# Numerical simulation of cavitating flows: comparison between two-fluid and homogeneous approaches

Jacques Ferhat, Christophe Leclercq, Regiane Fortes Patella, Antoine Archer, Stéphane Mimouni, Tayeb Aiouaz

► To cite this version:

Jacques Ferhat, Christophe Leclercq, Regiane Fortes Patella, Antoine Archer, Stéphane Mimouni, et al.. Numerical simulation of cavitating flows: comparison between two-fluid and homogeneous approaches. IOP Conference Series: Earth and Environmental Science, 2022, 1079 (1), pp.012045. 10.1088/1755-1315/1079/1/012045 . hal-04987425

HAL Id: hal-04987425

https://hal.science/hal-04987425v1

Submitted on 12 Mar 2025

HAL is a multi-disciplinary open access
archive for the deposit and dissemination of sci-
entific research documents, whether they are pub-
lished or not. The documents may come from
teaching and research institutions in France or
abroad, or from public or private research centers.

L'archive ouverte pluridisciplinaire HAL, est
destinée au dépôt et à la diffusion de documents
scientifiques de niveau recherche, publiés ou non,
émanant des établissements d'enseignement et de
recherche français ou étrangers, des laboratoires
publics ou privés.

<figure><img src="image_1.png" /></figure>

Distributed under a Creative Commons Attribution 4.0 International License
PAPER • OPEN ACCESS

# Numerical simulation of cavitating flows: comparison between two-fluid and homogeneous approaches

To cite this article: J Ferhat et al 2022 IOP Conf. Ser.: Earth Environ. Sci. 1079 012045

View the [article online](#) for updates and enhancements.

You may also like

- [Experimental measurements of the cavitating flow after horizontal water entry](#)
Thang Tat Nguyen, Duong Ngoc Hai, Nguyen Quang Thai et al.

- [Hydrodynamic cavitation in microfluidic devices with roughened surfaces](#)
Morteza Ghorbani, Abdolali K Sadaghiani, L Guillermo Villanueva et al.

- [Evaluation of the physical forces exerted on a spherical bubble inside the nozzle in a cavitating flow with an Eulerian/Lagrangian approach](#)
Seyed Mohammad Javad Zeidi and Miralam Mahdi

UNITED THROUGH SCIENCE & TECHNOLOGY

<figure><img src="image_2.png" /></figure>

The Electrochemical Society
Advancing solid state & electrochemical science & technology

248th
ECS Meeting
Chicago, IL
October 12-16, 2025
Hilton Chicago

<figure><img src="image_3.png" /></figure>

Science +
Technology +
YOU!

SUBMIT
ABSTRACTS by
March 28, 2025

SUBMIT NOW
# Numerical simulation of cavitating flows: comparison between two-fluid and homogeneous approaches

J Ferhat<fnref n="1" />,<fnref n="2" />, C Leclercq<fnref n="1" />,<fnref n="2" />,<fnref n="4" />, R Fortes-Patella<fnref n="1" />, A Archer<fnref n="2" />, S Mimouni<fnref n="2" /> and T. Aiouaz<fnref n="3" />

**Abstract.** The paper presents a new two-phase flow approach to simulate unsteady cavitating flows. The study applied the in-house code *neptune_cfd*, which allows two-fluid modelling of liquid-vapor flows [1]. The code solves the ensemble-averaged equations of mass, momentum and energy conservation for each phase (liquid and vapour) for a total of six conservation equations. The equations system requires closure laws for the interfacial terms that represent the mass, momentum and energy transfers occurring between the liquid and vapor phases. An original approach is implemented by using an energy-source term based on the difference between the local enthalpy and its saturation value. 2D and 3D simulations are carried out for a NACA 65-012 hydrofoil with an angle of attack of 6°, a cavity length of 40% of the hydrofoil chord and different flow velocities. The methodology to obtain the cavity length and the main frequency of its periodic behavior is presented. Then the numerical results are compared with those previously obtained by a homogeneous approach [2] and with the available experimental data [3]. The quantitative predictions of the hydrodynamic characteristics (i.e. cavitation sigma number, cavity length, shedding frequency and cavity shape) obtained from two-phase flow modeling appear in better accordance with experimental data.

