[Gennaro]

Hi all,

I'm working on a solver based on Laplacian Foam.

This solver compiles but then crashes returning the following error:

Create time
Create mesh for time = 0
Reading field T
Reading thermophysicalProperties
Selecting thermodynamics package
{
type heSolidThermo;
mixture pureMixture;
transport polynomial;
thermo hPolynomial;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}
Reading Alambda
Reading Slambda
Reading Tlambda
No finite volume options present
Radiation model not active: radiationProperties not found
Selecting radiationModel none
Calculating temperature distribution
SIMPLE: no convergence criteria found. Calculations will run for 0.01 steps.
Time = 1e-06
#0 Foam::error:rintStack(Foam::Ostream&) in "/afs/cern.ch/project/cfd/OpenFOAM/SLC6/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/afs/cern.ch/project/cfd/OpenFOAM/SLC6/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so"
#2
at sigaction.c:0
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/afs/cern.ch/project/cfd/OpenFOAM/SLC6/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so"
#4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/afs/cern.ch/user/g/gbozza/OpenFOAM/gbozza-2.3.x/platforms/linux64Gcc46DPOpt/bin/laplacianFoamCustom"
#5
at laplacianFoamCustom.C:0
#6
in "/afs/cern.ch/user/g/gbozza/OpenFOAM/gbozza-2.3.x/platforms/linux64Gcc46DPOpt/bin/laplacianFoamCustom"
#7 __libc_start_main in "/lib64/libc.so.6"
#8
in "/afs/cern.ch/user/g/gbozza/OpenFOAM/gbozza-2.3.x/platforms/linux64Gcc46DPOpt/bin/laplacianFoamCustom"
Floating exception (core dumped)

I don't understand what SIMPLE: no convergence criteria found means.

Please find in attachment the solver and a case.

Can you please help?

Thanks

Best regards

[alexeym]

Hi,

currently you have in your fvSolution

SIMPLE
{
    nNonOrthogonalCorrectors 4;
}

if you take a look at simpleFoam tutorials, you'll find several additional lines, with tolerances:

    residualControl
    {
        p               1e-2;
        U               1e-3;
        "(k|epsilon|omega)" 1e-3;
    }

these are the values of residual for SIMPLE algorithm to stop (or it will run till the endTime if given residuals are not reached).

Concerning the message you've mentioned, it is written by simpleControl constructor:

src/finiteVolume/cfdTools/general/solutionControl/simpleControl/simpleControl.C

Foam::simpleControl::simpleControl(fvMesh& mesh)
:
    solutionControl(mesh, "SIMPLE"),
    initialised_(false)
{
...
    if (residualControl_.empty())
    {
        Info<< algorithmName_ << ": no convergence criteria found. "
            << "Calculations will run for " << mesh_.time().endTime().value()
            << " steps." << nl << endl;
    }
...
}

so basically message just says: I will run till the endTime (though steady state can be reached earlier).

[Gennaro]

Hi Alex,

thanks for your reply, it was very useful!

Best regards

Genn

[schweb]

Hi Alex,

I don't usually write on forums but I want to thank you for that solution!

That was helpful while running a modified case of laplacianFoam.
The case in the tutorial imports an ANSYS file. I have modified it to import and mesh an stl file.