simpleFoam crushes at 1st Time loop.

seav · May 28, 2013, 12:02

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : simpleFoam
Date   : May 28 2013
Time   : 17:49:50
Host   : "seav-eME730G"
PID    : 17447
Case   : /home/seav/oFOAM/c1
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 RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    sigmaEps        1.3;
}

Creating finite volume options
No finite volume options present


SIMPLE: no convergence criteria found. Calculations will run for 100 steps.


Starting time loop

Time = 1

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8  Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#10  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#11  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#12  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#13  
 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#14  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#15  
 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"

fvSolution

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.05;
        smoother        GaussSeidel;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 20;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    U
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-07;
        relTol          0.1;
    }

    k
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-07;
        relTol          0.1;
    }

    epsilon
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-07;
        relTol          0.1;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
    convergenceCriterion 1.0e-6;
}

relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.5;
        k               0.5;
        epsilon         0.5;
    }
}


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

Hello World !

As I`ve posted up I have strange error and i dont have clue how to repair it. I seek for help in this case.

Arthur.

Lieven · May 28, 2013, 12:49

Hello Arthur,

Welcome to the forum!

You will need to post a bit more information about your case before anyone can really help you out. Else it will be just guessing for the cause of the error (boundary conditions, initial conditions, mesh quality, ...)

So briefly explain what you are simulating, give a description of the mesh (e.g. using checkMesh-output), summarize your boundary conditions and initial conditions, ...

Cheers,

Lieven

seav · May 28, 2013, 13:20

Code:

$checkMesh

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : checkMesh
Date   : May 28 2013
Time   : 18:56:29
Host   : "seav-eME730G"
PID    : 19145
Case   : /home/seav/oFOAM/c1
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 polyMesh for time = 0

Time = 0

Mesh stats
    points:           198319
    faces:            491700
    internal faces:   402300
    cells:            149000
    faces per cell:   6
    boundary patches: 14
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     149000
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
 ***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
   *Number of regions: 149
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    in_gora             100      121      ok (non-closed singly connected)  
    out_gora            100      121      ok (non-closed singly connected)  
    in_dol              100      121      ok (non-closed singly connected)  
    out_dol             100      121      ok (non-closed singly connected)  
    bloki_obliczeniowe  11800    14278    ok (non-closed singly connected)  
    podstawaDol1        100      121      ok (non-closed singly connected)  
    podstawaDol2        100      121      ok (non-closed singly connected)  
    metalStripDol       100      121      ok (non-closed singly connected)  
    metalStripGora      100      121      ok (non-closed singly connected)  
    metalStripS1        100      121      ok (non-closed singly connected)  
    metalStripS2        100      121      ok (non-closed singly connected)  
    podstawaGora1       100      121      ok (non-closed singly connected)  
    podstawaGora2       100      121      ok (non-closed singly connected)  
    defaultFaces        76400    78908    ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (0 0 0) (0.45 0.0115 0.14)
    Mesh (non-empty, non-wedge) directions (0 0 0)
    Mesh (non-empty) directions (0 0 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (5.85253e-18 -1.13453e-16 1.21199e-18) OK.
    Max cell openness = 1.32349e-16 OK.
    Max aspect ratio = -1 OK.
    Minimum face area = 5e-08. Maximum face area = 0.00063.  Face area magnitudes OK.
    Min volume = 1.11665e-10. Max volume = 3.36e-08.  Total volume = 0.0007236.  Cell volumes OK.
    Mesh non-orthogonality Max: 0 average: 0
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 2.23882e-05 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

Boundaries:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

14
(
    in_gora
    {
        type            patch;
        nFaces          100;
        startFace       402300;
    }
    out_gora
    {
        type            patch;
        nFaces          100;
        startFace       402400;
    }
    in_dol
    {
        type            patch;
        nFaces          100;
        startFace       402500;
    }
    out_dol
    {
        type            patch;
        nFaces          100;
        startFace       402600;
    }
    bloki_obliczeniowe
    {
        type            empty;
        inGroups        1(empty);
        nFaces          11800;
        startFace       402700;
    }
    podstawaDol1
    {
        type            wall;
        nFaces          100;
        startFace       414500;
    }
    podstawaDol2
    {
        type            wall;
        nFaces          100;
        startFace       414600;
    }
    metalStripDol
    {
        type            wall;
        nFaces          100;
        startFace       414700;
    }
    metalStripGora
    {
        type            wall;
        nFaces          100;
        startFace       414800;
    }
    metalStripS1
    {
        type            wall;
        nFaces          100;
        startFace       414900;
    }
    metalStripS2
    {
        type            wall;
        nFaces          100;
        startFace       415000;
    }
    podstawaGora1
    {
        type            wall;
        nFaces          100;
        startFace       415100;
    }
    podstawaGora2
    {
        type            wall;
        nFaces          100;
        startFace       415200;
    }
    defaultFaces
    {
        type            empty;
        inGroups        1(empty);
        nFaces          76400;
        startFace       415300;
    }
)

