
[Sponsors] 
Cavitation around NACA hydrofoil using interPhaseChangeFoam 

LinkBack  Thread Tools  Search this Thread  Display Modes 
July 16, 2015, 04:48 

#21 
New Member
jiri kozak
Join Date: Jan 2013
Posts: 21
Rep Power: 10 
Thanks.
Of course, but I want to make single phase simulation of the flow with multiphase condition, to compute the aditional vorticity which is introduced by the cavitation under the same condition. 

September 2, 2015, 10:16 

#22 
New Member
Daniel Rodriguez Calvete
Join Date: Mar 2012
Location: Ferrol (A Coruņa) Spain
Posts: 10
Rep Power: 11 
Dear All,
I am retrieving similar strange behaviour using InterPhaseChangeFoam as it is posted in this treatment. And I would like to know if some one can help me or give some tips to solve it. The case what I am running is a 3D geometry of a Globe Valve in a pressure drive condition. I have run the case with following pressure drops:  No Cavitation Condition (According to experimental results) DP = 0.7, 0.8 and 1.0 bar (Pin = 1.62, 1.74 and 1.98 bar)  Cavitation Condition (According to experimental results) DP = 1.5 and 1.8 bar (Pin = 2.1, 2.5, 3 bar) The cavitation model using here is SchneerSauer, n = 1e+14, dNuc = 1e05, Cc =1; Cv =1 The problem is that in all of the cases there are several cells with negative pressure (fluctuating around 0), what is no physical when absolute pressure at inlet and outlet is used. In any case I get less value than saturation pressure (3500 Pa), even when I did not expect cavitation. Normally, the negative pressure (or pressure below the saturation pressure) is located at the ring intersection between pipe and the globe valve, as is shown in this figure: https://www.dropbox.com/s/gwywsu4pjr...eDp07.png?dl=0 Firstly, I was using the interPhaseChangeFoma of OF2.3.0 which give a high negative pressure, of order of 200000 Pa Then, changing some lines in the code, I am retrieving better results but still negative ( order of 2500 Pa) as you can see in the next figure: https://www.dropbox.com/s/jqdq8j0juk...Pmin.png?dl=0 The changes in code are: 1. phaseChangeTwoPhaseMixture.C in line 105 Code:
Foam::tmp<Foam::volScalarField> Foam::phaseChangeTwoPhaseMixtures::SchnerrSauer::pCoeff ( const volScalarField& p ) const { volScalarField limitedAlpha1(min(max(alpha1_, scalar(0)), scalar(1))); volScalarField rho ( limitedAlpha1*rho1() + (scalar(1)  limitedAlpha1)*rho2() ); return (3*rho1()*rho2())*sqrt(2/(3*rho1())) *rRb(limitedAlpha1)/(rho*sqrt(mag(p  pSat()) + 0.001*mag(pSat()))); //** 0.01*pSat> 0.001*mag(pSta) } 2. alphaEqnSubCycle.H in line 31 Code:
else { #include "alphaEqn.H" } alpha1.max(dimensionedScalar("zero", alpha1.dimensions(), 0.0)); //** alpha1.min(dimensionedScalar("zero", alpha1.dimensions(), 1.0)); //** rho == alpha1*rho1 + alpha2*rho2; } 3. UEqn.H Code:
/* VERSION 2.1.1*/ if (pimple.momentumPredictor()) { solve ( UEqn == fvc::reconstruct ( fvc::interpolate(rho)*(g & mesh.Sf()) + ( fvc::interpolate(interface.sigmaK())*fvc::snGrad(alpha1)  fvc::snGrad(p) ) * mesh.magSf() ) ); // // /* VERSION OF2.3.x if (pimple.momentumPredictor()) { solve ( UEqn == fvc::reconstruct ( ( interface.surfaceTensionForce()  ghf*fvc::snGrad(rho)  fvc::snGrad(p_rgh) ) * mesh.magSf() ) ); } */ } The setup of the case is: BOUNDARY CONDITIONS p_rgh Inlet → TotalPressure Outlet → fixedPressure Wall → fixedFluxPressure U Inlet → pressureInletVelocity Oultet → zeroGradient Wall → fixedFluxPressure Turbulence Model kOmegaSST ControlDict Adaptative time step → Co = 0.9 (PISO mode with nCorr = 4) maximum yPlus < 3 I attach the system file for more information. system.zip I will be very greatful if some can help me in order to obtain more physical results using this solver. Kind Regards, Last edited by DanielRCalvete; September 17, 2015 at 11:59. 

