[souvlaki41]

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:

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.

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  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)

/*--------------------------------*- 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;
    }
}


// ************************************************************************* //

/*--------------------------------*- 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;
    }
}

// ************************************************************************* //

[souvlaki41]

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.

[HPE]

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?

[souvlaki41]

Hey,


you can reproduce the error by running the T3A tutorial case with a different grad scheme:

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+

[HPE]

I will try it tomorrow or the earliest time possible. Thank you.

>> Shouldn't this normally work?

Yes, it should, I would expect so.

[HPE]

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`.

[souvlaki41]

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!