## 1. Introduction

The vast majority of existing work developed to simulate cavitating flows is based on homogeneous approaches (initially proposed, for example, by [4-6]). Only few studies develop two-fluid methods to simulate cavitation. They are essentially based on dispersed phase flow approaches, which can be classified into:

* the Eulerian-Lagrangian approach: the liquid is considered as a continuum while the dispersed phase consists in particles that are tracked during the simulation [7-11]

* Eulerian-Eulerian approach: both phases are considered as continua interacting each other by means of interfaces [1,12].

In previous studies developed in the frame of collaborations between the University of Grenoble (France), EDF (Electricité de France) and the CETIM (technical centre for the mechanical industries), a methodology for predicting the aggressiveness of cavitation has been proposed and applied in the case of hydrofoils and centrifugal pumps by using homogeneous numerical approaches [2,13-16].

Currently, unsteady viscous cavitating flows simulations are carried out using the code *neptune_cfd*, which allows two-fluid modelling of liquid-gas flows and assumes a pressure equilibrium between phases [1]. This paper describes the recent improvements in physical modelling to adapt the code to cavitating flow simulations. The first validations of the numerical and physical models are carried out for a NACA 65-012 hydrofoil tested by [3]. The numerical

<figure><img src="image_4.png" /></figure>

<footnote n="1">¹Univ. Grenoble Alpes, Grenoble INP, LEGI, 38000 Grenoble, France</footnote>

<footnote n="2">²EDF R&D, 6 quai Watier, 78400 Chatou, France</footnote>

<footnote n="3">³CETIM, 74 route de la Jonelière, 44300 Nantes, France</footnote>

<footnote n="4">⁴OSE Engineering, 1 route de Versailles, 78470 Saint-Rémy-Lès-Chevreuse, France
Corresponding author's e-mail address: regiane.fortes-patella@univ-grenoble-alpes.fr</footnote>
results are compared also with those previously obtained by homogeneous approach described in [2].

The section 2 presents the hydrofoil geometry, the mesh, and the tests conditions considered in the study. The homogeneous and the two-phase flow approaches are detailed in the section 3. Simulation results using these two approaches are compared to each other and to experimental data in section 4. Qualitative visualization and then quantitative results for cavity length, sigma number and shedding frequency are defined and analysed.

## 2. Hydrofoil geometry, meshes and test conditions

The geometry considered in this study is a NACA 65-012 hydrofoil tested at EPFL [3] (figure 1). The profile chord is 100 mm long and its spanwise is 150 mm. The test cross section is 150 mm\*150 mm. The analyses presented in this paper concern results obtained with an angle of attack of 6°.

<figure><img src="image_5.png" /><figcaption>**Figure 1.** Test-section and hydrofoil geometry - NACA 65-012 [2].</figcaption></figure>

The simulations have been carried out for three different mesh levels (table 1). The influence of the mesh has been analyzed in [2] for homogeneous approach and in [17] for two-fluid model. A medium mesh has been chosen for two-fluid approach but differs from homogeneous one. The *Code_saturne* mesh is coarser but was considered fine enough for the homogeneous approach. The results presented in this paper with the two-fluid approach concern the medium mesh (92 cells on chord and 200 cells spanwise for the 3D case) (figure 2). The applied boundary conditions are indicated in figure 2a.

<table><caption>**Table 1.** 2D Mesh characteristics for the two-fluid study. 3D meshes for two-fluid study are obtained with extrusion of 200 cells spanwise. The 3D mesh used for the homogeneous study is the coarse mesh with 59 cells spanwise.</caption><thead><tr><td>Mesh</td><td>Cells on chord [-]</td><td>1<sup>st</sup> cell height [m]</td><td>Mean y<sup>+</sup></td><td>Total number of cells [-]</td></tr></thead><tbody><tr><td>Coarse</td><td>58</td><td>1.10<sup>-4</sup></td><td>70</td><td>15.5.10<sup>3</sup></td></tr><tr><td>Medium</td><td>92</td><td>5.10<sup>-5</sup></td><td>38</td><td>21.7.10<sup>3</sup></td></tr><tr><td>Fine</td><td>177</td><td>5.10<sup>-5</sup></td><td>38</td><td>89.7.10<sup>3</sup></td></tr></tbody></table>
<figure><img src="image_6.png" /><figcaption>**Figure 2.** (a) Numerical boundary conditions; (b) enlarged view around the foil of the H-grid of the medium mesh used with *neptune_cfd*.</figcaption></figure>

The tests conditions are presented in table 2. For these operating points the length of the cavity is 40% of the chord and the cavitation number $\sigma$ is defined as:

$$ \sigma = \frac{P_{in} - P_{sat}}{0.5 \rho_l V_{in}^2} \quad (1) $$

where $P_{in}$ and $V_{in}$ are the inlet pressure and the inlet axial mean velocity; $P_{sat}$ is the ambient saturation pressure at 20°C. The sigma number is fixed in order to have a constant mean cavity length of 40% of the chord length. It slightly increases with the increase of the inlet velocity. Experimental results of pitting tests carried out by [3] are available for these operating points and will allow the validation of the upcoming numerical prediction of cavitation aggressiveness. Further simulations will be done in the future by considering other angles of attack and operating conditions.

