|
[Sponsors] |
kOmegaSSTLM - Floating Point exception during ReThetat solving |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
April 2, 2020, 10:30 |
kOmegaSSTLM - Floating Point exception during ReThetat solving
|
#1 |
New Member
Iason Tsiapkinis
Join Date: Jul 2019
Posts: 8
Rep Power: 7 |
Hello community,
I'm simulating an airfoil with pimpleFoam and kOmegaSST model. As a next step I wanted to try out the kOmegaSSTLM model. I copied the boundary files for ReThetaT and gammaInt from the tutorial case T3A and changed the parameters according to my case. I also added solver and schemes for the two transport equations. Unfortunately I get an Floating point error during the first iteration of ReThetat (see below). As far as troubleshooting goes I tried different divSchemes and Solvers dor Rethetat and gammaInt, without any success. According to the error message the problem lies in kOmegaSSTLM.C, specifically in the Fthetat function: Code:
const volScalarField::Internal Fthetat(this->Fthetat(Us, Omega, nu)); { const volScalarField::Internal t(500*nu/sqr(Us)); const volScalarField::Internal Pthetat ( alpha()*rho()*(cThetat_/t)*(1 - Fthetat) ); // Transition onset momentum-thickness Reynolds number equation tmp<fvScalarMatrix> ReThetatEqn ( fvm::ddt(alpha, rho, ReThetat_) + fvm::div(alphaRhoPhi, ReThetat_) - fvm::laplacian(alpha*rho*DReThetatEff(), ReThetat_) == Pthetat*ReThetat0(Us, dUsds, nu) - fvm::Sp(Pthetat, ReThetat_) + fvOptions(alpha, rho, ReThetat_) ); ReThetatEqn.ref().relax(); fvOptions.constrain(ReThetatEqn.ref()); solve(ReThetatEqn); fvOptions.correct(ReThetat_); bound(ReThetat_, 0); } The problematic variables are either sqrt(Us) or t. I can't find out what t is. Has anyone had any similar issues? The tutorial case T3A is working as intended and I can't find anything I did different, besides using pimpleFoam instead of simpleFoam. Code:
/*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v1612+ | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : v1612+ Exec : pimpleFoam Date : Apr 02 2020 Time : 15:14:37 Host : "c8.hfi.lan" PID : 23326 Case : /home/tsiapkinis/sims191214/sim200214_a174_h10_u10_w20_yplus4_komegaSSTL nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 PIMPLE: Operating solver in PISO mode Reading field p Reading field U Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting turbulence model type RAS Selecting RAS turbulence model kOmegaSSTLM Selecting patchDistMethod meshWave kOmegaSSTCoeffs { alphaK1 0.85; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.856; gamma1 0.555556; gamma2 0.44; beta1 0.075; beta2 0.0828; betaStar 0.09; a1 0.31; b1 1; c1 10; F3 false; } No MRF models present No finite volume options present Starting time loop forces forceCoeffs1: Not including porosity effects forceCoeffs forceCoeffs1: Not including porosity effects Courant Number mean: 0.00154654 max: 0.561152 deltaT = 1.14233e-06 Time = 1.14233e-06 PIMPLE: iteration 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 9.64608e-08, No Iterations 13 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 3.67252e-08, No Iterations 13 DICPCG: Solving for p, Initial residual = 1, Final residual = 9.60166e-06, No Iterations 964 DICPCG: Solving for p, Initial residual = 0.824066, Final residual = 9.74111e-06, No Iterations 804 DICPCG: Solving for p, Initial residual = 0.0603952, Final residual = 9.87242e-06, No Iterations 748 time step continuity errors : sum local = 3.8042e-11, global = 1.6609e-13, cumulative = 1.6609e-13 DICPCG: Solving for p, Initial residual = 0.0361928, Final residual = 9.95209e-06, No Iterations 743 DICPCG: Solving for p, Initial residual = 0.0665034, Final residual = 9.97027e-06, No Iterations 719 DICPCG: Solving for p, Initial residual = 0.011146, Final residual = 9.9849e-06, No Iterations 619 time step continuity errors : sum local = 3.47666e-11, global = -4.71376e-13, cumulative = -3.05287e-13 #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 ? in "/lib64/libc.so.6" #3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:? #4 Foam::tmp<Foam::DimensionedField<double, Foam::volMesh> > Foam::operator/<Foam::volMesh>(Foam::DimensionedField<double, Foam::volMesh> const&, Foam::DimensionedField<double, Foam::volMesh> const&) at ??:? #5 Foam::RASModels::kOmegaSSTLM<Foam::IncompressibleTurbulenceModel<Foam::transportModel> >::Fthetat(Foam::DimensionedField<double, Foam::volMesh> const&, Foam::DimensionedField<double, Foam::volMesh> const&, Foam::DimensionedField<double, Foam::volMesh> const&) const