Effect of Blade Number on Internal Flow and Performance Characteristics in Low-Head Cross-Flow Turbines

Abstract

Cross-flow turbines are widely used in microhydropower systems because of their cost-effectiveness, environmental sustainability, adaptability, and robust design. However, their relatively lower efficiency than other turbine types limit their application in large-scale projects. Previous studies have identified poor flow profiles as a significant factor contributing to inefficiency, with the number of blades playing a critical role in the flow behavior, efficiency, and structural stability. This study employed numerical simulations to analyze how varying the number of blades affects the internal flow characteristics and performance of the turbine at, and off, its best operating points. Configurations with 16, 20, 24, 28, 32, 36, 40, and 44 blades were investigated under constant low-head conditions, fully open valve settings, and varying runner speeds. Simulations were performed using ANSYS CFX, incorporating steady-state conditions, a two-phase flow model with a movable free surface, and a shear stress turbulence model. The results indicate that the 28-blade configuration achieved a maximum hydraulic efficiency of 83%, outperforming the preset 24-blade setup by 6%. Flow profiles were examined using pressure and velocity gradients to identify regions of adverse pressure. Due to the impulse nature of the turbine, the flow profile is more sensitive to changes in the flow speed than to pressure. The flow trajectory showed stability in the first stage but exhibited discrepancies in the second stage, which were attributed to turbulence, recirculation, and shaft flow impingement. The observed performance improvements were linked to reduced hydraulic losses due to flow separation and friction, emphasizing the significance of the number of blades and the regions of optimal efficiency under low-head conditions.

1. Introduction

Recent studies have emphasized the critical importance and feasibility of the full-scale deployment of renewable energy systems as a sustainable solution to mitigate climate change and enhance energy security [1,2,3]. In rural regions without access to electricity, microhydropower plants (MHPs) with capacities ranging from 5 kW to 100 kW have demonstrated significant effectiveness as a reliable solution for electrification [4,5,6]. Such capacities are generally adequate to satisfy the energy demands of off-grid rural communities, providing both domestic and commercial applications. MHPs play a pivotal role in fostering socioeconomic development in rural communities [6,7]. Typically, a run-of-river configuration eliminates the need for large dams, thereby minimizing environmental impact. However, their efficiency and sustainability depend on the availability of perennial water sources and favorable topographic conditions. Among the MHP technologies, the cross-flow turbine (CFT) is widely recognized as the most ideal candidate for low-head applications because it operates efficiently within the head ranges of 3–30 m [8,9].

The popularity of the CFT stems from its simplicity, cost-effectiveness, reliability, and inherent self-cleaning capability [8]. The original turbine was invented by Australian inventor Anthony Mitchell and was subsequently improved by a Hungarian engineer named Donát Bánki. By 1920, the focus had shifted to reducing costs and adapting the turbines to remote locations [10]. CFTs operate based on the impulse (pressure-free) principle, converting the kinetic energy of water into rotational motion, which is subsequently transformed into electricity via alternators. The turbine design includes a cylindrical runner composed of two parallel circular disks connected by a series of curved horizontal blades. The system consists of two primary components: a nozzle, which converts the available head into kinetic energy, and a runner, which converts the water’s kinetic energy into mechanical energy through fluid–blade interactions. A unique characteristic of the CFT is that water interacts with the runner blades twice, enabling operation in both water and air phases [11].

The CFT performance was highly dependent on the head and flow rate conditions. For high-head applications (typically > 100 m) [12], the turbine operates in pure impulse mode along two distinct stages. In the first stage, water flows from the runner’s outer periphery to its interior, exerting pressure on the blades and generating reactive forces. In the second stage, water moves from the inner periphery to the outer region before being discharged through casing, operating under the pure impulse principle at atmospheric pressure. Studies have indicated that approximately 70% of energy transfer occurs in the first stage, while 30% is realized in the second stage, including entrained flow effects [13]. By contrast, under low-head conditions (generally < 30 m), the turbine operates on the partial impulse principle during both stages, leveraging water’s kinetic energy for energy conversion. This adaptability makes the turbine versatile and effective for diverse hydropower applications. Despite these versatile characteristics, these turbines have lower efficiency than their counterparts, such as the Pelton, Kaplan, and Francis turbines. The theoretical maximum efficiency of the CFT was initially reported to be 87%; however, experimental studies by Mock and Merrifield demonstrated a more modest actual efficiency of 68% [8]. Since its inception, numerous experimental and numerical studies have been conducted to identify the key causes of underperformance and performance discrepancies. However, the reported efficiency values often exhibit inconsistencies and conflicting interpretations, likely due to variations in laboratory settings, parameter control, and the complexity of the flow dynamics involved.

These discrepancies and conflicting views indicate further room for improvement, leading to the need to optimize the turbine’s key geometric parameters, such as the nozzle orientation, angle of attack, blade angle, nozzle entry angle, diameter ratio, and number of blades. Several studies have shown that refining the internal flow profile is critical for improving the performance of CFTs [14,15,16]. Poor flow profiles contribute to efficiency losses, and a comprehensive understanding of these profiles requires detailed flow visualization and characterization [17]. To address the complex flow physics associated with CFTs, numerical methods, particularly those based on solving the Navier–Stokes equations, are essential for accurately estimating turbine flow characteristics and efficiency [18,19]. Numerical approaches are the most effective and preferred tools for addressing the complex flow profiles encountered in CFTs. Although experimental techniques are the most reliable and effective methods for capturing system performance, they have limited ability to provide detailed and time-based insights into internal flow characteristics. By contrast, numerical analysis, particularly through advancements in computational fluid dynamics (CFD), has emerged as a powerful tool for optimizing turbine designs.

Modern CFD solvers and post-processing software enable in-depth analysis of the pressure and velocity fields, facilitating the identification of critical flow phenomena, such as recirculation zones and negative pressure regions. By identifying these problematic areas, it becomes possible to modify geometric design parameters to improve turbine performance [20]. However, the accuracy of CFD simulations is dependent on several assumptions and simplifications, including turbulence models and boundary conditions, which may not fully capture the complexities of actual flow conditions. To ensure the reliability of CFD models, they must be rigorously validated against experimental data, as inaccuracies can arise from factors such as mesh quality and the numerical techniques employed [21]. Numerical prediction and performance study of CFTs presents unique challenges due to the complex nature of flow physics.

