Hi to everyone,
I am trying to simulate cavitation inside nozzle with kOmega SST turbulence model using interPhaseChangeFoam (at least for this case).When i run the case, after 40 or 50 time-steps always giving following floating point error:
smoothSolver: Solving for alpha.water, Initial residual = 4.1184e-06, Final residual = 3.80347e-09, No Iterations 1
Phase-1 volume fraction = 0.98612 Min(alpha1) = 0.000310125 Max(alpha1) = 1
MULES: Correcting alpha.water
MULES: Correcting alpha.water
Liquid phase volume fraction = 0.98612 Min(alpha1) = 0.000310125 Max(alpha1) = 1
smoothSolver: Solving for Ux, Initial residual = 1.98514e-05, Final residual = 1.02782e-09, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 5.44074e-06, Final residual = 1.94705e-10, No Iterations 2
smoothSolver: Solving for Uz, Initial residual = 8.8507e-05, Final residual = 3.80435e-09, No Iterations 2
GAMG: Solving for p_rgh, Initial residual = 2.79212e-08, Final residual = 2.04895e-10, No Iterations 1
GAMG: Solving for p_rgh, Initial residual = 6.59936e-09, Final residual = 6.59936e-09, No Iterations 0
GAMG: Solving for p_rgh, Initial residual = 6.61102e-09, Final residual = 6.61102e-09, No Iterations 0
GAMGPCG: Solving for p_rgh, Initial residual = 6.61138e-09, Final residual = 6.61138e-09, No Iterations 0
smoothSolver: Solving for omega, Initial residual = 5.4048e-06, Final residual = 6.75835e-10, No Iterations 2
smoothSolver: Solving for k, Initial residual = 9.03591e-06, Final residual = 2.43949e-09, No Iterations 2
ExecutionTime = 97153.3 s ClockTime = 98393 s
Max pressure: 323086
Min pressure: -35072.5
Max velocity: 28.9586
Min velocity: 0
Courant Number mean: 0.00779459 max: 0.0996774
deltaT = 3.50877e-08
Time = 0.01051926
smoothSolver: Solving for alpha.water, Initial residual = 4.11863e-06, Final residual = 3.80331e-09, No Iterations 1
Phase-1 volume fraction = 0.986119 Min(alpha1) = 0.000310159 Max(alpha1) = 1
MULES: Correcting alpha.water
MULES: Correcting alpha.water
Liquid phase volume fraction = 0.986119 Min(alpha1) = 0.000310159 Max(alpha1) = 1
smoothSolver: Solving for Ux, Initial residual = 1.98021e-05, Final residual = 1.02634e-09, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 5.44207e-06, Final residual = 1.94729e-10, No Iterations 2
smoothSolver: Solving for Uz, Initial residual = 8.84228e-05, Final residual = 3.80449e-09, No Iterations 2
GAMG: Solving for p_rgh, Initial residual = 2.58283e-08, Final residual = 1.86337e-10, No Iterations 1
[5] #0 Foam::error::printStack(Foam::Ostream&) at ??:?
[5] #1 Foam::sigFpe::sigHandler(int) at ??:?
[5] #2 in "/lib/x86_64-linux-gnu/libc.so.6"
[5] #3 Foam::divide(Foam::Field&, Foam::UList const&, Foam::UList const&) at ??:?
[5] #4 Foam::tmp Foam::operator/(Foam::tmp const&, Foam::tmp const&) at ??:?
[5] #5 Foam::phaseChangeTwoPhaseMixtures::SchnerrSauer::pCoeff(Foam::GeometricField const&) const at ??:?
[5] #6 Foam::phaseChangeTwoPhaseMixtures::SchnerrSauer::mDotP() const at ??:?
[5] #7 Foam::phaseChangeTwoPhaseMixture::vDotP() const at ??:?
[5] #8
[5] at ??:?
[5] #9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[5] #10
[5] at ??:?
