Development of a Cavitation Indicator for Prediction of Failure in Pump-As-Turbines Using Numerical Simulation

Abstract

The increasing deployment of pumps-as-turbines in small-scale hydropower applications in off-design conditions strengthens the need for the monitoring of the operation and maintenance (O&M) needs. PATs (pumps-as-turbines, pumps operated in reverse to generate electric current) are increasingly used because of their low cost as micro-hydropower plants; however, limited research has focused on their maintenance needs during operation. This is an important consideration given their use under conditions for which they were not originally designed. One of the most challenging O&M issues in hydromachinery is cavitation, which can harm turbines and reduce their efficiency. In this study, Computational Fluid Dynamics (CFD) was used for 15 different simulations of PAT configurations and their cavitation behaviour was investigated under varying inlet pressure and mass flow conditions. A cavitation strength indicator was developed using linear regression, describing the strength of cavitation from 0 (no cavitation) to 100 (extreme cavitation). This parameter depends on mass flow rate and head, which are easily measured parameters using standard sensors. With this approach, it is possible to monitor cavitation status in a continuous manner in a working PAT without the need for complex sensors. With this application, it is also possible to avoid costly damage, shutting down turbines when cavitation strength is exceptionally high.

1. Introduction

The use of pumps running in reverse as turbines—referred to as pump-as-turbines (PATs)—has become an increasingly attractive option for small-scale energy generation. One of the major advantages of PATs is their lower investment cost compared to traditional hydraulic turbines and easier maintenance [1]. Since they are usually standardized, mass-produced centrifugal pumps, replacement parts are readily available and cheap, compared to replacement parts for other types of hydro turbines [2]. Furthermore, the wide accessibility of these pumps improves their versatility as turbines and makes spare parts easier to obtain compared to traditional turbines.

In recent years, the growing interest in renewable energy solutions has pushed for more adaptable, flexible technologies, allowing for the optimization of energy generation in diverse conditions. For PATs, these systems might be deployed in either remote areas or more urbanized environments with frequent changes in energy demand. This flexibility is one of the primary reasons for their increasing adoption, as it enables energy generation in situations where traditional turbines might not be viable due to cost, space limitations, or regulatory constraints [1,3].

Like other types of renewable energy technologies, there is an increasing demand for hydro turbines to be adjusted to changing flow conditions. This requirement causes PATs to operate in conditions that can often be far from the best-efficiency point (BEP). While some aspects of cavitation in PAT systems have been studied—including numerical investigations such as those by Wenguang and Zhang (2017) [4]—the broader topic of PAT failure mechanisms remains insufficiently explored. As noted by Stephen et al. (2024) [5], there is a clear gap in the literature regarding the systematic analysis of failures in PATs, including cavitation-related damage. This highlights the need for further research focused not only on cavitation itself, but also on its role in overall system degradation and failure. Cavitation occurs when certain criteria are met, i.e., the local pressure in a fluid falls below its vapour pressure, causing the creation of vapour. It appears in low-pressure zones and forms bubbles, which collapse violently when they enter high-pressure areas [6]. This causes a sudden implosion, which results in intense shockwaves that can cause significant damage to metal surfaces, leading to the creation of pits and cavities [6,7]. On the other hand, cavitation also directly lowers the efficiency of working PATs, decreasing the amount of generated energy [8].

Additionally, cavitation negatively impacts the economic viability of PATs, especially when they are subjected to extended operation under cavitation. It leads to erosion of turbine components, reducing their operational lifetime and increasing maintenance costs [8]. In addition to wear, cavitation also generates excessive vibrations and noise [5]. For small-scale hydropower applications, where downtime and repair costs can quickly outweigh the benefits, understanding and mitigating cavitation becomes crucial. This is especially more pressing in recent times due to the aforementioned need for more flexible operation of hydropower devices [9].

Typical hydro turbines usually operate in relatively steady flow conditions, which allows for the analysis and mitigation of the chances of cavitation occurring, using, for example, dimensionless parameters. For this purpose, one of the most often used indicators is the Thoma number (σ) [10]. Utilizing this, it is possible to choose the proper type of turbine for given conditions and adjust its design accordingly. However, this approach leaves a large gap in the understanding of flow properties inside the turbine, which are not within the scope of these methods. This is because dimensionless numbers like the Thoma number cannot provide any information about local variations in pressure or flow velocity within the turbine [11]. These analytical tools focus on global operating parameters and neglect the flow behaviour, which plays a critical role in phenomena such as cavitation or efficiency losses [12].

For this reason, to understand the flow inside a PAT working in off-design conditions and analyse how its properties are related to the existence and strength of cavitation, there is a need for the application of modelling methods, particularly Computational Fluid Dynamics (CFD) [13]. CFD is considered a trustworthy and reliable tool for fluid flow analysis in various engineering applications. It enables detailed flow investigation, especially in complex geometries and under turbulent, transient, or multi-phase conditions. The most meaningful advantage of CFD is in its ability to provide data on local pressure and velocity distributions, which are often inaccessible through experimental methods [3]. As a result, CFD has become an essential method for studying internal flow phenomena in hydraulic machines.

