <Application PropType="string">All</Application> <Validation PropType="vector&lt;string>">Elemental,Nodal</Validation> <Default PropType="string">Elemental</Default> </DAAttribute> <DAAttribute ObjId="102" Type="DAAttribute" Ver="2"> <AttributeName PropType="string">Inverse</AttributeName> <AttributeType PropType="string">DropDown</AttributeType> <Application PropType="string">All</Application> <Validation PropType="vector&lt;string>">Yes,No</Validation> <Default PropType="string">Yes</Default> </DAAttribute> </Attributes> <AttributeGroups ObjId="3" Type="CAERepBase" Ver="2"> </AttributeGroups> <DAScripts ObjId="4" Type="DAScripts" Ver="2"> <Solve PropType="string">%DAUSERFILES%\SolveFailure.py</Solve> <Evaluate PropType="string">%DAUSERFILES%\EvaluateFailure.py</Evaluate> <DAData PropType="int">1</DAData> <CombResults PropType="int">0</CombResults> <SelectionExtra PropType="vector&lt;string>"></SelectionExtra> </DAScripts> <Results ObjId="5" Type="CAERepBase" Ver="2"> <DAResult ObjId="110001" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> 972 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment <GroupSubtype PropType="string">Maximum strain</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100</AttributeIDs> </DAResult> <DAResult ObjId="110002" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">Maximum stress</GroupSubtype> <AttributeIDs PropType="vector<unsigned int>">101,100</AttributeIDs> </DAResult> <DAResult ObjId="110003" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">Tsai-Wu strength index</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100,102</AttributeIDs> </DAResult> <DAResult ObjId="110004" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">Inverse of Tsai-Wu strength ratio index</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100,102</AttributeIDs> </DAResult> <DAResult ObjId="110005" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">Hashin fiber failure</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100,102</AttributeIDs> </DAResult> <DAResult ObjId="110006" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">Hashin matrix failure</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100,102</AttributeIDs> </DAResult> <DAResult ObjId="110007" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">Puck fiber failure</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100,102</AttributeIDs> </DAResult> <DAResult ObjId="110008" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">Puck inter-fiber (matrix) failure</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100,102</AttributeIDs> </DAResult> <DAResult ObjId="110009" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">LaRc03 fiber failure</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100,102</AttributeIDs> </DAResult> <DAResult ObjId="110010" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">LaRc03 matrix failure</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100,102</AttributeIDs> </DAResult> <DAResult ObjId="110011" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">LaRc04 fiber failure</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100,102</AttributeIDs> </DAResult> <DAResult ObjId="110012" Type="DAResult" Ver="2"> <GroupType PropType="string">Layer Dependant Failure</GroupType> <GroupSubtype PropType="string">LaRc04 matrix failure</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">101,100,102</AttributeIDs> </DAResult> <DAResult ObjId="120000" Type="DAResult" Ver="2"> <GroupType PropType="string">Maximum Failure Criteria</GroupType> <GroupSubtype PropType="string">Layer</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>"></AttributeIDs> <DisplayType PropType="string">Elemental</DisplayType> </DAResult> <DAResult ObjId="120001" Type="DAResult" Ver="2"> <GroupType PropType="string">Maximum Failure Criteria</GroupType> <GroupSubtype PropType="string">Failure Criteria</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>"></AttributeIDs> <DisplayType PropType="string">Elemental</DisplayType> </DAResult> Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 973 Features <DAResult ObjId="120002" Type="DAResult" Ver="2"> <GroupType PropType="string">Maximum Failure Criteria</GroupType> <GroupSubtype PropType="string">Value</GroupSubtype> <AttributeIDs PropType="vector&lt;unsigned int>">102</AttributeIDs> <DisplayType PropType="string">Elemental</DisplayType> </DAResult> </Results> </DARoot> Creating the Script to be Run on Solve, SolveFailure.py This is not used as everything is run on the fly, so it is just a simple print statement to say as such. Creating the Script to be Run on Evaluate All Results, EvaluateFailure.py Example 1 covers some aspects of this evaluate function. For example reading the CSV file into a dictionary. The following sections concentrate on the new techniques used here: Using a Dictionary to Avoid a Long if/elif/else Statement. Writing the MADPL .inp File from Within Design Assessment Running Mechanical APDL Multiple Times Using a Dictionary to Avoid a Long if/elif/else Statement. At the beginning of the script it sets up a dictionary matching the XML Type and XML SubType to the Type and SubType of result required in Mechanical APDL: TypeSubTypeDict = {} TypeSubTypeDict["Layer TypeSubTypeDict["Layer TypeSubTypeDict["Layer TypeSubTypeDict["Layer TypeSubTypeDict["Layer TypeSubTypeDict["Layer TypeSubTypeDict["Layer TypeSubTypeDict["Layer TypeSubTypeDict["Layer TypeSubTypeDict["Layer TypeSubTypeDict["Layer TypeSubTypeDict["Layer Dependant Dependant Dependant Dependant Dependant Dependant Dependant Dependant Dependant Dependant Dependant Dependant Failure","Maximum strain"] = "fail","emax" Failure","Maximum stress"] = "fail","smax" Failure","Tsai-Wu strength index"] = "fail","twsi" Failure","Inverse of Tsai-Wu strength ratio index"] = "fail","twsr" Failure","Hashin fiber failure"] = "fail","hfib" Failure","Hashin matrix failure"] = "fail","hmat" Failure","Puck fiber failure"] = "fail","pfib" Failure","Puck inter-fiber (matrix) failure"] = "fail","pmat" Failure","LaRc03 fiber failure"] = "fail","l3fb" Failure","LaRc03 matrix failure"] = "fail","l3mt" Failure","LaRc04 fiber failure"] = "fail","l4fb" Failure","LaRc04 matrix failure"] = "fail","l4mt" TypeSubTypeDict["Maximum Failure Criteria","Layer"] = "FCMX","lay" TypeSubTypeDict["Maximum Failure Criteria","Failure Criteria"] = "FCMX","fc" TypeSubTypeDict["Maximum Failure Criteria","Value"] = "FCMX","val" These can then be easily looked up using: MAPDLKeys = TypeSubTypeDict[str(DAResult.XmlType),str(DAResult.XmlSubType)] MAPDLKeys can then be accessed like a regular array; i.e. MAPDLKeys[0] will return “fail” or “FCMX” appropriately. Writing the MADPL .inp File from Within Design Assessment In this case we want to write the input file for Mechanical APDL from within Design Assessment so that multiple paths can be set, etc., without having to use command line parameters. Most of the common functionality is extracted to the macro file so the input file mainly just sets up these parameters. def CreateMAPDLInputFile(MAPDLKeys,Layer,Display): ArgList = str(",'" + MAPDLKeys[0]) + "','" + str(MAPDLKeys[1]) + "'," + str(Display) + "," + str(Layer) currentdirectory = os.getcwd() 974 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Design Assessment RunMapdlFile = open(TempMAPDLRunFilePath, "w") WriteLine(RunMapdlFile,"/batch") WriteLine(RunMapdlFile,"*DIM,SYS_Directory,string,248") RSTFileLoc = DesignAssessment.SolutionSelections()[0].SolutionByRow(1).ResultFilePath.rstrip('.rst') WriteLine(RunMapdlFile,"'SYS_Directory(1)' = " + "'" + RSTFileLoc + "'") WriteLine(RunMapdlFile,"*DIM,CSVFile_Directory,string,248") WriteLine(RunMapdlFile,"'CSVFile_Directory(1)' = " + "'" + DesignAssessment.Helper.ResultPath + "\\TempRes" WriteLine(RunMapdlFile,"*DIM,CSVFileScratch_Directory,string,248") WriteLine(RunMapdlFile,"'CSVFileScratch_Directory(1)' =" + "'" + currentdirectory + "\\TempRes" + "'") WriteLine(RunMapdlFile,"*DIM,Current_Directory,string,248") WriteLine(RunMapdlFile,"'Current_Directory(1)' =" + "'" + currentdirectory + "'") WriteLine(RunMapdlFile,"*USE,LayerMultiPly.mac" + ArgList) WriteLine(RunMapdlFile,"fini") WriteLine(RunMapdlFile,"/exit") RunMapdlFile.close() Running Mechanical APDL Multiple Times Mechanical APDL is run repeatedly for each DA Result object. In each case, the CSV file is read and the results displayed. In-line if statements are used to determine, among other things, if the value is to be inverted and what the value is if it is inverted. def runStressEvaluate(DesignAssessment): #Change to the result path as the local folder, to save passing in long file names to the MAPDL solve originaldir = os.getcwd() os.chdir(DesignAssessment.Helper.ResultPath) # Make sure the mapdl macro is in this directory shutil.copy2(DesignAssessment.Helper.UserFilesDirectory + "\\LayerMultiPly.mac",DesignAssessment.Helper.Resu # For now just assume one upstream but could make the code generic if required if (DesignAssessment.SolutionSelections()[0].SolutionCount > 1): print "only the first solution in the solution selection object will be used" for DAResult in DesignAssessment.DAResults(): #Identify the type and subtype to be passed into MAPDL MAPDLKeys = TypeSubTypeDict[str(DAResult.XmlType),str(DAResult.XmlSubType)] print MAPDLKeys #in-line if / else statements, format of N = ValueA if statement [is true] else [N =] ValueB. Layer = 0 if (DAResult.Attribute("Layer") == None) else DAResult.Attribute("Layer").ValueAsInt Display = "Elemental" if (DAResult.Attribute("Display") == None) else DAResult.Attribute("Display").Valu Inverse = False if (DAResult.Attribute("Inverse") == None) else DAResult.Attribute("Inverse").ValueAsStr #Create the results temp file by running a post script with MAPDL if Display == "Elemental": CreateMAPDLInputFile(MAPDLKeys,Layer,0) elif Display == "Nodal": CreateMAPDLInputFile(MAPDLKeys,Layer,1) #Run MAPDL DesignAssessment.Helper.RunMAPDL(TempMAPDLRunFilePath,"out.lis","/minimise") DesignAssessment.Helper.ReplaceSolverOutputFile("out.lis") #Read the results from the temp file to memory. IDToDataDict = CSVToDictionary(DesignAssessment.Helper.ResultPath + "tempres.csv") #Present the results #Elemental if Display == "Elemental": Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 975 Features DAResultSet = DAResult.CreateDAResultSet("Scalar","Elemental") for Element in DesignAssessment.MeshData.Elements(): Value = 1/max(IDToDataDict[Element.Id][0],0.01) if Inverse else IDToDataDict[Element.Id][0] DAResultSet.SetElementalValue(Element.Id,1,Value) #Nodal elif Display == "Nodal": DAResultSet = DAResult.CreateDAResultSet("Scalar","Nodal") for Node in DesignAssessment.MeshData.Nodes(): Value = 1/max(IDToDataDict[Node.Id][0],0.01) if Inverse else IDToDataDict[Node.Id][0] DAResultSet.SetNodalValue(Node.Id,1,Value) os.chdir(originaldir) Expanding the Example The example could be expanded to perform combinations of results and factor the values based on the coefficient provided for the upstream system. Virtual Topology in the Mechanical Application All virtual topology operations in the Mechanical application are described in the Virtual Topology section of the Meshing Help. 976 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Objects Reference Welcome to the Mechanical Objects Reference. This reference provides a specification for every Mechanical object in the tree. Each object is represented in either its own reference page, or is combined with similar objects and represented on one group reference page. For example, the Joint object is represented on its own Joint object reference page, whereas the Acceleration object is represented on the Loads and Supports (Group) object reference page. All pages representing groups of objects include "(Group)” as part of the page's title. Note Certain types of objects do not appear in the tree but are still represented on their own pages in this reference. These include Virtual Cell objects, Virtual Hard Vertex objects, Virtual Split Edge objects, and Virtual Split Face objects. When these types of objects are created, they are saved in the database and have editable properties similar to other objects. For details, refer to the individual reference pages for these objects. A complete alphabetical listing of Mechanical objects reference pages is included below. To determine the reference page for an object in a group, consult the group page whose title matches the object, and check the entry: “Applies to the following objects”. The following is a description of each component of a Mechanical object reference page: • Title - For individual object reference pages, the title is the default name of the object as it appears in the tree. For group reference pages, the title is a name given to the collection of objects represented. • Object definition - A brief description of the individual object or group of objects. • Applies to the following objects - Appears only on group reference pages and includes the default name of all objects represented on the group reference page. • Tree dependencies - The valid location of the object or group of objects in the tree (Valid Parent Tree Object), as well as other possible objects that you can insert beneath the object or group of objects (Valid Child Tree Objects). • Insertion options - Procedure for inserting the object (individual or one in the group) in the tree. Typically this procedure includes inserting the object from a context toolbar button or through a context menu option when you click the right mouse button with the cursor on the object. • Additional related information - a listing of topics related to the object or object group that are in the help. Included are links to those topics. • Tree location graphic - an indication of where the object or group of objects appears in the tree. • Object Properties - a listing of every setting or indication available in the Details view (located directly beneath the object tree) for the object. Included are links to more detailed information on an item within the help. • Relevant right mouse button context menu options - a listing of options directly relevant to the objects that are available in the context menu through a right mouse click on the object. Included are Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 977 Objects Reference links to more detailed information on an item within the help. The options listed are in addition to options that are common to most of the objects (such as Solve, Copy, Cut, Duplicate, and Delete). The objects reference is not intended to be your primary source of procedural information for performing simulations -- see the Mechanical Approach section for introductory and procedural guidelines concerning when and where to use Mechanical objects. Page Listings The following is an alphabetical listing of object reference pages: Alert Analysis Settings Angular Velocity Beam Body Body Interactions Body Interaction Chart Commands Comment Connections Connection Group Construction Geometry Contact Region Contact Tool (Group) Convergence Coordinate System Coordinate Systems Direct FE (Group) End Release Environment (Group) Fatigue Tool (Group) Figure Fluid Surface Gasket Mesh Control Geometry Global Coordinate System Image Imported Layered Section Imported Load (Group) Imported Thickness Imported Thickness (Group) Initial Conditions Initial Temperature Joint Layered Section Loads, Supports, and Conditions (Group) Mesh Mesh Connection Mesh Control Tools (Group) Mesh Group (Group) Mesh Grouping Mesh Numbering 978 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Alert Modal Model Named Selections Numbering Control Part Path Periodic/Cyclic Region Point Mass Pre-Stress Probe Project Remote Point Remote Points Result Tracker Results and Result Tools (Group) Solution Solution Combination Solution Information Spot Weld Spring Stress Tool (Group) Surface Symmetry Symmetry Region Thermal Point Mass Thickness Validation Velocity Virtual Body Virtual Body Group Virtual Cell Virtual Hard Vertex Virtual Split Edge Virtual Split Face Virtual Topology Alert Sets pass or fail thresholds for individual results. When a threshold is exceeded, the status symbol changes in front of the associated result object. The status is also displayed in the Details view of the Alert object. Alerts facilitate the presentation of comparisons in automatic reports. Tree Dependencies: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 979 Objects Reference • Valid Parent Tree Objects: All result objects (independent, or under result tools), except Damage Matrix, Fatigue Sensitivity, Hysteresis, Phase Response, Probe, Rainflow Matrix, Reactions, Status, Vector Principal Elastic Strain, Vector Principal Stress. • Valid Child Tree Objects: Comment Insertion Options: Click right mouse button on a result object or in the Geometry window after you select the result object, and then> Insert> Alert. Object Properties The Details view properties for this object include the following. Category Fields Definition Fails If - Set failure threshold as Minimum Below Value or Maximum Above Value, where you set the value in the next field. Value - Threshold value in the units of the associated result. Results Status - Read-only indication of the pass/fail status; also includes criterion (for example: “Passed: Minimum Above Value”). Analysis Settings Allows you to define various solution settings that are customized to specific analysis types. Tree Dependencies: • Valid Parent Tree Object: Any environment object. • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Appears by default when you create an analysis system. Additional Related Information: • Establish Analysis Settings (p. 9) • Analysis Settings (p. 499) Object Properties For more information on this object's properties, see the Analysis Settings for Most Analysis Types (p. 499) section. Angular Velocity Applies angular velocity as an initial condition for use in an explicit dynamics analysis. 980 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Angular Velocity Note • For explicit dynamics analyses, the center of rotation for an angular velocity is defined by the origin of the coordinate system associated with the angular velocity. • Angular Velocity initial conditions are not supported for 2D axisymmetric Explicit Dynamics analyses. Tree Dependencies: • Valid Parent Tree Object: Initial Conditions • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Initial Conditions object: • Click Angular Velocity button on Initial Conditions context toolbar . • Click right mouse button on Initial Conditions object or in the Geometry window>Insert>Angular Velocity. Additional Related Information: • Define Initial Conditions • Explicit Dynamics Analysis Object Properties The Details view properties for this object include the following. Category Fields Scope Scoping Method Geometry– appears if Scoping Method is set to Geometry Selection. In this case, use selection filters to pick geometry, click in the Geometry field, then click Apply. Named Selection – appears if Scoping Method is set to Named Selection. Definition Input Type - choose either Angular Velocity or Velocity. Define By Total - magnitude; appears if Define By is set to Vector. Direction- appears if Define By is set to Vector. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 981 Objects Reference Category Fields Coordinate System – available list; appears if Define By is set to Components. X, Y, Z Component – values; appears if Define By is set to Components. Suppressed Beam A beam is a structural element that carries load primarily in bending. Tree Dependencies: • Valid Parent Tree Object: Connections • Valid Child Tree Objects: Commands, Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Connections object: • Click Body-Ground> Beam or Body-Body> Beam, as applicable on Connections context toolbar. • Click right mouse button on Connections object or in the Geometry window> Insert> Beam. Additional Related Information: • Connections Context Toolbar • Beam Connections (p. 483) The following right mouse button context menu options are available for this object. • Enable/Disable Transparency - similar behavior to feature in Contact Region. • Rename Based on Definition - similar behavior to feature in Results. • Promote Remote Point Object Properties The Details view properties for this object include the following. Category Fields Graphics Properties Visible – toggles visibility of the beam. Definition Material - determined in Engineering Data. Cross Section - read-only indication. Radius Suppressed 982 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Body Scope - information on springs also applies to beams. Scope Reference - information on springs also applies to beams. Reference Component - appears if Scope (under Scope group) is set to Body-Body and Scoping Method is set to Named Selection. Scope - appears if Scope (under Scope group) is set to Body-Body and Scoping Method is set to Geometry Selection. Choose geometry entity then click on Apply. Body- appears if Scope (under Scope group) is set to Body-Body and Scoping Method is set to Geometry Selection. Read-only indication of scoped geometry. Coordinate System Reference X Coordinate Reference Y Coordinate Reference Z Coordinate Reference Location Behavior Pinball Region Mobile - information on springs also applies to beams. Reference Component - appears if Scoping Method is set to Named Selection. Scope - appears if Scoping Method is set to Geometry Selection. Choose geometry entity then click on Apply. Body- appears if Scoping Method is set to Geometry Selection. Read-only indication of scoped geometry. Coordinate System Mobile X Coordinate Mobile Y Coordinate Mobile Z Coordinate Mobile Location Behavior Pinball Region Body Defines a component of the attached geometry included under a Geometry object, or under a Part object if considered a multibody part (shown in the figure below). Also see the description of the Virtual Body (p. 1064) object (applicable to assembly meshing algorithms only). Tree Dependencies: • Valid Parent Tree Object: Geometry or Part (if under a multibody part) • Valid Child Tree Objects: Commands, Comment, Figure, Gasket Mesh Control, Image Insertion Options: Appears by default when geometry is attached. Additional Related Information: • Define Part Behavior (p. 6) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 983 Objects Reference • Geometry in the Mechanical Application (p. 315) The following right mouse button context menu options are available for this object. • Search Faces with Multiple Thicknesses • Create Selection Group • Generate Mesh • Preview> Surface Mesh - appears only for a solid body. • Preview> Inflation Object Properties The Details view properties for this object include the following. Category Fields Graphics Properties Visible - turns part display On or Off in the Geometry window Transparency - varies the body between being completely transparent (0) to completely opaque (1) Color - sets the color of the body. Definition Suppressed Stiffness Behavior - appears only for a single solid body that is not a component of a multibody part Brick Integration Scheme - appears only if Element Control is set to Manual in the Details view of the Geometry object; not available if Stiffness Behavior is set to Rigid Coordinate System - assign a local coordinate system to specify the alignment of the elements of the body if previously defined using one or more Coordinate System objects; not available if Stiffness Behavior is set to Rigid Reference Temperature Reference Temperature Value - available only when you select By Body as the Reference Temperature Reference Frame - appears only for solid bodies when an Explicit Dynamics system is part of the solution Thickness - appears only for a surface body Thickness Mode - appears only for a surface body; read-only indication Offset Mode - appears only for a line body Offset Type - appears only for a line body Model Type - appears only for a line body Material Assignment Nonlinear Effects - not available if Stiffness Behavior is set to Rigid. Thermal Strain Effects Fluid/Solid - available only in the Meshing application (i.e., not available if you are using the meshing capabilities from within the Mechanical application). Useful in assembly meshing. Allows you to control the physics that occur on a model. Valid options are Fluid, Solid, and Defined By Geometry. When set to Defined By Geometry, the value is based on the Fluid/Solid material property that was assigned to the body in the DesignModeler application. Bounding Box Length X Length Y 984 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Body Interactions Length Z Properties Indications of the properties originally assigned to the body. Volume Mass Length - appears only for line bodies Note If the material density is temperature dependent, the Mass will be computed at the body temperature, or at 22oC (default temperature for an environment). The following appear for all bodies except line bodies: Centroid X Centroid Y Centroid Z Moment of Inertia Ip1 Moment of Inertia Ip2 Moment of Inertia Ip3 Surface Area (approx.) - appears only for a surface body The following appear for line bodies only: Cross Section Cross Section Area Cross Section IYY Cross Section IZZ The following appear for surface bodies only: Offset Type Membrane Offset - appears for surface bodies when Offset Type = User Defined Statistics: Read-only indication of the entities that comprise the body. Nodes Elements Mesh Metric Body Interactions Sets global options for all Body Interaction objects in an Explicit Dynamics Analysis. Tree Dependencies: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 985 Objects Reference • Valid Parent Tree Object: Connections • Valid Child Tree Objects: Body Interaction, Comment, Figure, Image Insertion Options: Automatically inserted in the tree if contact is detected when model is attached. Also, use any of the following methods after highlighting Connections object: • Click Body Interaction button on Connections context toolbar. • Click right mouse button on Connections object or in the Geometry window>Insert>Body Interaction. Additional Related Information: • Body Interaction (p. 986) • Body Interactions in Explicit Dynamics Analyses (p. 487) • Explicit Dynamics Analysis (p. 35) Object Properties The Details view properties for this object include the following. Category Fields Advanced Contact Detection Formulation - appears if Contact Detection = Trajectory. Shell Thickness Factor - appears if the geometry includes one or more surface bodies and if Contact Detection = Trajectory. Pinball Factor - appears if Contact Detection = Proximity Based. Timestep Safety Factor - appears if Contact Detection = Proximity Based. Limiting Timestep Velocity - appears if Contact Detection = Proximity Based. Edge on Edge Contact - appears if Contact Detection = Proximity Based. Body Self Contact Element Self Contact Tolerance - appears if Contact Detection = Trajectory and Element Self Contact = Yes. Body Interaction Creates contact between bodies in an Explicit Dynamics Analysis. Tree Dependencies: 986 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Body Interaction • Valid Parent Tree Object: Body Interactions • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: • Automatically inserted in the tree if model includes a Body Interactions object. • For manual insertion, use any of the following methods after highlighting Connections object. – Choose Body Interaction on Connections context toolbar. – Click right mouse button on Connections object, or in the Geometry window>Insert>Body Interaction. Additional Related Information: • Body Interactions (object reference) • Body Interactions • Explicit Dynamics Analysis Object Properties The Details view properties for this object include the following. Category Fields Scope Scoping Method Geometry – appears if Scoping Method is set to Geometry Selection. In this case, use selection filters to pick geometry, click in the Geometry field, then click Apply. Named Selection – appears if Scoping Method = Named Selection. Definition Type Maximum Offset – appears if Type = Bonded. Breakable – appears if Type = Bonded. Normal Stress Limit – appears if Type = Bonded and Breakable = Stress Criteria. Normal Stress Exponent – appears if Type = Bonded and Breakable = Stress Criteria. Shear Stress Limit – appears if Type = Bonded and Breakable = Stress Criteria. Shear Stress Exponent – appears if Type = Bonded and Breakable = Stress Criteria. Friction Coefficient – appears if Type = Frictional. Dynamic Coefficient – appears if Type = Frictional. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 987 Objects Reference Category Fields Decay Constant – appears if Type = Frictional. Suppressed Chart Represents a chart that you can create for loads and/or results against time, or result quantities against a load or another result quantity. Tree Dependencies: • Valid Parent Tree Object: Model • Valid Child Tree Objects: Comment, Image Insertion Method: Click the Chart and Table button on the standard toolbar. Additional Related Information: • Chart and Table (p. 729) • Standard Toolbar Object Properties For more information on this object's properties, see the Chart and Table (p. 729) section. Commands • Allows use of Mechanical APDL application commands or APDL programming in a simulation. • Allows use of Python for the Transient Structural (Rigid Dynamics) system. Tree Dependencies: • Valid Parent Tree Objects: Body, Contact Region (shown in figure), environment objects, Joint, Pre-Stress, Solution, Spring • Valid Child Tree Objects: Comment, Image Insertion Options: Choose one of the following: • Click right mouse button on either the parent object (see above) or in the Geometry window> Insert> Commands. • Highlight the parent object (see above) and choose the Insert Commands button from the toolbar. Additional Related Information: • Commands Objects Tree Dependencies for the Transient Structural (Rigid dynamics) system: 988 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Comment • Valid Parent Tree Objects: Connections Folder, Joint, Spring, Environment, Joint Condition . The following right mouse button context menu options are available for this object. • Export... • Import... • Refresh • Suppress • Search Parameters - appears only if Commands object is under a Solution object. • Rename Based on Definition Object Properties The Details view properties for this object include the following. Category Fields/Descriptions File File Name - Read-only indication of imported text file name (including path) if used. File Status - Read-only indication of the status of an imported text file if used. Definition Suppressed Target - displays a list of solvers. Invalidate Solution - applicable for the Solution object only. Output Search Prefix - applicable for the Solution object only. Step Selection Mode - applicable only for stepped analyses, and only when inserting under an environment object. Step Number - applicable only for stepped analyses, and only when inserting under an environment object. Input Arguments ARG1 through ARG9 Results Applicable only when inserting under a Solution object. Comment Inserts a comment for a Mechanical parent object. The comment editor creates a fragment of HTML, and the object itself consists of that HTML fragment, a string denoting the author's name, and a color. Report adds the resulting HTML fragment directly in line, in the specified color and notes the author. The Comment context toolbar provides buttons to insert an image or to apply various text formatting tags. Tree Dependencies: • Valid Parent Tree Objects: All objects. • Valid Child Tree Objects: None. Insertion Method: Click the Comment button on the standard toolbar. Additional Related Information: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 989 Objects Reference • Comments, Images, Figures (p. 401) • Comment Context Toolbar • Reporting Object Properties The Details view properties for this object include the following. Category Fields/Descriptions Author Name Connections Defines connections between two or more parts or bodies. Includes global settings in Details view that apply to all Contact Region, Spot Weld, Mesh Connection, Body Interaction (for explicit dynamics analyses), Joint, Spring, and Beam child objects. Tree Dependencies: • Valid Parent Tree Object: Model • Valid Child Tree Objects: Beam, Body Interactions, Comment, Connection Group (including those named Contacts, Joints, and Mesh Connections; Contact Tool, Figure, Image, Joint, Solution Information, Spot Weld, Spring, Insertion Options: • Automatically inserted in the tree if connection is detected when model is attached. • For setting connections manually, use any of the following methods after highlighting Model object: – Click Connections button on Model context toolbar. – Click right mouse button on Model object or in the Geometry window> Insert> Connections. Note These options are not available if a Connections object already exists in the tree. Additional Related Information: 990 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Connection Group • Beams • Body Interactions • Connections Overview • Automatically Generated Connections • Contact Region Settings • Mesh Connection • Contact Ease of Use Features • Contact Tool and Results • Contact Options Preferences • Joints • Spot Welds • Springs The following right mouse button context menu options are available for this object. • Create Automatic Connections - available only if at least one Connection Group folder is present. • Redundancy Analysis - available if at least one Joint object is present. • Enable/Disable Transparency • Search Connections for Duplicate Pairs • Rename Based on Definition Object Properties The Details view properties for this object include the following. Category Fields Auto Detection Generate Automatic Connection On Refresh Transparency Enabled Connection Group Defines connections among selected bodies. Includes global settings in Details view that apply to all Contact Region, Mesh Connection, or Joint child objects. Tree Dependencies: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 991 Objects Reference • Valid Parent Tree Object: Connections • Valid Child Tree Objects: Comment, Contact Region, Figure, Image, Joint, Mesh Connection Insertion Options: Use any of the following methods after highlighting Connections object: • Click Connection Group on Connections context toolbar. • Click right mouse button on Connections object (or on another Connection Group object), or in the Geometry window; then Insert> Connection Group. • Insert a Contact Region, Mesh Connection, or Joint object. A separate parent Connection Group object is created automatically for each of these three types of objects, and is renamed Contacts, Mesh Connections, or Joints accordingly. Additional Related Information: • Automatically Generated Connections • Contact Region Settings • Mesh Connection • Joints (p. 433) The following right mouse button context menu options are available for this object. • Create Automatic Connections • Enable/Disable Transparency • Search Connections for Duplicate Pairs • Rename Based on Definition Object Properties The Details view properties for this object include the following. Category Fields Definition Connection Type Scope Scoping Method Geometry– appears if Scoping Method is set to Geometry Selection. In this case, use selection filters to pick geometry, click in the Geometry field, then click Apply. Named Selection – appears if Scoping Method is set to Named Selection. 992 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Construction Geometry Category Fields Auto Detection Tolerance Type Tolerance Slider Tolerance Value Use Range Min Distance Percentage Min Distance Value Face/Face Face/Edge - appears only for contacts and mesh connection groups. Edge/Edge - appears only for contacts and mesh connection groups. Priority - appears only for contacts and mesh connection groups. Group By Search Across Revolute Joints - appears only for joint groups. Fixed Joints - appears only for joint groups. Construction Geometry Houses one or more Path and/or Surface objects. You can apply results to paths and surfaces that you define. Tree Dependencies: • Valid Parent Tree Object: Model • Valid Child Tree Objects: Comment, Figure, Image, Path, Surface. Insertion Options: Use any of the following methods after highlighting Model object: • Click Construction Geometry button on Model context toolbar • Click right mouse button on Model object or in the Geometry window >Insert>Construction Geometry. Note You can add only one Construction Geometry Object under Model. Additional Related Information: • Path (Construction Geometry) (p. 376) • Surface (Construction Geometry) (p. 381) • Path (p. 1037) object reference • Surface (p. 1057) object reference Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 993 Objects Reference Contact Region Defines conditions for individual contact and target pairs. Several Contact Regions can appear as child objects under a Connection Group object. The Connection Group object name automatically changes to Contacts. Tree Dependencies: • Valid Parent Tree Object: Connection Group • Valid Child Tree Objects: Commands, Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Connections or Connection Group object: • Inserted automatically if you choose Create Automatic Connections through a right mouse click on Connections (or Contacts) object. • Click Contact on Connections context toolbar and choose a contact type. • Click right mouse button on Connections (or Connection Group) object or in the Geometry window; then Insert> Manual Contact Region. Additional Related Information: • Contact Region Settings • Automatically Generated Connections • Global Connection Settings • Connections Context Toolbar • Setting Contact Conditions Manually • Contact Ease of Use Features • Contact Tool and Results • Contact Options Preferences The following right mouse button context menu options are available for this object. • Enable/Disable Transparency • Hide All Other Bodies • Flip Contact/Target • Search Connections for Duplicate Pairs • Go To Connections for Duplicate Pairs - available if connection object shares the same geometries with other connection objects. • Save Contact Region Settings • Load Contact Region Settings • Reset to Default • Rename Based on Definition 994 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Contact Region Object Properties Choose the object properties below that apply to your analysis type. Object Properties - Most Structural Analyses Object Properties - Explicit Dynamics Analyses Object Properties - Thermal and Electromagnetic Analyses Object Properties - Most Structural Analyses The Details view properties for this object include the following. Category Fields/Conditions Scope Scoping Method Contact Target Contact Bodies Target Bodies Contact Shell Face - appears for surface bodies. Target Shell Face - appears for surface bodies. Definition Type Friction Coefficient - if Type = Frictional Scope Mode Behavior Suppressed Advanced Formulation Constraint Type - if Formulation = MPC and scoping of Contact Bodies or Target Bodies is to a surface body. Interface Treatment Offset - if Interface Treatment = Add Offset Normal Stiffness Normal Stiffness Factor - if Normal Stiffness = Manual Update Stiffness - if Formulation = Augmented Lagrange or Pure Penalty Stabilization Damping Factor — Helps reduce the risk of rigid body motion. Available for Frictionless, Rough, and Frictional contact types. Pinball Region Pinball Radius - if Pinball Region = Radius Time Step Controls - if Type = Frictionless, Rough, or Frictional Basics of Contact Region object Object Properties - Explicit Dynamics Analyses The Details view properties for this object include the following. Category Fields/Conditions Scope Scoping Method Contact Target Contact Bodies Target Bodies Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 995 Objects Reference Category Fields/Conditions Definition Type Friction Coefficient - if Type = Frictional Dynamic Coefficient - if Type = Frictional Decay Constant - if Type = Frictional Scope Mode Behavior Maximum Offset - if Type = Bonded Breakable - if Type = Bonded Normal Stress Limit - if Type = Bonded and Breakable = Stress Criteria Normal Stress Exponent - if Type = Bonded and Breakable = Stress Criteria Shear Stress Limit - if Type = Bonded and Breakable = Stress Criteria Shear Stress Exponent - if Type = Bonded and Breakable = Stress Criteria Suppressed Basics of Contact Region object Object Properties - Thermal and Electromagnetic Analyses The Details view properties for this object include the following. Category Fields/Conditions Scope Scoping Method Contact Target Contact Bodies Target Bodies Contact Shell Face - appears for surface bodies. Target Shell Face - appears for surface bodies. Definition Type Friction Coefficient - if Type = Frictional Scope Mode Behavior Suppressed Advanced Formulation Constraint Type - if Formulation = MPC and scoping of Contact Bodies or Target Bodies is to a surface body. Interface Treatment Offset - if Interface Treatment = Add Offset. Normal Stiffness (Magnetostatic analyses and all thermal analyses) - if Formulation = Augmented Lagrange, Pure Penalty, or MPC. Normal Stiffness Factor (Magnetostatic analyses and all thermal analyses) - if Normal Stiffness = Manual Update Stiffness (Magnetostatic analyses and all thermal analyses) - if Formulation = Augmented Lagrange, Pure Penalty, or MPC. Thermal Conductance (Magnetostatic analyses and all thermal analyses) Thermal Conductance Value (Magnetostatic analyses and all thermal analyses) - if Thermal Conductance = Manual. Electrical Conductance (Electric and Magnetostatic analyses) 996 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Contact Tool (Group) Category Fields/Conditions Electrical Conductance Value (Electric and Magnetostatic analyses) - if Electric Conductance = Manual. Pinball Region Pinball Radius - if Pinball Region = Radius. Time Step Controls - if Type = Frictionless, Rough, or Frictional. Basics of Contact Region object Contact Tool (Group) Determines contact conditions on an assembly both before loading and as part of the final solution. Applies to the following objects: Contact Tool, Frictional Stress, Gap, Initial Information, Penetration, Pressure, Sliding Distance, Status Tree Dependencies: • • Valid Parent Tree Objects: – For Contact Tool: Connections, Solution – For Frictional Stress, Pressure, and Sliding Distance: Contact Tool under Solution object – For Gap, Penetration, and Status: Contact Tool under Connections object or Solution object – For Initial Information: Contact Tool under Connections object only Valid Child Tree Objects: – For Contact Tool under Connections object: Comment, Gap, Image, Initial Information, Penetration, Status – For Contact Tool under Solution object: Comment, Gap, Frictional Stress, Image, Penetration, Pressure, Sliding Distance, Status – For Frictional Stress, Gap, Penetration, Pressure, and Sliding Distance: Alert, Comment, Convergence, Figure, Image – For Initial Information: Comment, Image – For Status: Comment, Figure, Image Insertion Options: • • For Contact Tool under Connections object, use any of the following methods after highlighting Connections object: – Choose Contact Tool on Connections context toolbar under the Contact drop down menu. – Click right mouse button on Connections object or in the Geometry window> Insert> Contact Tool. For Contact Tool under Solution object, use any of the following methods after highlighting Solution object: – Choose Tools> Contact Tool on Solution context toolbar. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 997 Objects Reference – • Click right mouse button on Solution object or in the Geometry window> Insert> Contact Tool> Contact Tool. For any Contact Tool result object, use any of the following methods after highlighting Contact Tool object: – Choose Contact> (result object) on Contact Tool context toolbar. – Click right mouse button on Contact Tool object or in the Geometry window> Insert> (result object). Additional Related Information: • Connections Context Toolbar • Contact Overview • Global Contact Settings • Setting Contact Conditions Manually • Contact Ease of Use Features • Contact Tool and Results • Contact Options Preferences The following right mouse button context menu options are available for this object. • Generate Initial Contact Results - available for Contact Tool and all child objects when the Contact Tool is inserted under a Connections object. • Evaluate All Results - available for Contact Tool and all child objects when the Contact Tool is inserted under a Solution object. Object Properties For more information on this object's properties, see the Contact Tool section. Convergence Controls the relative accuracy of a solution by refining solution results on a particular area of a model. The Convergence object is applicable to static structural, modal, linear buckling, steady-state thermal, and magnetostatic analyses. Tree Dependencies: • Valid Parent Tree Objects: Several result objects. Insertion Options: Click right mouse button on a result object or in the Geometry window> Insert> Convergence. 998 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Convergence Note Only one Convergence object is valid per result object. Convergence is not supported: • For result objects that belong to linked analyses. • If an imported load object exists in the environment. • When Imported Layered Section or Imported Thickness objects are used. When running background solutions, only one maximum refinement loop is performed. Additional Related Information: • Adaptive Convergence • Error (Structural) • Error (Thermal) • Mechanical Options - Convergence Object Properties The Details view properties for this object include the following. Category Fields Definition Type Allowable Change Results Last Change - Read-only indication of the most recent change in convergence. Converged - Read-only indication of the convergence state (Yes or No). Note • Convergence objects inserted under an environment that is referenced by an Initial Condition object or a Thermal Condition load object, will invalidate either of these objects, and not allow a solution to progress. • Results cannot be converged when you have a Mesh Connection object or a Pinch control with PinchBehavior set to Post. • To use Convergence, you must set Calculate Stress to Yes under Output Controls in the Analysis Settings details panel. However, you can perform Modal and Buckling Analysis without specifying this option. • You cannot use Convergence if you have an upstream or a downstream analysis link. • Convergence is not available when you import loads into the analysis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 999 Objects Reference Coordinate System Represents a local coordinate system that you can add under a Coordinate Systems object. Tree Dependencies: • Valid Parent Tree Object: Coordinate Systems • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Coordinate Systems object, or Global Coordinate System object, or another Coordinate System object: • Choose Create Coordinate System button on Coordinate Systems context toolbar. • Click right mouse button on Coordinate Systems object, or Global Coordinate System object, or another Coordinate System object, or in the Geometry window> Insert> Coordinate System. Additional Related Information: • Coordinate Systems • Creating Coordinate Systems Object Properties For more information on this object's properties, see the Creating Coordinate Systems (p. 389) section. Coordinate Systems Houses any new coordinate systems that can include a Global Coordinate System object and local Coordinate System objects. Tree Dependencies: • Valid Parent Tree Object: Model • Valid Child Tree Objects: Comment, Coordinate System, Figure, Global Coordinate System, Image Insertion Options: The Coordinate Systems object is automatically inserted into the tree. Note Only one Coordinate Systems (Parent) object is valid per Model. Additional Related Information: • Coordinate Systems 1000 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. End Release • Creating Coordinate Systems Direct FE (Group) Defines the node-based boundary conditions that are used in the Environment object of a model. Applies to the following objects: Nodal Orientation, Nodal Force, Nodal Pressure, FE Displacement, and FE Rotation. Tree Dependencies: • Valid Parent Tree Objects: Environment • Valid Child Tree Objects: – Nodal Orientation – Nodal Force – Nodal Pressure – FE Displacement – FE Rotation Insertion Options: Use any of the following methods after highlighting Environment object: • Click Direct FE on Environment context toolbar. • Click right mouse button on Environment object or in the Geometry window; then Insert> {load type}. Object Properties See the Direct FE section for more information about the load options as well as Details View properties. End Release Allows chosen DOFs to be released on a vertex between line bodies. Tree Dependencies: • Valid Parent Tree Object: Connections • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Connections object: • Click End Release on Connections context toolbar. • Click right mouse button on Connections object or in the Geometry window; then Insert> End Release. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1001 Objects Reference Additional Related Information: • End Releases (p. 486) • Connections Context Toolbar The following right mouse button context menu option is available for this object. • Rename Based on Definition (1) (1) - Description for Contact Region object also applies to Mesh Connection object. The Details view properties for this object include the following. Object Properties The Details view properties for this object include the following. Category Fields/Conditions Scope Scoping Method – Geometry Selection or Named Selection. Edge Geometry Vertex Geometry Definition Coordinate System Translation X Translation Y Translation Z Rotation X Rotation Y Rotation Z Behavior Suppressed Environment (Group) An environment object holds all analysis related objects in a given Model object. The default name of the environment object is the same as the name of the analysis type. All result objects of an analysis are grouped under the Solution object. Tree Dependencies: • Valid Parent Tree Object: Model • Valid Child Tree Objects: Analysis Settings, Comment, Figure, Image, Initial Condition (for some analysis types), all load and support objects, Solution Insertion Options: Appears by default based on the analysis type chosen in the Project Schematic. Additional Related Information: • Analysis Types (p. 17) • Environment Context Toolbar 1002 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Fatigue Tool (Group) • Types of Loads • Types of Supports The following right mouse button context menu options are available for this object. • Solve • Open Solver Files Directory - available for Windows OS only. Object Properties The Details view properties for this object include the following. Category Fields Definition read-only indications. Physics Type Analysis Type Solver Target Options Environment Temperature - the temperature of the body unless this temperature is specified by a particular load such as a thermal condition or an imported temperature. This will also be the material reference temperature unless overridden by the Body (see Reference Temperature (p. 7) under Define Part Behavior (p. 6) for more information). Environment Temperature is not valid for any type of thermal analysis. Generate Input Only Fatigue Tool (Group) Determines life, damage, and factor of safety information using a stress-life or strain-life approach. The Fatigue Tool is available only for Static Structural and Transient Structural analyses. Applies to the following objects: Biaxiality Indication, Damage, Damage Matrix, Equivalent Alternating Stress, Fatigue Sensitivity, Fatigue Tool, Hysteresis, Life, Rainflow Matrix, Safety Factor Tree Dependencies: • • Valid Parent Tree Object: – For Fatigue Tool: Solution – For Biaxiality Indication, Damage, Damage Matrix, Equivalent Alternating Stress, Fatigue Sensitivity, Hysteresis, Life, Rainflow Matrix, Safety Factor: Fatigue Tool Valid Child Tree Objects: – For Fatigue Tool: Biaxiality Indication, Comment, Damage, Damage Matrix, Equivalent Alternating Stress, Fatigue Sensitivity, Hysteresis, Image, Life, Rainflow Matrix, Safety Factor – For Biaxiality Indication, Damage, Equivalent Alternating Stress, Life, Safety Factor: Alert, Comment, Convergence, Figure, Image – For Damage Matrix, Fatigue Sensitivity, Hysteresis, Rainflow Matrix: Comment, Image Insertion Options: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1003 Objects Reference • • For Fatigue Tool, use any of the following methods after highlighting Solution object: – Choose Tools> Fatigue Tool on Solution context toolbar. – Click right mouse button on Solution object or in the Geometry window> Insert> Fatigue> Fatigue Tool. For all fatigue results under Fatigue Tool, use any of the following methods after highlighting Fatigue Tool object: – Choose Contour Results or Graph Results> [specific fatigue result] on Fatigue Tool context toolbar. – Click right mouse button on Fatigue Tool object or in the Geometry window> Insert> [specific fatigue result]. Additional Related Information: • Fatigue Overview • Mechanical Fatigue Material Properties • Fatigue Analysis and Loading Options • Reviewing Fatigue Results The following right mouse button context menu options are available for this object. • Evaluate All Results - available for Fatigue Tool and all child objects. Object Properties The Details view properties for this object include the following. For the Fatigue Tool: Category Fields Materials Fatigue Strength Factor (Kf) Loading Type Loading Ratio - appears only if Type is set to Ratio. History Data Location - appears only if Type is set to History Data. Scale Factor Definition Display Time - enter a time value (within the analysis time limit) to display results at that moment of the analysis. Options Analysis Type Mean Stress Theory Stress Component Bin Size - appears only if Type is set to History Data. Use Quick Rainflow Counting - appears only if Type is set to History Data. Infinite Life - appears if Analysis Type is set to Strain Life; or if Analysis Type is set to Stress Life and Type is set to History Data. Maximum Data Points To Plot - appears only if Type is set to History Data. Life Units Units Name 1004 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Fatigue Tool (Group) 1 cycle is equal to For Biaxiality Indication, Damage, Equivalent Alternating Stress, Life, Safety Factor: Category Fields Scope Scoping Method Path Geometry - Use selection filters to pick geometry, click in the Geometry field, then click Apply. Definition Design Life - available for Damage and Safety Factor. Type - Read-only indication of fatigue object name. Use Average Identifier Results - Readonly indication of the following quantities. Minimum - available for Life, Safety Factor, Biaxiality Indication, Equivalent Alternating Stress. Minimum Occurs On - available for Life, Safety Factor, Biaxiality Indication, Equivalent Alternating Stress. Maximum - available for Damage, Biaxiality Indication, Equivalent Alternating Stress. Maximum Occurs On - available for Damage, Biaxiality Indication, Equivalent Alternating Stress. Information available for Life and Equivalent Alternating Stress. Read-only indication of the following quantities. Time Load Step Substep Iteration Number For Damage Matrix, Fatigue Sensitivity, Hysteresis, Rainflow Matrix: Category Fields Scope Geometry - Use selection filters to pick geometry, click in the Geometry field, then click Apply. Definition available only for Damage Matrix and Fatigue Sensitivity. Sensitivity For - available only for Fatigue Sensitivity. Design Life - available only for Damage Matrix; and Fatigue Sensitivity if Sensitivity For is set to Damage or Safety Factor. General Stress Strain Type - if set to Shear Stress, the General, Options, and Results categories are replaced by a Definition category that includes a Type setting. Options Lower Variation - available only for Fatigue Sensitivity. Upper Variation - available only for Fatigue Sensitivity. Number of Fill Points - available only for Fatigue Sensitivity. Chart Viewing Style - available only for Damage Matrix, Fatigue Sensitivity, and Rainflow Matrix. Points per Segment - available only for Hysteresis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1005 Objects Reference Category Fields Results - available only for Damage Matrix, Hysteresis, and Rainflow Matrix. Read-only indication of the following quantities. Minimum Range - available only for Damage Matrix and Rainflow Matrix. Maximum Range - available only for Damage Matrix and Rainflow Matrix. Minimum Mean - available only for Damage Matrix and Rainflow Matrix. Maximum Mean - available only for Damage Matrix and Rainflow Matrix. Minimum Strain - available only for Hysteresis. Maximum Strain - available only for Hysteresis. Minimum Stress - available only for Hysteresis. Maximum Stress - available only for Hysteresis. Figure Captures any graphic displayed for a particular object in the Geometry window. A Figure object can be further manipulated (rotated for example), unlike an Image object, which is a static screen shot of the current model view or an imported static figure. Popular uses of a Figure object are for presenting specific views and settings for later inclusion in a report. Tree Dependencies: • Valid Parent Tree Object: All objects except Alert, Commands, Comment, Convergence, Image, Project, Result Tracker, Solution Combination, Solution Information • Valid Child Tree Objects: None Insertion Method: Click the New Figure or Image button on standard toolbar and select Figure. Additional Related Information: • Comments, Images, Figures (p. 401) • Viewports • Reports • Standard Toolbar Object Properties Caption is the only property available for the Figure object. It provides an editable text field. Fluid Surface Fluid Surface objects allow you to identify faces that should be grouped together in support of a virtual body for assembly meshing. Tree Dependencies: 1006 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Gasket Mesh Control • Valid Parent Tree Objects: Virtual Body Insertion Options: Use any of these methods: Highlight the Virtual Body object, and then: • In the Details view for the Virtual Body, set Used By Fluid Surface to Yes. • Click the right mouse button and select Insert> Fluid Surface from the context menu. Additional Related Information: • Meshing Capabilities in Workbench • Mesh Context Toolbar • Assembly Meshing • Defining Virtual Bodies Object Properties The Details view properties for this object include the following. Category Fields Scope Faces To Group - Set of faces that should be members of the group. Master Virtual Body - Read-only name of the master Virtual Body. Priority - Determines which group will claim cells in cases where groups overlap. The priority is initially based on the rule: the smaller the volume, the higher the priority. Definition Suppressed - Read-only setting inherited from the Virtual Body. Gasket Mesh Control Available when Body object's Stiffness Behavior is set to Gasket. The control applies a sweep mesh in a chosen direction and drops midside nodes on gasket elements that are parallel to the sweep direction. Tree Dependencies: • Valid Parent Tree Object: Body • Valid Child Tree Objects: None. Insertion Options: Appears automatically when a Body object's Stiffness Behavior is set to Gasket. Additional Related Information: • Using Gaskets (p. 387) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1007 Objects Reference Object Properties The Details view properties for this object include the following. Category Fields Definition Free Face Mesh Type Mesh Method Element Midside Nodes Scope Src/Trg Selection Source Target Geometry Represents attached geometry in the form of an assembly or multibody part from a CAD system or from DesignModeler. Assembly parameters, if available, are viewable under the Geometry object. Tree Dependencies: • Valid Parent Tree Object: Model • Valid Child Tree Objects: Comment, Figure, Image, Layered Section, Part, Point Mass, Thickness Insertion Options: Appears by default with a Model object. Additional Related Information: • Geometry in the Mechanical Application (p. 315) • Attach Geometry The following right mouse button context menu options are available for this object. • Search Faces with Multiple Thicknesses • Refresh Geometry • Reset Body Colors • Show Missing Tessellations • Insert > Virtual Body Object Properties The Details view properties for this object include the following. Category Fields Definition Source - Read-only indication of the path and file name associated with the geometry. Type - Read-only indication of how the original geometry was created (CAD product name or DesignModeler). 1008 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Geometry Category Fields Length Unit - Read-only indication of the length unit originally assigned to the geometry. Exceptions are when importing geometry from CATIA V5 or ACIS, where length units must be specified from a drop down menu. Element Control - Allows manual control of the underlying Mechanical APDL element options (KEYOPTS) for individual Part or Body objects beneath the Geometry object. To manually set Mechanical APDL element options, set Element Control to Manual, then select the Part or Body object. Any element options that are available for you to manually set appear in the Details view of the Part or Body object. For example, the Brick Integration Scheme setting for a Part or Body object becomes available only when Element Control is set to Manual. When Element Control is set to Program Controlled, all element options are automatically controlled and no settings are displayed. The Mechanical APDL application equivalent to this setting is the inclusion of the ETCON,SET command in the input file, which automatically resets options for current-technology elements to optimal settings. Refer to the Mechanical APDL Element Reference in the Mechanical APDL Help for more information about Mechanical APDL elements and element options. Display Style - The default is Body Color which assigns unique colors to individual bodies in a part. Other choices include Part Color, Material, Non linear Material Effects, and Stiffness Behavior. 2D Behavior - Appears only for a designated 2-D simulation. Bounding Box Properties Length X Length Y Length Z Volume Mass - Appears only in the Mechanical application. Any suppressed Part or Body child objects are not included in the mass property values that are displayed. Note If the material density is temperature dependent, the Mass will be computed at the body temperature, or at 22oC (default temperature for an environment). Scale Factor Value - The factor applied to imported geometry for the purpose of modifying the size of the model. The scale factor value of newly imported geometry is 1.0. You can modify the value and that value is expected to be preserved on updated models. Due to tolerances, models that are scaled (especially larger) sometimes have problems meshing. The scale factor limit is from 1e-3 to 1e3. Factors entered beyond that range are ignored. Statistics: - Readonly indication of the entities that comprise the geometry. Active Bodies are those Bodies Active Bodies Nodes Elements Mesh Metric Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1009 Objects Reference Category Fields that are unsuppressed compared to the total number of Bodies. Preferences Import Solid Bodies Import Surface Bodies Import Line Bodies Parameter Processing Personal Parameter Key CAD Attribute Transfer CAD Attribute Prefixes Named Selection Processing Named Selection Prefixes Material Properties Transfer CAD Associativity Import Coordinate Systems Reader Save Part File Import Using Instances Do Smart Update Analysis Type Mixed Import Resolution Enclosure and Symmetry Processing Global Coordinate System Represents the default coordinate system. The origin is defined as 0,0,0 in the model coordinate system. This location serves as the reference location for any local Coordinate System objects inserted under the Global Coordinate System object. Tree Dependencies: • Valid Parent Tree Object: Coordinate Systems • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Automatically inserted in the tree. Additional Related Information: • Coordinate Systems • Creating Coordinate Systems Object Properties The Details view properties for this object include the following. The following are all read-only status indications of the global coordinate system: 1010 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Imported Layered Section Category Fields Definition Type Mechanical APDL System Number - assigns the coordinate system reference number (the first argument of the Mechanical APDL LOCAL command). Origin Origin X Origin Y Origin Z Directional Vectors X Axis Data Y Axis Data Z Axis Data Image Inserts a screen shot of the model in its current view or imports any image in .bmp, .jpg, or png format under a parent object. Its use is similar to inserting a Comment object. Inserted images appear in the Report. Image is a static picture of the current model view. It differs from the Figure object, which is also a picture of the current model view that can be further manipulated (rotated for example). Note Duplicating an image in the tree will result in both the original object and the copied object using the same image file on disk. Altering or deleting either the original or the copied object will result in modification and/or deletion of the image file on disk. Both items in the tree will be affected by the change to one of the objects. Tree Dependencies: • • Valid Parent Tree Objects: – For importing images: All objects – For static image captures: Same parent tree objects as for Figure Valid Child Tree Object: Comment Insertion Method: Click the New Figure or Image button on the standard toolbar and select Image. For importing an image, choose Image from File, then choose an image file from the browse window. Filters are available for listing only image files in .bmp, .jpg, or.png formats. Additional Related Information: • Comments, Images, Figures (p. 401) • Reporting Imported Layered Section Imported Layered Section objects provide layer data that has been made available from an external system upstream of the analysis system. The external system must share the model with the downstream analysis system. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1011 Objects Reference Tree Dependencies: • Valid Parent Tree Objects: Model • Valid Child Tree Object: Comment, Image Insertion Method: • Appears automatically when importing layer data from an external system. Additional Related Information: • Specifying Surface Body Layered Sections (p. 325) Object Properties The Details view properties for this object include the following. Category Fields Definition Type - appears as Imported Layered Section and is a read-only field. Suppressed - select Yes to suppress this object. Material Nonlinear Effects - select yes to include the nonlinear effects from the material properties. The reference temperature specified for the body on which a layered section is defined is used as the reference temperature for the layers. Thermal Strain Effects - select yes to send the coefficient of thermal expansion to the solver. Note These fields are not supported for an Explicit Dynamics analysis. Graphic Properties Layer to Display - defines which layer to display on the model. For information on setting the Layer to Display see Viewing Individual Layers (p. 327). Note that the layer number will correspond to the layer number used by the Mechanical APDL solver, which may not match the layer number of the system providing the layered data. Imported Load (Group) The Imported Load group includes the loads that you have imported from an earlier analysis and want to apply in the present analysis. You can add valid loads under the Imported Load object folder. Applies to: Imported Load object folder and all imported load child objects under the folder. Tree Dependencies: 1012 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Imported Load (Group) • Valid Parent Tree Objects: Any Environment object. • Valid Child Tree Object: Comment, Image, imported load objects Insertion Method: Appears by default for specific analyses with data transfer. Additional Related Information: • Imported Loads Object Properties The Details view properties for the Imported Load object folder include the following. Category Fields Definition Type - read-only indication. Interpolation Type - read-only indication. Suppressed The Details view properties for the imported load object include the following. Category Fields Scope Scoping Method Geometry – appears if Scoping Method is set to Geometry Selection. In this case, use selection filters to pick geometry, click in the Geometry field, then click Apply. Named Selection – appears if Scoping Method is set to Named Selection. Definition Type - read-only indication of imported load. Suppressed Display Preview Row - appears if multiple load steps are used. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1013 Objects Reference Imported Thickness Use the Imported Thickness object to import thickness data generated in a previous analysis for application in a current analysis. Imported Thickness objects are created in Mechanical by linking an External Data system to an analysis’ Model cell in the Project Schematic by right-clicking Setup>Transfer Data To New and selecting an analysis type for the External Data system in the Project Schematic. You can also right-click the Model cell of your project on the Project Schematic and select Transfer Data From New>External Data. Solver Notes: • For the MAPDL solver, thickness on 3D shells is represented at the nodal level via the SECFUNCTION command. For 2D plane stress, thicknesses are calculated as an average value from the element's nodal thickness values and it is input as a real constant for the element. • For the Explicit Dynamics solver the element's nodal thicknesses are converted to an average element thickness. • For Explicit Dynamics (LS-DYNA Export) analyses, thicknesses are applied to the nodes. This is also true for 2D analyses. Applies to: Imported Thickness object folder and all thickness child objects under the folder. Tree Dependencies: • Valid Parent Tree Objects: Imported Thickness Group • Valid Child Tree Object: Comment, Image Insertion Method: • Appears by default for specific analyses with data transfer • Click right mouse button on the Imported Thickness Group object • Click on Thickness in the Geometry toolbar. Additional Related Information: • External Data Import (p. 153) • Specifying Surface Body Thickness (p. 323) • POLYFLOW to Mechanical Data Transfer (p. 158) The following right mouse button context menu options are available for this object. • Search Faces with Multiple Thicknesses 1014 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Imported Thickness (Group) Object Properties The Details view properties for this object include but are not limited to the following. Please see Appendix B. Data Transfer Mesh Mapping for additional information about other categories and settings for Imported Thicknesses. Category Fields Scope Scoping Method- Select the method of choosing objects to which the load is applied: Geometry Selection or Named Selection. Geometry– appears if Scoping Method is set to Geometry Selection. In this case, use selection filters to pick geometry, click in the Geometry field, then click Apply. Named Selection – appears if Scoping Method is set to Named Selection. Definition Type- appears as Imported Thickness and is a read-only field. Suppressed- Select Yes to suppress this load. External Data Identifier- Choose the appropriate data identifier which represents the thickness data from the file. Scale- The amount by which the imported thickness values are scaled before being used for display or solution. Offset- An offset that is added to the imported thickness values before being used for display or solution. Shell Offset- Set the desired shell offset. Advanced Unmapped Data Value- You can specify a thickness value for the unmapped target nodes using the Unmapped Data Value property. By default, a zero thickness value is assigned to the unmapped nodes. For the ANSYS solver, the thickness value at each node must be greater than zero. See External Data Import in the ANSYS Mechanical Application User's Guide for details. Imported Thickness (Group) The External Thickness group includes the thicknesses that you have imported from an earlier analysis and want to apply in the present analysis. You can add valid thicknesses under the Geometry > Imported Thickness object folder by right-clicking the Imported Thickness or the Thickness objects. For a 3D analysis, imported data is specified as a shell thickness but for a 2D analysis, it is defined as a plane element thickness. Plane element thicknesses are calculated as an average value from nodal thickness values and it is input as a real constant for the element. Applies to: Imported Thickness object folder and all external thickness child objects under the folder. Tree Dependencies: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1015 Objects Reference • Valid Parent Tree Objects: Geometry object. • Valid Child Tree Object: Comment, Image, imported thickness objects Insertion Method: • Appears by default when a Mechanical Model cell is connected to an External Data system. • Create a link to an upstream POLYFLOW system. Additional Related Information: • External Data Import (p. 153) • POLYFLOW to Mechanical Data Transfer (p. 158) Object Properties The Details view properties for the Imported Thickness object folder include the following. Category Fields Definition Type A read-only description of the Imported Thickness property. Interpolation Type A read-only description of the Interpolation Type property. Suppressed Enables you to control whether the Imported Thickness characteristics are considered in the solving of the simulation. Initial Conditions Houses initial condition objects for use in a Transient Structural analysis (Velocity only) or an explicit dynamics analysis (Velocity and Angular Velocity). Tree Dependencies: 1016 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Initial Temperature • Valid Parent Tree Object: Transient Structural [for Velocity only], or Explicit Dynamics environment object [for either Velocity or Angular Velocity]. • Valid Child Tree Objects: Angular Velocity (Explicit Dynamics object only), Comment, Figure, Image, Pre-Stress (Explicit Dynamics object only), Velocity Insertion Options: Appears by default for a Transient Structural analysis or an explicit dynamics analysis. Additional Related Information: • Define Initial Conditions • Transient Structural Analysis (p. 91) • Explicit Dynamics Analysis (p. 35) Initial Temperature Defines an initial temperature or an initial temperature distribution for use in a steady-state thermal or transient thermal analysis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1017 Objects Reference Tree Dependencies: • Valid Parent Tree Object: Steady-State Thermal or Transient Thermal analysis environment. • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Appears by default for a steady-state thermal analysis or a transient thermal analysis. Additional Related Information: • Define Initial Conditions • Steady-State Thermal Analysis (p. 84) • Transient Thermal Analysis (p. 133) Object Properties The Details view properties for this object include the following. Category Fields Definition Initial Temperature Initial Temperature Value Joint Defines conditions for reference and mobile pairs that make up a joint. Several Joint objects can appear as child objects under a Connection Group object. The Connection Group object name automatically changes to Joints. Tree Dependencies: 1018 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Layered Section • Valid Parent Tree Object: Connection Group • Valid Child Tree Objects: Comment, Coordinate System, Figure, Image Insertion Options: Use any of the following methods after highlighting Connections object: • Inserted automatically if joints are defined in the CAD model and you choose Create Automatic Connections through a right mouse button click on the Connections (or Joints) object. • Click Body-Ground> {type of joint} or Body-Body> {type of joint} on Connections context toolbar. • Click right mouse button on Connections (or Joints ) object in the Geometry window> Insert> Joint. Additional Related Information: • Joints (p. 433) • Joint Load (p. 581) • Connections Context Toolbar The following right mouse button context menu options are available for this object. • Enable/Disable Transparency • Hide All Other Bodies • Flip Reference/Mobile • Search Connections for Duplicate Pairs • Go To Connections for Duplicate Pairs - available if connection object shares the same geometries with other connection objects. • Promote Remote Point • Rename Based on Definition Object Properties For more information on this object's properties, see the Joint Properties and Application (p. 442) section for specific details. Layered Section Allows you to define layered section properties on selected surface bodies or on selected faces of surface bodies. Tree Dependencies: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1019 Objects Reference • Valid Parent Tree Object: Geometry • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Geometry object : • Click Layered Section button on Geometry context toolbar. • Click right mouse button on Geometry object > Insert> Layered Section. Additional Related Information: • Specifying Surface Body Layered Sections (p. 325) • Geometry Context Toolbar The following right mouse button context menu options are available for this object. • Search Faces with Multiple Thicknesses Object Properties The Details view properties for this object include the following. Category Fields Scope Scoping Method Geometry - appears if Scoping Method is set to Geometry Selection. In this case, use selection filters to pick geometry, click in the Geometry field, then click Apply. Named Selection - appears if Scoping Method is set to Named Selection. Definition Material 1020 Coordinate System Offset Type (this field is not supported for an Explicit Dynamics analysis) Membrane Offset - appears if Offset Type is set to User Defined. Layers - click here to open the worksheet to enter the layer data. Suppressed Nonlinear Effects - select yes to include the nonlinear effects from the material properties. The reference temperature specified for the body on which a layered section is defined is used as the reference temperature for the layers. Thermal Strain Effects - select yes to send the coefficient of thermal expansion to the solver. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Loads, Supports, and Conditions (Group) Note These fields are not supported for an Explicit Dynamics analysis. Graphic Properties Layer to Display - defines which layer to display on the model. Properties Total Thickness - total thickness of all of the layers in the Layered Section. Total Mass - total mass of all of the layers in the Layered Section. Loads, Supports, and Conditions (Group) Defines the individual loads, supports, and conditions used as boundary conditions in the environment for a model. Applies to the following objects: Acceleration, Bearing Load, Bolt Pretension, Compression Only Support, Conductor, Constraint Equation, Convection, Coupling, Current, Cylindrical Support, Detonation Point, Displacement, Elastic Support, FE Displacement, FE Rotation, Fixed Rotation, Fixed Support, Fluid Solid Interface, Force, Frictionless Support, Generalized Plane Strain, Heat Flow, Heat Flux, Hydrostatic Pressure, Impedance Boundary, Internal Heat Generation, Joint Load, Line Pressure, Magnetic Flux Parallel, Moment, Nodal Orientation , Nodal Force, Nodal Pressure, Perfectly Insulated, Pipe Idealization, Pipe Pressure, Pipe Temperature, Pressure, PSD Base Excitation, Radiation, Remote Displacement, Remote Force, Rotational Velocity, RS Base Excitation, Simply Supported, Standard Earth Gravity, Temperature, Thermal Condition, Velocity, Voltage Tree Dependencies: • • Valid Parent Tree Object: – For Magnetostatic Analysis only: Source Conductor when specifying a Current or Voltage – For all other objects: an analysis environment object. Valid Child Tree Objects: – For Magnetostatic Analysis Source Conductor: Comment, Current, Figure, Image, Voltage (Solid Source Conductor only) – For all other objects: Comment, Figure, Image Insertion Options: • • For Current or Voltage, scope to a body, then use any of the following methods: – Choose Conductor or Current on Environment context toolbar, then choose Current or Voltage from the toolbar. – Click right mouse button on Magnetostatic object, or in the Geometry window> Insert> Conductor then > Insert> Current or Voltage For all other objects, use any of the following methods after highlighting Environment object: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1021 Objects Reference – Choose Inertial, or Load, or Supports, or Conditions> {Load, support, or condition name} on Environment context toolbar. – Click right mouse button on Environment object, any load, support, or condition object, or in the Geometry window> Insert> {Load, support, or condition name} Additional Related Information: • Create Analysis System • Apply Loads and Supports Object Properties See the Applying Boundary Conditions section for more information about Loads, Supports, and Conditions. Mesh Manages all meshing functions and tools for a model; includes global controls that govern the entire mesh. Tree Dependencies: • Valid Parent Tree Object: Model • Valid Child Tree Objects: all mesh control tool objects, Comment, Figure, Image Insertion Options: Appears by default when geometry is attached. Additional Related Information: • Meshing Capabilities in Workbench • Mesh Context Toolbar The following right mouse button context menu options are available for this object. • Update • Generate Mesh • Preview> Surface Mesh • Preview> Inflation • Show> Removable Loops • Show> Sweepable Bodies • Show> Mappable Faces 1022 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Mesh • Show> Geometry in Overlapping Named Selections • Show> Program Controlled Inflation Surfaces • Create Pinch Controls • Clear Generated Data Object Properties The Details view properties for this object include the following. Category Defaults Fields Physics Preference Solver Preference (appears if Physics Preference is CFD) Relevance Note Solver Preference also appears in the Mechanical application if the Physics Preference is Mechanical in a Transient Structural or Rigid Dynamics system during the initial geometry attach. See Solver Preference for more information. Sizing Use Advanced Size Function Relevance Center Element Size Initial Size Seed Smoothing Transition Span Angle Center Curvature Normal Angle Proximity Accuracy Num Cells Across Gap Proximity Size Function Sources Min Size Proximity Min Size Max Face Size Max Size Growth Rate Minimum Edge Length Inflation Use Automatic Inflation Inflation Option Transition Ratio Maximum Layers Growth Rate Number of Layers Maximum Thickness First Layer Height First Aspect Ratio Aspect Ratio (Base/Height) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1023 Objects Reference Category Fields Inflation Algorithm View Advanced Options Collision Avoidance Fix First Layer Maximum Height over Base Gap Factor Growth Rate Type Maximum Angle Fillet Ratio Use Post Smoothing Smoothing Iterations Assembly Meshing Method Feature Capture Tessellation Refinement Keep Solid Mesh Patch Conforming Options Triangle Surface Mesher Advanced Shape Checking Element Midside Nodes Straight Sided Element - appears if the model includes an enclosure from DesignModeler. Number of Retries Extra Retries For Assembly Rigid Body Behavior Mesh Morphing Defeaturing Use Sheet Thickness for Pinch Pinch Tolerance Generate Pinch on Refresh Sheet Loop Removal Loop Removal Tolerance Defeaturing Tolerance Statistics Nodes - Read-only indication Elements - Read-only indication Mesh Metric Mesh Connection Defines conditions for joining meshes of topologically disconnected surface bodies. Several Mesh Connection objects can appear as child objects under a Connection Group object. The name of the Connection Group object automatically changes to Mesh Connections. Tree Dependencies: 1024 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Mesh Connection • Valid Parent Tree Object: Connection Group • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Connections or Connection Group object: • Inserted automatically if you choose Create Automatic Connections through a right mouse click on the Connections or Mesh Connections objects. • Click Mesh Connection on Connections context toolbar. • Click right mouse button on Connections (or Mesh Connections) object or in the Geometry window; then Insert> Manual Mesh Connection. Additional Related Information: • Mesh Connection • Automatically Generated Connections • Connections Context Toolbar • Common Connections Folder Operations for Auto Generated Connections (p. 407) The following right mouse button context menu options are available for this object. • Enable/Disable Transparency (1) • Hide All Other Bodies (1) • Flip Master/Slave (1) • Search Connections for Duplicate Pairs (1) • Go To Connections for Duplicate Pairs (1) - available if connection object shares the same geometries with other connection objects. • Rename Based on Definition (1) (1) - Description for Contact Region object also applies to Mesh Connection object. Object Properties The Details view properties for this object include the following. Category Fields/Conditions Scope Scoping Method – Geometry Selection or Named Selection. Master Geometry Slave Geometry Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1025 Objects Reference Category Fields/Conditions Master Bodies - read-only indication. Slave Bodies - read-only indication. Definition Scope Mode - read-only indication of Manual or Automatic. Tolerance Type Tolerance Slider - appears if Tolerance Type = Tolerance Slider. Tolerance Value - appears if Tolerance Type = Tolerance Slider (readonly) or Tolerance Value. Thickness Scale Factor - appears if Tolerance Type = Use Sheet Thickness. Suppressed Snap to Boundary Snap Type - appears if Snap to Boundary = Yes. Snap Tolerance - appears if Snap Type = Manual Tolerance. Master Element Size Factor - appears if Snap Type = Element Size Factor. Mesh Control Tools (Group) Objects available for fine tuning the mesh. Applies to the following objects: Method, Mesh Grouping, Sizing, Contact Sizing, Refinement, Mapped Face Meshing, Match Control, Pinch, Inflation, Sharp Angle, Gap Sizing, Gap Tool Tree Dependencies: • • Valid Parent Tree Object: – For Gap Sizing: Gap Tool – For all other objects: Mesh Valid Child Tree Objects: Comment, Figure, Image Insertion Options: • For Gap Sizing, automatic insertion under the Gap Tool based on detection of gap face pairs. • For all other objects, use any of the following methods after highlighting Mesh object: – Choose Mesh Control> {Mesh control tool name} on Mesh context toolbar. – Click right mouse button on Mesh object, any mesh control tool object, or in the Geometry window> Insert> {Mesh control tool name}. Additional Related Information: • Meshing Capabilities in Workbench • Mesh Context Toolbar 1026 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Mesh Control Tools (Group) • Gap Tool Context Toolbar - applicable to Gap Sizing and Gap Tool • Convergence - applicable to Refinement • Error (Structural) - applicable to Refinement The following right mouse button context menu options are available. Availability is dependent on the selected object. • Inflate This Method - available only for Method control where Method is set to anything other than Hex Dominant, Uniform Quad/Tri, Uniform Quad, or Sweep (unless a source has been specified). • Update • Generate Mesh • Preview> Surface Mesh • Preview> Source and Target Mesh • Preview> Inflation • Show> Sweepable Bodies • Show> Mappable Faces • Create Gap Sizes - available only for Gap Tool • Rename Based on Definition Object Properties The Details view properties for this object include the following. Except where noted, the following applies to all objects other than Gap Tool: Category Fields Scope Scoping Method - specify either Geometry Selection or Named Selection. Not applicable to Contact Sizing, Gap Sizing, Pinch, or Match Control. Geometry - appears if Scoping Method is set to Geometry Selection. In this case, use selection filters to pick geometry, click in the Geometry field, then click Apply. Not applicable to Contact Sizing, Gap Sizing, Pinch, or Match Control. Named Selection - appears if Scoping Method is set to Named Selection. Not applicable to Contact Sizing, Gap Sizing, Pinch, or Match Control. Contact Region - applicable only to Contact Sizing Definition Suppressed Note Additional Definition settings may be available, depending on the specific mesh control tool. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1027 Objects Reference The following applies only to the Gap Tool: Category Fields Definition Define By Minimum Maximum Gap Aspect Ratio Gap Density Generate on Update Mesh Group (Group) Mesh Group objects allow you to identify bodies that should be grouped together for assembly meshing. Also see the description of the Fluid Surface (p. 1006) object (applicable to assembly meshing algorithms only). Tree Dependencies: • Valid Parent Tree Objects: Mesh Grouping Insertion Options: Highlight the Mesh object (or its Mesh Grouping or Mesh Group child object if any exist), and then: • Select Mesh Control> Mesh Group on the Mesh Context Toolbar. • Click the right mouse button on the object you highlighted and select Insert> Mesh Group from the context menu. These methods insert a Mesh Group object beneath the Mesh Grouping object. The Mesh Grouping object is inserted automatically when the first Mesh Group object is inserted. Additional Related Information: • Meshing Capabilities in Workbench • Mesh Context Toolbar • Defining Mesh Groups • Assembly Meshing Object Properties The Details view properties for this object include the following. 1028 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Mesh Numbering Category Fields Scope Bodies To Group - Set of bodies that should be members of the group. All bodies within a group, including the Master Body, should be of the same type (i.e., Fluid or Solid, as defined by the Fluid/Solid material property). Otherwise, unexpected results may occur. Surface bodies cannot be selected for grouping. Master Body - Body that should act as the master of the group. The master body is the body to which all mesh of the group members will be associated. By default, the first body that is selected for Bodies To Group is the Master Body. Priority - Determines which group will claim cells in cases where groups overlap. The priority is initially based on the rule: the smaller the volume, the higher the priority. Definition Suppressed - Toggles suppression of the selected group. The default is No. If set to Yes, the group will be suppressed. Mesh Grouping Represents all definitions of mesh groups within a model. Each definition is represented in a Mesh Group object. May contain any number of Mesh Group objects, which are used for assembly meshing. Tree Dependencies: • Valid Parent Tree Object: Mesh • Valid Child Tree Object: Mesh Group Insertion Options: Automatically inserted in the tree when the first Mesh Group object is inserted. Additional Related Information: • Meshing Capabilities in Workbench • Mesh Context Toolbar • Defining Mesh Groups • Assembly Meshing Mesh Numbering Folder object that includes any number of Numbering Control objects, used for mesh numbering, which allows you to renumber the node and element numbers of a generated meshed model consisting of flexible parts. Tree Dependencies: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1029 Objects Reference • Valid Parent Tree Object: Model • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after selecting Model object: • Click Mesh Numbering button on Model context toolbar. • Click right mouse button on Model object or in the Geometry window> Insert>Mesh Numbering. Additional Related Information: • Mesh Numbering • Model Context Toolbar The following right mouse button context menu options are available for this object. • Renumber Mesh Object Properties The Details view properties for this object include the following. Category Definition Fields Node Offset Element Offset Suppressed Compress Numbers Modal Defines the modal analysis whose mode shapes are to be used in a random vibration, response spectrum, or harmonic (MSUP) linked analysis (not shown below). 1030 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Model Tree Dependencies: • Valid Parent Tree Object: Random Vibration, Response Spectrum, or Harmonic Response (linked) environment object. • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Appears by default for a random vibration analysis, response spectrum analysis, or harmonic (MSUP) linked analysis. Additional Related Information: • Random Vibration Analysis (p. 70) • Response Spectrum Analysis (p. 75) • Harmonic Analysis Using Linked Modal Analysis System (p. 64) Object Properties The Details view properties for this object include the following. Category Definition Fields Modal Environment Model Defines the geometry for the particular branch of the tree. The sub-levels provide additional information about the Model object, including loads, supports and results, but do not replace the geometry. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1031 Objects Reference Graphic settings applied to the Model object apply to lower level objects in the tree. The Model object groups geometry, material assignments, connections, and mesh settings. The Geometry, Connections and Mesh objects are not created until geometry is successfully attached. Tree Dependencies: • Valid Parent Tree Object: Project • Valid Child Tree Objects: Chart, Comment, Connections, Coordinate Systems, environments, Figure, Geometry, Image, Mesh, Named Selection, Solution Combination, Symmetry, Virtual Topology Insertion Options: Appears by default for attached geometry. Additional Related Information: • Attaching Geometry • Model Context Toolbar The following right mouse button context menu options are available for this object. • Solve • Disable Filter/Auto Filter Object Properties The Details view properties for this object include the following. Category Fields Filter Options Control Lighting Ambient Light Diffuse Light Specular Light Light Color Named Selections Named Selections is a folder object that includes any number of individual user-defined Selection objects. Tree Dependencies: 1032 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Named Selections • Valid Parent Tree Object: Model • Valid Child Tree Objects: Individual named selection objects, Comment, Figure, Image Note Comment, Figure, and Image are also child objects of individual named selection objects. Insertion Options: Use any of the following methods: • Click Named Selection button on the Model Context Toolbar (p. 288). • Select geometry items for grouping in the Geometry window, or select Body objects in the tree, then choose Create Named Selection (left button on the Named Selection Toolbar or right-click context menu choice). • Import named selections from a CAD system or from DesignModeler. • Automatically inserted in the event of a mesher failure so that problem surface bodies can be identified. Additional Related Information: • Named Selections • Named Selection Toolbar • Geometry Preferences • Named Selection (DesignModeler Help) • Enclosure (DesignModeler Help) The following right mouse button context menu options are available for child objects of a Named Selections object. • Select Items in Group • Add to Current Selection • Remove from Current Selection • Generate Named Selections Object Properties The Details view properties for this object include the following. The following applies only to the Named Selections object folder: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1033 Objects Reference Category Fields/Descriptions Display Show Mesh Show Annotation Worksheet Based Named Selections Generate on Refresh Generate on Remesh — Updates the Node ids and locations based on the new mesh. The following applies only to the child objects of a Named Selections object folder: Category Fields/Descriptions Scope Geometry Selection Worksheet Definition Send to Solver controls whether the named selection is passed to the solver. Also see Passing Named Selections to the Solver in the Meshing help. Visible - displays named selection when set to Yes. Program Controlled Inflation (Include/Exclude) determines whether faces in the named selection are selected to be inflation boundaries for Program Controlled inflation. Also see Program Controlled inflation in the Meshing help. Statistics Type - Manual if named selection was created in the Mechanical application or generated due to a mesher failure; Imported if named selection was imported. Total Selection Suppressed Hidden Used by Mesh Worksheet - Yes if named selection is being used by the Mesh worksheet. Also see the description of the Mesh worksheet in the Meshing help. Read-only status indications • Tolerance Tolerance Type Program Controlled — Assigns default values. Manual — Makes Zero Tolerance and Relative Tolerance available. • Zero Tolerance • Relative Tolerance — Multiplying factor applied to the values in the entire Worksheet. Numbering Control Represents a part, vertex, or Remote Point whose nodes/elements can be renumbered. Any number of these objects can exist within a Mesh Numbering folder. Tree Dependencies: 1034 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Part • Valid Parent Tree Object: Mesh Numbering • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after selecting Mesh Numbering object: • Click Numbering Control button on Mesh Numbering context toolbar. • Click right mouse button on Mesh Numbering object or in the Geometry window> Insert> Numbering Control. Additional Related Information: • Mesh Numbering • Model Context Toolbar The following right mouse button context menu options are available for this object. • Renumber Mesh Object Properties The Details view properties for this object include the following. Category Fields Scope Scoping Method - specify either Geometry Selection or Remote Point. Geometry - appears if Scoping Method is set to Geometry Selection. Remote Points - appears if Scoping Method is set to Remote Point. Definition Begin Node Number - appears if Geometry is set to a part. End Node Number - appears if Geometry is set to a part. Begin Element Number - appears if Geometry is set to a part. End Element Number - appears if Geometry is set to a part. Node Number - appears if Geometry is set to a vertex or if Remote Points is set to a specific Remote Point. Suppressed Part Defines a component of the attached geometry included under a Geometry object. The Part object is assumed to be a multibody part with Body objects beneath it as depicted in the figure below. The Part object label in your Project tree inherits the name from the CAD application you use to create the part and may differ based on the CAD application. Refer to the Body objects reference page if the Geometry object does not include a multibody part, but instead only includes individual bodies. Also see the description of the Virtual Body Group (p. 1065) object (applicable to assembly meshing algorithms only). Tree Dependencies: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1035 Objects Reference • Valid Parent Tree Object: Geometry • Valid Child Tree Objects: Body, Comment, Figure, Image Insertion Options: Appears by default when geometry is attached that includes a multibody part. Additional Related Information: • Attaching Geometry The following right mouse button context menu options are available for this object. • Search Faces with Multiple Thicknesses • Create Selection Group • Generate Mesh • Preview> Surface Mesh - appears only for a solid body. • Preview> Inflation Object Properties The Details view properties for this object include the following. Category Fields Graphics Properties Visible - Turns part display On or Off in the Geometry window. Definition Suppressed Assignment Brick Integration Scheme - appears only if Element Control is set to Manual in the Details view of the Geometry object. Coordinate System - Assign a local coordinate system to specify the alignment of the elements of the part if previously defined using one or more Coordinate System objects; not available if Stiffness Behavior is set to Rigid. Bounding Box Length X Length Y Length Z Properties - Readonly indication of the properties originally assigned to the part. Volume Mass - Appears only in the Mechanical application. Note If the material density is temperature dependent, the Mass will be computed at the body temperature, or at 22oC (default temperature for an environment). Centroid X Centroid Y Centroid Z 1036 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Path Moment of Inertia Ip1 Moment of Inertia Ip2 Moment of Inertia Ip3 Surface Areas (approx.) Statistics - Readonly indication of the entities that comprise the part. Nodes Elements Mesh Metric Path Represents a spatial curve to which you can scope results. The results are evaluated at discrete points along this curve. Tree Dependencies: • Valid Parent Tree Object: Construction Geometry • Valid Child Tree Objects: Comment, Figure, Image. Insertion Options: Use any of the following methods after selecting Construction Geometry object: • Click Path button on Construction Geometry context toolbar. • Click right mouse button on Construction Geometry object or in the Geometry window> Insert>Path. Additional Related Information: • Path (Construction Geometry) (p. 376) • Construction Geometry (p. 993) object reference The following right mouse button context menu options are available for this object. • Snap to mesh nodes • Export Object Properties The Details view properties for this object include the following. Category Fields Definition Path Type Path Coordinate System Number of Sampling Points Suppressed Show Mesh Start Coordinate System Start X Coordinate Start Y Coordinate Start Z Coordinate Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1037 Objects Reference Category Fields Location Coordinate System End X Coordinate End Y Coordinate End Z Coordinate Location End Periodic/Cyclic Region Defines an individual plane for periodic conditions, anti-periodic conditions, or cyclic conditions. The collection of all Periodic/Cyclic Region objects exists under one Symmetry object. Tree Dependencies: • Valid Parent Tree Object: Symmetry • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Symmetry object: • Choose Periodic/Cyclic Region on Symmetry context toolbar. • Click right mouse button on Symmetry object, on an existing Periodic/Cyclic Region or Symmetry Region object, or in the Geometry window> Insert> Periodic/Cyclic Region. Additional Related Information: • Symmetry • Symmetry Context Toolbar The following right mouse button context menu option is available for this object. • Flip High/Low 1038 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Point Mass Object Properties The Details view properties for this object include the following. Category Fields Scope Scoping Method Low Boundary - appears if Scoping Method is set to Geometry Selection. High Boundary - appears if Scoping Method is set to Geometry Selection. Low Selection - appears if Scoping Method is set to Named Selection. High Selection - appears if Scoping Method is set to Named Selection. Definition Scope Mode Type - appears for Periodic Region only. Coordinate System Suppressed Point Mass Represents the inertial effects from a body. Tree Dependencies: • Valid Parent Tree Object: Geometry • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Geometry object or Body object: • Click Point Mass button on Geometry context toolbar. • Click right mouse button on Geometry object, Body object, or in the Geometry window> Insert> Point Mass. Additional Related Information: • Point Mass • Coordinate Systems • Geometry Context Toolbar The following right mouse button context menu options are available for this object. • Promote Remote Point Object Properties The Details view properties for this object include the following. Category Fields Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1039 Objects Reference Scope Scoping method Geometry - Use selection filters to pick geometry, click in the Geometry field, then click Apply. Coordinate System - Assign load to a local coordinate system if previously defined using one or more Coordinate System objects. The Point Mass will automatically be rotated into the selected coordinate system if that coordinate system differs from the global coordinate system. X Coordinate - Define x coordinate location; can be designated as a parameter. Y Coordinate - Define y coordinate location; can be designated as a parameter. Z Coordinate - Define z coordinate location; can be designated as a parameter. Location - Change location of the load. Pick new location, click in the Location field, then click Apply. Definition Mass - Define mass; can be designated as a parameter. Mass Moment of Inertia X - Available for 3D models only. Mass Moment of Inertia Y - Available for 3D models only. Mass Moment of Inertia Z - Available for 2D and 3D models. Suppressed Behavior Pinball Region Pre-Stress Defines the structural analysis whose stress results are to be used in a modal analysis, or whose stressstiffening effects are to be used in a linear buckling analysis, or whose stresses, strains, and/or displacements, or velocities are to be used in an explicit dynamics analysis . Tree Dependencies: • Valid Parent Tree Object: Modal, or Linear Buckling , or Explicit Dynamics environment object. • Valid Child Tree Objects: Commands, Comment, Figure, Image Insertion Options: Appears by default for a modal analysis, a linear buckling analysis, or an explicit dynamics analysis. Additional Related Information: • Modal Analysis (p. 25) • Linear Buckling Analysis (p. 20) • Explicit Dynamics Analysis (p. 35) 1040 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Pre-Stress • Define Initial Conditions Object Properties The Details view properties for this object include the following. Category Definition Fields Pre-Stress Environment Pre-Stress Define By - (applicable only to Modal or Linear Buckling environments) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1041 Objects Reference Pre-Stress Time - (applicable only to Modal or Linear Buckling environments) Reported Loadstep - (applicable only to Modal or Linear Buckling environments) Reported Substep - (applicable only to Modal or Linear Buckling environments) Reported Time - (applicable only to Modal or Linear Buckling environments) Contact Status - (applicable only to Modal or Linear Buckling environments) Mode (applicable only to an Explicit Dynamics environment) Time (applicable only to an Explicit Dynamics environment) Time Step Factor (applicable only to an Explicit Dynamics environment for Mode = Displacements) Note Links in this Fields column describe applicability to a Modal analysis. The same descriptions apply to a Linear Buckling analysis. Probe Determines results at a point on a model or finds minimum or maximum results on a body, face, vertex, or edge. Tree Dependencies: • Valid Parent Tree Object: Solution • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: • Use any of the following methods after highlighting Solution object or an existing Probe object: – Choose Probe> {specific probe} on Solution context toolbar. – Click right mouse button on Solution object or in the Geometry window> Insert> Probe> {specific probe}. Additional Related Information: • Probes (p. 737) The following right mouse button context menu options are available for this object: Evaluate All Results Object Properties See the Probe Details View (p. 739) section. 1042 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Project Project Includes all objects in the Mechanical application and represents the highest level in the object tree. Only one Project can exist per Mechanical session. Tree Dependencies: • Valid Parent Tree Object: None - highest level in the tree. • Valid Child Tree Objects: Comment, Model Insertion Options: Appears by default in every Mechanical session. Object Properties The Details view properties for this object include the following. Category Fields Title Page - You can enter the following information that will appear on the title page of the report. Author Subject Prepared for Information - The Mechanical application provides the following information that will appear on the title page of the report. First Saved Last Saved Product Version Project data Management Save Project Before Solution- Saves the entire project immediately before solving (after any required meshing). If the project had never been previously saved, you can now select a location to save a new file. Save Project After Solution- Saves the project immediately after solving but before postprocessing. If the project had never been previously saved, nothing will be saved. Note • The default values can be specified in Tools > Options under the Miscellaneous section. • The Save Options defaults are applicable only to new projects. These settings will not be changed for existing projects. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1043 Objects Reference Remote Point Allows scoping of remote boundary conditions. Tree Dependencies: • Valid Parent Tree Object: Remote Points. • Valid Child Tree Objects: Commands, Comment, Figure Insertion Options: Use any of the following methods after highlighting Model or Remote Points object: • Choose Remote Point on Model or Remote Points context toolbar. • Click right mouse button on the Model or Remote Points object or in the Geometry window and select Insert> Remote Point. Additional Related Information: • Remote Point • Remote Boundary Conditions The Details view properties for this object include the following. Category Fields Scope Scoping Method Geometry - appears if Scoping Method is set to Geometry Selection. Choose geometry entity then click on Apply. Named Selection - appears if Scoping Method is set to Named Selection. Choose a Named Selection from the drop-down menu. Coordinate System X Coordinate Y Coordinate Z Coordinate Location Definition Suppressed Behavior Pinball Region Remote Points Houses all Remote Point objects. 1044 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Result Tracker Tree Dependencies: • Valid Parent Tree Object: Model • Valid Child Tree Objects: Comment Remote Point Insertion Options: Use any of the following methods after highlighting Model object: • Choose Remote Point on Model context toolbar. • Click right mouse button on the Model object or in the Geometry window, select Insert> Remote Point. Additional Related Information: • Remote Point • Remote Boundary Conditions Object Property The Details view property for this object includes the following. Category Fields Graphics Show Connection Lines Result Tracker Provides results graphs of various quantities (for example, deformation, contact, temperature, kinetic energy, stiffness energy) vs. time. Tree Dependencies: • Valid Parent Tree Object: Solution Information • Valid Child Tree Objects: Comment, Image Insertion Options: Use any of the following methods after highlighting Solution Information object: • Choose Result Tracker> {name of Result Tracker} on Solution Information context toolbar. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1045 Objects Reference Note You will not be able to add a Result Tracker from the Solution Information context toolbar if the solution is in a solved state. You will need to clear the solution before adding a Result Tracker. • Click right mouse button on Solution Information object or in the Geometry window> Insert> {name of Result Tracker}. Additional Related Information: • Result Tracker Objects • Solution Context Toolbar The following right mouse button context menu options are available for this object. • Export - available after solution is obtained. • Rename Based on Definition Object Properties The Details view properties for this object include the following. Note Properties may differ for Result Trackers in Explicit Dynamics systems. See Explicit Dynamics Result Trackers (p. 777) for more information. Category Fields Definition Type - Read-only indication of result tracker type for Deformation and Temperature objects. For Contact object, specify contact output. Orientation - appears for a Deformation result tracker object. Suppression – Prior to solving, you can include or exclude the result from the analysis. The default is value is No. Scope Scoping Method - appears for a Temperature result tracker object. Geometry - appears for a Deformation result tracker object, or for a Temperature object if Scoping Method is set to Geometry Selection. Use selection filters to pick geometry, click in the Geometry field, then click Apply. Contact Region - appears for a Contact result tracker object. Results Minimum - Read-only indication of the minimum value of the result tracker type. Maximum - Read-only indication of the maximum value of the result tracker type. 1046 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results and Result Tools (Group) Filter - displayed only for Explicit Dynamics systems. Type Cut Frequency - appears if Type = Butterworth. Minimum filtered value - appears if Type = Butterworth. Maximum filtered value - appears if Type = Butterworth. Results and Result Tools (Group) Defines the engineering output for displaying and analyzing the results from a solution. Applies to the following objects: Category Object Structural Bending Stress, Campbell Diagram, Directional Acceleration, Directional Deformation, Directional Velocity, Elastic Strain Intensity, Equivalent Creep Strain, Equivalent Plastic Strain, Equivalent Stress,Equivalent Total Strain,Frequency Response,Linearized Stresses,Maximum Principal Elastic Strain, Maximum Principal Stress, Maximum Shear Elastic Strain, Maximum Shear Stress, Membrane Stress, Middle Principal Elastic Strain, Middle Principal Stress, Minimum Principal Elastic Strain,Minimum Principal Stress,Normal Elastic Strain,Normal Gasket Pressure, Normal Gasket Total Closure, Normal Stress, Phase Response, Shear Elastic Strain, Shear Gasket Pressure,Shear Gasket Total Closure,Shear Stress,Strain Energy,Stress Intensity, Structural Error, Thermal Strain, Total Acceleration, Total Deformation, Total Velocity, Vector Principal Elastic Strain, Vector Principal Stress Structural Beams Axial Force, Beam Tool, Bending Moment, Direct Stress, Maximum Bending Stress, Maximum Combined Stress, Minimum Bending Stress, Minimum Combined Stress, Shear Force, ShearMoment Diagram, Torsional Moment Thermal Directional Heat Flux, Temperature, Thermal Error, Total Heat Flux Magnetostatic Current Density, Directional Field Intensity, Directional Flux Density, Directional Force, Electric Potential, Flux Linkage, Inductance, Magnetic Error, Total Field Intensity, Total Flux Density, Total Force Electric Directional Current Density, Directional Electric Field Intensity, Electric Voltage, Joule Heat, Total Current Density, Total Electric Field Intensity General Coordinate Systems Results (group), User Defined Result Tree Dependencies: • • Valid Parent Tree Object: – For Direct Stress, Maximum Bending Stress, Maximum Combined Stress, Minimum Bending Stress, Minimum Combined Stress: Beam Tool – For Directional Deformation, Total Deformation: Beam Tool, Solution – For all other result objects: Solution Valid Child Tree Objects: – For Beam Tool: Comment, Direct Stress, Directional Deformation, Figure, Image, Maximum Bending Stress, Maximum Combined Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1047 Objects Reference Stress, Minimum Bending Stress, Minimum Combined Stress, Total Deformation – For all other objects: Comment, Figure, Image Note Alert and Convergence may also apply. Insertion Options: • • For results and result tools that are direct child objects of a Solution object, use any of the following methods after highlighting the Solution object: – Choose toolbar button or result category on Solution context toolbar. – Click right mouse button on Solution object, or in the Geometry window> Insert> {result or result category}. For results that are direct child objects of a specific result tool, use any of the following methods after highlighting the specific result tool object: – Choose result on the context toolbar related to the result tool. – Click right mouse button on specific result tool object> Insert> {specific result related to result tool} Additional Related Information: • Results in the Mechanical Application (p. 634) • Solution Context Toolbar • Surface Body Results (p. 727) The following right mouse button context menu options are available for this object. • Evaluate All Results • Convert To Path Result (for Results scoped to Edges Only) Object Properties The Details view properties for this object may include the following. The following applies to many result objects whose direct parent object is Solution. Many exceptions are noted. For more complete information check individual descriptions for all results and result tools. Category Fields Scope Scoping Method - Geometry Selection, Named Selection, Path, or Surface. Geometry - appears if Scoping Method = Geometry. Use selection filters to pick geometry, click in the Geometry field, then click Apply. Named Selection - appears if Scoping Method = Named Selection. Specify named selection. 1048 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Results and Result Tools (Group) Path - appears if Scoping Method = Path. Select defined path. Surface - appears if Scoping Method = Surface. Select defined surface. Shell - appears only for stress and strain results scoped to a surface body. Layer — Specifies the layer to calculate Shell result values. Definition Type - result type indication, can be changed within the same result category. Read-only indication for: Current Density, Electric Potential, Equivalent Plastic Strain, Strain Energy, Magnetic Error, Structural Error, Temperature, Thermal Error, User Defined Result, Vector Principal Elastic Strain, Vector Principal Stress. Orientation - appears only for: Axial Force, Directional Deformation, Directional Field Intensity, Directional Flux Density, Directional Force, Directional Heat Flux, Normal Elastic Strain, Normal Stress, Shear Elastic Strain, Shear Stress, Torsional Moment, Shell Membrane Stress, Shell Bending Stress. Expression - appears only for User Defined Result. Input Unit System - appears only for User Defined Result. Output Unit - appears only for User Defined Result. Identifier - appears only for User Defined Result. Coordinate System - only displayed for results that change with respect to a coordinate system, such as Normal Stress. For these result types you can specify: default Global Coordinate System, local Coordinate System, or Solution Coordinate System (for most element types the Solution Coordinate System aligns with the global coordinate system, however, for surface and line bodies, elements may align themselves on a per element basis and therefore create random alignments. To correct this, specify a local coordinate system on each part and choose Solution Coordinate System option to ensure that the displayed elements have a consistent alignment). By - Maximum Over “...” is the maximum result over an independent variable for the node, element, or sample point. “...” of Maximum is the value of the independent variable that the maximum occurred for the node, element, or sample point. Neither option is available for non-cyclic modal results, or linearized stress results. Display Time - appears if By is set to Time. (See Note below.) Frequency - appears if By is set to Frequency. (See Note below.) Set Number - appears if By is set to Set. Mode - appears for Modal analyses. Calculate Time History - appears if By is set to Time or Set. Phase Angle - appears if By is set to Frequency, Set (harmonic and cyclic modal analyses), Maximum Over Frequency, or Frequency of Maximum. Identifier - appears only for User Defined Result. Suppressed — Suppresses the object if set to Yes. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1049 Objects Reference Note If you specify a Display Time or Frequency value which exceeds the final time or frequency in the result file, then Mechanical will not allow the result to be evaluated. If you specify a Display Time or Frequency value for which no results are available, then Mechanical performs a linear interpolation to calculate the results at that specified time. The two times or frequencies in the result file that are the closest to the specified time/frequency are used in the interpolation. Integration Point Results Display Option - appears only for result items that can display un-averaged contour results. Results - Readonly status indication of result object. Minimum - not available for Vector Principal Stress. Maximum - not available for Vector Principal Stress. Minimum Occurs On - not available for: Current Density, Electric Potential, Strain Energy, Vector Principal Stress. Maximum Occurs On - - not available for: Current Density, Electric Potential, Strain Energy, Vector Principal Stress. Information Read-only status indication of time stepping. Time Load Step Substep Iteration Number Solution Defines result types and formats for viewing a solution. Tree Dependencies: • Valid Parent Tree Object: Any environment object. • Valid Child Tree Objects: All general Results and Result Tools, Commands, Comment, Figure, Image, Solution Information Insertion Options: Appears by default for any analysis. Note A Solution object cannot be deleted from the tree. Additional Related Information: • Solving Overview (p. 751) • Solution Context Toolbar • Adaptive Convergence The following right mouse button context menu options are available for this object. 1050 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Solution Information • Evaluate All Results • Stop Solution - available only for RSM solutions. • Interrupt Solution - available only for RSM solutions. • Open Solver Files Directory - available for Windows OS only. Object Properties The Details view properties for this object include the following. Category Fields Adaptive Mesh Refinement Max Refinement Loops Refinement Depth Refinement Controls appears only for magnetostatic analyses if a Convergence object is inserted under a result. Element Selection Energy Based - appears if Element Selection is set to Manual. Error Based - appears if Element Selection is set to Manual. Solution Combination Manages solutions that are derived from the results of one or more environments. See Design Assessment for additional Solution Combination capabilities. Tree Dependencies: • Valid Parent Tree Object: Model • Valid Child Tree Objects: all stress and strain result objects, Directional Deformation, Total Deformation, Contact Tool (only for Frictional Stress, Penetration, Pressure, and Sliding Distance), Fatigue Tool , Stress Tool, Comment, Image Insertion Options: Use any of the following methods after highlighting Model object: • Choose Solution Combination on Model context toolbar. • Click right mouse button on Model object or in the Geometry window> Insert> Solution Combination. Additional Related Information: • Solution Combinations • Underdefined Solution Combinations (Troubleshooting) The Evaluate All Results right mouse button context menu option is available for this object. Solution Information Allows tracking, monitoring, or diagnosing of problems that arise during a nonlinear solution. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1051 Objects Reference Also allows viewing certain finite element aspects of the engineering model. Tree Dependencies: • Valid Parent Tree Object: Connections, Solution • Valid Child Tree Objects: Comment, Image, Result Tracker (available only when Solution is the parent) Insertion Options:: • Automatically inserted under a Solution object of a new environment or of an environment included in a database from a previous release. • Click right mouse button on Connections object or in the Geometry window> Insert> Solution Information. Additional Related Information: • Solution Information The following right mouse button context menu option is available for this object. • Export FE Connections Object Properties The Details view properties for this object include the following. Category Fields Solution Information Solution Output - not applicable to Connections object. Newton-Raphson Residuals - applicable only to Structural environments. Update Interval - appears for synchronous solutions only Display Points - not applicable to Connections object. Display Filter During Solve - appears for Explicit Dynamics systems only. FE Connection Visibility Activate Visibility Display Line Color Color - appears if Line Color is set to Manual. Visible on Results Line Thickness Spot Weld Defines conditions for individual contact and target pairs for a spot weld, which is used to connect individual surface body parts to form a surface body model assembly , just as a Contact Region object is used to form a solid model assembly. Several Spot Weld objects can appear as child objects under a Connection Group object. The Connection Group object name automatically changes to Contacts. Tree Dependencies: 1052 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Spot Weld • Valid Parent Tree Object: Connections • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Connections object: • Inserted automatically if spot welds are defined in the CAD model and you choose Create Automatic Connections through a right mouse click on Connections (or Contacts) object. • Click Spot Weld button on Connections context toolbar. • Click right mouse button on Connections (or Connection Group) object or in the Geometry window > Insert> Spot Weld. Additional Related Information: • Spot Welds • Connections Context Toolbar The following right mouse button context menu options are available for this object. • Enable/Disable Transparency • Hide All Other Bodies • Flip Contact/Target • Merge Selected Contact Regions - appears if contact regions share the same geometry type. • Save Contact Region Settings • Load Contact Region Settings • Reset to Default • Rename Based on Definition Object Properties The Details view properties for this object include the following. Category Fields Scope Scoping Method Contact Target Contact Bodies Target Bodies Definition Scope Mode ed Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1053 Objects Reference Spring An elastic element that regains its undeformed shape after a compression or extension load is removed. Tree Dependencies: • Valid Parent Tree Object: Connections • Valid Child Tree Objects: Commands, Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Connections object: • Click Body-Ground> Spring or Body-Body> Spring, as applicable on Connections context toolbar. • Click right mouse button on Connections object or in the Geometry window> Insert> Spring. Additional Related Information: • Connections Context Toolbar • Springs (p. 478) The following right mouse button context menu options are available for this object. • Enable/Disable Transparency - similar behavior to feature in Contact Region. • Rename Based on Definition - similar behavior to feature in Contact Region. • Promote Remote Point Object Properties The Details view properties for this object include the following. Category Fields Graphics Properties Visible Definition Type - read only indication of Longitudinal Spring Behavior (rigid dynamics analyses only) Longitudinal Stiffness Longitudinal Damping Preload ed Spring Length - read only indication. (rigid dynamics analyses only) Scope Scope Reference Scoping Method Reference Component - appears if Scope (under Scope group) is set to BodyBody and Scoping Method is set to Named Selection. Scope - appears if Scope (under Scope group) is set to Body-Body and Scoping Method is set to Geometry Selection. Choose geometry entity then click on Apply. 1054 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Stress Tool (Group) Body- appears if Scope (under Scope group) is set to Body-Body and Scoping Method is set to Geometry Selection. Read-only indication of scoped geometry. Coordinate System Reference X Coordinate Reference Y Coordinate Reference Z Coordinate Reference Location Behavior Pinball Region Mobile Mobile Component - appears if Scoping Method is set to Named Selection. Scope - appears if Scoping Method is set to Geometry Selection. Choose geometry entity then click on Apply. Body- appears if Scoping Method is set to Geometry Selection. Read-only indication of scoped geometry. Coordinate System Mobile X Coordinate Mobile Y Coordinate Mobile Z Coordinate Mobile Location Behavior Pinball Region Stress Tool (Group) Provides stress safety tools for analyzing simulation results. Applies to the following objects: Safety Factor, Safety Margin, Stress Ratio, Stress Tool Tree Dependencies: • • Valid Parent Tree Object: – For Stress Tool: Solution in a static structural or transient structural analysis. – For Safety Factor, Safety Margin, or Stress Ratio: Stress Tool Valid Child Tree Objects: – For Stress Tool: Comment, Figure, Image, Safety Factor, Safety Margin, Stress Ratio – For Safety Factor, Safety Margin, or Stress Ratio: Alert, Comment, Convergence, Figure, Image Insertion Options: • For Stress Tool, use any of the following methods after highlighting Solution object in a static structural or transient structural analysis: – Choose Tools> Stress Tool on Solution context toolbar. – Click right mouse button on Solution object or in the Geometry window> Insert> Stress Tool> Max Equivalent Stress or Max Shear Stress or Mohr-Coulomb Stress or Max Tensile Stress. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1055 Objects Reference • For Safety Factor, Safety Margin, or Stress Ratio, use any of the following methods after highlighting Stress Tool object: – Choose Safety Factor, Safety Margin, or Stress Ratio on Stress Tool context toolbar. – Click right mouse button on Stress Tool object or in the Geometry window> Insert> Stress Tool>Safety Factor, Safety Margin, or Stress Ratio. Additional Related Information: • Stress Tools (p. 658) • Maximum Equivalent Stress Safety Tool (p. 659) • Maximum Shear Stress Safety Tool (p. 661) • Mohr-Coulomb Stress Safety Tool (p. 662) • Maximum Tensile Stress Safety Tool (p. 664) The right mouse button context menu option Evaluate All Results - is available for Safety Factor, Safety Margin, Stress Ratio, and Stress Tool . Object Properties The Details view properties for this object include the following. For Stress Tool: Category Fields Definition Theory Factor - appears only if Theory is set to Max Shear Stress. Stress Limit - appears only if Stress Limit Type is set to Custom Value. Stress Limit Type - appears if Theory is set to any stress tool except Mohr-Coulomb Stress. Tensile Limit - appears only if Theory is set to Mohr-Coulomb Stress and Tensile Limit Type is set to Custom Value. Compressive Limit - appears only if Theory is set to Mohr-Coulomb Stress and Compressive Limit Type is set to Custom Value. Tensile Limit Type - appears only if Theory is set to Mohr-Coulomb Stress. Compressive Limit Type - appears only if Theory is set to Mohr-Coulomb Stress. For Safety Factor, Safety Margin, or Stress Ratio: Category Fields Scope Scoping Method Geometry - Use selection filters to pick geometry, click in the Geometry field, then click Apply. Definition Type – Read-only display of specific stress tool object name. By Display Time Calculate Time History Use Average 1056 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Symmetry Identifier Results - Readonly display of the following values: Minimum Maximum - appears only for Stress Ratio. Minimum Occurs On Maximum Occurs On - appears only for Stress Ratio. Information Read-only display of the following values: Time Load Step Substep Iteration Number Surface Represents a section plane to which you can scope results. Tree Dependencies: • Valid Parent Tree Object: Construction Geometry • Valid Child Tree Objects: Comment, Figure, Image. Insertion Options: Use any of the following methods after selecting Construction Geometry object: • Click Surface button on Construction Geometry context toolbar. • Click right mouse button on Construction Geometry object or in the Geometry window> Insert> Surface. Additional Related Information: • Surface (Construction Geometry) (p. 381) • Construction Geometry (p. 993) object reference Object Properties The Details view properties for this object include the following. Category Fields Definition Coordinate System ed Symmetry Represents all definitions of symmetry or periodic/cyclic planes within a model. Each symmetry definition is represented in a Symmetry Region object, each periodic definition is represented in a Periodic Region object, and each cyclic definition is represented in a Cyclic Region object. Tree Dependencies: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1057 Objects Reference • Valid Parent Tree Object: Model • Valid Child Tree Objects: Comment, Figure, Image, Periodic/Cyclic Region, Symmetry Region Insertion Options: • Automatically inserted in the tree if model includes symmetry planes defined in DesignModeler (using the Symmetry or Enclosure feature). • For manual insertion, use any of the following methods after highlighting Model object: – Choose Symmetry on Model context toolbar. – Click right mouse button on Model object or in the Geometry window> Insert> Symmetry. Note Only one Symmetry object is valid per Model. Additional Related Information: • Symmetry • Symmetry Context Toolbar Symmetry Region Defines an individual plane for symmetry or anti-symmetry conditions. The collection of all Symmetry Region objects exists under one Symmetry object. Tree Dependencies: • Valid Parent Tree Object: Symmetry • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: • Automatically inserted in the tree if model includes symmetry planes defined in DesignModeler (using the Symmetry or Enclosure feature). • For manual insertion, use any of the following methods after highlighting Symmetry object: – Choose Symmetry Region on Symmetry context toolbar. – Click right mouse button on Symmetry object, on an existing Symmetry Region, Periodic Region, or Cyclic Region object, or in the Geometry window > Insert> Symmetry Region. Additional Related Information: • Symmetry 1058 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Thermal Point Mass • Symmetry Context Toolbar Object Properties The Details view properties for this object include the following. Category Fields Scoping Method Geometry - appears if Scoping Method is set to Geometry Selection. Named Selection - appears if Scoping Method is set to Named Selection. Scope Definition Scope Mode Type Coordinate System Symmetry Normal Suppress Thermal Point Mass Represents heat from surrounding objects. Tree Dependencies: • Valid Parent Tree Object: Geometry • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Geometry object or Body object: • Click Thermal Point Mass button on Geometry context toolbar. • Click right mouse button on Geometry object, Body object, or in the Geometry window> Insert> Thermal Point Mass. Additional Related Information: • Thermal Point Mass • Coordinate Systems • Geometry Context Toolbar The following right mouse button context menu options are available for this object. • Promote Remote Point Object Properties The Details view properties for this object include the following. Category Fields Scope Scoping method Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1059 Objects Reference Geometry - Use selection filters to pick geometry, click in the Geometry field, then click Apply. Coordinate System - Assign load to a local coordinate system if previously defined using one or more Coordinate System objects. The Thermal Point Mass will automatically be rotated into the selected coordinate system if that coordinate system differs from the global coordinate system. X Coordinate - Define x coordinate location; can be designated as a parameter. Y Coordinate - Define y coordinate location; can be designated as a parameter. Z Coordinate - Define z coordinate location; can be designated as a parameter. Location - Change location of the load. Pick new location, click in the Location field, then click Apply. Thermal Capacitance Suppressed Behavior Pinball Region Definition Thickness Allows you to define variable thickness properties on selected faces of surface bodies. Tree Dependencies: • Valid Parent Tree Object: Geometry • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Geometry object or Body object: • Click Thickness button on Geometry context toolbar. • Click right mouse button on Geometry object, Body object, or in the Geometry window> Insert> Thickness. Additional Related Information: • Specifying Surface Body Thickness (p. 323) • Geometry Context Toolbar The following right mouse button context menu options are available for this object. • Search Faces with Multiple Thicknesses • Promote Remote Point Object Properties The Details view properties for this object include the following. Category 1060 Fields Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Validation Scoping Method Scope Geometry– appears if Scoping Method is set to Geometry Selection. In this case, use selection filters to pick geometry, click in the Geometry field, then click Apply. Named Selection – appears if Scoping Method is set to Named Selection. Definition Scope Mode- read-only indication of Manual or Automatic. Suppressed Thickness Offset Type Tabular Data - appears if Thickness is set to Tabular Data. Independent Variable Coordinate System Function - appears if Thickness is set to a function. Unit System - read only indication of the active unit system. Angular Measure - read only indication of the angular measure used to evaluate trigonometric functions. Graph Controls - appears if Thickness is set to a function. Number of Segments Range Minimum Range Maximum Note The above description applies to a Thickness object that you manually insert into the tree. When you include thickness associated with a surface body that you import from DesignModeler, an automatically generated Thickness object is added as a child object beneath the associated Surface Body object. Read only object properties in the Scope and Definition categories are available for these automatically generated Thickness objects. Additionally, the right-click context menu item Make Thickness Manual is available for the automatically generated version of the object. Validation The Validation object enables you to evaluate the quality of mapping across source and target meshes. It provides quantitative measures that help in identifying regions on the target where the mapping failed to provide an accurate estimate of the source data. You can add validation objects under the Imported Load or Imported Thickness objects. Applies to: Validation objects. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1061 Objects Reference Tree Dependencies: • Valid Parent Tree Objects: Imported Load or Imported Thickness objects. • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting the Imported Load or Imported Thickness objects: • Select Validation in the Environment/Geometry Context Toolbar • Click the right-mouse button on the object you highlighted and select Insert > Validation from the context menu. Additional Related Information: • Imported Load • Imported Thickness • Mapping Validation in the ANSYS Mechanical Application User's Guide Right-mouse Options: • Analyze: Invokes calculation of Validation object. See Mapping Validation in the ANSYS Mechanical Application User's Guide. • Export: Exports the data to a text file in tabbed delimited format. See Exporting Data in the ANSYS Mechanical Application User's Guide. Object Properties The Details view properties for this object include the following. Category Fields Definition File Identifier - File identifier(s) from parent object. Settings Type - Specify Reverse Validation, Distance Based Average Comparison, or Source Value. Number of Points - available when Distance Based Average Comparison is selected. Specifies how many points to use in the distance based average mapping calculations. Output Type - Specify either Relative Difference or Absolute Difference. (This is not displayed for the Source Value type.) Graphics Controls Display – Specify either Scaled Spheres, Colored Spheres, or Colored Points 1062 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Scale – Specify scale multiplier for increasing and decreasing sphere sizes. Not displayed for Colored Points. Velocity Category Fields Display Minimum – appears if object state is solved. Graphics display will use this value to show only items above this threshold. Must be greater than the Minimum and less than the Maximum property. Display Maximum – appears if object state is solved. Graphics display will use this value to only show items below this threshold. Must be greater than Minimum and less than Maximum property. Display In Parent – graphics items can be overlaid on parent objects when this item is set to On. Statistics Minimum –- read-only minimum value for entire mapped points. Maximum – read-only maximum value for entire mapped points. Number Of Items – read-only number of currently displayed items Velocity Applies velocity as an initial condition for use in a transient structural analysis or an explicit dynamics analysis. Tree Dependencies: • Valid Parent Tree Object: Initial Conditions • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Initial Conditions object: • Click Velocity button on Initial Conditions context toolbar. • Click right mouse button on Initial Conditions object or in the Geometry window > Insert> Velocity. Additional Related Information: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1063 Objects Reference • Define Initial Conditions • Transient Structural Analysis (p. 91) • Explicit Dynamics Analysis Object Properties The Details view properties for this object include the following. Category Fields Scope Scoping Method Geometry – appears if Scoping Method is set to Geometry Selection. In this case, use selection filters to pick geometry, click the Geometry field, then click Apply. Named Selection – appears if Scoping Method is set to Named Selection. Definition Input Type - choose either Angular Velocity or Velocity. Define By Total– magnitude; appears if Define By is set to Vector. Direction- appears if Define By is set to Vector. Coordinate System – available list; appears if Define By is set to Components. X, Y, Z Component – values; appears if Define By is set to Components. Virtual Body Defines an individual virtual body. Virtual bodies are supported for assembly meshing only. Tree Dependencies: 1064 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Virtual Body Group • Valid Parent Tree Object: Virtual Body Group • Valid Child Tree Objects: Fluid Surface, Comment, Figure, Image Insertion Options: Use either of the following methods after highlighting the Geometry object: • Click right mouse button on the Geometry object and select > Insert> Virtual Body. • Choose Virtual Body on the Geometry context toolbar. Additional Related Information: • Assembly Meshing • Defining Virtual Bodies Object Properties The Details view properties for this object include the following. Category Fields Graphics Properties Visible - Toggles visibility of the selected virtual body in the Geometry window. Definition Suppressed - Toggles suppression of the selected virtual body. Used By Fluid Surface - Defines whether the virtual body is being used by a set of fluid surfaces. If you change the setting from Yes to No, the Fluid Surface object will be hidden. Material Point - Specifies the coordinate system to be used for the selected virtual body. The default is Please Define. The Fluid Surface object and the Virtual Body object will remain underdefined until a material point is specified. You can select the default coordinate system or define a local coordinate system. In either case, the setting will be retained, even if the Used By Fluid Surface setting is changed later. Material Fluid/Solid - Read-only and always set to Fluid for virtual bodies. Statistics Nodes - Read-only indication of the number of nodes associated with the virtual body when meshed. Elements - Read-only indication of the number of elements associated with the virtual body when meshed. Mesh Metric - Read-only metric data associated with the virtual body when meshed. Virtual Body Group Represents all definitions of virtual bodies within a model. Each definition is represented in a Virtual Body object. Virtual bodies are supported for assembly meshing only. Tree Dependencies: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1065 Objects Reference • Valid Parent Tree Object: Geometry • Valid Child Tree Objects: Virtual Body, Comment, Figure, Image Insertion Options: When you insert the first Virtual Body object into the tree, the Virtual Body Group object is inserted automatically. Additional Related Information: • Assembly Meshing • Defining Virtual Bodies Object Properties The Details view properties for this object include the following. Category Fields Graphics Properties Visible - Toggles visibility of the virtual body group in the Geometry window Definition Suppressed - Toggles suppression of the virtual body group object Statistics Nodes - Read-only indication Elements - Read-only indication Mesh Metric - Read-only indication Virtual Cell Defines an individual face or edge group, defined manually or automatically. Virtual Cell objects do not appear in the tree. Creation Options: • For automatic creation of virtual cell regions, a Virtual Cell object is created for each region that meets the criterion specified in the Details view of the Virtual Topology object. • For manual creation of Virtual Cell objects, highlight the Virtual Topology object, select one or more faces or one or more edges in the Geometry window, and then do one of the following: – Choose Merge Cells on the Virtual Topology context toolbar. – Click right mouse button on the Virtual Topology object and select Insert> Virtual Cell from the context menu. – Click right mouse button in the Geometry window and select Insert> Virtual Cell from the context menu. Additional Related Information: 1066 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Virtual Hard Vertex • Virtual Topology Overview • Virtual Topology Context Toolbar • "Meshing: Virtual Topology" (in the Meshing help) Object Properties The properties for this object include the following. For related information, refer to Using the Virtual Topology Properties Dialog to Edit Properties. Category Fields General Cell Class - Read-only indication of cell class for selected Virtual Cell object. Geometry - Read-only indication of components that make up the Virtual Cell object. Suppressed - Read-only indication of suppression status of selected Virtual Cell object. Project to Underlying Geometry - Defines whether the mesh should project to the original underlying geometry (Yes) or faceted geometry (No). Virtual Hard Vertex Defines a virtual hard vertex, which allows you to define a hard point according to your cursor location on a face, and then use that hard point in a split face operation.Virtual Hard Vertex objects do not appear in the tree. Creation Options: Highlight the Virtual Topology object. Select the face to split in the Geometry window. Position your cursor on the face where you want the hard point to be located, left-click, and do one the following: • Right-click in the Geometry window and select Insert> Virtual Hard Vertex at + from the context menu. • Choose Hard Vertex at + on the Virtual Topology context toolbar. Additional Related Information: • Virtual Topology Overview • Virtual Topology Context Toolbar • "Meshing: Virtual Topology" (in the Meshing help) Object Properties The properties for this object include the following. For related information, refer to Using the Virtual Topology Properties Dialog to Edit Properties. Category Fields General Geometry - Read-only indication showing that one vertex makes up the Virtual Hard Vertex object. Suppressed - Read-only indication of suppression status of selected Virtual Hard Vertex object. Virtual Hard Vertex Location - Read-only indication of the XYZ location of the Virtual Hard Vertex object. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1067 Objects Reference Virtual Split Edge Defines a virtual split edge. Virtual Split Edge objects do not appear in the tree. Creation Options: Highlight the Virtual Topology object, select the edge to split in the Geometry window, and then do the following: • To define the split location according to your cursor location on the edge, right-click in the Geometry window and select Insert> Virtual Split Edge at + from the context menu, or choose Split Edge at + on the Virtual Topology context toolbar. • To define the split without specifying the location, right-click in the Geometry window and select Insert> Virtual Split Edge from the context menu, or choose Split Edge on the Virtual Topology context toolbar. By default the split ratio will be set to 0.5, but it can be changed later using the Virtual Topology Properties dialog. Additional Related Information: • Virtual Topology Overview • Virtual Topology Context Toolbar • "Meshing: Virtual Topology" (in the Meshing help) Object Properties The properties for this object include the following. For related information, refer to Using the Virtual Topology Properties Dialog to Edit Properties. Category Fields General Geometry - Read-only indication of components that make up the Virtual Split Edge object. Suppressed - Read-only indication of suppression status of selected Virtual Split Edge object. Split Ratio - Defines the location of the split for the selected Virtual Split Edge object. Represented as a fraction of the total length of the edge. The default is 0.5. Virtual Split Face Defines a virtual split face. Virtual Split Face objects do not appear in the tree. Creation Options: Highlight the Virtual Topology object, select two vertices on the face that you want to split in the Geometry window, and then do one of the following: • Choose Split Face at Vertices on the Virtual Topology context toolbar. • Click right mouse button on the Virtual Topology object and select Insert> Virtual Split Face at Vertices from the context menu. • Click right mouse button in the Geometry window and select Insert> Virtual Split Face at Vertices from the context menu. Note Virtual Hard Vertex objects can be defined for use in split face operations. 1068 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Virtual Topology Additional Related Information: • Virtual Topology Overview • Virtual Topology Context Toolbar • "Meshing: Virtual Topology" (in the Meshing help) Object Properties The properties for this object include the following. For related information, refer to Using the Virtual Topology Properties Dialog to Edit Properties. Category Fields General Geometry - Read-only indication of components that make up the Virtual Split Face object. Suppressed - Read-only indication of suppression status of selected Virtual Split Face object. Vertices - Read-only indication showing that two vertices were selected. Virtual Topology Represents all definitions of face or edge groups, and all definitions of virtual split edges, virtual split faces, and virtual hard vertices within a model. Each definition is represented in a Virtual Cell, Virtual Split Edge, Virtual Split Face, or Virtual Hard Vertex object, respectively. Virtual Cell, Virtual Split Edge, Virtual Split Face, and Virtual Hard Vertex objects do not appear in the tree. Tree Dependencies: • Valid Parent Tree Object: Model • Valid Child Tree Objects: Comment, Figure, Image Insertion Options: Use any of the following methods after highlighting Model object: • Choose Virtual Topology on Model context toolbar. • Click right mouse button on Model object or in the Geometry window> Insert> Virtual Topology. Note Only one Virtual Topology object is valid per Model. Additional Related Information: • Virtual Topology Overview • Virtual Topology Context Toolbar • "Meshing: Virtual Topology" (in the Meshing help) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1069 Objects Reference The following right mouse button context menu options are available for this object. • Generate Virtual Cells • Generate Virtual Cells on Selected Entities Object Properties The Details view properties for this object include the following. The Lock position of dependent edge splits setting applies to virtual split edge behavior. Category Fields Definition Behavior Advanced Generate on Update Merge Face Edges Lock position of dependent edge splits Statistics Virtual Faces - Read-only indication Virtual Edges - Read-only indication Virtual Split Edges - Read-only indication Virtual Split Faces - Read-only indication Virtual Hard Vertices - Read-only indication Total Virtual Entities - Read-only indication 1070 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. CAD System Information For detailed CAD-related information specific to the ANSYS DesignModeler application and ANSYS Workbench, see the CAD Integration section of the product help. When accessing the ANSYS Workbench Help from the Help menu, click the Contents tab and open the CAD Integration folder in the hierarchical tree. The CAD Integration section includes topics about: • Overview • Geometry Interface Support for Linux and Windows • Project Schematic Presence • Mixed import Resolution • CAD Configuration Manager • Named Selection Manager • Caveats and Known Issues • Installation and Licensing • File Format Support (with information specific to the Mechanical application) ACIS AutoCAD BladeGen CATIA Creo Elements/Direct Modeling Creo Parametric (formerly Pro/ENGINEER) ANSYS DesignModeler GAMBIT IGES Inventor JT Open Monte Carlo N-Particle NX Parasolid Solid Edge SolidWorks SpaceClaim STEP • ANSYS Teamcenter Connection • SpaceClaim Related to CAD Integration • Frequently Asked Questions • Troubleshooting • Glossary Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1071 CAD System Information • Updates Mechanical application topics: General Information (p. 1072) General Information Body Filtering Property There are four body filtering properties: Process Solid Bodies, Process Surface Bodies, Process Line Bodies and Mixed Import Resolution. Their value is set in the Project Schematic and they determine what bodies will get imported to the Mechanical application. The default setting is: Yes for Solid and Surface Bodies, No for Line Bodies and, None for Mixed Import Resolution. Material Properties The CAD system interfaces will process only the isotropic material type. Multiple Versions of CAD Systems For most CAD systems, you cannot use geometry that was created in a newer version of the same CAD system. For example, if you have both SolidWorks 2011 and SolidWorks 2010 installed, but only the 2010 version is registered, and you attempt to insert geometry created in SolidWorks 2011 from the Project Schematic, the registered 2010 version will not recognize the geometry created in the 2011 version. This situation applies to all supported CAD systems except Creo Parametric, NX, and Solid Edge. For NX, you can set environment variables to specify the version. Solid Edge does not support the installation of multiple versions. 1072 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Troubleshooting Problem Situations (p. 1073) Recommendations (p. 1089) Problem Situations A Linearized Stress Result Cannot Be Solved. A Load Transfer Error Has Occurred. Although the Exported File Was Saved to Disk Although the Solution Failed to Solve Completely at all Time Points. An Error Occurred Inside the SOLVER Module: Invalid Material Properties An Error Occurred While Solving Due To Insufficient Disk Space An Error Occurred While Starting the ANSYS Solver Module An Internal Solution Magnitude Limit Was Exceeded. An Iterative Solver Was Used for this Analysis At Least One Body Has Been Found to Have Only 1 Element Animation Does not Export Correctly Assemblies Missing Parts CATIA V5 and IGES Surface Bodies Constraint Equations Were Not Properly Matched Error Inertia tensor is too large Failed to Load Microsoft Office Application Illogical Reaction Results Large Deformation Effects are Active MPC Equations Were Not Built for One or More Contact Regions One or More Contact Regions May Not Be In Initial Contact One or more MPC contact regions or remote boundary conditions may have conflicts One or More Parts May Be Underconstrained One or More Remote Boundary Conditions is Scoped to a Large Number of Elements Problems Unique to Background (Asynchronous) Solutions Problems Using Solution Running Norton AntiVirusTM Causes the Mechanical Application to Crash The Correctly Licensed Product Will Not Run The Deformation is Large Compared to the Model Bounding Box The Initial Time Increment May Be Too Large for This Problem The Joint Probe cannot Evaluate Results The License Manager Server Is Down Linux Platform - Localized Operating System The Low/High Boundaries of Cyclic Symmetry The Solution Combination Folder The Solver Engine was Unable to Converge The Solver Has Found Conflicting DOF Constraints Unable to Find Requested Modes You Must Specify Joint Conditions to all Three Rotational DOFs Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1073 Troubleshooting A Linearized Stress Result Cannot Be Solved. ... The path is not entirely contained within the finite element mesh. To solve a Linearized Stress result, a necessary condition is that the associated path be totally contained within the model. If the start/endpoints of the path are not within the model (likely to occur when the mesh is coarse and when using the XYZ Coordinate toolbar button for picking), you can use the Snap to mesh nodes feature to adjust the endpoints to be coincident with the nearest nodes in the mesh. Occasionally however, other internal “knots” of the path are not inside the model due to a hole or other missing material in the model. These situations can prevent the solving of a Linearized Stress result and cause this error message to appear, even after using the Snap to mesh nodes feature. To verify that a discontinuity is the cause of the error, apply a result other than a Linearized Stress result to that path, and solve it. By doing so you will take advantage of the fact that other results do not require that the full path be inside the model. The results are displayed and discontinuities are indicated by any gaps or missing fields shown in the Graph and Tabular Data windows. The following example illustrates a Total Deformation result where gaps in the Graph window and empty fields in the Tabular Data window provide evidence of discontinuities. A Load Transfer Error Has Occurred. ... A load could not be applied to small or defeatured entity. Please see the Troubleshooting section of the Help System for more information. At least one load is not able to be applied. This may be due to mesh-based defeaturing of the geometry. You can modify the mesh defeaturing settings to restore the nodes and elements where the loads need to be applied. 1074 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Problem Situations Although the Exported File Was Saved to Disk ... the Microsoft Office application failed to load. See the Troubleshooting section for details. This message is displayed when you have chosen to export a file to Microsoft Excel, but the Microsoft application is either not supported or not installed correctly. The Microsoft Excel file is still exported and can be opened provided the application is resident. To prevent this error message from appearing again, you can either install Microsoft Excel or set Automatically Open Excel to No in the Export preferences, accessible from the Main Menu under Tools> Options. Although the Solution Failed to Solve Completely at all Time Points. ... partial results at some points have been able to be solved. Refer to Troubleshooting in the Help System for more details. This message displays if for some reason (such as non convergence or the user choosing the Stop button) the simulation does not run to completion, but the solution does produce at least some results that can be post processed. If such a condition occurs, any applicable results in the tree that you request will be calculated (that is, they are defined at a sequence number or time that has been solved). These results will be assigned a green check state (up to date) but the solution itself will still be in an obsolete state because it is not fully complete. Use the Evaluate Results right mouse button option on a Solution object or a result object in order to additionally postprocess the partial solution. See Unconverged Results (p. 728) for further details. An Error Occurred Inside the SOLVER Module: Invalid Material Properties ... Please see the Troubleshooting section of the Help system for possible causes. Check the following: Material Definition Check the Details view for each part to see that you selected the correct material for each part. Go to Engineering Data to edit and check your material files and data and to verify the material definitions (including numbers and units). Note that, depending on the type of result, you will have a minimum of properties to be set. Structural, Vibration, Harmonic, and Shape Results: • Need to define the Modulus of Elasticity • If you don't define the Poisson's Ratio it will default to 0.0. Also note that the Solver engine will not accept values of Poisson's Ratio smaller than 0.1 or larger than 0.4 for Shape Results. • For Vibration and Harmonic results, include the Mass Density of your material. • For Thermal-stress results, you will need the Coefficient of Thermal expansion. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1075 Troubleshooting Thermal Results: Thermal conductivity is required. Can be constant or temperature-dependent. Specific Heat is required in a thermal transient analysis. Can be constant or temperature-dependent. Check Thermal Data For thermal analysis, go to the Engineering Data to edit and check thermal conductivity in the material files and to check thermal convection in the convection files. Verify the 'smoothness' of the temperaturedependent conductivity data and convection data. Non-smooth curves will lead to Solve failures. Electromagnetic Materials - Minimum Requirements For a Conductor scoped to a body, the associated material must have either Resistivity or Orthotropic Resistivity specified in order for the simulation to continue on to a solve. For all materials in an electromagnetic simulation, one of the following four conditions must be met. These conditions are mutually exclusive of each other so only one condition can exist at a time for a material. • Linear “Soft” Magnetic Material properties specified: Either Relative Permeability or Linear Orthotropic Permeability are set. • Linear “Hard” Magnetic Material properties specified. Only Linear “Hard” Magnetic Material property is set. • Nonlinear “Soft” Magnetic Material properties specified: Either only BH Curve or BH Curve and Nonlinear Orthotropic Permeability are set. • Nonlinear “Hard” Magnetic Material properties specified: Only Demagnetization BH Curve is set. An Error Occurred While Solving Due To Insufficient Disk Space ... Please see the Troubleshooting section of the Help system for more information. Possible reasons that this message appears: • You may be running out of disk space during the Mechanical APDL solution due to the writing of large solution files. Verify that there is sufficient free disk space on the drive where the solver directory exists. • You do not have write permissions to the solution directory. • Files from a previous Workbench or Mechanical APDL session already reside in the solution directory. An Error Occurred While Starting the ANSYS Solver Module To get further information on what the issue may be, insert a Solution Information object under Solution in the tree, and view the contents. Possible reasons that the ANSYS solver may fail are: • Insufficient memory - You may not have enough virtual memory assigned to your system. To increase the allocation of virtual memory (total paging file size), go to Settings> Control Panel> System (on your Windows Start Menu). Click the Advanced tab and then click Performance Options. Increase the size of your virtual memory. 1076 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Problem Situations • Insufficient disk space - You may not have enough disk space to support the increase in virtual memory and the temporary files that are created in the analysis. Be sure you have enough disk space or move to an area where you have enough. • Corrupt product installation • License request rejected • The startup directory for cmd.exe has been overridden by the AUTORUN option and as a result causes the solver to be unable to locate the solver input files. Solving and UNC Paths If a Workbench database resides on a UNC path (for example, \\pghxpuser\Shares) for which you have write permissions, the ANSYS input file will be written successfully but will fail to start the solver executable. If you did not have write permissions, Workbench will instead write the ANSYS input file to your temp directory (%tmp%) and will solve there. An Internal Solution Magnitude Limit Was Exceeded. … Please check your Environment for inappropriate load values or insufficient supports. Please see the Troubleshooting section of the Help System for more information. In most cases this message will occur if your model is improperly constrained or extremely large load magnitudes are applied relative to the model size. First check that the applied boundary conditions are correct. In some cases, loads that are self-equilibrating with no support may be desired. To help in these cases, if this message occurs, consider adjusting the weak spring stiffness or turning on inertia relief. An Iterative Solver Was Used for this Analysis ...However, a direct solver may enhance performance. Consider specifying the use of a direct solver. An iterative solver was used to obtain the solution; however, a large number of iterations were needed in order to get a converged answer. By default, the program will either choose a direct or iterative solver based on analysis type and geometric properties. (In general, thin models perform better with a direct solver while bulky models perform better with an iterative solver.) However, sometimes the iterative solver is chosen when the direct solver would have performed better. In such cases, you may want to force the use of the direct solver. You may specify the solver type in the Details view of the Analysis Settings folder. At Least One Body Has Been Found to Have Only 1 Element ...in at least 2 directions along with reduced integration. This situation can lead to invalid results. Consider changing to full integration element control or meshing with more elements. Refer to Troubleshooting in the Help System for more details. This scenario is based on the following conditions: • Structural solid model. • Brick meshes that have only 1 element in less then 2 directions. • Reduced element integration is assigned (This can happen by default if Element Control in the Geometry object is set to Program Controlled.). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1077 Troubleshooting If the above conditions are met, there is a strong likelihood that your analysis will excite hourglass modes. In such cases solver pivot warnings will be reported and nonphysical deformations will result (see examples below). If this occurs, first determine which bodies have one element through the thickness (Right-click in Geometry window, choose Go To> Bodies With One Element Through the Thickness, and observe selected body objects in the tree). The offending bodies can then be corrected by doing one of the following: • Modify the mesh to have more than 1 element in at least 2 directions. This will remove the hourglass modes in most cases. In rare cases you may need to modify the mesh such that more than 1 element exists in all 3 directions. • Use Full integration on the offending bodies. • Consider using lower order elements. Example of a "bad" mesh for reduced integration: Example of a "good" mesh for reduced integration: Animation Does not Export Correctly When exporting an AVI file, make sure that you keep the Workbench module window in front of other windows until the exporting is complete. Opening other windows in front of the module window before the exporting is complete may cause those windows to be included in the AVI file capture. Assemblies Missing Parts When reading assemblies from CATIA V5, all part files that are referenced by assemblies must be accessible in order for the importing to occur. 1078 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Problem Situations CATIA V5 and IGES Surface Bodies CATIA V5 and IGES surface bodies consisting of closed faces are transferred as solid bodies. Constraint Equations Were Not Properly Matched ... for all node pairs across the low and high sector boundaries in the cyclic symmetry. Please see the Troubleshooting section of the Help System for more information This message may occur if the solver does not succeed to reproduce the exact pairing of nodes between the low and high sector. An approximate technique was used to group like nodes and distribute the loads, but this can reduce solution accuracy. Error Inertia tensor is too large This message is shown by the LS-DYNA solver if your model includes rigid bodies with large dimensions, for example a few meters in length. Such rigid geometries cause the inertia tensor limit of the solver to be exceeded. You can attempt to resolve this issue by running the double precision LS-DYNA solver, which has a much larger inertia tensor limit. The double precision solver executable can be accessed with the -dp command line option as follows LSDYNA120.exe -dp. Failed to Load Microsoft Office Application ... See the Troubleshooting section for details. This message is displayed when you have chosen a feature that is dependent on a Microsoft Office application, such as exporting a file to Microsoft Excel, and the related Microsoft Office application is not installed correctly. Illogical Reaction Results Cause Loads, supports, or contact items are applied to the same or shared topology. Reason It is unclear or ambiguous as to which reaction should be attributed to which support, load, or contact item. Refer to this Note for details. Large Deformation Effects are Active ... Which may have invalidated some of your applied supports such as displacement, cylindrical, frictionless, or compression only supports. Refer to Troubleshooting in the Help System for more details. In a large deformation analysis, the program updates the nodal coordinates as the solution progresses towards the final configuration. As a result, supports that fix only some of the degrees of freedom of a node but not all (for example fix only UX=0), may become invalid as the model's nodal coordinates and Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1079 Troubleshooting thus nodal rotation angles are updated. The imposed DOF displacement directions do not change even though rotation angles change. This may or may not be a desirable situation. A classic example is a simple torsion of a rod. Initially the nodes at zero degrees have a circumferential direction of UY but after a twist of 90 degrees, have a circumferential direction of UX. The user is responsible for determining if any nodal rotation at the support is significant enough to cause undesired results. The following is a list of supports which only fix the movement of a node partially and thus are susceptible to large deformation effects: • Displacement • Cylindrical support • Frictionless In addition a Compression Only Support may be susceptible to large deformation effects because if large sliding occurs, the face can literally "slide off" the compression only support. MPC Equations Were Not Built for One or More Contact Regions ... Due to potential conflicts with the cyclic symmetry constraints. This may reduce solution accuracy. Please refer to the Troubleshooting section. Cyclic symmetry is enforced with the help of constraint equations between pairs of nodes on the low and high sector boundaries respectively. When such nodes also participate in MPC contact, which requires constraint equations of its own, conflicts may arise. Please review results carefully, since the MPC contact will be compromised at these locations. One or More Contact Regions May Not Be In Initial Contact … Check results carefully. Refer to Troubleshooting in the Help System for more details. During the solution it was found that one or more of the contact pairs was not initially in contact. You may check the solution output located in the Worksheet of a Solution Information object to determine exactly which contact pairs are initially open, and take the appropriate action. • This message is expected if a contact pair is meant to be initially open and may become closed after the load application. • If initial contact was desired and the contact pair has a significant geometric gap, setting the Pinball Radius manually to a sufficiently large value may be required. • If symmetric contact is active, it is possible that one pair may be initially open and its symmetric pair be initially in contact. Check the solution output to confirm this. 1080 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Problem Situations One or more MPC contact regions or remote boundary conditions may have conflicts ...With other applied boundary conditions or other contact regions. Tip: You can graphically display FE Connections from the Solution Information Object. Refer to Troubleshooting in the Help System for more details. During solution it was found that one or more contact pairs using MPC (multi point constraint) contact formulation overlaps with another contact region or boundary condition. The same is true for remote boundary conditions overlapping with another contact region or boundary condition. Due to the fact that MPC formulation can cause over constraint if applied to the same nodes more than once, the program may have not been able to completely bond the desired entities together. You may check the solution output located in the Worksheet of a Solution Information object to determine which pairs and nodes are affected by this condition. Specifically this can happen when: • A contact pair entity (either an edge or face) also has a Dirichlet (prescribed displacement/temperature) boundary condition applied to it. In this case the MPC constraints will not be created at nodes that have prescribed conditions thus possibly causing parts to lose contact. Sometimes this warning may be disregarded in cases such as a large face with a fixed support at one edge and a contact pair on another. If it is determined that overlap does indeed exist, consider relocating the applied support or using a formulation other than MPC. • Two MPC contact pairs share topology (such as a face or an edge). Again it is possible for one or both of these pairs to lose contact. This message may especially occur when edge/face contact is automatically generated by the program because often 2 complementary contact pairs (that is, edge part 1/face part 2 and edge part 2/face part 1) are created. Often in this case the message can be ignored after verifying result correctness and if necessary, deleting/suppressing one of the inverse pairs. This condition may also occur when 1 part (typically a surface body), is being contacted by 2 or more parts in the same spatial region. In this case it is possible for one or more of the parts to lose contact. Consider reducing the Pinball Radius to avoid overlap or changing one or more of the regions in question to use a contact formulation other than MPC. • When MPC contact is used to connect rigid bodies and joints, the overconstraint situation can sometimes occur. One or More Parts May Be Underconstrained ...and experiencing rigid body motion. This message may occur for one of several reasons: If the program detects that the model may be underconstrained, weak springs will be added to the finite element model to help obtain a solution. In addition, the program will automatically add weak springs if unstable contact (frictionless, no separation, rough) or compression only supports are active in order to make the problem more numerically stable. Since the weak springs have a low stiffness relative to the model stiffness, they will not have an effect on a properly constrained model. If you are confident that weak springs are not needed for a solution and the program adds them anyway, you may disable them by setting the Weak Springs option to Off in the Details view of the Analysis Settings object. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1081 Troubleshooting One or More Remote Boundary Conditions is Scoped to a Large Number of Elements ...which can adversely affect solver performance. Consider using the Pinball setting to reduce the number of elements included in the solver. Remote boundary conditions scoped to a large number of elements can cause the solver to consume excessive amounts of memory. Point masses in an analysis where a mass matrix is required and analyses that contain remote displacements are the most sensitive to this phenomenon. If this situation occurs, consider modifying the Pinball setting to reduce the number of elements included in the solver. Forcing the use of an iterative solver may help as well. The reason for the excessive memory consumption is that the remote boundary conditions generate internal constraint equations to distribute the remote mass, displacement, or loads from one node of the model to all other selected nodes. As described in Chapter 15.14. Constraint Equations, in the Mechanical APDL Theory Reference, constraint equations could change a sparse matrix (for example, a stiffness matrix, mass matrix, or damping matrix) to a dense matrix. An increase in the number of constraint equations used increases the density of the final matrix, which in turn places a higher demand for more memory (or longer CPU time) in the solution of a problem. Normally, if the maximum number of remote nodes selected is about 3000, then the increased memory usage or CPU time is not significant. Caution should be taken to not use too many remote nodes in these applications. Other techniques are available to distribute loads or masses. For example, to distribute a point mass to the entire model, you might consider specifying density directly instead of using the point mass approach. Problems Unique to Background (Asynchronous) Solutions Consider the following hints when troubleshooting background (asynchronous) solution problems: • For security reasons, RSM will not allow any job to be run by the "root" user on Linux, including primary and alternate accounts. • It may sometimes be necessary for you to enter the full path to the solver executable file in the Solve Process Settings. • It may sometimes be necessary for you to enter the full path to the Linux working directory in the Linux Working Folder field of the Solve Process Settings. • The LSF administrator should configure the Workbench job server to disallow multiple, simultaneous jobs. Two solves running on the same server will interfere with each other, preventing successful completion of each. • To help in debugging solver startup problems on the remote machine, it is sometimes useful for you to use the Solution Information object under the Solution object in the tree. The Solution Information object will show the contents of the solve.out file that the remote solver produced, if the application was able to start. • When using the Stop Solution option to stop a solve running on a Linux machine, it is possible that the solver will continue to run on that machine even though the Mechanical application thinks it has stopped. If this happens and you don't want the solve job to continue on the Linux machine it will be necessary for you to kill the process manually. The ability to solve to two different Linux machines simultaneously is not allowed. • The solve command may have failed to execute on the remote Linux server. Verify the command's spelling and/or path. Solve commands are issued to the remote server using the rexec interface. Failures 1082 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Problem Situations may occur if the resulting path ($path) is insufficient. $path can be verified by issuing rexec on the command prompt on the local machine. For example: rexec machinename -l username echo $path > diagnosticsfile (where "l" is the letter "el)" The machinename and username match the entries in the Solve Process Settings, and diagnosticsfile corresponds to the recipient on the local machine for the command output. Note After issuing rexec, if you receive the following message, rexec isn't enabled on the remote Linux server. This feature must be enabled on the remote Linux server in order for the solution to proceed. > rexec:connect:Connection refused rexec: can't establish connection If the path to the solve command is unavailable on the remote server, it can be added to user or system-wide files that initialize the startup shell (for example, .cshrc or /etc/csh.login on C-shells). Consult the Linux server's rexec interface and appropriate shell manual pages for details. • If you cannot make ASCII transfers to a Linux server, changes need to be made on the server. Background solutions on a remote Linux server use file transfer protocol (ftp). Therefore, the system administrator must install ftp and enable it. Ftp uses ASCII transfer mode to convert PC text to Linux text. If ASCII mode is disabled, it is not obvious because error messages do not imply this. On some ftp servers (vsftpd, for example), by default, the server will pretend to allow ASCII mode, but in fact, will ignore the request. You will need to ensure that the ASCII upload and download options are enabled to have the server actually do ASCII mangling on files when in ASCII mode. To enable these options, the system administrator should consult the operating system documentation. The following vsftp.conf modification procedure is Linux platform specific and is provided as an example only. 1. In /etc/vsftpd/vsftpd.conf, uncomment the following lines (that is, remove the # at the beginning of these lines): ascii_upload_enable=YES ascii_download_enable=YES 2. Restart the server. Problems Using Solution If Solution fails to complete, try the following suggestions. Verify the Environment Verify that the loads and supports in the Environment meet the requirements for Stress, Thermal, Thermal-Stress, Shape or Vibration. You can verify the environment quickly by looking at the icons adjacent to each environment item in the Tree Outline. A green check indicates that the requirements are met. A indicates that the requirements were not met. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1083 Troubleshooting Check System Requirements Verify that your system meets the minimum requirements at the time you start Solution. Disk space and memory may fluctuate depending on how the system is used. See also General Solver Error. For Thin-Walled or Finely Detailed Parts If your parts contain features whose size or thickness is extremely small in comparison to the principal dimensions of the assembly, try adjusting the variables used in modeling geometry. • Set the variable DSMESH DEFEATUREPERCENT to 1e-5. To set variables, click Tools> Variable Manager. • If that fails, change the setting to 1e-6. Invalid or Poorly Defined Models At the end of the Solution procedure, the region of a part that caused the problem is usually labeled. . If the geometry that is notated looks valid, but is small compared to the rest of the model, adjusting the Sizing Control may correct the problem. Running Norton AntiVirusTM Causes the Mechanical Application to Crash If the Norton AntiVirusTM product is running and you choose Allow the entire script once to resolve a script error, the Mechanical application crashes. Choose Authorize this script to allow the Mechanical application to function normally. The Correctly Licensed Product Will Not Run If you have installed a license file for a valid Mechanical product, but the product continues to run in read-only mode or, in the case of an upgrade to a higher product, continues to run the lower product, make sure you have specified the correct product in the launcher. This situation can occur if you install the Mechanical application before creating your license file. In this case, the Mechanical application will run only in read-only mode. When you create your license file later, you must choose a license under Mechanical APDL Product Launcher in the Start menu. Once there, select the product that you have licensed to reset the default to the correct product. Otherwise, the Mechanical application will continue to run in read-only mode. This situation can also occur if you upgrade your license to a higher Mechanical product. Again, you must choose a license under Mechanical APDL Product Launcher in the Start menu. Then reset to the appropriate product. Otherwise, the Mechanical application will continue to run as the lower, previously-licensed product. 1084 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Problem Situations The Deformation is Large Compared to the Model Bounding Box ... Verify boundary conditions or consider turning large deflection on. This message will be displayed any time the software detects nodal deformations exceeding 10% of the model diagonal. Exceeding 10% of this length suggests model mechanics that depart from linearity in response to the applied boundary conditions. Load magnitudes, surface body thicknesses, and contact optionsoe, if applicable, should be verified. If these are intended, a nonlinear analysis is advised. To request a nonlinear analysis, set Large Deflection to On in the Details view of the Analysis Settings folder. The Initial Time Increment May Be Too Large for This Problem ... Check results carefully. Refer to Troubleshooting in the Help System for more details. This message will appear if the program determines that the initial time increment used in the thermal transient analysis may be too large based on the "Fourier modulus" (Fo). This dimensionless quantity can be used as a guideline to define a conservative time step based on thermal material properties and element sizes. It is defined as: Fo = k (∆t) / ρ c (lengthe2) where: lengthe = Average element length ∆t = Time step k = Thermal Conductivity c = Specific Heat ρ = Density Specifically this warning will be issued if the program finds that the Fourier modulus is greater than 100, that is, Fo > 100. Stated in terms of the initial time step (ITS), this warning appears when the ITS is 100 times greater than the time step suggested by the Fourier modulus in the form expressed below: ∆t = lengthe2 / (k / (c ρ)) This check is done on a per body basis and the results are echoed in the Mechanical APDL output listing. For example: ********* Initial Time Increment Check And Specified Initial Time Increment: .75 Estimated Increment Needed, le*le/alpha, Estimated Increment Needed, le*le/alpha, Estimated Increment Needed, le*le/alpha, Estimated Increment Needed, le*le/alpha, Fourier Modulus ********* Body Body Body Body 1: 2: 3: 4: 0.255118 1.30416 0.158196 0.364406 If this warning is issued make sure that the specified time step sizes are sufficiently fine to accurately capture the transient phenomenon. The proper use of this guideline depends on the type of problem being solved and on accuracy expectations. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1085 Troubleshooting The Joint Probe cannot Evaluate Results ...A possible cause is that the joint is a fixed body-body joint on a rigid body. This message displays because fixed body-body joints on rigid bodies do not report a reaction. See the Probes section of the help for more information. The License Manager Server Is Down Unless a connection is reestablished, the Mechanical application will exit in nn minutes. Cause This message occurs in a one-server license environment if your license manager has quit running. In a three-license server environment, the ANSYS license manager must be running on at least two of the three license server machines at all times. If two of the license server machines go down, or two of the machines are not running the license manager, this error message will appear in the program output or in a message box. The program will continue to run for nn minutes to allow the license manager to be restarted or to be started on a second machine if using redundant servers. When the message first displays, nn = 60. The message then reappears every five minutes with nn displaying the elapsed time at each 5 minute increment (55, 50, 45, etc.) until the connection is established. Resolution When this error message appears, start the license manager on the other machines designated as license servers. If you get this message and determine that the license manager is still running, and you are running in a one-server environment, then the IP address of the license server machine was changed while the application was running (this is usually caused by connecting to or disconnecting from an Internet Service Provider (ISP) that dynamically allocates IP addresses). To correct this situation, you must return the IP address to the same address that the license server had when the application was started. If the IP address changes after you start the application (either because you connected to or disconnected from your ISP), you can correct the error by restarting the application. You should not need to restart the license manager. You can avoid this problem by remaining connected to or disconnected from the ISP the entire time you are running the application. Linux Platform - Localized Operating System Specific to the Linux platform: if you are using a localized operating system (such as French or German), or set your preferences to use regional settings for numbers and dates (comma delimiter versus period), there is a discrepancy between applications: The ANSYS Workbench will honor the setting and display the numbers with comma delimiter. However, some of the components (e.g. Geometry, Meshing, Mechanical, etc.) can only recognize periods; numbers will be displayed and entered with periods. As a result, you may have to use commas when working in Workbench, and periods when working within those components. If this causes any inconvenience or confusion, define the "LANG" environment variable and set to "en-us" (e.g. "setenv LANG en-us" for csh shell) to force ALL applications (including Workbench) to use the period delimiter consistently throughout. Note that setting LANG to en-us may also cause some strings to be displayed in English, even if your language preference was set to a nonEnglish language. Within Mechanical, analysis settings for Explicit Dynamics and Rigid Dynamics, as well as Imported Load mapping settings are not localized. 1086 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Problem Situations If you are using a localized operating system (such as French or German), you must set the following VisualMainWin control on any machines running these applications in order for these applications to recognize the correct numerical format. ANSYS Workbench must already be installed before setting this control. 1. cd to: <wb_install directory>/v140/aisol 2. Issue the following command: ./.workbench -cmd mwcontrol 3. On the MainWin Control Panel, select Regional Settings. 4. Select the Regional Settings tab. 5. Change the language in the drop-down to match the language you want to use. The Low/High Boundaries of Cyclic Symmetry ... Have been found to include one or more nodes along the axis of symmetry.This may reduce solution accuracy. Please refer to the Troubleshooting section. Cyclic symmetry does not support the presence of nodes along the axis of symmetry. There, the node pair on the high and low sector boundary degenerates to a single node. Consider removing the axial nodes, fixing the nodes, or providing a much finer mesh in the vicinity. The Solution Combination Folder ...is underdefined due to invalid input environments. When the Solution Combination Folder is underdefined, verify that: • At least one environment is checked in the Solution Combination Worksheet. • The selected environments are static structural analyses. • The selected environments do not contain convergence. For more information, see Solution Combinations (p. 750). The Solver Engine was Unable to Converge Cause The solver engine was unable to converge on a solution of a nonlinear problem. Recommendations • When Advanced Contact is NOT Present in the Model ... 1. Check for sufficient supports to prevent rigid body motion (structural) or check for thermal material curves or convection curves which rise and/or fall sharply over the temperature range (thermal). 2. If you encounter a convergence error during a thermal analysis that is using contact, consider modifying the Thermal Conductance property. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1087 Troubleshooting • When Advanced Contact IS Present in the Model ... 1. Check for sufficient supports to prevent rigid body motion or that contact with other parts will prevent rigid motion. 2. Check that the loading is of a reasonable nature. Unlike linear problems whose results will scale linearly with the loading, advanced contact is nonlinear and convergence problems may arise if the loading is too big or small in a real world setting. 3. If the contact type is frictionless, try setting the type to rough. This may help some problems to converge if any possible sliding is not constrained. 4. Check that the mesh is sufficiently fine on faces that may be in contact. Too coarse a mesh may cause inaccurate answers and convergence difficulties. 5. Consider softening the normal contact stiffness KN to a value of .1. The default value is 1 and may be changed by setting the Normal Stiffness. Smaller KN multipliers will allow more contact penetration which may cause inaccuracies but may allow problems to converge that would not otherwise. 6. If symmetric contact is being used (by default the contact is symmetric), consider using asymmetric contact pairs. This may help problems that experience oscillating convergence patterns due to contact chattering. The program can be directed to automatically use asymmetric contact in the Details view of the Contact Folder. The Solver Has Found Conflicting DOF Constraints ...at one or more nodes. Please refer to the Troubleshooting section in the Help System. A variety of boundary conditions in Workbench direct the solver to apply a specific value of displacement or rotation to one or more nodes. Among these are fixed supports, simple supports, rotational supports, frictionless supports, cylindrical supports, symmetry planes and displacements. Workbench also allows to rotate nodes using the Nodal Orientations object in the tree. A typical example would be to apply non-zero displacements to two faces of a model that meet at an edge, especially when the displacements do not act in perpendicular directions. Nodes along the edge may find conflicting instructions as they are instructed to move different amounts along the same direction in space. If this is the case, consider modifying the non-zero displacements so they act in perpendicular directions. Although Workbench attempts to negotiate these constraints, along with the nodal rotations applied, there may be instances in which a node is directed to take on different and incompatible values of displacement or rotation by two or more of these boundary conditions. For such situations, Workbench will report a conflict. One example could be to apply non-zero displacements to two faces of a model that meet at an edge, especially when the displacements do not act in perpendicular directions. Nodes along the edge may find conflicting instructions as they are instructed to move different amounts along the same direction in space. If this is the case, consider modifying the non-zero displacements so they act in perpendicular directions. Another example could be when one or more Nodal Orientations are added in Workbench with other boundary conditions which are applied to same section of geometry (for example by selecting the same “Scope”, or one “Scope” being a part of the other). Each Nodal Orientation prescribes a Nodal Coordinate System to a subset of nodes. Only one Nodal Coordinate System can be prescribed to a given node. Whenever this condition is not met, Workbench creates an error that “The solver has found conflicting DOF constraints with Direct FE loading at one or more nodes”. 1088 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Recommendations Direct FE boundary conditions cannot be applied to nodes that are already scoped with geometrybased constraints which may modify Nodal Coordinate system. Unable to Find Requested Modes If this message occurs during a modal analysis, most likely a frequency search range was specified but no natural frequencies were found in the specified range. Either increase search range or specify that the first N frequencies be found. If this message occurs during an linear buckling analysis, verify that the loading is in the correct direction (that is, compressive) and that the structure is well constrained so that no rigid body motion can occur. If the applied boundary conditions appear to be correct, it is likely that a buckling failure will not occur. You Must Specify Joint Conditions to all Three Rotational DOFs ...for one or more joints in the model. Please refer to the Troubleshooting section in the ANSYS Workbench Manual Rotations are not independent in 3D. You must define all three rotations for a Joint Condition before proceeding to a solve. The problem is mathematically different on the velocities, as the 3 components are perfectly independent, thus you can define any of the components. Recommendations Microsoft ClearType edge smoothing option may cause font display problem If you use Microsoft ClearType edge smoothing method with Large size DPI setting, you may see distorted dimension text in DesignModeler and legend text in the Mechanical application. The problem occurs when the user minimizes or maximizes the Workbench window. In DesignModeler the display can be corrected on some machines by nudging the graphics window pane a pixel or two. This will cause a resize event in the graphics browser which will redraw the dimension text properly. Nudging the graphics window pane does not correct the problem in the Mechanical application, however. Alternatively, if the edge smoothing method is set to Standard instead of ClearType, then the text display appears correctly in both applets. Please note though, this is machine dependent, so the suggestions may not work on all machines. To ensure the text appears properly, it is recommended to turn off edge smoothing entirely. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1089 1090 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Appendices Appendix A. Glossary of General Terms API Application Program Interface: This is a defined interface of functions that can be called by the scripts. This interface will remain reasonably constant and no functions will be removed without deprecation and warning. Callout A message that appears as a result of an action initiated within the wizard. Callouts usually point to a toolbar button, a row in the Details View (p. 274), or object in the Tree Outline (p. 235). The message contains descriptive and instructive text. Context Menu Provides a short list of options applicable to a specific object or window. To view a context menu, click the right mouse button on an object or in a window. Context Toolbar A toolbar containing options appropriate for the current level in the Tree Outline (p. 235). Deprecate When a function in the API is removed it will be deprecated and undocumented. This means that it will still be available for the next release, but will be removed in the future. A warning will be provided with a suggested alternative method of achieving the same function. Details View Provides information on the highlighted object in the Tree Outline (p. 235). Displacement A vector quantity used to measure the movement of a point from one location to another. The basic unit for displacement is (Length). Double Data type that can be assigned to real (decimal) numbers, e.g. 2.3462 Drag Moving an on-screen object in the Tree Outline (p. 235) from one location to another using the mouse cursor while holding down the left button. The drag is interpreted as "move" if the object is dragged from the outline and "copy" if the object is dragged from the outline while holding down the Ctrl key Edge A selectable entity on a part that occurs at the intersection of two surfaces. In a surface model, an edge can also exist on the edge of one surface. Elastic Strain Normal elastic strain is a measure of the elongation or contraction of a hypothetical line segment inside a body per unit length. Normal elastic strain is dimensionless, however in practice it is common to assign normal elastic strain the basic unit of (Length / Length). Shear elastic strain is a measure of the change in angle that occurs between Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1093 Appendix A. Glossary of General Terms two initially perpendicular hypothetical line segment inside a body. The basic unit for shear elastic strain is radians. Face A selectable area on a part bordered on all sides by edges. Periodic, non-boundary edged faces (like spheres) may occasionally appear. Factor of Safety Factor of safety is defined as the ratio of the limit strength of a material to the maximum stress predicted for the design. This definition of factor of safety assumes that the applied load is linearly related to stress (an assumption implicit in all calculations performed in the application). A factor of safety of less than one generally predicts failure of the design; in practice a factor of safety of one or greater is required to help avoid the potential for failure. FEA Finite Element Analysis. A robust and mature technique for approximating the physical behavior of a complex system by representing the system as a large number of simple interrelated building blocks called elements. Fundamental Frequencies The fundamental frequencies are the frequencies at which a structure under free vibration will vibrate into its fundamental mode shapes. The fundamental frequencies are measured in Hertz (cycles per second). Heat Flux A measure of heat flow per unit area. The basic unit for heat flux is (Heat / Length*Length). Int Data type that can be assigned to integer (whole) numbers, e.g.2 Margin of Safety Margin of safety is always equal to the factor of safety minus one. Multiple Select Select more than one surface, edge or vertex by holding the Ctrl key. Object A set of information displayed visually as an icon (usually in the Tree Outline (p. 235)). Python This is a non-proprietary scriptable programming language that is commonly used throughout the world. Full details can be found at www.python.org. A number of debuggers are available to enable a script to be stepped through. Reference Temperature The reference temperature defines the temperature at which strain in the design does not result from thermal expansion or contraction. For many situations, reference temperature is adequately defined as room temperature. The reference temperature is defined for each body in a model. A coefficient of thermal expansion curve will be adjusted for the body's reference temperature if the reference temperature of the coefficient of thermal expansion is different. Right-Hand Rule The right-hand rule is a convenient method for determining the sense of a rotation defined by a vector: close your right hand and extend your thumb in the direction of the vector defining the rota- 1094 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. tion. Your fingers will indicate the sense or direction of the rotation. The direction in which your fingers curl is the positive direction. Rigid Body Motion Might occur when the part is free to translate or rotate in one or more directions. For example, a body floating in space is free to move in the X-, Y-, and Z-directions and to rotate about the X-, Y-, and Z-directions. Stress A measure of the internal forces inside a body. The basic unit for stress is (Force / Length*Length). String Data type that can be assigned to one or more characters of text, e.g. Hello World Temperature A scalar quantity used to measure the relative hotness or coldness of a point from one location to another. The basic units for temperature are degrees Fahrenheit or Celsius. Vertex A selectable entity on a part that occurs at the intersection of two or more edges. World Coordinate System The fixed global Cartesian (X, Y, Z) coordinate system defined for a part by the CAD system. XML eXtensible Markup Language: This is a standard layout of text based files in a metalanguage that allows users to define their own customized markup languages. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1095 1096 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Appendix B. Data Transfer Mesh Mapping To transfer data across a dissimilar mesh interface, the nodes of one mesh must be mapped to the local coordinates of a node/element in the other mesh. This section describes the settings that are available in Mechanical when data is mapped across two different meshes. You can add the exported mesh and loads as external data in the project schematic and couple a new Mechanical analysis system with this external data. The Mapping Settings described below are available within Mechanical when the source data comes from an External Data system, an upstream thermal analysis (Thermal-Stress coupling with dissimilar mesh), or when temperatures are transferred from Mechanical to Ansoft. Mapping Settings • Mapping Control: By default, when Program Controlled is selected, the software will determine the appropriate algorithm and settings based on the source and target mesh data, as well as the data type being transferred. See Program Controlled Mapping for additional information. You may choose to modify the advanced features by setting this to Manual. • Mapping: A read-only field displaying that a "Profile Preserving" algorithm is being used. The following is a list of data that are available for transfer: • – Pressure – Heat Flux – Heat Generation – Temperature – Heat Transfer Coefficient – Thickness Weighting: Choose which type of weighting should be performed. This option can be changed only if Mapping Control is set to Manual. – Triangulation creates temporary elements from the n closest source nodes to find the closest points that will contribute portions of their data values. For 3D, 4-node tetrahedrons are created, and for 2D, 3-node triangles are created by iterating over all possible combinations of the source points (maximum number controlled by the Limit property), starting with the closest points. If the target point is found within the element, weights are calculated based on the target’s location inside the element. – Distance Based Average uses the distance from the target node to the specified number of closest source node(s) to calculate a weighting value. – Shape Function loops over the source elements and tries to locate an element that each target node can be mapped to. Weights for each of the source nodes are then assigned based on the location of the target node and the shape function of the element. For each target node, the search efficiency can be improved by restricting the search to a subset of the source elements. The search algorithm works by: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1097 Appendix B. Data Transfer Mesh Mapping – 1. Distributing all source elements into Cartesian boxes or buckets. The number of buckets is controlled by the Scale property. 2. Locating each of the target nodes in a box. 3. Finding an element that each target node can be mapped to by restricting the search with each target's box. Kriging is a regression-based interpolation technique that assigns weights to surrounding source points according to their spatial covariance values. The algorithm combines the kriging model with a polynomial model to capture local and global deviations. The kriging model interpolates the source points based on their localized deviations, while the polynomial model globally approximates the source space. See Kriging Algorithms in the Design Exploration User Guide for more information. Note By default, the Kriging technique uses a higher-order Cross Quadratic polynomial to capture the global trend, which may fail to correctly interpolate data for a target point if multiple source points are spaced close to one another or if the target point is outside the region enclosed by the source points that are selected for interpolation. This may introduce gross errors in the estimation of the target value and manifests itself mostly when mapping data on surface or edge geometries. In such cases, we suggest that you change the Polynomial Type to Constant or Linear and, if necessary, reduce the number of source points to be included for the interpolation. • • Transfer Type: Enables you to choose the dimension of the transfer (for 3D transfers only). This option is available only for Triangulation. – The Surface option tries to map each target point by searching triangles that are created from the set of closest source points. The target point will be projected onto the plane relative to the triangle surface. If the point is found inside the triangle, the weights are calculated based on the target’s projected location inside the triangle. Use this option when mapping data across surfaces. – The Volumetric option tries to map each target point by searching tetrahedrons that are created from the set of closest source points. Use this option when mapping data across volumes. 2D Projection: Available only for 2D to 3D data transfers from an External Data system connected to Mechanical. The default option is Normal To Plane. You will be able to choose between the default as well as all application and user input coordinate systems. Graphics Controls These options are available only when importing data from an External Data System. • Display Source Points: Toggle display of source point data. This can be helpful in visualizing where the source point data is in reference to the target mesh. • Display Interior Points: Available when Display Source Points is set to On. Toggle allowing source point data to be displayed through the model so that interior points can be seen. • Display Projection Plane: Toggle display of project plane (available only for 2D to 3D mapping). Advanced Advanced settings are filtered based on the Mapping Control and Weighting type selected in the previous section. 