N UMERICAL S TUDY O F C AVITATING F LOW I NSIDE A F LUSH V ALVE - - PDF document

Conference on Modelling Fluid Flow (CMFF’09) The 14th International Conference on Fluid Flow Technologies Budapest, Hungary, September 9-12, 2009

NUMERICAL STUDY OF CAVITATING FLOW INSIDE A FLUSH V

ALVE

Annie-Claude BAYEUL-LAINẺ1, Sophie SIMONET2, Guy CAIGNAERT3

1 Arts et Metiers PARISTECH, LML, UMR CNRS 8107, 8, boulevard Louis XIV 59046 LILLE Cedex Tel.: +33 20 62 39 04, Fax: +33

20 53 55 93, E-mail: annie-claude.bayeul@ensam.eu

2 Arts et Metiers PARISTECH, LML, UMR CNRS 8107, E-mail: sophie.simonet@ensam.eu 3 Arts et Metiers PARISTECH, LML, UMR CNRS 8107, E-mail: guy.caignaert@ensam.eu

ABSTRACT

In water supply installations, noise pollution

• ften occurs. As a basic component of a system, a

flush valve may frequently be a source of noise and vibration, of which cavitation can be the problem, especially during valve closing or valve opening. The aim of this paper is to show how a numerical industrial code can point out a cavitation problem even if this code doesn’t use a cavitation

• model. This approach shows a good agreement with
• ne using a cavitation model. The numerically
• btained contours of the volume fraction of water

vapour show cavitation inception distribution behind the poppet of the valve. Computational Fluid Dynamics (CFD) simulations of cavitating flow through water hydraulic industrial flush valve were performed using the Reynolds averaged Navier-Stokes (RANS) equations with a near-wall turbulence

• model. The flow was turbulent, incompressible and
• steady. The flush valve under study is a real one.

The structure of this flush valve was simplified due to symmetry considerations. The model used is three dimensional. Flow field vizualization was numerically achieved. The effects of inlet pressure as well as mesh size and mesh type on cavitation intensity (assessed by pressure intensity) in the flush valve were numerically investigated thanks to two commercial codes : Fluent 6.3 and Star CCM+ 3.04.009. Keywords: Cavitation, Noise, Numerical simulation, Water supply systems

NOMENCLATURE

Nbub [-] number of vapour bubbles in a control volume Ncells [-] number of cells Nit [-] number of iterations Npl [-] number of prism layer Q [kg/s] mass flow rate Qref [kg/s] reference mass flow rate R [m] micro bubble radius Vl [m3] volume of liquid in a control volume Vv [m3] volume of vapour in a control volume e1 [μm] first prism layer thickness et [μm] total prism layer thickness pmin [MPa] minimal absolute static pressure p [MPa] static pressure pi [MPa] static pressure at valve inlet piref [MPa] static reference pressure at valve inlet tref [s] reference time t [s] time vmax [m/s] maximal velocity in narrow zone αl [-] liquid volume fraction αv [-] vapour volume fraction

• 1. INTRODUCTION

The effects of borough’s improvement on working and living environment cannot be ignored. These can include air pollution, noise and vibration, contamination of land and water. One of the most important parameters in building construction is noise control. Cavitation noise generated by components such as valves in water supply systems has frequently raised serious

• problems. In each country, there are legal codes of

practice and today new building sites and major construction projects are well controlled. Taps and valves can, therefore, be classified on the basis of their acoustic behaviour, in accordance with the ISO 3822 or NF EN 12541 standards ([1, 2]). In order to determine the sources of noise and the best design methods to minimize noise generation, experimental and numerical analyses were carried out in our laboratory. The aim of this paper is to present some numerical results. Figures 1 and 2 describe respectively flow rate (fig. 1) and upstream static pressure (fig. 2)

evolutions during one operating cycle, from

• pening to closure, in a non dimensional form. Such

tests results are obtained in an open test rig composed of : (i) a vessel with a control of pressure, (ii) a steel pipe with a laminar flow element flow meter, (iii) a deformable pipe in order to limit pressure surges during the valve closure, (iiii) a pipe with various pressure transducers upstream of the tested valve. The main aim of such a valve is to deliver a fixed volume of liquid (6 or 9 l, for example) with a high enough momentum. It is clear, from these two figures, that the operation of such a valve is unsteady and transitory. Nevertheless, the cycle duration (about 10s) allows to consider the flow inside the valve as a succession of quasi- steady operating conditions. This is the main assumption that has been made in the present study, because CFD codes are not really still able to describe accurately such a transitional behaviour with a control of the opening and closure of the valve by the flow itself. Figure 1. Flow rate in a flush valve during a cycle (non dimensional presentation) Figure 2. Upstream static pressure in a flush valve during a cycle (non dimensional presentation) This work deals with the problem of noise generated by a flush valve in water supply systems with conditions of valve opening or closing especially when cavitation can occur. This is the case when pressure in the liquid drops below the vapour pressure. Vapour bubbles are formed, and rapidly collapse when pressure increases. That collapse of bubbles is clearly associated with noise generation ([3, 4]). GAO H., FU X., YANG H. and TSUKIJI T. ([5]) also showed the importance of predicting cavitation in water hydraulic valve and the necessity