In impulse turbines, the jet flow intermittently interacts with the runner, and the interface between the water jet and the surrounding air forms a dynamic, movable free surface. This interaction results in an inherently unsteady two-phase flow with a dynamic free surface. Two primary numerical methods are employed to analyze such flows: the particle tracking method (PTM) and the classical CFD method (CCM), both of which track the free surface. The PTM, which is based on Lagrangian principles, follows individual fluid particles without requiring discretization of the flow domain. By contrast, the CCM, which is commonly implemented through the volume of fluid (VOF) method, tracks the free surface within a discretized flow domain [22,23]. The CCM is computationally more efficient than the PTM and was selected for this study.

Several studies have demonstrated that the number of blades significantly affect a turbine’s structural integrity, internal flow dynamics, and overall performance [24,25,26]. The optimal number of blades in the CFT is critical for validating the internal flow characteristics and optimizing the efficiency. An excessive number of blades increases momentum energy transfer and power output but also leads to higher blade friction, increased weight, and enhanced turbulence, resulting in greater hydraulic losses and operational difficulties. Conversely, too few blades mitigate these problems because they reduce efficiency and compromise structural stability. Therefore, determining the optimal number of blades is essential for optimizing turbine performance under specific operating conditions. In low-head applications, optimizing the number of blades is particularly important for improving efficiency and power output, which could significantly contribute to national electrification programs (NEPs) in rural areas, especially within renewable energy initiatives [27].

To our knowledge, no direct empirical relationship has been established between the number of blades and the performance of CFTs under specific operating conditions. Furthermore, previous studies have presented inconsistent and occasionally conflicting views on the optimal number of blades (see Table 1). These discrepancies may have arisen because of variations in the laboratory conditions and design parameters over time; nevertheless, they offer valuable insights for future optimization efforts and efficiency improvements. To resolve these inconsistencies, it is essential to examine how the number of blades affects the internal flow characteristics and turbine performance, particularly by varying the runner speed at, and off, its best operating efficiency point (BEP). This research aims to determine the optimal number of blades for turbine performance based on the existing turbine configuration at the NTNU Waterpower Laboratory. Using numerical methods, this study investigates the effect of the number of blades on the turbine’s internal flow profile and efficiency under low-head conditions, with a fully open valve at, and off, its BEP. This study builds upon Kaunda’s previous experimental and numerical work. The turbine performance was analyzed under low-head conditions of 3, 5, 7, and 10 m, with valve openings ranging from 20% to 100% in 20% increments, and at runner speeds of 250 and 350 rpm. The experimental results indicated that, at a 5-m head with the valve fully open and a runner speed of 350 rpm, the maximum achieved efficiency was 77% [28]. In parallel, the numerical study predicted a maximum hydraulic efficiency of 79% under the same operating conditions [10].

1.1. Previous Studies

This literature review examines the impact of the number of blades and design parameters on turbine performance under low-head operating conditions. Table 1 Summarizes the BEPs reported by various researchers. Although the findings from these numerical and experimental studies may have been influenced by variations in the laboratory conditions and design parameters over time, they provide valuable insights for continued optimization and potential efficiency improvements.

Table 1. Summary of the effect of the number of blades on CFT performance reported by various researchers.

Investigators	Number of Blades Used in the Study	Optimal Number of Blades	Maximum Efficiency (%)	Reference
Khosrowpanah et al.	10,15,20	20	80	[29]
Desai and Aziz	15,20,25,30	30	88	[30]
Totapally and Aziz	15,20,25,30,35,40	30	91	[31]
Joshi et al.	8,10,16,20,24,30	28	64.8	[32]
Pereira and Borges	10,25	25	73.8	[33]
Olgun	20,24,28,32	28	72	[34]
Choi et al.	15,26,30	30	65.5	[35]
Sammartano et al.	30,35,40	35	82.1	[36]
Acharya et al.	16,18,20,22	22	76.6	[37]

Table 1. Summary of the effect of the number of blades on CFT performance reported by various researchers.

Investigators	Number of Blades Used in the Study	Optimal Number of Blades	Maximum Efficiency (%)	Reference
Khosrowpanah et al.	10,15,20	20	80	[29]
Desai and Aziz	15,20,25,30	30	88	[30]
Totapally and Aziz	15,20,25,30,35,40	30	91	[31]
Joshi et al.	8,10,16,20,24,30	28	64.8	[32]
Pereira and Borges	10,25	25	73.8	[33]
Olgun	20,24,28,32	28	72	[34]
Choi et al.	15,26,30	30	65.5	[35]
Sammartano et al.	30,35,40	35	82.1	[36]
Acharya et al.	16,18,20,22	22	76.6	[37]

As shown in Table 1 the results regarding the effect of the number of blades on the turbine performance are inconsistent. According to a few studies, an increase in the number of runner blades has a favorable impact on performance, whereas in other studies, it did not. Therefore, it is important to resolve this contradiction and determine the optimum number of blades required for the best performance.

1.2. Model Specification

The design configuration of the CFT, as analyzed by Kaunda [10], served as the foundational reference for this study. A detailed summary of these specifications is provided in

Table 2. Design Specifications of the Proposed CFT.