While the Thoma number is often used in the design of conventional turbines, its application to PATs is limited due to the dynamic nature of their operating conditions. PATs often experience fluctuating flow patterns and varying loads, which makes it difficult to predict cavitation risk. This highlights the need for more accurate methods that take into account the local conditions within the turbine. Therefore, relying on the Thoma number or similar dimensionless parameters for cavitation prediction in PATs is not sufficient, especially in systems operating in off-design conditions [7]. The Thoma number is usually applied during the design phase of a hydropower plant to ensure that cavitation will not occur under relatively steady operating conditions. It is not designed to quantify the intensity of cavitation once it appears. In the case of PATs, they often operate under unstable flow conditions, so cavitation may still develop even if the model of PAT was selected based on the Thoma number. When cavitation occurs, the Thoma number offers a limited description of its severity. Therefore, additional indicators are needed to quantify cavitation intensity in such conditions.

Using CFD, internal flow properties can be linked to cavitation, evaluating the existence and strength of cavitation based on properties that are easily measurable in real time with digital sensors, like mass flow rate. The application of CFD also allows for examining cases that are hard to capture in real, working hydropower plants, either with extremely high or low flow rates or with high or low heads, which occur rarely during the year in natural conditions.

The goal of this work is to create a cavitation strength indicator, which will describe the strength of cavitation with a gradual scale, where 0 means no cavitation and 100 relates to an extreme case of cavitation. Its application will allow it to predict the cavitation in working PATs based on flow properties measured with digital sensors and let the user of the PAT know when the turbine should be shut off to protect its parts from damage. Additionally, CFD will be used as a tool to better understand the development of cavitation in the environment of increasing mass flow rate for a given PAT.

The key contribution of the paper is the analysis of cavitation in PATs. The cavitation in pumps has been extensively studied, but in reverse as a turbine, it has been neglected. This oversight is particularly important when considering that PATs operate in reverse under conditions they were not designed for, and as a result, PATs are more susceptible to cavitation. Understanding this failure mechanism in PATs is, therefore, crucial given their recent increased prevalence in hydropower practice, their increased susceptibility, and the increasing demand for flexible operation. Flexible operation of PATs is a particularly crucial consideration given that their typical efficient and safe operating envelope is much narrower than conventional turbines.

2. Methodology

2.1. The Goal of This Study

The goal of this study is to develop a CFD-based cavitation strength indicator (CI) that can be used to estimate the onset and severity of cavitation in a pump-as-turbine (PAT). To achieve this, a series of CFD simulations were performed for a selected PAT. The CFD model was validated against experimental results of the pump used as a PAT and experiencing cavitation. This experimental data is described in [5]. Simulation results were post-processed to extract flow parameters, which were then used to construct and evaluate the CI.

2.2. PAT Geometry

In this study, the model used was the KSB 050-32-200 centrifugal pump (manufacturer: KSB SE & Co. KGaA, Frankenthal, Germany), operated in PAT mode. The operating points for mass flow rate and head were chosen to cover three distinct regimes: pre-cavitation, cavitation inception, and fully developed cavitation. While the inception point is considered relatively fixed, the other two points were selected in an arbitrary but representative way to capture the general progression of cavitation severity.

Its specifications are summarized in

Table 1. Specification of KSB 050-32-200 (pump mode).

Specification	Value
Brand/Model	KSB Etanorm 050-32-200
Max Pressure	<16 bar
Flow Rate	<604 L/min (<36 m3/h)
Rotational Speed	960/1450/2900/3500 rpm
Power	0.75 kW
Temperature Range	−30 °C to +140 °C

. While the nominal impeller diameter is known from manufacturer data (170 mm), the exact geometry of the impeller blades—such as blade profile—was not available. These features, which significantly affect flow behaviour and energy conversion efficiency, were estimated using ANSYS software 2023 R1, especially Ansys Vista CPD 2023 R1, Ansys Bladegen 2023 R1. This process is more deeply described in Section 2.3.5.

The pump operates within a wide range of flow rates, which are detailed in the specifications. In PAT mode, the geometry of a chosen pump allows it to convert excess pressure into mechanical energy, thus acting as a turbine. The performance of PAT is dependent on its ability to maintain stable operation while handling varying flow conditions.

For accurate simulations, the corresponding data was used in CFD simulations to evaluate its performance in different operational scenarios.

Experimental Validation Data

The experimental dataset employed in this research originates from the test rig developed by Novara [14]. The test rig is schematically described in Figure 1 and consists of a 9.2 kW supply pump, a single-suction volute centrifugal pump used in a turbine mode (PAT) powered by an induction motor (5.5 kW). The pump used to construct the rig was a six-blade KSB ETN 050-32-200 (manufacturer: KSB SE & Co. KGaA, Frankenthal, Germany). To conduct measurements, two sensors were installed—a flow meter and a pressure meter (A, C). The inlet pressure is measured using a Gems Sensors Series 3000 relative pressure transducer with a 4–20 mA current output, offering an accuracy of ±0.25%. Flow is measured by an Omega FDT506 inline ultrasonic flow meter (Omega Engineering, Norwalk, CO, USA), also featuring a 4–20 mA current output, with a typical accuracy of ±2% and repeatability of ±0.2%. Downstream of the PAT, a Gems Sensors 3500 Series absolute pressure sensor (Gems Sensors, Plainville, MA, USA) (B) with a 4–20 mA current output is mounted, while two torque transducers (D and E) are positioned at the connection point between the PAT and the generator to monitor torque on the generator shaft and the PAT output shaft, respectively. At point D, Torque meter Datum Electronics, model M425-1D (Series 425) (Datum Electronics Ltd, East Cowes, UK). This offered a nonlinearity better than ±0.1% Full Scale and repeatability within ±0.05% Full Scale. Based on the manufacturer’s specifications, the overall uncertainty of the instrumentation is estimated to be within ±0.5% for pressure, ±2% for flow, and ±0.1% for torque.