1098 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. • Pinball: When finding the closest source points, a bounding box is created around the target point based on the value of the pinball. Any point outside of the bounding box will not be used. By default, the Program Controlled value is 0.0, which calculates the distance based on .05% of the source region's bounding box size. The bounding box will automatically resize if the mapping is unable to find the minimum number of points required to calculate weighing factors. (Note that resizing occurs only for Program Controlled.) The Pinball option is not available when Weighting is set to Kriging or Shape Function. • Limit: Number of nearby points considered for interpolation. Defaults to 20. Lower values will reduce processing time, however, some distorted or irregular meshes will require a higher Limit value to successfully encounter nodes for triangulation. When Weighting is set to Kriging, the minimum value that can be used is based on the selected Polynomial type. • Weighting Minimum Limit Maximum Limit Triangulation 5 20 Kriging (Constant) 3 (3D), 2 (2D) Number of source points Kriging (Linear) 4 (3D), 3 (2D) Number of source points Kriging (Pure Quadratic) 7 (3D), 5 (2D) Number of source points Kriging (Cross Quadratic) 10 (3D), 6 (2D) Number of source points Outside Option: Enables you to ignore or choose a different weighting algorithm for target points that cannot be found within tetrahedrons/triangles when Triangulation is used. This option is available only for Triangulation. Defaults to Distance Based Average. – Distance Based Average: The mapping will use a weighted average based on distances to the closest Number of Points. – Ignore: Target points will be ignored and no value will be applied. – Projection: Triangles will be created from the closest Number of Points and the target point will be projected onto the plane relative to the triangle surface. If the point is found inside the triangle, the weights are calculated based on the target’s projected location inside the triangle. This option is available only for 3D transfers when the Transfer Type is set to Volumetric. • Number of Points: When Weighting is set to Distance Based Average, or when Outside Option is set to Distance Based Average or Projection, this option is available to specify how many closest source points should be used when calculating weights. Valid range is from 1 to 8 for Distance Based Average and 3 to 20 for Projection. Defaults to 3. • Outside Distance Checking: When Weighting is set to Triangulation and Outside Option is set to Distance Based Average or Projection, this option enables you to specify a Maximum Distance cutoff beyond which source points will be ignored. Defaults to Off. The maximum number of source points is limited to the value specified by the Number of Points setting. – If the Outside Option is set to Distance Based Average, only source points that lie on or within a sphere (centered at the targets location and radius defined by the Maximum Distance value) will provide contributions. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1099 Appendix B. Data Transfer Mesh Mapping – If the Outside Option is set to Projection, the algorithm only uses triangles with centroids that lie on or inside a sphere (centered at the targets location and radius defined by the Maximum Distance value). In Figure: Outside Nodes (Pink) with Mesh Overlay (p. 1100), all the pink nodes on the surface are found “Outside” the source points and will use the Outside Distance Checking based on the Maximum Distance specified. Figure: Outside Nodes (Pink) with Mesh Overlay In Figure: Maximum Distance set to 0.005 (m) (p. 1100), the circle is at the mouse location with radius set to 0.005 (m). Nodes within this radius will be mapped. The source nodes are drawn as black dots and come from an extremely coarse mesh. Figure: Maximum Distance set to 0.005 (m) In Figure: Mapped Nodes (p. 1101), the “Outside” nodes get mapped because they are located within the Maximum Distance. 1100 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Figure: Mapped Nodes The result of the import is shown in Figure: Imported Data using Maximum Distance for Outside Nodes (p. 1101). Transparent areas show target nodes that do not get mapped because there are no source nodes within the Maximum Distance. Figure: Imported Data using Maximum Distance for Outside Nodes When Weighting is set to Kriging, this option allows you to ignore target points that lie outside the source bounding box. Defaults to Off. When this option is set to On, the Bounding Box Tolerance property enables you to include target points that lie outside the source bounding box by specifying a tolerance value. The algorithm adds this tolerance value to the source bounding box when it checks to see if a target point should be ignored or not. • Scale: When weighting is set to Shape Function, the scaling factor (%) determines the number of buckets used to distribute the source elements. Defaults to 50% (2 buckets). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1101 Appendix B. Data Transfer Mesh Mapping • Edge Tolerance: Dimensionless mapping tolerance (default = 0.05). – Shape Function for Surface/Edge topology. • Correlation Function: When weighting is set to Kriging, this property enables you to change the mathematical function that is used to model the spatial correlation between the sample points. Defaults to Gaussian. • Polynomial: When weighting is set to Kriging, this property enables you to change the mathematical function that is used to globally approximate the sample. Defaults to Cross Quadratic. Named Selection Creation These settings enable you to select whether Named Selections should be created for the following items: • Unmapped Nodes: Create a named selection containing all points that cannot be mapped. Defaults to Off. – • Mapped Nodes: Create a named selection containing all mapped points. Defaults to Off. – • Name: Field for the name that will be used when creating the named selection. Defaults to “Unmapped Nodes”. Name: Field for the name that will be used when creating the named selection. Defaults to “Mapped Nodes”. Outside Nodes: Create a named selection containing all the points that cannot be found within tetrahedrons/triangles when Triangulation is used. Defaults to Off. – Name: Field for the name that will be used when creating the named selection. Defaults to “Outside Nodes”. Program Controlled Mapping When Program Controlled mode is selected, the software will use the following table to determine which type of mapping algorithm to use. Default settings will be used based on the properties described above. Source mesh can provide: Target mesh can provide: Weighting that will be used: Nodes Only Nodes Only Uses Triangulation to calculate mapping data. Nodes and Elements Nodes Only Uses Shape Function to calculate mapping data. Manual Mapping When manual mode is selected, you will be able to control advanced settings for the mapper. Based on the mesh data provided from the source and target, you will be able to choose the type of weighting algorithm. If the source mesh contains only points, you will be able to select from the following: • Triangulation • Distance Based Average • Kriging. 1102 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. If the source mesh also contains element data, you will have the items listed above as well as: • Shape Function Element shapes supported during mapping when Shape Function is selected: Element Shape Supported 3 Node Triangle X (2D) 6 Node Triangle X (2D) 4 Node Quadrilateral X (2D) 8 Node Quadrilateral X (2D) 4 Node Tetrahedron X (3D) 10 Node Tetrahedron X (3D) 8 Node Hexahedron X (3D) 20 Node Hexahedron X (3D) 6 Node Wedge X (3D) 15 Node Wedge X (3D) 2D to 3D Mapping Mapping point data from 2D to 3D analyses is possible using the External Data system connected to a downstream Mechanical system. This mapping is performed by collapsing the 3D mesh data into a 2D plane and calculating target point weighting factors from the source point data. 2D results in the XY Plane: You will be able to select the 2D project plane to use based on the available coordinate systems as well as an option to select normal to the 2D source point data (Normal To Plane). Using the Graphics Controls described above, you will be able to turn on and off visualization of the source point data and the 2D projection plane. Source point and 2D projection plane displayed: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1103 Appendix B. Data Transfer Mesh Mapping When selecting Cartesian coordinate systems, the projection will be done on the XY Plane. If the coordinate system is cylindrical, the projection will be rotated about the Z axis into the ZX Plane. Normal To Plane will project the target points into the source point plane. 3D mapped data using cylindrical coordinate system projection: 1104 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Mapping Validation 3D mapped data using Normal To Plane: Notes When mapping point cloud data, the mapping utility does not know where body boundaries are. If you have a model with contact between two bodies, the mapping may pick up points from both bodies causing undesired results. Mapping Validation Mapping Validation objects can be inserted under imported data objects to allow for an evaluation of how the mapping operation performed, by either right-clicking and selecting Insert > Validation from the context menu, or by clicking the Validation button in the toolbar. To perform a validation, right-click the Validation object and select Analyze. The following sections describe different methods to help analyze and determine if the mapping and interpolation that was performed produced an accurate representation of the mapped value data transferred from the source mesh onto the target mesh. Definition A list of variables obtained from the parent object will be listed in the File Identifier drop down. The validation information will be displayed based on the selected item. Settings Within the Settings category, the Type of validation must be specified by selecting Reverse Validation, Distance Based Average Comparison, or Source Value: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1105 Appendix B. Data Transfer Mesh Mapping • Reverse Validation. Reverse Validation takes the results of the imported data (based on the File Identifier) and maps these values back onto the source points. These newly mapped values are compared to the source variables original values. • Distance Based Average Comparison. Distance Based Average Comparison compares the results from the parent (based on the File Identifier) to mapped results obtained by using the distance-based average algorithm. Distance-based mapping will be done using the Number of Points specified. The output graphics will be displayed at the nodal locations of the target mesh. • Source Value. Source Value displays the selected File Identifier data values. With the Display In Parent turned On and the parent of the validation tree node item selected, the interpolated values calculated on the target mesh can easily be compared to the original source point values. The Output Type can be set to Absolute or Relative Difference (default). For Relative Difference, the percent error is calculated and any values that are above 0.01% will be displayed in the graphics window. For Absolute Difference, any non-zero difference will be displayed. The Minimum and Maximum values will be displayed in the Statistics category of the details view. Subsets of the full set for either relative or absolute differences can be shown by adjusting the Display Minimum and Display Maximum fields. These fields must be within the Maximum and Minimum range defined within the Statistics category. Graphics Controls There are multiple display options available: Scaled Spheres, Colored Spheres, Colored Diamonds, and Colored Points. Colored Spheres and Scaled Spheres consume more memory and take longer to display on the screen due to the number of sides being drawn for each sphere. Colored Diamonds consume less memory and time, and Colored Points use the least amount. All displays will be based on the range entered in the Display Minimum/Display Maximum fields. Display items that can are colored will have a discrete legend displayed based on the Display Minimum and Display Maximum, divided equally into six ranges. Scaled Spheres, Colored Spheres, and Colored Diamonds can be scaled based on the Scale field value. If the Display In Parent property is set to On, the validation data currently displayed will also be displayed when the parent object is selected. Statistics The Maximum and Minimum read-only fields show the full range of available results from the validation. Number Of Items shows how many items are currently being displayed in the graphics window. This number is based on the Display Minimum and Display Maximum values. Once a validation has been performed, the data can be exported to a file by simply right-clicking the Validation object and selecting Export. 1106 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis This appendix describes the following: Supported LS-DYNA Keywords LS-DYNA General Descriptions Supported LS-DYNA Keywords The following gathers the supported keywords and their syntax for Explicit Dynamics (LS-DYNA Export) systems. The exported keyword file follows the same format as the corresponding Mechanical APDL application. Keywords conform to the “LS_DYNA Keyword User’s Manual” versions 970 and 971 (version 971 has particular features for the handling of beam cross section and integration options). Each keyword consists of one or more cards, each with one of more parameters. If a parameter is not shown, it will be assigned default values by the LS-DYNA solver. In addition some descriptions to Workbench features that do not relate directly to keywords are given at the end of this section, entitled General Descriptions. *BOUNDARY_NON_REFLECTING Specifies impedance boundaries. Impedance boundaries can only be applied on solid elements in LSDYNA. Card • SSID = ID of segment on whose nodes the boundary is applied (see *SET_SEGMENT bellow). • AD = 0.0 (default) for setting the activation flag for dilatational waves to on. • AS = 0.0 (default) for setting the activation flag for shear waves to on. *BOUNDARY_PRESCRIBED_MOTION_NODE_ID See *BOUNDARY_PRESCRIBED_MOTION_SET *BOUNDARY_PRESCRIBED_MOTION_RIGID_ID See *BOUNDARY_PRESCRIBED_MOTION_SET *BOUNDARY_PRESCRIBED_MOTION_SET_ID Specifies velocity and displacement boundary conditions. Card required for keyword option ID. • ID = ID of the prescribed motion keyword. This parameter is optional and does not have to be unique. An index number is added. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1107 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis • HEADING = Name of the specific boundary condition data. The name is taken from the caption of the applied velocity or displacement in the tree outline of the Mechanical application. Card1 • ID = ID of set of nodes or part (for rigid bodies) to which the boundary condition is applied. • DOF = 1, 2 or 3 depending whether the boundary condition is in the x, y or z direction respectively. Setting 4 is used if the boundary is applied according to a local coordinate system. • VAD = 0 or 2 depending whether the boundary condition is velocity or displacement. • LCID = ID of the curve prescribing the magnitude of the boundary condition. Constant values of velocity are applied as a step function from time = 0. Constant values of displacement are ramped from zero at time = 0 to the constant value at termination time. This is done to make sure that displacements are applied in a transient fashion. • SF = 1.0 (default) scale factor for load curve. • VID = 0 (default). ID of vector that defines the local coordinate system the boundary condition is applied with. • DEATH = 0.0 (default), sets it to 1E28. • BIRTH = 0, the motion is applied from the beginning of the solution. Card2: not required. *BOUNDARY_SPC_SET Specifies Fixed Support, Simple Support and Fixed Rotation constraints. Card • NSID = ID of set of nodes to which the boundary is applied. • CID = ID of the associated coordinate system. 0 specifies the global coordinate system. • DOFX = 0 or 1 for free or fixed translation, respectively, along the x direction. It is set to 0 for Fixed Rotation and to 1 otherwise. • DOFY = 0 or 1 for free or fixed translation, respectively, along the y direction. It is set to 0 for Fixed Rotation and to 1 otherwise. • DOFZ = 0 or 1 for free or fixed translation, respectively, along the z direction. It is set to 0 for Fixed Rotation and to 1 otherwise. • DOFRX = 0 or 1 for free or fixed translation, respectively, along the x direction. It is set to 0 for Simple Support and to 1 otherwise. • DOFRY = 0 or 1 for free or fixed translation, respectively, along the y direction. It is set to 0 for Simple Support and to 1 otherwise. • DOFRZ = 0 or 1 for free or fixed translation, respectively, along the z direction. It is set to 0 for Simple Support and to 1 otherwise. *CONSTRAINED_RIGID_BODIES Specifies rigid bodies to be merged into one part. The resulting Part ID matches the ID of the rigid body designated as the master. 1108 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords This keyword is created for rigid bodies which belong to the same multibody part. By constraining the rigid bodies together using a single multibody part you avoid specifying conflicting motion on the nodes shared among the rigid bodies. All boundary conditions applied to the master body will also be applied to all the slaves. Any boundary conditions that were applied to the slaves will be ignored. The body that is selected to be master is the first one that appears in the multibody-part list. Card • PIDM = ID of the master rigid body. • PIDS = ID of the slave rigid body. *CONSTRAINED_SPOTWELD Specifies spot welds between non-contiguous nodal pairs of shell elements. This keyword is created when a spot weld contact is defined in the Mechanical application. Card • N1 = ID of the first node used in the weld. • N2 = ID of the second node present in the weld. • SN = Normal force at weld failure. • SS = Shear force at weld failure. • N = Exponent of normal force. • M = Exponent of shear force. *CONTACT_AUTOMATIC_GENERAL Specifies friction or frictionless contacts between line bodies (beams). This keyword is created if the contact is specified using Body Interactions and the geometry contains line bodies. All the parameter cards are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. *CONTACT_AUTOMATIC_NODES_TO_SURFACE Specifies nodes-to-surface friction or frictionless contacts. This keyword is created if the contact is specified using a Contact Region and the Behavior is set to Asymmetric. Card1 - mandatory • SSID = ID for the set of slave nodes involved in the contact. • MSID = ID for the set of master segments involved in the contact. • SSTYP = 4, the slave entities for the contact are nodes. • MSTYP = 0, the master entities for the contact are segments. • SBOXID, MBOXID, SPR and MPR are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Parameter Card2 and Card3 is the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1109 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis *CONTACT_AUTOMATIC_SINGLE_SURFACE Specifies friction or frictionless contacts between parts. This keyword is created if the contact is specified using Body Interactions. Card1 - mandatory • SSID = ID for the set of parts created for the bodies in the Body Interaction. If the contact is applied to all the bodies in the geometry then this parameter is set to 0. • MSID = 0. • SSTYP =2, the slave entities are parts. If the contact is applied to all the bodies in the geometry then this parameter is set to 5. • MSTYP = 2, the master entities are parts. If the contact is applied to all the bodies in the geometry then this parameter is set to 0. • SBOXID = It is not used, will be left blank. • MBOXID = It is not used, will be left blank. • SPR = 1 (constant) requests that forces on the slave side of the contact be included in the results files NCFORC (ASCII) and INTFOR (binary). These two results files are not currently specified in the exported K file and are not created. The user will need to manually specify the *DATABASE_NCFORC and *DATABASE_BINARY_INTFOR keywords to obtain them. • MPR = 1 (constant) requests that forces on the master side of the contact be included in the results files NCFORC (ASCII) and INTFOR (binary). These two results files are not currently specified in the exported K file and are not created. The user will need to manually specify the *DATABASE_NCFORC and *DATABASE_BINARY_INTFOR keywords to obtain them. Card2 - mandatory • FS = Friction Coefficient value from the inputs for frictional contact. • FD = Dynamic Coefficient value from the inputs for frictional contact. • DC = Decay Constant value from the inputs for frictional contact. • VC = 0 (LS-DYNA default). • VDC = 10 (constant). This parameter specifies the percentage of the critical viscous damping coefficient to be used in order to avoid undesirable oscillation in the contact. Card3 - mandatory, left blank for defaults to be used. Card A is the same as for *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE. *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE Defines specific surface-to-surface friction or frictionless contacts. This keyword is created if the contact is specified using a Contact Region and the Behavior is set to Symmetric. Card1 - mandatory • SSID = ID for the set of slave segments involved in the contact. • MSID = ID for the set of master segments involved in the contact. • SSTYP = 0, the slave entities for the contact are segments. 1110 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords • MSTYP = 0, the master entities for the contact are segments. • SBOXID, MBOXID, SPR and MPR are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Parameter Card2 and Card3 are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Card A • SOFT = 2 except for asymmetric contacts like NODES_TO_SURFACE and unbreakable bonded contacts for which it is set to 1. • SOFSCL = left blank, the default value of 0.1 will be used. This scale factor is used to determine the stiffness of the interface when SOFT is set to 1. For SOFT = 2 scale factor SLSFAC (see *CONTROL_CONTACT) is used instead. • LCIDAB = left blank. • MAXPAR= left blank. • SBOPT = 3. • DEPTH = 5. *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK Specifies breakable symmetric bonded contacts. This keyword is created for Bonded contact when the Breakable option is set to Stress Criteria and the contact Behavior is set to Symmetric. Card 1 is the same as in *CONTACT_TIED_SURFACE_TO_SURFACE_OFFSET. Card2 - mandatory • FS = Normal Stress Limit value for the bonded contact. • FD = Shear Stress Limit value for the bonded contact. • DC = 0 (LS-DYNA default). This parameter is not required for bonded contacts. • VC and VDC are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Card3 - mandatory, is left blank. Card A is the same as for *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE. *CONTACT_ONEWAY_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK Specifies breakable asymmetric bonded contacts. This keyword is created for Bonded contact when the Breakable option is set to Stress Criteria and the contact Behavior is set to Asymmetric. Parameter cards are the same as in *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TIEBREAK. Card A is not used for this keyword. *CONTACT_TIED_NODES_TO_SURFACE_OFFSET Specifies non breakable asymmetric bonded contacts. This keyword is created for Bonded contacts that are not designated as Breakable whose Behavior is set to Asymmetric. This keyword is not used for Body Interactions as these types of contacts are always symmetric. Card1 - mandatory Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1111 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis • SSID = ID for the set of slave nodes involved in the contact. • MSID = ID for the set of master segment or for the set of parts involved in the contact. • SSTYP = 4. SSID indicates the ID for a set of nodes. • MSTYP = 0, MSID indicates the ID for a set of segments. • SBOXID, MBOXID, SPR and MPR are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Card 2 left blank. Card 3 • SFS = left blank, the default value of 1.0 will be used. Default slave penalty stiffness scale factor for SLSFAC (see *CONTROL_CONTACT). • SFM= left blank, the default value of 1.0 will be used. Default master penalty stiffness scale factor for SLSFAC (see *CONTROL_CONTACT). • SST = the negative value of: "Maximum Offset" is the Definition parameter available for bonded contacts and body interactions. "Maximum Offset" is obtained from the inputs of the Contact Region of Bonded type. • MST = SST. *CONTACT_TIED_SURFACE_TO_SURFACE_OFFSET Specifies general non-breakable bonded contacts that are symmetric. This keyword is created for Bonded and non-breakable contacts which are defined by Contact Regions that are Bonded, non-breakable and whose Behavior is set to Symmetric. Card1 - mandatory • SSID = ID for a set of slave segments or a set of parts involved in the contact. • MSID = ID for the set of master segments or the set of parts involved in the contact. • SSTYP = specifies whether the ID used in SSID represents parts or segments. It is set to 0 if SSID represents a set of segments and 2 if it represents a set of parts. • MSTYP = SSTYP. • SBOXID, MBOXID, SPR and MPR are the same as in *CONTACT_AUTOMATIC_SINGLE_SURFACE. Cards 2 and 3 are the same as in *CONTACT_TIED_NODES_TO_SURFACE_OFFSET. Card A is the same as for *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE. *CONTROL_ACCURACY Specifies control parameters that can improve the accuracy of the calculation. Card 1112 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords • OSU = 1. Global flag for objective stress updates. Required for parts that undergo large rotations. When set to 1 the flag is on. • INN = 4. Invariant node numbering for shell and solid elements. When set to 4 the flag is on for both shell and solid elements. *CONTROL_BULK_VISCOSITY Sets the bulk viscosity coefficients globally. Card • Q1 = Quadratic Artificial Viscosity from the "Damping Controls" in the Analysis Settings. • Q2 = Linear Artificial Viscosity from the "Damping Controls" in the Analysis settings. • TYPE = -2. Internal energy dissipated by the viscosity in the shell elements is computed and included in the overall energy balance. *CONTROL_CONTACT Specifies the defaults for computations of contact surfaces. Card 1 • SLSFAC = 0 (default). Scale factor for sliding interface penalties. When set to 0 the value used is 0.1. This scale factor together with the SFS and SFM parameters of the individual contact keyword (see Card 3 of *CONTACT_TIED_NODES_TO_SURFACE_OFFSET) is used to determine the stiffness of the interface when SOFT is set to 2 (see Card A of *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE). • RWPNAL = 0 (there is no default value). Scale factor for rigid wall penalties. When equal to 0 the constrain method is used and nodal points which belong to rigid bodies are not considered. • ISLCHK = 1 (default). Initial penetration check in contact surfaces. When set to 1 there is no checking. • SHLTHK = 1 (default). Shell thickness considered in surface to surface and node to surface contact types. When set to 1, thickness is considered but rigid bodies are excluded. • PENOPT = 1 (default). Penalty stiffness value option. • THKCHG = 0 (default). • ORIEN = 2. Automatic reorientation for contact segments during initialization. When set to 2 it is active for manual (segment) and automated (part) input. • ENMASS = 0 if the Retain Inertia Of Eroded Material option of the Erosion Controls in the Details window of the analysis settings is set to No. = 2 (default) if Retain Inertia Of Eroded Material option of the Erosion Controls in the Details view of the analysis settings is set to Yes. This parameter regulates the treatment of the mass for eroded nodes in contact. When set to 0 eroding nodes are removed from the calculation. Card 2 • USRSTR = 0. Storage per contact interface for user supplied interface control subroutine. When set to 0 no input data is read and no interface storage is permitted in the user subroutine. • Default values are used for all other parameters. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1113 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis Card3 • SFRIC = 0. Default static coefficient of friction. • Default values are used for all other parameters. Card4 • IGNORE = 2. Specifies whether to ignore initial penetrations in the *CONTACT_AUTOMATIC options. When set to 2 initial penetrations are allowed to exist by tracking them. Also warning messages are printed with the original and the recommended coordinates of each slave node. • FRCENG = 0 (default). • SKIPRWG = 0 (default). • OUTSEG = 1. Yes, output each beam spot weld slave node and its master segment for *CONTACT_SPOTWELD into D3HSP file. • SPOTSTP = 0 (default). • SPOTDEL = 1.Yes, delete the attached spot weld element if the nodes of a spot weld beam or solid element are attached to a shell element that fails and the nodes are deleted. • SPOTHIN = 0.5. This factor can be used to scale the thickness of parts within the vicinity of the spot weld. This factor helps avert premature weld failures due to contact of the welded parts with the weld itself. Should be greater than zero and less than one. *CONTROL_ENERGY Specifies the controls for energy dissipation options. Card • HGEN = 2. Hourglass energy is computed and included in the energy balance. Results are reported in ASCII files GLSTAT and MATSUM. • RWEN = 2 (default). • SLNTEN = 2. Sliding interface energy dissipation is computed and included in the energy balance. Results are reported in ASCII files GLSTAT and SLEOUT. • RYLEN = 2. Rayleigh energy dissipation is computed and included in the energy balance. Results are reported in ASCII file GLSTAT. *CONTROL_HOURGLASS Specifies the global hourglass parameters. Card • IHQ = 1 if Hourglass Damping of type Standard is selected in the Analysis Settings. Also this parameter is equal to 1 if the Flanagan Belytschko option is selected but both the coefficients are zero. = 5 if the Flanagan Belytschko option is selected and the Stiffness Coefficient is non-zero. = 3 if the Flanagan Belytschko option is selected, the Stiffness Coefficient is zero and the Hex Integration Type of the Solver Controls is set to Exact. = 2 if the Flanagan Belytschko option is selected, the Stiffness Coefficient is zero and the Hex Integration Type of the Solver Controls is set to 1pt Gauss. 1114 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords • QH = Viscous Coefficient of the Hourglass Damping section of the Analysis Settings if IHQ is equal to 1, 2, or 3. = Stiffness Coefficient if IHQ is 5. *CONTROL_SHELL Specifies global parameters for shell element types. Card • WRPANG = 20 (default). • ESORT = 1, full automatic sorting of triangular shell elements to treat degenerate quadrilateral shell elements as C0 triangular shells. • IRNXX = -2, shell normal update option. When set to -2 unique nodal fibers are incrementally updated based on the nodal rotation at the location of the fiber. • ISTUPD = 4, shell thickness update option for deformable shells. Membrane strains cause changes in thickness in 3 and 4 node shell elements, however elastic strains are neglected. This option is very important in sheet metal forming or whenever membrane stretching is important. For crash analysis, setting 4 may improve energy conservation and stability. • THEORY = 2 (default). Belytschko-Tsay formulation. • BWC = 1 if Shell BWC Warp Correction option is set to Yes in the Solver Controls section of the Analysis Settings. For this setting, Belytschko-Wong-Chiang warping stiffness is added. = 2 if Shell BWC Warp Correction option is set to No. • MITER = 1 (default). Plane stress plasticity: iterative with 3 secant iterations. • PROJ = 1, the full projection method is used for the warping stiffness in the Belytschko-Tsay and Belytschko-Wong-Chiang shell elements. This option is required for explicit calculations. *CONTROL_SOLID Specifies global parameters for solid element types. Card • ESORT = 1, full automatic sorting of tetrahedron and pentahedron elements to treat degeneracies. Degenerate tetrahedrons will be treated as ELFORM = 10 and pentahedron as ELFORM = 15 solids respectively (see *SECTION_SOLID). *CONTROL_TERMINATION Specifies the termination criteria for the solver. Card • ENDTIM = End Time in the Step Controls section of the Analysis Settings. • ENDCYC = Maximum Time Steps of the Step Controls section of the Analysis Settings. • DTMIN = 0.01 (constant). • ENDENG = Maximum Energy Error from the Step Controls section of the Analysis Settings. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1115 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis • ENDMAS = Maximum Part Scaling from the Step Controls section of the Analysis Settings, if Automatic Mass Scaling is set to Yes. If Automatic Mass Scaling is set to No, the default value of 0.0 is used. *CONTROL_TIMESTEP Specifies conditions for determining the computational time step. Card • DTINIT = Initial Time Step from the Step Controls section of the Analysis Settings. • TSSFAC = Time Step Safety Factor from the Step Controls section of the Analysis Settings. • ISDO = 0 (default). Basis of time size calculation for 4-node shell elements. • TSLIMT = Minimum Element Timestep from the Erosion Controls section of the Analysis Settings, if On Minimum Element Timestep is set to Yes. If On Minimum Element Timestep is set to No the default value of 0.0 is used. • DT2MS = the negative value of Minimum CFL Timestep specified in the Step Controls section of the Analysis Settings, if Automatic Mass Scaling is set to Yes. If Automatic Mass Scaling is set to No the default value of 0.0 is used. • LCTM = ID of the load curve which uses Maximum Time Step from the Step Controls section of the Analysis Settings. • ERODE = 1 (constant). • MS1ST = 0 (default). *DAMPING_GLOBAL Specifies the mass weighted nodal damping applied globally to the nodes of deformable bodies and the center of mass of rigid bodies. Card • LCID = 0, a constant damping factor will be used as specified in VALDMP. • VALDMP = Static Damping from the Damping Controls section of the Analysis Settings. *DATABASE_BINARY_D3PLOT Specifies the sampling parameters for the binary D3PLOT results plotting file. Card • DT = Time from the Output Controls section of the Analysis Settings if Save Results on is set to Time. = End Time divided by the Number of Points if Save Results On is set to Equally Spaced Points. *DATABASE_BINARY_RUNRSF Specifies the sampling parameters for the RUNRSF restart file. Card 1116 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords • CYCL = Time Steps from the Output Controls section of the Analysis Settings if Save Restart Files on is set to Time Steps. = Maximum Time Steps divided by the Number of Points if Save Results On is set to Equally Spaced Time Points. *DATABASE_ELOUT Specifies the sampling parameters for the ELOUT results file (stores stress and strain results). Card • DT = (see *DATABASE_BINARY_D3PLOT). *DATABASE_FORMAT Specifies the format in which to write binary results files like D3PLOT and D3THDT. Card • IFORM = 0, binary results will be written only in the LS-DYNA format. *DATABASE_GLSTAT Specifies the sampling parameters for the GLSTAT results file (stores general energy results). Card • DT = (see *DATABASE_BINARY_D3PLOT). *DATABASE_MATSUM Specifies the sampling parameters for the MATSUM results file (stores general energy and velocity results as the GLSTAT file but it stores them per body. It is necessary for rigid bodies). Card • DT = (see *DATABASE_BINARY_D3PLOT). *DATABASE_NODOUT Specifies the sampling parameters for the NODOUT results file (stores displacement and velocity results). Card • DT = (see *DATABASE_BINARY_D3PLOT). *DEFINE_COORDINATE_SYSTEM Specifies a local coordinate system with three points: one at the local origin, one on the local x-axis and one on the local x-y plane. Card1 • CID = ID of the coordinate system, must be unique. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1117 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis • XO = global X-coordinate of the origin. • YO = global Y-coordinate of the origin. • ZO = global Z-coordinate of the origin. • XL = global X-coordinate of a point on the local x-axis. • YL = global Y-coordinate of a point on the local x-axis. • ZL = global Z-coordinate of a point on the local x-axis. Card2 • XP = global X-coordinate of a point on the local x-y plane. • YP = global Y-coordinate of a point on the local x-y plane. • ZP = global Z-coordinate of a point on the local x-y plane. *DEFINE_CURVE Specifies magnitudes that are given in tabular format. Some keywords require magnitudes to be specified as a load curve. Should a constant be needed, it may be represented as a curve by repeating its value for time steps 0 and 1. Card1 • LCID = ID for load curve, is incremented every time a new load curve is defined. Card2, 3, 4... • A = abscissa value, usually time. • O = ordinate (function) value. *DEFINE_VECTOR Specifies a vector by defining the coordinates of two points. This keyword defines the local coordinate system with respect to which a *BOUNDARY_PRESCRIBED_MOTION is prescribed. The ID of this coordinate system is specified with parameter CID. Card • VID = ID of the vector. • XT = 0, the local x-coordinate of the origin of the coordinate system specified with CID below. • YT = 0, the local y-coordinate of the origin of the coordinate system specified with CID below. • ZT = 0, the local z-coordinate of the origin of the coordinate system specified with CID below. • XH = 1 if the vector has a component in the x direction of the coordinate system specified with CID. Otherwise, this is set to 0. • YH = 1 if the vector has a component in the x direction of the coordinate system specified with CID. Otherwise, this is set to 0. • ZH = 1 if the vector has a component in the x direction of the coordinate system specified with CID. Otherwise, this is set to 0. • CID = ID of the coordinate system used to define the vector. If no coordinate system is specified this parameter is set to 0 to specify the global coordinate system. 1118 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords *ELEMENT_BEAM Specifies beam elements. Card • EID = ID of the element. • PID = ID of the part it belongs to. • N1 = ID of nodal point 1. • N2 = ID of nodal point 2. • N3 = ID of nodal point 3, used for cross section orientation. *ELEMENT_SHELL Specifies three, four, six and eight noded shell elements. Card • EID = ID of the element. • PID = ID of the part it belongs to. • N1 = ID of nodal point 1. • N2 = ID of nodal point 2. • N3 = ID of nodal point 3. • N4 = ID of nodal point 4. • N5-8 = ID of mid side nodes for six and eight noded shells. *ELEMENT_SHELL_THICKNESS_OFFSET This keyword is the same as *ELEMENT_SHELL above with two additional cards for specifying thicknesses per node and the offset of the shell. Card1 - the same as *ELEMENT_SHELL Card2 • THIC1 = shell thickness at node 1. • THIC2 = shell thickness at node 2. • THIC3 = shell thickness at node 3. • THIC4 = shell thickness at node 4. • BETA or MCID = 0 (Default). These parameters specify the base offset angle for Orthotropic materials. Card3 • OFFSET = offset distance from the nodal points plane to the reference surface of the shell. This is specified in the direction of the normal vector of the shell. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1119 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis *ELEMENT_SOLID Specifies 3D solid elements including 10-noded tetrahedrons (second order). Apart from the second order case the two cards are combined into one. Card1 • EID = ID of the element. • PID = ID of the part it belongs to. Card2 • N1 = ID of nodal point 1. • N2 = ID of nodal point 2. • N3 = ID of nodal point 3. • N4 = ID of nodal point 4. • . • . • . • N10 = ID of nodal point 10. *END Terminates the keyword file. It has no parameter cards. Equation Of State (EOS) keywords The following are descriptions for *EOS keywords natively supported by the LS-DYNA export feature. More generally, any *EOS keyword may be introduced into the export file with the help of Commands objects in the Mechanical application (termed Keyword Snippet when referring to the LS-DYNA solver). To use it, insert a Keyword Snippet under a Geometry body in the Tree Outline. The program will automatically substitute the EOSID parameter, in accordance with the *PART keyword (see below) of the associated body. All other parameters in the Keyword Snippet are transcribed literally, overriding any values that would otherwise derive from the Engineering Data workspace. If the *EOS keyword is entered in a Keyword Snippet anywhere else in the Tree Outline, it will be exported literally and the Engineering Data EOS information will also be exported, if present. This practice is not recommended, however, and a warning is provided in the header of Keyword Snippet objects when detected. *EOS_GRUNEISEN Specifies a shock equation of state. This keyword is created when a Shock EOS linear equation of state is present in the properties of a material that is used in the simulation and the Johnson Cook plasticity model is also present. The bilinear version of this equation of state is not currently supported. Card1 • EOSID = ID of the keyword, must be unique between the *EOS keywords. • C = parameter C1 for a Linear Shock EOS property. 1120 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords • S1 = parameter S1 for a Linear Shock EOS property. • S2 = Parameter Quadratic S2 for a Linear Shock EOS property. • S3 = 0. • GAMAO = Gruneisen Coefficient for a Linear Shock EOS property. • A = 0. Card2 - mandatory, left blank. *EOS_LINEAR_POLYNOMIAL Specifies the coefficients for a linear polynomial elastic EOS. The *EOS_LINEAR_POLYNOMIAL keyword is only created when the Johnson Cook strength property is added to the material model (which requires an EOS), but no other EOS has been specified. It is not directly available from the Engineering Data workspace, however. Card1 • EOSID = ID of the keyword, must be unique between the *EOS keywords. • C0 = 0. • C1 = elastic bulk modulus • C2 = 0. • C3 = 0. • C4 = 0. • C5 = 0. • C6 = 0. Card2 - mandatory, left blank. *HOURGLASS Defines hourglass and bulk viscosity properties that are referenced in the *PART keyword via its HGID parameter (see *PART keyword bellow). This keyword can only be created directly with the Keyword Snippet(also, Commands objects) for the LS-DYNA solver. To use it, insert a Keyword Snippet under a Geometry body in the Tree Outline. The program will automatically substitute the HGID parameter in accordance with the *PART keyword (see below) of the associated body. All other parameters in the Keyword Snippet are transcribed literally. If the keyword is entered in a Keyword Snippet anywhere else in the Tree Outline, it will be exported literally. This practice is not recommended, however, and a warning is provided in the header of Keyword Snippet objects when detected. *INITIAL_VELOCITY_GENERATION Specifies initial translational and rotational velocities. Card1 • ID = ID of part where the initial velocity is applied. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1121 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis • STYP = 2, the velocity is applied to a whole part. In Workbench initial velocities can only be applied to whole parts. • OMEGA = angular velocity about the rotational axis. • VX = initial translational velocity in the x direction. • VY = initial translational velocity in the y direction. • VZ = initial translational velocity in the z direction. • IVATN = 0 (default) slave bodies of a multibody part are not assigned the initial velocities of the master part. Card2 • XC = x coordinate of the origin of the applied coordinate system. • YC = y coordinate of the origin of the applied coordinate system. • ZC = z coordinate of the origin of the applied coordinate system. • NX = 0 if there is no angular velocity around the x-axis. = 1 if there is angular velocity around the x-axis. • NY = 0 if there is no angular velocity around the y-axis. = 1 if there is angular velocity around the y-axis. • NZ = 0 if there is no angular velocity around the z-axis. = 1 if there is angular velocity around the z-axis. • PHASE = 0 (default), velocities are applied immediately. *INITIAL_VELOCITY_RIGID_BODY Specifies initial translational and rotational velocities at the center of gravity for rigid bodies. Card • PID = ID of the rigid body. • VX = initial translational velocity in the x direction. • VY = initial translational velocity in the y direction. • VZ = initial translational velocity in the z direction. • VXR = initial rotational velocity around the x-axis. • VYR = initial rotational velocity around the y-axis. • VZR = initial rotational velocity around the z-axis. *INTEGRATION_BEAM Specifies the particulars of the integration method required for complex or user-defined cross sections of beam elements. Card1 • IRID = incremented every time a new keyword is required. 1122 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords • NIP = 0, number of integration points are not specified, instead ICST is used below to choose a standard cross sectional area. • RA = 0, number of integration points are not specified, instead ICST is used below to choose a standard cross sectional area. • ICST = 1-21 depending on the cross sectional area specified in the GUI for the beam geometry. Card2 • D1-D4 = cross sectional dimensions for width and height. • SREF = 1, orientation for s-axis. • TREF = 1, orientation for t-axis. *KEYWORD Marks the beginning of a keyword file. *LOAD_BODY_X Specifies gravitational or other acceleration loads in the x direction. The load is applied to all nodes in the model. Card • LCID = ID of the load curve that represents the magnitude of the load (see *DEFINE_CURVE). • SF = 1.0 (default), load curve scale factor. • LCIDDR = 0 (default), ID of load curve defined for dynamic relaxation. • XC = 0.0 (default), X-center of rotation needed for angular velocities. • YC = 0.0 (default), Y-center of rotation needed for angular velocities. • ZC = 0.0 (default), Z-center of rotation needed for angular velocities. • CID = ID of local coordinate system used. Set to 0 for the global coordinate system. *LOAD_BODY_Y Specifies gravitational or other acceleration loads in the y direction. The load is applied to all nodes in the model. Card (see *LOAD_BODY_X). *LOAD_BODY_Z Specifies gravitational or other acceleration loads in the z direction. The load is applied to all nodes in the model. Card (see *LOAD_BODY_X). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1123 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis *LOAD_NODE_POINT Applies a concentrated force to a node. Card • NODE = ID of the node on which the force is applied. • DOF = 1, 2 or 3 depending on the force direction x, y or z. • LCID = ID of the load curve that describes the magnitude of the force (see *DEFINE_CURVE). • SF = 1.0 (default), load curve scale factor. • CID = ID of local coordinate system used. Set to 0 for the global coordinate system. *LOAD_NODE_SET Applies a concentrated nodal force to a set of nodes. Card (see *LOAD_NODE_POINT. Note that parameter NODE here is replaced by NSID which is the ID of the set of nodes where the force is applied). *LOAD_RIGID_BODY Applies a concentrated nodal force to a rigid body. The force is applied at the center of mass. Card (see *LOAD_NODE_POINT. Note that parameter NODE here is replaced by PID which is the ID of the part the force is applied on). *LOAD_SEGMENT Applies a distributed pressure load over a triangular or quadrilateral face defined by three, four, six (second order triangles) or eight (second order quadrilateral) nodes. Card • LCID = ID of the load curve that describes the magnitude of the pressure (see *DEFINE_CURVE). • SF = 1.0 (default), load curve scale factor. • AT = arrival time for pressure is assigned the time at load step 1 if pressure is given in tabular form or 0 if constant pressure. • N1-N4 = IDs of nodes that define the face. For triangles N4 = N3. • N5-N8 = IDs of mid-side nodes for second order triangles or quadrilaterals. Materials keywords The following are descriptions for *MAT keywords natively supported by the LS-DYNA export feature. More generally, any *MAT keyword may be introduced into the export file with the help of Commands objects in the Mechanical application (termed Keyword Snippet when referring to the LS-DYNA solver). To use it, insert a Keyword Snippet under a Geometry body in the Tree Outline. The program will 1124 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords automatically substitute the MID parameter in accordance with the *PART keyword (see below) of the associated body. All other parameters in the Keyword Snippet are transcribed literally, overriding any values that would otherwise derive from the Engineering Data workspace. If the *MAT keyword is entered in a Keyword Snippet anywhere else in the Tree Outline, it will be exported literally and Engineering Data EOS information will also be exported, if present. This practice is not recommended, however, and a warning is provided in the header of Keyword Snippet objects when detected. *MAT_ELASTIC (or *MAT_001) Specifies isotropic elastic materials. It is available for beam, shell and solid elements. This keyword is used if the selected material includes the Isotropic Elasticity strength model and the Stiffness Behavior is set to Deformable in the Definition section of the body. Card • MID = ID of material type. Must be unique between the material keyword definitions. • RO = density of the material from the Engineering Data workspace. • E = Young's modulus of the material from the Engineering Data workspace, either specified directly or calculated from Bulk and Shear moduli. • PR = Poisson's ratio of the material from the Engineering Data workspace, either specified directly or calculated from Bulk and Shear moduli. *MAT_HYPERELASTIC_RUBBER (or *MAT_077_H) Specifies a general hyperelastic rubber model, optionally combined with viscoelasticity. This keyword is used if the material includes the Mooney-Rivlin, Polynomial or Yeoh hyperelastic strength model and the Stiffness Behavior is set to Deformable in the Definition section of the body. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of the material from the Engineering Data workspace. • PR = Poisson's ratio of the material from the Engineering Data workspace. Values higher than 0.49 are recommended. Smaller values may not work and should not be used. • N = 0, specifies that the constants in card 2 will be defined. • NV = 0. This parameter is not used if N = 0 above. • G = Shear modulus of the material from the Engineering Data workspace. • SIGF = 0. This parameter is not used if N = 0 above. Card2 • C10 = constant C10 from the Engineering Data workspace. • C01 = constant C01 from the material properties in the Engineering Data. Set to zero for Yeoh models. • C11 = constant C11 from the Engineering Data workspace. Set to zero for Yeoh models. • C20 = constant C20 from the Engineering Data workspace. • C02 = constant C02 from the Engineering Data workspace. Set to zero for Yeoh models. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1125 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis • C30 = constant C30 from the Engineering Data workspace. *MAT_JOHNSON_COOK (or *MAT_015) Defines a Johnson - Cook type of material. Such materials are useful for problems with large variations in strain rates where adiabatic temperature increases due to plastic heating cause material softening. This keyword is used if the material specified includes a Johnson Cook strength model. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • G = Shear modulus of material. • E = Young's modulus of the material (shell elements only). • PR = Poisson's ratio of the material (shell elements only). Card2 • A = Initial yield stress from the Johnson Cook strength parameters. • B = Hardening Constant from the Johnson Cook strength parameters. • N = Hardening Exponent from the Johnson Cook strength parameters. • C = Strain Rate Constant from the Johnson Cook strength parameters. • M = Thermal Softening Exponent from the Johnson Cook strength parameters. • TM = Melting Temperature from the Johnson Cook strength parameters. • TR = 15, room temperature. • EPSO = Reference Strain Rate from the Johnson Cook strength parameters. Card3 • CP = Specific Heat from the material properties. • PC = 0 (LS-DYNA default). • SPALL = 2.0 (LS-DYNA default). • IT = 0 (LS-DYNA default). • D1 = D1 parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. • D2 = D2 parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. • D3 = D3 parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. • D4 = D4 parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. Card4 • D5 = D5 parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. • C2/P = "Reference Strain Rate (/sec)" parameter of the Johnson Cook failure model definition, if present. Otherwise it is 0. 1126 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords *MAT_OGDEN_RUBBER (or *MAT_077_O) Specifies the Ogden rubber model, optionally combined with viscoelasticity. This keyword is used if the material includes the Ogden hyperelastic strength model and the Stiffness Behavior is set to Deformable in the Definition section of the body. For card 1 see *MAT_HYPERELASTIC_RUBBER Card2 • MU1 = Material Constant MU1 from the Ogden model. • MU2 = Material Constant MU2 from the Ogden model. • MU3 = Material Constant MU3 from the Ogden model. • MU4 = 0. • MU5 = 0. • MU6 = 0. • MU7 = 0. • MU8 = 0. Card3 • ALPHA1 = Material Constant A1 from the Ogden model. • ALPHA2 = Material Constant A2 from the Ogden model. • ALPHA3 = Material Constant A3 from the Ogden model. • ALPHA1 = 0. • ALPHA1 = 0. • ALPHA1 = 0. • ALPHA1 = 0. • ALPHA8 = 0. *MAT_ORTHOTROPIC_ELASTIC (or *MAT_002) Specifies the model for an elastic-orthotropic behavior of solids, shells and thick shells. This keyword is created when the Orthotropic Elasticity property is present in a material that is used. The Poisson's ratios required with this keyword must be in their minor version, however Workbench requires their major versions hence they are converted by multiplying them by the relevant Young's modulus ratios. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • EA = Young's Modulus X direction from the Orthotropic Elasticity model. • EB = Young's Modulus Y direction from the Orthotropic Elasticity model. • EC = Young's Modulus Z direction from the Orthotropic Elasticity model. • PRBA = Poisson's Ratio XY from the Orthotropic Elasticity model multiplied by Young's Modulus Y / Young's Modulus X. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1127 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis • PRCA = Poisson's Ratio YZ from the Orthotropic Elasticity model multiplied by Young's Modulus Z / Young's Modulus X. • PRCB = Poisson's Ratio XZ from the Orthotropic Elasticity model multiplied by Young's Modulus Z / Young's Modulus Y. Card2 • GAB = Shear Modulus XY from the Orthotropic Elasticity model. • GBC = Shear Modulus YZ from the Orthotropic Elasticity model. • GCA = Shear Modulus XZ from the Orthotropic Elasticity model. • AOPT = 0 (default). When this parameter is set to zero the locally orthotropic material axes are determined from three element nodes. The first node specifies the local origin, the second specifies one of the axes and the third specifies the plane on which the axis rests. = - ID of local coordinate system assigned to the body with this material model. Card3 - mandatory, left blank. Card4 - mandatory, left blank. *MAT_MODIFIED_PIECEWISE_LINEAR_PLASTICITY (or *MAT_123) Defines elasto-plastic materials with arbitrary stress-strain curve and arbitrary strain rate dependency. This keyword is used if the material specified includes a Bilinear or Multilinear Isotropic Hardening (BISO or MISO) strength model. Cards 3 and 4 bellow, are only used if the strength model is MISO. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • E = Young's modulus of the material. • PR = Poisson's ratio of the material. • SIGY = Yield Strength from the BISO strength model. It is not required for MISO models. • ETAN = Tangent Modulus from the BISO strength model. It is not required for MISO models. • FAIL = Maximum Equivalent Plastic Strain EPS parameter of the Plastic Strain failure model, if present. Otherwise it is set to 10E+20. Card2 • C = 0. • P = 0. • LCSS = 0. Card3 - specified only for MISO models. Otherwise it is left blank. • EPS1 = Plastic Strain data from the MISO strength model. If the strength model contains more than 8 data points, the extra data set is ignored. • EPS2 = • EPS3 = 1128 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords • ... • EPS8 = Card4 - specified only for MISO models. Otherwise it is left blank. • ES1 = Yield Stress data that correspond to the above plastic strain data. If the strength model contains more than 8 data points, the extra data set is ignored. • ES2 = • ES3 = • ... • ES8 = *MAT_PLASTIC_KINEMATIC (or *MAT_003) Specifies isotropic and kinematic hardening plastic behavior in materials. This keyword is created when the Bilinear Kinematic Hardening (BKIN) strength model is present in a material. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • E = Young's modulus of the material. • PR = Poisson's ratio of the material. • SIGY = Yield Strength from the BKIN strength model. • ETAN = Tangent Modulus from the BKIN strength model. • BETA = 0. Card2 • SRC = left blank. • SRP = left blank. • FS = Maximum Equivalent Plastic Strain EPS parameter of the Plastic Strain failure model, if present. Otherwise it is left blank. *MAT_RIGID (or *MAT_020) Specifies materials for rigid bodies. This keyword is created when the Stiffness Behavior is set to Rigid under the Definition section of the body. Any strength or EOS material properties defined are ignored. Card1 • MID = ID of material type, must be unique between the material keyword definitions. • RO = density of material. • E = Young's modulus of the material. • PR = Poisson's ratio of the material. Card2 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1129 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis • CMO = 0 if there are no constraints on the rigid body. = -1 if rigid body is constrained in any way. • CON1 = 0 if there are no constraints on the rigid body. = Local Coordinate System ID if associated with the constraint. Otherwise it is set to 0. • CON2 = 0 if there are no constraints on the rigid body. = 111111 if the body is constrained with a fixed support or with a combination of a simple support and a fixed rotation. = 111000 if the body is constrained with a simple support. = 000111 if the body is constrained with a fixed rotation. Card3 • LCO = CON1 if non-zero. Otherwise it will remain blank. *NODE Defines nodes. All the parameters are obtained from mesh definitions of the model. Card • NID = ID of the node. • X = x coordinate. • Y = y coordinate. • Z = z coordinate. *PART Defines geometry bodies. Card1 • HEADING = name of the body specified in the Workbench environment. Card2 • PID = ID of the part. It is set in the LS-DYNA solver and does not reflect the ID specified in the mesh definition of the model. • SECID = ID of the section keyword associated with the part (see *SECTION). • MID = ID of the material keyword associated with the part (see *MAT). • EOSID = ID of the equation of state associated with the material of this part (*EOS and *MAT). If there is no EOS keyword associated with this part then this parameter is set to 0. • HGID = ID of the hourglass keyword associated with the part (see *HOURGLASS). If there is no hourglass keyword associated with this part then this parameter is set to 0. 1130 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Supported LS-DYNA Keywords *SECTION_BEAM Defines cross sectional properties for beam, truss, spot weld and cable elements. Card1 • SECID = ID of the section. • ELFORM = 1. The element formulation option is changed to 3 if the Beam Solution Type option of the Analysis Settings is set to Truss. • SHRF = 1.0 (default). If the cross sectional shape is rectangular or complex (see CST bellow) then SHRF is set to 0.833. • QR = 2 (default), quadrature rule is 2x2 Gauss. If the cross sectional area of the beam is complex or userdefined, this parameter becomes IRID and is assigned the negative value of the IRID parameter in the corresponding *INTEGRATION_BEAM keyword (see above for details). • CST = 0 for solid cross sections = 1 for hollow cross sections = 2 for complex or user defined cross sections. Such cross sections include: hollow rectangular, I, C, L, T, Z, trapezoidal, U and hat shapes. Card2 • • • for solid types – TS1 = width of beam. This refers specifically to the dimension at node 1. – TS2 = TS1. This refers specifically to the dimension at node 2. – TT1 = height of beam. This refers specifically to the dimension at node 1. Set to zero circular solids. – TT2 = TT1. This refers specifically to the dimension at node 2. Set to zero circular solids. for hollow circular types – TS1 = outer diameter of beam. This refers specifically to the dimension at node 1. – TS2 = TS1. This refers specifically to the dimension at node 2. – TT1 = inner diameter of beam. This refers specifically to the dimension at node 1. – TT2 = TT1. This refers specifically to the dimension at node 2. for truss types – • A = cross-sectional area. for general symmetric types – A = cross-sectional area. – ISS = Iyy, moment of inertia about the local s-axis. – ITT = Izz, moment of inertia about the local t-axis. *SECTION_SHELL Defines section properties for shell elements. Card1 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1131 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis • SECID = ID of the section. • ELFORM = 2, if the Full Shell Integration option of the Solver Controls of the Analysis Settings is set to No. = 16 (default) if the Full Shell Integration option of the Solver Controls of the Analysis Settings is set to Yes. • SHRF = Shell Shear Correction Factor option of the Solver Controls of the Analysis Settings. The default value is set to 0.8333. • NIP = Shell Sublayers option of the Solver Controls of the Analysis Settings. The default value is 3. Card2 • T1 = thickness of body. • T2-T4 = T1, shell thickness at nodes 2, 3 and 4. *SECTION_SOLID Defines section properties for solid elements. Card • SECID = ID of the section. • ELFORM = 1 (default). Also, used for first-order hexahedral elements, 5-noded pyramids, 6-noded wedges or bodies with mixed element types that include tetrahedrons together with hexahedrons, pyramids or wedges. = 10 if elements are first-order tetrahedrons and Tet Pressure Integration option of the Solver Controls of the Analysis Settings is set to Constant. = 13 if elements are first-order tetrahedrons and Tet Pressure Integration option of the Solver Controls of the Analysis Settings is set to Average Nodal. = 16 if the elements are second-order tetrahedrons. *SET_NODE_LIST Defines a set of nodes. Card2 is repeated as many times as required to specify all the node IDs in the set. Card1 • SID = ID of the set. Card2 • NID1-NID8 = IDs for eight of the nodes in the set. *SET_PART_LIST Defines a set of parts. Card2 is repeated as many times as required to specify all the part IDs in the set. Card1 1132 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. LS-DYNA General Descriptions • SID = ID of the set. Card2 • PID1-PID8 = IDs for eight of the parts in the set. *SET_SEGMENT Defines triangular and quadrilateral segments. Card2 is repeated as many times as required to specify all the segments in the set. Card1 • SID = ID of the set. Card2 • N1-N4 = IDs of nodes that define one of the segments. For triangular segments N4=N3. *TITLE Defines a job title. Card • TITLE = a user input. This can only be entered manually after the .k file is exported. LS-DYNA General Descriptions All the exported keywords are grouped into their respective sections in the .k file. These sections are the same as the ones used by the Mechanical APDL application exporting facility apart from the "KEYWORD SNIPPETS" section. The section titles and their order is the following: • NODE DEFINITIONS • SECTION DEFINITIONS • MATERIAL DEFINITIONS • PARTS DEFINITIONS • ELEMENT DEFINITIONS • LOAD DEFINITIONS • CONTACT DEFINITIONS • CONTROL OPTIONS • TIME HISTORY • INITIAL VELOCITY DEFINITIONS • LIST SETS • BOUNDARY CONDITIONS • KEYWORD SNIPPETS Keyword-snippets are supported for geometry bodies, for Connections and the Explicit Dynamics analysis section. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1133 Appendix C. LS-DYNA Keywords Used in an Explicit Dynamics Analysis For geometry bodies, you can enter LS-DYNA specific material and equation of state types together with the *HOURGLASS keyword. These keywords should always have a non zero value entered for their ID. This is usually the first parameter of the keyword and can be any integer that fits within the 10 character field-width of the parameter. The same number can be entered for all of these keywords as the software will replace it with an appropriate unique value. The IDs of these keywords will be assigned to the *PART keyword associated with the body that the keyword-snippet belongs to. You will be informed with a comment shown at the beginning of the text editor of the snippet, about the keywords that should be entered. For the Connections, you can enter LS-DYNA contact keywords which are not available for definition from the GUI. These keywords can be assigned to the geometry by using the names of pre-defined Named Selections. When the keywords are exported, these names will be replaced with IDs from the *SET keywords created for the relevant Named Selections. If the contact region associated with the Keyword Snippet has its scoping defined, by entering "contact" and "target" for the master and slave entries of the contact keyword, the IDs of the *SET keywords for the Contact Region scoping will be used instead. One contact keyword should be entered per snippet, which can be followed by as many other keywords as required. The latter will not be processed and will be exported as entered. For the analysis, you will be asked to enter global parameters with keywords like *CONTROL and *DATABASE. As these parameters are global they do not need to be associated with any other keywords so their contents will only be transferred to the .k file and will not be utilized in any other way. Other project tree entries apart from the ones mentioned above, where keyword snippets could be useful can be implemented at a later date if requested, or proved to be necessary. Keywords that are entered with the keyword-snippet facility are grouped under a common section called "KEYWORD SNIPPETS" at the end of the .k file. Named selections whether having anything assigned to them or not, like for example a load or constrain, will be exported as a set of IDs. This set can then be used in LS-PREPOST or by editing the .k file manually to assign LS-DYNA specific keywords which are not represented in Workbench. Due to the restriction of the field widths specified for each keyword, if the number to be used has more characters than the field width allows, the following process is followed to make sure the number fits within the field: • The number is converted to scientific. • If the scientific format is still larger than the required field width then digits are removed from the decimal part. This is done by cleaning first the exponential number from any leading zeroes. • If all the decimals are removed and the number is still larger then digits from the mantissa are removed and the exponent increased by 1 for every digit removed. 1134 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Appendix D.Workbench Mechanical Wizard Advanced Programming Topics This appendix examines programming techniques and provides a reference for customizing the Mechanical Wizard. Topics Overview (p. 1135) URI Address and Path Considerations (p. 1136) Using Strings and Languages (p. 1137) Guidelines for Editing XML Files (p. 1138) About the TaskML Merge Process (p. 1138) Using the Integrated Wizard Development Kit (WDK) (p. 1139) Using IFRAME Elements (p. 1139) TaskML Reference (p. 1140) Standard Object Groups Reference (p. 1169) Tutorials (p. 1172) Wizard Development Kit (WDK) Groups (p. 1182) Overview From a programming perspective, the Mechanical Wizard system is best described as a "task browser." As a "web browser" used to view and navigate pages on the Internet, a task browser is used to view and navigate tasks in an engineering system. A web browser accesses HTML files and resources on a network; a task browser accesses TaskML files and resources on a network. TaskML is an XML vocabulary that defines the rules and data necessary to display and process pages of tasks in the Mechanical application. Like HTML, TaskML allows for general scripting and for inserting arbitrary HTML content and user interface controls. Basic wizard customization using TaskML is similar to working with HTML and requires only a text editor. The Mechanical Wizard runs as a web application (specifically, a dynamic HTML page) inside of a web browser control (Microsoft Internet Explorer). The web browser control is hosted by the Mechanical application. Consequently, the Mechanical Wizard system has full access to the capabilities of the web browser and the Mechanical application. Development of the Mechanical Wizard involves use of the HTML, CSS, XML, JScript web standards, and, for access to and automation of the application, use of the Mechanical application object model. The Mechanical Wizard displays tasks organized into groups. A task displays a caption and a status or descriptive icon. Activating a task (by clicking) typically involves automatic navigation to a particular context and selection in the user interface and display of a "callout" with a text message pointing to a specific control. Custom tasks may perform any operation via TaskML elements or scripting. The Mechanical Wizard responds to events that occur in the Mechanical application. Adding a load is an example of an event. When such an event occurs, each task is given the opportunity to determine its status or take an action. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1135 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics The user may open a TaskML file inside the Mechanical Wizard from their local disk or from a network location. Therefore, saving TaskML to a network server makes custom wizard definitions available to any user with access to the server. Additionally, the Mechanical Wizard system itself may be run by any number of clients from a network location. TaskML, along with HTML and scripting, offers an efficient and powerful means of extending the Mechanical application user interface. URI Address and Path Considerations The Merge (p. 1141), Script (p. 1142), task (p. 1147), set-icon (p. 1166), open-url (p. 1161), display-help-topic (p. 1158) and iframe (p. 1150) TaskML elements use URIs to link together files to form a complete wizard definition. TaskML supports the following URI formats. Note Standard network security conditions apply to these URIs. As a general rule, if a user cannot open a linked file in their web browser, the file cannot be accessed by the Mechanical Wizard. Local Machine and LAN C:\folder\Wizard.xml M:\folder\Wizard.xml \\server\share\Wizard.xml Standard Protocols http://webserver/share/Wizard.xml ftp://ftp.webserver.com/pub/Wizard.xml file:///C:/folder/Wizard.xml SIMWIZ Protocol The SIMWIZ protocol supports paths relative to the location of the Mechanical Wizard (specifically, relative to the location of the file Default.htm in the Mechanical Wizard folder). The SIMWIZ protocol allows custom TaskML files published to any arbitrary location to reuse standard TaskML files and other components of the system. simwiz://Tasks/StandardTasks.xml Relative Paths All relative paths are relative to the location of the file containing the link. Note that this behavior is different from version 6.0, in which relative links were relative to the location of the Mechanical Wizard. folder/Wizard.xml ./folder/Wizard.xml ../folder/Wizard.xml /rootfolder/Wizard.xml 1136 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Using Strings and Languages Using Strings and Languages The Mechanical Wizard obtains all strings from TaskML. The language-related section of the TaskML uses the following structure: <strings> <language xml:lang="language-code"> <string id="String_ID">Sample Text</string> </language> </strings> The Mechanical Wizard determines which strings to use by matching the Language setting in the Wizard page of the Control Panel to the xml:lang attribute of a language element. If no language element with a matching xml:lang attribute exists, or if no string element with the necessary ID exists, the Mechanical Wizard takes the string from the language element with the xml:lang attribute set to "enus" (English, United States). If the default English string doesn't exist, the Mechanical Wizard takes the first string with a matching ID or displays the string ID in place of the text. Recommended Localization Process This process describes how to localize all strings in a TaskML file: 1. Open the TaskML file in a text editor. 2. Copy the section of the file from: <language xml:lang="en-us"> to </language> 3. Paste the copy into the<string> element below the last <language> close tag. 4. Change the language code from en-us to the code appropriate for the localization. 5. Localize each <string> element within the new <language> element. String IDs must remain unchanged. 6. Test the new language by entering the language code in the Language setting in the Wizard page of the Control Panel. English Customization Process This process describes how to customize individual English strings with specific information or terminology: 1. Create a new <language xml:lang="x-foo"> element at the bottom of the <string> element below the last </language> close tag. Set the xml:lang attribute to an arbitrary “x-code” descriptive of the customization (no spaces). 2. Copy individual <string> elements to customize from the < language xml: lang="en-us"> element to the new <language xml: lang="x-foo"> element. Strings omitted from the new <language> element will be obtained from the <language xml: lang="en-us"> element. 3. Customize the strings. String IDs must remain unchanged. 4. Test the customized strings by entering the x-code in the Language setting in the Wizard page of the Control Panel. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1137 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Guidelines for Editing XML Files TaskML is an XML vocabulary. As such, TaskML consists of Unicode (wide character) text files that must follow the standard XML rules for well-formedness. When editing a TaskML file, use caution to ensure that the XML remains well-formed. For example, omitting a close tag will cause an error and may prevent the wizard from loading. To test for well-formedness, open the file in Internet Explorer 5 or later. Note • XML is case-sensitive. All TaskML tags are lower-case. • Attribute values must be in quotes. • Use only the five predefined XML entity references for special characters if needed: & (&amp;), < (&lt;) > (&gt;) " (&quot;) ' (&apo;). • White space (new lines, tabs, etc) is generally discarded. However, within a string element extra white space may result in multiple spaces between words. At this release there is no way to insert a line break within a string element. • string elements contain only text; string (p. 1146) elements may not contain any XML or HTML elements. • XML comments are allowed. About the TaskML Merge Process The merge process facilitates reuse of wizard components from local or network locations. The merge process is the first step in loading TaskML into the Mechanical Wizard. The process involves selectively copying information from a merged TaskML document into a parent TaskML document. The parent document includes a Merge (p. 1141) element linking to the merged file. The merge process generates a composite TaskML document in memory; neither the parent or merged TaskML files are modified. The merge process consists of the following steps: 1. If the merged TaskML document contains Merge (p. 1141) elements, this process is called recursively. That is, a TaskML document may merge a file that merges a file, and so on. 2. Script (p. 1142) elements are copied to the parent only if the src attribute is unique. 3. object-group (p. 1142) elements are copied to the parent only if the merged object-group has a unique name attribute. 4. status (p. 1144) elements are copied to the parent only if the merged status has a unique id. 5. language (p. 1145) collections (and contained string elements) are copied only if the language has a unique xml:lang attribute. 6. string (p. 1146) elements are copied only if the merged string has a unique id. 7. task (p. 1147) elements are copied only if the merged task has a unique id. 8. If both the parent and the merged TaskML documents contain a group (p. 1149) with the same id: 1138 • Attributes defined for the merged group but omitted in the parent group are copied to the parent group. • All children of the merged group are appended to the parent group. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Using IFRAME Elements For diagnostic purposes the merge process automatically adds a merged-from attribute to elements added to the parent TaskML file. The merged-from attribute contains the url of the TaskML file from which the element was obtained. Using the Integrated Wizard Development Kit (WDK) The Mechanical Wizard system includes an integrated toolkit to assist in customizing wizards. The following topics describe the tools: • WDK: Tools Group • WDK: Commands Group • WDK Tests: Actions • WDK Tests: Flags (Conditions) To enable the toolkit: • In the Mechanical application, select Tools>Options. • Select Wizard and set Enable WDK Tools to yes. Enabling the WDK toolkit adds four groups to the bottom of every panel displayed in the Mechanical Wizard. The WDK toolkit does not change the behavior of other groups in the panel. Using IFRAME Elements An IFRAME (inline frame) functions as an HTML document within a Mechanical Wizard group. An IFRAME may contain any content, from static text to detailed user interface controls. IFRAMEs have full script access to the Mechanical Wizard, and therefore full access to the Mechanical application. The Options group in the Insert Geometry panel demonstrates a simple user interface extension using an IFRAME. Other examples of IFRAME usage in the Mechanical application include the WDK: Tools group and "Tip of the Day." IFRAMEs in the Mechanical Wizard provide a way to customize the Mechanical application without modifying the main user interface. IFRAMEs may be published on a network, enabling customized user interfaces for multiple users without requiring changes to each installation. Working with IFRAMEs requires familiarity with HTML and JScript coding. See also Tutorial: Adding a Web Search IFRAME (p. 1176). Security Restrictions Due to the cross-frame scripting security model enforced by the web browser control, custom IFRAME HTML pages should reside in the same location as the Mechanical Wizard. IFRAME pages from a different domain as the parent page cannot access the parent via script. IFRAME Toolkit The WDK includes the following resources for developing IFRAMEs: • The file MechanicalWizard\WDK\Info_IFRAME.htm contains a template HTML document for an IFRAME. View the source for descriptions of recommended HTML elements and JScript functions. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1139 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics • The file MechanicalWizard\System\IFrame.js implements generic functions for use in IFRAMEs. The following files demonstrate use of IFRAMEs: • MechanicalWizard\WDK\Tools_IFrame.htm contains implementation for the WDK: Tools IFRAME. See MechanicalWizard\WDK\Tools_Merge.xml for corresponding TaskML. • MechanicalWizard\Panels\InsertGeometry_IFrame.htm contains implementation for the Insert Geometry panel Options group. See MechanicalWizard\Panels\InsertGeometry.xml for corresponding TaskML. • MechanicalWizard\TipoftheDay\IFrame.htm contains implementation for Tip of the Day. See MechanicalWizard\Panels\Startup.xml for corresponding TaskML. TaskML Reference This reference describes each element defined in TaskML. See XML Notes for general usage guidelines. The Overview Map contains a diagram showing the basic structure of TaskML. • Document Element (p. 1141) • External References (p. 1141) • Object Grouping (p. 1142) • Status Definitions (p. 1144) • Language and Text (p. 1145) • Tasks and Events (p. 1146) • Wizard Content (p. 1148) • Rules (p. 1151) • Scripting (p. 1167) Overview Map of TaskML The following illustrates the basic hierarchical structure of TaskML. • simulation-wizard (p. 1141) document element – Merge (p. 1141) elements – Script (p. 1142) elements – object-groups (p. 1143) collection – statuses (p. 1144) collection – strings (p. 1146) collection – tasks (p. 1148) collection → task (p. 1147) elements • update-event (p. 1148) element – Rules (p. 1151) sequence • activate-event (p. 1146) element – Rules (p. 1151) sequence 1140 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference – body (p. 1148) element → group (p. 1149) elements • taskref (p. 1150) elements • iframe (p. 1150) elements • eval (p. 1167) statements → eval (p. 1167) statements Document Element • simulation-wizard (p. 1141) simulation-wizard Identifies the start of a TaskML file. <simulation-wizard version="1.0"> Attributes version Specifies the version of the TaskML vocabulary. The current version is "1.0." Element Information Parents None.This is the document element (root) of the XML structure. Children Merge, Script, object-groups, statuses, strings, tasks, body End Tag Required External References • Merge (p. 1141) • Script (p. 1142) Merge Merges an external TaskML file. <merge src="url" /> Attributes src Specifies the URL of the TaskML file to merge. Table D.1 Element Information Parents simulation-wizard Children None Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1141 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics End Tag No - close element with "/>" See Also About the TaskML Merge Process (p. 1138) and URI Address and Path Considerations (p. 1136). Script Specifies an external JScript file to load into the Mechanical Wizard. <merge src="url" /> Attributes src Specifies the URL of the JScript file to load. Remarks • JScript files use the .js file extension. • Code in the JScript file outside of any function is evaluated immediately upon loading. • The eval element may directly call functions defined in the JScript file. Table D.2 Element Information Parents simulation-wizard Children None End Tag No - close element with "/>" See Also URI Address and Path Considerations (p. 1136). Object Grouping • object-group (p. 1142) • object-groups (p. 1143) • object-type (p. 1143) object-group Organizes objects by placing them in an assigned group. <object-group name="group_name"> Attributes name Specifies the name of the group. 1142 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference Element Information Parents object-groups Children object-type End Tag Required See Also object (p. 1155), select-first-object (p. 1163), select-all-objects (p. 1161), Standard Object Groups Reference (p. 1169). object-groups Contains an unordered collection of object group definitions. <object-groups> Element Information Parents simulation-wizard Children object-group End Tag Required See Also Standard Object Groups Reference (p. 1169). object-type Specifies an Outline object by its internal identifiers. <object-type class="id_Constant" type="id_Constant" /> Attributes class Identifies the class ID constant. type Identifies the type ID constant. Applies only for a class of "id_Load" or "id_Result." Remarks ID constants are defined in the script file DSConstants.js. The class attribute corresponds to the "Class" property of the Mechanical application objects. The type attribute corresponds the "loadType" or "ResultType" property of specific the Mechanical application objects. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1143 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Element Information Parents object-group Children None End Tag No - close element with "/>" See Also Standard Object Groups Reference (p. 1169). Status Definitions • status (p. 1144) • statuses (p. 1144) status Defines a task status. <status id="statusID" css-class="status-class" tooltip="statusID_Tooltip" /> Attributes id Unique identifier for the status. css-class Specifies the class in the skin (cascading style sheet) to apply to the task. The style class defines the visual appearance of task status. tooltip Optional. Specifies the string ID of text to display in a tooltip when the cursor hovers over the task. Defaults to "statusID_Tooltip." Element Information Parents statuses Children None End Tag No - close element with "/>" See Also set-status (p. 1167). statuses Contains an unordered collection of status definitions. 1144 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference <statuses> Element Information Parents simulation-wizard Children status End Tag Required See Also set-status (p. 1167). Language and Text • data (p. 1145) • language (p. 1145) • string (p. 1146) • strings (p. 1146) data Data placeholder within a string. <string id="stringID">string text<data />string text</string> Remarks Used only with the Lookup method on a Strings object as defined in StringLookupObject.js. Allows JScript functions to retrieve a localized string containing arbitrary data. Element Information Parents string Children None End Tag No - close element with "/>" language Contains an unordered collection of strings in a specified language. <language [xml:lang="en us"]> Attributes xml:lang Specifies the language code. Defaults to "en-us" (English, United States). Remarks The language code corresponds to the Language setting in the Wizard page of the Control Panel. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1145 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Element Information Parents strings Children string End Tag Required string Specifies the text for a given string ID. <string id="stringID">string text</string> Attributes id Unique identifier assigned to the string. Element Information Parents language Children data End Tag Required strings Contains an unordered collection of languages. <strings> Element Information Parents simulation-wizard Children language End Tag Required Tasks and Events • activate-event (p. 1146) • task (p. 1147) • tasks (p. 1148) • update-event (p. 1148) activate-event Contains a sequence of rules to process when the user clicks on a task. <activate-event tab="{design | print | report | help | any}"> 1146 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference Attributes tab Optional. Selects a specific tab before processing the activate event rules. design Selects the Design View tab. Default behavior if attribute omitted. print Selects the Print Preview tab. report Selects the Report Preview tab. help Selects the Quick Help tab. any Does not change tab selection. Element Information Parents task Children if, set-icon, set-caption, set-status, select-first-object, select-all-objects, select-field, select-first-undefined-field, select-first-parameter-field, select-zero-thickness-sheets, click-button, display-taskcallout, display-outline-callout, display-details-callout, display-toolbar-callout, display-tab-callout, display-status-callout, open-url, display-help-topic, send-mail, eval, update, debug End Tag Required task Defines a task. <task id="uniqueID" caption="uniqueID_Caption" tooltip="uniqueID_Tooltip" disable-if-missing="group_name" hide-if-missing="group_name" check-ambiguity="{model | environment | solution}" icon="url" deemphasize="{yes | no}"> Table D.3 Attributes Attribute Description id Arbitrary unique identifier assigned to the task. caption Optional. Specifies the string ID of the text to display in the task caption. Defaults to "uniqueID_Caption" if not specified. tooltip Optional. Specifies the string ID of the text to display in the task tooltip. Defaults to "uniqueID_Toolip" if not specified. disable-if-missing Optional. Disables the task if an object matching the group name does not exist. hide-if-missing Optional. Hides the task if an object matching the group name does not exist. check-ambiguity Optional. Automatically tests for ambiguity of an outline level prior to processing event rules. icon Optional. Specifies the URI of an image to use as the task icon. See URI Address and Path Considerations. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1147 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Attribute Description deemphasize Optional. Causes a task inside an emphasized group to render with a deemphasized style. Table D.4 Element Information Parents tasks Children update-event, activate-event End Tag Required Also See: taskref tasks Contains an unordered collection of task definitions. <tasks> Element Information Parents simulation-wizard Children task End Tag Required update-event Contains a sequence of rules to process when the user navigates or modifies information in the Mechanical application. <update-event> Element Information Parents task Children if, set-icon, set-caption, set-status, select-first-object, select-all-objects, select-field, select-first-undefined-field, select-first-parameter-field, select-zero-thickness-sheets, click-button, display-taskcallout, display-outline-callout, display-details-callout, display-toolbar-callout, display-tab-callout, display-status-callout, open-url, display-help-topic, send-mail, eval, debug End Tag Required Wizard Content • body (p. 1148) • group (p. 1149) • iframe (p. 1150) • taskref (p. 1150) body Specifies content to display inside the Mechanical Wizard. 1148 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference <body title="stringID"> Attribute title Optional. Specifies the string ID of text to display in the title of the panel containing the Mechanical Wizard. Defaults to the text "Mechanical Wizard." Element Information Parents simulation-wizard Children group, eval End Tag Required group Defines a collapsible group of tasks or iframes. <group id="uniqueID" caption="uniqueID_Caption" description="uniqueID_Description" emphasize="{yes | no}" collapsed="{yes | no}" onupdate="foo()"> Attributes id Arbitrary unique identifier assigned to the group. caption Optional. Specifies the string ID of the text to display in the group caption. Defaults to "uniqueID_Caption" if not specified. description Optional. Specifies the string ID for a brief paragraph to display at the top of the group. Defaults to "uniqueID_Description" if not specified. If the string ID is undefined the group contains no description. emphasize Optional. Emphasizes the group via different visual styles. Defaults to "no." collapsed Optional. Initially displays the group collapsed. After first use the collapsed status of each group is persisted. Defaults to "no." onupdate Optional. JScript expression to evaluate on the Update event prior to processing the update-event (p. 1148) rules for tasks the group contains. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1149 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Element Information Parents body Children taskref, iframe, eval End Tag Required iframe Inserts an HTML IFRAME element within a group. The IFRAME may contain any arbitrary web page and may communicate with the Mechanical Wizard via script. <iframe src="uri" /> Attributes src Specifies the URI of the web page to load into the IFRAME. See the topic on IFRAME Elements for notes on security restrictions. Table D.5 Element Information Parents group Children None End Tag No - close element with "/>" See Also Using IFRAME Elements (p. 1139). taskref Inserts a task into a group. <taskref task="uniqueID" /> Attributes task Specifies the ID of a task defined elsewhere in the merged TaskML file. Element Information Parents group Children None End Tag No - close element with "/>" See Also task (p. 1147). 1150 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference Rules • Statements (p. 1151) • Conditions (p. 1153) • Actions (p. 1156) Statements • and (p. 1151) • debug (p. 1151) • if then else stop (p. 1151) • not (p. 1152) • or (p. 1153) • update (p. 1153) and Performs a logical conjunction on two conditions. Equivalent to the JScript && operator. condition1 <and> condition2 </and> Element Information Parents if Children Conditions: level, object, changeable-length-unit , assembly-geometry, geometry-includes-sheets, zero-thickness-sheetActions: select-first-object, select-all-objects, select-field, select-first-undefinedfield, select-first-parameter-field, select-zero-thickness-sheets, eval End Tag Required debug Attempts to launch a script debugger to debug the JScript code corresponding to the rules in the current event. Equivalent to the JScript debugger keyword. <debug /> Element Information Parents update-event, activate-event, then, else Children None End Tag No - close element with "/>" if then else stop Conditionally processes a sequence of rules, depending on the value of a condition. <if> condition <then> rules <stop/> </then> <else> Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1151 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics rules <stop/> </else> </if> Remarks eval (p. 1167) statement. The not (p. 1152) operator negates the value of a condition. The and (p. 1151) and or (p. 1153) operators perform logical operations on two conditions within an if statement. The then statement contains a sequence of rules to process when the resolved value of the condition is true. An if statement must contain one then statement. The else statement contains a sequence of rules to process when the resolved value of the condition is false. The else statement is optional. If used it must follow the close of the then statement. The if...then...else structure is equivalent to the if...else statement in JScript: if( condition ) { statements } else { statements } The stop statement ends processing of an event at a specific point. If a stop statement is not included within a then or else statement, rules following the if statement are processed. The stop statement is equivalent to the JScript return statement. Element Information for <if> Parents update-event and activate-event Children Operators: and, or, not Conditions: level, object, changeable-length-unit , assembly-geometry, geometry-includes-sheets,zero-thickness-sheet Actions: select-first-object,select-all-objects,select-field, select-first-undefined-field, select-first-parameter-field, select-zero-thickness-sheets, eval Element Information for <then> and <else> Parents if Children set-icon, set-caption, status, select-first-object, select-all-objects, select-field, select-first-undefinedfield,select-first-parameter-field,select-zero-thickness-sheets,click-button,display-task-callout,displayoutline-callout, display-details-callout, display-toolbar-callout, display-tab-callout, display-statuscallout, open-url, display-help-topic, send-mail, eval, update, debug End Tag Required not Performs logical negation on a condition. Equivalent to the JScript ! operator. <not> condition </not> Element Information Parents if Children Conditions: level, object, changeable-length-unit , assembly-geometry, geometry-includes-sheets, zero-thickness-sheet Actions: select-first-object, select-all-objects, select-field, select-first-undefinedfield, select-first-parameter-field, select-zero-thickness-sheets, eval 1152 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference End Tag Required or Performs a logical disjunction on two conditions. Equivalent to the JScript || operator. condition1 <or> condition2 </or> Element Information Parents if Children Conditions: level, object, changeable-length-unit , assembly-geometry, geometry-includes-sheets, zero-thickness-sheet Actions: select-first-object, select-all-objects, select-field, select-first-undefinedfield, select-first-parameter-field, select-zero-thickness-sheets, eval End Tag Required update Forces an Update event to fire. In general, this statement is necessary only if preceding rules in the event cause the status of other tasks to become out of sync. <update /> Element Information Parents activate-event, then, else Children None End Tag No - close element with "/>" Conditions • assembly-geometry (p. 1153) • changeable-length-unit (p. 1154) • geometry-includes-sheets (p. 1154) • level (p. 1154) • object (p. 1155) • zero-thickness-sheet (p. 1156) assembly-geometry Tests if the geometry in context of the current selection contains an assembly or a single part. <assembly-geometry /> Element Information Parents if, and, or, not Children None End Tag No - close element with "/>" Return Value True if the geometry contains an assembly. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1153 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics changeable-length-unit Tests if the geometry in context of the current selection does not explicitly specify a length unit (e.g. for ACIS geometry types). Useful in prompting the user to verify a correct length unit setting. <changeable-length-unit /> Element Information Parents if, and, or, not Children None End Tag No - close element with "/>" Return Value True if the length unit is not read-only. geometry-includes-sheets Tests if the geometry in context of the current selection contains sheet parts. <geometry-includes-sheets /> Element Information Parents if, and, or, not Children None End Tag No - close element with "/>" Return Value True if the geometry contains one or more sheets. level Tests the level of the current selection in the Outline. <level type="{project | model | environment | solution}" condition="{is-ambiguous | is-not-ambiguous | is-selected | is-not-selected}" /> Attributes type Identifies the level. A level consists of a container (e.g., the Environment) and all children excluding other containers. condition Specifies a condition to test. is-ambiguous Returns true if a specific container cannot be resolved given the current Outline selection. is-not-ambiguous Returns true if a specific container is identified given the current Outline selection. is-selected Returns true if any object at the given level is currently selected. is-not-selected Returns true if no object at the given level is currently selected. 1154 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference Element Information Parents if, and, or, not Children None End Tag No - close element with "/>" Return Value As defined by the condition attribute. object Tests the Outline tree for an object matching the given criteria. Searches only non-ambiguous objects given the current selection. <object type="group_name" state="{any | stateless | fully-defined | under-defined | suppressed | not-updated | updated | obsolete | error | bad-license}" name-regexp="regular_expression" condition="{exists | does-not-exist | is-selected | is-not-selected}" /> Note It was necessary to “word wrap” the long line of code in the above example. Attributes type Optional. Identifies an object group name or an object type constant as a search criteria. If omitted, the object type is not considered. Object groups are defined by using the object-group (p. 1142) element. Refer to the Standard Object Groups Reference (p. 1169). Type constants for specific objects (prefixed by "id_") are defined in the script file DSConstants.js. state Optional. Specifies an object state as a search criteria. If omitted, the default of "any" is used, meaning that object state is not considered. States are defined in the script file DSConstants.js. name-regexp Optional. Specifies a regular expression of an object's name as a search criteria. For example, "part" matches any object that includes "part" in its name (e.g. "part 2"). If omitted, object names are not considered. See the Microsoft Scripting site under JScript for a regular expressions reference. condition Specifies a condition to test. exists Returns true if an object matching the criteria exists. does-not-exist Returns true if no object matches the criteria. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1155 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics is-selected Returns true if an object matching the criteria is currently selected. is-not-selected Returns true if no object matching the criteria is currently selected. Element Information Parents if, and, or, not Children None End Tag No - close element with "/>" Return Value True if an object matching the criteria meets the condition. zero-thickness-sheet Tests if the geometry in context of the current selection contains any sheet with zero thickness specified. Useful in prompting the user to enter valid information for sheet thickness. <zero-thickness-sheet /> Element Information Parents if, and, or, not Children None End Tag No - close element with "/>" Return Value True if any sheet has a zero thickness value. valid-emag-geometry Tests if the geometry in context of the current selection meets the requirements for performing an electromagnetic simulation. <valid-emag-geometry /> enclosure-exists Tests if the geometry in context of the current selection contains an enclosure body for electromagnetic simulation. <enclosure-exists /> Actions • click-button (p. 1157) • display-details-callout (p. 1157) • display-help-topic (p. 1158) • display-outline-callout (p. 1158) • display-status-callout (p. 1159) • display-tab-callout (p. 1159) • display-task-callout (p. 1160) • display-toolbar-callout (p. 1160) • open-url (p. 1161) 1156 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference • select-all-objects (p. 1161) • select-field (p. 1162) • select-first-object (p. 1163) • select-first-parameter-field (p. 1164) • select-first-undefined-field (p. 1164) • select-zero-thickness-sheets (p. 1165) • send-mail (p. 1165) • set-caption (p. 1166) • set-icon (p. 1166) • set-status (p. 1167) click-button Simulates a toolbar button click. <click-button toolbar="key" button="key" /> Attributes Use the WDK command View Current Toolbar Keys to determine values for the attributes below. toolbar Specifies the key for the toolbar. button Specifies the key for the button. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if successful. See Also display-toolbar-callout (p. 1160). display-details-callout Displays a callout pointing to the currently selected Details field. <display-details-callout message="stringID" /> Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1157 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Attributes message Specifies the string ID of the text to display in the callout. Remarks Before using this action: Use select-first-object (p. 1163) or select-all-objects (p. 1161) to select one or more Outline objects prior to accessing the Details control. Use select-field (p. 1162) to select a Details field. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if successful. display-help-topic Displays a topic from a Windows HTML Help file. <display-help-topic href="uri" topic="path" /> Attributes href Optional. Defines the URI of the CHM file. Defaults to simwiz://../HHelp/DesignSpace.chm, the location of the ANSYS Workbench Help system relative to the standard Mechanical Wizard location. NOTE: The default value no longer exists - Please specify a valid help system path. See URI Address and Path Considerations (p. 1136). topic Optional. Specifies an internal path to a desired topic. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value None display-outline-callout Displays a callout pointing to the currently selected Outline object. 1158 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference <display-outline-callout message="stringID" /> Attributes message Specifies the string ID of the text to display in the callout. Remarks Use select-first-object (p. 1163) or select-all-objects (p. 1161) to select one or more Outline objects prior to displaying the callout. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if successful. display-status-callout Displays a callout pointing to a status bar panel. <display-status-callout panel="index" message="stringID" /> Attributes panel Specifies the index of the status bar panel. The index of the leftmost panel is 1. message Specifies the string ID of the text to display in the callout. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if successful. display-tab-callout Displays a callout pointing to a tab. <display-tab-callout tab="{design | print | report | help}" message="stringID" /> Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1159 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Attributes tab One of the following keywords: design Design View tab. print Print Preview tab. report Report Preview tab. help Quick Help tab. message Specifies the string ID of the text to display in the callout. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if successful. display-task-callout Displays a callout pointing to the task itself. <display-task-callout message="stringID" /> Attributes message Specifies the string ID of the text to display in the callout. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if successful. display-toolbar-callout Displays a callout pointing to a toolbar button. <display-toolbar-callout toolbar="key" button="key" message="stringID" /> 1160 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference Attributes Use the WDK command View Current Toolbar Keys to determine values for the toolbar and button attributes below. toolbar Specifies the key for the toolbar. button Specifies the key for the button. message Specifies the string ID of the text to display in the callout. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if successful. See Also click-button (p. 1157). open-url Opens a new web browser window and navigates to a given URI (URL). <open-url href="uri" /> Attributes href Any valid URI. See URI Address and Path Considerations (p. 1136). Element Information Parents activate-event, then, else Children None End Tag No - close element with "/>" Return Value None select-all-objects Selects a set of objects based on given criteria. Searches only non-ambiguous objects given the initial selection. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1161 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics <select-all-objects type="group_name" state="{any | stateless | fully-defined | under-defined | suppressed | not-updated | updated | obsolete | error | bad-license}" name-regexp="regular_expression" /> Note It was necessary to “word wrap” the long line of code in the above example. Attributes type Optional. Identifies an object group name or an object type constant as a search criteria. If omitted, the object type is not considered. Object groups are defined by using the object-group (p. 1142) element. Refer to the Standard Object Groups Reference (p. 1169). Type constants for specific objects (prefixed by "id_") are defined in the script file DSConstants.js. state Optional. Specifies an object state as a search criteria. If omitted, the default of "any" is used, meaning that object state is not considered. States are defined in the script file DSConstants.js. name-regexp Optional. Specifies a regular expression of an object's name as a search criteria. For example, "part" matches any object that includes "part" in its name (e.g. "part 2"). If omitted, object names are not considered. See the Microsoft Scripting site under JScript for a regular expressions reference. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if one or more objects meeting the criteria were selected. See Also select-first-object (p. 1163). select-field Selects a field in the Details control by name. <select-field name="stringID" /> 1162 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference Attributes name Specifies the string ID for name of the field. Use the Details Field String ID section in the WDK Tools group to determine the string ID of a field. Remarks Use select-first-object (p. 1163) or select-all-objects (p. 1161) to select one or more Outline objects prior to accessing the Details control. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if one Details meeting the criteria was selected. See Also select-first-parameter-field (p. 1164), select-first-undefined-field (p. 1164). select-first-object Selects the first object matching given criteria. Searches only non-ambiguous objects given the initial selection. <select-first-object type="group_name" state="{any | stateless | fully-defined | under-defined | suppressed | not-updated | updated | obsolete | error | bad-license }" name-regexp="regular_expression" /> Note It was necessary to “word wrap” the long line of code in the above example. Attributes type Optional. Identifies an object group name or an object type constant as a search criterion. If omitted, the object type is not considered. Object groups are defined by using the object-group (p. 1142) element. Refer to the Standard Object Groups Reference (p. 1169). Type constants for specific objects (prefixed by "id_") are defined in the script file DSConstants.js. state Optional. Specifies an object state as a search criteria. If omitted, the default of "any" is used, meaning that object state is not considered. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1163 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics States are defined in the script file DSConstants.js. name-regexp Optional. Specifies a regular expression of an object's name as a search criterion. For example, "part" matches any object that includes "part" in its name (e.g., "part 2"). If omitted, object names are not considered. See the Microsoft Scripting site under JScript for a regular expressions reference. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if one object meeting the criteria was selected. See Also select-all-objects (p. 1161). select-first-parameter-field Selects the first parameter field in the Details control. <select-first-parameter-field /> Remarks Parameter fields contain a check box to the left of the name. If checked, the parameter field is exposed for use in the Parameter Workspace. Use select-first-object (p. 1163) or select-all-objects (p. 1161) to select one or more Outline objects prior to accessing the Details control. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if one Details meeting the criteria was selected. See Also select-field (p. 1162), select-first-undefined-field (p. 1164). select-first-undefined-field Selects the first undefined Details field. <select-first-undefined-field /> Remarks The Details control highlights undefined fields in yellow. 1164 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference Use select-first-object (p. 1163) or select-all-objects (p. 1161) to select one or more Outline objects prior to accessing the Details control. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if one Details meeting the criteria was selected. See Also select-field (p. 1162), select-first-parameter-field (p. 1164). select-zero-thickness-sheets Selects all parts containing zero-thickness sheet geometry. <select-zero-thickness-sheets /> Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if one or more objects meeting the criteria were selected. select-enclosures Selects any enclosure bodies in the current geometry. <select-enclosures /> send-mail Opens a new email and fills in envelope information and default text. Does not send the email. <send-mail to="addr;addr" cc="addr;addr" bcc="addr;addr" subject="stringID" body="stringID" /> Attributes to Semicolon-delimited list of email addresses. cc Optional. Semicolon-delimited list of email addresses. bcc Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1165 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Optional. Semicolon-delimited list of email addresses. subject Optional. Default subject line. body Optional. Default body text. Element Information Parents activate-event, then, else Children None End Tag No - close element with "/>" Return Value None set-caption Sets the caption of the task. <set-caption caption="stringID" /> Attributes caption Specifies the string ID of the text. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if successful. See Also task (p. 1147). set-icon Sets the task icon to an image at a given URL. <set-icon src="url" /> Attributes src Specifies the URI of the icon. See URI Address and Path Considerations (p. 1136). 1166 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. TaskML Reference Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if successful. See Also task (p. 1147). set-status Sets the status of the task. <set-status status="{non-status | incomplete | complete | information | undefined | indeterminate | solve | obsolete | ambiguous | caution | warning | disabled | hidden}" /> Note It was necessary to “word wrap” the long line of code in the above example. Attributes status A status keyword. Status keywords are defined by using the status (p. 1144) element. Remarks The element definition shown above lists the standard statuses. The TaskML file MechanicalWizard\Data\Statuses.xml defines the standard statuses and is merged automatically while loading any wizard. Element Information Parents activate-event, if, and, or, not, then, else Children None End Tag No - close element with "/>" Return Value True if successful. Scripting • eval (p. 1167) eval Evaluates a JScript expression. <eval code="expression" /> Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1167 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Attributes code A string of valid JScript code. For example, "foo()" evaluates the global function foo. Remarks Use the Script (p. 1142) element to make custom JScript available for use with the eval statement. If the eval statement is a task rule, the expression is evaluated when the rule is processed as part of an event. Using eval in this context allows: • custom code to determine the status of a task • the task to perform any arbitrary operation The file MechanicalWizard\WDK\Tools_Merge.xml demonstrates use of the eval statement to: • Execute global functions defined in a script file referenced by a Script (p. 1142) element. • Access the DOM to manipulate the DHTML page containing the wizard. • Call methods on global objects to automate the Mechanical Wizard. If the eval statement exists inside of a body or group element, the expression evaluates at that point in the generation of the wizard DHTML. Using eval in this context allows for programmatically generating wizard content. See Startup.xml, New.xml and InsertGeometry.xml in the MechanicalWizard\Panels folder for examples. These examples call global functions defined in the script file MechanicalWizard\System\PanelFunctions.js. Complete coverage of scripting is beyond the present scope of this documentation. You may use the source code as a reference and a script debugger for exploring variables and object models. The following globally-available JScript objects are particularly useful: • g_Wizard - the global Wizard object that controls the Mechanical Wizard. Defined in MechanicalWizard\System\WizardObject.js. • g_Wizard.App - provides access to the key objects in the Mechanical application and ANSYS Workbench. Defined in MechanicalWizard\System\AppObject.js. • g_Wizard.App.Scripting - reference to the script block inside the Mechanical application. • g_Wizard.GlobalStrings - a Strings object (StringLookupObject.js) containing generic strings defined in MechanicalWizard\Data\GlobalStrings.xml. • g_Wizard.Strings - a Strings object containing strings from the loaded TaskML document. Element Information Parents As an action or condition:activate-event,update-event,if,and,or,not,then,else For evaluation as the wizard loads: body, group Children None End Tag No - close element with "/>" Return Value Return value of the expression or null. 1168 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Standard Object Groups Reference Standard Object Groups Reference The following table lists standard object-group (p. 1142) names and the object-type (p. 1143) elements they contain. The corresponding TaskML file is MechanicalWizard\Data\ObjectGroups.xml, and is merged automatically while loading any wizard. The elements object (p. 1155), select-first-object (p. 1163), and select-all-objects (p. 1161) use object groups. TaskML files may include an object-groups (p. 1143) section to define custom object-group (p. 1142) elements (for example, to identify a specific object such as pressure). See Tutorial: Creating a Custom Task (p. 1173) for an example. Class and Type correspond to constants defined in the script file DSConstants.js. Type corresponds to the "loadType" or "ResultType" property of specific Mechanical application objects. Group Name Class project id_Project model id_Model environment id_Environment solution id_AnswerSet geometry id_PrototypeGroup part id_Prototype contact id_ContactGroup contact region id_ContactRegion mesh id_MeshControlGroup mesh control id_MeshControl global load id_Acceleration Type id_Rotation load id_Load structural load id_Load id_SurfacePressure id_Load id_SurfaceForce id_Load id_EdgeForce id_Load id_VertexForce id_Load id_CylinderBoltLoad id_Load id_ForceAtAPoint id_Load id_SurfaceMoment id_Load id_SurfaceRotation id_Load id_EdgeRotation id_Load id_VertexRotation id_Load id_EdgeMoment id_Load id_VertexMoment Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1169 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Group Name Class Type displacement load id_Load id_SurfaceDisplacement id_Load id_EdgeDisplacement id_Load id_VertexDisplacement id_Load id_SurfaceSupport id_Load id_FixedEdgeSupport id_Load id_FixedVertexSupport id_Load id_CylinderRadialSupport id_Load id_CylinderRadialAndAxialSupport id_Load id_SurfaceFrictionlessSupport id_Load id_CylinderFixedSupport id_Load id_CylinderPinnedSupport id_Load id_SimpleEdgeSupport id_Load id_SimpleVertexSupport id_Load id_SurfaceHeatFlux id_Load id_SurfaceTemperature id_Load id_EdgeTemperature id_Load id_VertexTemperature id_Load id_SurfaceConvection id_Load id_SurfaceInsulation id_Load id_SurfaceHeat id_Load id_EdgeHeat id_Load id_VertexHeat id_Load id_InternalPartHeat thermal load stress tool id_StressSafetyTool stress tool result id_Result id_StressSafetyMargin id_Result id_StressSafetyFactor id_Result id_StressRatio result id_Result structural result id_Result id_EquivalentStress id_Result id_MaximumPrincipalStress id_Result id_IntermediatePrincipalStress id_Result id_MinimumPrincipalStress id_Result id_MaximumShearStress id_Result id_StressIntensity id_Result id_XComponentStress id_Result id_YComponentStress id_Result id_ZComponentStress id_Result id_XYShearStress 1170 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Standard Object Groups Reference Group Name thermal result Class Type id_Result id_YZShearStress id_Result id_XZShearStress id_Result id_EquivalentStrain id_Result id_MaximumPrincipalStrain id_Result id_IntermediatePrincipalStrain id_Result id_MinimumPrincipalStrain id_Result id_MaximumShearStrain id_Result id_StrainIntensity id_Result id_XComponentStrain id_Result id_YComponentStrain id_Result id_ZComponentStrain id_Result id_XYShearStrain id_Result id_YZShearStrain id_Result id_XZShearStrain id_Result id_TotalDisplacement id_Result id_XComponentDisplacement id_Result id_YComponentDisplacement id_Result id_ZComponentDisplacement id_Result id_Temperature id_Result id_TotalHeatFlux id_Result id_XComponentHeatFlux id_Result id_YComponentHeatFlux id_Result id_ZComponentHeatFlux id_Result id_MaximumPrincipalThermalStrain id_Result id_IntermediatePrincipalThermalStrain id_Result id_MinimumPrincipalThermalStrain id_Result id_XComponentThermalStrain id_Result id_YComponentThermalStrain id_Result id_ZComponentThermalStrain fatigue tool id_FatigueTool fatigue result id_Result id_FatigueLife id_Result id_FatigueSafetyFactor id_Result id_FatigueDamage id_Result id_FatigueBiaxialityIndication id_Result id_FatigueRainflowMatrix id_Result id_FatigueDamageMatrix id_Result id_FatigueSensitivity Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1171 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Group Name Class Type frequency id_Result id_Frequency Tutorials • Tutorial: Adding a Link (p. 1172) • Tutorial: Creating a Custom Task (p. 1173) • Tutorial: Creating a Custom Wizard (p. 1175) • Tutorial: Adding a Web Search IFRAME (p. 1176) Tutorial: Adding a Link This tutorial covers the steps needed to add a custom link to the Links group. The Links group is available in any of the standard wizards. View the completed TaskML file for this tutorial. Steps To add a link to the web site MatWeb: Open the TaskML file MechanicalWizard\Tasks\Links.xml in a text editor such as Notepad. All standard wizards Merge (p. 1141) the Links.xml file; changes made to this file automatically appear in all standard wizards. Create a new task (p. 1147) definition by adding the following to the tasks (p. 1148) section: <tasks> <task id="DesignSpaceHomePage" icon="simwiz://Icons/Link.gif"> <activate-event> <open-url href="http://www.designspace.com" /> </activate-event> </task> <task id="DesignSpaceResources" icon="simwiz://Icons/Link.gif"> <activate-event> <open-url href="http://www.designspace.com/designspace/user_support/" /> </activate-event> </task> <task id="MatWeb" icon="simwiz://Icons/Link.gif"> <activate-event> <open-url href="http://www.matweb.com/" /> </activate-event> </task> </tasks> The value for the id attribute is arbitrary. Define a new string (p. 1146) by adding the following to the strings (p. 1146) section: <strings> <language xml:lang="en-us"> <string id="Standard_Links_Caption"> Links </string> <string id="DesignSpaceHomePage_Caption"> DesignSpace.com </string> <string id="DesignSpaceResources_Caption"> DesignSpace Resources </string> 1172 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials <string id="MatWeb_Caption"> MatWeb Materials </string> </language> </strings> The value for the string id uses the built-in naming convention of the task id and "_Caption" to simplify the task element by omitting the caption attribute. The new string applies to the default language code "en-us." To support other languages, define a new string inside each language (p. 1145) section. Insert the new task into the Links group (p. 1149) by modifying the body (p. 1148) section as follows: <body> <group id="Standard_Links" collapsed="yes"> <taskref task="DesignSpaceHomePage" /> <taskref task="DesignSpaceResources" /> <taskref task="MatWeb" /> </group> </body> The task attribute matches the id of the task. Save the file. Open a wizard in the Mechanical application. The Links group will contain a new link to the MatWeb website. Tutorial: Creating a Custom Task This tutorial describes the steps needed to develop a custom task for inserting a 100 psi pressure load. The tutorial for Creating a Custom Wizard uses the task created below. View the completed TaskML file for this tutorial. Steps Copy the file MechanicalWizard\Tasks\InsertStructuralLoad.xml to a file named Insert100psi.xml in a different folder.Generally, the easiest way to create a custom task is to modify a similar existing task instead of starting from scratch. task (p. 1147) element as follows: <task id="Insert100psi" disable-if-missing="geometry" check-ambiguity="environment"> The other attributes on the task element disable the task if the Outline contains no geometry and prompts the user to select a particular Environment if the current selection is ambiguous. Create an object-groups (p. 1143) section at the top of the file: <simulation-wizard version="1.0"> <object-groups> <object-group name="pressure"> <object-type class="id_Load" type="id_SurfacePressure" /> </object-group> </object-groups> ... </simulation-wizard> This creates a custom object-group (p. 1142) named "pressure" that contains a single object-group (p. 1142) corresponding to the Pressure object type in the Outline. This object group is available in addition to the Standard Object Groups Reference (p. 1169) to wizards merging this task. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1173 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Modify the strings (p. 1146) section as follows: <strings> <language xml:lang="en-us"> <string id="Insert100psi_Caption"> Insert Pressure </string> <string id="Insert100psi_Message"> Use the Structural button to insert a Pressure load. Enter 100 psi for Magnitude. </string> </language> </strings> The value for the first string id uses the built-in naming convention of the task id and "_Caption" to simplify the task element by omitting the caption attribute. The value for the second string id is arbitrary and referenced by the display-details-callout action defined below. The strings apply to the default language code "en-us." To support other languages, define new strings inside each language (p. 1145) section. Modify the update-event (p. 1148) as shown: <update-event> <if><object type="pressure" condition="does-not-exist"/> <then> <set-status status="incomplete"/> <stop/> </then> </if> <if><object type="pressure" condition="exists" state="under-defined"/> <then> <set-status status="undefined"/> <stop/> </then> </if> <set-status status="complete"/> </update-event> Modify the activate-event (p. 1146) as shown: <activate-event> <if><object type="pressure" condition="exists" state="under-defined"/> <then> <select-first-object type="pressure" state="under-defined"/> <select-first-undefined-field/> <display-details-callout message="Insert100psi_Message" /> <stop/> </then> </if> <if><level type="environment" condition="is-not-selected"/> <then> <select-first-object type="environment"/> </then> </if> <click-button toolbar="DS_graphics" button="Surface"/> <display-toolbar-callout toolbar="Context" button="Structural" message="Insert100psi_Message" />*** </activate-event> Note ***Please note that it was necessary to “word wrap” the long line of code in the above example. 1174 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials The first if statement checks for an under-defined pressure. The second if statement ensures that the Outline selection is at the Environment level so that the user can insert a Pressure. The click-button action ensures that the surface selection mode is active. Save the file. Proceed to the tutorial Creating a Custom Wizard to use this custom task. Tutorial: Creating a Custom Wizard This tutorial describes the steps needed to develop a custom wizard. Before proceeding, complete the tutorial Creating a Custom Task. View the completed TaskML file for this tutorial. Steps Copy the file MechanicalWizard\StressWizard.xml to a file named CustomWizard.xml in the same folder as the file Insert100psi.xml created in the previous tutorial. Change "InsertStructuralLoad.xml" to "Insert100psi.xml" in the Merge (p. 1141) element: <merge src="Insert100psi.xml" /> This merge makes the custom task definition available to this wizard. Note that the URI to the file containing the task is relative to the location of the file containing the wizard. See URI Address and Path Considerations (p. 1136). Modify the strings (p. 1146) section as follows: <strings> <language xml:lang="en-us"> <string id="Title_Caption"> Tutorial Wizard </string> <string id="Title_Description"> Demonstrates a custom wizard with a task for inserting a 100 psi Pressure. </string> </language> </strings> Change "InsertStructuralLoad" to "Insert100psi" in the taskref (p. 1150) element: <taskref task="Insert100psi"/> This taskref adds the task (p. 1147) to the body (p. 1148) of the wizard by its id. Save the file. In the Mechanical application, click the Choose Wizard option from the top of a standard wizard. Choose "browse for a custom wizard definition.". Select the file CustomWizard.xml. Test the Insert Pressure task. The task should behave in the same way as the standard Insert Loads task but with specific instructions for defining a 100 psi pressure. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1175 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Tutorial: Adding a Web Search IFRAME This tutorial describes the steps needed to add an Internet search capability to a wizard as an IFRAME. This tutorial uses the wizard created in Tutorial: Creating a Custom Wizard (p. 1175). See Using IFRAME Elements (p. 1139) for a discussion on IFRAMEs. View the file Search.htm or the modified TaskML file CustomWizard.xml. Steps Create a new text file with the following contents: <html> <head> <script src="System/IFrame.js"></script> <link ID="Skin" REL="stylesheet"> <script> function IFrame_onload() { Skin.href = g_Wizard.GetSkin() } </script> <style> INPUT { width: 100%; margin-bottom: 4px; } </style> </head> <body scroll="no"> <center> <form method="GET" action="http://www.google.com/search" target="_blank"> <a HREF="http://www.google.com/" target="_blank"> <img SRC="http://www.google.com/logos/Logo_40wht.gif" border="0" ALT="Google" width="128" height="53"></a><br> <input TYPE="text" name="q" size="25" maxlength="255" value><br> <input type="submit" name="btnG" VALUE="Google Search"> </form> </center> </body> </html> Note It was necessary to “word wrap” the long line of code in the above example. Note 1176 • The script file MechanicalWizard/System/IFrame.js contains generic functions for use with IFRAMEs. • The link element initially lacks a href element. The script block implements the IFRAME_onload function (called by IFrame.js) and sets href to the url returned by the GetSkin method on the g_Wizard object. The file MechanicalWizard\WDK\Info_IFRAME.htm contains an inaccuracy in that the link is not automatically assigned. • The style element provides some additional formatting rules. • The body element has the scroll element set to "no" to preserve margins and prevent scrollbars from appearing. As long as a reference to IFrame.js appears in the IFRAME the Mechanical Wizard will autosize the height such that scrollbars are unnecessary. • The contents of the body is based on free code published by Google. • Note use of the target attribute to prevent the linked pages from opening in place of the Mechanical Wizard. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials Save the file as Search.htm in the Mechanical Wizard folder. The files must reside together for web browser security to permit cross-frame scripting. Open the file CustomWizard.xml from the previous tutorial. Add the following group at the bottom of the body: <group id="Search" collapsed="yes"> <iframe src="simwiz://Search.htm" /> </group> Add the following string to the <strings><language xml:lang="en-us"> section: <string id="Search_Caption"> Search the Web </string> Note the use of the "groupID_Caption" shortcut for the string id. Save the file and open the wizard in the Mechanical application. Completed TaskML Files The following sections examine examples of completed TaskML files. Links.xml <?xml version="1.0" encoding="ISO-8859-1"?> <?xml version="1.0"?> <simulation-wizard version="1.0"> <strings> <language xml:lang="en-us"> <string id="Standard_Links_Caption"> Links </string> <string id="DesignSpaceHomePage_Caption"> DesignSpace.com </string> <string id="DesignSpaceResources_Caption"> DesignSpace Resources </string> <string id="MatWeb_Caption"> MatWeb Materials </string> </language> </strings> <tasks> <task id="DesignSpaceHomePage" icon="simwiz://Icons/Link.gif"> <activate-event> <open-url href="http://www.designspace.com" /> </activate-event> </task> <task id="DesignSpaceResources" icon="simwiz://Icons/Link.gif"> <activate-event> <open-url href="http://www.designspace.com/designspace/user_support/" /> </activate-event> </task> <task id="MatWeb" icon="simwiz://Icons/Link.gif"> <activate-event> <open-url href="http://www.matweb.com/" /> </activate-event> </task> </tasks> <body> <group id="Standard_Links" collapsed="yes"> <taskref task="DesignSpaceHomePage" /> Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1177 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics <taskref task="DesignSpaceResources" /> <taskref task="MatWeb" /> </group> </body> </simulation-wizard> Insert100psi.xml <?xml version="1.0" encoding="ISO-8859-1"?> <?xml version="1.0"?> <simulation-wizard version="1.0"> <object-groups> <object-group name="pressure"> <object-type class="id_Load" type="id_SurfacePressure" /> </object-group> </object-groups> <strings> <language xml:lang="en-us"> <string id="Insert100psi_Caption"> Insert Pressure </string> <string id="Insert100psi_Message"> Use the Structural button to insert a Pressure load. Enter 100 psi for Magnitude. </string> </language> </strings> <tasks> <task id="Insert100psi" disable-if-missing="geometry" check-ambiguity="environment"> <update-event> <if><object type="pressure" condition="does-not-exist"/> <then> <set-status status="incomplete"/> <stop/> </then> </if> <if><object type="pressure" condition="exists" state="under-defined"/> <then> <set-status status="undefined"/> <stop/> </then> </if> <set-status status="complete"/> </update-event> <activate-event> <if><object type="pressure" condition="exists" state="under-defined"/> <then> <select-first-object type="pressure" state="under-defined"/> <select-first-undefined-field/> <display-details-callout message="Insert100psi_Message" /> <stop/> </then> </if> <if><level type="environment" condition="is-not-selected"/> <then> <select-first-object type="environment"/> </then> </if> <click-button toolbar="DS_graphics" button="Surface"/> <display-toolbar-callout toolbar="Context" button="Structural" message="Insert100psi_Message" />*** </activate-event> </task> </tasks> </simulation-wizard> 1178 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials Note ***Please note that it was necessary to “word wrap” the long line of code in the above example. CustomWizard.xml <?xml version="1.0" encoding="ISO-8859-1"?> <?xml version="1.0"?> <simulation-wizard version="1.0"> <merge src="Tasks/InsertGeometry.xml" /> <merge src="Tasks/VerifyLengthUnit.xml" /> <merge src="Tasks/DefineSheetThickness.xml" /> <merge src="Tasks/AssignMaterial.xml" /> <merge src="Insert100psi.xml" /> <merge src="Tasks/InsertDisplacementLoad.xml" /> <merge src="Tasks/ThermalStressNote.xml" /> <merge src="Tasks/InsertStructuralResults.xml" /> <merge src="Tasks/StressStiffeningNote.xml" /> <merge src="Tasks/Solve.xml" /> <merge src="Tasks/ViewResults.xml" /> <merge src="Tasks/ViewReport.xml" /> <merge src="Tasks/StandardTasks.xml"/> <strings> <language xml:lang="en-us"> <string id="Title_Caption"> Tutorial Wizard </string> <string id="Title_Description"> Demonstrates a custom wizard with a task for inserting a 100 psi Pressure. </string> </language> </strings> <body> <group id="Title"> <taskref task="ChooseWizard"/> </group> <group id="RequiredSteps" emphasize="yes"> <taskref task="InsertGeometry"/> <taskref task="VerifyLengthUnit"/> <taskref task="DefineSheetThickness"/> <taskref task="AssignMaterial"/> <taskref task="Insert100psi"/> <taskref task="InsertDisplacementLoad"/> <taskref task="ThermalStressNote"/> <taskref task="InsertStructuralResults"/> <taskref task="StressStiffeningNote"/> <taskref task="Solve"/> <taskref task="ViewResults"/> <taskref task="ViewReport"/> </group> <group id="Standard_OptionalTasks" /> <group id="Standard_ParameterTasks" /> <group id="Standard_GeneralTasks" /> <group id="Standard_AdvancedTasks" /> <group id="Standard_Links" /> </body> </simulation-wizard> Search.htm <?xml version="1.0" encoding="ISO-8859-1"?> <!doctype HTML public "-//W3C//DTD HTML 4.0 Frameset//EN"> <html> Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1179 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics <!--(==============================================================)--> <!--(Document created with RoboEditor. )============================--> <!--(==============================================================)--> <head> <title>Search</title> <!--(Meta)==========================================================--> <meta <meta <meta <meta <meta <meta <meta <meta <meta name=generator content="RoboHELP by eHelp Corporation - www.ehelp.com"> name=generator-major-version content=0.1> name=generator-minor-version content=1> name=filetype content=kadov> name=filetype-version content=1> name=page-count content=1> name=layout-height content=427> name=layout-width content=640> name=date content="07 9, 2003 11:30:11 AM"> <!--(Links)=========================================================--> <link ID=Skin REL=stylesheet> <!--(Style Sheet)===================================================--> <style> <!-INPUT { width: 100%; margin-bottom: 4px; } --> </style> <!--(Scripts)=======================================================--> <script src="System/IFrame.js"></script> <script>function IFrame_onload() { Skin.href = g_Wizard.GetSkin() }</script> </head> <!--(Body)==========================================================--> <body scroll=no> <form method=GET action="http://www.google.com/search" target=_blank> <p style="text-align: center;" align=center><a HREF="http://www.google.com/" target=_blank><img src="http://www.google.com/logos/Logo_40wht.gif" ALT=Google style="width: 128px; height: 53px; border-style: none;" width=128 height=53 border=0></a><br> <input TYPE=text name=q size=25 maxlength=255 value><br> <input type=submit 1180 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Tutorials name=btnG VALUE="Google Search"></p> </form> </body> </html> CustomWizardSearch.xml <?xml version="1.0"?> <simulation-wizard version="1.0"> <merge src="simwiz://Tasks/InsertGeometry.xml" /> <merge src="simwiz://Tasks/VerifyLengthUnit.xml" /> <merge src="simwiz://Tasks/DefineSheetThickness.xml" /> <merge src="simwiz://Tasks/AssignMaterial.xml" /> <merge src="Insert100psi.xml" /> <merge src="simwiz://Tasks/InsertDisplacementLoad.xml" /> <merge src="simwiz://Tasks/ThermalStressNote.xml" /> <merge src="simwiz://Tasks/InsertStructuralResults.xml" /> <merge src="simwiz://Tasks/StressStiffeningNote.xml" /> <merge src="simwiz://Tasks/Solve.xml" /> <merge src="simwiz://Tasks/ViewResults.xml" /> <merge src="simwiz://Tasks/ViewReport.xml" /> <merge src="simwiz://Tasks/StandardTasks.xml"/> <strings> <language xml:lang="en-us"> <string id="Title_Caption"> Tutorial Wizard </string> <string id="Title_Description"> Demonstrates a custom wizard with a task for inserting a 100 psi Pressure. </string> <string id="Search_Caption"> Search the Web </string> </language> </strings> <body> <group id="Title"> <taskref task="ChooseWizard"/> </group> <group id="RequiredSteps" emphasize="yes"> <taskref task="InsertGeometry"/> <taskref task="VerifyLengthUnit"/> <taskref task="DefineSheetThickness"/> <taskref task="AssignMaterial"/> <taskref task="Insert100psi"/> <taskref task="InsertDisplacementLoad"/> <taskref task="ThermalStressNote"/> <taskref task="InsertStructuralResults"/> <taskref task="StressStiffeningNote"/> <taskref task="Solve"/> <taskref task="ViewResults"/> <taskref task="ViewReport"/> </group> <group id="Standard_OptionalTasks" /> <group id="Standard_ParameterTasks" /> <group id="Standard_GeneralTasks" /> <group id="Standard_AdvancedTasks" /> <group id="Standard_Links" /> <group id="Search" collapsed="yes"> <iframe src="simwiz://Search.htm" /> </group> </body> </simulation-wizard> Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1181 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics Wizard Development Kit (WDK) Groups • WDK: Tools Group (p. 1182) • WDK: Commands Group (p. 1182) • WDK Tests: Actions (p. 1183) • WDK Tests: Flags (Conditions) (p. 1184) WDK: Tools Group The WDK: Tools group provides interactive access to the functionality of several of the most important TaskML elements and exposes some key internal data. The group also demonstrates how IFRAMEs allow arbitrary customization of the user interface. The WDK: Tools group updates automatically when the selection in the Outline changes. Level Testing The Outline Level section exercises the functionality of the level (p. 1154) element. Object Testing and Selection The second section exercises the functionality of the object (p. 1155), select-first-object (p. 1163) and selectall-objects (p. 1161) elements. Expert users may find this section useful for automating selection in the Outline. For example, typing "prt" under Name Regular Expression and clicking Select All Matching Objects selects all Outline objects with "prt" in their name. Details Field String ID The third section exposes the string ID of the currently selected Details field for use with the selectfield (p. 1162) element. Preview Event Code Advanced. If checked, displays a message box containing virtual JScript event code prior to its evaluation. Used for low-level debugging of task rules. Folder Displays the folder from which the Mechanical Wizard is currently running. Corresponds to "Mechanical Wizard URL" in the Control Panel. WDK: Commands Group The Commands group exposes options for viewing internal data and for manipulating the system. Reload Sim Wizard Reloads the HTML page containing the Mechanical Wizard. The system is reset and the Startup panel displayed. Open Wizard 1182 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Wizard Development Kit (WDK) Groups Displays an Open dialog to choose a TaskML file to load. Same as selecting the "browse" option from "Choose Wizard" on the Startup panel or in wizards. Fire Update Event Forces an update-event (p. 1148) to occur in the Mechanical Wizard. View Current Toolbar Keys Displays a temporary XML file containing the toolbar and button keys for the current state of the user interface. Toolbar and button keys are used to define the click-button (p. 1157) and display-toolbar-callout (p. 1160) elements. View Wizard XML Displays a temporary XML file containing the internal merged TaskML. Remove Merge Information Removes merge tracking information from the internal TaskML. Snapshot Wizard DHTML Saves an HTML file snapshot of the current Mechanical Wizard. The HTML snapshot is useful for developing CSS skins. Clear UserData Clears the Mechanical Wizard UserData store. The UserData store consists of Tip of the Day, group expansion, and other non-critical data. WDK Tests: Actions The Actions group exercises actions used to define task rules. Actions • display-outline-callout (p. 1158) • display-details-callout (p. 1157) • display-task-callout (p. 1160) • display-toolbar-callout (p. 1160) • display-tab-callout (p. 1159) • display-status-callout (p. 1159) • send-mail (p. 1165) • open-url (p. 1161) • display-help-topic (p. 1158) • select-zero-thickness-sheets (p. 1165) • select-first-undefined-field (p. 1164) • select-first-parameter-field (p. 1164) • select-enclosures (p. 1165) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1183 Appendix D. Workbench Mechanical Wizard Advanced Programming Topics WDK Tests: Flags (Conditions) The Flags group exercises conditions used to define task rules. Flags (Conditions) • changeable-length-unit (p. 1154) • assembly-geometry (p. 1153) • geometry-includes-sheets (p. 1154) • zero-thickness-sheet (p. 1156) • valid-emag-geometry (p. 1156) • enclosure-exists (p. 1156) 1184 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Appendix E. Material Models Used in Explicit Dynamics Analysis This appendix discusses the following: Introduction Explicit Material Library Density Linear Elastic Test Data Hyperelasticity Plasticity Brittle/Granular Equations of State Porosity Failure Strength Thermal Specific Heat Rigid Materials Introduction In general, materials have a complex response to dynamic loading and the following phenomena may need to be modeled. • Non-linear pressure response • Strain hardening • Strain rate hardening • Pressure hardening • Thermal softening • Compaction (e.g., porous materials) • Orthotropic response (e.g., composites) • Crushing damage (e.g., ceramics, glass, concrete) • Chemical energy deposition (e.g., explosives) • Tensile failure • Phase changes (i.e., solid-liquid-gas) The modeling of such phenomena can generally be broken down into three components: Equation of State An equation of state describes the hydrodynamic response of a material. This is the primary response for gases and liquids, which can sustain no shear. Their response to dynamic loading is assumed hydrodynamic, with pressure varying as a function of density and internal energy. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1185 Appendix E. Material Models Used in Explicit Dynamics Analysis This is also the primary response for solids at high deformation rates, when the hydrodynamic pressure is far greater than the yield stress of the material. Material Strength Model Solid materials may initially respond elastically, but under highly dynamic loadings, they can reach stress states that exceed their yield stress and deform plastically. Material strength laws describe this nonlinear elastic-plastic response. Material Failure Model Solids usually fail under extreme loading conditions, resulting in crushed or cracked material. Material failure models simulate the various ways in which materials fail. Liquids will also fail in tension, a phenomenon usually referred to as cavitation. Engineering Data properties for explicit analysis in the Mechanical application cover a wide range of materials and material behaviors. Some examples are provided below: Class of Material Material Effects Metals Elasticity Shock Effects Plasticity Isotropic Strain Hardening Kinematic Strain Hardening Isotropic Strain Rate Hardening Isotropic Thermal Softening Ductile Fracture Brittle Fracture (Fracture Energy based) Dynamic Failure (Spall) Concrete/Rock Elasticity Shock Effects Porous Compaction Plasticity Strain Hardening Strain Rate Hardening in Compression Strain Rate Hardening in Tension Pressure Dependent Plasticity 1186 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Explicit Material Library Class of Material Material Effects Lode Angle Dependent Plasticity Shear Damage/Fracture Tensile Damage/Fracture Solid/Sand Elasticity Shock Effects Porous Compaction Plasticity Pressure Dependent Plasticity Shear Damage/Fracture Tensile Damage/Fracture Rubbers/Polymers Elasticity Viscoelasticity Hyperelasticity Orthotropic Orthotropic Elasticity The Engineering Data properties supported by explicit analysis are described below. Please note that additional material modeling options, particularly in the areas of composite materials and reactive materials, are available in the ANSYS AUTODYN product. Explicit Material Library An extensive set of material data is provided in the Engineering Data Explicit library. We strongly recommend that you review the material data before using it in production applications. In particular, some of the materials only contain a partial definition of the material. This data may need to be complemented with additional properties to give the full definition required for the simulation. Explicit Material Library PlasticsADIPRENE LUCITE NEOPRENE POLYCARB POLYRUBBER POLYRUBBERH Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1187 Appendix E. Material Models Used in Explicit Dynamics Analysis POLYSTYRENE RUBBER1 RUBBER2 RUBBER3 EPOXY RES EPOXY RES2 PHENOXY PLEXIGLAS POLYURETH NYLONS POLYETHYL TEFLON TEFLONH Sand/ConcreteCONC 140MPA CONC 35 MPA CONCRETEL INCENDPOWD PERICLASE SAND Mineral/ElementANTIMONY BARIUM BISMUTH CALCIUM GERMANIUM POTASSIUM QUARTZ SODIUM CHLORIDE 1188 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Explicit Material Library SODIUM SULFUR VANADIUM VANADIUM2 Glass/CeramicsBORON CARBIDE FLOATGLASB FLOATGLASS LiquidParafin WATER WATER2 WATER3 Metals/AlloysAL 1100–O AL 2024 AL 2024–T4 AL 6061–T6 AL 7039 AL 7075–T6 AL 921–T AL 2024T351 AL 203–99.5 AL 203–99.7 AL203 CERA AL5083H116 ALUMINUM BERYLLIUM BERYLLIUM2 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1189 Appendix E. Material Models Used in Explicit Dynamics Analysis BRASS CADMIUM CART BRASS CHROMIUM COBALT COPPER COPPER2 CU OFHC CU OFHC CU OFHC2 CU-OFHC-F DU-.75TI GOLD GOLD 5%CU GOLD2 HAFNIUM HAFNIUM–2 INDIUM IRIDIUM IRON IRON-ARMCO IRON-ARMCO2 IRON-C.E. LEAD LEAD2 LEAD3 LITHIUIM LITHIUM F LITH-MAGN 1190 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Explicit Material Library MAG AZ-31B MAGNESIUM MAGNESIUM2 MERCURY MOLYBDENUM NICKEL NICKEL ALL NICKEL Z NICKEL-200 NICKEL 3 NIOBIUM NIOBIUM AL NIOBIUM 2 PALLADIUM PLATE 20% IR PLATINUM PLATINUM2 RHA RHENIUM RHODIUM RUBIDIUM SILVER SILVER2 SIS 2541–3 SS 21–6–9 SS 304 SS-304 STEEL 1006 STEEL 4340 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1191 Appendix E. Material Models Used in Explicit Dynamics Analysis STEEL S-7 STEEL V250 STNL. STEEL STRONTIUM TANT 10%W TANTALUM TANTALLUM2 TANTALLUM3 THALLIUM THORIUM THORIUM2 TI 6% AL 4% V TIN TIN2 TITANIUM TITANIUM2 TITANIUM-2 TUNG.ALLOY TUNGSTEN TUNGSTEN2 TUNGSTEN3 U 0.75% TI U 5% MO U 8% NB3 %ZR U – 0.75% TI U3 WT %MD URANIUM URANIUM2 URANIUM3 1192 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Linear Elastic W 4% Ni 2%FE ZINC ZIRCONIUM ZIRCONIUM2 Density Density is the initial mass per unit volume of a material at time = 0.0. Note The temperature dependence of the linear elastic properties is not available for explicit dynamics systems. Only a single value can be used. The first defined values in temperature dependent data will be used in the solver. Linear Elastic • Young's Modulus • Poisson's Ratio Note The temperature dependence of the linear elastic properties is not available for explicit dynamics systems. Only a single value can be used. The first defined values in temperature dependent data will be used in the solver. Isotropic Elasticity Define isotropic linear elastic material behavior by specifying • Young's Modulus • Poisson's ratio Note The temperature dependence of the linear elastic properties is not available for explicit dynamics systems. Only a single value can be used. The first defined values in temperature dependent data will be used in the solver. Orthotropic Elasticity Define orthotropic linear elastic material behavior by specifying: • Young's Modulus in direction X • Young's Modulus in direction Y • Young's Modulus in direction Z Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1193 Appendix E. Material Models Used in Explicit Dynamics Analysis • Poisson's ratio XY • Poisson's ratio YZ • Poisson's ratio XZ • Shear Modulus XY • Shear Modulus YZ • Shear Modulus XZ Note The coordinate system X, Y, Z relates to the local coordinate system assigned to the body. This material can only be applied to solid bodies. Viscoelastic To represent strain rate dependent elastic behavior, a linear viscoelastic model can be used. The long term behavior of the model is described by the long term or elastic shear modulus G∞. Viscoelastic behavior is introduced via an instantaneous shear modulus 0 and a viscoelastic decay constant β . The viscoelastic deviatoric stress at time increment n+1 is calculated from the viscoelastic stress at time increment n and the deviatoric strain increments at time increment n via σ′v,n+1 = σ′v,n − β∆t + (