[baris-desktop:10415] *** Process received signal ***
[baris-desktop:10415] Signal: Floating point exception (8)
[baris-desktop:10415] Signal code: (-6)
[baris-desktop:10415] Failing at address: 0x3e8000028af
[baris-desktop:10415] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x36d40) [0x7ff21608cd40]
[baris-desktop:10415] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x39) [0x7ff21608ccc9]
[baris-desktop:10415] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x36d40) [0x7ff21608cd40]
[baris-desktop:10415] [ 3] /home/baris/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so(_ZN4Foam6divideERNS_5FieldIdEERKNS_5UListIdEES6_+0xd5) [0x7ff21734cc05]
[baris-desktop:10415] [ 4] /home/baris/OpenFOAM/baris-2.3.1/platforms/linux64GccDPOpt/lib/libphaseChangeTwoPhaseMixtures.so(_ZN4FoamdvINS_12fvPatchFieldENS_7volMeshEEENS_3tmpINS_14GeometricFieldIdT_T0_EEEERKS8_SA_+0x19b) [0x7ff21ae2aaab]
[baris-desktop:10415] [ 5] /home/baris/OpenFOAM/baris-2.3.1/platforms/linux64GccDPOpt/lib/libphaseChangeTwoPhaseMixtures.so(_ZNK4Foam27phaseChangeTwoPhaseMixtures12SchnerrSauer6pCoeffERKNS_14GeometricFieldIdNS_12fvPatchFieldENS_7volMeshEEE+0x33c) [0x7ff21ae2f3cc]
[baris-desktop:10415] [ 6] /home/baris/OpenFOAM/baris-2.3.1/platforms/linux64GccDPOpt/lib/libphaseChangeTwoPhaseMixtures.so(_ZNK4Foam27phaseChangeTwoPhaseMixtures12SchnerrSauer5mDotPEv+0xff) [0x7ff21ae2ff8f]
[baris-desktop:10415] [ 7] /home/baris/OpenFOAM/baris-2.3.1/platforms/linux64GccDPOpt/lib/libphaseChangeTwoPhaseMixtures.so(_ZNK4Foam26phaseChangeTwoPhaseMixture5vDotPEv+0xa2) [0x7ff21ae18242]
[baris-desktop:10415] [ 8] MRinterPhaseChangeFoam() [0x431350]
[baris-desktop:10415] [ 9] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf5) [0x7ff216077ec5]
[baris-desktop:10415] [10] MRinterPhaseChangeFoam() [0x433792]
[baris-desktop:10415] *** End of error message ***
When I check the results of Pressure, velocity and α distributions seem OK? What I did is:
==> Run the case single and parallel (nothing changed same problem)
==> Increased the mesh number gradually (Still same problem)
==> Change initial conditions, schemes of k and omega (nothing changed)
==>Tried with RNGkeps model. (Fortunately it worked)
==>As a result, i recognized that I am getting this floating error since Omega value is excessively high.
So, does anyone have any idea why it happens? By the way, is there anyone who already obtained good result with kOmegaSST using multiphase solvers of OpenFOAM?
Thanks in advance.
Baris
Hi Daniel,
Thank you for reply. I already checked what you said. I think that main problem is in the implementation of the phase chance model into openfoam due to zero dividing. I have corrected it and i am trying again. If it works, i will post here.
Best Regards.
Baris
I suppose it happened due to CFL restriction too. When I used interPhaseChangeDyMFoam solver for a propeller before, it blowed up and gave me the same error. I advice you to use smaller CFL number, better mesh quality and Kunz cavitation model. Sauer model can be unstable for some cases, but Kunz works
My CFL number is quite small around 0.1 and mesh quality is already tested. Also, I already tried with Kunz model and RNG epsilon model and got good result. However, I would like know the reason why kwSST model does not work properly for the same conditions? Let me know which turbulence model did you use with interPhaseChangeDyFoam? have you ever tried with kwSST model? and obtained good result with multiphase solvers? Also let me know please for which cases Sauer model can give unstable results and WHY?