In the piping loop, a transparent pipe fragment is installed after the PAT, which allows the onset of cavitation to be observed (see Figure 2). All the measurements are carried out in the situation where PAT’s RPM is equal to 1500. Behind the pump, the throttle valve is installed, which allows it to modify the flow rate. Using all of this data, a Thoma number was calculated for each case selected for numerical replication and for each of these cases, the state of cavitation was visually observed. Finally, the outcome of these measurements includes head, mass flow rate, Thoma number, and visual observation of cavitation state. Terms “intense cavitation”, “cavitation”, and “no visible cavitation” refer to purely visual observations made during the experiment. “Cavitation inception” denotes the moment when a vortex rope begins to form and becomes visible in the transparent section of the pipe behind the PAT. “No visible cavitation” corresponds to the phase before any visible vapour structures appear, while “cavitation” and “intense cavitation” describe the development or presence of a fully developed vortex rope. Experimental data is described in

Table 2. Experimental data used for this research.

Case Number	Mass Flow Rate [kg/s]	Head [bar]	Thoma Number [-]	Cavitation State
1	2.189180392	46.55656055	0.0617	intense cavitation
2	2.275925362	46.92028188	0.062	intense cavitation
3	2.488844834	47.50478544	0.0631	cavitation
4	2.733307932	46.63453287	0.0633	cavitation
5	2.930455591	46.89430884	0.064	cavitation
6	3.127603251	46.63450627	0.0637	cavitation inception
7	3.427267693	47.02418544	0.065	cavitation inception
8	3.797905293	46.9332874	0.0654	no visible cavitation
9	3.939851608	45.51738444	0.0656	no visible cavitation
10	4.129113361	45.23159742	0.0661	no visible cavitation
11	4.32623432	45.77723423	0.066	no visible cavitation
12	4.602267744	46.34871925	0.0663	no visible cavitation
13	4.941361718	43.49089469	0.0668	no visible cavitation
14	5.375086569	45.53026456	0.0676	no visible cavitation
15	5.564348322	44.37421357	0.0681	no visible cavitation

.

2.3. CFD Methodology

This section describes the numerical simulation used for modelling the PAT with application of CFD using Ansys CFX 2023 R1 software. The model was developed to analyze the properties of the flow and performance of the PAT. Simulations were carried out in steady-state “Turbo” mode, which is specifically created for turbomachinery and simplifies the setup for rotating domains. Later, these simulations were used as a starting point for transient simulations with the timestep 3.43 × 10⁻⁴ s and total simulation time 0.4 s, which corresponds to 10 full rotations of the impeller.

2.3.1. Governing Equations

The simulation was considered incompressible and Newtonian, using Reynolds-Averaged Navier–Stokes (RANS) equations. These describe the conservation of mass and momentum and depending on the chosen turbulence model, the conservation of other variables. As the k–ω turbulence model was implemented, these variables were k-turbulent kinetic energy and ω, the specific dissipation rate.

2.3.2. Turbulence Model

The k–ω SST (Shear Stress Transport) model is considered the industry standard for turbomachinery turbulence modeling [15,16] because it connects the advantages of k–ω and k–ε approaches, allowing for efficient and robust modelling of both near-wall and free-stream flow. For the inner layer, k–ω is applied and the algorithm switches to the k–ε approach for areas far from the wall, which can be considered as free-stream. This allows for good prediction of flow separation and adverse pressure gradients [15,16]. Additionally, this approach is suggested as the default approach and a robust methodology for turbomachinery applications in Ansys CFX documentation [17].

More advanced models, such as Large Eddy Simulation (LES) or Detached Eddy Simulation (DES), can be a source of more accurate description of cavitating flows. However, their application usually requires large meshes, which result in increased computational cost. For this study, the SST model was used as a practical balance between accuracy and computational feasibility, and a similar approach performed well in other cavitation-related simulations, including recent studies such as Khan et al. (2021) [18].

2.3.3. Rayleigh–Plesset Model

The Rayleigh–Plesset equation is used to describe the dynamics of one spherical vapour bubble in an incompressible environment. It describes the bubble inertia, liquid viscosity and surface tension. The Rayleigh–Plesset approach was proven in terms of accuracy and mass transfer between the liquid and vapour phase [19]. In general form, the Rayleigh–Plesset (RP) model was presented as Equation (1).

$${\rho }_L(RR¨+\frac{3}{2}{R\dot{}}^2)=P_{\infty }\left(t\right)-P_B\left(t\right)-\frac{2\sigma }{R}-4{\mu }_L\frac{R\dot{}}{R}$$

(1)

where R(t)—bubble radius as a function of time [m], Ṙ, R¨—first and second time derivatives of the radius (radial velocity and acceleration) [m/s, m/s²], ${\rho }_L$—liquid density, assumed constant [kg/m³], $P_{\infty }\left(t\right)$—ambient pressure far from the bubble [Pa], $P_B\left(t\right)$—pressure inside the bubble, assumed uniform [Pa], σ—surface tension at the liquid–vapour interface [N/m], ${\mu }_L$—dynamic viscosity of the liquid [Pa·s]. In cavitation modelling, Rayleigh–Plesset model is considered the default and robust way of simulation [20].