September 21, 2015, 05:42 

#23 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Hi,
Can you post some logoutput?
__________________
The skeleton ran out of shampoo in the shower. 

September 21, 2015, 06:34 

#24 
New Member
Daniel Rodriguez Calvete
Join Date: Mar 2012
Location: Ferrol (A Coruņa) Spain
Posts: 10
Rep Power: 11 
Hi Philipp,
Thank you for replying me. Here you have time steps of my log. There is extra information (as min max pressure) from the implementation of solver introduced above: Code:
Courant Number mean: 0.002765 max: 0.898738 deltaT = 8.6489e07 Time = 0.3482777 qt = 1 Restart: no CurTim= 24310 startN= 25 DILUPBiCG: Solving for alpha.phase1, Initial residual = 5.02842e05, Final residual = 6.1601e08, No Iterations 1 Phase1 volume fraction = 0.999962 Min(alpha1) = 0.013006 Max(alpha1) = 1 MULES: Correcting alpha.phase1 Liquid phase volume fraction = 0.999962 Min(alpha1) = 0.013006 Max(alpha1) = 1 DILUPBiCG: Solving for Ux, Initial residual = 2.6906e05, Final residual = 4.255e09, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.000145688, Final residual = 5.84061e09, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 3.83835e05, Final residual = 6.46781e11, No Iterations 2 Max vDotcP: 0 Min vDotcP: 1577.04 Max vDotvP: 1682.15 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 7.81377e06, Final residual = 4.49767e09, No Iterations 1 Max vDotcP: 0 Min vDotcP: 1574.63 Max vDotvP: 1682.24 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 6.24766e07, Final residual = 3.15494e09, No Iterations 1 Max vDotcP: 0 Min vDotcP: 1574.57 Max vDotvP: 1682.43 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 2.94952e07, Final residual = 3.28958e09, No Iterations 1 Max vDotcP: 0 Min vDotcP: 1574.57 Max vDotvP: 1682.53 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 1.44687e07, Final residual = 1.87927e09, No Iterations 1 qt = 1 Restart: no CurTim= 24311 startN= 25 smoothSolver: Solving for omega, Initial residual = 3.9347e06, Final residual = 9.11554e10, No Iterations 2 smoothSolver: Solving for k, Initial residual = 4.26664e05, Final residual = 6.30417e10, No Iterations 3 bounding k, min: 5.69094e16 max: 33.7742 average: 1.50846 Max pressure: 249424 Min pressure: 35086.3 Max velocity: 35.3398 ExecutionTime = 582869 s ClockTime = 583548 s MassFlows: OUT.1 = 0.00550569 IN = 0.00543226 fieldMinMax minmaxdomain output: min(p_rgh) = 35222.6 at position (0.0345468 0.0091031 0.0643302) on processor 2 max(p_rgh) = 248788 at position (0.0343493 0.00930316 0.0649426) on processor 2 min(p) = 35086.3 at position (0.0345468 0.0091031 0.0643302) on processor 2 max(p) = 249424 at position (0.0343575 0.00931293 0.0649496) on processor 2 forceCoeffs forceCoeffs_object output: Cm = 0.94257 Cd = 54.1206 Cl = 23.8589 Cl(f) = 10.9869 Cl(r) = 12.872 Courant Number mean: 0.002765 max: 0.898441 deltaT = 8.6489e07 Time = 0.3482786 qt = 1 Restart: no CurTim= 24312 startN= 25 DILUPBiCG: Solving for alpha.phase1, Initial residual = 5.01624e05, Final residual = 6.05526e08, No Iterations 1 Phase1 volume fraction = 0.999962 Min(alpha1) = 0.0129547 Max(alpha1) = 1 MULES: Correcting alpha.phase1 Liquid phase volume fraction = 0.999962 Min(alpha1) = 0.0129547 Max(alpha1) = 1 DILUPBiCG: Solving for Ux, Initial residual = 2.69632e05, Final residual = 4.20864e09, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.000145753, Final residual = 4.02108e09, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 3.84138e05, Final residual = 6.53723e09, No Iterations 1 Max vDotcP: 0 Min vDotcP: 1574.56 Max vDotvP: 1681.62 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 7.78914e06, Final residual = 5.28696e09, No Iterations 1 Max vDotcP: 0 Min vDotcP: 