[wyldckat]

1. How exactly is "decomposeParDict" configured?
2. Is the case 2D or 3D?

[guilha]

These are the first lines of the decomposeParDict

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    note        "mesh decomposition control dictionary";
    object      decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

numberOfSubdomains  8;

//- Keep owner and neighbour on same processor for faces in zones:
// preserveFaceZones (heater solid1 solid3);

//- Keep owner and neighbour on same processor for faces in patches:
//  (makes sense only for cyclic patches)
//preservePatches (cyclic_half0 cyclic_half1);

preservePatches (
                           tras
                           frente
);

//- Use the volScalarField named here as a weight for each cell in the
//  decomposition.  For example, use a particle population field to decompose
//  for a balanced number of particles in a lagrangian simulation.
// weightField dsmcRhoNMean;

method          scotch;
// method          hierarchical;
// method          simple;
// method          metis;
// method          manual;
// method          multiLevel;
// method          structured;  // does 2D decomposition of structured mesh

It always seemed to me weird, but I've always used the number of subdomains 8 for either case I run, I did not get bigger problems. To change it I have to ask to the administrator.

The case is 3D.

[wyldckat]

I suspect that you're getting an error similar to the one explained here: http://www.openfoam.org/mantisbt/view.php?id=241

Another possibility is that there aren't enough cells near the front and back patches to ensure enough cells for calculations in parallel. You can check this from the face count given by checkMesh for each patch. The number of faces will imply the number of cells associated to them.
If the number of faces for each of the two patches is lesser than 90000, then this is a very big problem. The other count is if the number of faces are more than "90000/2" or "90000/3"; the reason for this is because a single cell of thickness for a mesh sub-domain can lead to serious calculation problems.
I say this because of the numbers given by decomposePar in the lines "Number of cells".

I also suggest that your try another decomposition method, possibly "simple" or "hierarchical".

[guilha]

It works with the simple decomposition method, however some probes are lost.

[wyldckat]

Hi guilha,

Are the probes lost because you continued the simulation or even if you restart from t=0s?

Best regards,
Bruno

[Jetfire]

Hi

I am simulating compressor stage of a turbocharger with the rhoPimpleDyMFoam solver. running moveDynamicMesh -checkAMI was smooth without any errors which assures that my mesh rotates properly and i have defined my interfaces correctly , please point out if i am assuming this wrong.

However running the solver my simulation crashes showing this

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.0-f5222ca19ce6
Exec   : rhoPimpleDyMFoam
Date   : Oct 22 2014
Time   : 12:58:52
Host   : "EAT-Standalone"
PID    : 3546
Case   : /home/eatin/OpenFOAM/eatin-2.3.0/run/tutorials/TurboCharger/Trial_4
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

Selecting dynamicFvMesh solidBodyMotionFvMesh
Selecting solid-body motion function rotatingMotion
Applying solid body motion to cellZone FLUID_ROTOR

PIMPLE: Operating solver in PISO mode

Reading thermophysical properties

Selecting thermodynamics package 
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       sutherland;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

AMI: Creating addressing and weights between 1900 source faces and 32076 target faces
AMI: Patch source sum(weights) min/max/average = 0.995594, 1, 0.999764
AMI: Patch target sum(weights) min/max/average = 0.432794, 1, 0.996788
AMI: Creating addressing and weights between 17748 source faces and 5456 target faces
AMI: Patch source sum(weights) min/max/average = 0.435302, 1.03344, 1.00009
AMI: Patch target sum(weights) min/max/average = 0.816766, 1.00271, 0.999924
AMI: Creating addressing and weights between 17839 source faces and 1957 target faces
AMI: Patch source sum(weights) min/max/average = 0.86998, 1, 0.999108
AMI: Patch target sum(weights) min/max/average = 0.991279, 1, 0.99992
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon
#0  Foam::error::printStack(Foam::Ostream&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::compressible::mutkWallFunctionFvPatchScalarField::calcMut() const in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#4  Foam::compressible::mutWallFunctionFvPatchScalarField::updateCoeffs() in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#5  Foam::fvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam"
#6  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam"
#7  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::fluidThermo const&, Foam::word const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#8  Foam::compressible::RASModel::adddictionaryConstructorToTable<Foam::compressible::RASModels::kEpsilon>::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::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#9  Foam::compressible::RASModel::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::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#10  Foam::compressible::turbulenceModel::addturbulenceModelConstructorToTable<Foam::compressible::RASModel>::NewturbulenceModel(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::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#11  Foam::compressible::turbulenceModel::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::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleTurbulenceModel.so"
#12  
 in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam"
#13  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#14  
 in "/home/eatin/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam"
Floating point exception (core dumped)

