Numerical modeling of cavitating flows for simple geometries using FLUENT V 6 . 1

Cavitation is a phenomenon that can be present in several agro-forestry applications such as irrigation pressure-reducing valves, sprinkler orifices or even in the flow through xylem vessels inside plants. In the present research, numerical predictions of cavitation in a series of orifices, nozzles and venturis were compared to experimental measurements to show the possibilities and performances of the new cavitation model in the commercial Computational Fluid Dynamics (CFD) code FLUENT V6.1. A flashing study is also presented for the nozzle case. Model predictions for the orifice cases accurately capture cavitation inception and its influence on the orifice discharge coefficient. However, when an unsteady flow is modeled, the cavitation phenomenon is not simulated properly and leads to a steady situation. In general, the new cavitation model in FLUENT V6.1 provides very reliable simulation for easy geometries when steady flow is assumed. Additional key words: computational fluid dynamic technique, flow simulation, steady flow, unsteady flow.


Introduction
According to Knapp et al. (1970), cavitation can be classified into several different regimes: traveling, fixed and vortex cavitation.In each, the onset of cavitation occurs due to flow acceleration and consequently an accompanying drop in pressure at a point within the liquid flow that causes vapor bubble formation.Bubbles travel downstream until the increase of pressure causes the bubbles to implode.This two-step process is known as cavitation.Cavitating flows often lead to performance degradation and structural damage to many hydraulic devices.These effects are related to the size, the timeaveraged shapes of the vaporized structures and their area of influence.
Pumps, valves, propellers, nozzles and numerous other devices can be affected by cavitation.For several
The use of CFD (Computational Fluid Dynamics) in designing engineering devices has increased over the past few years due to the availability of commercial codes featuring state-of-the-art robust models and the ability to run the code on desktop PC's.Agro-forestry engineering applications of CFD have also increased in recent years.Palau-Salvador et al. (2004) and Wei et al. (2006) are excellent examples of this, as both used the commercial code FLUENT V6.1 (FLUENT, 2001) to predict the hydrodynamic behavior inside the labyrinth of an in-line emitter.Other applications in agricultural applications range from food industry processes (Norton and Sun, 2006;Smale et al., 2006) to farm and greenhouse ventilation (Norton et al., 2007).
Evaluating cavitation requires a multiphase flow model.This model may be based on either a separate treatment of the continuum and particulate phase using an Eulerian/Lagrangian approach (Farrel, 2003;Cerutti et al., 2000) or as a homogeneous fluid using an Eulerian/Eulerian approach (Kubota et al., 1992;Singhal et al., 2002;Xing and Frankel, 2002).Many studies have contributed to improving CFD cavitation models to obtain a more realistic approach to simulating vapor formation, which allows cavitation characteristics to be predicted in the areas most affected inside the hydraulic devices.
A flashing flow is a non-recoverable cavitating flow.This phenomenon is very important in flows with strong thermodynamic effects, such as light water nuclear reactors during accidental loss of cooling (Xu et al., 1997).There have been several experimental studies of flashing flows (Abuaf et al., 1981) and prediction modeling studies (Elias and Chambre, 2000;Muñoz-Cobo et al., 2000).Nevertheless, all the studied models presented considerable differences between their predictions and experimental results, such as the study carried out with the commercial code FLUENT V5.0 by Xing (2002), which concluded that the cavitation model in this code underestimated the upstream pressure in a flashing flow.
Cavitation in agricultural applications plays an important role in the efficient performance of valves (Palau-Salvador et al., 2005), venturis (Manzano and Palau-Salvador, 2005), flowmeters (Palau et al., 2004), sprinklers (Pascal et al., 2006) located in pressure irrigation systems and even in xylem vessels of plants when sap travels long distances from root to leaves (Cochard et al., 2007or Maheraly et al., 2006).
The objective of this work is to study the characteristics and performance of the new cavitation model of the commercial code FLUENT V6.1 for predicting cavitation in orifices, nozzles and venturis, in both steady and unsteady situations, highlighting their applications in rural environments.The ability of this new model to predict flashing flow is also investigated.

General lines
The cavitation model of FLUENT V6.1 is based on the full cavitation model developed by Singhal et al. (2002).This model involves two phases and a certain fraction of non-condensable gases, whose mass fraction must be known in advance.This model takes into account the formation and collapse of the bubbles.This new code improves the old cavitation model in Fluent, where, for instance, bubbles were neither created nor destroyed.A comparison between the main characteristics of the cavitation model in FLUENT V5.0 and the new cavitation model of FLUENT V6.1 is presented in Table 1.

