Joint Assessment of Hydraulic Instabilities and Pressure-Fluctuation Signatures in a Pump as Turbine (PAT) Using Transient Computational Fluid Dynamics and Signal Processing

2.1 Geometry and Pump as Turbine description

The hydraulic machine analyzed in this study corresponds to a centrifugal pump model 32-125 adapted to operate as a PAT. The internal fluid domain was reconstructed in ANSYS Space Claim based on the main geometric dimensions of the original equipment. The machine consists of a radial impeller housed inside a single-volute casing and connected to a rotating shaft.

The impeller diameter is 154 mm, the nominal rotational speed is 2,900 rpm, and the rotor contains nine blades. The nominal pump flow rate under conventional operation is 20 m³/h.

The main geometric and operating parameters of the analyzed PAT are summarized in Table 1.

Table 1. Main geometric and operating parameters of the Pump as Turbine (PAT)

Regarding materials, the casing was considered as grey cast iron EN-GJL-250, while the impeller was assumed to be manufactured from AISI 316 stainless steel due to its superior resistance to corrosion and cavitation damage.

2.2 Computational domain and mesh generation

The computational domain was divided into three regions: the inlet section, the rotating impeller domain, and the outlet volute region. To ensure the proper transfer of flow variables between the stationary and moving zones, the shared topology technique was used, and non-conforming mesh interfaces were configured. An unstructured mesh was generated using primarily tetrahedral elements due to the geometric complexity of the impeller and volute, which facilitates adequate discretization of curved surfaces and regions with abrupt geometric changes. This type of mesh is widely used in CFD simulations of hydraulic turbomachinery due to its geometric flexibility and ability to represent complex rotating domains [11, 18-25]. Additionally, automatic local refinements were applied in regions near the blades and areas of high curvature to improve the resolution of velocity and pressure gradients.

To properly capture the flow gradients and complex geometry of the blades, automatic refinement functions for curvature and proximity were activated on the impeller surfaces. This allows for a smooth mesh transition and an automatic increase in element density at the leading and trailing edges of the blades, ensuring the quality necessary for model convergence.

The three-dimensional geometry of the PAT is illustrated in Figure 1.

Figure 1. Geometry of the Pump as Turbine (PAT)

The computational mesh generated for the CFD simulations is presented in Figure 2.

Figure 2. Computational domain mesh

2.3 Governing equations

The internal hydrodynamic behavior of the PAT was investigated using a transient CFD model, combined with post-processing of the pressure signal. The methodology combines flow simulation with turbulence resolution, cavitation prediction, vortex identification, and time-frequency analysis to characterize the relationship between hydraulic instabilities and pressure-based vibro-acoustic indicator.

The governing flow field was solved using the incompressible Reynolds-Averaged Navier-Stokes (RANS) equations. The continuity equation is written as Eq. (1):

$\begin{gathered}\frac{\partial \bar{u}_i}{\partial x_i}=0 \rho\left(\frac{\partial \bar{u}_i}{\partial t}+\bar{u}_j \frac{\partial \bar{u}_i}{\partial x_j}\right) =-\frac{\partial \bar{p}}{\partial x_i}+\frac{\partial}{\partial x_j}\left(\mu \frac{\partial \bar{u}_i}{\partial x_j}-\rho \overline{u_i u_j}\right) \bar{u}_i\end{gathered}$          (1)

where, $\bar{u}_i$ and $\bar{p}$, are the averaged velocity and pressure, and $y-\rho \overline{u_i u_j}$ is the Reynolds stress tensor.

To improve the prediction of unstable separated flow and rotor-stator interaction, the SAS-SST turbulence model was adopted. This model allows for the capture of transient turbulent structures and separation regions with greater accuracy than conventional RANS models, especially in applications dominated by vortex shedding and strong pressure gradients. Previous studies related to vortex dynamics, cavitation, and transient CFD simulations in turbomachinery have demonstrated that adaptive resolution approaches are suitable for analyzing highly unstable hydraulic phenomena [14-20]. Consequently, the SAS-SST model is appropriate for studying the hydrodynamic and vibro-acoustic behavior of the analyzed PAT system.