• f continuing investigation.

In this type of valve, when closing or opening, static pressure remains relatively constant before and behind the singularity formed by piston and seat (called narrow zone in the next text : detail (a) in fig. 4) where quite all the part of the head drop

• ccurs.

The cavitation model in commercial CFD codes, designed for two interpenetrating fluids (generally liquid and vapour phases of the same fluid: water in the case of this paper), describes the formation of bubbles when the local pressure becomes lower than the vapour pressure. The cavitation model solves a single set of momentum equations shared by the two fluids, a continuity equation for the liquid (primary phase) and a volume fraction equation for the secondary phase. It is assumed that all vapour bubbles in a control volume have the same radius R and a homogenous

• distribution. This assumption leads to describing the

bubble distribution by a single scalar field, the vapour volume fraction αv.

v l bub v v

V V R N V V

3

3 4 (1) Assuming that only one liquid phase (volume Vl) and the corresponding liquid-vapour phase (volume Vv) can occupy a control volume V where cavitation takes place, the mass of produced vapour depends on the vapour density, the anticipated average size (radius R) and vapour bubbles density. Cavitation model also includes mass transfer between the fluids. Models in commercial codes can predict the inception of cavitation but few can predict the collapse of the bubbles. Cavitation is a complex process influenced by a lot of factors. The formation of bubbles followed by their collapse makes this problem highly unsteady. Consequently we have to choose between steady or unsteady approaches for cavitation. In both cases, simulation takes a lot of time. The steady approach is sufficient to confirm that cavitation occurs. This paper shows how a commercial CFD code can point out a cavitation problem with a classical model without using a cavitation model. Two commercial codes were used: Fluent 6.3 and Star CCM+ 3.04.009. t/tref Q/Qref 1 1 t/tref pi /piref 1 1

In a first step, a comparison between the two models (no cavitation and cavitation with steady approach) thanks of code Fluent for a relatively fine mesh is presented. In a second step, a comparison between the two codes is proposed. In a third step, the influence of the mesh (size and type) is analyzed.

• 2. DESCRIPTION OF THE VALVE

The geometry of the flush valve, used for the present study, is shown in figure 3. The main path

• f water stream is represented by white arrows.

Figure 3. Flush valve geometry (cut ¾ view) Figure 4 presents details on position between piston and valve seat (a) and the narrow zone for the fluid between the piston and the seat. The height

• f this zone is 0.8 mm. Simulations show that

cavitation can occur in this narrow zone. Figure 4. Flush valve geometry (zoom on narrow zone) The associated fluid zone is presented in figure 5. Only the flow in one half of the geometry is calculated due to the symmetry of the valve and to the symmetry of boundary conditions. The choice

• f this hypothesis can be discussed because of

possible cavitation, but the main goal of this work is to show if cavitation occurs and this model is sufficient to do so.

• 3. COMPARISON BETWEEN NO

CAVITATION MODEL AND CAVITATION MODEL

In this paragraph, the flush valve is studied using first a no cavitation model and then a cavitation model. Figure 5. Flush valve geometry: fluid zone The first geometric model, shown in figures 6 and 7 is a tetrahedral mesh with 607 210 cells. The grid of the fluid domain has been created in pre- processor GAMBIT. The mesh size depends on the

• position. In order to well represent the flow field in

the narrow zone, a refined mesh is used there. Small size lies near narrow zone where it is about 0.1 mm and that size increases up to 1mm far away from narrow zone (at the inlet and at the outlet). So there are about 8 cells in the passage height of the narrow zone. Figure 6. Mesh of fluid zone (a) (a) (a)