<table><caption>**Table 2.** Experimental flow conditions and frequency f of the shedding cavitating structures (corresponding to a cavity length of ~ 40% of the chord).</caption><thead><tr><th>V<sub>in</sub> [m/s]</th><th>15</th><th>20</th><th>25</th><th>30</th></tr></thead><tbody><tr><td>σ [-]</td><td>1.59</td><td>1.60</td><td>1.62</td><td>1.63</td></tr><tr><td>f [Hz]</td><td>100</td><td>140</td><td>190</td><td>220</td></tr></tbody></table>

### 3. Numerical approaches

To simulate the unsteady cavitating flow around the hydrofoil, two codes have been applied: the homogeneous numerical *Code_Saturne* with cavitating module [2] and the two-fluid code *neptune_cfd* [1]. The former is a free open source CFD software developed by EDF while the latter is a solver co-developed by EDF, CEA (Commissariat à l'Energie Atomique et aux Energies Alternatives), IRSN (Institut de Radioprotection et de Sûreté Nucléaire) and Framatome for nuclear safety applications. This code has been widely used and validated with various types of flows: adiabatic and thermal two-phase flows, boiling and pressurized thermal shocks.
The two codes are based on 3D finite-volume discretization of turbulent Navier-Stokes equations with a collocated arrangement of variables. They share common libraries and can handle large meshes with large parallelization capabilities. Hereafter the main features of both codes are presented.

### 3.1 Homogeneous approach of Code_Saturne

Code_Saturne has a dedicated cavitation module that enables the resolution of homogeneous mixture model for mass (2) and momentum (3) conservation associated with the mass conservation equation for the vapor phase (4). Pure phases have constant properties (density $ρ_l$ and dynamic viscosity $μ_l$) following the relations: $ρ = αρ_v + (1 - α)ρ_l$ and $μ = αμ_v + (1 - α)μ_l$. The energy equation is not solved.

$$ \frac{\partial \rho}{\partial t} + \text{div}(\rho u) = 0, \qquad (2) $$

$$ \frac{\partial \rho u}{\partial t} + \text{div}(u \otimes \rho u) = -\nabla p + \text{div}(\tau), \qquad (3) $$

$$ \frac{\partial \rho_v \alpha}{\partial t} + \text{div}(\rho_v \alpha u) = \Gamma_v, \qquad (4) $$

$\Gamma_v$ is the vaporization source term modeled using the Merkle model [18]:

$$ \Gamma_v = m^+ + m^-, \qquad (5) $$

$$ \text{with: } m^+ = - \frac{c_{prod} \rho_l \min(p-p_{sat},0)(1-\alpha)}{\frac{1}{2} \rho_l u_{\infty}^2 t_{\infty}} \quad \text{and} \quad m^- = - \frac{c_{dest} \rho_v \max(p-p_{sat},0)\alpha}{\frac{1}{2} \rho_l u_{\infty}^2 t_{\infty}}. $$

Here $C_{prod} = 10 000$, $C_{dest} = 50$ are empirical constants, $t_{\infty} = l_{\infty}/u_{\infty}$ is a reference time scale and $p_{sat}$ is the reference saturation pressure. The parameters $l_{\infty}$, $u_{\infty}$ and $p_{sat}$ should be provided by the user ($l_{\infty} = 0.1 \text{ cm}$, $u_{\infty} = 15$ to $30 \text{ m.s}^{-1}$, $p_{sat} = 2000 \text{ Pa}$, $ρ_l = 1000 \text{ kg.m}^{-3}$, $ρ_v = 1 \text{ kg.m}^{-3}$, $μ_l = 10^{-3} \text{ Pa.s}$ and $μ_v = 10^{-5} \text{ Pa.s}$ in this study). A standard k-ε turbulent model with Reboud correction [19] is used to take into account the influence of the compressibility of the two-phase medium on turbulence. The resolution scheme is based on a co-located fractional step scheme, which is associated with the SIMPLEC-type algorithm (see [2] for more details). Simulations are performed with a Courant-Friedrichs-Lewy (CFL) kept under 1.