Design Parameter	Normalized Expression	Value	Unit
Effective head	H	5	m
Flow rate	Q	0.3	m3/s
Optimal runner speed	N	350	rpm
Outer runner diameter	D1	270	mm
Inner runner diameter	D2	187	mm
${\mathrm{D}}_{\mathrm{r}}$ (Diameter ratio)	${\displaystyle \frac{{\mathrm{D}}_2}{{\mathrm{D}}_1}}$	0.693	-
Number of blades	Z	24
Angle of attack	${\mathsf{\alpha }}_1$	16	degree
Outer Blade entry angle (1st stage)	${\mathsf{\beta }}_1$	30	degree
Inner Blade exit angle (1st stage)	${\mathsf{\beta }}_2$	90	degree
Water admission angle	λ	90	degree
Shaft diameter	${\mathsf{\varphi }}_{\mathrm{s}}$	40	mm
${\mathrm{r}}_{\mathrm{b}}$ (Radius of the blade)	${0.378\ast \mathrm{D}}_1$	102	mm
${\mathrm{N}}_{\mathrm{t}}$ (Nozzle throat height)	${0.254\ast \mathrm{D}}_1$	68.5	mm
${\mathrm{N}}_{\mathrm{o}}$ (Nozzle opening)	$2.2\ast {\mathrm{N}}_{\mathrm{t}}$	150	mm
${\mathrm{r}}_{\mathrm{n}}$ (Radius of the nozzle entry arc)	${0.567\ast \mathrm{D}}_1$	153	mm
Blade thickness	${\mathrm{t}}_{\mathrm{b}}$	3	mm

. Using this established configuration, a numerical validation was performed to assess the performance of the proposed model by varying the number of blades and runner speed.

2. Methods and Materials

2.1. CFD Model Description

This study employed a CFD-based numerical approach to investigate the internal flow characteristics and performance of a CFT under low-head conditions with a fully open valve. The proposed turbine incorporates a flow-control mechanism comprising a manually operated screw system equipped with a graduated-level indicator. To accurately analyze the flow behavior, this study exclusively considered a fully open valve configuration. The turbine configuration was examined by varying the number of blades from 16 to 44 in increments of 4 (as illustrated in Figure 1), while the runner speeds ranged from 140 to 560 rpm, with 350 rpm identified as the theoretical optimal speed for the BEP.

Flow profiles and performance were further assessed under the specified operating conditions at, and off, their optimal ranges to analyze their effects on flow dynamics and turbine performance. Figure 2 shows a detailed flowchart outlining the methodology of the proposed CFD-based numerical analysis.

Upon determining the design specifications and operational requirements, the turbine geometry was developed using SolidWorks^® 2019. The two-dimensional geometry was subsequently extruded by 1 mm to satisfy the three-dimensional modeling requirements for compatibility with the ANSYS CFX solver [38].

Figure 3 presents the complete geometry and computational domain of the proposed CFT.

This turbine configuration uses a multiple frame-of-reference approach, as outlined in the ANSYS Theory Guide [39], to effectively distinguish between the rotating and stationary regions of the flow domain. At the interfaces between these regions, the turbine casing and nozzle interact with the inner and outer free surfaces at a 360° pitch angle. This interface ensures the continuity of mass, momentum, and energy throughout the entire computational domain, thereby maintaining the consistency and accuracy of the simulations.

A standard homogeneous free-surface model was used to simulate two-phase (air and water) flows, assuming shared velocity, pressure, and turbulence fields for both phases. This approach ensures consistency throughout the computational domain. A general grid interface (GGI) was implemented to facilitate proper coupling between the meshing domains. The frozen rotor model was applied to manage frame mixing at the interfaces while maintaining the fixed relative positions of the components while accommodating both rotating and stationary reference frames. This method accurately captures the interactions between the stationary and rotating domains without changing their relative orientations. The computational domain of the turbine, which includes the nozzle, turbine casing, and runner, was defined and imported into ANSYS CFX^® 2023 for detailed numerical analysis. The domain was partitioned into stationary and rotating zones with the casing, nozzle, and inner free surfaces designated as the stationary zones and the runner as the rotating zone, as shown in Figure 4. Inlet boundary conditions were set with static pressure at a 5-m effective net head and specified volume fractions (VOF) of 1 for water and 0 for air. The outlet was modeled as an opening with zero-gauge pressure and a VOF of 1 for air and 0 for water. No-slip conditions were applied to all walls, and symmetry boundary conditions were imposed at the front and rear of the computational domain. The specific interface configurations, as presented in Figure 4, ensure unified transfer of energy and momentum across the domain.

2.2. Numerical Equation

The choice of turbulence model depends on the specific flow characteristics and the available computational resources [40,41]. In this study, the Reynolds-averaged Navier–Stokes (RANS) equations were used in conjunction with the Shear Stress Transport (SST) turbulence model. The SST model was selected over the traditional k-ε method due to its superior ability to accurately predict boundary layer dynamics, flow separation, and adverse pressure gradients [38]. As a hybrid turbulence model, the SST approach combines features from both the k-ε and k-ω models, with the eddy viscosity concept serving as its foundation.

2.2.1. Two-Phase Flow Model and Rotational Effects

This computational study investigates a two-phase system with a dynamic free surface, where one domain operates within a rotating reference frame. The phase densities were determined based on their respective volume fractions. To account for the rotational effects induced by the runner, the SST momentum equations were modified to include centrifugal and Coriolis forces, as described in the ANSYS theory guide [39]. These forces, which play a significant role in turbomachine applications, are integrated into the modified RANS equations. The flow dynamics of the two-phase system are governed by the continuity and momentum equations, represented by Equations (1) and (2), respectively. Equation (1) defines the continuity equation for the two-phase flow, and Equation (2) presents the modified momentum equation.

$${\displaystyle \frac{\partial \left({\mathsf{\alpha }}_{\mathrm{P}}{\mathsf{\rho }}_{\mathrm{P}}\right)}{\partial \mathrm{x}}}+\nabla ·\left({\mathsf{\alpha }}_{\mathrm{P}}{\mathsf{\rho }}_{\mathrm{P}}\right)={\mathrm{S}}_{\mathrm{P}}$$