Numerical method
The model equations are solved using the solver in FLUENT V6.1.In all cases, a structured grid generated using GAMBIT 2.0 is used to mesh the domain.The momentum equations are discretized using both first and second order upwind scheme options.The turbulence models used were the standard k-ε, RNG k-ε or SST k-ω according to each particular case [See Launder and Spalding (1972) or Veersteg and Malalasekera (1995) for more information on this topic].
The governing equations were the mass conservation and the momentum balance equations.These were solved using the SIMPLE algorithm developed by Patankar (1980).On the one hand, the mass conservation equation is expressed for an incompressible and Newtonian fluid as: where v is the mean velocity and ∇ is the vector operator On the other hand, the momentum balance equation is formulated as: where ρ is the fluid density, is the local acceleration that is equal to zero for steady flow, g is the gravity acceleration, z is the height, P is the static pressure and ∇τ* stands for the divergence of the stress tensor.In this term, the number of unknowns turns out to be 13 (velocity components, pressure and stress field), which makes the above equation very difficult to solve.However, calculations are simplified by using the Navier-Stokes equations, which relate the stress field to fluid viscosity.In all the cases modelled a second order upwind scheme was used to discretize the equations involved.Normalized residuals set at six orders of magnitude were used for the convergence criteria.In each case, the boundary conditions and specific conditions of the runs were specified.
When the cavitation model is activated, the working fluid is assumed to be a mixture of three species (liquid, vapor and non-condensable gas).The vapour fraction, f, affects the fluid density and its governing equation is: where ρ m is the mixture density, f the mass fraction, ρv v the velocity vector of the vapor phase and γ the effective exchange coefficient.The source terms R e and R c represent vapor generation and collapse rates, which can be expressed as a function of the main flow parameters.In fact, the expressions used in this cavitation model are functions of static pressure and are given by the two equations (Singhal et al., 2002): where C e and C c are empirical constants, v ch a characteristic velocity, σ the surface tension of the liquid; ρ l and ρ v the liquid and vapor density; P the pressure and P sat the liquid saturation vapor pressure at the working temperature.The Eq. [4] is used when ρ is smaller than P sat and the Eq.[5] when ρ is greater than P sat .
The new cavitation model provides a wider range of options than the old model.The turbulence model can be selected from all the Reynolds Average Navier Stokes possibilities.In the present study, different situations have been validated, choosing the option that leads to the best agreements with the experimental data extracted from the literature.-The system under research involves only two phases.
-Bubbles are neither created nor destroyed.
-The population or number of bubbles per volume unit must be known in advance.
-The system under research involves only two phases (liquid-vapour) and a certain fraction of separately modelled non-condensable gases.-Both bubble formation (evaporation) and collapse (condensation) are considered in the model.-The mass fraction of non-condensable gases must be known in advance.
However, the model still has several limitations.First, its study is based on the Eulerian/Eulerian approach, so bubbles cannot be modelled as separate particles.Also, this model cannot be used together with the Large Eddy Simulation (LES) models.This limitation reflects the basic nature of the research efforts related to applying LES to simple cavitating flows such as jets (Cerutti et al., 2000).
It is especially interesting that the FLUENT V6.1 cavitation model allows the use of a slip velocity between bubbles and liquid.However, this slip velocity was not considered in any of the models used in this study.

Cases studied
Several easy geometries were selected to test and validate the new cavitation model in FLUENT V6.1.These geometries included a circular orifice, a rectangular orifice, a nozzle and a rectangular venturi.In the nozzle, a study of the flashing phenomena was also addressed and an unsteady situation was studied in the rectangular venturi.Only CFD simulations were carried out.The experimental data, geometries and results were obtained from different papers in the bibliography: Nurick (1976) for the circular and rectangular orifices; Abuaf et al. (1981) for the nozzle; and Stutz and Reboud (2000) for the rectangular venturi.Schemes of all the modeled geometries are given in Figure 1.In Table 2 the possible agricultural application of the analyzed geometries are highlighted.More information about each particular case is provided in the following sections.