### 3.2 Two-fluid approach of neptune_cfd

neptune_cfd is based on the so called two-fluid one pressure model extended to n-phases [1]. An ensemble-average is applied on constitutive conservation equations (mass, momentum and energy). This leads to a dedicated system of conservation equations and variables for each phase, except for pressure, which is the same for the phases. The present work considers two phases (liquid and vapor water) and a system of 6 conservation equations.

The system of equations is solved using a pressure correction along with fractional time-step approach. Physical properties of the pure phases such as density, heat coefficient, saturation properties, etc are obtained via the CATHARE thermodynamic tables for water [20]. Solved variables are two sets (for both phases) of velocity, total enthalpy, temperature and void fraction.

For each phase k (assumed l for liquid and v for vapor), the conservation equations for mass and momentum are (6) and (7):

$$ \frac{\partial \alpha_k}{\partial t} + \text{div}(\alpha_k \rho_k \bar{U}_k) = \Gamma_k, \qquad (6) $$
$$ \frac{\partial \alpha_k \rho_k \bar{U}_k}{\partial t} + \overline{div}(\bar{U}_k \otimes \alpha_k \rho_k \bar{U}_k) = \overline{div}(\alpha_k \bar{\Sigma}_k) - \alpha_k \overline{\nabla} P + \alpha_k \rho_k \bar{g} + \overline{M}_k, \quad (7) $$

where, $\alpha_k$ is the void fraction, $\rho_k$ is the density, $\bar{U}_k$ is the velocity, $\Gamma_k$ is a closure term responsible for mass transfer at the interface, $\bar{\Sigma}_k$ is the strain tensor, $P$ is the pressure, $\bar{g}$ is the gravity and $\overline{M}_k = \Gamma_k \bar{U}_k^l + \overline{M}_k^l$ is a closure term for momentum exchange between phases. The energy equation (8) is expressed as total enthalpy: $H_k = e_k + \frac{1}{2} u_k^2 + \frac{P}{\rho_k}$, with $e_k$ the internal energy.

$$ \frac{\partial \alpha_k \rho_k H_k}{\partial t} + \overline{div}(\alpha_k \rho_k H_k \bar{U}_k) = \alpha_k \frac{\partial}{\partial t} P + \alpha_k \rho_k \bar{g} \cdot \bar{U}_k - \overline{div}(\alpha_k Q_k) + \overline{div}(\alpha_k \bar{\Sigma}_k \cdot \bar{U}_k) + \overline{M}_k^l \cdot \bar{U}_k^l + \pi_k, \quad (8) $$

where, $Q_k$ is heat transfer, $\overline{M}_k^l$ and $\bar{U}_k^l$ are the momentum transfer and the velocity at the interface, and $\pi_k = \Gamma_k H_k^l + Q_k^l$ is the source term for energy exchange between phases.

Interfacial source terms ($\Gamma_k$, $\overline{M}_k$, $\pi_k$) appear in the conservation equations (6, 7, 8). They account for interaction between phases and need to be modelized (see [17]). They follow jump conditions to close the system, respectively by developing the source terms expressions:

$$ \sum_k^n \Gamma_k = 0, \quad (9) $$

$$ \sum_k^n \Gamma_k \bar{U}_k^l + \overline{M}_k^l = 0, \quad (10) $$

where, the momentum source terms $\overline{M}_k^l$ are those from the dispersed bubble flows [17].

$$ \sum_k^{l,v} \Gamma_k H_k^l + Q_k^l = 0, \quad (11) $$

In this work, an original energy source term based on enthalpy is proposed to account for cavitation. Using the energy-jump equation (11) and the mass-jump condition (9) that implies $\Gamma_l = -\Gamma_v$ and finally considering that at the interface $H_k^l = H_k^{sat}$, the equation can be rewritten as:

$$ \sum_k^{l,v} \Gamma_k H_k^l + Q_k^l = 0 \Leftrightarrow \Gamma_l H_l^l + Q_l^l + \Gamma_v H_v^l + Q_v^l = 0, \quad (12) $$

$$ \text{Therefore:} \qquad \Leftrightarrow \Gamma_l = -\Gamma_v = \frac{Q_l^l + Q_v^l}{H_v^{sat} - H_l^{sat}}, \quad (13) $$

where $H_v^{sat} - H_l^{sat}$ is the definition of the latent heat $L$.