at ??:? #6 Foam::RASModels::kOmegaSSTLM<Foam::IncompressibleTurbulenceModel<Foam::transportModel> >::correctReThetatGammaInt() at ??:? #7 Foam::RASModels::kOmegaSSTLM<Foam::IncompressibleTurbulenceModel<Foam::transportModel> >::correct() at ??:? #8 ? at ??:? #9 __libc_start_main in "/lib64/libc.so.6" #10 ? at ??:? Floating point exception (core dumped) Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: plus | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object ReThetat; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 0 0 0 0]; internalField uniform 200; boundaryField { #includeEtc "caseDicts/setConstraintTypes" inlet { type fixedValue; value $internalField; } outlet { type zeroGradient; } airfoil { type zeroGradient; } topAndBottom { type zeroGradient; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: plus | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object gammaInt; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 0 0 0 0]; internalField uniform 1; boundaryField { #includeEtc "caseDicts/setConstraintTypes" inlet { type fixedValue; value $internalField; } outlet { type zeroGradient; } airfoil { type zeroGradient; } topAndBottom { type zeroGradient; } frontAndBack { type empty; } } // ************************************************************************* // |
|
April 13, 2020, 13:19 |
|
#2 |
New Member
Iason Tsiapkinis
Join Date: Jul 2019
Posts: 8
Rep Power: 7 |
I fixed it.
Apparently the kOmegaSSTLM Model has a problem with my grad(U) specification. I had it at cellLimited Gauss linear 1. Gauss linear works just fine. |
|
April 13, 2020, 16:16 |
|
#3 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 13 |
Hmm interesting. Any chance for you to provide a minimal working example? Might be useful to report such example as a bug by using one of the links below corresponding to the relevant OpenFOAM version?
__________________
The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror |
|
April 13, 2020, 16:29 |
|
#4 |
New Member
Iason Tsiapkinis
Join Date: Jul 2019
Posts: 8
Rep Power: 7 |
Hey,
you can reproduce the error by running the T3A tutorial case with a different grad scheme: Code:
gradSchemes { default Gauss linear; grad(U) cellLimited Gauss linear 1; } Shouldn't this normally work? At least for kOmegaSST. I tried with openfoam5 and v1612+ |
|
April 13, 2020, 16:31 |
|
#5 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 13 |
I will try it tomorrow or the earliest time possible. Thank you.
>> Shouldn't this normally work? Yes, it should, I would expect so.
__________________
The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror |
|
April 14, 2020, 05:15 |
|
#6 |
Senior Member
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 931
Rep Power: 13 |
For
- OpenFOAM-v2002 patch=200316, which is the latest development state, - `tutorials/incompressible/simpleFoam/T3A`, - `grad` scheme changes above, the tutorial simulation has been completed. Might the version update a solution? FYI: I couldn't find a `T3A` tutorial using `pimpleFoam`.
__________________
The OpenFOAM community is the biggest contributor to OpenFOAM: User guide/Wiki-1/Wiki-2/Code guide/Code Wiki/Journal Nilsson/Guerrero/Holzinger/Holzmann/Nagy/Santos/Nozaki/Jasak/Primer Governance Bugs/Features: OpenFOAM (ESI-OpenCFD-Trademark) Bugs/Features: FOAM-Extend (Wikki-FSB) Bugs: OpenFOAM.org How to create a MWE New: Forkable OpenFOAM mirror |
|
April 14, 2020, 07:48 |
|
#7 |
New Member
Iason Tsiapkinis
Join Date: Jul 2019
Posts: 8
Rep Power: 7 |
Yes this is exactly what I tested. With simpleFoam.
Seems like it was fixed, but I can't see any differences in the source code. I'll try out the new version, thank you! |
|
Tags |
floating point exception, komegasst, komegasstlm |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Maximum number of iterations exceeded chtmultiregionsimpleFoam | Moncef | OpenFOAM Running, Solving & CFD | 28 | July 13, 2020 15:26 |
problem with Min/max rho | tH3f0rC3 | OpenFOAM | 8 | July 31, 2019 10:48 |
Suppress twoPhaseEulerFoam energy | AlmostSurelyRob | OpenFOAM Running, Solving & CFD | 33 | September 25, 2018 18:45 |
Unstabil Simulation with chtMultiRegionFoam | mbay101 | OpenFOAM Running, Solving & CFD | 13 | December 28, 2013 14:12 |
Differences between serial and parallel runs | carsten | OpenFOAM Bugs | 11 | September 12, 2008 12:16 |