The boundaries of the valve are relative pressure inlet (0.12 MPa), relative pressure outlet (0 MPa), and wall boundaries. That pressure inlet is the lowest pressure usually used in such valves ([1]). The fluid is water (density=998.2 kg/m3, viscosity=1.003 10-3 Pa.s) for non cavitating model and mixture between water liquid and water vapour (density constant equal to 0.02558 kg/m3, viscosity=1.26 10-6 Pa.s). The density ratio between water and vapour is about 39000. The flow is assumed incompressible (the two phases are treated as incompressible fluids), steady and turbulent. The Reynolds number based on the height of the narrow zone is 19000 for water and 400 for water vapour (for a maximal velocity of 25 m/s). So flows occur at rather low Reynolds number. The standard k-

• mega turbulence model is used in both cases. The

cavitation model used is the Rayleigh one. Figure 7. Mesh detail in narrow zone A steady state solution was calculated in the cavitation model to simulate the formation of vapour in the narrow zone. This steady solution needed about 1500 iterations. It is obvious that a more intensive unsteady calculation should be necessary to simulate the formation and the growth

• f bubbles but it was not the aim of this work.

The question of the possible use of a laminar model arises, due to the low Reynolds numbers. In fact, it must be pointed out that a liquid-vapour mixture occurs in cavitating conditions and laminar conditions are really questionable in such situations. Nevertheless a calculation with laminar assumptions has been carried out in non cavitating

• hypothesis. The results are discussed in paragraph

5, even if convergence problems appeared. Simulation with the model with no cavitation shows that absolute pressure becomes negative in the narrow zone (Fig. 8), which has no physical

• sense. So it can be supposed that cavitation occurs

in this zone. Simulation with a cavitation model effectively shows that there is cavitation in this zone (Figs. 9, 10, table 1). In case of cavitation model, it can be seen in fig. 10 that pressure is generally higher than vapour pressure and that the cavitation area is limited to the narrow zone. Figure 8. Contours of absolute static pressure (Pa) with no cavitation model (FLUENT) It can be seen in fig. 9 that the volume fraction

• f water (αl ) drops to 31 % in this zone.

Figure 9. Contours of volume fraction of water with a cavitation model (FLUENT) Figure 10. Contours of absolute static pressure (Pa) with a cavitation model (FLUENT) Table 1. results with the two models with Fluent no cavitation cavitation Nit 600 1500 Q (kg/s) 0.374 0.366 pmin (MPa)

• 0.16

Table 1 presents the number of iterations, the flow rate and the minimal absolute pressure

• btained with each model. The use of a cavitation

model increases the number of iterations (for a

steady state solution) compared to the use of a no cavitation model. The flow rates for the two models are quite equal (the difference is lower than 2 %).

• 4. COMPARISON BETWEEN TWO

CODES 4-1 Model with no cavitation.

For the same mesh model (tetrahedral mesh with 607 210 cells), with the same boundary conditions, the same turbulence model (k- ), results between Fluent and Star CCM+ codes are compared. Overall results are given in table 2. Minimal absolute pressure and maximal velocity are given for cell centroid base values. Table 2. Results with the two CFD simulation, no cavitation model Fluent Star CCM+ Nit 600 500 Q (kg/s) 0.374 0.540 pmin (MPa)

• 0.16
• 0.343

vmax (m/s) 25 32.15 The two CFD codes give the same type of results: cavitation occurs in the narrow zone. But there is a rather high difference between the flow rate and the minimal absolute pressure (See table 2). These differences can be explained by the fact that Star CCM+ is known to give better results with polyhedral mesh and that there is a low Reynolds

• problem. Perhaps, a low Reynolds mesh should be

used. Figure 11. Contours of absolute static pressure (Pa) with no cavitation model (k- turbulence model) (Star CCM+ x_z plane view) Figures 11 and 12 present contours of absolute pressure (in case of no cavitation model) in two planes for the narrow zone cavitation. It can be seen on fig. 13 contours of static absolute pressure for pressure only lower than vapour pressure. This can be used to locate cavitating zones (area in the circle). Figure 12. Contours of static pressure (Pa) with no cavitation model (k- turbulence model) (Star CCM+ x_y plane view) Figure 13. Contours of static pressure (Pa) with no cavitation model (k- turbulence model): zones where pressure is lower than vapour pressure (Star CCM+ )

4-2 Model with cavitation

Results are compared for the same mesh model (tetrahedral mesh with 607 210 cells), the same boundary conditions, with turbulence model (k- ) for Fluent and turbulence model (k-ε) for Star CCM+. The Turbulence model (k- ) leads to some convergence problem with this mesh for Star CCM+, this is the reason why the turbulence model (k-ε) was used with Star CCM+. RAYLEIGH cavitation model ([6]) is used for Fluent and RAYLEIGH-PLASSET cavitation model ([7]) for Star CCM+ Table 3. Results with the two CFD simulations, with cavitation model Fluent Star CCM+ Turbulence model k- k- Nit 1500 1000 Q (kg/s) 0.366 0.409 pmin (MPa)

• 0.028

vmax (m/s) 25 20.9 αl min 0.31 0.41 Table 3 summarizes results for cavitation simulation with the two codes. The two simulations show cavitation and results are in better agreement than those obtained with the simulation with no cavitation, especially for the flow rate.