This model expresses the energy transfer between the liquid water and vapor based on three heat transfer scenarios:

- If ($H_l < H_l^{sat}$), liquid is stable and no transfer is needed:
  $$ Q_l^l = 0 \quad (14) $$

- If ($H_l > H_l^{sat}$), liquid vaporizes:
  $$ Q_l^l = f(\alpha_l, \alpha_v) \frac{H_l^{sat}(P) - H_l(P, T_l)}{\tau_l} \quad (15) $$

- If ($H_v < H_l^{sat}$), vapor condenses:
  $$ Q_v^l = f(\alpha_l, \alpha_v) \frac{H_v^{sat}(P) - H_v(P, T_v)}{\tau_v} \quad (16) $$
- then, if ($H_v > H_l^{sat}$), vapor is stable but it is forced to return to the saturation. It is considered that vapor pressure is always close to its saturation value, because it is the dispersed phase:

$$Q_v^I = f(\alpha_l, \alpha_v) \frac{H_v^{sat}(P) - H_v(P, T_v)}{\tau_v} \quad (17)$$

with $f(\alpha_l, \alpha_v) = \max(\alpha_l, 10^{-5}) * \max(\alpha_v, 10^{-5})$ a numerical weighting parameter ensuring transition between phases. The relaxation time parameter $\tau_k$ [s], which could be different for each phase, is fixed at $10^{-4}$s for both phases in this study. Numerical tests are in progress to evaluate the influence of the values of $f(\alpha_l, \alpha_v)$ and of $\tau_k$.

The turbulence model is a k-ε linear production [20] that is only solved for the liquid phase since vapor is considered as dispersed inclusions at the simulation scale. The subscripts “l” are omitted for variables $\rho$, $\mu$, $\bar{U}$, $k$ and $\epsilon$.

$$\left\{ \begin{array}{l} \rho \frac{\partial k}{\partial t} + \text{div} \left[ \rho \bar{U} k - \left( \mu + \frac{\mu_t}{\sigma_k} \right) \nabla k \right] = P + G - k \text{div}(\rho \bar{U}) \\ \\ \rho \frac{\partial \epsilon}{\partial t} + \text{div} \left[ \rho \bar{U} \epsilon - \left( \mu + \frac{\mu_t}{\sigma_\epsilon} \right) \nabla \epsilon \right] = C_{\epsilon 1} \frac{\epsilon}{k} [P + (1 - C_{\epsilon 1})G] - \rho C_{\epsilon 2} \frac{\epsilon^2}{k} + \epsilon \text{div}(\rho \bar{U}) \end{array} \right. , \quad (18)$$

$$\text{with:} \quad \left\{ \begin{array}{ll} P & \text{the viscous production term} \\ G & \text{gravitational term} \\ \mu_t = \rho C_\mu \frac{k^2}{\epsilon} & \text{the turbulent viscosity} \end{array} \right. $$

<table><caption>**Table 3.** Coefficients values of the $k-\epsilon$ linear production model.</caption><thead><tr><th>C<sub>μ</sub></th><th>C<sub>ε1</sub></th><th>C<sub>ε1</sub></th><th>σ<sub>k</sub></th><th>σ<sub>ε</sub></th></tr></thead><tbody><tr><td>0.09</td><td>1.44</td><td>1.92</td><td>1</td><td>1.3</td></tr></tbody></table>

For all the simulations, the Courant-Friedrichs-Lewy (CFL) is kept under 1 except in few cells with *neptune_cfd* for cases at 25 and 30 m/s (*CFLmax* is then around 1.5 ~2.5). The associated time step varies between 6 µs and 1 µs for the different flow conditions.

## 4. Comparisons between numerical approaches and experimental data

### 4.1 Qualitative comparisons

The cavitating flow is found to be periodic for both approaches, as for the experiment. Some 3D simulations visualizations with *neptune_cfd* are presented in figure 3 (b). The vapor cavity breaks at 40% of the chord length and releases structures that are convected downstream along the hydrofoil chord. This is in qualitative accordance with pictures of the experiment (a). In the previous study with *Code_Saturne* (see figures 4 and 9), the shedded structures are less frequent and condense rapidly.
<figure><img src="image_7.png" /><figcaption>**Figure 3.** Qualitative comparison between experiment [3] (a) and two-fluid simulation with *neptune_cfd* (b) by displaying the 10% void fraction isosurface at $V_{in} = 15$ m/s and $\sigma = 1.59$ for a cavity of 40% chord length.</figcaption></figure>