2.3.4. Boundary Conditions

Boundary conditions were chosen to match those of the experimental data used for model validation [5]. Mass flow rate on the inlet was measured and the pressure was measured on the outlet and inlet during the experiments conducted by Stephen et al. [5] on the selected PAT.

Using Ansys CFX, it is—to apply the boundary template “Mass Flow inlet P-Static outlet”. This template is suggested for turbines as it provides numerical stability and excels in calculating velocity and pressure profile of the inside of hydro machinery [21]. For walls, the no-slip boundary condition was used, assuming the velocity at walls of the turbine equal to zero, which is a fundamental assumption in fluid dynamics [22], except for foams. Boundary conditions are summarised in

Table 3. Set-up used for CFD simulation.

Feature	Settings
Turbulence model	k-omega SST
Boundary condition	Inlet—fixed mass flow rate (2–6 kg/s) Outlet—average static pressure (0 Pa gauge pressure) Walls—No slip condition
Mass flow rate	2–6 kg/s
Cavitation model	Rayleigh–Plesset
RPM	1500
Number of cells	1.12 mln

.

At the inlet, a “Mass Flow Inlet” boundary condition was applied, where the total mass flow rate entering the domain was explicitly prescribed. Values used for simulations are shown in

Table 4. Properties used in Vista CPD.

Parameter	Value
Volumetric flow rate	14.25 m3/h
Total head	13.75 m
Rotational speed	1500 RPM
Inlet flow angle to impeller	Rayleigh–Plesset
Volute axial length	1500

. The flow angle was set normal to the inlet surface. At the outlet, a Static Pressure Outlet boundary condition was applied. This combination of boundary conditions is common for turbomachinery and was used in previous studies, for example by Laouari, Ghenaiet (2016) [23] and Ortiz [24] (2019).

2.3.5. Creation of Mesh

As the exact 3D geometry of the turbine’s impeller and volute was not provided, it was necessary to obtain a similar geometry using reverse-engineering software. The initial step of its creation was to generate a 2D sketch of the impeller and volute, which will later be expanded into the 3rd dimension. Using documentation from the pump described in Table 1, several working conditions were used (listed in Table 4).

Based on given properties, Vista CPD was used to compute velocity triangles and optimize energy losses caused by the geometry to create 2D sketches. This is carried out using Equation (2):

$$\mathsf{\Delta }h = {\displaystyle \frac{u_2{c}_2 -u_1{c}_1}{g}}$$

(2)

where $\mathsf{\Delta }h$ is a pressure head, which is equal to the product of head and gravitational acceleration $g$. $u_1$ and $u_2$ are the blade tangential speeds at inlet and outlet [m/s], $c_1$ and $c_2$ are the tangential components of the absolute velocity at inlet and outlet [m/s], $g$ is the gravitational acceleration [m/s²]. Tangential speeds are calculated using Equation (3).

$$u=\omega r={\displaystyle \frac{2\pi n}{60}} \ast r$$

(3)

where $u$ is the blade peripheral speed at radius r [m/s], ω is the angular velocity [rad/s], $n$ is the rotational speed [rpm], $r$ is the radial position from the shaft axis [m] [25]. Finally, the obtained sketches were calculated and drawn, as shown in Figure 3.

In the next step, BladeGen was used to find relationships to determine the impeller shape and positioning with an iterative approach. The aim of this optimization was to ensure that the created 3D impeller model achieves energy transfer while also maintaining high hydraulic efficiency, and the ability to be manufactured. Initially, the outlet blade angle β2 was found using the Euler equation. It was later used to calculate the relative velocity at the outlet, which can be computed with Equation (4).

$$w2=u2-c2$$

(4)

Later, these relative velocities are applied to compute the tangent of β2 using Equation (5).

$$tan (\beta 2)={\displaystyle \frac{Q}{w2 \ast Am}}$$

(5)

where $Q$ is the volumetric flow rate [m³/s], $Am$ is the meridional flow area at the blade section [m²]. Once $\beta 2$ was computed, BladeGEN constructed a mean line, which is a curve that connects the midpoints between the pressure and suction sides of the blade profile. Its proper selection minimizes separation of the flow and turbulence, so the acceleration of flow is smooth across the blade length. Consequently, bladeGEN created a blade thickness distribution. The stacking line was created with axial stacking, which is a common choice for turbomachinery applications. Subsequently, the blade thickness distribution was applied by offsetting the camber line on pressure and suction surfaces according to a chosen profile shape. The thickness distribution has a direct impact on local pressure gradients and potential flow separation [25].

