[OMN]

Hello

I tried to set up a rough wall for a run with buoyantSimpleFoam in OF 1.7 using the syntax:

wall
{
type mutRoughWallFunction;
Ks uniform 0.005;
Cs uniform 0.5;
value uniform 0;
}

and I got this error message after starting buoyantSimpleFoam:

Selecting RAS turbulence model realizableKE
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam170/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam170/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3 log in "/lib/tls/i686/cmov/libm.so.6"
#4 Foam::compressible::RASModel::yPlusLam(double, double) const in "/opt/openfoam170/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#5 Foam::compressible::RASModels::mutRoughWallFunctio nFvPatchScalarField::calcMut() const in "/opt/openfoam170/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#6 Foam::compressible::RASModels::mutWallFunctionFvPa tchScalarField::updateCoeffs() in "/opt/openfoam170/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#7 Foam::fvPatchField<double>::evaluate(Foam::Pstream ::commsTypes) in "/opt/openfoam170/applications/bin/linuxGccDPOpt/buoyantSimpleFoam"
#8 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/opt/openfoam170/applications/bin/linuxGccDPOpt/buoyantSimpleFoam"
#9 Foam::compressible::RASModels::realizableKE::reali zableKE(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/opt/openfoam170/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#10 Foam::compressible::RASModel::adddictionaryConstru ctorToTable<Foam::compressible::RASModels::realiza bleKE>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/opt/openfoam170/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#11 Foam::compressible::RASModel::New(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/opt/openfoam170/lib/linuxGccDPOpt/libcompressibleRASModels.so"
#12
in "/opt/openfoam170/applications/bin/linuxGccDPOpt/buoyantSimpleFoam"
#13 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#14
in "/opt/openfoam170/applications/bin/linuxGccDPOpt/buoyantSimpleFoam"
Floating point exception

Would someone know what the problem is? Everything works fine with mutWallFunction.

I also tried to use mutRoughWallFunction in the hotroom tutorial for buoyantSimpleFoam but I got the same error message. I also tried this with rhoPorousSimpleFoam and got the same error message. Is this a bug or my lack of understanding of the use of mutRoughWallFunction?

Cheers

Olivier

[mattijs]

We've finally got a proper bug reporting system :-)
Please report any 1.7 bugs on http://www.openfoam.com/bugs.

Thanks,

Mattijs

[anger]

Hi Olivier,

I checked your and andy's communication on the bug tracker; is the issue resolved for you?
Background: I tried the same for rhoPorousSimpleFoam with the angledDuctImplicit tutorial case. All my efforts failed miserably and I did not get the case to run, even with initializing all values in the 0/mut file (error message below).

Selecting RAS turbulence model kEpsilon
#0 Foam::error:rintStack(Foam::Ostream&) in "/soft/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/soft/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 ?? in "/lib/libm.so.6"
#4 log in "/lib/libm.so.6"
#5 Foam::compressible::RASModel::yPlusLam(double, double) const in "/soft/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#6 Foam::compressible::RASModels::mutRoughWallFunctio nFvPatchScalarField::calcMut() const in "/soft/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#7 Foam::compressible::RASModels::mutWallFunctionFvPa tchScalarField::updateCoeffs() in "/soft/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#8 Foam::fvPatchField<double>::evaluate(Foam::Pstream ::commsTypes) in "/soft/OpenFOAM/OpenFOAM-1.7.x/applications/bin/linux64GccDPOpt/rhoPorousSimpleFoam"
#9 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/soft/OpenFOAM/OpenFOAM-1.7.x/applications/bin/linux64GccDPOpt/rhoPorousSimpleFoam"
#10 Foam::compressible::RASModels::kEpsilon::kEpsilon( Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/soft/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#11 Foam::compressible::RASModel::adddictionaryConstru ctorToTable<Foam::compressible::RASModels::kEpsilo n>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/soft/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#12 Foam::compressible::RASModel::New(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/soft/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#13 main in "/soft/OpenFOAM/OpenFOAM-1.7.x/applications/bin/linux64GccDPOpt/rhoPorousSimpleFoam"
#14 __libc_start_main in "/lib/libc.so.6"
#15 _start at /build/buildd/eglibc-2.10.1/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception

To my surprise the case ran through valgrind; I'm in no way an expert what this could mean, but probably an initialisation issue exists. What else did you change to get the case running?

Regards,
--
Thomas

[OMN]

Hello

I ran the case with mutWallFunction for about 100 iterations, then I switched to mutRoughWallFunction. But I did that on my own case, not the tutorial. But it should work: it is indeed an initialization problem. But it is weird that it would affect the solution so strongly.

Kind regards

Olivier

[anger]

Hi,

thanks for your input, Olivier.
Sadly, this did not work for me so I tried to track down this issue.
The problem comes from ypl getting negative at around line 166 of file RASModel.C, so catching this resolves the issue technically; however I do not know what this means physically, i.e. whether an error may be introduced here.
Maybe someone having more insight into the OF internals can comment on this.

Best regards,
--
Thomas

[aerothermal]

I got same messages when trying to use mutRoughWallFunction with kOmegaSST in rhoSimpleFoam.

Is it a confirmed bug? Did someone know how to use wall functions wiht roughness?