1572.17 Max vDotvP: 1682.33 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 6.16447e07, Final residual = 4.98827e09, No Iterations 1 Max vDotcP: 0 Min vDotcP: 1572.08 Max vDotvP: 1682.6 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 2.88262e07, Final residual = 3.09586e09, No Iterations 1 Max vDotcP: 0 Min vDotcP: 1572.08 Max vDotvP: 1682.72 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 1.36217e07, Final residual = 1.77707e09, No Iterations 1 qt = 1 Restart: no CurTim= 24313 startN= 25 smoothSolver: Solving for omega, Initial residual = 3.93651e06, Final residual = 9.08068e10, No Iterations 2 smoothSolver: Solving for k, Initial residual = 4.26737e05, Final residual = 6.35238e10, No Iterations 3 bounding k, min: 5.62527e16 max: 33.7998 average: 1.50844 Max pressure: 269391 Min pressure: 33755.8 Max velocity: 35.345 ExecutionTime = 582909 s ClockTime = 583589 s MassFlows: OUT.1 = 0.00550573 IN = 0.00543224 fieldMinMax minmaxdomain output: min(p_rgh) = 33895.6 at position (0.0343758 0.0097322 0.0639272) on processor 2 max(p_rgh) = 268795 at position (0.0331139 0.0126315 0.0609156) on processor 2 min(p) = 33755.8 at position (0.0343758 0.0097322 0.0639272) on processor 2 max(p) = 269391 at position (0.0331139 0.0126315 0.0609156) on processor 2 forceCoeffs forceCoeffs_object output: Cm = 0.935114 Cd = 54.0699 Cl = 23.716 Cl(f) = 10.9229 Cl(r) = 12.7931 Courant Number mean: 0.002765 max: 0.898713 deltaT = 8.6489e07 Time = 0.3482795 qt = 1 Restart: no CurTim= 24314 startN= 25 DILUPBiCG: Solving for alpha.phase1, Initial residual = 5.00192e05, Final residual = 6.0447e08, No Iterations 1 Phase1 volume fraction = 0.999962 Min(alpha1) = 0.0128896 Max(alpha1) = 1 MULES: Correcting alpha.phase1 Liquid phase volume fraction = 0.999962 Min(alpha1) = 0.0128896 Max(alpha1) = 1 DILUPBiCG: Solving for Ux, Initial residual = 2.70395e05, Final residual = 5.07551e09, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.000145814, Final residual = 2.27001e10, No Iterations 3 DILUPBiCG: Solving for Uz, Initial residual = 3.84436e05, Final residual = 1.07789e10, No Iterations 2 Max vDotcP: 0 Min vDotcP: 1572.04 Max vDotvP: 1681.8 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 7.74807e06, Final residual = 8.27649e09, No Iterations 1 Max vDotcP: 0 Min vDotcP: 1569.69 Max vDotvP: 1683.2 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 6.10419e07, Final residual = 3.94837e09, No Iterations 1 Max vDotcP: 0 Min vDotcP: 1569.55 Max vDotvP: 1683.5 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 2.88158e07, Final residual = 3.24262e09, No Iterations 1 Max vDotcP: 0 Min vDotcP: 1569.55 Max vDotvP: 1683.6 Min vDotvP: 0 GAMGPCG: Solving for p_rgh, Initial residual = 1.38128e07, Final residual = 2.63841e09, No Iterations 1 qt = 1 Restart: no CurTim= 24315 startN= 25 smoothSolver: Solving for omega, Initial residual = 3.93721e06, Final residual = 9.06762e10, No Iterations 2 smoothSolver: Solving for k, Initial residual = 4.26732e05, Final residual = 6.32552e10, No Iterations 3 bounding k, min: 5.56502e16 max: 33.8248 average: 1.50841 Max pressure: 245957 Min pressure: 33841.4 Max velocity: 35.3512 ExecutionTime = 582950 s ClockTime = 583629 s MassFlows: OUT.1 = 0.00550577 IN = 0.00543221 fieldMinMax minmaxdomain output: min(p_rgh) = 33981.1 at position (0.0343758 0.0097322 0.0639272) on processor 2 max(p_rgh) = 245322 at position (0.0341428 0.0100374 0.0648713) on processor 2 min(p) = 33841.4 at position (0.0343758 0.0097322 0.0639272) on processor 2 max(p) = 245957 at position (0.0341505 0.0100462 0.0648775) on processor 2 forceCoeffs forceCoeffs_object output: Cm = 0.942619 Cd = 54.2101 Cl = 23.8661 Cl(f) = 10.9904 Cl(r) = 12.8757 