Figure 4 shows a distribution of Theta and Beta in degrees over the blade profile, which is displayed as the normalized chord length from the leading edge (LE) to the trailing edge (TE). The β curve represents the blade metal angle, while the θ curve shows the blade twist angle, derived from the relative rotation of each profile along the stacking axis. According to the BladeGEN guide, these angles can be described as:

β (Beta)—the blade metal angle, defined as the inclination of the blade surface relative to the local meridional direction. It reflects how the blade redirects the relative flow from inlet to outlet. The angle is typically measured at various spanwise sections (e.g., hub, mid-span, shroud) and varies from the leading edge (LE) to the trailing edge (TE).

θ (Theta)—the twist angle, which quantifies the rotation of the blade profile about the stacking axis. It describes how the orientation of each 2D profile changes along the span (from hub to shroud), affecting the alignment of the blade with the three-dimensional flow field [25].

In the next step, the meridional plane was generated from an outlet to the inlet (including the shroud and its contours), and the number of blades was set as 6 to reflect the existing PAT geometry and satisfy Equation (6).

$$\sigma ={\displaystyle \frac{Z \ast Sm}{2\pi Rm}}$$

(6)

where is the dimensionless blade solidity, $Sm$ is the blade spacing and $Rm$ is the mid-span radius [m] [25]. The result of this approach can be seen on Figure 5.

Using these parameters, BladeGEN generated the 3D shape of impeller, which consisted of the geometry of ⅙ of the impeller and the blade itself, which can be seen in Figure 6.

Geometry created with BladeGEN (Figure 6) was later meshed, and the mesh consisted of three parts. The first part (rotor mesh) was a fully-structured mesh created with Ansys ICEM and the remaining two parts (the extension of an outlet, volute mesh) were created with the built-in ANSYS package meshing software. In ANSYS ICEM, the mesh was created from manually distributed blocks, and the distribution of blocks used is presented in Figure 7. Later, these meshes were connected with Frozen Rotor [21] interfaces and used as an input to the CFD simulation.

The rotor was created by revolution of the meshed geometry created in previous steps. It consisted of approximately 400 × 10³ cells, while the volute was created with the element size of 2 × 10⁻³ m, with 10 boundary layers, achieving for both meshes the y+ value around 1, which is required for the application of k–ω SST turbulence modelling.

2.3.6. Mesh Independence

To ensure mesh independence, 7 meshes were examined, consisting of 160 k, 195 k, 480 k, 640 k, 1120 k, 1400 k and 1550 k elements. As the experimental measurements included efficiency, this was examined using Equation (6), set with Ansys expression. Each mesh was created with identical boundary conditions and number of boundary layers, and they were examined on the same CFD setup (solver settings, SST k–ω turbulence model). The convergence criteria were to achieve the mean residual range of 10⁻⁵, which became possible at meshes with the number of elements equal to 480 k and larger. The performance of each mesh was examined based on efficiency and its closeness to experimental results. The expected result of the mesh independence studies was that the turbine’s efficiency should not fluctuate by more than 1% between successive mesh refinements, proving that the numerical solution is independent of the mesh size. The lowest size of mesh that could satisfy this requirement was the mesh size of 1.12 mln elements, which can be seen in Figure 8. The final mesh had skewness below 0.65 and orthogonality above 0.75, ensuring sufficient quality for cavitation simulations. The rotor region was meshed using a fully structured grid in Ansys ICEM, achieving skewness below 0.5 and orthogonality above 0.85, which improves accuracy in critical flow regions.

2.3.7. CFD Setup

The CFD process was carried out using ANSYS CFX. To reflect the physical conditions of the working PAT, the starting conditions summarized in Table 2 were applied. Geometries with Vista CPD and BladeGen were created using the data listed in Table 4.

Because steady-state simulations failed to reproduce experimental results, the simulation was carried out in transient mode. The time step of 3.43 × 10⁻⁴ s was set to maintain a Courant number below 1, which is a critical value for accuracy.

The mean Courant number for the final mesh was 0.863, with a maximum of 1.5. Previous meshes had similar cell topology (they were only later refined), so it is assumed that their Courant numbers were also below 1. Furthermore, to improve the quality of the final solution, the rotor mesh was created fully structured in ICEM CFD with skewness around 0.5 and mean orthogonality 0.82, which allowed for larger cells near critical regions without compromising accuracy. The chosen time step allowed the solution to remain stable and consistent with physical observations. The rotational velocity was set to 1500 RPM and total simulation time was set to 0.4 s, which is approximately the time required for 10 full rotations of the rotor. This choice was made to allow for the flow stabilisation, ensuring sufficient time for flow development and later convergence of the simulation.