I am not able to identify what exactly is the problem and i suppose this is not due to the AMI interfaces as moveDynamicMesh was running perfectly. I have understood after reading few threads that it might be related to my boundary conditions, fvSchemes or fvSolution but i have no idea how to correct this. Please help me solve this and let me know if you need anymore details regarding my simulation.

Thanks

[alexeym]

Hi,

as you've got FPE in mutkWallFunctionFvPatchScalarField::calcMut(), look at the source of the wall function:

tmp<scalarField> mutkWallFunctionFvPatchScalarField::calcMut() const
{
    const label patchi = patch().index();
    const turbulenceModel& turbModel =
        db().lookupObject<turbulenceModel>("turbulenceModel");
    const scalarField& y = turbModel.y()[patchi];
    const scalarField& rhow = turbModel.rho().boundaryField()[patchi];
    const tmp<volScalarField> tk = turbModel.k();
    const volScalarField& k = tk();
    const scalarField& muw = turbModel.mu().boundaryField()[patchi];
    
    const scalar Cmu25 = pow025(Cmu_);
    
    tmp<scalarField> tmutw(new scalarField(patch().size(), 0.0));
    scalarField& mutw = tmutw();
    
    forAll(mutw, faceI)
    {
        label faceCellI = patch().faceCells()[faceI];

        scalar yPlus =
            Cmu25*y[faceI]*sqrt(k[faceCellI])/(muw[faceI]/rhow[faceI]);

        if (yPlus > yPlusLam_)
        {
            mutw[faceI] = muw[faceI]*(yPlus*kappa_/log(E_*yPlus) - 1);
        }
    }

    return tmutw;
}

There's several possible reasons for FPE:
1. rhow[faceI] == 0
2. muw[faceI] == 0
3. k[faceCellI] < 0
4. E_*yPlus <= 0 (this is not the case, cause yPlus > yPlusLam_)

So you need to check if any of conditions 1-3 is true in your case.

[Jetfire]

Hi alexeym,

Thanks for figuring out what the problem is.

There's several possible reasons for FPE:
1. rhow[faceI] == 0
2. muw[faceI] == 0
3. k[faceCellI] < 0
4. E_*yPlus <= 0 (this is not the case, cause yPlus > yPlusLam_)

So you need to check if any of conditions 1-3 is true in your case.

But I am not able to interpret what the above means due to my limited openfoam knowledge. Can you please explain me in a more simplified and detailed way on how do i check the above conditions.

[alexeym]

Hi,

well, it's more-or-less clear from the piece of code, I've posted:

1. rhow is density value on the boundary
2. muw is dynamic viscosity value of the boundary (mu is calculated by thermophysical model)
3. k is turbulent kinetic energy volume field

Also as the error happens during construction of k-epsilon turbulence model, I guess, you have to double check initial values of mu and rho.

[Howard]

Originally Posted by tfuwa

Awesome analysis. Also solved my problem. Thanks.

Hello, friend. Could I ask how you solved your problem in detail? I have met the same situation and maybe your solution can enlighten me. Thank you!