(1)

$$\begin{array}{c}{\displaystyle \frac{\partial \left({\mathsf{\alpha }}_{\mathrm{P}}{\mathsf{\rho }}_{\mathrm{P}}{\overrightarrow{\mathrm{V}}}_{\mathrm{r}}\right)}{\partial \mathrm{t}}}+\nabla ·\left({\mathsf{\alpha }}_{\mathrm{P}}{\mathsf{\rho }}_{\mathrm{P}}{\overrightarrow{\mathrm{V}}}_{\mathrm{r}}\ast {\overrightarrow{\mathrm{V}}}_{\mathrm{r}}\right)-\nabla ·\left({\mathsf{\mu }}_{\mathrm{e}\mathrm{f}\mathrm{f}}\nabla {\overrightarrow{\mathrm{V}}}_{\mathrm{r}}\right)+{\mathsf{\alpha }}_{\mathrm{P}}{\mathsf{\rho }}_{\mathrm{P}}(2\overrightarrow{\mathsf{\omega }}\times {\overrightarrow{\mathrm{v}}}_{\mathrm{r}}+\overrightarrow{\mathsf{\omega }}\times \overrightarrow{\mathsf{\omega }}\times \overrightarrow{\mathrm{r}}\\ +\overrightarrow{\mathsf{\alpha }}\times \overrightarrow{\mathrm{r}}+\overrightarrow{\mathrm{a}}=\nabla \dot{\mathrm{P}}+{\nabla ·\left({\mathsf{\mu }}_{\mathrm{e}\mathrm{f}\mathrm{f}}\nabla {\overrightarrow{\mathrm{V}}}_{\mathrm{r}}\right)}^{\mathrm{T}}+{\mathrm{S}}_{\mathrm{M}\mathrm{P}}\end{array}$$

(2)

where

$$\dot{\mathrm{P}}=\mathrm{P}+{\displaystyle \frac{2}{3}}{\mathsf{\rho }}_{\mathrm{P}}\mathrm{k}+{\displaystyle \frac{2}{3}}{\mathsf{\mu }}_{\mathrm{e}\mathrm{f}\mathrm{f}}\nabla ·\overrightarrow{\mathrm{V}}$$

(3)

where ${\mathsf{\alpha }}_{\mathrm{P}}$ is the phase volume fraction, ${\mathsf{\rho }}_{\mathrm{P}}$, is phase density, ${\mathrm{S}}_{\mathrm{P}}$, is the phase mass flow rate, ${\overrightarrow{\mathrm{V}}}_{\mathrm{r}}$ is relative flow velocity, $\overrightarrow{\mathsf{\omega }}$ is angular flow velocity, $2\overrightarrow{\mathsf{\omega }}\times {\overrightarrow{\mathrm{v}}}_{\mathrm{r}}$ is the Coriolis acceleration, $\overrightarrow{\mathsf{\omega }}\times \overrightarrow{\mathsf{\omega }}\times \overrightarrow{\mathrm{r}}$ is the centripetal acceleration, $\overrightarrow{\mathsf{\alpha }}\times \overrightarrow{\mathrm{r}}$ is the acceleration due to an unsteady change in the rotational speed of the runner, and $\overrightarrow{\mathrm{a}}$ is the acceleration due to an unsteady change in the linear relative speed ${\overrightarrow{\mathrm{V}}}_{\mathrm{r}}$. In both equations, the subscript ‘p’ refers to the properties of each phase.

2.2.2. Turbulent Viscosity and Governing Equations

The effective viscosity used in the momentum equation is determined by Equation (4), which applies the eddy viscosity concept [14]:

$${\mathsf{\mu }}_{\mathrm{e}\mathrm{f}\mathrm{f}}=\mathsf{\mu }+{\mathsf{\mu }}_{\mathrm{t}}$$

(4)

where $\mathsf{\mu }$ (kg/m.s) represents the mean viscosity and ${\mathsf{\mu }}_{\mathrm{t}}$ (kg/m.s) denotes the turbulent viscosity. For the k−ε model, the turbulent viscosity is expressed by Equation (5), which is related to the turbulent kinetic energy (k) and the turbulent dissipation (ε). By contrast, for the k−ω model, the turbulent viscosity is calculated from the turbulent kinetic energy, and the turbulent frequency (ω), as shown in Equation (6)

$${\mathsf{\mu }}_{\mathrm{t}}={\displaystyle \frac{{\mathrm{C}}_{\mathsf{\mu }}\mathsf{\rho }{\mathrm{k}}^2}{\mathsf{\epsilon }}}$$

(5)

$${\mathsf{\mu }}_{\mathrm{t}}=\mathsf{\rho }{\displaystyle \frac{\mathrm{k}}{\mathsf{\omega }}}$$

(6)

where ${\mathrm{C}}_{\mathsf{\mu }}$ (−) is a constant, $\mathsf{\rho }$ (kg/m³) is the fluid density, k (J/kg) is the turbulent kinetic energy, ε (m²/s³) is the turbulent dissipation rate, and ω (s⁻¹) is the mean turbulent frequency.

2.2.3. Multiphase Flow Treatment

To simplify the multiphase flow calculations, a homogeneous free-surface flow model was used. The effective density and viscosity of the mixture were determined based on the volume fractions, as described in Equations (7) and (8). The density of air (ρ_a) was modeled as a function of pressure (P) using the equation of state presented in Equation (9).

Volume fractions (${\mathsf{\alpha }}_{\mathrm{P}})$ were used to evaluate the proportion of control volumes occupied by each phase, with water being considered the denser secondary fluid. In the volume fraction approach to multiphase flow, the assumption of homogeneous coexistence of the phases resulted in effective fluid properties for each control volume, which were defined by Equation (7) for density and Equation (8) for viscosity.

$$\mathsf{\rho }=\sum _{\mathrm{p}}{\mathsf{\alpha }}_{\mathrm{P}}{\mathsf{\rho }}_{\mathrm{P}}$$

(7)

$$\mathsf{\mu }=\sum _{\mathrm{p}}{\mathsf{\alpha }}_{\mathrm{P}}{\mathsf{\mu }}_{\mathrm{P}}$$

(8)

where α (−) is the volume fraction, subscript p refers to the phase, $\mathsf{\rho }$ (kg/m³) and $\mathsf{\mu }$ (kg/m.s) are the density and viscous, respectively, of the average mixture used in the modified RANS equations. Air density ρ_a (kg/m³) is modeled as a function of the pressure P (N/m²), according to the equation of state presented in Equation (9).

$${\mathsf{\rho }}_{\mathrm{a}}={\mathsf{\rho }}_{\mathrm{a}},0{\mathrm{e}}^{\mathsf{\gamma }(\mathrm{P}-{\mathrm{P}}_{\mathrm{O}})}$$

(9)

Here, the subscript 0 denotes reference state values, and $\mathsf{\gamma }$ (−) represents the air compressibility coefficient. The volume fraction quantifies the proportion of the water-occupied control volume in this study. In the two-phase flow analysis, the secondary fluid, water, was considered to have a higher density.