The discretization scheme used was a second-order upwind for all convective terms. For pressure, a central difference scheme was applied. Convergence was achieved at mean residual target of 10⁻⁵. The simulation was set using CFX Turbo mode. Three components (impeller, volute, outlet extension pipe) were connected with a frozen rotor interface type, where only the impeller rotates with a speed of 1500 RPM. The rotation was negative to enable PAT mode. Finally, CFX recognized 7 boundaries, which were set as an inlet, outlet and wall Boundary type. For wall influence on flow, no-slip wall condition was set, representing null velocity of fluid at the wall, which is fundamental CFD assumption for liquids. In terms of working fluid, “water” from Ansys library was removed and replaced with the mix of liquid water and vapour water. To ensure that the liquid entering the computational domain consists only of liquid water, the mass fraction of liquid water on the inlet was set to 1 while the mass fraction of vapour water was set to zero. This condition was required to enable the cavitation simulation and change of phase during simulation. The chosen interphase transfer was the mixture-model, and mass transfer setting was set for cavitation, which was described with the Rayleigh–Plesset model. The interface length scale and mean diameter of the vapour bubble were set, respectively, to 1 mm and 2 × 10⁻⁶, which are default values for this mode, while the saturation pressure was set at 2.34 kPa, which is the value of choice for water at a temperature of 293 K. As the temperature changes in the indoor location of the experimental measurement were negligible and the saturation pressure is not influenced by them in large quantities, this value was set as constant.

2.4. Thoma Number Limitations and the Purpose of the New Indicator

The Thoma number (σ) is a dimensionless parameter used in turbomachinery planning to determine the presence of cavitation. It is expressed as the ratio of the difference between the outlet pressure and the saturation pressure of the fluid to the hydraulic head, which is stated in Equation (7).

$$\sigma ={\displaystyle \frac{Poutlet-Psat}{\rho gh}}$$

(7)

where $Poutlet$ is the static pressure at the turbine outlet [Pa], $Psat$ is the saturation pressure of the working fluid [Pa],$\rho$ is the density of fluid [kg/m³], $g$ is gravitational acceleration [m/s²] and $h$ is the total head [m].

Equation (7) aims to identify situations when local pressure falls below the vapour pressure which will lead to phase change, thus cavitation. When the Thoma number is below the critical threshold specific to the turbine and design conditions, cavitation is likely to occur. It works mainly as a binary indicator, either showing the cavitation presence or lack of it. To address this limitation, a cavitation index (later called cavitation strength) was developed, which is created using the value of vapour volume fraction achieved through CFD simulation. CI will provide a quantitative estimate of the cavitation intensity, describing its power on a normalized scale from 0 (no cavitation) to 100 (extremely intense cavitation). While the Thoma number is a valuable and robust preliminary metric for the design stage of turbines working in steady conditions, CI enables deeper insight into the scale of this phenomenon. Additionally, when created, it can be computed using non-sophisticated data, such as pressure on the inlet and mass flow rate, which can be derived from standard sensors.

After creation of the meshes, they were used for CFD simulations. The obtained results were measured for efficiency using Equation (8). To check the robustness of simulations, their results were compared with experimental results.

$$n={\displaystyle \frac{T \ast \omega }{\mathrm{\Delta }P \ast V}}$$

(8)

where $T$—Torque [N*m],$\omega$—angular velocity [rad/s], $\mathsf{\Delta }P$—change of pressure between the inlet and the outlet [Pa], $V$—volumetric flow rate [m³/s]

When the solution was considered mesh independent at 1.12 mln total cell number, an entire flow curve of PAT was simulated using CFD. Later, these results were compared with experimental results on a previously created test rig with obtained efficiencies of the turbine at different flow rates. The result of this comparison can be seen in Figure 9.

When the CFD results were trustworthy enough to display proper efficiency of the turbine, cavitation prediction was added. Using the Rayleigh–Plesset model, it was decided to keep most of the properties at default for Ansys CFX turbomachinery application, while Saturation pressure was also set to default for the water at a temperature of 20 °C. According to experimental results, it could be seen that the cavitation was visible after the mass flow rate decreased to around 3.42 kg/s, which could also be seen in the CFD results (Figure 10). Further lowering the mass flow rate resulted in an increase in cavitation intensity in the experimental test rig.

2.5. Data Used for CI Indicator Construction

To quantify the cavitation strength, vapour volume fractions were categorized into three classes: Cells75 (vapour volume fraction > 0.75), Cells50 (0.50 < vapour volume fraction ≤ 0.75), and Cells25 (0.25 < vapour volume fraction ≤ 0.50). This classification allows weighting of the most intense cavitation zones more heavily. The number of cells with a vapour volume fraction in these brackets was considered. These quantities were calculated relative to the total number of cells in the mesh. Subsequently, an objective function was created to determine the cavitation intensity on a scale from 0 to 100. These values were then linked to the head and mass flow rate to predict cavitation.

2.6. CI Development

The algorithm utilizes two variables-head and mass flow rate to determine the strength of cavitation ongoing inside the PAT. Mass flow rate is a boundary condition that is set during the simulation. To calculate the cavitation strength, data from CFD was post-processed to obtain the percentage of cells with values of vapour volume fraction higher than 0.75, 0.5 and 0.25, respectively. All of these parameters were obtained directly from CFD analysis. For every case, the value of cavitation strength was calculated using Equation (9).

$$Cavitation strength=Cells75 \ast 3+Cells50 \ast 2+Cells25$$

(9)

where $Cells75$, $Cells50$ and $Cells25$ are the percentage of cells that show the vapour volume fraction over, respectively, 75%, 50% and 25%. Cells with vapour volume fraction lower than 25% were ignored in this approach.