[diananilminikumari]

Dear all,
I come to this place with a similar issue. I have used buoyantBoussinesqPimpleFoam and got the following error ,

Courant Number mean: 0 max: 0

PIMPLE: Operating solver in PISO mode


Starting time loop

Time = 0.005

Courant Number mean: 0 max: 0
DILUPBiCG:  Solving for T, Initial residual = 1, Final residual = 5.2697e-08, No Iterations 4
DICPCG:  Solving for p_rgh, Initial residual = 1, Final residual = 0.00909687, No Iterations 13
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3   at tensorField.C:?
#4  
 at ??:?
#5  
 at ??:?
#6  
 at ??:?
#7  
 at ??:?
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  
 at ??:?
Floating point exception (core dumped)

Hope someone can help me
Thank you

[wyldckat]

Quick answer: You need to revise the boundary conditions you have defined. As explained before in this thread, the error is due to a division by zero... which means that you have defined one or more field fields to use 0.

[kush verma]

Dear All,
I am trying to solve compressible vortex tube case as my compulsory M.E submission and my official guide has no clue about OpenFoam. I am experimenting with both 3D and 2D(axis-symmetric) mesh with various b.c's and schemes but I am getting errors with immediate crash, particularly in compressible solvers like rhoSimpleFoam, sonicFoam, and all. What I wish is to get p, T and U field solution in which you people help .I am attaching 2D mesh and the complete case along with this message I want to mail the 3D case which exceeded the upload limit.

The error report for sonicFoam is here:

Create time

Create mesh for time = 0

Reading thermophysical properties

Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo<eConstThermo<perfectGas>>>>>
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type RASModel
Selecting RAS turbulence model realizableKE
bounding epsilon, min: 0 max: 1408.72 average: 1408.72
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::compressible::RASModels::mutkWallFunctionFvPatchScalarField::calcMut() const in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#4  Foam::compressible::RASModels::mutkWallFunctionFvPatchScalarField::updateCoeffs() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#5  Foam::fvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/sonicFoam"
#6  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/sonicFoam"
#7  Foam::compressible::RASModels::realizableKE::realizableKE(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&, Foam::word const&, Foam::word const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#8  Foam::compressible::RASModel::adddictionaryConstructorToTable<Foam::compressible::RASModels::realizableKE>::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&, Foam::word const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#9  Foam::compressible::RASModel::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&, Foam::word const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#10  Foam::compressible::turbulenceModel::addturbulenceModelConstructorToTable<Foam::compressible::RASModel>::NewturbulenceModel(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&, Foam::word const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#11  Foam::compressible::turbulenceModel::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&, Foam::word const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libcompressibleTurbulenceModel.so"
#12  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/sonicFoam"
#13  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#14  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/sonicFoam"
Floating point exception (core dumped)

Regards:
Kush Verma
kushonthego@gmail.com
9950431523

[Antimony]

Hi,

Your simulation crashes due to floating point error, which from the stack trace seems to be from epsilon value being zero (minimum value).

Check your BC for epsilon and if there is zero, change to a number that is non-zero and realistic for the problem.

Hope this helps.

Cheers,
Antimony

[esujby]

Hello I have a similar issue and i am running the debug version but still can't understand the problem. i would really appreciate some guidance, please find attached my log file. heres a snippet:

/

*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 3.0.x-21cbbf7beb56
Exec   : chtMultiRegionFoam -parallel
Date   : Jan 28 2016
Time   : 21:20:10
Host   : "ubuntu"
PID    : 25149
Case   : /home/parallels/OpenFOAM/OpenFOAM-3.0.x/chtMRF
nProcs : 16
Slaves : 
15
(
"ubuntu.25150"
"ubuntu.25151"
"ubuntu.25152"
"ubuntu.25153"
"ubuntu.25154"
"ubuntu.25155"
"ubuntu.25156"
"ubuntu.25157"
"ubuntu.25158"
"ubuntu.25159"
"ubuntu.25160"
"ubuntu.25161"
"ubuntu.25162"
"ubuntu.25163"
"ubuntu.25164"
)

Pstream initialized with:
    floatTransfer      : 0
    nProcsSimpleSum    : 0
    commsType          : nonBlocking
    polling iterations : 0
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create fluid mesh for region fluid for time = 0