Coherent vortical structures are identified and quantified using the Q-criterion [18], defined as the second invariant of the velocity gradient tensor $\nabla v$:

$Q=\frac{1}{2}\left(\|\Omega\|^2-\|S\|^2\right)$          (2)

where, S is the strain-rate tensor:

$S=\frac{1}{2}\left(\nabla \vec{v}+(\nabla \vec{v})^T\right)$          (3)

and Ω is the rotation tensor:

$\Omega=\frac{1}{2}\left(\nabla \vec{v}-(\nabla \vec{v})^T\right)$          (4)

Regions with Q > 0 (where rotation dominates over shear strain) are identified as vortex cores. Vorticity is written as Eq. (5):

$\vec{\omega}=\nabla \times \vec{v}$          (5)

Cavitation is predicted using a mass transport model for the vapor fraction α_v. The Schnerr-Sauer model is employed, defining the evaporation and condensation rates $\dot{\mathrm{R}}_{\mathrm{e}}$ and $\dot{\mathrm{R}}_{\mathrm{c}}$ as:

$\begin{aligned} & \dot{R}_e=\frac{3 \rho_v \rho_l}{\rho} \alpha_v\left(1-\alpha_v\right) \frac{1}{R_B} \sqrt{\frac{2}{3} \frac{\max \left(\rho_v-\rho, 0\right)}{\rho_l}}, \text { si } \mathrm{p} \leq \mathrm{pv}\end{aligned}$          (6)

$\dot{R}_c=\frac{3 \rho_v \rho_l}{\rho} \alpha_v \frac{1}{R_B} \sqrt{\frac{2}{3} \frac{\max \left(\rho-\rho_v, 0\right)}{\rho_l}}$, si $\mathrm{p} \geq \mathrm{pv}$          (7)

where, ρ_l and ρ_v are the liquid and vapor densities, R_B is the bubble radius, ρ is the local pressure, and ρ_v is the vapor pressure. The evolution of the vapor fraction is written as Eq. (8):

$\frac{d}{d t}\left(\alpha_v \rho_v\right)+\nabla \cdot\left(\alpha_v \rho_v \vec{v}\right)=\dot{R}_e-\dot{R}_c$          (8)

The cavitation number σ was calculated as Eq. (9):

$\sigma=\frac{p_{ {inlet }}-p_v}{\frac{1}{2} \rho U_{{tip }}^2}$          (9)

The cavitation parameters obtained were used as supplementary indicators to assess trends in cavitation susceptibility under various operating conditions of the PAT.

And the available suction head is written as Eq. (10):

$N P S H_d=\frac{p_{{inlet }}-p_v}{\rho g}$          (10)

Here, U_tip is the impeller tip speed and p_inlet is the inlet pressure. In this study, a practical engineering criterion was adopted whereby cavitation susceptibility was considered significant when the vapor volume exceeded 0.5% of the rotor-domain volume. This threshold was introduced as an internal indicator to facilitate comparison among operating conditions and should not be interpreted as a universally validated cavitation inception criterion. This criterion is used as a practical reference to identify the initial development of significant cavitation within hydraulic turbomachines, allowing the growth of vapor cavities to be associated with increased hydraulic instabilities and pressure fluctuations [7, 12].

Vibrational excitation is analyzed based on time series of fluctuating pressure p(t) extracted at critical points in the domain (housing, blade, rotor-volute interface). The frequency content is obtained using the FFT, by calculating the Power Spectral Density (PSD):

$P_{x x}(f)=\frac{1}{N F_s}\left|\sum_{n=1}^n p[n] e^{-\frac{i 2 \pi f n}{F_s}}\right|^2$          (11)

To evaluate transient spectral evolution caused by intermittent cavitation and vortex shedding, the STFT was applied:

$\operatorname{STFT}(t, f)=\int_{-\infty}^{\infty} p(\tau) w(\tau-t) e^{-i 2 \pi f \tau} d \tau$          (12)

Using a Hamming window w(t). The blade passing frequency (BPF) and its harmonics, which are mainly responsible for forced excitation, are calculated with Eq. (13):

$B P F=\frac{N_{ {blades }} \cdot R P M}{60}$          (13)

This parameter allows quantifying the dynamic correlation between pressure sources in different regions of the PAT.