− ∞ ) (− − β∆t β ) ∆ε′n ∆ n where ∞ is the long term shear modulus of the material  is the instantaneous shear modulus of the material. This value is derived from linear elastic properties or defined directly using the equation of state, shear modulus property β is the viscoelastic decay constant The deviatoric viscoelastic stress is added to the elastic stress to give the total stress at the end of each cycle. Note The model must be combined with either the linear elastic property or an equation of state property (including shear modulus). The model can only be applied to solid bodies. Table E.1 Input Data Name Instantaneous Shear Modulus (High rate) 1194 Symbol  Units Notes Stress Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Hyperelasticity Name Symbol Units Viscoelastic Decay Constant β 1/ time Notes Custom results variables available for this model. Name Description Solids Shells Beams VTXX Viscoelastic stress XX Yes No No VTYY Viscoelastic stress YY Yes No No VTZZ Viscoelastic stress ZZ Yes No No VTXY Viscoelastic stress XY Yes No No VTYZ Viscoelastic stress YZ Yes No No VTZX Viscoelastic stress ZX Yes No No Test Data Uniaxial Test Data Biaxial Test Data Shear Test Data Volumetric Test Data Hyperelasticity Following are several forms of strain energy potential (Ψ) provided for the simulation of nearly incompressible hyperelastic materials. The different models are generally applicable over different ranges of strain as illustrated in the table below, however these numbers are not definitive and users should verify the applicability of the model chosen prior to use. Currently hyperelastic materials may only be used in solid elements for explicit dynamics simulations. Model Applied Strain Range Neo-Hookean 30% Mooney-Rivlin 30%-200% depending on order Polynomial Ogden Up to 700% Neo-Hookean The strain energy function for the Neo-Hookean hyperelastic model is, ψ= µ 2 (l1 - )+ d (J − ) where is the deviatoric first principal invariant, J is the Jacobian and the required input parameters are defined as: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1195 Appendix E. Material Models Used in Explicit Dynamics Analysis µ = initial shear modulus of the material d= incompressibility parameter. and the initial bulk modulus is defined as: K = 2/d Mooney-Rivlin The strain energy function of a hyperelastic material can be expanded as an infinite series in terms of the first and second deviatoric principal invariants m ∞ n ψ = ∑ Cmn (l1 − ) (l2 − ) + mn −0 d and , as follows, 2 (J − ) The 2, 3, 5 and 9 parameter Mooney-Rivlin hyperelastic material models have been implemented and are described in turn below. 2–Parameter Mooney-Rivlin Model The strain energy function for the 2–parameter model is, ψ
 ( − )+
 ( − )+  ( − ) where: C10, C01 = material constants d = material incompressibility parameter. The initial shear modulus is defined as: µ= ( + ) and the initial bulk modulus is defined as: K = 2/d 3–Parameter Mooney-Rivlin Model The strain energy function for the 3–parameter model is, ψ  ( − )+  ( − )+  ( − )( − )+   ( − ) where the required input parameters are defined as: C10, C01,C11 = material constants d = material incompressibility parameter 1196 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Hyperelasticity The bulk and shear modulus are as defined for the 2–parameter Mooney-Rivlin model. 5–Parameter Mooney-Rivlin Model The strain energy function for the 5–parameter model is,   ψ =C10 (l − )+ C
(l − )+ C11 (l − )(l − )+ C
(l − ) + C02 (l − ) +  d (J − ) where the required input parameters are defined as: C10,C01,C20,C11,C02 = material constants d = material incompressibility parameter. The bulk and shear modulus are as defined for the 2–parameter Mooney-Rivlin model. 9–Parameter Mooney-Rivlin Model The strain energy function for the 9–parameter hyperelastic model is, ψ  ( − )+  ( − )+  ( − )( − ) + ( − ) +  ( − ) +  ( − ) ( − ) 3 3 + ( − )( − ) +   ( − ) +  ( − ) + ( − ) where the required input parameters are defined as: C10,C01,C20,C11, C02, C30, C21, C12,C03 = material constants d = material incompressibility parameter. The bulk and shear modulus are as defined for the 2–parameter Mooney-Rivlin model. Polynomial The strain energy function of a hyperelastic material can be expanded as an infinite series of the first and second deviatoric principal invariants l1 and l2. The polynomial form of strain energy function is given below: ψ = N ∑ mn (I m ,n = m n N − ) (I − ) + ∑ k =  k k ( − ) 1st, 2nd, and 3rd order polynomial hyperelastic material models have been implemented in the solver where N is 1, 2 or 3 respectively. Cmn = material constants dk = material incompressibility parameters. The initial shear modulus is defined as: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1197 Appendix E. Material Models Used in Explicit Dynamics Analysis µ = (C10 + C01 ) and the initial bulk modulus is defined as: K = 2/d1 Yeoh The Yeoh hyperelastic strain energy function is similar to the Mooney-Rivlin models described above except that it is only based on the first deviatoric strain invariant. It has the general form, N i N 2i I − + ∑ (J − ) ( )

i −
i −
di ψ =∑ Yeoh 1st order The strain energy function for the first order Yeoh model is, ψ =  ( − )+ −  ( ) where: N=1 C10 = material constant d1 = incompressibility parameter The initial shear modulus is defined as: µ = 2c10 and the initial bulk modulus is defined as: K = 2/d1 Yeoh 2nd order The strain energy function for the second order Yeoh hyperelastic model is ψ =  (  − )+  (  −  ) +   ( − ) +  4 ( − ) where the required input parameters are defined as: N = 2. C10, C20 = material constants d1, d2 = incompressibility parameters See 1st order Yeoh model for definitions of the initial shear and bulk modulus. 1198 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Hyperelasticity Yeoh 3rd order The strain energy function for the third order Yeoh hyperelastic model is, 2 3 ψ = C10 (I1 − )+ C20 (I1 − ) + C30 (I1 − ) + d1 2 (J − ) + d2 4 (J − ) + d3 6 (J − ) where the required input parameters are defined as: N = 3. C10, C20, C30 = material constants d1, d2, d3 = incompressibility parameters See 1st order Yeoh model for definitions of the initial shear and bulk modulus. Ogden The Ogden form of the strain energy function is based on the deviatoric principal stretches of the leftCauchy-Green tensor and has the form, µ  α α α ψ = i (λ l + λ  + λ  − )+ (
− ) αi i Ogden 1st Order The strain energy function for the first order Ogden hyperelastic model is, where: λ p = deviatoric principal stretches of the left-Cauchy-Green tensor J = determinant of the elastic deformation gradient µp, αp and dp = material constants The initial shear modulus is given as: µ = (µα ) and the initial bulk modulus is: K =  Ogden 2nd order The strain energy function for the first order Ogden hyperelastic model is, Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1199 Appendix E. Material Models Used in Explicit Dynamics Analysis ψ = µ2 α z µ1 α α α α α (λ1 + λ2 + λ2 − )+ (λ1 + λ2 z + λ2 z − ) α2 α1 + (J − ) + 2 d 1 4 (J − ) d 2 where: λ p= deviatoric principal stretches of the left-Cauchy-Green tensor J = determinant of the elastic deformation gradient µp, αp and dp = material constants The initial shear modulus is given as: µ0 = (µ
α
) and the initial bulk modulus is: K  =   Ogden 3rd order The strain energy function for the first order Ogden hyperelastic model is, ψ = + µ α µ α α α α α (λ + λ  + λ  − )+ (λ + λ + λ − ) α α µ3 α  α α (λ + λ  + λ  − )+ α3  ( − ) +  ( − )  6 + ( − ) 3 where: λ p= deviatoric principal stretches of the left-Cauchy-Green tensor J = determinant of the elastic deformation gradient µp, αp and dp = material constants The initial shear modulus is given as: µ = (µα + µα  + µα  ) and the initial bulk modulus is: 1200 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Plasticity K0 = d1 Plasticity All stress-strain input should be in terms of true stress and true (or logarithmic) strain and result in all output as also true stress and true strain. For small-strain regions of response, true stress-strain and engineering stress-strain are approximately equal. If your stress-strain data is in the form of engineering stress and engineering strain you can convert: • strain from engineering strain to logarithmic strain using: • engineering stress to true stress using: σ tru σ
 ( ln
 ( eng ) ) Note This stress conversion is only valid for incompressible materials. The following Plasticity models are discussed in this section: Bilinear Isotropic Hardening Multilinear Isotropic Hardening Bilinear Kinematic Hardening Multilinear Kinematic Hardening Johnson-Cook Strength Cowper-Symonds Strength Steinberg-Guinan Strength Zerilli-Armstrong Strength Bilinear Isotropic Hardening This plasticity material model is often used in large strain analyses. A bilinear stress-strain curve requires that you input the Yield Strength and Tangent Modulus. The slope of the first segment in the curve is equivalent to the Young's modulus of the material while the slope of the second segment is the tangent modulus. Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes Yes* Yes* SUBL_EPS Effective sublayer plastic strain No Yes No *Resultant value over shell/beam section. Multilinear Isotropic Hardening This plasticity material model is often used in large strain analyses. Do not use this model for cyclic or highly nonproportional load histories in small-strain analyses. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1201 Appendix E. Material Models Used in Explicit Dynamics Analysis You must supply the data in the form of plastic strain vs. stress. The first point of the curve must be the yield point, that is, zero plastic strain and yield stress. The slope of the stress-strain curve is assumed to be zero beyond the last user-defined stress-strain data point. No segment of the curve can have a slope of less than zero. Note You can define up to 10 stress strain pairs using this model in explicit dynamics systems. Temperature dependence of the curves is not directly supported. Temperature dependent plasticity can be represented using the Johnson-Cook plasticity model. Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes Yes* Yes* SUBL_EPS Effective sublayer plastic strain No Yes No *Resultant value over shell/beam section. Bilinear Kinematic Hardening This plasticity material model assumes that the total stress range is equal to twice the yield stress, to include the Bauschinger effect. This model may be used for materials that obey Von Mises yield criteria (includes most metals). The tangent modulus cannot be less than zero or greater than the elastic modulus. Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes Yes* Yes* SUBL_EPS Effective sublayer plastic strain No Yes No *Resultant value over shell/beam section. Multilinear Kinematic Hardening This plasticity model simulates metal plasticity behavior under cyclic loading. You must supply the data in the form of plastic strain vs. stress. The first point of the curve must be the yield point, that is, zero plastic strain and yield stress. No segment can have a slope of less than zero. The slope of the stressstrain curve is assumed to be zero beyond the last user-defined stress-strain data point. No segment of the curve can have a slope of less than zero. Note You can define up to 10 stress strain pairs using this model in explicit dynamics systems. Temperature dependence of the curves is not directly supported. Temperature dependent plasticity can be represented using the Johnson-Cook plasticity model. This model is available for solid elements in explicit dynamics systems. 1202 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Plasticity Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes No No SUBL_EPS Effective sub layer plastic strain No No No Note This material property can only be applied to solid bodies. Johnson-Cook Strength Use this model to represent the strength behavior of materials, typically metals, subjected to large strains, high strain rates and high temperatures. Such behavior might arise in problems of intense impulsive loading due to high velocity impact. With this model, the yield stress varies depending on strain, strain rate and temperature. The model defines the yield stress Y as Y =  A + Bε pn   + C ε p∗   − THm  where ε ε
= effective plastic strain * = normalized effective plastic strain rate TH = homologous temperature = (T-Troom)/(Tmelt -Troom) The five material constants are A, B, C, n and m. ε  The expression in the first set of brackets gives the stress as a function of strain when  = 1.0 sec-1 and TH = 0 (i.e. for laboratory experiments at room temperature). The constant A is the basic yield stress at low strains while B and n represent the effect of strain hardening. The expressions in the second set of brackets represent the effects of strain rate on the yield strength of the material. The reference strain rate against which the material data was measured is used to normalize the plastic strain rate enhancement. 1.0/second is used by default. The expression in the third set of brackets represents thermal softening such that the yield stress drops to zero at the melting temperature Tmelt. The plastic flow algorithm used in this model has an option to reduce high frequency oscillations that are sometimes observed in the yield surface under high strain rates. A first order rate correction is applied by default. The Johnson-Cook strength model can be used in all element types and in combination with all equations of state and failure properties. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1203 Appendix E. Material Models Used in Explicit Dynamics Analysis Note A specific heat capacity property should be defined to enable the calculation of temperature hence thermal softening effects. Table E.2 Input Data Name Symbol Units Initial Yield Stress A Stress Hardening Constant B Stress Hardening Exponent n None Strain Rate Constant C None Thermal Softening Exponent m None Melting Temperature Tmelt Temperature Reference Strain Rate Notes None Units fixed at 1/sec Default = 1.0 Strain Rate Correction None Option List: None 1st Order (Default) Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes Yes* Yes* EFF_PL_STN_RATE Effective Plastic Strain Rate Yes Yes* Yes* TEMP Temperature** Yes Yes* Yes* SUBL_EPS Effective sublayer plastic strain No Yes No *Resultant value over shell/beam section. **Temperature will be non-zero only if a specific heat capacity is defined. Cowper-Symonds Strength The Cowper-Symonds strength model lets you define the yield strength of isotropic strain hardening, strain rate dependent materials. The yield surface is defined as Y = n (A + Bε pl   εɺ  1q  pl ) +     D     where A is yield stress at zero plastic strain 1204 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Plasticity B is the strain hardening coefficient n is the strain hardening exponent D and q are the strain rate hardening coefficients ɺ It should be noted that, in the implementation within the AUTODYN solver, the plastic strain rate (
) used in the Cowper Symonds model has a minimum value of unity to allow for compatibility with the linear strain rate correction method. The consequence of this is that for plastic strain rates less then unity, the material will exhibit a strain rate hardening effect equal to that for a strain rate of unity. The plastic flow algorithm used in this model has an option to reduce high frequency oscillations that are sometimes observed in the yield surface under high strain rates. A first order rate correction is applied by default. Note that the strain rate constants should be input assuming that the units of strain rate are 1/second. The Cowper-Symonds strength model can be used in all element types and in combination with all equations of state and failure properties. Name Symbol Units Initial Yield Stress A Stress Hardening Constant B Stress Hardening Exponent n None Strain Rate Constant D None Strain Rate Constant q None Strain Rate Correction - None Notes Assumed 1/second in all cases Option List: None 1st Order (Default) Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes Yes* Yes* EFF_PL_STN_RATE Effective Plastic Strain Rate Yes Yes* Yes* SUBL_EPS Effective sublayer plastic strain No Yes No *Resultant value over shell/beam section. Steinberg-Guinan Strength In this formulation the authors have assumed that while yield stress initially increases with strain rate, experimental data on shock-induced free surface velocity versus time records indicate that at high strain rates (greater than 105sec-1) strain rate effects become insignificant compared to other effects and that the yield stress reaches a maximum value which is subsequently strain rate independent. They have also postulated that the shear modulus increases with increasing pressure and decreases with increasing temperature and in doing this they have attempted to include modeling of the Bauschinger effect into their calculations. They have therefore produced expressions for the shear Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1205 Appendix E. Material Models Used in Explicit Dynamics Analysis modulus and yield strength as functions of effective plastic strain, pressure and internal energy (temperature). The constitutive relations for shear modulus G and yield stress Y for high strain rates are :   G' G = G0  +     G0 Y   Y   P 
  = Y  +     +  τ  ( −   Y  η  
  subject to   )   p  Gt'   1 / 3 +   (T −  G0  η  ) (  + βε )n [ +βε ] ≤ max where ε = effective plastic strain T = temperature (degrees K) η = compression = ν0/ ν and the primed parameters with the subscripts p and T are derivatives of that parameter with respect to pressure and temperature at the reference state (T = 300 K, p= 0, ε = 0). The subscript zero also refers to values of G and Y at the reference state. If the temperature of the material exceeds the specified melting temperature the shear modulus and yield strength are set to zero. Note A specific heat capacity property should be defined to enable the calculation of temperature hence the melting effect. Table E.3 Input Data Name Symbol Units Initial Yield Stress Y Stress Maximum Yield Stress Ymax Stress Hardening Constant β None Hardening Exponent n None Derivative dG/dP G'P None Derivative dG/dT G'T Stress/Temperature Derivative dY/dP Y'P None Melting Temperature Tmelt Temperature Notes Custom results variables available for this model: 1206 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Plasticity Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes Yes* Yes* EFF_PL_STN_RATE Effective Plastic Strain Rate Yes Yes* Yes* TEMP Temperature** Yes Yes* Yes* SUBL_EPS Effective sublayer plastic strain No Yes No *Resultant value over shell/beam section. **Temperature will be non-zero only if a specific heat capacity is defined. Zerilli-Armstrong Strength While the Johnson-Cook model predicted the behavior of most materials in the Taylor tests, the model's prediction and test results for OFHC (oxygen free high conductivity) copper did not agree well. In an approach seeking to improve on Johnson-Cook, Zerilli and Armstrong proposed a more sophisticated constitutive relation obtained through the use of dislocation dynamics. The effects of strain hardening, strain-rate hardening and thermal softening (based on thermal activation analysis) have been incorporated into the formulation. The effect of grain size has also been included. The relation has a relatively simple expression and should be applicable to a wide range of fcc (face centered cubic) materials. A relation for iron has also been developed and is also applicable to other bcc (body centered cubic) materials. An important point made by Zerilli and Armstrong is that each material structure type (fcc, bcc, hcp) will have its own constitutive behavior, dependent on the dislocation characteristics for that particular structure. For example, a stronger dependence of the plastic yield stress on temperature and strain rate is known to result for bcc metals as compared with fcc metals. With this model, the yield stress varies depending on strain, strain rate and temperature. The yield stress is given by: For fcc metals Y = Y0 + C2 ε [−C3T + C4T εɺ ] For bcc metals: =  +
1 [−
 +
 εɺ ] +
5ε n where ε = effective plastic strain = normalized effective plastic strain rate T = temperature (degrees K) The parameters Y0, C1, C2, C3, C4, C5 and n are material constants. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1207 Appendix E. Material Models Used in Explicit Dynamics Analysis Note A specific heat capacity property should be defined to enable the calculation of temperature hence the melting effect. Table E.4 Input Data Name Symbol Units Initial Yield Stress Y0 Stress Hardening Constant #1 C1 Stress Hardening Constant #2 C2 Stress Hardening Constant #3 C3 None Hardening Constant #4 C4 None Hardening Constant #5 C5 Stress Hardening Constant n n None Reference Strain Rate Notes None Units fixed at 1/sec Default = 1.0 Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes Yes* Yes* EFF_PL_STN_RATE Effective Plastic Strain Rate Yes Yes* Yes* TEMP Temperature** Yes Yes* Yes* SUBL_EPS Effective sublayer plastic strain No Yes No *Resultant value over shell/beam section. **Temperature will be non-zero only if a specific heat capacity is defined. Brittle/Granular A number of properties are available to allow modeling of brittle/granular materials such as concrete, rock, soil, glass and ceramics. Drucker-Prager Strength Linear Drucker-Prager Strength Stassi Drucker-Prager Strength Piecewise Johnson-Holmquist Strength Continuous Johnson-Holmquist Strength Segmented RHT Concrete Strength MO Granular Drucker-Prager Strength Linear This model is used to represent the behavior of dry soils, rocks, concrete and ceramics where the cohesion and compaction behavior of the materials result in an increasing resistance to shear up to a limiting 1208 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Brittle/Granular value of yield strength as the loading increases. The yield strength of these materials is highly dependent on pressure. There are three forms available for this model; linear, stassi and piecewise. Although the yield stress is pressure dependent in each case, the flow rule is volume independent, i.e., a Prandtl-Reuss type. Figure: Drucker-Prager Strength Linear Y P The yield stress is a linear function of pressure (the original Drucker-Prager model) Note This property can only be applied to solid bodies. Table E.5 Input Data Name Symbol Yield Stress (at zero pressure) Units Notes Stress Θ Slope (degrees) None Slope in degrees Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes No No Pressure Material Pressure Yes No No Note This material property can only be applied to solid bodies. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1209 Appendix E. Material Models Used in Explicit Dynamics Analysis Drucker-Prager Strength Stassi Figure: Drucker-Prager Strength Stassi Y P The Stassi yield condition takes the form: J2 = Y0 kY0 + 3 (k − 1) p  3  where J2Y is the second invariant of the deviatoric stress yield Y0 is the yield strength in simple tension k is the ratio between the yield strengths in compression and tension p is the pressure Note This property can only be applied to solid bodies. Table E.6 Input Data Name Symbol Units Notes Yield Stress Uniaxial Tension Y0 Stress Measure under uniaxial stress conditions Stress Measure under uniaxial stress conditions Yield Stress Uniaxial Compression Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes No No Pressure Pressure Yes No No 1210 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Brittle/Granular Drucker-Prager Strength Piecewise Figure: Drucker-Prager Strength Piecewise Yield stress Y varies with pressure as a piecewise linear function. Constant shear modulus G Yield Stress Y Ymax Piecewise Linear Pressure P The yield stress is a piecewise linear function of pressure. In tension (negative values of pressure), such materials have little tensile strength and this is modeled by dropping the yield stress rapidly to zero as pressure goes negative to give a realistic value for the limited tensile strength. Note You can use up to 10 pressure-yield points to define the material strength curve. This property can only be applied to solid bodies. Table E.7 Input Data Name Symbol Units Yield Stress vs Pressure Y vs P Stress Notes Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes No No Pressure Material Pressure Yes No No Johnson-Holmquist Strength Continuous This model is used for modeling brittle materials such as glass and ceramics (Johnson & Holmquist 1993)1 subjected to large pressures, shear strain and high strain rates. Two forms of this model are found in the literature and are available in explicit dynamics systems; continuous (JH2), segmented (JH1). Both these forms can be used with a linear or energy dependent polynomial equation of state. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1211 Appendix E. Material Models Used in Explicit Dynamics Analysis The strength of the brittle material is described as a smoothly varying function of intact strength, fractured strength, strain rate and damage via a dimensionless analytic function as described below. P* is the pressure normalized by the pressure at the Hugoniot Elastic Limit (PHELL) and T* is the maximum tensile hydrostatic pressure normalized by PHELL. Yield Stress, Y Figure: Johnson-Holmquist Strength Model Pressure, P (1 = C ln ε ) Damage (0<D<1.0) D Fractured (D=1.0) = MIN B [( m (1 C ln ) ] As the material undergoes inelastic deformation, damage is assumed to accumulate which degrades the overall load carrying capacity of the materials. The Johnson-Holmquist Damage model was developed for the simulation of the compressive and shear induced strength and failure of brittle materials. Damage is accumulated as the ratio of incremental plastic strain over the current estimated fracture strain. The effective fracture strain is pressure dependent as described below. 1212 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Brittle/Granular Figure: Johnson-Holmquist Damage Model There are two methods for the application of damage to the material strength. The default Gradual failure type results in damage being incrementally applied to the material strength as it accumulates. If the Instantaneous failure type is selected, damage accumulates over time, however it is only applied to the failure surface when its value reaches unity. The material strength instantaneously transitions from intact to fully failed in this case. The model includes an option to represent volumetric dilation of the material due to shear deformation (Bulking). The work done in deforming the material inelastically in shear can be converted into a pressure increase, hence volumetric dilation (if unconstrained). The amount of work which is converted into dilation pressure is controlled through the Bulking constant, B. This can have values ranging from 0.0 (representing no shear induced dilatancy) to 1.0 (producing maximum dilatancy effects). Note If the Bulking constant, B is greater than zero then the Johnson-Holmquist model should be used in conjunction with a polynomial equation of state or linear elasticity. This property can only be applied to solid bodies. Table E.8 Input Data Name Symbol Units Notes Hugoniot Elastic Limit σHEL Stress Elastic limit under dynamic compressive uniaxial strain conditions Intact Strength Constant A A None Intact Strength Exponent n n None Strain Rate Constant C C None Fracture Strength Constant B B None Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1213 Appendix E. Material Models Used in Explicit Dynamics Analysis Name Symbol Units Fracture Strength Exponent m m None Maximum Fracture Strength Ratio σF Max None Damage Constant D1 D1 None Damage Constant D2 D2 None Bulking Constant B None Hydrodynamic Tensile Limit T Stress Notes Maximum fracture strength as fraction of intact strength Failure Type Option list: Gradual (Default) Instantaneous Custom results variables available for this model: Name Description Solids Shells Beams EFF_Pl_STN Effective Plastic Strain Yes No No EFF_Pl_STN_RATE Effective Plastic Strain Rate Yes No No PRESSURE Pressure Yes No No DAMAGE Damage Yes No No STATUS Material Status** Yes No No PRES_BULK Dilation pressure Yes No No ENERGY_DAM Damage energy contributing to bulking Yes No No **Material status indicators (1= elastic, 2= plastic, 3 = bulk failure, 4 = bulk failure, 5 = failed principal direction 1, 6 = failed principal direction 2, 7 = failed direction 3) 1 Johnson-Holmquist Strength Segmented Recent studies (Holmquist and Johnson 2002) have showed that gradual softening in the JH2 model has not been supported by available experimental data yet while there are some indications that an early variant of the model, known as JH1, may be more accurate. In the JH1 material model, material strength is described by linear segments and the damage is always applied instantaneously. 1 Johnson G. R. & Holmquist T. J. (1993). An Improved Computational Constitutive Model for Brittle Materials, Joint AIRA/APS Conference, Colorado Springs, Colorado, June 1993. 1214 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Brittle/Granular Intact Material (D<1.0) S2 >1.0 Failure Strain, =1.0 S1 Failed Material (D=1.0) SFMAX P3 T >1.0 Pressure, P =1.0 D=1.0 T P1 Pressure, P Equivalent Stress, σ f Figure: Johnson-Holmquist Strength Segmented P2 Pressure, P T ε max f D<1.0 Volumetric strain, µ Note If the Bulking constant, B is greater than zero then the Johnson-Holmquist model should be used in conjunction with a polynomial equation of state or linear elasticity. This property can only be applied to solid bodies. Holmquist, T.J. & Johnson, G.R. (2002). Response of silicon carbide to high velocity impact. Journal of Applied Physics, pp 5858-5866, Vol 91, No. 9, May 1, 2002. Table E.9 Input Data Name Symbol Units Notes Hugoniot Elastic Limit σHEL Stress Elastic limit under dynamic compressive uniaxial strain conditions Intact Strength Constant S1 S1 Stress Intact Strength Constant P1 1 Stress 2 Stress 2 Stress Intact Strength Constant S2 P S Intact Strength Constant P2 P Strain Rate Constant C C FMax None Maximum Fracture Strength S Stress Failed Strength Constant α None Damage Constant D1 None Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1215 Appendix E. Material Models Used in Explicit Dynamics Analysis Damage Constant D2 None Bulking Constant B None Hydrodynamic Tensile Limit T Stress Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes No No EFF_PL_STN_RATE Effective Plastic Strain Rate Yes No No PRESSURE Pressure Yes No No DAMAGE Damage Yes No No STATUS Material Status** Yes No No PRES_BULK Dilation pressure Yes No No ENERGY_DAM Damage energy contributing to bulking Yes No No **Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4 = bulk failure, 5 = failed principal direction 1, 6 = failed principal direction 2, 7 = failed principal direction 3) RHT Concrete Strength The RHT concrete model is an advanced plasticity model for brittle materials developed by Riedal et al 23 4 , , . It is particularly useful for modeling the dynamic loading of concrete. It can also be used for other brittle materials such as rock and ceramic. The RHT constitutive model is a combined plasticity and shear damage model in which the deviatoric stress in the material is limited by a generalized failure surface of the form: f (P,σ eq ,θ ,εɺ ) = σ eq − YTXC (P ) ∗ FCAP (P ) ∗ R3(θ ) ∗ (F )RATE (εɺ ) (E–1) This failure surface can be used to represent the following aspects of the response of geological materials • Pressure hardening • Strain hardening • Strain rate hardening in tension and compression • Third invariant dependence for compressive and tensile meridians • Strain softening (shear induced damage) • Coupling of damage due to porous collapse The model is modular in nature and is designed such that individual aspects of the material behavior can be turned on and off. This gives the model significant practical usefulness. Further details of how the model represents the various aspects of the material behavior are now presented. 1216 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Brittle/Granular Fracture surface The fracture surface is represented through the expression NFail * YTXC = fc'  AFail (P ∗ − Pspall FRATE )    (E–2) where fc' is the cylinder strength AFAIL, NFAIL are user defined parameters P* is pressure normalized with respect to fc' Pspall* is the normalized hydrodynamic tensile limit FRATE is a rate dependent enhancement factor Additionally, there is an option to truncate the fracture surface to fit through the characteristic points that can be observed experimentally at low pressures, while retaining the flexibility to match data at high pressures. This feature is described in the figure below. Figure: RHT Representation of Compressive Meridian Y Pure shear strength Uniaxial compressive strength Biaxial tensile strength P Tensile and Compressive Meridians The RHT model can represent the difference between the compressive and tensile meridian in terms of material strength using the third invariant dependence term (R3). This can be utilized to represent the observed reduction in strength of concrete under triaxial extension, compared with triaxial compression. The third invariant dependence term is formulated using the expression Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1217 Appendix E. Material Models Used in Explicit Dynamics Analysis R3 = 2 (1 − Q22 )cos θ + (2Q2 − 1) 4 (1 − Q22 )cos 2 θ − 4Q2 2 4 (1 − Q22 )cos 2 θ + (1 − 2Q2 ) where cos (3θ ) = (E–3) 3 3 .J3 3 2 2 J2 Q2 = Q2,0 + BQ.P * and 0.5 < Q2 < 1, BQ = 0.0105 The input parameter Q2.0 defines the ratio of strength at zero pressure and the coefficient BQ defines the rate at which the fracture surface transitions from approximately triangular in form to a circular form with increasing pressure ( Figure: Third invariant dependence (p. 1218)). Figure: Third invariant dependence Tensile meridian Q 2 = 1.0 Compressive meridian Q 2 = 0.5 Strain Hardening Strain hardening is represented in the model through the definition of an elastic limit surface and a “hardening” slope. The elastic limit surface is scaled down from the fracture surface by user defined ratios; (elastic strength/fc) and (elastic strength/ft). The pre-peak fracture surface is subsequently defined through interpolation between the elastic and fracture surfaces using the “hardening”  Gelastic  G − Gplastic slope,  elastic    . This is shown in Figure: Bi-linear strain hardening function (p. 1219) for the case of uniaxial compression. Y * = Yelastic + 1218 ε pl ε pl ( pre −softening ) (Yfail − Yelastic ) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Brittle/Granular where ε pl ( pre −softening ) = Yfail − Yel  Gelastic ∗  3G  Gelastic − Gplastic    Figure: Bi-linear strain hardening function f c’ f c’*comprat ε pl (pre-soft) ε pl Shear Damage Damage is assumed to accumulate due to inelastic deviatoric straining (shear induced cracking) using the relationships D=∑ ε failure p ε ε pl failure p (E–4) ∗ D2 ∗ spall = D1 (P − P ) where D1 and D2 are material constants used to describe the effective strain to fracture as a function of pressure. Damage accumulation can have two effects in the model • Strain softening (reduction in strength) The current fracture surface (for a given level of damage) is scaled down from the intact surface using the expression ∗ ∗ ∗ + DYresidual Yfractured = (1 − D )Yfailure (E–5) where M ∗ Yresidual = Min B (P ∗ ) ,YXTC ∗ SFMAX    (E–6) The term Y XTC*SFMAX is used to limit the maximum residual shear strength (for completely damaged material) to be a fraction (SFMAX) of the current fracture strength. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1219 Appendix E. Material Models Used in Explicit Dynamics Analysis • Reduction in shear stiffness The current shear modulus is defined through the expression Gfractured = (1 − D )Gelastic + DGresidual (E–7) Porous Collapse Damage The model includes the option to include a cap to limit the elastic deviatoric stress under large compressions. This effectively leads to the assumption that porous compaction results in a reduction in deviatoric strength. The final combination of elastic, fracture and residual failure surfaces is shown schematically below in Figure: RHT Elastic, Fracture and Residual Failure Surfaces (p. 1220). Figure: RHT Elastic, Fracture and Residual Failure Surfaces Elastic/Hardening Failure Surface Y Failure Surface Elastic Limit Surface Residual Surface P Strain Rate Effects Strain rate effects are represented through increases in fracture strength with plastic strain rate. Two different terms can be used for compression and tension with linear interpolation being used in the intermediate pressure regime. FRATE   εɺ α  1 +   for P > 1 fc (compression ) 3   εɺ 0   =  δ   εɺ   1 1 +  ɺ  for P < 3 ft (tension )    ε0   where 1220 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Brittle/Granular εɺ 0 = 3e-6 in tension and 30e-6 in compression. Tensile Failure By default, tensile failure is achieved using a hydrodynamic tensile limit. The maximum tensile pressure in the material is limited to P = max [D * Pmin , P ( ρ , e )] (E–8) Using this option, no additional user input is required since the value of Pmin is derived from ft, which forms part of the input for the strength model. Note that the principal tensile stress and crack softening failure properties may also be used in conjunction with this model. Data for concrete with cube strengths of 35MPa and 140MPa are included in the distributed material library. The model is formulated such that input can be scaled with the cube strength, fc i.e. you can retrieve one of the two concretes in the library, change its cube strength to match the concrete you want to model and the remaining terms will automatically scale proportionately. The resulting data set will be approximate and we recommend validation of the material data against experimental characterization tests in all cases. Note This property can only be applied to solid bodies. Table E.10 Input Data Name Symbol Units Compressive Strength fc Stress Tensile Strength ft/fc None Shear Strength fs/fc None Intact failure surface constant A AFAIL None Intact failure surface exponent N NFAIL None Tens./Comp. Meridian ratio Q2.0 None Brittle to Ductile Transition BQ None Hardening Slope None Elastic Strength/ft None Elastic Strength/fc None Notes Gel/(Gel-Gpl) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1221 Appendix E. Material Models Used in Explicit Dynamics Analysis Name Symbol Units Fracture Strength Constant B None Fracture Strength Exponent m None Compressive strain rate exponent α None Tensile strain rate exponent δ None Maximum fracture strength ratio SFMAX None Use cap on elastic surface Notes None Option: Yes (default) No Damage constant D1 D1 None Damage constant D2 D2 None Minimum strain to failure None Residual Shear modulus fraction None Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes No No EFF_PL_STN_RATE Effective Plastic Strain Rate Yes No No PRESSURE Pressure Yes No No DAMAGE Damage Yes No No STATUS Material Status** Yes No No **Material status indicators (1=elastic, 2= plastic, 3 = bulk failure, 4 = bulk failure, 5= failed principal direction 1, 6= failed principal direction 2, 7 = failed principal direction 3) 234 2 Riedel W., Thoma K., Hiermaier S., Schmolinske E.: Penetration of Reinforced Concrete by BETA-B-500, Numerical Analysis using a New Macroscopic Concrete Model for Hydrocodes. Proc. (CD-ROM) 9. Internationales Symposium , Interaction of the Effects of Munitions with Structures, Berlin Strausberg, 03.-07. Mai 1999, pp 315 - 322 3 W. Riedel, Beton unter dynamischen Lasten: Meso- und makromechanische Modelle und ihre Parameter, Ed.: Fraunhofer-Institut für Kurzzeitdynamik, Ernst-Mach-Institut EMI, Freiburg/Brsg., Fraunhofer IRB Verlag 2004, ISBN 3-8167-6340-5, http://www.irbdirekt.de/irbbuch/ 4 Werner Riedel, Nobuaki Kawai and Ken-ichi Kondo, Numerical Assessment for Impact Strength Measurements in Concrete Materials, International Journal of Impact Engineering 36 (2009), pp. 283-293 DOI information: 10.1016/j.ijimpeng.2007.12.012 1222 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Equations of State MO Granular This model is an extension of the Drucker-Prager model that takes into account effects associated with granular materials such as powders, soil and sand. In addition to pressure hardening, the model also represents density hardening and variations in the shear modulus with density. The yield stress is made up of two components, one dependent on the density and one dependent on the pressure, σy = σp +σρ where σy, σp and σρ denote the total yield stress, the pressure yield stress and the density yield stress respectively. The unload/reload slope is defined by the shear modulus which is defined as a function of the zero pressure density of the material. Note The yield stress is defined by a yield stress - pressure and a yield stress - density curve with up to 10 points in each curve. The shear modulus is defined by a shear modulus - density curve with up to 10 points. All three curves must be defined. This model can only be applied to solid bodies. Table E.11 Input Data Name Symbol Units Notes Yield Stress vs Pressure Stress Tabular data Yield Stress vs Density Stress and Density Tabular data Shear Modulus vs Density Stress and Density Tabular data Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes No No PRESSURE Pressure Yes No No DENSITY Density Yes No No Equations of State Background information is discussed in this section along with available EOS models: Background Bulk Modulus Shear Modulus Ideal Gas EOS Polynomial EOS Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1223 Appendix E. Material Models Used in Explicit Dynamics Analysis Shock EOS Linear Shock EOS Bilinear JWL EOS Background A general material model requires equations that relate stress to deformation and internal energy (or temperature). In most cases, the stress tensor may be separated into a uniform hydrostatic pressure (all three normal stresses equal) and a stress deviatoric tensor associated with the resistance of the material to shear distortion. Then the relation between the hydrostatic pressure, the local density (or specific volume) and local specific energy (or temperature) is known as an equation of state. Hooke's law is the simplest form of an equation of state and is implicitly assumed when you use linear elastic material properties. Hooke's law is energy independent and is only valid if the material being modeled undergoes relatively small changes in volume (less than approximately 2%). One of the alternative equation of state properties should be used if the material is expected to experience high volume changes during an analysis. Before looking at the various equations of state available, it is good to understand some of the fundamental physics behind their formulations. Details are provided in Explicit Dynamics Analysis Guide (to be published). Bulk Modulus Bulk Modulus — A bulk modulus can be used to define a linear, energy independent equation of state. Combined with a shear modulus property, this material definition is equivalent to using linear elasticity i.e., Young's Modulus and Poisson's ratio. Shear Modulus Shear Modulus — A shear modulus must be used when a solid or porous equation of state is selected to fully define the elastic stiffness of a material. To represent fluids, specify a small value. Ideal Gas EOS One of the simplest forms of equation of state is that for an ideal polytropic gas which may be used in many applications involving the motion of gases. This may be derived from the laws of Boyle and GayLussac and expressed in the form p = (γ − 1) ρ e This form of equation is known as the “Ideal Gas” equation of state and only the value of the adiabatic exponent γ needs to be supplied. In order to avoid complications with problems with multiple materials where initial small pressures in the gas would generate small unwanted velocities the equation is modified for use in these cases = (γ − 1) ρ
− Pshift where pshift is a small initial pressure defined to give a zero starting pressure. 1224 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Equations of State The definition of a non-zero adiabatic constant, c, will turn the energy dependent ideal gas equation of state into the following energy independent adiabatic equation of state p = cρ T Note This equation of state can only be applied to solid bodies. A specific heat capacity should be defined with this property to allow the calculation of temperature. Table E.12 Input Data Name Symbol Units Adiabatic exponent γ None Adiabatic constant c None Pressure shift Pshift Pressure Notes This equation of state can only be used with solid elements. Custom results variables available for this model: Name Description Solids Shells Beams PRESSURE Pressure Yes No No DENSITY Density Yes No No COMPRESSION Compression Yes No No INT_ENERGY Internal Energy Yes No No TEMPERATURE Temperature Yes No No Polynomial EOS This is a general form of the Mie-Gruneisen form of the equation of state and it has different analytic forms for states of compression and tension. This equation of state defines the pressure as µ> 0 (compression): p = A1µ + A2 µ 2 + A3 µ 3 + (B0 + B1µ ) p0e µ< 0 (tension) p = T1µ + T2 µ 2 + B0 p0e where µ = compression = ρ/ρ0-1 ρ0 = solid, zero pressure density e = internal energy per unit mass A1, A2, A3, B0,, B1, T1 and T2 are material constants If T1 is input as 0.0 it is reset to T1 = A1 in the solver. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1225 Appendix E. Material Models Used in Explicit Dynamics Analysis The validity of this equation depends upon the ability to represent the variation of pressure at e = 0 (or some other reference curve) as a simple polynomial in µ of no more than three terms. This is probably true as long as the range in density variation (and hence range in µ) is not too large. The Polynomial equation of state defines the Gruneisen parameter as Γ (v ) = B0 + B1µ 1+ µ This allows a number of useful variants of the Gruneisen parameter to be described: B0 = B1 Γ = B0 = cons tan t B1 = 0 Γ = B0 / ( 1 + µ ) Γ / v = B0 / v 0 = cons tan t B0 ≠ B1 ≠ 0 Γ = B0 + ( B1 - B0 ) ( v 0 - v ) / v 0 i .e. Γ is linear in v . Note This equation of state can only be used with solid elements. The Poisson's ratio is assumed to be zero when calculating effective strain. A specific heat capacity should be defined with this property to allow the calculation of temperature. Table E.13 Input Data Name Symbol Units Notes Parameter A1 A1 Stress Often equivalent to the material bulk modulus Parameter A2 A2 Stress Parameter A3 A3 Stress Parameter B0 B0 None Parameter B1 B1 None Parameter T1 T1 Stress Parameter T2 T2 Stress This value will be automatically set to the material bulk modulus if entered as zero. Custom results variables available for this model: Name Description Solids Shells Beams PRESSURE Pressure Yes No No 1226 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Equations of State Name Description Solids Shells Beams DENSITY Density Yes No No COMPRESSION Compression Yes No No VISC_PRESSURE Viscous Pressure Yes No No INT_ENERGY Internal Energy Yes No No TEMPERATURE Temperature Yes No No Shock EOS Linear The Rankine-Hugoniot equations for the shock jump conditions can be regarded as defining a relation between any pair of the variables ρ(density), P (pressure), e (energy), up (particle velocity) and U (shock velocity). In many dynamic experiments making measurements of up and U it has been found that for most solids and many liquids over a wide range of pressure there is an empirical linear relationship between these two variables: U = c0 + su p It is then convenient to establish a Mie-Gruneisen form of the equation of state based on the shock Hugoniot: p = pH + Γ p (e - eH ) where it is assumed that Γ ρ = Γ0 ρ0 = constant and pH = p0c02 µ (1 + µ ) 2 1 - (s - 1) µ  1 pH  µ  eH =   2 p0  1 + µ  Note that for s>1 this formulation gives a limiting value of the compression as the pressure tends to infinity. The denominator of the first equation above becomes zero and the pressure therefore becomes infinite for 1– (s-1)µ= 0 giving a maximum density of ρ = s ρ0 (s-1). However, long before this regime is approached, the assumption of constant Γ ρ is probably not valid. Furthermore, the assumption of linear variation between the shock velocity U and the particle velocity up does not hold for too large a compression. Γ is known as the Gruneisen coefficient and is often approximated to Γ ~2s-1 in the literature. The Shock EOS linear model lets you optionally include a quadratic shock velocity, particle velocity relation of the form: Us = C0 + S1u p + S2u p2 The input parameter, S2, can be set to a non-zero value to better fit highly non-linear Us - up material data. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1227 Appendix E. Material Models Used in Explicit Dynamics Analysis Data for this equation of state can be found in various references and many of the materials in the explicit material library. Note This equation of state can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. A specific heat capacity should be defined with this property to allow the calculation of temperature. Table E.14 Input Data Name Symbol Units Notes Gruneisen coefficient Γ None Parameter C1 C1 Velocity Parameter S1 S1 None Parameter Quadratic S2 S2 1/Velocity Custom results variables available for this model: Name Description Solids Shells Beams PRESSURE Pressure Yes No No DENSITY Density Yes No No COMPRESSION Compression Yes No No VISC_PRESSURE Viscous Pressure Yes No No INT_ENERGY Internal Energy Yes No No TEMPERATURE Temperature Yes No No Shock EOS Bilinear This is an extension of the Shock EOS Linear property. At high shock strengths nonlinearity in the shock velocity - particle velocity relationship is apparent, particularly for non-metallic materials. To account for this nonlinearity, the input calls for the definition of two linear fits to the shock velocity - particle velocity relationship; one at low shock compressions defined by Up > VB and one at high shock compressions defined by Up < VE. The region between VE and VB is covered by a smooth interpolation between the two linear relationships as shown below. 1228 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Equations of State Figure: Fit to Shock Velocity-Particle Velocity Relationship Shock Velocity V U2 = c 2+ s 2.u p U1 = c 1+ s 1.u p VB VE Particle Velocity In the input you are prompted for values of the parameters c1, c2, s1, s2, VE/Vo, VB/Vo, Γo and ρo . Then U1 = c1 + s1u p U2 = c2 + s2u p U = U1 for v ≥ VB U = U1 + U = U2 for v ≤ VE (U2 − U1 )(v − VB ) for VE < v < VB (VE − VB ) Note This equation of state can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. A specific heat capacity should be defined with this property to allow the calculation of temperature. Table E.15 Input Data Name Symbol Units Gruneisen coefficient Γ None Parameter C1 C1 Velocity Parameter S1 S1 None Parameter C2 C2 Velocity Parameter S2 S2 None Relative Volume VB/V0 VB/V0 None Relative Volume VE/V0 VE/V0 None Notes This equation of state can only be used with solid elements. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1229 Appendix E. Material Models Used in Explicit Dynamics Analysis Custom results variables available for this model: Name Description Solids Shells Beams PRESSURE Pressure Yes No No DENSITY Density Yes No No COMPRESSION Compression Yes No No VISC_PRESSURE Viscous Pressure Yes No No INT_ENERGY Internal Energy Yes No No TEMPERATURE Temperature Yes No No JWL EOS The JWL equation of state describes the detonation product expansion down to a pressure of 1 kbar for high energy explosive materials and has been proposed by Jones, Wilkins and Lee according to the following equation p = A(1 − wη R1 − )e 1 η + B (1 − wη R2 − )e 2 η + wρ e , where ρ0 is the reference density, ρ the density and η = ρ/ρ0. The values of the constants A, B, R1, R2 and ω for many common explosives have been determined from dynamic experiments. Figure: Pressure as function of density for the JWL equation of state The standard JWL equation of state can be used in combination with an energy release extension whereby additional energy is deposited over a user-defined time interval. Thermobaric explosives show this behavior and produce more explosive energy than conventional high energy explosives through combustion of inclusions, like aluminum, with atmospheric oxygen after detonation. 1230 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Equations of State This option is activated when the additional specific energy is specified different from zero. Burn on Compression In this process the detonation wave is not predefined but the unburned explosive is initially treated similarly to any other inert material. However, as an initiating shock travels through the unburned explosive and traverses elements within the explosive the compression of all explosive elements is monitored. If and when the compression in a cell reaches a predefined value the chemical energy is allowed to be released at a controlled rate. Burn on compression may be defined in one of two ways: • Pre-burn bulk modulus KBK is zero. The elements start to release their energy when the element compression µ exceeds a specified fraction of the Chapman-Jouguet compression: µ > BCJµCJ, where µCJ = PCJ/(ρDCJ2) • Pre-burn bulk modulus KBK is non zero. The elements start to release their energy when the element pressure exceeds a specified fraction of the Chapman-Jouguet pressure: P = KBK(ρ/ρ0–1) > BCJPCJ The critical threshold compression and the release rate are parameters that must be chosen with care in order to obtain realistic results. The burn on compression option may give unrealistic results for unconfined regions of explosive since the material is free to expand at the time of initial shock arrival and may not achieve sufficient compression to initiate energy release in a realistic time scale. Typically, a burn logic based upon compression is more successful in Lagrangian computations rather than Eulerian. Note The constants A, B, R1, R2 and ω should be considered as a set of interdependent parameters and one constant cannot be changed unilaterally without considering the effect of this change on the other parameters. This equation of state can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. A specific heat capacity should be defined with this property to allow the calculation of temperature. Table E.16 Input Data Name Symbol Units Parameter A A Stress Parameter B B Stress Parameter R1 R1 None Parameter R2 R2 None Parameter ω ω None Notes Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1231 Appendix E. Material Models Used in Explicit Dynamics Analysis Name Symbol Units C-J Detonation Velocity DCJ Velocity C-J Energy/unit mass Notes Energy/mass C-J Pressure PCJ Stress Burn on compression logic Burn on compression fraction BCJ None Burn on compression logic Pre-burn bulk modulus KBK Stress Burn on compression logic Adiabatic constant None Additional specific internal energy/unit mass Energy/mass Additional energy release Begin Time Time Start time of additional energy release End Time Time End time of additional energy release This equation of state can only be used with solid elements. Custom results variables available for this model: Name Description Solids Shells Beams PRESSURE Pressure Yes No No DENSITY Density Yes No No COMPRESSION Compression Yes No No INT_ENERGY Internal Energy Yes No No TEMPERATURE Temperature Yes No No BURN_FRAC Burn Fraction Yes No No Porosity The following Porosity models are discussed in this section: Porosity-Crushable Foam Compaction EOS Linear Compaction EOS Non-Linear P-alpha EOS Porosity-Crushable Foam This is a relatively simple strength model designed to represent the crush characteristics of foam materials under impact loading conditions (non-cyclic loading). The model principal stress vs volumetric strain behavior is shown below. 1232 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Porosity The strength model must be used with isotropic elasticity and the following incremental elastic update of pressure and stress deviators is used. P n +1 = P n + K εɺ vn +1 / 2 ∆f n +1 / 2 Sijn +1 = S n + 2G (ε ijn +1 / 2 − δ ij εɺ νn +1 / 2 )∆f n+1 / 2 The magnitude of the resulting principal stresses is compared against the allowable principal compaction stress, for the current volumetric strain. If the principal stress exceeds the maximum allowable, it is reduced to the allowable value. if σ i• n+1 >= σ iCompaction (ε v ) then σ in+1 = σ iCompaction (ε v ) σ i• ,n+1 σ i• ,n+1 After scaling back of the principal stresses they are transformed back to the global system to give the final stress update. Note that the return of the principal stress back to the compaction stress is performed independently in each of the principal directions, implying zero plastic Poisson's ratio. The compaction curve can be defined as a piecewise linear principal stress vs volumetric strain curve. The volumetric strain is defined as the natural log of the volume ratio, where V0 is the original volume and V is the current volume. V  ε v = ln  0  V  In tension, the model additionally includes the possibility to apply a tension cut-off to the maximum allowable principal tensile stress. If the tensile stress exceeds this value, it is maintained at this value. The model cannot currently be used with other failure properties. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1233 Appendix E. Material Models Used in Explicit Dynamics Analysis Note This property must be used in combination with isotropic elasticity. The property can only be applied to solid bodies. Note that the plastic strain variable is used to store the inelastic volumetric strain for this porosity model. Table E.17 Input Data Name Symbol Units Notes Maximum Principal Stress vs In (volumetric strain) Stress and strain Tabular data Maximum Tensile Stress Stress Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes No No PRESSURE Pressure Yes No No DENSITY Density Yes No No Porous Materials Porous materials are extremely effective in attenuating shocks and mitigating impact pressures. The material compacts to its solid density at relatively low stress levels but, because the volume change is relatively large, a large amount of energy is irreversibly absorbed thereby attenuating shocks by lengthening the wave in time and reducing it in amplitude as more material is compacted. Cellular porous materials contain a population of microscopic cells separated by cell walls. When stressed the initial elastic compression is assumed to be due to elastic buckling of the cell walls and the plastic flow to be due to plastic deformation of these cell walls. Materials with low initial porosity has fewer cells and thicker cell walls so that the stress required to cause buckling and subsequent deformation of the cell walls will be greater. Once some plastic flow has taken place, even if the fully compacted density hasn't been reached, unloading to zero stress and reloading to the elastic limit will be elastic. This phenomenological behavior is illustrated in the following figure. 1234 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Porosity pressure Figure: Loading-Unloading Behavior for a Porous Solid Plastic compaction Fully compacted Elastic loading Elastic unloading (variable slope) density Compaction EOS Linear The response of porous materials is represented via • A plastic compaction path defined as a piecewise linear function of pressure versus density • The elastic unloading/reloading path defined via a piecewise linear function of sound speed versus density. The use of a fixed compaction path (which may be derived from static compression data, either in its original state or arbitrarily enhanced to model dynamic data) is equivalent to using a Mie-Gruneisen equation of state with an assumed value of zero for the Gruneisen Gamma. This ignores the pressure enhancement due to the energy absorption. The elastic bulk stiffness of the material is defined as a piecewise linear curve of sound speed (c) versus density (ρo). The bulk stiffness of the material is given by K = ρ0c 2 The level of compaction in the material is given by α= ρs ρ0 Initially, ρo will be equal to the value defined in the density property of the material. Material property ρs is the solid zero pressure density of the material and corresponds to the fully compacted material density. For a porous material the initial density will be less than the solid density hence the value of α will be greater than 1.0. As compaction takes place, α will reduce to a value of 1.0 for the fully compacted state. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1235 Appendix E. Material Models Used in Explicit Dynamics Analysis Note It is important when using the model to ensure that the input data is such that the elastic loading line from the initial porous density intersects the plastic compaction curve at the intended position. This property must be used in combination with a shear modulus to define the total elastic stiffness of the material. The property can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. The input data for the porous model is as follows: Name Symbol Solid Density ρs Units Notes Density at zero pressure for fully compacted material Compaction Curve Tabular data of compaction pressure against density Linear Unloading Curve Tabular data of sound speed against density Custom results variables available for this model: Name Description Solids Shells Beams PRESSURE Pressure Yes No No DENSITY Density Yes No No COMPRESSION Compression Yes No No VISC_PRESSURE Viscous Pressure Yes No No INT_ENERGY Internal Energy Yes No No ALPHA Porosity (Alpha) Yes No No Compaction EOS Non-Linear This property is an extension of the Compaction EOS linear property and can provide a more accurate representation of non-linearity when unloading a porous material. The response of porous materials is represented via • A plastic compaction path defined as a piecewise linear function of pressure versus density • The non-linear unloading defined by means of a piecewise curve of bulk modulus versus density For the non-linear unloading, if the current pressure is less than the current compaction pressure, the pressure is defined by K (ρ ) = ρ dP dρ This produces a nonlinear unloading pattern, an example of which is shown below: 1236 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Porosity Note It is important when using the model to ensure that the input data is such that the elastic loading line from the initial porous density intersects the plastic compaction curve at the intended position. This property must be used in combination with a shear modulus to define the total elastic stiffness of the material. The property can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. The input data for the porous model is as follows: Name Symbol Solid Density ρs Units Notes Density at zero pressure for fully compacted material Compaction Curve Tabular data of compaction pressure against density Nonlinear Unloading Curve Tabular data of bulk modulus against density Custom results variables available for this model: Name Description Solids Shells Beams PRESSURE Pressure Yes No No DENSITY Density Yes No No COMPRESSION Compression Yes No No VISC_PRESSURE Viscous Pressure Yes No No INT_ENERGY Internal Energy Yes No No ALPHA Porosity (Alpha) Yes No No Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1237 Appendix E. Material Models Used in Explicit Dynamics Analysis P-alpha EOS Although the compaction models give good results for low stress levels and low α materials, it is very desirable to obtain a single formulation for the modeling of a porous material which gives a good representation over a wide stress range and variety of materials. Such a model has been derived by Hermann (1960)5 and this is available in explicit dynamics. Hermann's P-alpha model uses a phenomenological approach to devising a representation which gives the correct behavior at high stresses but at the same time provides a reasonably detailed description of the compaction process at low stress levels. The principal assumption is that the specific internal energy is the same for a porous material as for the same material at solid density at identical conditions of pressure and temperature. Then the porosity, α, is given by α= v vs (E–9) where v is the specific volume of the porous material and vs is the specific volume of the material in the solid state and at the same pressure and temperature (note that vs is only equal to 1/ρsolid at zero pressure). α becomes unity when the material compacts to a solid. If the equation of state of the solid material, neglecting shear strength effects, is given by p = f (v , e ) (E–10) then the equation of state of the porous material is simply v  p = f  ,e  α  (E–11) This function can be any of the equations of state which describe the compressed state of material, i.e., Linear, Polynomial and Shock, but not those describing the expanded state. In order to complete the material description the porosity α must be specified as a function of the thermodynamic state of the material, say, α = g (p , e ) (E–12) There is not enough data usually available to determine the function g(p,e) completely but fortunately most problems of interest involve shock compaction of the porous material, i.e. the region of interest lies on or near the Hugoniot. On the Hugoniot, pressure and internal energy are related by the RankineHugoniot conditions so therefore along the Hugoniot equation Equation E–12 (p. 1238) can be expressed as 1238 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Porosity α = g (p ) (E–13) with the variation with energy implicitly assumed. It is assumed this equation Equation E–13 (p. 1239) remains valid in the neighborhood of the Hugoniot (tacitly assuming that the compaction strength is insensitive to the small changes in temperature in extrapolating small distances from the Hugoniot). The general behavior of the compacting porous material has been described earlier and the P-α model is constructed to reproduce this behavior. The P-α variation to provide this performance is shown schematically in the figure below. The material deforms elastically up to a pressure pe and subsequent deformation is plastic until the material is fully compacted at a pressure ps. Intermediate unloading and reloading is elastic up to the plastic loading curve. The choice of a suitable function g(p) is somewhat arbitrary as long as it satisfies certain simple analytic properties enumerated by Herrmann in his original paper, and several forms have been used by different researchers. A simple form (Butcher & Karnes 1968) 6 found adequate for porous iron is a quadratic form  p −p  α = 1 + (α p − 1) 1   ps − pe  2 (E–14) but cubic and exponential forms have also been proposed and the parameters adjusted to fit experimental data. The exponent in the Butcher and Karnes α equation has been changed to a user defined material parameter, n. This allows for more flexibility in the fitting procedure. The parameters αp, ps and pe are shown in the above figure. Other workers have developed the basic P-α model of Herrmann to give better fits to experimental data for specific materials. Carroll & Holt (1972) 7 modified the equation of state of the porous material to give Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1239 Appendix E. Material Models Used in Explicit Dynamics Analysis  1 v  p =   f   ,e α  α  (E–15) where the factor 1/α was included to allow for their argument that the pressure in the porous material is more nearly 1/α times the average pressure in the matrix material. It is this form of the model that is available in explicit dynamics. Note The solid equation of state must be defined using one of the following properties Bulk modulus Polynomial EOS Shock EOS Linear Shock EOS Bilinear This property must be used in combination with a shear modulus to define the total elastic stiffness of the material. The property can only be applied to solid bodies. The Poisson's ratio is assumed to be zero when calculating effective strain. Table E.18 Input Data Name Symbol Units Solid Density ρsolid Density Porous Soundspeed Notes Velocity Initial Compaction Pressure Pe Stress Solid Compaction Pressure Ps Stress Compaction Exponent n None Custom results variables available for this model: Name Description Solids Shells Beams PRESSURE Pressure Yes No No DENSITY Density Yes No No COMPRESSION Compression Yes No No VISC_PRESSURE Viscous Pressure Yes No No INT_ENERGY Internal Energy Yes No No ALPHA Porosity (Alpha) Yes No No 5 5 Herrmann, W (1969). “Constitutive Equation for the Dynamic Compaction of Ductile Porous Materials”, J. Appl. Phys., 40, 6, pp 24902499, May 1969 1240 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Failure 6 7 Failure Background Materials are not able to withstand tensile stresses which exceed the material's local tensile strength. The computation of the dynamic motion of materials assuming that they always remain continuous, even if the predicted local stresses reach very large values, will lead to unphysical solutions. A model has to be constructed to recognize when tensile limits are reached to modify the computation to deal with this and to describe the properties of the material after this formulation has been applied. Several different modes of failure initiation can be represented in the explicit dynamics system. Element failure in the explicit dynamics system has two components: Failure initiation A number of mechanisms are available to initiate failure in a material (see properties Plastic Strain Failure, Principal Stress Failure, Principal Strain Failure, Tensile Pressure Failure, Johnson-Cook Failure, Grady Spall Failure). When specified criteria are met within an element, a post failure response is activated. Failure initiation can be identified in the model via the custom result MAT_STATUS. The following key is used. MAT_STATUS Meaning 1 Material is currently undergoing elastic deformation, or no deformation 2 The plastic strain in the material increased during the last time increment 3 The material has failed due to isotropic (bulk) criteria 4 The material has failed due to isotropic (bulk) criteria 5 The material has failed in tension due to principal value 1 6 The material has failed in tension due to principal value 2 7 The material has failed in tension due to principal value 3 Post failure response After failure initiation in an element, the subsequent strength characteristics of the element will change depending on the type of failure model • Instantaneous Failure Upon failure initiation, the element deviatoric stress will be immediately set to zero and retained at this level. Subsequently, the element will only be able to support compressive pressures. 6 Butcher, B M, & Karnes, C H (1968). Sandia Labs. Res Rep. SC-RR-67-3040, Sandia Laboratory, Albuquerque, NM, April 1968 7 Carroll, M M, & Holt, A C (1972). “Static and Dynamic Pore Collapse Relations for Ductile Porous Materials.” J. Appl.Phys., 43, 4, pp1626 et seq., 1972 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1241 Appendix E. Material Models Used in Explicit Dynamics Analysis • Gradual Failure (Damage) After failure initiation, the element stress is limited by a damage evolution law. Usually this results in a gradual reduction in an elements capability to carry deviatoric and/or pressure stresses. By default, tensile failure models will produce an instantaneous post failure response. Inserting the crack softening failure property, in addition to other failure initiation properties results in a gradual failure response. The following Failure models are discussed in this section: Plastic Strain Failure Principal Stress Failure Principal Strain Failure Stochastic Failure Tensile Pressure Failure Crack Softening Failure Johnson-Cook Failure Grady Spall Failure Plastic Strain Failure Plastic strain failure can be used to model ductile failure in materials. Failure initiation is based on the effective plastic strain in the material. The user inputs a maximum plastic strain value. If the material effective plastic strain is greater than the user defined maximum, failure initiation occurs. The material instantaneously fails. Note This failure model must be used in conjunction with a plasticity or brittle strength model. Name Maximum Equivalent Plastic Strain Symbol Units Notes max None Input data > zero Epl Custom results variables available for this model: Name Description Solids Shells Beams EFF_PL_STN Effective Plastic Strain Yes Yes Yes STATUS Material Status** Yes No No **Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3) Principal Stress Failure Principal stress failure can be used to represent brittle failure in materials. Failure initiation is based on one of two criteria • Maximum principal tensile stress • Maximum shear stress (derived from the maximum difference in the principal stresses) 1242 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Failure Failure is initiated when either of the above criteria is met. The material instantaneously fails. If this model is used in conjunction with a plasticity model, it is often recommended to deactivate the Maximum Shear stress criteria by specifying a large value. In this case the shear response will be handled by the plasticity model. Note The crack softening failure property can be combined with this property to invoke fracture energy based softening. Name Symbol Units Notes Maximum Tensile Stress Stress User must input a positive value. Default = +1e+20 Maximum Shear Stress Stress User must input a positive value. Default = +1e+20 Custom results variables available for this model: Name Description Solids Shells Beams STATUS Material Status** Yes No No **Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3) Principal Strain Failure Principal strain failure can be used to represent brittle or ductile failure in materials. Failure initiation is based on one of two criteria • Maximum principal tensile strain • Maximum shear strain (derived from the maximum difference in the principal stresses) Failure is initiated when either of the above criteria is met. The material instantaneously fails. If this model is used in conjunction with a plasticity model, it is often recommended to deactivate the maximum shear strain criteria by specifying a large value. In this case the shear response will be treated by the plasticity model. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1243 Appendix E. Material Models Used in Explicit Dynamics Analysis Note The crack softening failure property can be combined with this property to invoke fracture energy based softening. Table E.19 Input Data Name Symbol Units Notes Maximum Principal Strain None User must input a positive value. Default = +1e+20 Maximum Shear Strain None User must input a positive value. Default = +1e+20 Custom results variables available for this model: Name Description Solids Shells Beams STATUS Material Status** Yes No No **Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3) Stochastic Failure To model fragmentation for symmetric loading and geometry it is necessary to impose some material heterogeneity. Real materials have inherent microscopic flaws, which cause failures and cracking to initiate. An approach to reproducing this numerically is to randomize the failure stress or strain for the material. Using this property, a Mott distribution is used to define the variance in failure stress or strain. Each element is allocated a value, determined by the Mott distribution, where a value of one is equivalent to the failure stress or strain of the material. The Mott distribution takes the form P(ε ) = 1 − exp  − C (exp(γε ) − 1)  γ  where P is the probability of fracture ε is the strain C and γ are material constants For the implementation in explicit dynamics, the fracture value of 1 is forced to be at a probability of 50%, therefore the user needs only specify a gamma value and the constant C is derived from this. 1244 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Failure Figure: Mott Distribution for Varying Values of Gamma The stochastic failure option may be used in conjunction with many of the failure properties, including hydro (Pmin), plastic strain, principal stress and/or strain. It can also be used in conjunction with the RHT concrete model. You must specify a value of the stochastic variance, γ, and also the distribution seed type. If the “random” option is selected every time a simulation is performed a new distribution will be calculated. If the “fixed” option is selected the same distribution will be used for each solve. Table E.20 Input Data Name Symbol Units Notes Distribution Type Option List: Random Fixed (default) γ Stochastic Variance Minimum Fail Fraction None None Default = 0.1 Custom results variables available for this model: Name Description Solids Shells Beams STATUS Material Status** Yes No No STOCH_FACT Stochastic Factor Yes No No **Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1245 Appendix E. Material Models Used in Explicit Dynamics Analysis Tensile Pressure Failure The tensile pressure failure model allows a maximum hydrodynamic tensile limit to be specified. This is used to represent a dynamic spall (or cavitation) strength of the material. The algorithm simply limits the maximum tensile pressure in the material as ∗ P < Pmin (1 − D ) If the material pressure P becomes less than the defined maximum tensile pressure, failure initiation occurs. The material instantaneously fails. If the material definition contains a damage evolution law, the user defined maximum tensile pressure is scaled down as the damage increases from 0.0 to 1.0. Note The property can only be applied to solid bodies. The crack softening failure property can be combined with this property to invoke fracture energy based softening. Table E.21 Input Data Name Symbol Maximum Tensile Pressure Units Notes Stress User must input a negative value. Default = –1e+20 Custom results variables available for this model: Name Description Solids Shells Beams PRESSURE Pressure Yes No No STATUS Material Status** Yes No No **Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3) Crack Softening Failure The tensile crack softening model is fracture energy based damage model which can be used with many different types of failure initiation models to provide a gradual reduction in the ability of an element to carry tensile stress. The model is primarily used for investigating failure of brittle materials, but has been applied to other materials to reduce mesh dependency effects. • Failure initiation is based on any of the standard tensile failure models. e.g., Hydro, Principal Stress/Strain • On failure initiation, the current maximum principal tensile stress in the element is stored (custom result FAIL.STRES) • A linear softening slope (custom result SOFT.SLOPE) is then defined to reduce the maximum possible principal tensile stress in the material as a function of crack strain. This softening slope is defined as a function of the local element size and a material parameter, the fracture energy Gf. 1246 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Failure σ Slope = Area = G f /L Lf t2 2G f ε Total Fracture ε The extent of damage in a material can be inspected by using the custom result DAMAGE. The damage is defined to be 0.0 for an intact element and 1.0 for a fully failed element. • After failure initiation, a maximum principal tensile stress failure surface is defined to limit the maximum principal tensile stress in the element and a flow rule is used to return to this surface and accumulate the crack strain There are currently three options in relation to the crack softening plastic return algorithm: – Radial Return — Non-associative in π– and meridian planes – No-Bulking — Associative in π– plane only (Default) – Bulking — Associative in π– and meridian planes The default setting has been selected based on practical experiences of using the model to simulate impacts onto brittle materials such as glass, ceramics, and concrete. The crack softening algorithm can only be used with solid elements. It can be used in combination with any solid equation of state, plasticity model or brittle strength model. When used in conjunction with a plasticity/brittle strength model, the return algorithm will return to the surface giving the minimum resulting effective stress, J2. Meridian Plane Trial Elastic Stresses Rankine Failure Surface J2 Associate flow in Meridional Plane(Option) Yield Surface (Strength Model) Non-associative flow-in Meridional Plane (Default) Pressure Rankine Plasticity Yielding (Tensile Cracking) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1247 Appendix E. Material Models Used in Explicit Dynamics Analysis π- space Trial Elastic Stresses Associative flow in x-Plane (Default) Non-Associative flow in x-Plane (Default) Rankine Failure Surface Von Mises Surface Note The property can only be applied to solid bodies. Table E.22 Input Data Name Symbol Units Fracture Energy Gf Energy/Area Flow rule Notes Option List: Radial Return No Bulking (Default) Bulking (Associative) Custom results variables available for this model: Name Description Solids Shells Beams DAMAGE Current damage level Yes No No FAIL.STRES Principal tensile failure stress Yes No No SOFT.SLOPE Softening slope Yes No No Johnson-Cook Failure The Johnson-Cook failure model can be used to model ductile failure of materials experiencing large pressures, strain rates and temperatures. This model is constructed in a similar way to the Johnson-Cook plasticity model in that it consists of three independent terms that define the dynamic fracture strain as a function of pressure, strain rate and temperature: 1248 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Failure The ratio of the incremental effective plastic strain and effective fracture strain for the element conditions is incremented and stored in custom results variable, DAMAGE. The material is assumed to be intact until DAMAGE = 1.0. At this point failure is initiated in the element. An instantaneous post failure response is used. Note The property can only be applied to solid bodies. Table E.23 Input Data Name Symbol Units Damage Constant D1 D1 None Damage Constant D2 D2 None Damage Constant D3 D3 None Damage Constant D4 D4 None Damage Constant D5 D5 None Melting Temperature Notes Temperature Custom results variables available for this model: Name Description Solids Shells Beams DAMAGE Damage Yes No No **Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3) Grady Spall Failure The Grady Spall model can be used to model dynamic spallation of metals under shock loading. The critical spall stress for a ductile material can be calculated according to: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1249 Appendix E. Material Models Used in Explicit Dynamics Analysis This critical spall stress is calculated for each element in the model at each time step and compared with local maximum principal tensile stress. If the maximum element principal tensile stress exceeds the critical spall stress, instantaneous failure of the element is initiated. A typical value for the critical strain is 0.15 for aluminum. Note The property can only be applied to solid bodies. The property must be used in conjunction with a plasticity model. Table E.24 Input Data Name Symbol Units Critical Strain Value εc None Notes Custom results variables available for this model: Name Description Solids Shells Beams STATUS Material Status Yes No No **Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3) Strength The following table summarizes the applicable strength-limit constants for each failure criterion: Strength Limit Constant Orthotropic Stress Limit Orthotropic Strain Limit Tsai-Wu Constants Tensile X-Direction Y Y Y Tensile Y-Direction Y Y Y Tensile Z-Direction Y Y Compressive X Y Compressive Y Y Compressive Z Shear XY Y Y Shear YZ Y Y Shear XZ Y Y Y Coupling Coefficient XY Coupling Coefficient YZ 1250 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Rigid Materials Coupling Coefficient XZ Tsai-Wu Constants must be used in conjunction with Orthotropic Stress Limit. Tsai-Wu Constants used in conjunction with Orthotropic Strain Limit are not supported. The TSai-Wu coefficients are always reset to -1 in an Explicit solve. The Tsai-Wu Constants property changes how the Explicit Dynamics solver uses the data from the Orthotropic Stress Limit property. Without the Tsai-Wu Constants property, the Explicit Dynamics solver uses all three tensile stress and all three shear stress constants from the Orthotropic Stress Limit. With the Tsai-Wu Constants property, the Explicit Dynamics solver uses the tensile and compressive stress constants in the X and Y direction only (not Z) and the XY shear stress constant (not YZ and XZ shears). Thermal Specific Heat Specific heat is the amount of heat per mass required to raise the temperature of a material. Custom results variables available for this model: Name Description Solids Shells Beams TEMPERATURE Temperature Yes Yes Yes **Material status indicators (1 = elastic, 2 = plastic, 3 = bulk failure, 4= bulk failure, 5 = failed principal direction1, 6 = failed principal direction 2, 7 = failed principal direction 3) Rigid Materials Rigid materials can be modeled in an explicit dynamics system by selecting geometry, “Stiffness behavior = rigid” on a body. In such cases only the density property of the material associated with the body will be used. For explicit dynamics systems all rigid bodies must be discretized with a full mesh. This will be specified by default for the explicit meshing physics preference. The mass and inertia of the rigid body will be derived from the elements and material density for each body. By default, a kinematic rigid body is defined in explicit dynamics and its motion will depend on the resultant forces and moments applied to it through interaction with other parts of the model. Elements filled with rigid materials can interact with other regions via contact. Constraints can only be applied to an entire rigid body. For example, a fixed displacement cannot be applied to one edge of a rigid body; it must be applied to the whole body. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1251 1252 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Appendix F. Explicit Dynamics Theory Guide This appendix describes the theoretical basis of the Explicit Dynamics system available in Workbench. The following topics are covered in this appendix: Why use Explicit Dynamics? What is Explicit Dynamics? Analysis Settings References Why use Explicit Dynamics? The Explicit Dynamics system is designed to enable you to simulate nonlinear structural mechanics applications involving one or more of the following: • Impact from low [(0)1m/s] to very high velocity [(0)5000m/s] • Stress wave propagation • High frequency dynamic response • Large deformations and geometric nonlinearities • Complex contact conditions • Complex material behavior including material damage and failure • Nonlinear structural response including buckling and snapthrough • Failure of bonds/welds/fasteners • Shock wave propagation through solids and liquids • Rigid and flexible bodies Explicit Dynamics is most suited to events which take place over short periods of time, a few milliseconds or less. Events which last more than 1 second can be modelled; however, long run times can be expected. Techniques such as mass scaling and dynamic relaxation are available to improve the efficiency of simulations with long durations. What is Explicit Dynamics? An overview of the solution methodology used in an Explicit Dynamics simulation is provided in this section. The Solution Strategy Basic Formulations Time Integration Wave Propagation Reference Frame Explicit Fluid Structure Interaction (Euler-Lagrange Coupling) Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1253 Appendix F. Explicit Dynamics Theory Guide The Solution Strategy In an Explicit Dynamics solution, we start with a discretized domain (mesh) with assigned material properties, loads, constraints and initial conditions. This initial state, when integrated in time, will produce motion at the node points in the mesh. • The motion of the node points produces deformation in the elements of the mesh • The deformation results in a change in volume (hence density) of the material in each element • The rate of deformation is used to derive material strain rates using various element formulations • Constitutive laws take the material strain rates and derive resultant material stresses • The material stresses are transformed back into nodal forces using various element formulations • External nodal forces are computed from boundary conditions, loads and contact (body interaction) • The nodal forces are divided by nodal mass to produce nodal accelerations • The accelerations are integrated Explicitly in time to produce new nodal velocities • The nodal velocities are integrated Explicitly in time to produce new nodal positions • The solution process (Cycle) is repeated until a user defined time is reached Basic Formulations An introduction to the basic equations which are solved in Explicit Dynamics is provided in this section. Implicit Transient Dynamics Explicit Transient Dynamics Implicit Transient Dynamics The basic equation of motion solved by an implicit transient dynamic analysis is 1254 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. What is Explicit Dynamics? Where: m = mass matrix c = damping matrix k = stiffness matrix F(t) = load vector At any given time, t, these equations can be thought of as a set of "static" equilibrium equations that also take into account inertia forces and damping forces. The Newmark time integration method (or an improved method called HHT) is used to solve these equations at discrete time points. The time increment between successive time points is called the integration time step. Explicit Transient Dynamics The partial differential equations to be solved in an Explicit Dynamics analysis express the conservation of mass, momentum, and energy in Lagrangian coordinates. These, together with a material model and a set of initial and boundary conditions, define the complete solution of the problem. For the Lagrangian formulations currently available in the Explicit Dynamics system, the mesh moves and distorts with the material it models and conservation of mass is automatically satisfied. The density at any time can be determined from the current volume of the zone and its initial mass The partial differential equations that express the conservation of momentum relate the acceleration to the stress tensor σij. Conservation of energy is expressed via: These equations are solved explicitly for each element in the model, based on input values at the end of the previous time step. Small time increments are used to ensure stability and accuracy of the solution. Note that in Explicit Dynamics we do not seek any form of equilibrium; we simply take results from the previous time point to predict results at the next time point. There is no requirement for iteration. In a well-posed Explicit Dynamics simulation, mass, momentum, and energy should be conserved. Only mass and momentum conservation is enforced. Energy is accumulated over time and conservation is monitored during the solution. Feedback on the quality of the solution is provided via summaries of momentum and energy conservation (as opposed to convergent tolerances in implicit transient dynamics). Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1255 Appendix F. Explicit Dynamics Theory Guide Time Integration In this section, the Explicit Dynamics time integration scheme is described and compared with an implicit formulation. Implicit Time Integration Explicit Time Integration Mass Scaling Implicit Time Integration For implicit time integration, ANSYS solves the transient dynamic equilibrium equation using the Newmark approximation (or an improved method known as HHT). For more information, see Transient Analysis in the Mechanical APDL Theory Reference. For linear problems, the implicit time integration is unconditionally stable for certain integration parameters. The time step size will vary to satisfy accuracy requirements. For nonlinear problems: • The solution is obtained using a series of linear approximations (Newton-Raphson method), so each time step may have many equilibrium iterations. • The solution requires inversion of the nonlinear dynamic equivalent stiffness matrix. • Small, iterative time steps may be required to achieve convergence. • Convergence tools are provided, but convergence is not guaranteed for highly nonlinear problems. Explicit Time Integration The Explicit Dynamic solver uses a central difference time integration scheme (often referred to as the Leapfrog method). After forces have been computed at the nodes of the mesh (resulting from internal stress, contact, or boundary conditions), the nodal accelerations are derived by equating acceleration to force divided by mass. Therefore the accelerations are Where: are the components of nodal acceleration (i=1,2,3) Fi are the forces acting on the nodal points bi are the components of body acceleration m is the mass attributed to the node. With the accelerations at time n determined, the velocities at time 1256 are found from Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. What is Explicit Dynamics? and finally the positions are updated to time n+1 by integrating the velocities The advantages of using this method for time integration for nonlinear problems are: • The equations become uncoupled and can be solved directly (explicitly). There is no requirement for iteration during time integration. • No convergence checks are needed because the equations are uncoupled. • No inversion of the stiffness matrix is required. All nonlinearities (including contact) are included in the internal force vector. To ensure stability and accuracy of the solution, the size of the timestep used in Explicit time integration is limited by the CFL (Courant-Friedrichs-Lewy [1 (p. 1284)]) condition. This condition implies that the timestep be limited such that a disturbance (stress wave) cannot travel farther than the smallest characteristic element dimension in the mesh, in a single timestep. Thus the timestep criteria for solution stability is Where ∆t is the time increment f is the stability timestep factor (= 0.9 by default) h is the characteristic dimension of an element c is the local material soundspeed in an element The element characteristic dimension, h is calculated as follows: Table F.1 Characteristic Element Dimensions Hexahedral/Pentahedral The volume of the element divided by the square of the longest diagonal Tetrahedral The minimum distance of any element node to it’s opposing element face Quad Shell The square root of the shell area Tri Shell The minimum distance of any element node to it’s opposing element edge Beam The length of the element of the zone and scaled by The time steps used in Explicit time integration will generally be smaller than those used in Implicit time integration. For example, for a mesh with a characteristic dimension of 1mm and a material soundspeed of 5000m/s. The resulting stability time step would be 0.18µ seconds. To solve this simulation to a termination time of 0.1 seconds will require 555,556 time increments. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1257 Appendix F. Explicit Dynamics Theory Guide Note The minimum value of h/c for all elements in the model is used to calculate the time step that will be used for all elements in the model. This implies that the number of time increments required to solve the simulation is dictated by the smallest element in the model. Care should therefore be taken when generating meshes for Explicit Dynamics simulations to ensure that one or two very small elements do not control the timestep. The patch-independent meshing methods available in Workbench will generally produce a more uniform mesh with a higher timestep than patch-dependent meshing methods. Mass Scaling The maximum timestep that can be used in Explicit time integration is inversely proportional to the soundspeed of the material, hence directionally proportional to the square root of the mass of material in an element Where Cii is the material stiffness (i=1,2,3) ρ is the material density m is the material mass V is the element volume By artificially increasing the mass of an element, one can increase the maximum allowable stability timestep, and reduce the number of time increments required to complete a solution. When mass scaling is applied in an Explicit Dynamics system, it is applied only to those elements which have a stability timestep less than a specified value. If the model contains a relatively small number of small elements, this can be a useful mechanism for reducing the number of time steps required to complete an Explicit simulation. Note Mass scaling changes the inertial properties of the portions of the mesh to which scaling is applied. The user is responsible for ensuring that the model remains representative for the physical problem being solved. Wave Propagation The Explicit Dynamics systems are particularly well suited to capturing various types of wave propagation phenomena in solid and liquid materials. Elastic Waves Plastic Waves Shock Waves 1258 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. What is Explicit Dynamics? Elastic Waves Different types of elastic waves can propagate in solids depending on how the motion of points in the solid material is related to the direction of propagation of the waves (Meyers [2 (p. 1284)]). The primary elastic wave is usually referred to as the longitudinal wave. Under uniaxial stress conditions (i.e. an elastic wave traveling down a long slender rod), the wave propagation speed is given by For the more general three-dimensional case, the additional components of stress lead to the more general expression for the primary longitudinal elastic wave speed The secondary elastic wave is usually referred to as the distortional/shear wave and it’s propagation speed can be calculated as Other forms of elastic waves include surface (Rayleigh) waves, Interfacial waves and bending (or flexural) waves in bars/plates. Further details are provided by Meyers [2 (p. 1284)]. Plastic Waves Plastic (inelastic) deformation takes place in a ductile metal when the stress in the material exceeds the elastic limit. Under dynamic loading conditions the resulting wave propagation can be decomposed into elastic and plastic regions (Meyers [2 (p. 1284)]). Under uniaxial strain conditions, the elastic portion of the wave travels at the primary longitudinal wave speed whilst the plastic wave front travels at a local velocity For an elastic perfectly plastic material, it can be shown [3 (p. 1284)] that the plastic wave travels at a slower velocity than the primary elastic wave Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1259 Appendix F. Explicit Dynamics Theory Guide Shock Waves Typical stress strain curves for a ductile metal under uniaxial stress and uniaxial strain conditions are given below. Table F.2 Typical stress strain curves for a ductile metal a) Uniaxial stress b) Uniaxial strain Under uniaxial stress conditions, the tangent modulus of the stress strain curve decreases with strain. The plastic wave speed therefore decreases as the applied jump in stress associated with the stress wave increases – shock waves are unlikely to form under these conditions. Under uniaxial strain conditions the plastic modulus (AB) increases with the magnitude of the applied jump in stress. If the stress jump associated with the wave is greater than the gradient (OZ), the plastic wave will travel at a higher speed than the elastic wave. Since the plastic deformation must be preceded by the elastic deformation, the elastic and plastic waves coalesce and propagate as a single plastic shock wave. A shock wave can be considered to be a discontinuity in material state (density(ρ), energy(e), stress(σ), particle velocity(u)) which propagates through a medium at a velocity equal to the shock velocity (Us). Figure: Conditions at a Moving Shock Front Relationships between the material state across a shock discontinuity can be derived using the principals of conservation of mass, momentum and energy. The resulting Hugoniot equations are given by 1260 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. What is Explicit Dynamics? Reference Frame You can define the reference frame for bodies in an explicit dynamics analysis to be either Lagrangian or Eulerian. The following sections describe the two reference frames and how their use affects the analysis. Lagrangian and Eulerian Reference Frames Eulerian (Virtual) Reference Frame in Explicit Dynamics Post-Processing a Body with Reference Frame Euler (Virtual) Key Concepts of Euler (Virtual) Solutions Lagrangian and Eulerian Reference Frames By default, all bodies in an Explicit Dynamics analysis system are discretized and solved in a Lagrangian reference frame: The material associated with each body is discretized in the form of a body-fitted mesh. Each element of the mesh is used to represent a volume of material. The same amount of material mass remains associated with each element throughout the simulation. The mesh deforms with the material deformation. Solving using a Lagrangian reference frame is the most efficient and accurate method to use for the majority of structural models. However, in simulations where the material undergoes extreme deformations, such as in a fluid or gas flowing around an obstacle, the elements will become highly distorted as the deformation of the material increases. Eventually the elements may become so distorted that the elements become inverted (negative volumes) and the simulation cannot proceed without resorting to numerical erosion of highly distorted elements. In an Eulerian reference frame, the grid remains stationary throughout the simulation. Material flows through the mesh. The mesh does not therefore suffer from distortion problems and large deformations of the material can be represented. If the material you are going to model is likely to experience very large deformations, using an Eulerian reference frame is therefore preferable. Solving using an Eulerian reference frame is generally computationally more expensive than using a Lagrangian reference frame. The additional cost comes from the need to transport material from one cell to the next and also to track in which cells each material exists. Each cell in the grid can contain one or more materials (to a maximum of 5 in the Explicit Dynamics system). The location and interface of each material is tracked only approximately (to first order accuracy). The representative example below shows a block of material impacting a rigid wall. First the block is represented in the Lagrangian reference frame. During the impact process the nodes of the mesh follow the deformation of the material. The same problem can be modelled in an Eulerian reference frame; here the nodes of the mesh are fixed in space, they do not move. Instead the material is tracked as it moves through the mesh. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1261 Appendix F. Explicit Dynamics Theory Guide Solid, Liquid and Gaseous materials can be used with an Eulerian (Virtual) reference frame in the Explicit Dynamics system. Because of the computational cost and approximate tracking of material interfaces, the Eulerian reference frame should be used only when very large deformation or flow of the material is expected. Eulerian (Virtual) Reference Frame in Explicit Dynamics Switching the reference frame of a solid body in Explicit Dynamics systems from Lagrangian to Eulerian will result in that body being mapped into an Eulerian background grid at solve time and the material associated with the body will be solved in an Eulerian reference frame. If one or more solid bodies have a reference frame set to Eulerian (Virtual), the following process is used on initialization to map the Euler bodies to a background Eulerian domain: Virtual Euler Domain A background Eulerian (Virtual) domain is automatically generated to enclose all bodies in the model. By default, the domain size is set to 1.2 times the size of the bounding box of all bodies in the model. The domain is always aligned with the global Cartesian X, Y, and Z axes. Additional options to control the size of the domain are provided in the Analysis Settings. 1262 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. What is Explicit Dynamics? The background Euler domain is discretized with a mesh of uniform cell size. The cell size is defined to give approximately 500,000 cells in total. Additional options to control the cell size are provided in the Analysis Settings. The entire Euler domain is initialized as void; the cells contain no material. Mapping of bodies with Euler reference frame to virtual Euler domain The standard mesh generated on bodies marked with Eulerian (Virtual) reference frame is only used to represent the geometry of the body during initialization of the model for the solver. The material and initial conditions defined on bodies marked as Eulerian reference frame are mapped to the Euler domain. The mesh associated with the original body is then deleted, prior to the solve. A unique material is created for each body that is mapped into the Euler domain for the purposes of post processing Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1263 Appendix F. Explicit Dynamics Theory Guide If multiple bodies marked as Eulerian (Virtual) overlap, the body higher in the Outline view will take precedence. Therefore, the material assigned to the region of overlap will correspond to that assigned to the first Eulerian body. The exterior faces of the Euler domain can each have one of three types of boundary condition applied. The type of boundary condition for each face is controlled in the Analysis Settings: Flow-out (Default) This condition will allow any material reaching the boundary of the Euler domain to flow out of the domain at constant velocity. Rigid Wall This condition makes the external boundaries of the domain act as a rigid wall. Impedance This condition will transmit normal stress waves out of the domain into a pseudo material of the same impedance (perfect transmission, no reflection); see Impedance Boundary (p. 557). Post-Processing a Body with Reference Frame Euler (Virtual) Results objects in the Explicit Dynamics system can be scoped to bodies which have an Euler (Virtual) reference frame defined. During the initialization of the solve for the model, the mesh associated with such bodies is discarded. Results cannot therefore be displayed on the original mesh applied to the Euler bodies. Instead, a mesh is reconstructed for each material associated with the original body to which the result object is scoped. The reconstruction of the mesh is approximate and includes: • Finding the exterior surface of each material, in its current location in the Euler domain. This is achieved by forming an isosurface on the volume fraction of each material in a cell (at 50%). • Filling the interior of the material with cells from the Euler domain that are completely inside the material. • Reconstructing an unstructured mesh for any gaps between the exterior surface and interior cells. The example below illustrates a typical mesh displayed for a Results object scoped to a Body with Eulerian (Virtual) reference frame: 1264 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. What is Explicit Dynamics? 1 2 When the Show Undeformed Wireframe option is selected for a results object scoped to Euler bodies, the wireframe of the background Euler domain is displayed. Only the Euler domain cells that contain material at a given point in time are used to construct the wireframe (cells that only contain void are not displayed). An example is given below: Key Concepts of Euler (Virtual) Solutions The conservation equations of mass, momentum and energy are solved on a block structured background mesh using a 2nd order accurate multi-material Godunov numerical scheme[17 (p. 1285)] with the second order upwind method by Van Leer [19 (p. 1285), 20 (p. 1285)]. The computational cycle for bodies represented in an Eulerian reference frame is outlined below: Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1265 Appendix F. Explicit Dynamics Theory Guide In comparison to a traditional Lagrangian numerical scheme, note the points in the following sections. Multiple Material Stress States Multiple Material Transport Supported Material Properties Multiple Material Stress States During the simulation, material can flow from one cell to another. At some stage in the computation a given cell is likely to contain more than one material. Note that void (free space) is also considered as a material in this sense; a cell containing one material and void is typical at any free surface of the material. In the example below we can see two solid materials (green and yellow) and free surfaces (white, void material) represented in an Eulerian reference frame. 1266 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. What is Explicit Dynamics? A volume of fluid (VOF) method is used track the amount of material in each cell. Each material has a volume fraction and the sum of the volume fraction of each material, plus the volume fraction of void, will equate to unity. ∑

==  1
+ 
 = 1 Nearly all isotropic material properties can be used in an Eulerian reference frame to represent Solids, Liquids or gases. Special treatment is required to allow calculation of the strain rates, pressure and stresses in each material in a cell, and also to calculate a resultant stress tensor which is then used to calculate cell face impulses, momentum and mass transport. Two algorithms are used for this purpose: 1. A cell containing two different gases; here we use an iterative procedure to establish an Equilibrium state (a density and energy of each gas which results in a uniform pressure across both gases). 2. A cell containing two or more non-gaseous materials; here we use a stiffness weighted averaging technique to distribute strain rates and establish the resultant pressure and deviatoric stress in each cell. The choice of the above algorithms is automatic and local to each cell in the model. Important At any point in time during the solution, only the volume fraction of each material in each cell is recorded and stored. The location of the material within the cell is not known. During post-processing of the model you will see an outline of the material displayed, this outline is an approximation derived from the volume fraction distribution in the cells. It is only accurate to within one cell dimension. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1267 Appendix F. Explicit Dynamics Theory Guide Multiple Material Transport To move the solution through the mesh from one timestep to another, material must be transported across cell faces. If a cell contains only one material then we have a trivial solution and a volume fraction of that material will be transported across the face. If however we have multiple materials in a cell we need to employ an algorithm to decide which materials to transport and how much of each material to transport across each cell face. We are using the SLIC (Single Line Interface Construction) method [18 (p. 1285)] to calculate the order and quantity of material to transport across a cell face. This method takes information from both the upstream and downstream cells to make decisions on material transport. Supported Material Properties The supported material properties are Density, Specific Heat, Isotropic Elasticity, Bilinear Isotropic Hardening, Multilinear Isotropic Hardening, Johnson Cook Strength, Cowper Symonds Strength, Steinberg Guinan Strength, Zerilli Armstrong Strength, Drucker-Prager Strength Linear, Drucker-Prager Strength Stassi, Drucker-Prager Strength Piecewise, Johnson-Holmquist Strength Continuous, Johnson-Holmquist Strength Segmented, RHT Concrete, MO Granular, Ideal Gas EOS, Bulk Modulus, Shear Modulus, Polynomial EOS, Shock EOS Linear, Shock EOS Bilinear, Explosive JWL, Explosive JWL Miller, Compaction EOS Linear, Compaction EOS Non-Linear, P-alpha EOS, Plastic Strain Failure, Tensile Pressure Failure, Johnson Cook Failure, Grady Spall Failure. Explicit Fluid Structure Interaction (Euler-Lagrange Coupling) In the Explicit Dynamics system, solid bodies can be assigned either a Lagrangian reference frame or an Eulerian (Virtual) reference frame. The reference frames can be combined in the simulation to allow the best solution technique to be applied to each type of material being modelled. During the simulation, bodies represented in the two reference frames will automatically interact with each other. For example, if one body is filled with steel using a Lagrangian reference frame, and another body filled with water using an Eulerian reference frame, the two bodies will automatically interact with each other if they come into contact. The interaction between Eulerian and Lagrangian bodies provides a capability for tightly coupled two way fluid structure interaction in the Explicit Dynamics system. In the simple example below, a body with Lagrangian reference frame (grey) is moving from left to right over a body with Eulerian reference frame. As the body moves, it acts as a moving boundary in the Euler domain by progressively covering volumes and faces in the Euler cells. This induces flow of material in the Euler Domain. At the same time, a stress field will develop in the Euler domain which results in external forces being applied on the moving Lagrangian body. These forces will feedback into the motion and deformation (and stress) of the Lagrangian body. In more detail, the Lagrangian body covers regions of the Euler domain. The intersection between the Lagrangian and Eulerian bodies results in an updated control volume on which the conservation equation of mass, momentum and energy are solved. 1268 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. What is Explicit Dynamics? At the same time, the normal stress in the intersected Euler cell will act on the intersected area of the Lagrangian surface. This provides a two-way closely coupled fluid-structure (or more generally Eulerian-Lagrangian) interaction. During a simulation, the Lagrangian structure can move and deform. Large deformations may also result in erosion of the elements from the Lagrangian body. The coupling interfaces are automatically updated in such cases. For accurate results when coupling Lagrangian and Eulerian bodies in Explicit Dynamics it is necessary to ensure that the size of the cells of the Euler domain are smaller than the minimum distance across the thickness of the Lagrangian bodies. If this is not the case, you may see leakage of material in the Euler domain through the Lagrange structure. Shell Coupling In the case of coupling to thin bodies (typically modelled with shells), an equivalent solid body is generated to enable intersection calculations to be performed between a Lagrangian volume and the Euler domain. The thickness of the equivalent solid body is automatically calculated based on the Euler Domain cell size to ensure that at least one Euler element is fully covered over the thickness and no leakage occurs across the coupling surface. Note this 'artificial' thickness is only used for volume intersection calculations for the purposes of coupling and is independent of the physical thickness of the shell/surface body. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1269 Appendix F. Explicit Dynamics Theory Guide Sub-cycling The Lagrangian reference frame is most frequently used to model solid structures with materials which have soundspeeds in the order of several thousand meters/second. The Eulerian reference is most frequently used to represent fluids or gases which typically have soundspeeds in the order of hundreds of meters/second. In Explicit Dynamics simulations the maximum timestep that can be used is inversely proportional to the soundspeed of the material. The timestep required to model structures is therefore often significantly smaller than the timestep required to accurately model a gas. To enable the Lagrangian and Eulerian parts of a coupled simulation proceed at the optimum timestep (for efficiency and accuracy) a sub-cycling technique is used where possible. The Lagrangian domain uses its critical timestep. The Euler domain uses its critical timestep. Coupling information is exchanged at the end of each Euler domain timestep. Analysis Settings In the following sections you find theoretical background for specific controls available in the Explicit Dynamics system. Step Controls Damping Controls Solver Controls Erosion Controls Step Controls Maximum Energy Error Energy conservation is a measure of the quality of an explicit dynamic simulation. Bad energy conservation usually implies a less than optimal model definition. This parameter allows you to automatically stop the solution if the energy conservation becomes poor. Enter a fraction of the total system energy at the reference cycle at which you want the simulation to stop. For example, the default value of 0.1 will cause the simulation to stop if the energy error exceeds 10% of the energy at the reference cycle. The global energy is accounted as follows: 1270 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Reference Energy = [Internal Energy + Kinetic Energy + Hourglass Energy] at the reference cycle Current Energy = [Internal Energy + Kinetic Energy + Hourglass Energy] at the current cycle Work Done = Work done by constraints + Work done by loads + Work done by body forces + Energy removed from system by element erosion + Work done by contact penalty forces Figure: Example energy conservation graph for model with symmetry plane and erosion Damping Controls Treatment of Shock Discontinuities Strong impacts on solid bodies can give rise to the formation of shock waves in the material. Because of the nonlinearity of the equations being solved, shocks can form even though the initial conditions are smooth. In order to handle the discontinuities in the flow variables associated with such shocks, viscous terms are introduced into the solutions. These additional terms have the effect of spreading out the shock discontinuities over several elements and thus allow the simulation to continue to compute a smooth solution, even after shock formation and growth. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1271 Appendix F. Explicit Dynamics Theory Guide Figure: Comparison of pressure solution at a shock wave discontinuity a) using no artificial viscosity b) using the default artificial viscosity The viscous terms used in the Explicit Dynamics system is based on the work of von Neumann and Richtmeyer [4 (p. 1284)] and Wilkins [5 (p. 1284)]. Where CQ is the Quadratic Artificial Viscosity coefficient CL is the Linear Artificial Viscosity coefficient ρ is the local material density d is a typical element length scale c is the local sound speed is the rate in change of volume The quadratic term smooths out shock discontinuities while the linear term acts to damp out oscillations which may occur in the solution behind the shock discontinuity. 1272 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Figure: Effects of artificial viscosity on the solution a) Quadratic term stabilizes b) The linear term reduces noise Note • The pseudo-viscous term applies only to Solid bodies • The pseudo-viscous term is usually added only when the flow is compressing. The Linear Viscosity in Expansion option can be used to apply the pseudo-viscous term in both compression and expansion. This can lead to excessive dispersion in the solution. • The inclusion of the pseudo-viscous pressure imposes further restrictions on the time step in order to ensure stability: Due to the quadratic term, Due to the linear term, The resulting critical time step is, • The pseudo-viscous pressure is stored for each element and can be contoured using the custom variable VISC_PRESSURE Hourglass Damping The reduced integration eight node hexahedral elements, or 4 node quadrilateral elements, used in Explicit Dynamics can exhibit “hourglass” modes of deformation. Since the expressions for strain rates and forces involve only differences in velocities and/or coordinates of diagonally opposite nodes of the cuboidal element, if the element distorts in such a way that these differences remain unchanged there will be no strain increase in the element and therefore no resistance to this distortion. Hourglass modes of deformation occur with no change in energy (also called zero energy modes) and are unphysical. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1273 Appendix F. Explicit Dynamics Theory Guide An example of such a distortion in two dimensions is illustrated below where the two diagonals remain the same length even though the cell distorts. Visualization in three dimensions is much more difficult but if such distortions occur in a region of many elements, patterns such as that shown below occur and the reason for the name of “hourglass instability” is more easily understood. To avoid these zero energy modes of deformation from occurring, corrective forces (Hourglass forces) are added to the solution to resist the hourglass modes of deformation. Hexahedral Elements Two formulations for calculating the Hourglass forces are available for Hexahedral elements: The Standard formulation is based on the work of Kosloff and Frazier [6 (p. 1284)] and generates hourglass forces proportional to nodal velocity differences. This is often referred to as a viscous formulation. Where is a vector of the hourglass forces at each node of the element CH is the Viscous Coefficient for hourglass damping ρ is the material density c is the material soundspeed V is the material volume is a vector function of the element nodal velocities aligned with the hourglass shape vector The standard formulation is the most efficient formulation in terms of CPU and is therefore the default option. It is not however invariant under rigid body rotation (i.e. under rigid body rotation the hourglass forces may not sum to zero) 1274 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings The Flanagan Belytschko [7 (p. 1285)] formulation is invariant under rigid body rotation and is therefore recommended for simulations in which large rotations of hexahedral elements are expected. The Flanagan Belytschko formulation is similar to the standard form. The difference lies in the construction of the vector function of element nodal velocities, are constructed to be orthogonal to both linear velocity field and the rigid body field. . These Note • The Viscous Coefficient for hourglass forces usually varies between 0.05 and 0.15. The default value is 0.1. • The sum of the hourglass forces applied to an element is normally zero. The momentum of the system is therefore unaffected by hourglass forces. • The hourglass forces do however do work on the nodes of the elements. The energy associated with hourglass forces is a) stored locally in the specific internal energy of the element b) recorded globally over the entire model and available to review via the Solution Output, Energy Summary. Static Damping The Explicit Dynamics system is primarily designed for solving transient dynamic events. Using the static damping option, a static equilibrium solution can also be obtained. The procedure is to introduce a damping force which is proportional to the nodal velocities and which is aimed to critically damp the lowest mode of oscillation of the static system. The solution is then computed in time in the normal manner until it converges to an equilibrium state. The user is required to judge when the equilibrium state is achieved. If the lowest mode of the system has period T then we may expect the solution to converge to the static equilibrium state in a time roughly 3T if the value of T is that for critical damping. When the dynamic relaxation option is used the velocity update is modified to where the Static Damping Coefficient, Rd, is input by the user. The value of Rd for critical damping of the lowest mode is where T is the period of the lowest mode of vibration of the system (or a close approximation to it). Usually A reasonable estimate of T must be used to ensure convergence to an equilibrium state but if the value of T is not known accurately then is it recommended that the user overestimates it, rather than underestimating it. Approximate values of ∆t and T can usually be obtained by first performing a dynamic analysis without static damping. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1275 Appendix F. Explicit Dynamics Theory Guide A static damping coefficient may be defined, or removed, at any point during an Explicit Dynamic simulation. Typical examples of its use would be: • To establish an initial stress distribution in a structure, prior to solving a transient dynamic event. For example applying gravity to a structure. • To establish the final static equilibrium position of a structure after it has experienced a transient dynamic event. For example finding the equilibrium position of structure after it has undergone large plastic deformation during a dynamic event. Solver Controls Hexahedral Elements The preferred element for solid bodies in Explicit Dynamics systems is the eight node reduced integration hexahedral. These elements are well suited to transient dynamic applications including large deformations, large strains, large rotations and complex contact conditions. The basic element characteristics are Connectivity 8 Node Nodal Quantities Position, Velocity, Acceleration, Force Mass (lumped mass matrix) Element Quantities Volume, Density, Strain, Stress, Energy Other material state variables Material Support All available materials Points to Note Preferred element for Explicit Dynamics Reduced integration, constant strain element Requires hourglass damping to stabilize zero energy “hourglass” modes (see section Damping Controls, Hourglass Damping) The default Integration Type for hexahedral elements is the Exact option. Here the element formulation based upon the work of Wilkins [8 (p. 1285)] results in an exact volume calculation even for distorted elements. This formulation is therefore the most accurate option, especially if the faces of the hex elements become warped. This is also computationally the most expensive formulation. It is possible to speed-up simulations by using the 1pt Gaussian quadrature integrated hexahedral element. This uses the element formulation described by Hallquist [9 (p. 1285)]. There will be some loss in accuracy when using this formulation with warped element faces which are common place in large deformation analysis. 1276 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Tetrahedral Elements Linear 4 noded tetrahedron elements are available for use in Explicit Dynamic analysis. Connectivity 4 Node Nodal Quantities Position, Velocity, Acceleration, Force Mass (lumped mass matrix) Additionally ANP formulation: Volume, Pressure, Energy Additionally NBS: Volume, Density, Strain, Stress, Energy, Pressure and other material state variables Element Quantities Volume, Density, Strain, Stress, Energy Other material state variables Additionally NBS: If PUSO stability coefficient is set to a non-zero value, there is an additional variable set for all variables for the PUSO solver Material Support SCP: All available materials Only Isotropic materials can be used with the ANP formulation Only ductile materials can be used with the NBS formulation Points to Note Only the ANP and NBS are recommended for use in majority tetrahedral meshes For NBS models exhibiting zero energy modes, the Puso coefficient can be set to a non-zero value. A value of 0.1 is recommended. Reduced integration, constant strain element The four noded linear tetrahedron is available with three forms of Pressure Integration • Standard Constant pressure integration (SCP), Zienkiewicz [10 (p. 1285)]. • Average Nodal Pressure (ANP) integration, based around the work of Burton [11 (p. 1285)]. • Nodal Based Strain (NBS) integration, based on work of (Bonet [21 (p. 1285)] and Puso [22 (p. 1285)]). The SCP tetrahedral element is a basic, constant strain element and can be used with all the material models. The element is intended as a “filler” element in meshes dominated by hexahedral elements. The element is known to exhibit locking behavior under both bending and constant volumetric straining (that is, plastic flow). If possible the element should therefore not be used in such cases. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1277 Appendix F. Explicit Dynamics Theory Guide The ANP tetrahedral formulation used here is an extension of the advanced tetrahedral element (Burton [11 (p. 1285)]) and can be used as a majority element in the mesh. The ANP tetrahedral overcomes problems of volumetric locking. The NBS tetrahedral formulation based on the work of (Bonet [21 (p. 1285)] and Puso [22 (p. 1285)]) is a further extension of the ANP tetrahedral element and can also be used as a majority element in the mesh. The NBS tetrahedral overcomes both problems of volumetric and shear locking, therefore is recommended over the other two tetrahedral formulations for models involving bending. Figure: Comparison of results of a Taylor test solved using SCP, ANP and NBS Tetrahedral elements. Results using NBS and ANP tetrahedral elements compare more favourably with experimental results than results using SCP (see table below). Tet-SCP Tet-ANP Tet-NBS Table F.3 Comparison of the performance of SCP, ANP, NBS and hex elements in a model involving bending. The displacement of the beam with NBS tetrahedral elements is the most similar to the beam meshed with hexahedral elements as it does not exhibit shear locking as is seen in the beams solved using SCP and ANP tetrahedral elements. Experiment SCP Tet ANP Tet NBS Tet Cylinder length (mm) 31.84 30.98 30.97 31.29 Impact diameter (mm) 12.0 10.66 11.32 11.28 1278 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Figure: Example bending test using SCP (1), ANP (2), NBS tetrahedral (3), and hex (4) elements. The displacement of the beam with NBS tetrahedral elements is the most similar to the beam meshed with hexahedral elements as it does not exhibit shear locking. Figure: Taylor test: Iron cylinder impacting rigid wall at 221m/s. Good correlation between ANP and Hex element results is obtained Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1279 Appendix F. Explicit Dynamics Theory Guide Figure: Example pull out test simulated using both hexahedral elements and ANP tetrahedral elements. Similar plastic strains and material fracture are predicted for both element formulations used. Pentahedral Elements Linear 6 noded pentahedral elements are available for use in Explicit Dynamics analysis. Connectivity 6 Node Nodal Quantities Position, Velocity, Acceleration, Force Mass (lumped mass matrix) Element Quantities All available materials Other material state variables Material Support All available materials Points to Note Reduced integration, constant strain element The pentahedral element is a basic constant strain element and is intended as a filler element in meshes dominated by hexahedral elements. Pyramid Elements Pyramid elements are not recommended for Explicit Dynamic simulations. Any pyramid elements present in the mesh will be converted to 2 tetrahedral elements in the solver initialization phase. Results are mapped back onto the Pyramid element for postprocessing purposes. 