2.2.4. Performance Metrics and Flow Visualization

Equation (10) was used to calculate the torque generated by the turbine by integrating the blade contributions across the rotating region. The flow trajectories and velocity distributions were analyzed by examining the vector gradients at the entrance and exit points of each stage. The flow patterns and velocity triangles are illustrated in Figure 5 and Figure 6.

$$\mathrm{T}=⌈\int \mathrm{r}\ast \left(\stackrel{̿}{\mathsf{\tau }}.\mathrm{n}\left)\right)\mathrm{d}\mathrm{s}\right)⌉.\mathrm{a}$$

(10)

where “ds” is the surface area of the rotating domain, “n” is the unit vector normal to the surface, “r” is the position vector, “a” is the unit vector parallel to the axis of rotation, and “t” represents the total stress tensor, which captures the stress within the fluid material at any given point in continuum mechanics. Turbine efficiency was calculated using Equation (11), which is defined as the ratio of the output power along the shaft axis to the available power at the nozzle.

$$\eta ={\displaystyle \frac{{\mathrm{P}}_{\mathrm{s}\mathrm{h}\mathrm{a}\mathrm{f}\mathrm{t}}}{{\mathrm{P}}_{\mathrm{w}\mathrm{a}\mathrm{t}\mathrm{e}\mathrm{r}}}}={\displaystyle \frac{\sum \mathrm{T}\ast \mathsf{\omega }}{\gamma \ast \mathrm{H}\ast \mathrm{Q}}}$$

(11)

Turbine efficiency can also be calculated using Euler’s equation based on Newton’s second law of motion. The total power generated by the runner, as shown in Equation (14), is the sum of the powers produced in the first and second stages, represented by Equations (12) and (13), respectively.

To visualize the flow trajectories, an XY plane was inserted into the computational domain, and the velocity and pressure vector gradients were analyzed. The runner’s rotational speed was defined in the “rotating domain” within ANSYS CFX-Pre; with the blade walls assigned a relative velocity of zero (no slip condition). The flow profile at each stage was captured using the velocity vector gradient. The flow trajectory profiles and velocity triangles at the entry and exit circular paths of each stage are illustrated in Figure 5 and Figure 6.

$${\mathrm{P}}_{1-2}=\dot{\mathrm{m}}\ast \left[{\mathrm{U}}_1{\mathrm{V}\mathrm{u}}_1–{\mathrm{U}}_2{\mathrm{V}\mathrm{u}}_2\right]$$

(12)

$${\mathrm{P}}_{3-4}=\dot{\mathrm{m}}\ast \left[{\mathrm{U}}_3{\mathrm{V}\mathrm{u}}_3–{\mathrm{U}}_4{\mathrm{V}\mathrm{u}}_4\right]$$

(13)

where ${\mathrm{P}}_{1-2}$ and ${\mathrm{P}}_{3-4}$ are the powers developed in the first and second stages, $“\dot{\mathrm{m}}”$ is the mass flow rate, “α” is the angle of attack, and “β” is the blade angle. The absolute flow velocity, peripheral runner speed, and relative velocity are denoted by V (m/s), U (m/s), and W (m/s), respectively. The radial and circumferential velocity components are represented by V_f (m/s) and V_u (m/s), respectively. Subscripts 1 and 2 correspond to the inlet and outlet of the first stage, and subscripts 3 and 4 correspond to the inlet and outlet of the second stage. The circumferential velocity component influences the rotational effects, whereas the radial velocity component contributes to the flow stability and the overall flow profile at both stages. A detailed presentation of both velocity components based on variations in the number of blades and the runner speed is provided in

Table A4. Influence of Blade Number Configuration and Runner Speed on the Radial and circumferential Velocity Components of Flowing Water.

Radial Velocity Component (Vf): represents the inward/outward motion of flow relative to the rotor’s center, influenced by the turbine’s rotational speed (N) and blade count (Z). Sign Conventions: Inward Flow: Negative radial direction (−)            Outward Flow: Positive radial direction (+) Role of Radial Velocity: impacts energy transfer, efficiency, and fluid-blade interaction in the runner.
This figure (see Table A4-A) illustrates the impact of number of blade on the radial velocity component of the CFT along the outer periphery of the runner. The study reveals that configurations with fewer blades (e.g., 16 and 20 blades) lead to uneven flow, resulting in increased energy losses. In contrast, configurations with a higher number of blades promote smoother flow, though they also increase friction and resistance, which leads to a reduced overall efficiency.	This figure (see Table A4-B) demonstrates the effect of runner speed on the radial velocity component of the CFT along the outer periphery of the runner. The study indicates that lower runner speeds (<350 rpm) result in higher radial velocity and faster fluid passage, which reduces energy transfer efficiency and increases turbulence. Conversely, higher runner speeds (>350 rpm) lead to reduced radial velocity, as the extended interaction time between the blades and the jet enhances energy transfer and improves overall efficiency.
A.	B.
Circumferential Velocity Component (Vu): represents the tangential component of the flow velocity, which directly contributes to the turbine’s torque and power output Sign Conventions: Positive (+ve): Flow direction is counterclockwise, producing positive torque and power.            Negative (−ve): Flow direction is clockwise, resulting in negative torque and power Role of Circumferential Velocity: Vu is essential for torque and power generation. Proper alignment with the flow direction maximizes efficiency, while misalignment leads to energy losses.
This figure (see Table A4-C) illustrates the effect of runner speed on the circumferential velocity component of the CFT along the outer periphery of the runner. The study shows that at lower runner speeds (<350 rpm), the relative tangential velocity of the water is higher due to slower blade movement compared to the jet. This results in greater impact forces but may lead to inefficient energy transfer, as water exits with significant residual energy. In contrast, at higher runner speeds (>350 rpm), the blade speed more closely matches the jet’s tangential velocity, optimizing energy transfer and torque production. However, excessively high runner speeds may cause the jet to misalign with the blades, resulting in reduced torque generation and power output. An optimal runner speed exists at which the radial and circumferential velocity components are balanced, maximizing energy transfer. This occurs when the blade speed aligns with the jet velocity, ensuring efficient interaction and minimal energy loss.	This figure (see Table A4-D) demonstrates the effect of number of blade on the circumferential (tangential) velocity component of the CFT along the outer periphery of the runner. The study indicates that configurations with fewer blades (e.g., 16 and 20) result in poor alignment with the blade curvature, leading to reduced efficiency. Conversely, configurations with a higher number of blades enhance energy transfer but may obstruct flow and reduce efficiency if the blade count is excessive. The optimal number of blade maximizes energy transfer, minimizes flow disturbances, and reduces friction.
C.	D.