Create solid mesh for region insulator for time = 0

Create solid mesh for region s1 for time = 0

Create solid mesh for region s2 for time = 0

Create solid mesh for region s3 for time = 0

Create solid mesh for region s4 for time = 0

Create solid mesh for region s5 for time = 0

Create solid mesh for region s6 for time = 0

Create solid mesh for region s7 for time = 0

Create solid mesh for region s8 for time = 0

Create solid mesh for region s9 for time = 0

Create solid mesh for region s10 for time = 0

Create solid mesh for region s11 for time = 0

Create solid mesh for region s12 for time = 0

Create solid mesh for region s13 for time = 0

Create solid mesh for region s14 for time = 0

Create solid mesh for region s15 for time = 0

Create solid mesh for region lens for time = 0

*** Reading fluid mesh thermophysical properties for region fluid

    Adding to thermoFluid

Selecting thermodynamics package 
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

[3] #0  Foam::error::printStack(Foam::Ostream&)[10] #0  Foam::error::printStack(Foam::Ostream&)[13] #0  Foam::error::printStack(Foam::Ostream&)[5] #0  Foam::error::printStack(Foam::Ostream&)[1] #0  Foam::error::printStack(Foam::Ostream&)[9] #0  Foam::error::printStack(Foam::Ostream&)[11] #0  Foam::error::printStack(Foam::Ostream&)[14] #0  Foam::error::printStack(Foam::Ostream&)[7] #0  Foam::error::printStack(Foam::Ostream&)[0] #0  Foam::error::printStack(Foam::Ostream&)[6] #0  Foam::error::printStack(Foam::Ostream&)[15] #0  Foam::error::printStack(Foam::Ostream&)[8] #0  Foam::error::printStack(Foam::Ostream&)[12] #0  Foam::error::printStack(Foam::Ostream&)[2] #0  Foam::error::printStack(Foam::Ostream&)[4] #0  Foam::error::printStack(Foam::Ostream&) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[7] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[11] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[13] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[8] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
 at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
 at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[15] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[3] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[9] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[10] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[6] #1  Foam::sigFpe::sigHandler(int)[12] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[4] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[0] #1  Foam::sigFpe::sigHandler(int)[14] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
 at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
 at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/printStack.C:218
[2] #1  Foam::sigFpe::sigHandler(int)[1] #1  Foam::sigFpe::sigHandler(int)[5] #1  Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[0] #2  ? at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[15] #2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
[15] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const in "/lib/x86_64-linux-gnu/libc.so.6"
[0] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[5] #2  ? at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[11] #2  ? at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[1] #2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
[5] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const in "/lib/x86_64-linux-gnu/libc.so.6"
[11] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[14] #2  ? at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[2] #2  ? at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[3] #2  ? at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[7] #2  ? at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[4] #2   at ?~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[10] #2  ? at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[6] #2  ? at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[9] #2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
 in "/lib/x86_64-linux-gnu/libc.so.6"
[14] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const[2] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[8] #2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
[10] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const in "/lib/x86_64-linux-gnu/libc.so.6"
[6] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const in "/lib/x86_64-linux-gnu/libc.so.6"
[4] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const in "/lib/x86_64-linux-gnu/libc.so.6"
[3] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[13] #2  ? at ~/OpenFOAM/OpenFOAM-3.0.x/src/OSspecific/POSIX/signals/sigFpe.C:108
[12] #2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
[7] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const in "/lib/x86_64-linux-gnu/libc.so.6"
[9] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const in "/lib/x86_64-linux-gnu/libc.so.6"
[8] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const in "/lib/x86_64-linux-gnu/libc.so.6"
[13] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const in "/lib/x86_64-linux-gnu/libc.so.6"
[12] #3  Foam::perfectGas<Foam::specie>::psi(double, double) const at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[11] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[5] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[0] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[15] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[1] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
 at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[14] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate()[3] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[2] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[10] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
 at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[7] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate()[4] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[6] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[8] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[9] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[13] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/perfectGasI.H:95
[12] #4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
[5] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&) at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
[3] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&) at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
 at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
[0] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&)[15] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&) at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
[14] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&) at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
 at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
[7] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&)[10] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&) at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
[11] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&) at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
[2] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&) at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
[1] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&) at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
[6] #5  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::heRhoThermo(Foam::fvMesh const&, Foam::word const&) at ~/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/basic/rhoThermo/heRhoThermo.C:82 (discriminator 2)
[4] #5  Foam::heRhoThermo<Foam::rhoThermo,

kind regards

[wyldckat]