Finally, the combined hydraulic and spectral indicators were integrated into an operational map that correlates mass flow rate, pressure head, vortex intensity, and dominant spectral amplitudes. This approach makes it possible to identify stable, transient, and potentially unstable operational regions for PAT applications.

The hydraulic head was calculated from the pressure difference between the inlet and outlet sections according to Eq. (14):

$H=\frac{P_{ {inlet }}-P_{ {outlet }}}{\rho g}$          (14)

where, H is the hydraulic head (m), P_inlet and P_outlet are the area-average static pressures obtained from CFD (Pa), ρ is the water density (kg·m^-3) and g is the gravitational acceleration (9.81 m·s^-2).

2.4 Mesh independence study

To ensure that the numerical results were independent of mesh resolution while maintaining a reasonable computational cost, a mesh independence study was carried out. Five meshes with different densities were generated by varying the base element size. The study was performed under nominal operating conditions, using an inlet mass flow rate of 5 kg/s for the simulation. The control variable selected to evaluate convergence was the torque generated by the impeller. The details of the evaluated meshes are summarized in Table 2.

Table 2. Mesh independence study and torque convergence

A mesh independence analysis was performed to evaluate the influence of mesh refinement on the torque obtained in the simulation. To this end, five mesh levels were generated with progressively smaller element sizes, ranging from 0.003 m to 0.0015 m. The results show that the torque exhibits significant variations in the initial stages of refinement, with a relative difference of 4.95% between the first two meshes. However, starting with the third mesh, these variations decrease considerably, reaching values of 2.66%, 1.22%, and finally 0.04% between consecutive refinements. This behavior demonstrates a clear trend toward numerical convergence, indicating that the result becomes practically independent of the mesh size. Consequently, mesh 4 is considered an adequate solution, as it offers an optimal balance between accuracy and computational cost, without additional refinements generating significant changes in the calculated torque.

The convergence trend observed in this study is consistent with previous numerical research on hydraulic turbomachinery and PAT systems, where further refinements beyond a certain number of elements result in minimal changes in integral parameters such as head, torque, or efficiency. Several authors report that differences of less than 2% between consecutive refinements can be considered acceptable to ensure mesh independence in transient CFD simulations of hydraulic pumps and turbines [18, 19]. In this case, mesh 4 showed a reduced variation compared to the most refined mesh, maintaining adequate numerical stability and a reasonable computational cost.

Mesh 4, consisting of 923, 376 elements, was selected for all subsequent steady and transient simulations because the torque difference relative to the finest mesh (Mesh 5) was only 0.04%, while requiring lower computational cost.

2.5 Boundary conditions and numerical setup

The numerical simulation was developed considering the operation of the pump in turbine mode (PAT), reversing the flow direction compared to its conventional operation. The main numerical setup and boundary conditions are summarized in Table 3. The computational domain consisted of two stationary regions (suction and volute) and one rotating region corresponding to the impeller.

Table 3. Main numerical setup and boundary conditions

At the inlet of the domain, corresponding to the original discharge of the pump, a mass flow inlet boundary condition was imposed, defining a mass flow rate of 5 kg/s for the case that used the SST-SAS turbulence model, a representative value of the hydraulic performance condition obtained in the study. At the outlet, associated with the original suction, an opening condition with a static reference pressure was established, allowing the development of a transient recirculation without compromising numerical stability.

The impeller was modeled using a rotating reference frame with a constant angular velocity of 2,900 rpm, while the remaining regions were maintained in a stationary reference frame. All solid surfaces were defined with a no-slip condition, assuming hydraulically smooth walls.