in the Appendix A. The total power generated by the runner is the sum of the powers produced in each stage:

$${\mathrm{P}}_{\mathrm{t}\mathrm{o}\mathrm{t}\mathrm{a}\mathrm{l}}={\mathrm{P}}_{1-2}+{\mathrm{P}}_{3-4}=\dot{\mathrm{m}}\ast \left[\left({\mathrm{U}}_1{\mathrm{V}\mathrm{u}}_1-{\mathrm{U}}_2{\mathrm{V}\mathrm{u}}_2\right)+\left({\mathrm{U}}_3{\mathrm{V}\mathrm{u}}_3–{\mathrm{U}}_4{\mathrm{V}\mathrm{u}}_4\right)\right]$$

(14)

The hydraulic (water) power, which is solely dependent on the head and flow rate, is expressed as follows:

$${\mathrm{P}}_{\mathrm{w}\mathrm{a}\mathrm{t}\mathrm{e}\mathrm{r}}=\dot{\mathrm{m}}\mathrm{g}\mathrm{H}$$

(15)

Here, g (m/s²) is the gravitational acceleration, and H(m) is the effective head at the turbine inlet. Hydraulic efficiency is defined as the ratio of the total power generated by the runner to the hydraulic (water) power:

$${\mathsf{\eta }}_{\mathrm{h}}={\displaystyle \frac{1}{\mathrm{g}\mathrm{H}}}\left[\left({\mathrm{U}}_1{\mathrm{V}\mathrm{u}}_1-{\mathrm{U}}_2{\mathrm{V}\mathrm{u}}_2\right)+\left({\mathrm{U}}_3{\mathrm{V}\mathrm{u}}_3–{\mathrm{U}}_4{\mathrm{V}\mathrm{u}}_4\right)\right]$$

(16)

In the ANSYS CFX-Post system, the velocities are measured by defining a circular path at both the outer and inner peripheries of the runner. Hydraulic efficiency was calculated by numerical integration.

2.3. Grid Independent Study and Simulation

Figure 7 presents the use of unstructured tetrahedral elements to discretize the computational flow domains. The proposed approach facilitates precise flow dynamics capture and supports automatic meshing adjustments during geometric modifications. To assess the accuracy of the wall boundary–layer simulation, the Y+ parameter was used. This dimensionless parameter quantifies the distance from the wall to the first grid cell, which corresponds to the thickness of the viscous sub layer. A target Y+ value of approximately 1 was aimed at ensuring an accurate representation of the flow separation and pressure gradients near the walls. The boundary surfaces, including those of the blade, shaft, and casing, were treated with a first-layer inflation technique, adding 30 layers to all wall surfaces with a 5% growth rate, thus enhancing the resolution of near-wall flow behavior.

To validate the accuracy and reliability of the flow profile representation, a mesh refinement analysis was performed. This analysis confirmed that the numerical results were unaffected by mesh size variations, thereby demonstrating that the computational outcomes were independent of the discretization parameters. For the sensitivity analysis, the torque was selected as the monitored variable. The results revealed that, with an average element size of 2 mm, corresponding to approximately 675,000 mesh elements, the torque value (0.454 N·m) stabilized after 600 iterations, as shown in Figure 8.

3. Results and Discussion

3.1. Overview of Flow Characteristics in CFTs

The CFT operates through a dual-stage momentum transfer mechanism involving multiple blades, which results in distinct flow dynamics influenced by the interaction between the water jets and the turbine blades. Key parameters, such as the number of blades and the runner speed, play critical roles in shaping the flow behavior and determining the turbine performance. These relationships were examined by considering the distributions of total pressure, water velocity, and water volume fraction across the turbine domain. The analysis of these parameters refined and optimized the flow profiles, ultimately enhancing the hydraulic efficiency of the turbine.

3.1.1. Effect of Blade Number Configuration and Runner Speed on the Total Pressure Distribution

The total pressure distribution, which represents the combined static and dynamic forces acting on the turbine blades, was significantly influenced by both the number of blades and the runner speed. Achieving an optimal pressure distribution is crucial for maximizing the energy transfer because it improves the fluid forces during the interactions between the fluid and blade surfaces in both stages. The static pressure is governed by the effective operating head and is typically maximized at the nozzle entry. The dynamic pressure, on the other hand, Increased along the nozzle as the flow area decreased, reaching a peak at the nozzle throat, where the flow area was minimal. As shown in Figure 9, increasing the number of blades from 16 to 44 resulted in a more uniform pressure distribution, which was attributed to the reduced turbulence and flow variability. However, the use of a larger number of blades led to increased drag and flow obstruction, causing significant pressure losses due to friction between the fluid and blade surfaces. Moreover, they also reduce the maximum dynamic pressure spikes, leading to a more consistent total pressure across the turbine. This improves the overall turbine efficiency, particularly by reducing the risk of cavitation in regions where the static pressure is low.

In this study, the pressure distribution in the first stage remained relatively uniform across all configurations. However, in the second stage, the pressure distribution became progressively more uneven, primarily due to the influence of turbulence and recirculation effects, as shown in Figure 10. Additionally, the pressure profile within the inner free zone of the runner remained nearly constant, except in areas where continuous interaction between the water and blade surfaces occurred. The configuration with 28 blades optimized the pressure distribution and minimized the extent of flow separation.