Later, results were divided by the highest-obtained value of cavitation strength to normalize them. In the next step, all were multiplied by 100 to achieve results between 0 and 100, where 0 means no cavitation and 100 means the most extreme cavitation out of the examined group. This improves interpretability by scaling results relative to the worst observed condition (cavitation strength 100), which makes it easier to understand (cavitation strength becomes the description of cavitation severity compared to the worst scenario examined with CFD). The results obtained for 15 cases examined in this research are presented in

Table 5. Results.

Case Number	Mass Flow Rate [kg/s]	Head [bar]	Thoma Number [-]	Cavitation Power [-]	Cavitation State
1	2.189180392	46.55656055	0.0617	81.16	intense cavitation
2	2.275925362	46.92028188	0.062	74.85	intense cavitation
3	2.488844834	47.50478544	0.0631	61.26	cavitation
4	2.733307932	46.63453287	0.0633	56.8	cavitation
5	2.930455591	46.89430884	0.064	53.46	cavitation
6	3.127603251	46.63450627	0.0637	46.41	cavitation inception
7	3.427267693	47.02418544	0.065 (critical)	47.40	cavitation inception
8	3.797905293	46.9332874	0.0654	33.65	no visible cavitation
9	3.939851608	45.51738444	0.0656	29.52	no visible cavitation
10	4.129113361	45.23159742	0.0661	25.30	no visible cavitation
11	4.32623432	45.77723423	0.066	16.81	no visible cavitation
12	4.602267744	46.34871925	0.0663	0.00410	no visible cavitation
13	4.941361718	43.49089469	0.0668	0.000108	no visible cavitation
14	5.375086569	45.53026456	0.0676	0.000068	no visible cavitation
15	5.564348322	44.37421357	0.0681	0.00040	no visible cavitation

. The amount was chosen to capture the variation in flow across the experimental range measured.

To construct the algorithm, head and mass flow rates were related to cavitation strength using linear regression.

3. Results

The first part of the CFD research was focused on matching the CFD efficiency results with the experimental measurements of Stephen et al. [5].

The simulation results showed a very good agreement with the experimental results across the examined mass flow rates. The coefficient of determination R² equals 0.973, indicating that the created CFD model is able to accurately reflect the physical experiments. The root mean square error RMSE was equal to 2.14%, which is a further confirmation that the differences are low.

In general, lowering the parameter of mass flow rate as a boundary condition increases the intensity of cavitation, with the inception starting around 3.42 kg/s. It is visible that cavitation starts around the shroud side of the blade and extends to the outlet, creating a cavitation rope. With a further decrease in mass flow rate at the inlet, the number of mesh cells with a vapour volume fraction higher than 0.75, 0.5 and 0.25 increases. It is necessary to mention that the volute is generally prone to cavitation and the most susceptible parts are the impeller blades. The results of the simulation agree with the observational results; however, it is difficult to accurately quantify the cavitation based on visual perception. Using the created test rig, cavitation can be observed only downstream of the PAT (around points D and E in Figure 1), which leaves no information about the cavitation inside the turbine, where blades are susceptible to cavitation. Based on previous research by Demirel [26], it can be seen that cavitation onset takes place inside the turbine. While the cavitation rope is a visible part seen behind the rotor, there is also cavitation taking place on the blades, especially on the shroud side (Figure 11).

3.1. Prediction Results

It can be seen that the Thoma number is described with nearly linear distribution, where lowering the mass flow rate—the most important factor for cavitation strength—significantly affects it.

The obtained empirical relationships between head and mass flow rate are displayed in Equation (10).

$$Cavitation power=-2.1361+(-20.7194) \ast mass flow+\left(2.4884\right) \ast head$$

(10)

Equation (10) was obtained using a linear regression technique implemented in Python 3.10, using scientific libraries NumPy, pandas and scikit-learn. The model received a score of R² of 0.86, indicating that there is a significant degree of correlation between the predicted and received cavitation power values. Additionally, the RMSE at 6.65 clarifies that the model maintains a reasonable prediction accuracy across the given dataset. Interpreting the cavitation behaviour, it can be seen that the mass flow rate has a negative coefficient, which agrees with expectations—increasing the flow rate influences local velocities, lowering static pressures, which stimulates cavitation. The head has a negative coefficient, which means it also stimulates cavitation onset.

It can be seen that the Thoma number shows relatively small fluctuations as the mass flow rate decreases, even when it is the primary factor influencing cavitation power. In contrast, cavitation power shows significantly greater sensitivity, indicating that cavitation develops in a nonlinear manner. Unlike the Thoma number, which decreases slowly and near linearly, cavitation power provides a more dynamic and informative representation of the intensity of cavitation. This makes it a good indicator for assessing how vapour formation evolves under changing flow conditions. The stronger response of cavitation power to reductions in mass flow rate suggests that it captures the physics of cavitation more directly, making it a valuable tool in characterizing cavitation behaviour beyond what the Thoma number alone can show. This is especially visible in lower mass flow rates, where the increase in cavitation power between cases varies significantly, while Thoma number values present similar patterns. According to Figure 12, it can be seen how the cavitation power value depends on CFD cases, where the cavitation power value is computed for points where the simulation was carried out. It is visible that cavitation is a nonlinear phenomenon and while it shows rather simple dependency (lower mass flow rate stimulates cavitation and higher head stimulates cavitation), it can be seen that the points are not linearly displaced. In Figure 13, the results of Equation (10) are presented on a heatmap, showing that the predictor indicates a similar trend that was visible for higher mass flow rates.