The interaction between the rotating and stationary domains was resolved using fluid-fluid interfaces. The frozen rotor scheme was used to initialize the flow field, obtaining an initial steady-state solution. Subsequently, the transient analysis was carried out using the transient rotor-stator model, which allowed capturing the unsteady effects associated with the periodic passage of the blades and the rotor-stator interaction.

The working fluid was modeled as incompressible liquid water at room temperature. Cavitation was represented using the Schnerr-Sauer model, which simulates the processes of evaporation and condensation based on the local fluid pressure.

The Schnerr-Sauer cavitation model was implemented using the default parameters of the ANSYS CFX solver for liquid water and water vapor at room temperature. The model considers a constant initial bubble radius, as well as evaporation and condensation mechanisms controlled by local differences between the fluid pressure and the vapor pressure. The vapor pressure of water was set considering operating conditions at 25 ℃, while the thermophysical properties of the liquid and vapor were automatically defined by the software library. This approach has been widely used in CFD simulations of cavitation in pumps and hydraulic turbomachines [7, 12, 17, 25].

A second-order scheme was employed for spatial discretization, ensuring an adequate resolution of pressure and velocity gradients. The pressure-velocity coupling was resolved using the implicit algorithm of the ANSYS CFX solver.

The convergence of the solution was evaluated by monitoring the residuals of the conservation equations, setting a criterion of values below 10⁻⁵. Additionally, the stability of integral variables such as torque and mean pressure at the control points was verified, ensuring the consistency of the transient solution.

The main numerical setup and boundary conditions adopted in the transient CFD simulations are summarized in Table 3.

Hydraulic performance calculations were performed for five operating conditions ranging from 1 to 5 kg/s. However, the detailed transient CFD simulation, including SAS-SST turbulence modeling, Schnerr, Sauer cavitation modeling, pressure signal extraction, FFT, STFT, turbulent kinetic energy (TKE) analysis and Q-criterion vortex identification, was conducted only for the 5 kg/s case, which exhibited the highest hydraulic head within the investigated range.

2.6 Transient configuration and monitoring points

The numerical analysis was performed using the transient solver ANSYS CFX to capture the unsteady state phenomena associated with vortex dynamics and cavitation in the PAT.

The SAS-SST model was used to model the turbulence. This model allows for the resolution of turbulent structures of different scales through the dynamic adaptation of the turbulent length scale, improving the prediction of transient phenomena compared to conventional RANS models.

The phenomenon of cavitation was incorporated using the Schnerr-Sauer model, based on the dynamics of spherical bubbles. This model simulates the processes of growth and collapse of vapor cavities based on local pressure variations.

The simulation was run in transient mode with a time step of 0.0005 s, chosen as a compromise between temporal resolution and computational cost. The total simulation time was 0.1148 s, approximately equivalent to 5.5 complete revolutions of the impeller. This time interval allowed for the proper capture of the periodic nature of pressure fluctuations and the development of transient vortical structures within the domain. Previous studies on transient hydraulic turbomachinery and PAT systems have shown that several consecutive revolutions are generally sufficient to obtain representative pressure signals for spectral analysis and characterization of unsteady flow phenomena [11, 12, 17]. Additionally, during the simulation, the periodic stabilization of monitored variables such as pressure and torque was verified, ensuring the temporal representativeness of the obtained results. This value allows for the correct capture of periodic fluctuations associated with the rotation frequency, rotor-stator interaction, and transient vortex structures present in hydraulic turbomachines. Previous research on transient CFD simulations of cavitating hydraulic machinery has employed time steps of the same order of magnitude to resolve unsteady pressure fluctuations and vortex related phenomena [11, 12, 17]. Moreover, the time step size provides sufficient resolution for subsequent spectral analysis using FFT and STFT.

It was verified that the time step size meets an appropriate temporal resolution criterion for the system's characteristic frequencies, particularly the rotational frequency and its harmonics.

For the vibro-acoustic analysis, three pressure monitoring points were defined in critical regions of the domain: (i) the suction zone, (ii) the interior of the impeller, especially in areas prone to cavitation, and (iii) the zone of the volute blade, where rotor-stator interaction occurs.