<figure><img src="image_8.png" /><figcaption>**Figure 4.** Example of homogeneous simulation with *Code_Saturne* by displaying the 10% void fraction isosurface at $V_{in} = 15$ m/s and $\sigma=1.35$ for a cavity of 40% chord length [2].</figcaption></figure>

The periodical dynamics of unsteady cloud cavitation is described in figure 5a where side views of the two-fluid simulation are presented for four consecutive instants. Firstly, the cavity grows and reaches a maximum length. A re-entrant jet then develops: this counter flow detaches the cavity. The detached structures are convected downstream and condense. Cavitation structure unsteadiness is analyzed by using a “space-time diagram” (figure 5b). This diagram shows, for each cell-element of the chord, the time evolution of the maximum void-fraction value perpendicular to the hydrofoil surface. It is a very useful graphical representation of the unsteady behavior of cavitation structures. This behavior is linked to the plot of total vapor volume (figure 5c): the evolution of the cavity length corresponds to the evolution of the total volume of vapor.
<figure><img src="image_9.png" /><figcaption>**Figure 5.** Slice-snapshots of the simulations taken at mid span (a) associated with corresponding instant on the space-time diagram (b) and total vapor volume time distribution (c).</figcaption></figure>

## 4.2 Cavity length determination

Cavitation experimental data are recorded for a given mean cavity length, corresponding to ~40% of the chord in the present paper. With numerical simulations, it requires to define a post processing procedure. Most often, visualization of the cavity contour is done by displaying the 10% void fraction isosurface, but it does not define unambiguously the cavity length, because the contour is time varying.

A first method to define the cavity length can be the use of the space-time diagram. The minimum and maximum cavity length are identified and the mean cavity is supposed to be the middle of the delimited framing.

A second methodology is proposed in this paper to estimate the mean cavity length with more precision. The mean temporal pressure field is considered on the foil surface. Then the gradient of this average is calculated (figure 6). This highlight the closure region of the cavity where the pressure variation is important and concentrated on a small space. The cavity length is chosen to be the distance from the leading edge to the middle of this zone where the gradient reaches a maximum. This methodology is in accordance with both visualization of 10% isovalues of mean void fraction and length obtained with the space-time diagram.
<figure><img src="image_10.png" /><figcaption>**Figure 6.** Illustration of the post processing to estimate cavity length. Color field is the gradient of average pressure and white lines are isovalues of mean void fraction [0, 0.1, 0.25, 0.5, 0.75]. *neptune_cfd* simulation at V<sub>in</sub> = 15 m/s and σ= 1.59.</figcaption></figure>

<figure><img src="image_11.png" /><figcaption>**Figure 7.** (a) Time evolution of the inlet and outlet pressures, (b) corresponding Fast Fourier Transforms (FFT), (c) time evolution of the total vapor volume and (d) corresponding FFT. 3D simulation at V<sub>in</sub> = 15 m/s and σ= 1.59 with *neptune_cfd*.</figcaption></figure>
### 4.3 Shedding frequency evaluations

To evaluate the frequency of the vapor shedding, the Fast Fourier Transforms (FFT) of the time evolutions of the inlet pressure and the total vapor volume have been carried out (figure 7). The sampling rates are the simulation time step and respect the Nyquist-Shannon sampling criteria. Both signals allow to recover the same frequency, equal to 109 Hz for $V_{in} = 15$ m/s and $\sigma= 1.59$.

### 4.4 Simulations results and comparisons

The experimental and simulation results for the considered cavitating flows conditions are presented in table 4 and plotted in figure 8. The two codes correctly capture the periodicity of unsteady cavitation with 3D simulations and results are in good agreement with experimental data. The results differ with the 2D simulations. With *neptune_cfd*, the simulated frequencies are kept in good agreement with experiment. With *Code_Saturne*, the simulated frequencies do not agree well with experimental data. For both 2D and 3D, *neptune_cfd* predicts sigma value that are close to experimental data (and even match it with 1.59 at 15m/s) where *Code_Saturne* gives sigma values that do not exceed 1.43 in the best case. This accordance decreases with the velocity increase for *neptune_cfd*, while still being in an acceptable range with the experiment.