September 21, 2015, 07:30 

#25 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Hi Daniel. I don't see anything unusual right now.
Some ideas: 1) Please read henry's first comment about limiting of gradient schemes: http://www.openfoam.org/mantisbt/view.php?id=1410#c3246 So you should not do that in your fvSchemes 2) Did you test the solver with some safe settings, such as first order upwind divergence schemes and so on? 3) Did you run your loop with much more pressure cycles? Now you run 4, but with let's say 8? Even your log doesn't look suspicious, I once had a problem due to too high residuals... You will probably also need to reduce tolerance of the solver then. 4) I don't know the solver you use... do you know 100% that this is actually absolute pressure?
__________________
The skeleton ran out of shampoo in the shower. 

September 25, 2015, 17:23 

#26 
New Member
Daniel Rodriguez Calvete
Join Date: Mar 2012
Location: Ferrol (A Coruņa) Spain
Posts: 10
Rep Power: 11 
Thank you Philipp,
I try three different setup according with your comments: 1) Using the scheme grad(p) Gauss linear; 2) Using upwin in div schemes 3) Using 8 pressure correctors in PISO Here you have a figure representing the minimum pressure in this three cases. https://www.dropbox.com/s/9vc02ca43p...ssure.png?dl=0 All of them give similar minimum pressure and always negative. I am realy confusing what can be happen. Trying to understand what can be happen, I would like to ask you if the turbulence model can have influence on this behaviour. I am using kOmegaSST with y+ ~ 1. Using nut = nutLowReWallFunction; k =kLowReWallFunction; omega = omegaWallFunction, to use kOmegaSST in lowRe mode. Also I try with nut = nutUSpaldingWallFunction as is indicated in this bug on the official OpenCFD bug tracker http://www.openfoam.org/mantisbt/view.php?id=179#c351. By the way, I know that you develop a turbulence model kOmegaSST in lowRe model. Did you validated? Do you think that is apropiate to use in my case? Thank you in advance. 

September 28, 2015, 09:54 

#27 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 23 
Daniel,
First of all: As I understand it your solver it is uncompressional. So it doesn't matter if the pressure goes below zero. Am I right? Secondly: I just implemented the Fluent version of lowRe SST into openFoam. Yes, I think I get the same results as in Fluent. I use it for all lowRe cases.
__________________
The skeleton ran out of shampoo in the shower. 

November 23, 2020, 10:21 
non cavitating simulation using InterPhaseChangeFoam

#28 
New Member
Kanishque Kumar
Join Date: Jul 2020
Posts: 1
Rep Power: 0 
Hello all,
I've been simulating a cavitation model on Naca66 airfoil using InterPhaseChangeFoam solver, and I'm pretty new to this. I was getting abrupt pressure fluctuations over my internal field and was getting very unsatisfactory Cp values for the simulation. So I wanted to check if my model is correct or not. For this i thought of using the same solver and same setup except the cavitation model. I was using the SchnerrSauer cavitation model and set all its coefficients to zero. But it didn't work. Can anyone help me through this ? 

Tags 
cavitation, hydrofoil, interphasechangefoam, numerical scheme, openfoam 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Hydrofoil Cavitation  Richy  STARCCM+  1  July 9, 2014 18:58 
How to select a cavitation model in interPhaseChangeFoam  simon95  OpenFOAM Running, Solving & CFD  1  December 4, 2013 23:42 
Cavitating Flow around a hydrofoil  kimotbwb  CFX  0  October 7, 2012 10:05 
Detecting Cavitation of a Hydrofoil  jacobjb  FloEFD, FloWorks & FloTHERM  1  September 1, 2010 02:48 
[Validation: marine] Hydrofoil NACA 0024  axpl  FLUENT  3  September 19, 2009 09:18 