An increase in the runner speed resulted in a higher dynamic pressure due to the associated increase in water velocity. However, this also decreases the static pressure in certain regions of the turbine. The overall effect on the total pressure is determined by the interplay between the increase in the dynamic pressure and the decrease in the static pressure. When the dynamic pressure increases substantially, the total pressure can rise, thereby improving the turbine performance. As shown in Figure 11 and Figure 12, a reduction in the runner speed causes a notable decrease in the dynamic pressure, leading to an uneven pressure distribution and worsening recirculation effects. These changes negatively affect the energy transfer efficiency. On the other hand, elevated runner speeds promote flow detachment and exacerbate turbulence, which increases the risk of cavitation near the leading edges of the blades. This further reduces the hydraulic efficiency by reducing the overall total pressure.

Figure 12 shows the total pressure distribution in the first stage, which increased with increasing runner speed. However, in the second stage, the pressure distribution becomes unstable and uneven, which is largely due to the onset of recirculation and turbulence. These findings underscore the complex relationship between maintaining stable flow dynamics and optimizing the runner speed to maximize hydraulic performance.

3.1.2. Effect of Blade Number Configuration and Runner Speed on Water Superficial Velocity Distribution

In the CFD context, superficial water velocity represents the effective velocity of water flowing through the turbine’s blade passages. This velocity was averaged over the cross-sectional area of the flow at a given point, assuming a constant depth or surface. The superficial velocity is a critical parameter for evaluating the momentum transfer between the water and the blades, and it directly influences the turbine’s energy conversion efficiency.

The water velocity distribution within the CFT is highly dependent on both the number of blades and the runner speed. As shown in Figure 13, the velocity distribution within the CFT is inherently non-uniform because of the dynamic interaction between the water jets and the rotating blades. A relatively uniform water velocity distribution is crucial for optimizing the energy transfer from the water to the turbine blades. The distribution profile is influenced by various factors, such as the blade profile, number of blades, and runner speed, all of which play significant roles in defining the hydraulic performance of the turbine.

Figure 14 presents the water velocity distribution profiles across the entire turbine domain for different numbers of blades at a constant runner speed of 350 rpm. Increasing the number of blades increased the uniformity of the water velocity distribution. With more blades, the water flow was distributed across a greater number of blade passages, which reduced velocity fluctuations between adjacent blades and resulted in a smoother flow profile. However, beyond a certain threshold, further increases in the number of blades led to higher flow resistance, which obstructed the flow and reduced the effective superficial velocity. This resulted in increased drag forces and a subsequent reduction in the kinetic energy of the system.

The configuration with 28 blades achieved optimal balance while maintaining high superficial velocities and minimizing flow separation and drag. This configuration effectively reduces hydraulic losses, thereby improving the overall hydraulic efficiency of the turbine. As shown in Figure 15, the 28-blade setup facilitates efficient energy extraction by enhancing the interaction between the water flow and the turbine blades. Additionally, the results indicate that, in the turbine’s inlet region, the water velocity experiences a slight decrease along the flow direction; whereas, in the exit stage, increased turbulence and recirculation contribute to greater instability in the velocity distribution. By contrast, the velocity profiles across the first and second stages remain nearly constant when operating at the ideal radial blade angle, ensuring optimal energy transfer. At optimal runner speeds, water enters the turbine blades at the ideal angle, maximizing the superficial velocity and thereby enhancing the energy transfer efficiency.

Figure 16 illustrates the impact of varying the runner speeds on the superficial water velocity distribution in the 28-blade configuration. At lower runner speeds, the superficial velocity decreases, resulting in less effective impact angles and reduced momentum transfer to the blades. This reduction in momentum results in flow recirculation and an uneven velocity distribution, which negatively affects the turbine performance. By contrast, higher runner speeds cause the water to bypass the blades more rapidly, which reduces the efficiency of energy extraction. The increased relative velocity between the water and the blades under these connditions induces flow detachment, further contributing to an uneven velocity distribution and compromised hydraulic performance.

3.1.3. Effect of Blade Number Configuration and Runner Speed on Water Volume Fraction Distribution

The water volume fraction represents the proportion of the flow field occupied by water relative to other phases, such as air, within the turbine. It is a critical parameter for understanding flow dynamics because it directly influences the interaction between the water jet and the turbine blades. The distribution of water volume fraction is significantly affected by factors such as the number of blades and runner speed, both of which play a crucial role in determining the hydraulic performance of the turbine. A higher water volume fraction indicates more effective utilization of the flow area for energy extraction, whereas a lower fraction can lead to inefficiencies due to air entrainment and flow separation.

As shown in Figure 17, increasing the number of blades (from 16 to 44) enhances the water volume fraction distribution by optimizing the flow channeling through the turbine. Enough blades ensure uniform coverage of the blade surfaces, thus maximizing the energy transfer. The 28-blade configuration, as shown in Figure 17, provides the most consistent water volume fraction with minimal air entrainment, thereby improving the energy extraction efficiency. However, an excessive number of blades can obstruct the flow area, leading to increased blockage and air pocket formation, which reduces the water volume fraction and results in higher turbulence and diminished hydraulic performance.

Figure 18 further illustrates the impact of varying the number of blades on the water volume fraction distribution at a constant runner speed of 350 rpm. While the number of blades is crucial, the runner speed also plays a vital role in ensuring a stable and uniform distribution of the water volume fraction within the turbine. As can be seen, increasing the number of blades generally promotes a more uniform flow distribution, thereby reducing the potential for flow separation. This improves water-fraction management and enhances the turbine’s overall performance by minimizing energy losses.

As illustrated in Figure 18, an increase in the runner speed resulted in a more uniform and streamlined flow path, minimizing significant obstruction along the shaft and the first and inner free surfaces of the domain. However, this effect is accompanied by heightened turbulence in the second stage.

At lower runner speeds, the momentum is insufficient to fully occupy the blade surfaces, reducing the water volume fraction. This incomplete coverage results in air pockets and recirculation zones that hinder effective energy transfer. Conversely, at higher runner speeds, centrifugal forces push water away from the blades, reducing the water volume fraction within the blade passages. Therefore, optimal runner speeds are crucial for maintaining a consistently high-water volume fraction, ensuring continuous contact with the blades, and maximizing the energy extraction efficiency.