<figure><img src="image_12.png" /><figcaption>**Figure 8.** Simulation results for the two codes against experimental data.</figcaption></figure>

<table><caption>**Table 4.** Simulation results for two codes (CS: *Code_Saturne* and NC: *neptune_cfd*) for 2D and 3D simulations, compared to experimental data. Simulations correspond to a cavity length of ~ 40% of the hydrofoil chord.</caption><thead><tr><th rowspan="2">Vin [m/s]</th><th colspan="6">Frequency [Hz]</th><th colspan="6">σ [-]</th></tr><tr><th colspan="3">3D</th><th colspan="3">2D</th><th colspan="3">3D</th><th colspan="3">2D</th></tr></thead><tbody><tr><td>15</td><td><strong>100</strong></td><td>114</td><td>109</td><td>78</td><td>112</td><td><strong>1.59</strong></td><td>1.43</td><td>1.59</td><td>1.35</td><td>1.59</td></tr><tr><td>20</td><td><strong>140</strong></td><td>158</td><td>138</td><td>103</td><td>150</td><td><strong>1.60</strong></td><td>1.40</td><td>1.56</td><td>1.35</td><td>1.54</td></tr><tr><td>25</td><td><strong>190</strong></td><td>182</td><td>173</td><td>132</td><td>188</td><td><strong>1.62</strong></td><td>1.44</td><td>1.54</td><td>1.35</td><td>1.53</td></tr><tr><td>30</td><td><strong>220</strong></td><td>221</td><td>227</td><td>148</td><td>228</td><td><strong>1.63</strong></td><td>1.43</td><td>1.51</td><td>1.35</td><td>1.57</td></tr></tbody></table>

### 4.5 Other differences between the two models

The cavity length and frequency are the main quantities to compare numerical simulations with experimental results. But a more rich and convenient way to sum up all this information is to use the space-time diagram presented before. Figure 9 shows space-time diagrams from the homogeneous simulation (a) and from the two-fluid simulation (b). Both codes are able to catch the periodic behavior of cloud cavitation, but the shape of the cavity differs. The cavity is clearly
identifiable and has a strong periodic pattern with *neptune_cfd* whereas the shape with *Code_Saturne* is less determined and vary between cycles. In fact, the repartition of maximum void fraction in the cavity is very different. It is close to 1 in the cavity for *neptune_cfd*, whereas the value varies between 0.5 and 1 for *Code_Saturne*, except locally at the leading edge and at the cavity closure where a void fraction near 1 is always present. The void fraction value has not been determined experimentally for this geometry. However, space-time diagrams obtained with grey levels of experimental movies from other geometries [21] indicate a vapor structure periodic behavior similar to one obtained from numerical simulations. As seen in section 4.1, with *Code_Saturne*, detached structures rapidly condense. This impacts the evaluation of the mean cavity length.

<figure><img src="image_13.png" /><figcaption>**Figure 9.** Space-time diagram at $l/c=40\%$ and $V_{in}=15$ m/s for 3D simulations of a) homogeneous approach with *Code_Saturne* [2] and $\sigma= 1.35$ and b) two-fluid model with *neptune_cfd* with $\sigma= 1.59$. White line indicates the 40% chord cavity length.</figcaption></figure>

**5. Conclusions**

In this work a closure model for the two-fluid code *neptune_cfd* is described and compared with the homogeneous model of *Code_Saturne*. Both codes give satisfactory results with 3D simulations: the periodic behavior of the vapor structures on the hydrofoil is adequately predicted. The two-fluid code gives better results in 2D than the homogeneous one. With 3D simulations it also allows a better description of unsteady cavitation flows by capturing convected structures in accordance with experimental visualization. There is also a quantitative improvement since cavitation parameter $\sigma$ is closest to its experimental value with the two-fluid approach. A sensibility study is ongoing for the parameters that could affect the model.

The next part of the work is to implement the cavitation intensity model used in [2,13] and to improve the comparison between these two modeling approaches in cavitation erosion prediction.

Results are encouraging but need to be extended with different geometries and flow conditions to ensure robustness of the model. Then the model will be applied to a centrifugal pump.