The pressure signals obtained at these points were recorded over time and subsequently processed using spectral analysis tools, specifically the FFT and the STFT, to identify the dominant frequencies and their temporal evolution. This configuration allowed for a direct correlation to be established between the unsteady flow structures, cavitation activity, and the pressure-based vibro-acoustic indicator of the system.

2.7 Signal processing (Fast Fourier Transform/Short-Time Fourier Transform)

The transient pressure signals recorded at the monitoring points (suction region, impeller zone, and tongue of the volute) were exported from ANSYS CFX in CSV format and subsequently processed in MATLAB. The sampling interval was equal to the transient CFD time step, Δt = 0.0005 s, resulting in a sampling frequency of 2000 Hz and a Nyquist limit of 1000 Hz.

Before the frequency analysis, the mean value of each pressure signal was removed to isolate the fluctuating component. Next, the FFT was applied to each dataset, and the corresponding unilateral amplitude spectra were obtained to identify the dominant excitation frequencies.

Comparative FFT spectra were generated for the three monitoring points in order to determine the region with the highest pressure pulsation intensity. Special attention was given to the impeller region due to its greater susceptibility to vortex interaction and cavitation-related instabilities.

To investigate the unsteady behavior, the STFT was applied to the impeller pressure signal using overlapping moving windows with an 80% overlap. The FFT length was automatically adjusted according to the selected window size. The resulting spectrograms allowed the identification of transient frequency bands possibly associated with vortex shedding, rotor-stator interaction and intermittent cavitation-related phenomena.

The MATLAB post-processing procedure provided the spectral indicators used to correlate the hydraulic instabilities predicted by CFD with the pressure-based vibro-acoustic indicator of the PAT.

A transient CFD methodology was developed to investigate the coupled hydraulic and dynamic behavior of a centrifugal PAT. The combination of the SAS-SST turbulence model with the Schnerr-Sauer cavitation model proved to be suitable for capturing the main unstable flow structures within the machine, including vortex formation, pressure fluctuations, and regions susceptible to the onset of cavitation.

The analysis of the internal flow revealed that the highest turbulent activity was concentrated near the trailing edges of the blades and the tongue of the volute. These regions were characterized by strong velocity gradients, wake interaction, and local recirculation, indicating that they are the main sources of hydraulic losses and dynamic excitation during reverse operation.

The Q-criterion analysis indicated the presence of coherent vortex structures within the impeller passages. Some vortices remained attached to the blade surfaces, while others were convected downstream, generating periodic disturbances in the pressure field. This demonstrates that the dynamics of the vortices play a fundamental role in the transient stability of PAT systems.

According to the hydraulic evaluation, the input mass flow rate of 5 kg/s produced the highest simulated lift height within the evaluated operating range, representing the hydraulically favorable condition within the investigated flow-rate range among the tested cases. This result is relevant for practical applications, as PAT systems often operate under variable flow demand and require stable operating zones.

The vibro-acoustic analysis revealed that the impeller region was the main source of pressure pulsations. An important spectral peak was identified at 94.45 Hz, close to the second harmonic of the shaft rotation frequency, indicating that the rotor movement and the interaction between the blades and the flow significantly influence the dynamic response.

The results of the STFT showed intermittent frequency bands over time, confirming that the pressure signal is non-stationary and influenced by multiple transient mechanisms, such as vortex shedding, rotor-stator interaction, and possible local cavitation-related phenomena. This finding underscores the importance of combining conventional FFT with time-frequency methods for the diagnosis of PAT.

Overall, the results suggest a relationship between internal hydraulic instabilities and the pressure-based vibro-acoustic indicator of the machine. Therefore, monitoring the pressure signal, with the support of CFD analysis, can be considered a useful tool for detecting unfavorable operating conditions and improving the reliability of the PAT.

The present study is limited by the absence of experimental validation and by the use of a rigid wall fluid model that does not consider the effects of fluid-structure interaction. In future work, laboratory measurements, the coupling of structural vibrations, efficiency calculations, and expanded operating maps under more diverse flow conditions should be included.