3.2. Effect of Blade Number Configuration on Hydraulic Performance

Figure 19 shows the hydraulic efficiency variations at different blade number configurations. The highest efficiency of 83.5% was achieved with the 28-blade configuration, which surpassed Kaunda’s experimental results by 6% and outperformed the corresponding numerical study by 4% under identical operating conditions. However, this overestimation may be influenced by several factors, such as the flow velocity, Reynolds number, and applied boundary conditions. In addition, discrepancies in the results may arise from the limitations inherent in the model assumptions, including the turbulence modeling and mesh resolution, which may not fully capture the intricate flow dynamics observed in the experimental settings.

The configuration with 16 blades exhibited the lowest hydraulic efficiency (70.2%), primarily due to inadequate energy extraction between the water jet and the blade surfaces. As the number of blades increased from 16 to 28, the hydraulic efficiency improved from 70.2% to 83.5%. However, for the 32-blade configuration, the efficiency slightly decreased by approximately 6%. The 36- and 40-blade configurations achieved efficiencies of 79.5% and 79.51%, respectively, which are comparable to those of the other turbine configurations. These results highlight the complex interplay between the number of blades and hydraulic efficiency, with diminished returns observed beyond the optimal 28-blade configuration.

Figure 20 illustrates that all turbine configurations demonstrated optimal performance at their respective runner speeds, with the exception of the 16-blade configuration, which exhibited a hydraulic efficiency of 75% at a runner speed of 280 rpm. This deviation indicates that the 16-blade configuration did not operate at peak efficiency at this particular runner speed, suggesting that the flow dynamics and energy transfer may not have been fully optimized under these conditions.

3.3. Validation of the Study

This study achieved a hydraulic efficiency of 83% with a 28-blade CFT, representing one of the highest efficiency designs reported in the recent literature. Figure 21 summarizes the findings of various researchers, emphasizing the significant influence of the blade count on the performance of CFTs.

Khosrowpanah [29] proposed an optimal number of blades in the range of 24 to 32 blades, which aligns with the high efficiency observed in the 28-blade configuration of this study. Similarly, Aziz and Desai [42] investigated the parametric effects of CFTs and found that 30-blade configurations achieved efficiencies of approximately 81%, suggesting that increasing the blade count beyond 28 does not lead to significant efficiency improvements. This can be attributed to the increased flow resistance and drag associated with higher blade counts. Totapally and Aziz [31] demonstrated that a 30-blade turbine can reach up to 80% hydraulic efficiency, indicating diminishing returns as the number of blades increases. Further work by Joshi et al. [43] analyzed various blade arrangements and concluded that configurations with 26–30 blades optimize the energy extraction by improving the flow uniformity and reducing the hydraulic losses. Conversely, Pereira and Borges [44] reported that exceeding the optimal blade range could adversely affect performance, resulting in flow separation and increased turbulence. Kokubu et al. [45] conducted both numerical and experimental analyses of CFTs and confirmed that an optimal number of blades enhances the hydraulic efficiency and flow pattern stability. Sinagra et al. [46] also found that a 28-blade turbine performs efficiently across a range of flow conditions, although it may not reach the maximum efficiency of designs with fewer blades. This study distinguishes itself by achieving 83% hydraulic efficiency with a 28-blade turbine, surpassing many of the other configurations reported in the literature. This represents a 4% improvement over the 24-blade design and a 7% increase compared to the experimental results reported by Kaunda [10,28]. These improvements are primarily attributed to the reduction in hydraulic losses, including the flow separation, recirculation, and friction.

4. Conclusions

This study provides a comprehensive evaluation of the impact of the number of blades and runner speed on the hydraulic performance of CFTs, emphasizing the interplay between these parameters and their influence on the flow dynamics. The results show that the 28-blade configuration, operating at an optimal runner speed of 350 rpm, yields the highest hydraulic efficiency of 83%, surpassing Kaunda’s previous experimental results by 6% and numerical simulations by 4%. This efficiency gain is largely attributed to reduced hydraulic losses, such as flow separation, recirculation, and friction, which are prevalent in turbine configurations with fewer or excessive blades. The results demonstrate that increasing the number of blades from 16 to 28 improves the hydraulic efficiency by enhancing the pressure distribution, water velocity, and volume fraction within the turbine. The optimal configuration strikes a balance between minimizing drag and maintaining high energy transfer efficiency, whereas a higher number of blades beyond 28 leads to diminishing returns due to increased flow resistance and turbulence. The 28-blade design also optimizes the water velocity distribution and water volume fraction, ensuring stable and uniform energy extraction.

This research advances cross-flow turbine design by uniquely combining numerical methods to analyze the pressure, velocity, and water volume fractions, thereby revealing the flow mechanisms that reduce hydraulic losses and enhance performance. The proposed method bridges the gaps in low-head turbine performance studies by addressing the inconsistencies in blade count optimization and aligning the results with those of renewable energy initiatives. Additionally, this research aligns with and extends the findings of previous studies, such as those by Khosrowpanah et al., who also identified 28 to 30 blades as the optimal range for maximizing efficiency. The results presented here reinforce the critical importance of balancing the number of blades and runner speed for achieving the best hydraulic performance and provide a foundation for further optimization of CFT designs for real-world applications. This study not only validates the 28-blade configuration as one of the most efficient configurations in the recent literature but offers valuable insights into the underlying flow mechanisms that contribute to improved turbine performance. The results will contribute to the ongoing development of more efficient and sustainable turbine designs, particularly in the context of energy extraction from fluid flows.

5. Recommendation

The results of the present computational study offer valuable insights into the performance characteristics and fluid dynamics of CFTs under various operating conditions. However, to ensure the accuracy and applicability of these findings in real-world scenarios, experimental validation is essential.

Moreover, further research is recommended to investigate additional design variables, such as blade geometry, including factors such as shape, thickness, and curvature. This exploration can provide further enhancements to turbine efficiency, particularly under low-head operating conditions.