Case A: Circular orifice
The effect of cavitation in circular orifices was experimentally investigated by Nurick (1976).Cavitation occurs when the flow passes through a very small orifice, which produces a high differential pressure.This effect can be observed in hydraulic valves (Palau-Salvador et al., 2005) or in flow-meters (Palau et al., 2004).In Nurick's paper, a large number of experiments were carried out on different geometries, and the experimental results were compared to those obtained by modeling the same geometries.In the present paper, only the geometry shown in Figure 1 is presented, but good agreement was also obtained for the other geometries studied by Nurick (1976).
The turbulence models used were the standard k-ε and RNG k-ε.Both presented good results and no differences were detected between them in the prediction of cavitation in the circular orifice.The characteristic geometric parameters of the circular orifice studied were D/d = 2.88 and L/d = 20.Uniform inlet and outlet static pressure were adopted as boundary conditions.The exit pressure was fixed at 9,500 Pa and the upstream pressure varied, as in Nurick's experiments, between 3 × 10 8 and 2 × 10 5 Pa.The parameters used to validate the model were the cavitation number (Σ) and the discharge coefficient (C d ): Cavitation number: [6] Discharge coefficient: [7] where P o , P sat and P b are the upstream, vapor and exit pressure, respectively; v b the velocity at the inlet; ρ the liquid density and m • the mass flow.An axysymmetric 2D domain with a structured grid of 42,860 nodes was f inally used after testing mesh sensitivity by using finer meshes and verifying that there was no influence on the predicted mass flow.
The effect of a temperature increase in the model is shown in Figure 2.Although the temperature effect is small, the predicted C d is consistently lower than the values found by Nurick (1976) when the cavitation number is greater than 1.6.In order to determine the reason for this difference, the same geometry was modeled with a different inlet pipe length (Fig. 3).C d prediction was better when the length (L i ) was around 15 outlet diameters (15 d) with an error of < 5%, even when the cavitation number was > 1.6.

Case B: Rectangular orifice
As in the case of the circular orifice, Nurick's (1976) experimental data were used.The parameters used to validate the model were the same as in the case of the circular orifice: discharge coefficient (C d ) and cavitation number (Σ).The geometry of the rectangular orifice modeled is shown in Figure 1, and is relevant due to its relation with jet cavitation, as happens in control valves (Palau-Salvador et al., 2005) or sprinkler guns (Pascal et al., 2006).
The turbulence model used for this case was the SST k-ω model, since the predicted C d for the rectangular orifice with the standard k-ε and RNG k-ε did not agree with the experimental results obtained by Nurick (1976), as shown in Figure 4.All solid boundaries were represented using no slip velocity conditions.With regard to the inlet and outlet boundaries, uniform static pressures were adopted.The downstream pressure was fixed at 9,500 Pa and the upstream pressure varied between 2 × 10 8 and 2 × 10 5 Pa, as in Nurick's assays.A 3D model was created with a symmetry boundary in the middle of the orifice.A structured mesh was considered.Several mesh sizes were used to check the grid sensitivity.The final mesh used featured 281,730 nodes, after checking that the prediction worsened with the coarsest grid and did not improve with the finest (Fig. 5).Mesh size effect on the vapor fraction prediction is shown in the symmetry plane in Figure 6.As can be seen, the coarse grid (33,948 cells) did not properly simulate the cavitation generated in the orifice outlet, so a finer mesh was needed in accordance with C d prediction results (Fig. 5).
Cavitation predictions for the rectangular orifice were not as good as for the circular one.However, with a considerably ref iner mesh (281,730 nodes), the model was in reasonable agreement with the experimental data obtained by Nurick (1976).The final error was < 10% when the cavitation number was < 1.3 and even lower with higher cavitation numbers.

Case C: Nozzle (Flashing flow)
Flashing flow is very difficult to predict, as the void fraction does not recover downstream of the nozzle.A previous study on flashing flow modeling was carried out by Xing (2002) using the FLUENT V5.With this version, there was an underestimation of the upstream pressure and the downstream vapor fraction.With the new cavitation model used by FLUENT V6.1, better results were obtained when modeling this kind of flow.
A model was built to study flashing flow in a nozzle with the geometry shown in Figure 1, which corresponds to the experimental tests carried out by Abuaf et al. (1981), who measured many runs with this geometry.A computational three-dimensional grid was built for the studied geometry, using a structured mesh of 100,000 cells.Mesh sensitivity was tested using a smaller cell size, but no influence on the final results was found.Solid boundaries were represented using no slip velocity conditions.A symmetry boundary was defined in the mirror plane of the nozzle.Inlet and outlet boundary conditions were set to the values of inlet and outlet static pressures of the runs corresponding to Abuaf et al. (1981).The turbulence model used was the SST k-ω model, since it provided the best convergence.
The mass flow rate was used to validate the model.The main study was done with the data of run 309 from Abuaf et al. (1981), although other runs were also validated, as shown in Table 3, with a difference of the predicted mass flow rate of less than 4%.In run 309, the upstream pressure was fixed at 5.55 × 10 6 Pa and the downstream pressure at 3.78 × 10 6 Pa.The temperature was 420 K and the mass flow 8.80 kg s -1 .
The evolution of the pressure (Fig. 7) and the vapor fraction (Fig. 8) in the axis of the nozzle at different temperatures were compared to the pressure and the vapor fraction, respectively, in the experimental essay of Abuaf et al. (1981) at a temperature of 420 K.However, this model presents problems of convergence when the temperature approaches the flashing situation.Nevertheless, the prediction of axial pressure and vapor fraction achieved with the best convergence criteria model is in good agreement with the experimental data obtained by Abuaf et al. (1981).
The vapor fraction in the symmetry plane of the nozzle at three different temperatures is shown in Figure 9.In the first and the second cases, with temperatures of 373    and 400 K, flashing flow did not develop, although, as expected, cavitation increased with temperature.However, in the third case with a temperature of 420 K, similar to the experimental measured value, flashing flow occurred and the liquid state did not recover.Similar agreement with other runs was obtained at their experimental temperature (Table 3).From all these results, it can be concluded that the new cavitation model of FLUENT V6.1 accurately simulated the flashing flow phenomenon in a nozzle.