Figure 14 displays what is the percentage difference between subsequent Thoma numbers of adjacent cases and how it relates to the percentage states of cavitation power. The first point compares the difference between states 1 and 2, and, respectively, point 13 compares states 13 and 14. The last point was removed with a value over 488%. This is caused by the division of very small numbers, which relate to a lack of cavitation and can be considered close to zero.

3.2. Sensitivity Studies

A sensitivity analysis was performed at five representative operating points (cases 1–5 in Table 2) to assess how the CI metric responds to potential measurement noise in head and flow inputs. Variability levels of 0.5%, 1%, and 5% were applied. The results show that CI remains relatively stable under low input noise (≤1%), but larger deviations (5%) can significantly affect CI. The indicator was found to be more sensitive to head than to mass flow. Figure 15 summarizes the results, including cases where both inputs were perturbed simultaneously (“2 var in Figure 15”).

4. Discussion

While the value of R² equal to 0.86 in Equation (10) suggests that the prediction method is solid, the value of RMSE at 6.65 additionally confirms it. The purpose of this approach is to initially determine the strength of cavitation using simple input data, which is fulfilled. To address the question of how significant the error is, it is necessary to consider the application of real-time prediction with this algorithm. According to Table 5, cavitation starts with a 3.42 kg/s mass flow and a cavitation strength equal to 47.4. Similarly to the Thoma number, there is no hard threshold for the inception of cavitation and this number will always be dependent on the case and chosen setups. While adjusted to the specific case, this approach should always keep as much space as possible for states where cavitation is present, which means, the lower the cavitation inception is (in terms of cavitation power value), the better the accuracy of this prediction. It is possible that further expansion of the data (more cases with different operating conditions) and more specific curve-fitting strategies might address this problem.

The developed approach can serve as a solid basis for further validation and development. Other regression models could be applied (especially polynomial regression with different levels of polynomials). Cavitation can be predicted with CFD and its results can be considered as input data for the building of predictive indicators. The data that can be acquired with CFD is abundant and it is possible that many parameters can be used for the creation of likewise indicators. However, it is important to choose easily measurable properties of flow that can be read with the simplest possible sensors (due to economic reasons). This work only uses head and mass flow rate as they are easily measurable; however, it is very likely that this kind of indicator can be expanded with other properties of flow, allowing for more accurate prediction. Additionally, it is possible that a larger pool of simulation results would allow further adjustment of the prediction ability of this approach. Furthermore, the work does not address the question of whether the approach can be generalized for other geometries (only one PAT geometry was used in the research) and could produce an error in prediction.

The main reason for the application of CFD in this research is to find a method of accurate quantitative description of cavitation. Visual observation of cavitation intensity is highly subjective and prone to significant error, making it unreliable. In case of the existence of other methods that could very accurately describe the cavitation intensity in an experimental environment, this approach could be repeated with a significant increase in the amount of data.

As presented in Figure 14, the Thoma number exhibits a relatively small and nearly linear variation across the operating points, typically within a ±5% range. Visual observations of cavitation inception and development show that the cavitation progresses in a nonlinear manner. There is an initial region where variations in the Thoma number have no impact on the cavitation (non-cavitating regime), followed by a narrow transition zone in which cavitation initiates abruptly (cavitation inception), and finally, a regime of rapidly intensifying cavitation (fully developed cavitation). The Thoma number does not capture these transitions effectively, as it continues to increase uniformly across all regimes—regardless of whether cavitation is present or not. In contrast, CP remains stable in the non-cavitating range but exhibits a significant increase precisely at the onset of cavitation, followed by a second large rise corresponding to the transition into intense cavitation. These stepwise changes in CP are consistent with visual evidence of vapour formation, underscoring the indicator’s ability to reflect critical changes in cavitation dynamics. This analysis shows that CI is a more sensitive and informative indicator of cavitation onset and severity than the Thoma number.

5. Conclusions

As CFD is a viable tool for the examination of cavitation occurring in the turbine, data provided by it can be used for building predictive models.

This study demonstrates that cavitation strength in a pump-as-turbine (PAT) can be reasonably predicted using simple and easily measurable parameters such as head and mass flow rate. In general, cavitation strength is able to predict cavitation like the Thoma number, but with improved accuracy in edge cases. The developed linear regression model achieved a high R² value, indicating good predictive potential. The simplicity of the method allows for quick, preliminary assessments of cavitation development, which can be particularly useful in real-time monitoring scenarios. While the prediction error is acceptable for distinguishing between strong and weak cavitation states, it might not capture more subtle behaviours. The findings using simple inputs can still offer a practical and scalable approach for early-stage diagnostics.

Furthermore, this work highlights the importance of using CFD simulations as a source of data for indicator development, particularly when visual methods fail to provide reasonable accuracy. The use of easily obtainable parameters increases the feasibility of implementation in real-world applications. To further improve the accuracy and generalizability, future development should consider expanding the dataset with more varied operating conditions and geometries, and exploring advanced regression techniques such as polynomial models or machine learning approaches.

Overall, the presented approach provides a solid foundation for developing practical cavitation prediction tools.