1280 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Shell Quad Elements Bilinear 4 noded quadrilateral shell elements are available for use in Explicit Dynamics analysis. Connectivity 4 Node Nodal Quantities Position, Velocity, Angular Velocity, Acceleration, Force, Moment Mass (lumped mass matrix) Element Quantities Strain, Stress, Energy Other material state variables Data stored per layer Material Support Linear elasticity must be used Equations of state and porosity are not applicable to shell elements Pressure dependant material strength is not applicable to shell elements Points to Note Reduced integration, constant strain element Based on Mindlin plate theory, transverse shear deformable Shells have zero through thickness stress and are therefore not suitable for modelling wave propagation through the thickness of the surface body The bilinear 4 noded quadrilateral shell element is based on the corotational formulation presented by Belytschko-Tsay [13 (p. 1285)]. The element has one quadrature point per layer and is stabilized using hourglass control. By default, additional curvature terms are added for warped elements in accordance with Belytschko [14 (p. 1285)]. This option can be deactivated using the Shell BWC Warp Correction setting in the Solver Controls. The number of through thickness integration points (sublayers) is controlled through the analysis settings option Solver Controls, Shell Sublayers. The default value is 3. The thickness of the shell element is updated during the simulation in accordance with the material response. The update is carried out at the shell nodes by default. The principal inertia of the shell nodes is recalculated every time increment (cycle) by default. This is the most robust method. It is more efficient to rotate the principal inertias rather than recalculate (although less robust for certain applications). The “Shell Thickness Update” option can be used to select this more efficient inertial update method. Shell Tri Elements Linear 3 noded triangular shell elements are available for use in Explicit Dynamics analysis. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1281 Appendix F. Explicit Dynamics Theory Guide Connectivity 3 Node Nodal Quantities Position, Velocity, Angular Velocity, Acceleration, Force, Moment Mass (lumped mass matrix) Element Quantities Volume, Density, Stress, Energy Other material state variables Data stored per layer Material Support Linear elasticity must be used Equations of state and porosity are not applicable to shell elements Pressure dependant material strength is not applicable to shell elements Points to Note Reduced integration, constant strain element This element is only recommended for use as a “filler” element in quad dominant shell meshes Shells have zero through thickness stress and are therefore not suitable for modelling wave propagation through the thickness of the surface body The bilinear 3 noded, C0, triangular shell element is based on the formulation presented by Belytschko et al. [15 (p. 1285)]. The number of through thickness integration points (sublayers) is controlled through the analysis settings option Solver Controls, Shell Sublayers. The default value is 3. The thickness of the shell element is updated during the simulation in accordance with the material response. The update is carried out at the shell nodes by default. Beam Elements Linear 2 noded beam elements are available for use in Explicit Dynamics analysis. Connectivity 1282 2 Node Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Analysis Settings Nodal Quantities Position, Velocity, Angular Velocity, Acceleration, Force, Moment Mass (lumped mass matrix) Element Quantities Resultant Strain/Stress, Energy Other material state variables Material Support Linear elasticity must be used Equations of state and porosity are not applicable to beam elements Pressure dependant material strength is not applicable to beam elements Points to Note Supports symmetrical circular, square, rectangular, IBeam and general cross sections Beams have zero transverse stress and are therefore not suitable for modelling wave propagation across the cross section The 2 noded beam element is based on the resultant beam formulation of Belytschko [16 (p. 1285)] and allows for large displacements and resultant elasto-plastic response. Erosion Controls Erosion is a numerical mechanism for the automatic removal (deletion) of elements during a simulation. The primary reason for using erosion is to remove very distorted elements from a simulation before the elements become inverted (degenerate). This ensures that the stability timestep remains at a reasonable level and solutions can continue to the desired termination time. Erosion can also be used to allow the simulation of material fracture, cutting and penetration. There are a number of mechanisms available to initiate erosion of elements. The erosion options can be used in any combination. Elements will erode if any of the criteria are met. Geometric Strain Geometric strain is a measure of the distortion of an element and is calculated from the principal strain components as Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1283 Appendix F. Explicit Dynamics Theory Guide This erosion option allows removal of elements when the local element geometric strain exceeds the specified value. Typical values range from 0.5 to 2.0. The default value of 1.5 can be used in most cases. Custom result EFF_STN can be used to review the distribution of effective strain in the model. Timestep This erosion option allows removal of elements when the local element timestep, multiplied by the time step safety factor falls below the specified value. Custom result TIMESTEP can be used to review the time step for each element. Material Failure Using this option, elements will automatically erode if a material failure property is defined in the material used in the elements, and the failure criteria has been reached. Elements with materials including a damage model will also erode if damage reaches a value of 1.0. Retained Inertia If all elements that are connected to a node in the mesh are eroded, the inertia of the resulting free node can be retained. The mass and momentum of the free node is retained and can be involved in subsequent impact events to transfer momentum in the system. If this option is set to No, all free nodes will be automatically removed from the simulation. Note • Erosion is not a physical process and should be used with caution. • The internal energy of elements which are eroded is always removed from the system. This energy is accumulated in the work done term for global energy conservation purposes. References The following references are cited in this appendix: 1. R. Courant, K. Friedrichs and H. Lewy, "On the partial difference equations of mathematical physics", IBM Journal, March 1967, pp. 215-234 2. Meyers, M. A., (1994) “Dynamic behaviour of Materials”, John Wiley & Sons, ISBN 0-471-58262-X. 3. Zukas, J. A., (1990) “High velocity impact dynamics”, John Wiley & Sons, ISBN 0-471-51444-6 4. von Neumann, J., Richtmeyer, R. D. (1950)., “A Method for the Numerical Calculation of Hydrodynamic Shocks”, J. App. Phys., 21, pp 232-237, 1950 5. Wilkins, M. L., (1980). “Use of Artificial Viscosity in Multidimensional Fluid Dynamic Calculations”, J. Comp. Phys., 36, pp 281-303, 1980 6. Kosloff D., Frazier G. A., (1978) “Treatment of hourglass patterns in low order finite element codes”, Int. J. Num. Anal. Meth. Geomech. 2, 57-72 1284 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. References 7. Flanagan D. P., Belytschko T., (1981) “A uniform strain hexahedron and Quadrilateral and Orthogonal Hourglass Control”, Int. J. Num. Meth. Eng. 17, 679-706. 8. Wilkins, M. L., Blum, R. E., Cronshagen, E. & Grantham, P. (1974). “A Method for Computer Simulation of Problems in Solid Mechanics and Gas Dynamics in Three Dimensions and Time.” Lawrence Livermore Laboratory Report UCRL-51574, 1974 9. Hallquist, J. O., (1982) "A theoretical manual for DYNA3D, LLNL Report UCID-19401. 10. Zienkiewicz, O. C., Taylor, R. L., "The finite element method, Volume 1", ISBN 0-07-084174-8 11. Burton, A..J.. (1996) 'Explicit, Large Strain, Dynamic Finite Element Analysis with Applications to Human Body Impact Problems', PhD Thesis, University of Wales. 12. Wilkins, M. L., Blum, R. E., Cronshagen, E., & Grantham, P. (1974). “A Method for Computer Simulation of Problems in Solid Mechanics and Gas Dynamics in Three Dimensions and Time.” Lawrence Livermore Laboratory Report UCRL-51574, 1974 13. Belytschko, T., et al. (1984), “Explicit algorithms for the nonlinear dynamics of shells”, Comp. Meth. Appl. Mech Eng., 42, 225-251. 14. Belytschko, T., et al. (1992), “Advances in one-point quadrature shell elements”, Comp. Meth. Appl. Mech Eng., 1992, 93-107. 15. Belytschko, T., et al. (1984), “A C0 Triangular Plate Element with One-point Quadrature”, Int. J. Num. Meth. Engng., 20, 787-802, 1984. 16. Belytschko, T. et al., 1977, “Large Displacement Analysis of Space Frames”, Int. J. Num. Meth. And Anal. Mech. Engng., 11, 65-84, 1977. 17. Godunov, S. K. (1959), "A Difference Scheme for Numerical Solution of Discontinuous Solution of Hydrodynamic Equations", Math. Sbornik, 47, 271-306, translated US Joint Publ. Res. Service, JPRS 7226, 1969. 18. Noh, W. F. and Woodward, P., “SLIC (Simple line interface calculation),” in Lecture Notes in Physics (A. I. van der Vooren and P. J. Zandbergen, eds.), pp. 330–340, Springer-Verlag, 1976. 19. Van Leer, B (1977). “Towards the Ultimate Conservative Difference Scheme. IV. A new Approach to Numerical Convection”, J. Comp. Phys. 23, pp 276-299, 1977. 20. Van Leer, B (1979). “Towards the Ultimate Conservative Difference Scheme. V. A Second Order Sequel to Godunov’s Method”, J. Comp. Phys. 32, pp 101-136, 1979. 21. Bonet J., Marriott H., Hassan O. “An averaged nodal deformation gradient linear tetrahedral element for large strain explicit dynamics applications”. Communications in Numerical Methods in Engineering 2001; 17, 551-561. 22. Puso M. A.,Solberg J. “A stabilized nodally integrated tetrahedral”. International Journal for Numerical Methods in Engineering 2006; 67, 841-867. Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1285 1286 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. Index Symbols 2-D analyses - description and characteristics, 332 2–parameter mooney-rivlin model, 1196 3–parameter mooney-rivlin model, 1196 5–parameter mooney-rivlin model, 1197 9–parameter mooney-rivlin model, 1197 A acceleration load description, 563 object reference, 1021 acceleration object reference, 1021 adaptive convergence, 787 adaptivity, 787 add linearized stress, 647 add offset no ramping contact region setting , 418 add offset ramped effects contact region setting, 418 adding beams, 483 adjust to touch contact region setting, 418 advanced contact region settings - listed and defined, 418 alert object reference, 979 alert object reference, 979 ambient temperature - in radiation load, 586 analysis 2-D analyses - description and characteristics, 332 apply loads and supports step, 14 apply mesh controls step, 9 apply preview mesh step, 9 approach - overall steps, 1 assign behavior to parts step, 6 attach geometry step, 2 create analysis system step, 1 create report step, 17 define initial condition step, 12 define resources step, 2 establish analysis settings, 9 interface - listing of components, 233 options - listed and described, 303 review results step, 16 role in Workbench, 1 set connections options step, 8 solve step, 15 types - listed, 17 window components - layout and description, 233 analysis data management - analysis settings, 549 analysis settings establishing - overall analysis step, 9 for explicit dynamics analyses, 511 for most analysis types, 499 object reference, 980 role of time, 525 steps and step controls overall topics, 525 topic listing, 499 analysis settings analysis data management, 549 analysis settings and solution options, 303 analysis settings object reference, 980 analysis settings output controls, 545 analysis settings rotordynamics controls, 551 analysis topics - special, 137 analysis type applicable analysis settings, 499 analysis types design assessment, 17 electric, 32 explicit dynamics, 35 harmonic, 57 linear buckling, 20 listing, 17 magnetostatic, 66 modal, 25 random vibration, 70 response spectrum, 75 rigid dynamics, 102, 161 static structural, 79 steady-state thermal, 84 thermal-electric, 87 transient structural, 91 transient thermal, 133 angular periodicity, 339 angular velocity object reference, 980 angular velocity object reference, 980 animation controls, 743 annotations basics, 396 environment, 396 highlight and selection graphics, 396 message, 396 positioning, 396 probe - in result context toolbar, 287 rescaling, 396 solution, 396 ANSYS CFX- solving with fluid solid interface , 607 ANSYS Workbench safety tools, 658 ANSYS Workbench product adaptive solutions, 787 anti-periodic symmetry type, 339 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1287 Index anti-symmetric electromagnetic symmetry type, 337 anti-symmetric structural symmetry type, 336 anti-virus causing crash - troubleshooting, 1084 APDL programming - using, 860 applying loads and supports overall analysis step, 14 applying pre-stress effects, 30 assemblies, 315 assemblies missing parts - troubleshooting, 1078 assemblies of surface bodies, 320 associative and non-associative coordinate systems, 390 asymmetric behavior contact region setting, 414 asynchronous solutions description, 754 troubleshooting, 1082 attaching geometry overall analysis step, 2 augmented Lagrange formulation contact region setting , 418 auto asymmetric behavior contact region setting , 414 Autodesk Inventor assigning parameters, 869 autohiding windows, 252 automatic contact, 426 automatic time stepping analysis settings, 527 automatically generated connections, 407 averaged vs. unaveraged contour results, 721 axial force result object reference, 1047 axisymmetric behavior - 2-D simulation, 332 B back-face culling - in view menu, 280 background solutions troubleshooting, 1082 beam, 483 beam end release object reference, 1001 beam end release object reference, 1001 beam end releases, 486 beam probe result, 680 beam results, 680 beam tool result description, 670 object reference, 1047 beam tool result object reference, 1047 bearing load description, 573 object reference, 1021 bearing load object reference, 1021 behavior contact region setting, 414 1288 bending moment result object reference, 1047 bending stress - beam tool, 670 biaxiality indication result in fatigue tool description, 699 object reference, 1003 biaxiality indication result object reference, 1003 bin size - fatigue simulations, 696 blips, 241 body description, 315 hide, 318 object reference, 983 suppress, 318 body interaction object reference, 986 body interaction object reference, 986 body interaction types, 494 bonded, 496 frictional, 495 frictionless, 494 reinforcement, 497 body interactions object reference, 985 body interactions folder properties body self contact, 492 contact detection, 489 edge on edge contact, 494 element self contact, 492 formulation, 491 limiting time step velocity, 494 listing, 488 pinball factor, 493 shell thickness, 492 time step safety factor, 493 tolerance, 493 body interactions in explicit dynamics analyses connections, 487 body interactions object reference, 985 body object reference, 983 body scoped result tracker, 781 body self contact for body interactions, 492 bolt pretension load description, 575 object reference, 1021 bolt pretension object reference, 1021 bonded body interaction type, 496 bonded type contact region setting, 414 boundary condition, 557 boundary conditions - electromagnetic, 591 boundary scoped result tracker, 784 box select, 241 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. box zoom - graphics toolbar button, 285 breakable setting for body interaction object, 496 brittle strength, 1208 C CAD parameters, 869 CAD systems general information, 1071 isotropic material limitation, 1072 multiple versions, 1072 callouts in details view, 274 campbell diagram chart result object reference, 1047 capped isosurfaces, 287, 745 CFD load transfer convections, 145 structural, 144 surface temperatures, 145 chart object reference, 988 chart and table, 729 chart object reference, 988 charts control, 241 tips, 241 clean results data, 722 CLOCAL Mechanical APDL application command - use, 642 color by parts, 317 colors - contact initial information table, 666 combined stress - beam tool, 670 commands - using the Mechanical APDL application, 860 commands object reference, 988 commands objects available parameter, 860 conflicts between the Mechanical and Mechanical APDL applications, 860 description, 856 features, 857 input arguments, 860 object reference, 988 solver target, 860 step selection mode, 860 comment context toolbar - screenshot and description, 287 object reference, 989 comment object reference, 989 compaction EOS linear, 1235 compaction EOS nonlinear, 1236 composite results, 723 compression only support description, 559 object reference, 1021 compression only support object reference , 1021 condition types - listed, 611 conditions constraint equations, 611 coupling, 611 joint, 562 nodal orientation, 611 pipe idealization, 611 conductor load current excitation for solid source conductors, 597 description, 593 object reference, 1021 solid body as conductor, 594 stranded source body as conductor, 598 stranded source conductor, 599 voltage excitation for solid source conductors, 596 conductor object reference, 1021 conflicts - between workbench and the Mechanical APDL application when using commands objects, 860 conflicts - thermal boundary condition, 855 conflicts with contact region(s) using MPC troubleshooting , 1081 conflicts with remote boundary condition(s) troubleshooting, 1081 connection detection global setting, 403 connection group object reference, 991 connection group object reference, 991 connection lines with remote point, 384 connections context toolbar - screenshot and description, 287 general description, 402 global settings - listed and defined, 403 object reference, 990 setting options - overall analysis step, 8 connections object reference, 990 constraint equation description, 612 constraint equation condition object reference, 1021 constraint equation object reference, 1021 constraint equations were not properly matchedtroubleshooting, 1079 constraint type contact region setting, 418 construction geometry object reference, 993 construction geometry object reference, 993 contact advanced region settings - listed and defined, 418 automatic, 426 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1289 Index controlling transparency for regions - animated example, 427 definition region settings - listed and defined, 414 ease of use features - listed, 426 flipping contact/target scope settings - animated example, 429 general description, 402 hiding bodies not scoped to contact region - procedure, 428 identifying regions - procedure, 429 initial, 666 loading region settings - procedure, 430 locating bodies without contact - application and procedure, 431 locating parts without contact - application and procedure, 431 manual, 426 merging regions - procedure, 430 options, 303 reactions, 666 region object reference, 994 region settings - categories, 402 renaming regions - animated example, 428 resetting regions to defaults - procedure, 431 results, 649 saving region settings - procedure, 430 scope region settings - listed and defined, 412 setting conditions manually - guidelines and procedure, 426 tool, 666 contact based reactions, 651 contact bodies scope region setting, 412 contact detection for body interactions, 489 contact region object properties electromagnetic analyses, 996 explicit dynamics analyses, 995 structural analyses, 995 thermal analyses, 996 contact region object reference, 994 contact region settings - categories, 402 contact region(s) not in initial contact - troubleshooting , 1080 contact scope region settings, 412 contact scoped result tracker, 784 contact sizing object reference, 1026 contact sizing object reference, 1026 contact tool result description, 666 object reference, 997 contact tool result object reference, 997 context toolbars 1290 location in the Mechanical application window, 233 overall description and listing, 287 contour options - in result context toolbar, 287 contour results, 732 contours during solve, 774 controlling transparency for contact regions - animated example, 427 convection load description, 584 object reference, 1021 convection object reference, 1021 convections at CFD boundary, 145 convective heat transfer, 584 convergence object reference, 998 plots, 769 convergence criteria analysis setting , 542 convergence object reference, 998 convergence options, 303 converting boundary conditions to nodal degree-offreedom constraints, 854 coordinate system object reference, 1000 coordinate systems applying local coordinate systems, 392 create section plane, 393 creating, 287, 389 global, 287 importing, 392 object reference, 1000 orientation, 391 overall topics, 389 principal axis, 391 reference number, 389 references, 392 transferring to the Mechanical APDL application,395 transformations, 391 use in specifying joint locations., 392 using, 389 coordinate systems object reference, 1000 coordinate systems result object reference, 1047 coordinate systems result object reference, 1047 coordinate systems results, 732 coordinates - graphics toolbar button, 285 coupling load description, 612 cowper symonds strength, 1204 crack softening, 1246 creep controls, 537 creep strain - equivalent, 645 Creo Parametric Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. assigning parameters, 869 crushable foam, 1232 current density result description, 689 object reference, 1047 current density result object reference, 1047 current excitation stranded source conductor body, 599 current excitation for solid conductors current object reference, 1021 current excitation for solid source conductors description, 597 current load description, 591 current object reference, 1021 cursors - rotation, 241 cursors - triad and rotation, 301 cyclic controls, 537 cyclic region, 342 object reference, 1038 cyclic region object reference, 1038 cyclic symmetry in a modal analysis, 345 cyclic symmetry in a static structural analysis, 343 cyclic symmetry in a thermal analysis, 351 cylindrical joints, 436 cylindrical support description, 560 object reference, 1021 cylindrical support object reference, 1021 cylindrical surface direction, 632 D damage matrix result in fatigue tool description, 699 object reference, 1003 damage matrix result object reference, 1003 damage result in fatigue tool description, 699 object reference, 1003 damage result object reference, 1003 damping controls - analysis settings, 542 data standard toolbar button - commands and descriptions, 283 data transfer POLYFLOW to Mechanical , 158 database file - saving results as a dsdb, 852 as a Mechanical APDL database file, 852 decay coefficient for body interaction object, 495 define initial condition overall analysis step, 12 definition contact region settings - listed and defined, 414 deformation , 635 deformed shape - scaling in result context toolbar, 287 degrees - in main menu, 280 degrees of freedom and joint types, 436 density, 1193 depth picking , 241 design assessment analysis type, 17 details view description and user interactions, 274 location in the Mechanical application window, 233 detonation point object reference, 1021 detonation point load, 608 detonation point object reference, 1021 dimensions - geometry, 6 direct fe fe displacement, 615 fe rotation, 615 nodal force, 615 nodal orientation, 615 Direct FE, 617 FE Displacement, 1021 FE Rotation, 1021 Nodal Force, 1021 Nodal Orientation, 1021 Nodal Pressure, 1021 direct fe object reference, 1001 direct fe types - listed, 615 direct stress result in beam tool description, 670 object reference, 1047 direct stress result object reference, 1047 direction defaults, 241 defining, 632 graphics toolbar button, 285 selecting, 241 directional acceleration result description, 635 object reference, 1047 directional acceleration result object reference, 1047 directional current density result object reference, 1047 directional deformation result description, 635 object reference, 1047 directional deformation result object reference , 1047 directional electric field intensity result object reference, 1047 directional field intensity result Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1291 Index object reference, 1047 directional field intensity result object reference, 1047 directional flux density result object reference, 1047 directional flux density result object reference, 1047 Directional Force electromagnetic result description, 689 directional force electromagnetic result object reference, 1047 directional force result object reference, 1047 directional heat flux result description, 686 object reference, 1047 directional heat flux result object reference , 1047 directional magnetic field intensity result description, 689 directional magnetic flux density result description, 689 directional velocity result description, 635 object reference, 1047 directional velocity result object reference, 1047 displacement edge, 553 object reference, 1021 remote, 553 surfaces, 553 vertex, 553 displacement object reference, 1021 displacement support object reference, 1021 display options for result tracker graphs, 785 display points - in solution information, 769 Distance Based Average Comparison option for Mapping Validation, 1105 docking windows, 252 duplicate - in main menu, 280 dynamic coefficient for body interaction object, 495 dynamic legend, 746 E ease of use contact features - listed, 426 edge direction, 632 edge on edge contact for body interactions, 494 edge options - in result context toolbar, 287 eigen response analysis type, 20 elastic strain intensity result description, 641 object reference, 1047 elastic strain intensity result object reference, 1047 elastic support description, 562 1292 object reference, 1021 elastic support object reference, 1021 electric analysis type, 32 electric loads, 562 electric potential result description, 688 object reference, 1047 electric potential result object reference, 1047 electric results, 693 electric voltage result object reference, 1047 electromagnetic loads - listed, 562, 591 electromagnetic periodic symmetry, 339 electromagnetic-thermal interaction, 146 electromagnetic-thermal load import, 146 element self contact for body interactions, 492 element through the thickness - troubleshooting,1077 elemental coordinate systems results, 732 emissivity - in radiation load, 586 enclosure - in radiation load, 586 energy accuracy tolerance analysis setting, 542 energy result, 654 environment annotations, 396 context toolbar - screenshot and description, 287 object reference, 1002 environment filtering of GUI, 238 environment object reference, 1002 Equation of state, 1185 equations of state, 1223 ideal gas, 1224 equivalent alternating stress result in fatigue tool description, 699 object reference, 1003 equivalent alternating stress result object reference, 1003 equivalent creep strain result description, 645 object reference, 1047 equivalent plastic strain result description, 644 object reference, 1047 equivalent plastic strain result object reference , 1047 equivalent stress result description, 640 object reference, 1047 equivalent stress result object reference, 1047 equivalent total strain result description, 645 object reference, 1047 eroded nodes, 733 error - magnetic result Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. description, 691 error result structural, 642 thermal, 687 error status symbol, 235 ESOL command, 711 Euler angle sequence, 642 excitations - electromagnetic, 591 explicit dynamics recommended guidelines when using pre-stress, 55 Explicit Dynamics, 557 detonation point, 608 explicit dynamics analysis LSDYNA commands, 1107 explicit dynamics analysis settings, 511 explicit dynamics analysis type, 35 Explicit Dynamics system analysis settings, 1270 body scoped result tracker, 781 boundary scoped result tracker, 784 elastic waves, 1259 erosion controls, 1283 Euler (Virtual) solutions, 1265 Euler-Lagrange Coupling, 1268 Eulerian reference frame, 1261 explicit time integration, 1256 force reaction result tracker, 784 implicit time integration, 1256 Lagrangian reference frame, 1261 mass scaling, 1258 material properties, 1268 moment reaction result tracker, 784 multiple material transport, 1268 operation of , 1254 plastic waves, 1259 point scoped result tracker, 777, 784 shell coupling, 1269 shock waves, 1260 solver controls, 1276 sub-cycling, 1270 theory, 1253 wave propagation, 1258 Explicit Material Library, 1187 explicit transient dynamic analysis, 1255 export description, 302 options, 303 exported file saved to disk but microsoft office failed to load - troubleshooting, 1075 exporting load history, 624 extend selection description, 241 graphics toolbar button, 285 extend to adjacent selection, 241 extend to connection selection, 241 extend to limits selection, 241 External Data Master file, 154 External Thickness, 1015 External Thickness reference, 1015 F failed to load microsoft office application troubleshooting, 1079 failure, 1241 Grady Spall, 1249 Johnson cook, 1248 plastic strain, 1242 post, 1241 principal strain, 1243 principal stress, 1242 stochastic, 1244 tensile pressure, 1246 fatigue sensitivity result in fatigue tool description, 699 object reference, 1003 fatigue sensitivity result object reference , 1003 fatigue simulations loading options, 696 material properties, 695 options, 303 overview, 695 results, 699 strain-life, 695 stress-life, 695 user life units, 696 fatigue tool result description, 699 object reference, 1003 fatigue tool result object reference , 1003 fe displacement description, 618 FE Displacement object reference, 1001 fe rotation description, 619 FE Rotation object reference, 1001 figure description, 401 object reference, 1006 figure object reference, 1006 file management in the Mechanical application, 792 file names - CAD limitation, 1072 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1293 Index filtering GUI based on environment, 238 filtering result tracker graphs, 785 filters selection, 241 fit - graphics toolbar button, 285 fixed joints, 436 fixed rotation object reference, 1021 fixed rotation support face - description, 561 object reference, 1021 fixed support edge - description, 552 object reference, 1021 surface - description, 552 vertex - description, 552 fixed support object reference, 1021 flip reference and mobile for joints, 466 flipping contact/target scope settings - animated example, 429 flipping periodic low and periodic high settings, 352 fluid solid interface description, 607 fluid solid interface load object reference, 1021 fluid solid interface object reference, 1021 fluid surface object reference, 1006 fluid surface object reference, 1006 fluid-structure interaction convections, 145 surface temperatures, 145 fluid-structure interaction - one-way, 143 fluid-structure interaction - overall description, 142 fluid-structure interaction - two-way, 146 fluid-structure interface face forces, 144 flux linkage result description, 690 object reference, 1047 force load description, 570 object reference, 1021 force object reference, 1021 formulation contact region setting, 418 formulation for body interactions, 491 foundation stiffness - in elastic support , 562 frequency response, 655 frequency response result object reference, 1047 frequency response result object reference, 1047 frequency simulations options, 303 1294 friction coefficient contact region setting , 418 friction coefficient for body interaction object, 495 frictional body interaction type, 495 frictional stress result in contact tool description, 666 object reference, 997 frictional stress result object reference , 997 frictional type contact region setting, 418 frictionless body interaction type, 494 frictionless support description, 558 object reference, 1021 frictionless support object reference, 1021 frictionless type contact region setting, 418 FSI - one-way, 143 FSI - overall description, 142 FSI - two-way, 146 full integration scheme, 317 function loads, 626 G gap result in contact tool description, 649 object reference, 997 gap result object reference, 997 gap sizing object reference, 1026 gap sizing object reference, 1026 gap tool context toolbar - screenshot and description, 287 object reference, 1026 gap tool object reference , 1026 gasket bodies, 387 gasket mesh control, 387 object reference, 1007 gasket mesh control object reference, 1007 gasket results, 682 gasketresults, 388 gaskets using, 387 general joints, 436 generalized plane strain behavior in 2-D analyses, 332 load description, 578 reactions, 651 using, 333 generate connections on update global setting, 403 generating reports publishing, 865 tables, 865 geometric axis direction, 632 geometry, 287 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. attach - overall analysis step, 2 context toolbar - screenshot and description, 287 object reference, 1008 options, 303 tab, 240 updating, 2 window, 240 geometry object reference, 1008 global connection settings - listed and defined , 403 global coordinate system description, 287 object reference, 1010 global coordinate system object reference, 1010 glossary, 1093 go to options in tree outline, 237 go to selected items - worksheet, 266 go to selected items in tree - worksheet, 266 Graph window, 268 graphics blips, 241 control, 241 options, 303 options in result context toolbar, 287 painting, 241 picking, 241 tips, 241 toolbar - commands and descriptions, 285 toolbar location in the Mechanical application window, 233 graphics - topic listing, 396 graphics option screenshot and description, 298 show mesh, 298 group by global connection setting, 403 H harmonic analysis, 57 harmonic analysis linked to modal, 64 heat flow load description, 587 object reference, 1021 heat flow object reference, 1021 heat flux load description, 589 object reference, 1021 heat flux object reference, 1021 heat flux results, 686 heat reaction result description, 687 hidden status symbol, 235 hide all other bodies, 318 hide body, 318 hide faces, 319 hide items, 239 hide other bodies for joints, 466 hiding bodies not scoped to contact region - procedure, 428 hydrostatic pressure load description, 569 object reference, 1021 hydrostatic pressure object reference, 1021 hysteresis result in fatigue tool description, 699 object reference, 1003 hysteresis result object reference , 1003 I Icepak Mechanical data transfer, 151 transient, 152 identifying contact regions - procedure, 429 illogical reaction results - troubleshooting, 1079 image from file, 1011 image object reference, 1011 impedance, 557 implicit transient dynamic analysis, 1254 import external file, 153 external thickness, 154 Import thickness, 324 imported body force density load, 601 imported body temperature load, 602 imported convection coefficient load, 603 imported heat flux load, 603 imported heat generation load, 604 Imported Layered Section, 1011 Imported Layered Section reference, 1011 imported load electromagnetic-thermal, 146 imported loads, 630 Imported Loads, 1012 Imported loads reference, 1012 imported pressure load, 604 imported surface force density, 605 imported temperature load, 605 Imported Thickness, 1014 Imported Thickness (Group), 1015 Imported Thickness reference, 1014–1015 importing coordinate systems, 392 importing load history, 623 in process solutions, 754 inductance result description, 689 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1295 Index object reference, 1047 inertia relief analysis setting, 533 inertia tensor is too large - troubleshooting, 1079 inertial loads - listed, 562 infinite life - fatigue simulations, 696 inflation object reference, 1026 inflation object reference, 1026 initial condition object reference, 1016 initial condition object reference, 1016 initial contact, 666 initial information object in contact tool description, 666 initial information result in contact tool colors in table, 666 description, 666 object reference, 997 initial information result object reference, 997 initial temperature object reference, 1017 initial temperature object reference, 1017 initial time increment problems - troubleshooting ,1085 inside pinball search direction contact region setting, 418 insufficient disk space - troubleshooting, 1076 integration scheme, 317 interaction loads - listed, 562 interface - listing of components, 233 interface behavior based on license levels, 239 interface treatment contact region setting , 418 internal heat generation load description, 590 object reference, 1021 internal heat generation object reference , 1021 invalid material properties - troubleshooting , 1075 invert suppressed body set, 239 iso - graphics toolbar button, 285 isotropic elasticity, 1193 isotropic materials - CAD limitation, 1072 iterative solver problem - troubleshooting, 1077 J Johnson cook strength, 1203 Johnson-holmquist strength, 1211 joint object reference, 1018 joint checker, 466 joint condition object reference, 1021 joint condition object reference, 1021 joint legend, 466 1296 joint load description, 581 joint object reference, 1018 joint probe problems - troubleshooting, 1086 joint probes results, 677 joints automatic creation, 464 characteristics, 433 detecting overconstrained conditions, 469 ease of use features, 466 example, 448, 458 manual creation, 442 topics, 433 types, 436 joule heat result object reference, 1047 K kelvin, 852 keyboard support, 285 known temperature load, 584 L large deflections analysis setting, 533 large deformation effects are active - troubleshooting , 1079 large deformation problems - troubleshooting, 1085 layered section object reference, 1019 layered section object reference, 1019 layered sections, 325 legend customization, 287 Library Explicit Material, 1187 license manager server problems - troubleshooting , 1086 licensed product issues - troubleshooting, 1084 life - fatigue user life units, 696 life result in fatigue tool description, 699 object reference, 1003 life result object reference, 1003 lighting controls, 401 limiting time step velocity for body interactions, 494 line bodies, 315 general description, 329 line pressure load description, 578 object reference, 1021 line pressure object reference, 1021 line search analysis setting, 542 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. linear buckling analysis type, 20 Linear Elastic, 1193 Linearized Equivalent Stress, 1047 Linearized Maximum Principal Stress, 1047 Linearized Maximum Shear Stress, 1047 Linearized Middle Principal Stress, 1047 Linearized Minimum Principal Stress, 1047 Linearized Normal Stress, 1047 Linearized Shear Stress, 1047 Linearized stress, 647 linearized stress error - troubleshooting, 1074 Linearized Stress Intensity, 1047 Linearized stresses, 1047 load transfer error - troubleshooting, 1074 load transfer mesh mapping, 1097 load types - listed, 562 loading contact region settings - procedure, 430 loading types - fatigue simulations, 696 loads and supports object reference, 1021 local coordinate system applying, 392 creating, 287 in coordinate system object reference, 1000 locating bodies without contact - application and procedure , 431 locating parts without contact - application and procedure , 431 look at - graphics toolbar button, 285 low/high cyclic symmetry - troubleshooting, 1087 ls-dyna analyses , 35 LSDYNA commands, 1107 M macros - usage and accessing, 313 magnetic error result, 691 object reference, 1047 magnetic error result object reference, 1047 magnetic field intensity result directional, 689 total, 689 magnetic flux boundary condition, 592 magnetic flux density result directional, 689 total, 688 magnetic flux parallel load description, 592 object reference, 1021 magnetic flux parallel object reference, 1021 magnetostatic analysis type, 66 magnetostatic results, 688 magnifier window - toggle graphics toolbar button, 285 main menu commands and descriptions, 280 location in the Mechanical application window, 233 manual contact, 426 manually insert connection objects, 407 mapped face meshing object reference, 1026 status symbol, 235 mapped face meshing object reference, 1026 mapping -CFD results, 145 Mapping Control Distance Based Average weighting, 1097 Manual enables modification of Advance Features, 1097 Program Controlled gives best accuracy, 1097 Shape Function weighting, 1097 Triangulation weighting, 1097 Mapping Validation objects, 1105 mass moment of inertia, 385 match control object reference, 1026 status symbol, 235 match control object reference, 1026 material properties nonlinear, 1195 material properties - fatigue, 695 material property usage in postprocessing, 723 materials, 6 assigning to parts - analysis step, 6 maximum bending stress result in beam tool description, 670 object reference, 1047 maximum bending stress result object reference ,1047 maximum combined stress result in beam tool description, 670 object reference, 1047 maximum combined stress result object reference,1047 maximum data points to plot - fatigue simulations ,696 maximum equivalent stress safety tool result description, 659 maximum offset for body interaction object , 496 maximum principal elastic strain result object reference, 1047 maximum principal stress result object reference ,1047 maximum principal stress/elastic strain result description, 640 object reference, 1047 maximum shear elastic strain result object reference, 1047 maximum shear stress result object reference, 1047 maximum shear stress safety tool result description, 661 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1297 Index maximum shear stress/elastic strain result description, 641 object reference, 1047 maximum tensile stress safety tool result description, 664 mean stress theory - fatigue simulations, 696 Mechanical APDL application - using commands, 860 Mechanical APDL application database file - saving results as, 852 Mechanical APDL application Euler angle sequence, 642 Mechanical APDL application input file - saving results as, 852 Mechanical APDL application memory options, 755 Mechanical APDL application plots , 860 Mechanical APDL application- conflicts with workbench when using commands objects, 860 Mechanical objects reference, 977 Mechanical tutorials, 166 memory options - the Mechanical APDL application setting defaults, 303 setting for a solution, 755 merging contact regions - procedure, 430 mesh connection, 470 object reference, 1024 snap to boundary, 470 mesh connection object reference, 1024 mesh control tools applying - overall analysis step, 9 object reference, 1026 mesh control tools object reference, 1026 mesh group object reference, 1028 mesh group object reference, 1028 mesh grouping object reference, 1029 mesh grouping object reference, 1029 mesh numbering, 374 object reference, 1029 mesh numbering object reference, 1029 mesh object reference, 1022 meshing context toolbar - screenshot and description, 287 messages window, 270 method mesh control tool object reference, 1026 method mesh control tool object reference, 1026 method scope contact region setting, 412 middle principal elastic strain result object reference, 1047 middle principal stress result object reference, 1047 middle principal stress/elastic strain result 1298 description, 640 object reference, 1047 minimum bending stress result in beam tool description, 670 object reference, 1047 minimum bending stress result object reference, 1047 minimum combined stress result in beam tool description, 670 object reference, 1047 minimum combined stress result object reference ,1047 minimum principal elastic strain result object reference, 1047 minimum principal stress result object reference, 1047 minimum principal stress/elastic strain result description, 640 object reference, 1047 miscellaneous options, 303 MO granular strength, 1223 modal object reference, 1030 modal analysis troubleshooting, 1089 modal analysis type, 25 modal object reference, 1030 model context toolbar - screenshot and description, 287 object reference, 1031 Model Material failure, 1186 Material strength, 1186 model object reference, 1031 Mohr-Coulomb stress safety tool result description, 662 moment load description, 577 object reference, 1021 moment object reference, 1021 moment of inertia, 385 mooney-rivlin model, 1196 2–parameter, 1196 3–parameter, 1196 5–parameter, 1197 9–parameter, 1197 motion load description, 605 solving with inertia relief, 605 move and copy connection objects, 407 moving windows, 252 mpc equations were not built for one or more contact regions - troubleshooting , 1080 MPC formulation contact region setting, 418 multibody parts, 316 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. multilinear kinematic hardening, 1202 multiple versions of CAD systems, 1072 N named selection exporting, 372 named selections converting to Mechanical APDL application components, 373 creating, 354 criteria rules, 362 display, 367 including in program controlled inflation, 371 object reference, 1032 overview, 354 scoping analysis objects to, 371 toolbar location in the Mechanical application window, 233 toolbar screenshot and description, 298 Named Selections importing, 372 managing, 370 named selections object reference, 1032 neo-hookean, 1195 new section plane, 271 Newton-Raphson residuals, 769 next view - graphics toolbar button, 285 no separation type contact region setting, 414 nodal coordinate systems results, 732 nodal force description, 616 Nodal Force object reference, 1001 nodal orientation description, 615 Nodal Orientation object reference, 1001 Nodal Pressure, 617 nodal rotation object reference, 1021 nonlinear controls analysis settings, 542 nonlinear formulation analysis setting, 542 nonlinear material effects assigning to parts - analysis step, 6 nonlinear solution, 769 normal elastic strain result description, 1093 object reference, 1047 normal elastic strain result object reference, 1047 normal gasket pressure object reference, 1047 normal gasket pressure object reference, 1047 normal gasket total closure object reference, 1047 normal gasket total closure object reference, 1047 normal Lagrange formulation contact region setting, 418 normal stiffness contact region setting, 418 normal stiffness factor contact region setting , 418 normal stress exponent for body interaction object,496 normal stress limit for body interaction object, 496 normal stress result description, 640 object reference, 1047 normal stress result object reference, 1047 number of processors solution setting, 755 numbering control object reference, 1034 numbering control object reference, 1034 NX assigning parameters, 869 O objects reference alphabetical listing, 977 description of page content, 977 offsets surface bodies, 321 ogden, 1199 ok status symbol, 235 options - analysis settings, 538 options - listed and described, 303 order of precedence in resolving thermal boundary condition conflicts, 855 orthotropic elasticity, 1193 other selection scoping in periodic symmetry region, 352 out of process solutions, 754 output controls - analysis settings, 545 overconstrained conditions joints, 469 P p-alpha EOS, 1238 painting graphics , 241 pan - graphics toolbar button, 285 parameters CAD, 869 defined in solution commands objects, 860 overall description, 867 parameterizing a variable, 279 restrictions, 867 specifying, 867 part description, 315 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1299 Index object reference, 1035 part object reference, 1035 partial solution returned - troubleshooting, 1075 path object reference, 1037 path - construction geometry, 376 path object reference, 1037 path results, 736 PDEF command, 711 peak result, 723 penetration result in contact tool description, 649 object reference, 997 penetration result object reference, 997 perfectly insulated load description, 589 object reference, 1021 perfectly insulated object reference, 1021 periodic high scoping in periodic symmetry region,352 periodic low scoping in periodic symmetry region, 352 periodic region object reference, 1038 using, 352 periodic region object reference, 1038 periodic symmetry type, 339 periodicity - angular, 339 phase angle in current for solid source conductor, 597 in current for stranded source conductor body, 599 in voltage for solid source conductor, 596 phase response, 655 phase response result object reference, 1047 phase response result object reference, 1047 picking - depth , 241 picking graphics, 241 pinball factor for body interactions, 493 pinball radius contact region setting, 418 pinball region contact region setting, 418 pinch object reference, 1026 pinch controls post, 470 pinch object reference, 1026 pipe idealization description, 614 pipe idealization condition object reference, 1021 pipe idealization object reference, 1021 pipe pressure load description, 569 pipe pressure object reference, 1021 1300 pipe temperature load description, 569 pipe temperature object reference, 1021 planar face direction, 632 planar joints, 436 plane strain behavior - 2-D simulation, 332 plane stress behavior - 2-D simulation, 332 plastic strain - equivalent, 644 plasticity, 1201 PLNSOL command, 711 plots - Mechanical APDL application, 860 point mass description, 385 object reference, 1039 point mass object reference, 1039 point scoped result tracker, 777 pointer modes, 241 POLYFLOW to Mechanical data transfer, 158 polynomial, 1197 polynomial EOS, 1225 porous collapse damage, 1220 porous materials, 1234 post pinch controls, 470 postprocessing commands objects, 860 postprocessing features, 774 pre stress object reference, 1040 pre-stress object reference, 1040 preprocessing commands objects, 860 pressure load at CFD boundary, 144 description, 568 object reference, 1021 pressure object reference, 1021 pressure result in contact tool description, 649 object reference, 997 pressure result object reference, 997 preview mesh - overall analysis step, 9 previous view - graphics toolbar button, 285 print preview, 301 context toolbar - screenshot and description, 287 tab, 240 priority global connection setting, 403 PRNSOL command, 711 probe annotations in result context toolbar, 287 description, 737 probe result object reference, 1042 probe result object reference , 1042 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. procedure overall steps in an analysis, 1 programming - using APDL, 860 project context toolbar - screenshot and description, 287 object reference, 1043 project object reference, 1043 psd base excitation load description, 579 PSD base excitation load object reference, 1021 PSD base excitation object reference, 1021 publishing reports, 865 pure penalty formulation contact region setting, 418 Q quick rainflow counting - fatigue simulations , 696 R rad/s - in main menu, 280 radians - in main menu, 280 radiation load description, 586 object reference, 1021 radiation object reference, 1021 radiosity controls, 537 rainflow counting - fatigue simulations, 696 rainflow matrix result in fatigue tool description, 699 object reference, 1003 rainflow matrix result object reference, 1003 random vibration analyses considerations for acceleration, 635 considerations for deformation, 635 considerations for velocity, 635 random vibration analysis type, 70 reactions bolt load, 651 contact, 666 generalized plane strain, 651 overall list, 651 reactions result in contact tool description, 649 recommended guidelines when using prestress with explicit dynamics, 55 reduced integration scheme, 317 reference number - coordinate system, 389 reference temperature, 6 refinement object reference, 1026 refinement object reference, 1026 regions types, 335 reinforcement body interaction type, 497 relative assembly tolerance analysis setting, 542 relative scaling - in result context toolbar, 287 remote boundary conditions, 628 remote boundary conditions - troubleshooting, 1082 remote displacement object reference , 1021 remote displacement support description, 555 object reference, 1021 remote force load description, 572 object reference, 1021 remote force object reference, 1021 remote point commands objects, 385 connection lines, 384 object reference, 1044 overview, 381 promote, 385 remote point object reference, 1044 remote points object reference, 1044 remote points object reference, 1044 remote solving, 754 rename based on definition commands objects, 860 results and result tools, 747 rename in tree outline, 235 renaming contact regions - animated example, 428 renaming joints based on geometry, 466 report context toolbar - screenshot and description, 287 creating - overall analysis step, 17 creating editions, 866 customizing, 866 options, 303 report preview tab, 240 reported frequency result object reference, 1047 reported frequency result object reference, 1047 resetting contact regions to defaults - procedure, 431 response psd results, 679 response spectrum analysis type, 75 restart analysis, 535 restart controls, 535 restore original window layout, 252 restore original window layout - in main menu , 280 result context toolbar - screenshot and description, 287 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1301 Index result tracker description, 774 explicit dynamics, 777 exporting, 787 features, 786 object reference, 1045 plotting, 786 renaming, 787 structural, 775 thermal, 776 result tracker object reference, 1045 results contour, 732 electric, 693 gasket, 682 geometry represented, 634 how to apply, 634 magnetostatic, 688 related topics, 718 reviewing - overall analysis step, 16 structural, 634 thermal, 685 unaveraged contour, 721 unconverged results, 728 vector plots, 743 results and result tools object reference, 1047 resume capability for explicit dynamics, 855 Reverse Validation option for Mapping Validation, 1105 revolute joints, 436 RHT concrete strength, 1216 rigid body motion - troubleshooting , 1081 rigid dynamics analysis to static structural analysis, 137 rigid dynamics analysis type, 102 rigid materials, 1251 rotate - graphics toolbar button, 285 rotation cursor, 301 rotation cursors, 241 rotational order of coordinate systems results, 733 rotational velocity load description, 567 object reference, 1021 rotational velocity object reference, 1021 rotordynamics controls - analysis settings, 551 rough type contact region setting, 414 rpm - in main menu, 280 rs base excitation load description, 580 RS base excitation load object reference, 1021 RS base excitation object reference, 1021 1302 S safety factor for maximum equivalent stress safety tool result,659 for maximum shear stress safety tool result, 661 for maximum tensile stress safety tool result, 664 for Mohr-Coulomb stress safety tool result, 662 safety factor result [fatigue] description, 699 [fatigue] object reference, 1003 [stress] description, 658 [stress] object reference, 1055 safety factor result object reference, 1055 safety margin for maximum equivalent stress safety tool result,659 for maximum shear stress safety tool result, 661 for maximum tensile stress safety tool result, 664 for Mohr-Coulomb stress safety tool result, 662 object reference, 1055 safety margin result object reference, 1055 saving contact region settings - procedure , 430 saving results as a database file, 852 as a simulation database file, 852 scale factor value, 1008 scaling deformed shape - result context toolbar, 287 relative - in result context toolbar, 287 scenarios - solving, 766 scope conflicts, 855 description, 634 graphics, 396 results, 724 scope contact region settings - listed and defined, 412 search across global connection setting, 403 search for connection duplicate pairs, 407 select mode - body, 285 select mode - edge, 285 select mode - face, 285 select mode - graphics toolbar button, 285 select mode - vertex, 285 select type - geometry, 285 select type - graphics toolbar button, 285 select type - node, 285 selecting direction, 241 selection box select, 241 extend selection, 241 extend to adjacent, 241 extend to connection, 241 extend to limits, 241 filters, 241 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. single select, 241 selection information window activating, 253 export, 264 overview, 252 reselect, 264 selection modes and reported information, 254 sort, 264 toolbar, 261 setting contact conditions manually - guidelines and procedure, 426 setting variables, 313 sharp angle tool object reference, 1026 sharp angle tool object reference, 1026 shear damage, 1219 shear elastic strain result description, 1093 object reference, 1047 shear elastic strain result object reference , 1047 shear force result object reference, 1047 shear gasket pressure object reference, 1047 shear gasket pressure object reference, 1047 shear gasket total closure object reference, 1047 shear gasket total closure object reference, 1047 shear moment diagram, 681 shear stress exponent for body interaction object, 496 shear stress limit for body interaction object, 496 shear stress result description, 639 object reference, 1047 shear stress result object reference, 1047 shell element results, 639 shell thickness for body interactions, 492 shock EOS linear, 1227 show all bodies, 318 show body, 318 show faces, 319 show vertices, 298 Simplorer Pins, 161 simply supported edge - description, 560 object reference, 1021 vertex - description, 561 simply supported object reference, 1021 simulation role in Workbench , 1 simulation wizard - features and types, 230 single selection, 241 sizing object reference, 1026 sizing object reference , 1026 slice plane - drawing/editing in result context toolbar, 287 sliding distance result in contact tool description, 649 object reference, 997 sliding distance result object reference, 997 slot joints, 436 snap to boundary, 470 snap to mesh nodes, 376 solid bodies, 315 solid bodies - using, 319 Solid Edge assigning parameters, 869 solid source conductor body, 594 SolidWorks assigning parameters, 869 solution annotations, 396 context toolbar - screenshot and description, 287 object reference, 1050 solution combination object reference, 1051 solution information object reference, 1051 solving overview, 751 troubleshooting (convergence problems), 1087 troubleshooting (general), 1083 solution combination description, 750 object reference, 1051 troubleshooting, 1087 solution combination object reference, 1051 solution coordinate system, 726 solution information description, 769 object reference, 1051 solution information object reference, 1051 solution magnitude limit exceeded - troubleshooting , 1077 solution object reference, 1050 solution restarts, 759 solve process settings, 755 solve status symbol, 235 solver - conflicting DOF constraints troubleshooting, 1088–1089 solver failure - troubleshooting, 1076 solver type, 533 solving overall analysis step, 15 overview, 751 units, 793 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1303 Index solving scenarios, 766 Source Value option for Mapping Validation, 1105 spatial displacements, 620 spatial load and displacement function data, 626 spatial load tabular data, 624 spatial loads, 620 spatially varying displacements, 620 spatially varying loads, 620 special analysis topics, 137 specify offset contact region setting, 418 specifying constant load expressions, 621 specifying constant load values, 621 specifying load values, 621 specifying surface body layered sections, 325 specifying surface body thickness, 323 specifying tabular loads, 623 spot weld object reference, 1052 using, 484 spot weld object reference, 1052 spot welds assumptions and restrictions, 484 spring object reference, 982, 1054 spring object reference, 982, 1054 springs preload, 478 results, 679 using, 478 stabilization analysis setting, 542 stabilization energy result description, 646 standard earth gravity load description, 566 object reference, 1021 standard earth gravity object reference, 1021 standard toolbar commands and descriptions, 283 location in the Mechanical application window, 233 startup options, 303 State Equation of, 1185 static structural analysis type, 79 status bar - location and description in the Mechanical application window, 233 status of variables, 313 status result in contact tool description, 649 object reference, 997 status result object reference, 997 status symbols , 235 1304 steady-state thermal analysis type, 84 steinberg guinan strength, 1205 steps details of equilibrium iterations, 526 details of steps, 526 details of substeps, 526 guidelines for integration step size, 527 overall topics, 525 step controls, 529 using multiple steps, 9 stiffness assigning to parts - analysis step, 6 strain energy result description, 647 object reference, 1047 strain energy result object reference, 1047 strain hardening, 1218 strain rate effects, 1220 strain-life fatigue, 695 stranded source conductor body, 598 strength factor - fatigue simulations, 696 stress intensity result description, 641 object reference, 1047 stress intensity result object reference, 1047 stress ratio for maximum equivalent stress safety tool result,659 for maximum shear stress safety tool result, 661 for maximum tensile stress safety tool result, 664 for Mohr-Coulomb stress safety tool result, 662 object reference, 1055 stress ratio result object reference, 1055 stress tool result object reference, 1047, 1055 stress tools how to add, 658 listed, 658 object reference, 1055 stress-life fatigue, 695 stress/strain results - overall description, 639 structural error result description, 642 object reference, 1047 structural error result object reference, 1047 structural loads - listed, 562 structural results, 634 supported function loads, 627 supported tabular loads, 625 supports types of supports, 551 suppress all other bodies, 318 suppress body, 318 suppress items, 239 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. suppress status symbol, 235 suppressed contact region setting, 414 surface object reference, 1057 surface - construction geometry, 381 surface bodies faces with multiple thicknesses and layers specified, 328 general description, 319 importing , 320 importing thickness, 321 offsets, 321 specifying layered sections, 325 specifying thickness, 323 thickness, 320 surface body results, 727 surface object reference, 1057 surface results, 742 surface temperatures at CFD boundary, 145 surfaces transferred as solids - troubleshooting, 1079 symmetric behavior contact region setting , 414 symmetric electromechanical symmetry type, 336 symmetric structural cyclic symmetry type, 336 symmetric structural symmetry type, 336 symmetry defining in DesignModeler, 351 defining in explicit dynamics, 337 defining in Mechanical, 352 object reference, 1057 using, 334 symmetry object reference, 1057 symmetry region object reference, 1058 using, 352 symmetry region object reference, 1058 synchronous solutions, 754 T tabs, 240 location in the Mechanical application window, 233 tabular data window, 268 target bodies scope contact region setting, 412 target normal search direction contact region setting, 418 target scope contact region setting, 412 temperature load description, 584 object reference, 1021 temperature object reference, 1021 temperature result description, 686 object reference, 1047 temperature result object reference, 1047 tensile failure, 1221 test data, 1195 thermal boundary condition conflicts, 855 thermal capacitance, 385 thermal condition load object reference, 1021 thermal condition object reference, 1021 thermal conductance contact region setting, 418 thermal conductance value contact region setting,418 thermal error result object reference, 1047 thermal error result object reference, 1047 thermal loads - listed, 562 thermal point mass description, 385 object reference, 1059 thermal point mass object reference, 1059 thermal results, 685 thermal specific heat, 1251 thermal steady-state analysis type, 84 thermal strain effects assigning to parts - analysis step, 6 thermal strain result, 643 thermal-electric analysis type, 87 thermal-stress analyses, 138 thermal/structural loads importing, 146 thermal/structural results exporting, 149 thickness object reference, 1060 thickness object reference, 1060 time role in analysis settings, 525 time step safety factor for body interactions, 493 tips working with charts and graphics, 241 tolerance for body interactions, 493 tolerance slider global connection setting, 403 tolerance type global connection setting, 403 tolerance value global connection setting, 403 toolbars context - overall description and listing, 287 graphics - commands and descriptions, 285 graphics option, 298 main menu - commands and descriptions, 280 named selection - screenshot and description, 298 overall description, 280 standard - commands and descriptions, 283 unit conversion - screenshot and description, 298 topics - special analysis, 137 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1305 Index torsional moment result object reference, 1047 total acceleration result description, 635 object reference, 1047 total acceleration result object reference, 1047 total current density result object reference, 1047 total deformation result description, 635 object reference, 1047 total deformation result object reference , 1047 total electric field intensity result object reference, 1047 total field intensity result object reference, 1047 total field intensity result object reference , 1047 total flux density result object reference, 1047 total flux density result object reference, 1047 total force electromagnetic result description, 689 object reference, 1047 total force result object reference, 1047 total heat flux result description, 686 object reference, 1047 total heat flux result object reference, 1047 total magnetic field intensity result description, 689 total magnetic flux density result description, 688 total strain - equivalent, 645 total velocity result description, 635 object reference, 1047 total velocity result object reference, 1047 transfer volumetric temperature, 145 transferring coordinate systems to the Mechanical APDL application, 395 transient structural analysis linked to modal, 99 transient structural analysis type, 91 transient thermal analysis type, 133 translational joints, 436 transparency for joints, 466 tree outline , 235 conventions and status symbols, 235 go to options, 237 location in the Mechanical application window, 233 triad cursor, 301 troubleshooting 1306 listing of overall problem situations, 1073 tutorials Mechanical, 166 two vertices direction, 632 type contact region setting, 414 U u. s. customary units - in main menu, 280 unaveraged contour results , 721 underconstrained parts - troubleshooting, 1081 underdefined status symbol, 235 unit conversion toolbar location in the Mechanical application window, 233 screenshot and description, 298 unit system behavior, 1 units - fatigue user life, 696 units - solving, 793 universal joints, 436 unsuppress all bodies, 318 unsuppress body, 318 unsuppress items, 239 update status symbol, 235 update stiffness contact region setting, 418 updating geometry , 2 use range global connection setting, 403 user defined result description, 702 object reference, 1047 user interactions - details view, 274 user preferences file, 303 V validation object reference, 1061 validation object reference, 1061 variable parameterizing, 279 setting, 313 status, 313 varying displacements, 620 varying loads, 620 vector heat flux result plots, 686 vector plot result display, 743 vector principal elastic strain result object reference, 1047 vector principal stress result object reference, 1047 vector principal stress/elastic strain result description, 642 object reference, 1047 velocity object reference, 1063 velocity object reference, 1063 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. velocity support description, 556 view results during solve, 774 viewing selected columns for contact - worksheet, 266 viewports description, 241 graphics toolbar button, 285 virtual body object reference, 1064 virtual body group object reference, 1065 virtual body group object reference, 1065 virtual body object reference, 1064 virtual cell object reference, 1066 virtual cell object reference, 1066 virtual hard vertex object reference, 1067 virtual hard vertex object reference, 1067 virtual split edge object reference, 1068 virtual split edge object reference, 1068 virtual split face object reference, 1068 virtual split face object reference, 1068 virtual topology context toolbar - screenshot and description, 287 in Mechanical, 976 object reference, 1069 virtual topology object reference, 1069 Viscoelastic, 1194 visibility - analysis settings, 551 visibility options, 303 voltage excitation for solid conductors voltage object reference, 1021 voltage excitation for solid source conductors description, 596 voltage load description, 590 voltage object reference, 1021 von Mises stress result, 640 simulation wizard - features and types, 230 workbench conflicts with the Mechanical APDL application when using commands objects, 860 working with charts and graphics, 241 worksheet go to selected items, 266 go to selected items in tree, 266 information display, 266 viewing selected columns for contact, 266 writing and reading files, 852 Y yeoh, 1198 Z zerilli armstrong, 1207 zoom - graphics toolbar button, 285 W weak springs analysis setting, 533 window geometry, 240 overall layout and component description, 233 windows manager, 252 wireframe - graphics toolbar button, 285 wizards description and screen location, 229 options, 303 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates. 1307 1308 Release 14.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.