Rectangular venturi
This case considered unsteady flow in a rectangular venturi.Experimental data were taken from Stutz and Reboud (2000).A previous numerical study with another commercial code was carried out by Coutier-Delgosha et al. (2003).In this study the RNG k-ε and the standard k-ω models were used, which led both to steady situations.However, a modif ication in the estimation of viscosity for both models improved the simulation of the unsteady cavitation flow.
The geometry of the Venturi used is shown in Figure 1 and was similar to that used in the experimental tests carried out by Stutz and Reboud (2000).This flow is similar to that found in sprinklers (Pascal et al., 2006) or in fertirrigation devices (Manzano and Palau-Salvador, 2005).The turbulence model used was the RNG k-ε model, due to its better convergence compared to other turbulence models assayed.The downstream pressure was f ixed at 64,000 Pa and the upstream pressure varied between 2 × 10 5 and 1 × 10 5 Pa.The grid was a structured mesh.Several mesh sizes were used for checking grid sensitivity and f inally a mesh of 112,000 nodes was selected.Time step was equal to 0.001 s, in accordance with the values obtained in the experimental data.
Figure 10 shows the time variation of the cavitation length after the throat of the Venturi.The cavitation length led to a constant value instead of varying, as had been observed in the experimental tests (Stutz and Reboud, 2000).There were two cycles in which the cavitation length varied, but after the third cycle it reached a steady situation.These results obtained with the new  cavitation model of FLUENT V6.1 did not improve the results presented by Coutier-Delgosha et al. (2003) using the RNG k-ε and the standard k-ω models.This showed that this model did not properly simulate cavitation flow when an unsteady situation was assumed.

Conclusions
Validation studies of the new cavitation model of FLUENT V6.1 have been presented in this paper.The geometries for this validation included a circular orifice, a rectangular orifice and a nozzle, with the assumption of steady flow.A prediction of flashing flow was made in the nozzle geometry.In all cases, good agreement between predictions and experimental data was obtained.
A venturi in an unsteady situation was also studied.In this case, the results obtained from the numerical model did not agree with experimental data and led to a steady situation.
In general, it can be said that the new cavitation model in FLUENT V6.1 provides very reliable simulation of easy geometries when steady flow is assumed.

Figure 1 .
Figure 1.Summary of the geometries used for validating the new cavitation model of FLUENT V6.1.

Figure 3 .
Figure 3.Effect of inlet pipe length on the C d prediction of the circular orifice.Inlet lengths tested were 3.28, 14.4 and 16.5 times the outlet diameter (d).

Figure 4 .Figure 2 .
Figure 4. Prediction of C d using the k-ε model compared with the experimental data obtained by Nurick (1976).

Figure 6 .
Figure 6.Vapor fraction in the rectangular orifice obtained with different mesh sizes.
Different runs from Abuaf et al. (1981), with the experimental and numerical mass flow values

Figure 5 .
Figure 5.Effect of different mesh sizes on the C d predictions in the rectangular orifice using SST k-ω model compared to the experimental data of Nurick (1976).

Figure 8 .
Figure 8. Evolution of the vapor fraction in the axis of the nozzle at different temperatures compared to that of the experimental assay of Abuaf et al. (1981) at 420 K.

Figure 9 .Figure 7 .
Figure 9. Vapor fraction at different temperatures in the symmetry plane of the nozzle.

Figure 10 .
Figure 10.Time variation of the cavitation length after the throat of the rectangular venturi.

Table 1 .
Differences between old and new cavitation models in Fluent

Table 2 .
Different examples of cavitation found in rural and irrigation applications