Thank you.
Hi Mukut,
Yes you are right.
I have found the main reason which is caused by zero dividing (as you said) in the cavitation model implementation.
Thank you
When you solve mass transfer equation, if you apply evoporation in Sauer model, your problem is going to be unphysical and numerically unstable. I determine my turbulence model according to my problem.(External or internal, near wall, far away from wall etc. I mean.) But you can try all of them for your case and you can see the difference between them. In conclusion, all of the turbulence models are approaches which we try to describe a physical and natural fact as mathematically.
What you mean if you apply evaporation? and still this is not answer to my question that WHY my problem is going to be unphysical and numerically unstable? Do you have any physical explanation? then what about the condensation term of Sauer model? Finally, i ask again that have you ever obtained any good results with kwSST? if so, just let me know that conditions....
Thank you
Ohh OK. Actually I suppose if mag(p - pSat()) + 0.01*pSat()) is negative, it blows up. When I use kwSST turbulence model during propulsion analysis, I have better convergence than kEpsilon. And my simulation was unsteady. You know that I solved VP1304 validation propeller with %0.4 absolute error.
Yeah this is one of the reason. The another reason is related unbounded value of the turbulence parameters.
Ohh OK. I calculate these turbulence parameters using a tool which has been developed in cfdonline.com . Generally I use turbulent length scale to define them. I do not really know how to define Eddy viscosity ratio. But I can estimate turbulent length scale as propeller radius or length over all of ship etc.
The problem is for the mesh quality and the delta time calculation due to you are using PIMPLE in PISO form. In fact, if you write to print the courant number as function on your system/control or call the function, you can see than the courant number increase quickly. My advises are: a) You can fix your mesh b) reduce the delta time c) You can set that the simulation have a dynamic delta t using maxCo
Hi Victor,
Thank you for your advises. Actually, the most probable floating point error in openfoam is caused by zero dividing. SInce i am using interphasechange foam which includes cavitation modelling. That was the reason in my case which results in zero dividing. Yes you are right not only my case for all CFD cases the mesh quality is one of the important reason which should be checked and therefore should be carried out mesh independency test.
Only regarding to your advice c) mostly i set the the Co number below zero? you mean adjustable deltaT by saying a dynamic delta t ? If not let me know clearly please what you mean.
Thank you.
Baris
Hi Baris,
I did some simulations for my PhD investigation using a modified version of interPhaseChangeFoam for cavitation with implicit LES as a turbulence model. I found that the if the quality of mesh is not good enough for some tips is possible avoid the the floating points reducing the delta T. Then I have used dynamic time with maxCo (maximum Courant Number) < 1 as external corrector based on Courant–Friedrichs–Lewy condition. Perhaps, you can use for your simulation and that is my advise c).
Hi Baris,
The following answer is from http://www.asergeev.com/files/qatar/openfoam/cases/courant/
"The Courant number is inversely proportional to square of grid spacing. This case shows the occurrence of numerical instability that starts at spots where the grid spacing is exceptionally small. Finally, the code gives "floating point overflow" numerical error." That can be a problem for interPhaseChangeFoam.
Kind regards
Hi Victor,
Thank you very much for reply and a link which gives nice explanation. Yes, you are right, sometimes refining mesh is also not a solution. I also encountered this problem during my LES simulation with interphasechangeFoam.
BR
Baris
Hello Barış,
Recently I also encountered the same problem as yours. In my case, the simulation went well with Kunz model and kOmega SST turbulence model using interPhaseChangeFoam. When it switched to other cavitation models, it crashed after few iterations.
From the error message I got, I knew that floating point exception is caused by zero dividing in cavitation model. But there are no coefficients of cavitation model to be zero. Could you refer me what you corrected in it?
Thank you.
- Badges
- Science topic
- Similar topics
- Thermodynamics
- Pressure