Figure 14. Contours of volume fraction of water with cavitation model with Star CCM+ In Star CMM+ code, negative absolute pressure still exists. Figure 14 shows cavitation zone thanks to the volume fraction of water αl.

• 5. INFLUENCE OF TURBULENCE

MODEL

For the same mesh model (tetrahedral mesh with 607 210 cells) and the same boundary conditions, results for Star CCM+ using different turbulence models are given for calculation with no cavitation model. A laminar flow was also

• simulated. This laminar model leads to some

convergence problem, so a turbulence model was used for initial conditions. In each case, cavitation was detected thanks to negative absolute pressure (table 4). Table 4. Results with different turbulence models, no model cavitation (Star CCM+) Turbulence model k- k- laminar Q (kg/s) 0.540 0.541 0.531 pmin (MPa)

• 0.359
• 0.343
• 0.300

vmax (m/s) 32.15 31.62 31.39

• 6. INFLUENCE OF MESH SIZE

Star CCM+ has been used to analyse the results sensitivity to the mesh size. In each case, tetrahedral cells have been used with the same boundary conditions, the same turbulence model ((k-ε) model with realizable (k-ε) two layers), and no cavitation

• model. The difference in mesh size is mainly near

the narrow zone as can be observed in figures 15 to 17. Results, given in table 5, show little influence for cavitation area, minimal absolute pressure and maximal velocity in narrow zone. Table 5. Results with different numbers of cells, no cavitation model and tetrahedral mesh (Star CCM+) case T1 T2 T3 Ncells 166 842 239 771 832 211 Q (kg/s) 0.464 0.474 0.474 pmin (MPa)

• 0.201
• 0.218
• 0.218

vmax (m/s) 26.08 25.59 25.6 Figure 15. Case T1 : 166842 tetrahedral cells Figure 16. Case T2 : 239771 tetrahedral cells Figure 17. Case T3 : 832211 tetrahedral cells

• 7. INFLUENCE OF MESH TYPE

7-1 polyhedral mesh without prism layer

Star CCM+ has been used to analyse the influence of mesh type, using polyhedral cells. In each case, the (k-ε) model with realizable (k-ε) two layers has been used with no cavitation model. Different meshes can be observed in figures 18 to 20.

In Star CCM+, the volume mesh is built thanks to the surface mesh. A similar surface mesh with triangular cells can generate tetrahedral mesh or polyhedral with or without prism layer. The basic tetrahedral model used in this paper (607210 cells,

• fig. 7) and the P0 Case (fig 18), have the same

surface mesh, so their size references are the same. Table 6. Results with different numbers of cells, no cavitation model and polyhedral mesh (Star CCM+) case P0 P1 P2 Ncells 167988 79006 142684 Q (kg/s) 0.538 0.512 0.532 pmin (MPa)

• 0.222
• 0.199
• 0.207

vmax (m/s) 27.5 26.26 27.94 Results given in table 6, show the mesh size has no great influence on different polyhedral

• calculations. Consequently the use of a coarse grid

can allow a gain of calculation time. These polyhedral meshes give results that are well comparable to those obtained with tetrahedral mesh thanks of Fluent (minimal absolute pressure and maximal velocity in narrow zone). The main advantage is, for a similar quality (in size), that polyhedral mesh needs fewer cells (607 210 cells for a tetrahedral mesh and 167 988 for a polyhedral). The Flow rate remains quite higher with Star CCM+ than with Fluent which is not yet explained. Figure 18. Case P0 : 167988 hexahedral cells Figure 19. Case P1 : 79006 hexahedral cells Figure 20. Case P2 : 142684 hexahedral cells

7-2 polyhedral mesh with prism layer (Low Reynolds mesh)

Prismatic near wall layers have been included for the above P0 mesh by using the prism meshing model in the volume meshing process. For a similar surface mesh, Star CCM+ creates a volume mesh including the prism layer model. A prism layer mesh is composed of orthogonal prismatic cells that usually reside next to wall boundaries in the volume mesh. Table 7. Results with different numbers of cells, no cavitation model, polyhedral mesh and prism layer (Star CCM+) case PL1 PL2 PL3 Ncells 308066 308066 399859 et 10 20 20 e1 2.11 4.22 1.51 Q (kg/s) 0.404 0.372 0.386 pmin (MPa)