The use of a two-fluid model with energy equation resolution could also allow to treat cavitation of thermosensitive fluids. The influence of the nature of fluids on cavitation behavior will be studied in a future work.
References:

[1] Mimouni S, Boucker M, Lavieville J, Guelfi A and Bestion D 2008 Modelling and computation of cavitation and boiling bubbly flows with the NEPTUNE CFD code, *Nuclear Engineering and Design*, 238 vol 3 p 680

[2] Leclercq C, Archer A, Fortes Patella R and Cerru F 2017 Numerical cavitation intensity on a hydrofoil for 3d homogeneous unsteady viscous flows, *Int. J. Fluid Mach. Syst.* 10 vol 3 p 254

[3] Pereira F, Avellan F and Dupont JM 1998 Prediction of cavitation erosion: an energy approach, *Journal of Fluid Engineering, Transactions of the ASME* vol 120

[4] Kunz R, Boger D, Chyczewski T, Stinebring D, Gibeling H and Govindan T 1999 Multi-phase CFD analysis of natural and ventilated cavitation about submerged bodies, *Proc. FEDSM 99*

[5] Singhal A, Athavale M, Li H and Jiang Y 2002 Mathematical basis and validation of the full cavitation model, *Journal of Fluids Engineering, Transactions of the ASME*, 124 vol 3 p 617

[6] Coutier-Delgosha O, Reboud JL and Delannoy Y 2003 Numerical simulation of the unsteady behaviour of cavitating flows, *Int. J. Numerical Methods Fluids* 42 vol 5 p 527

[7] Shams E, Finn J and Apte S 2011 A numerical scheme for euler-lagrange simulation of bubbly flows in complex systems, *Int. J. for Numerical Methods in Fluids* 67, 12 p 1865

[8] Maeda K and Colonius T 2018 Eulerian-lagrangian method for simulation of cloud cavitation, *Journal of Computational Physics* 371 p 994

[9] Giannadakis E, Gavaises M and Arcoumanis C 2008 Modelling of cavitation in diesel injector nozzles, *Journal of Fluid Mechanics* 616 p 153

[10] Ma J, Hsiao CT and Chahine G 2015 Modelling cavitating flows using an eulerian-lagrangian approach and a nucleation model, *J. of Physics: Conference Series* 656, 12 p 012160

[11] Ghahramani E, Arabnejad M H and Bensow R E 2018 Realizability improvements to a hybrid mixture-bubble model for simulation of cavitating flows, *Computational Fluids* 174 p 135

[12] Saurel R and Lemetayer O 2001 A multiphase model for compressible flows with interfaces, shocks, detonation waves and cavitation, *Journal of Fluid Mech.* 431 p 239

[13] Fortes Patella R, Archer A and Flageuil C 2012 Numerical and experimental investigations on cavitation erosion, *IOP Conf. Ser.: Earth Environ. Sci.* 15 p 022013

[14] Krumenacker L, Fortes Patella R and Archer A 2014 Numerical estimation of cavitation intensity, *IOP Conference Series: Earth and Environmental Science* 22 p 052014

[15] Leclercq C, Archer A, Fortes Patella R and Cerru F 2017 First attempt on numerical prediction of cavitation damage on a centrifugal pump, *Proc. of the ASME Fluids Eng. Division Summer Meeting FEDSM2017 Waikoloa, Hawaii, USA*

[16] Leclercq C, Fortes Patella R and Archer A 2021 Cavitation erosion mechanism: numerical study of the interaction between pressure waves and vapor bubbles, *IOP Conf. Ser.: Earth Environ. Sci.* p 774 012024

[17] Ferhat J, Archer A, Fortes Patella R and Mimouni S 2022 Numerical simulation of unsteady cavitation on a hydrofoil using a two-fluid model with neptune_cfd, 19th Int. Topical Meeting on Nuclear Reactor Thermal Hydraulics Log nr. 35939

[18] Merkle C L, Li D and Venkateswaran S 1992 A preconditioned Navier-Stokes method for two-phase flow with application to cavitation prediction, *Journal of Fluids Mech.* 29

[19] Coutier-Delgosha O, Fortes Patella R and Reboud JL 2003 Evaluation of the turbulence model influence on the numerical simulations of unsteady cavitation, *Journal of Fluids Engineering, Transactions of the ASME* 125.1 p 38

[20] Guelfi A, Bestion D, Boucker M, Boudier P, Fillion P, Grandotto M, Hérard JM, Hervieu E and Péturaud P 2007 NEPTUNE: a new software platform for advanced nuclear thermal hydraulics, *Nuclear Science and Engineering* 156 p 281

[21] Carrat JB, Fortes Patella R and Franc JP 2017 Assessement of cavitating flow aggressiveness on a hydrofoil: experimental and numerical approaches, *Proc. of the ASME Fluids Eng. Division Summer Meeting FEDSM2017 Waikoloa, Hawaii, USA*