[aerothermal]

just try

export FOAM_SIGFPE=false

or

unset FOAM_SIGFPE

[niklas]

find the file RASModel.C

in src/turbulenceModels/compressible/RAS/RASModel

and modify the line to calculate ypl to whats below

scalar RASModel::yPlusLam(const scalar kappa, const scalar E) const
{
    scalar ypl = 11.0;

    for (int i=0; i<10; i++)
    {
      ypl = log(max(E*ypl,1.0))/kappa;
    }

    return ypl;
}

then goto src/turbulenceModels/compressible/RAS
and type wmake libso

now try it again. Does that work better?

[aerothermal]

Originally Posted by niklas

find the file RASModel.C

in src/turbulenceModels/compressible/RAS/RASModel

and modify the line to calculate ypl to whats below

scalar RASModel::yPlusLam(const scalar kappa, const scalar E) const
{
    scalar ypl = 11.0;

    for (int i=0; i<10; i++)
    {
      ypl = log(max(E*ypl,1.0))/kappa;
    }

    return ypl;
}

then goto src/turbulenceModels/compressible/RAS
and type wmake libso

now try it again. Does that work better?

Thank you. It makes sense in order to prevent log(0) calculation. I will implement it anyway.

However, I have found another potential bugs in equations of mutRoughWallFunction. The implementation does not reflect the mathematical modelling found in some references:

• Fluent Documentation On-Line
  http://my.fit.edu/itresources/manual...ug/node512.htm
  http://my.fit.edu/itresources/manual...roughness-calc
  
• Tapia, X.P. PhD Thesis
  http://hig.diva-portal.org/smash/get...936/FULLTEXT01
  

In order to fix that bug, I implemented additional changes to the code, which I called mymutRoughWallFunctionFvPatchScalarField.C. As you can see, I commented out the original lines for reference and traceability.

tmp<scalarField> mymutRoughWallFunctionFvPatchScalarField::calcMut() const
{
    const label patchI = patch().index();

    const RASModel& rasModel = db().lookupObject<RASModel>("RASProperties");
    const scalarField& y = rasModel.y()[patchI];
    const scalarField& rhow = rasModel.rho().boundaryField()[patchI];
    const tmp<volScalarField> tk = rasModel.k();
    const volScalarField& k = tk();
    const scalarField& muw = rasModel.mu().boundaryField()[patchI];

    const scalar Cmu25 = pow(Cmu_, 0.25);

    tmp<scalarField> tmutw(new scalarField(*this));
    scalarField& mutw = tmutw();

    forAll(mutw, faceI)
    {
        label faceCellI = patch().faceCells()[faceI];

        scalar uStar = Cmu25*sqrt(k[faceCellI]);

        scalar yPlus = uStar*y[faceI]/(muw[faceI]/rhow[faceI]);

        scalar KsPlus = uStar*Ks_[faceI]/(muw[faceI]/rhow[faceI]);

//	scalar Edash = E_;
        scalar Edash = 0;
        scalar yPlusLamNew = yPlusLam_;
        if (KsPlus > 2.25)
        {
	    /* it was
            yPlusLamNew = rasModel.yPlusLam(kappa_, Edash);
            Edash /= fnRough(KsPlus, Cs_[faceI]);*/
	    
	    /* it becomes */
            Edash = 1/kappa_*log(fnRough(KsPlus, Cs_[faceI]));
            yPlusLamNew = rasModel.yPlusLam(kappa_, E_);
        }

        if (debug)
        {
            Info<< "yPlus = " << yPlus
                << ", KsPlus = " << KsPlus
                << ", Edash = " << Edash
                << ", yPlusLam = " << yPlusLam_
                << endl;
        }

        if (yPlus > yPlusLamNew)
        {
	    /* it was
            mutw[faceI] =
                muw[faceI]*(yPlus*kappa_/log(max(Edash*yPlus, 1+1e-4)) - 1);

	    Calculation from OpenFOAM original mutWallFunction (smooth wall!!)
            mutw[faceI] = muw[faceI]*(yPlus*kappa_/log(E_*yPlus) - 1);*/

            mutw[faceI] = muw[faceI]*(yPlus*kappa_/
		log(max(E_*yPlus/exp(kappa_*Edash),1+1e-4)) - 1);

        }
    }

    return tmutw;
}

I already run a rough cylinder flow of Re 2.2E5, heat transfer from isothermal wall at 333.15 K and freestream temperature of 303.15. The original OpenFoam gave me a Cp lowest value between the potential solution and the experimental; and provided me a Frossling (which is Nu/sqrt(Re)) three times less than experimental. With the new implementation, everything is in the same order. Both Frossling and Cp are very close to experimental data.

Regards,

Guilherme

[aerothermal]

E is a constant (non-zero).
yplus is 11 at the start and is calculated....

How does it go to zero anyway?

[newOFuser]

Hi

I tried "unset FOAM_SIGFPE" in the .bashrc file followed by the “. $HOME/.bashrc” command, but when I run the case, I still get the following before the simulation starts:
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
SetNaN : Initialising allocated memory to NaN (FOAM_SETNAN).

I tried "export FOAM_SIGFPE=false" as well but that didn't work either.

Do we have to run ./Allwmake in the top-level source directory $WM_PROJECT_DIR as well?

Can anyone who has successfully unset sigFpe provide the details?
Sorry, it seems like it is easy to implement, but I am new to using OF, and would appreciate any help.

Thanks so much.
ak

[rgarcia]

Hi all,

I have a quick and probably stupid question...

I don't understans the code line: "scalar Edash /= E_"

Even when E_ has not been initialised.

Thank you in advance.

Roger