[e_boesso]

Hi,
I'm trying to implement zeta-F turbulence model by Popovac in openfoam ver. 2.0.0.
After compiling a run time selectable library I'm trying to use it in a tutorial (incompressible/pisofoam/ras/cavity) but when I run the executable this error message appear:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.0.0-d79727c3fca7
Exec : pisoFoam
Date : Jul 14 2011
Time : 11:05:03
Host : ubuntu
PID : 2354
Case : /home/enrico/OpenFOAM/enrico-2.0.0/run/tutorials/incompressible/pisoFoam/ras/cavity
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RASModel
Selecting RAS turbulence model zetaF
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam200/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam200/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) in "/opt/openfoam200/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::dimensioned<double> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) in "/opt/openfoam200/platforms/linux64GccDPOpt/bin/pisoFoam"
#5 Foam::incompressible::RASModels::zetaF::Tau() const in "/home/enrico/OpenFOAM/enrico-2.0.0/platforms/linux64GccDPOpt/lib/libzetaF.so"
#6 Foam::incompressible::RASModels::zetaF::zetaF(Foam ::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&, Foam::word const&) in "/home/enrico/OpenFOAM/enrico-2.0.0/platforms/linux64GccDPOpt/lib/libzetaF.so"
#7 Foam::incompressible::RASModel::adddictionaryConst ructorToTable<Foam::incompressible::RASModels::zet aF>::New(Foam::GeometricField<Foam::Vector<double> , Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/home/enrico/OpenFOAM/enrico-2.0.0/platforms/linux64GccDPOpt/lib/libzetaF.so"
#8 Foam::incompressible::RASModel::New(Foam::Geometri cField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/opt/openfoam200/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#9 Foam::incompressible::turbulenceModel::addturbulen ceModelConstructorToTable<Foam::incompressible::RA SModel>::NewturbulenceModel(Foam::GeometricField<F oam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/opt/openfoam200/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#10 Foam::incompressible::turbulenceModel::New(Foam::G eometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::transportModel&, Foam::word const&) in "/opt/openfoam200/platforms/linux64GccDPOpt/lib/libincompressibleTurbulenceModel.so"
#11
in "/opt/openfoam200/platforms/linux64GccDPOpt/bin/pisoFoam"
#12 __libc_start_main in "/lib/libc.so.6"
#13
in "/opt/openfoam200/platforms/linux64GccDPOpt/bin/pisoFoam"
Floating point exception


I've no experience in c++ programming but I think the initial/boundary conditions are not correctly set: in "0" directory I copy the k file contents in f and zeta file and then change the dimensionset (1/dimTime for f and dimless for zeta).
Where is the error?

[Bernhard]

I am not able to compile your code without errors. Which version of OpenFOAM are you using?

How do you initialize the other fields? I can imagine that the floating point exception is caused by a division by zero somewhere.

[e_boesso]

Thanks for reply,
the other fields are initialized in the same manner as the tutorial do ("0" directory in the tutorial directory).
For compiling the library I use the command "wmake libso" from within the zetaF directory in $PROJECT_USER_DIR environment and no error appear. My version is 2.0.0.

[e_boesso]

I follow the development of the kEpsilon turbulence model as implemented in version 2.0.0 and modify it. If I try to compile my preceding version of zetaF turbulence model set up for openfoam 1.7.1 does not work in release 2.0.0.
I think this is caused by the different implementation of the RASModel base class from 1.7.1 to 2.0.0.

[Bernhard]

So it's obvious that your 2.0 version does not compile in my 1.7
But do I understand correctly that it did work with 1.7?

I understand you initialize with the 0 folder, but with what values?

[e_boesso]

In version 1.7 I compile the code... now I have to test it...right.. but... before do it... openCFD release the 2.0 version! So I change the code to fit into the new version. No tests has been made on this implementation of the turbulence model.
You find "0" case directory below.

[e_boesso]

I find the division by zero error. It's in zetaF.C in the function Tau() (line 52).
The velocity tensor at the denominator has all the components set to 0 because of the initial conditions. There are many other errors I'm trying to resolve.

[Bernhard]

Maybe you can start from a converged k-epsilon solution, so that you won't encounter problems with these kind of issues. An alternative is to add VSMALL or something like that to the denominator.

[e_boesso]

Thanks, it works now. I add fMin_ to the denominator (the same dimensionset is needed in the LHS and RHS of + operator), that is the lower limit value for volScalarField f_.
But I don't understand: the denominator in evaluating the time scale ( Tau() ) is the same that appear in the length scale ( L() ) but only in Tau() function the floating point exception is present.
Why?

[Bernhard]

Maybe because you call Tau() before L()?

By the way, be sure to check the correct implementatation for |S|, I think Hanjalic defines it as (2*S_ij*S_ij)^(1/2)

[e_boesso]

No, excluding the min part of Tau() function from the code, recompiling and running the case the floating point exception is not present.

I write |S| in openfoam as mag(symm(fvc::grad(U_))). Is it correct?

[Bernhard]

First thing: I have no idea.

Second, in your case.

But I think in the zeta-f model, it should be defined as

[e_boesso]

Thanks for the correction.

[e_boesso]

I'm trying to resolve channel flow or backward facing step to validate the model but I've no ideas on how to apply boundary conditions (inlet, outlet and wall) for zeta and f scalar variables.
Suggestions or references to the matter?
Thanks

[Bernhard]

I think Hanjalic proposes a transformation on f which reduces it's boundary condion to f=0. Did you try that?

[e_boesso]

I understand that transformation is valid only for the wall BC.
But for inlet and outlet?
I'm also unable to manage zeta BCs.