Quick answer @Nasir: The crash occurred in the file "src/thermophysicalModels/specie/equationOfState/perfectGas/perfectGasI.H", in this piece of code:

template<class Specie>
inline Foam::scalar Foam::perfectGas<Specie>::psi(scalar p, scalar T) const
{
    return 1.0/(this->R()*T);
}

So, either the R constant is 0, or the T value is 0. My guess is that you defined a boundary condition for the T field to be 0 or even the whole internal field is 0. Keep in mind that the units you're using are most likely in Kelvin.

[ranasa]

Hi every one
greetings,

dear Bruno, i really enjoyed your meticulous analysis over the cases.

here is a similar error i just faced while running buoyantBoussinesqSimpleFoam in a natural convection problem.
the geometry contains a continuously bending tube, carrying natural gas as well as the surrounding hot fluid to warm up the gas.

the complex geometry within the bends limits the mesh maneuvering. and i still get this message while asking for checkMesh
.... Failed 1 mesh checks.


afterwards i get the main error, without starting to solve!
i doubt whether or not the mesh would be in charge!!!



Create time

Create mesh for time = 0


Reading g
Reading thermophysical properties

Reading field T

Reading field p_rgh

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Creating turbulence model

Selecting RAS turbulence model laminar
Reading field alphat

Calculating field g.h

No finite volume options present


SIMPLE: convergence criteria
field p_rgh tolerance 0.01
field U tolerance 1e-05
field T tolerance 0.01
field "(k|epsilon|omega)" tolerance 0.001


Starting time loop

Time = 1

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 ? at tensorField.C:?
#4 ? at ??:?
#5 ? at ??:?
#6 ? at ??:?
#7 ? at ??:?
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9 ? at ??:?
Floating point exception (core dumped)



appreciating friends' helpful comments

regards,
Rana

[ranasa]

dear friends,

anyone who can give me a tip?

thanks in advance

[ghorob]

Hi everyone
I want to solve a simple heat conduction with phase change (solidification) to model cooling of a steel ingot.

My boundary conditions:
Velocities =0, pressure BC=zeroGradient (at this stage im not interested in flow, just simple heat conduction is desired)

Temperature boundary conditions:
I have 5 patches.
2 of them are fixed Gradient and 3 of them are uniformFixedGradient (reading data from the text files).

My Problem:
My solver works perfect when I set 2 of 5 patches to uniformFixedGradient boundary conditions and keep the other 3 fixedGradient.
But when I apply uniformFixedGradient for 3 patches it gives me the following error:





Starting time loop

***** Time ******* = 0.0001

Courant Number mean: 0 max: 0
smoothSolver: Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0
DICPCG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
DICPCG: Solving for p, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/magma/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/home/magma/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib64/libc.so.6"
#3 double Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) in "/home/magma/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/magma/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) in "/home/magma/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#6 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/magma/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/ingot4"
#7
in "/home/magma/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/ingot4"
#8
in "/home/magma/OpenFOAM/OpenFOAM-2.3.1/platforms/linux64GccDPOpt/bin/ingot4"
#9 __libc_start_main in "/lib64/libc.so.6"
#10
at /home/abuild/rpmbuild/BUILD/glibc-2.15/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception


the solver reads the thermal gradient for 3 BCs of uniformFixedGradient from 3 text files. there is no zero number there. These 3 text files are the same and they start from time zero to end of simulation (26sec).
*****my text file*****
(
(0 -15)
(5 -45)
(10 -30)
(15 -20)
(26 -32)
);
I know that "sigFpe" is related to the numeric calculation. But when I use 2 BCs instead of 3 BCs and read 2 text file instead of 3 my program works. So I think there is no problem with thermal gradient in the text file.

[iamranjitsingh]

while starting the simulation i am facing the following problem,, can anyone help me out

--> FOAM FATAL ERROR:
hanging pointer of type N4Foam11dimensionedIdEE at index 0 (size 1), cannot dereference