• 0.079
• 0.021
• 0.025

vmax (m/s) 22.7 20.84 21.2 Npl 3 3 5 y+

max

2.34 4.33 2.13 Table 7 presents the influence of the use of a low Reynolds mesh (prism layer). Polyhedral cells with the same boundary conditions and no cavitation model have been used. Calculations used a (k- turbulence model with a total prism layer thickness equal to 10 μm or 20 μm and a prism layer stretch of 1.5. Polyhedral mesh with prism layer thickness (Fig. 21) shows hardly any cavitation and calculations need to decrease under-relaxation parameters to obtain good convergence. For a total prism layer thickness equal to 10 μm and for a number of prism layers equal to 5, calculations do not converge. This problem seems to be associated to a tiny first prism layer thickness (less than 1 μm). Table 7 shows that for the three cases presented, the maximal value of y+ remains lower than 5 (value given by S.B. Pope ([9]) for a viscous sub layer). This maximal value occurs in the narrow

• zone. PL1 and PL3 cases lead to equivalent values
• f y+, for an equivalent prism layer thickness. The

first prism layer thickness seems to have a great importance in these cases. Furthermore, for the PL3 case, the flow rate is near the one obtained with Fluent, which is well correlated to experimental data. Figure 21. Case PL1 : 308066 hexahedral cells

• 8. INFLUENCE OF PRESSURE INLET

For the first mesh (607210 cells) simulation with relative inlet total pressure equal to 0.25 MPa (conditions of normalized tests [1]) was performed. Simulation leads to a minimal absolute pressure

• f -1 MPa, a flow rate of 0.786 kg/s and a maximal

velocity of 42.59 m/s. It can be seen in figure 21 that the area of cavitation is much greater than those in the case of pressure inlet of 0.12 MPa, which is quite normal and can be associated with the large increase in flow velocities in the narrow zone. Figure 22. pressure contours (Pa) for inlet pressure=0.25 MPa

• 9. CONCLUSIONS

Simulations of a flush valve in case of opening

• r closing conditions have been performed using

classical no cavitation models in Fluent and in Star CCM+ and cavitation models in the same CFD with steady state conditions. Results of the pressure field with classical models (with no cavitation) indicate areas where cavitation occurs: regions where the pressure is negative and also regions where the pressure is close to the vapour pressure value specified in the problem set up. Examination of water vapour fraction with cavitation model in Fluent (and in Star CCM+) confirms that cavitation indeed occurs in these regions. The influences of turbulence model, mesh size, mesh type and the value of total inlet pressure have been studied. Even with coarse mesh, cavitation was observed with classical model (with no cavitation), with no particular parameters unless in case of prism layer. On the contrary, cavitation models need some precautions to give available results (low under relaxation parameters, good meshes…). Best correlations with experimental results were obtained with polyhedral mesh and prism layers (5 prism layers with a first prism layer thickness of 1.5 μm and a prism stretch of 1.5). Using classical model is an economical method for testing trial flush valves and for detecting cavitation, source of noise through a large range of

• perating conditions. It remains an economical tool

for engineers to estimate the design of valve avoiding cavitation.

REFERENCES

[1] NF EN 12541, 2003, Pressure flushing valves and automatic closing urinal valves (PN10), ICS 91.140.70 [2] BS EN ISO 3822-3/A1, 1997, Acoustic laboratory tests on noise emission from appliances and equipment used in water supply installations [3] Lecoffre Yves, 1999, Cavitation Bubbles Trackers, Balkema. 399 pp. ISBN 90 5410 783

• 9. 75 Hfl.

[4] Brennen, CE, 1995, Cavitation and bubbles dynamics, Oxford University Press, 291 pp. ISBN 0-19-509409- [5] Gao, H, Fu, X, Yang, H , Tsukiji, T, 2002, “Numerical investigation of cavitating flow behind a poppet valve in water hydraulic system”, Journal of Zheijang University Science V3,No. 4, pp 395-400. [6] Fluent documentation user’s guide [7] Star CCM+ documentation [8] Romeu, J, Jiménez, S, Capdevilla R., 2004, “Noise emitted by water supply installations”, Applied Acoustics 65, pp 401-419. [9] Pope S. B., 2000, Turbulent Flows, Cambridge University Press, 771 pp ISBN 0-521-59886-9