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

fvSchemes:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;
    grad(p)         Gauss linear;
    grad(U)         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      bounded Gauss limitedLinearV 1;
    div(phi,k)      bounded Gauss limitedLinear 1;
    div(phi,epsilon) bounded Gauss limitedLinear 1;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         none;
    laplacian(nuEff,U) Gauss linear corrected;
    laplacian((1|A(U)),p) Gauss linear corrected;
    laplacian(DkEff,k) Gauss linear corrected;
    laplacian(DepsilonEff,epsilon) Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
    interpolate(U)  linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}


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

fvSolution:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.05;
        smoother        GaussSeidel;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 20;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    U
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-07;
        relTol          0.1;
    }

    k
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-07;
        relTol          0.1;
    }

    epsilon
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-07;
        relTol          0.1;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
    convergenceCriterion 1.0e-6;
}

relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.5;
        k               0.5;
        epsilon         0.5;
    }
}


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

controlDict:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     simpleFoam;

startFrom       latestTime;

startTime       0;

stopAt          endTime;

endTime         100;

deltaT          1;

writeControl    timeStep;

writeInterval   50;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;


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

RASproperties:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      RASProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

RASModel        kEpsilon;

turbulence      on;

printCoeffs     on;


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

transportProperties:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

transportModel  Newtonian;

nu              nu [ 0 2 -1 0 0 0 0 ] 1e-05;

CrossPowerLawCoeffs
{
    nu0             nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;
    nuInf           nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
    m               m [ 0 0 1 0 0 0 0 ] 1;
    n               n [ 0 0 0 0 0 0 0 ] 1;
}

BirdCarreauCoeffs
{
    nu0             nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;
    nuInf           nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;
    k               k [ 0 0 1 0 0 0 0 ] 0;
    n               n [ 0 0 0 0 0 0 0 ] 1;
}


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

I want to solve numerical simulation of convection heat transfer. To do this I use blockMesh and simpleFoam. However I got error which i posted in my last and first post in the same time

. For now long I am out off ideas what goes wrong.

If you need anything else to analyse my problem, just say.

Arthur.

Lieven · May 28, 2013, 14:01

Hi Arthur,

There is something strange going on in your mesh. The checkMesh-utility reports that the mesh is 3D (i.e. not 1D or 2D), yet you define an empty patch somewhere... This is only used for 2D cases (maybe it also works for 1D, don't know, anyway not the point). So could be post your blockmesh-file and a sketch of the geometry you want to draw cause I have the strong impression it is a mesh-related issue.

Cheers,

L

seav · May 28, 2013, 18:28

Hi Leiven, thank you for your response.

My blockMeshDict file is heavy one and excceds line limit. Sketch won`t show main problem with geometry, I mean the geometery is "sticky". I will try to show this file.

I do define empty patch. I looked up into pitzDaily tutorial from simpleFoam tutorials folder.

Cheers,
Arthur.

Lieven · May 29, 2013, 08:32

Normally you should be able to attach the file to the post without having to embed it in the text.

Can you explain a bit why you define the empty patch? It is indeed done in the simpleFoam tutorial but this is simply cause the tutorial is 2D.

Cheers,

L

seav · May 29, 2013, 10:06

Hi, Lieven.

Yes I did attachment. Here is a file, however its with *.c extension. I assume you have change it.

I think I didnt understand documentation properly. And you have right about difference 1D 2D and 3D with empty patch.

To notice what problem comes with geometery please use paraFoam -block and uncheck first three blocks before creating mesh.

Cheers,
Arthur.

Lieven · May 29, 2013, 10:12

That's a very big blockMeshDict file

But this confirms a bit my suspicion, the empty-patch should be defined for a 3D mesh. So I would recommend you to read the manual and try to correct the file.

Good luck,

Lieven

seav · May 29, 2013, 10:41

I did change empty patch to wall. In fact I dont know why I didnt do this at first.

However, it didnt solve my problem :

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : simpleFoam
Date   : May 29 2013
Time   : 16:20:43
Host   : "seav-eME730G"
PID    : 3462
Case   : /home/seav/oFOAM/c1
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 RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    sigmaEps        1.3;
}

Creating finite volume options
No finite volume options present


SIMPLE: no convergence criteria found. Calculations will run for 100 steps.


Starting time loop

Time = 1

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8  Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#10  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#11  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#12  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#13  
 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#14  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#15  
 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"

I assume this is the problem :

Code:

No finite volume options present

SIMPLE: no convergence criteria found. Calculations will run for 100 steps.

My blockMeshDict has been created by matlab script .

Arthur.

Lieven · May 29, 2013, 10:44

This is no problem

Code:

No finite volume options present  SIMPLE: no convergence criteria found. Calculations will run for 100 steps.

I'm more curious for the output of checkMesh. Could you post this again?

Cheers,

L

seav · May 29, 2013, 12:02

I found this : http://www.cfd-online.com/Forums/ope...ion-1-6-a.html

With similar problem with mine... so I used ;

Code:

refineMesh -overwrite

It did refine but the error is still the same.

checkMesh:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : checkMesh
Date   : May 29 2013
Time   : 18:00:02
Host   : "seav-eME730G"
PID    : 4262
Case   : /home/seav/oFOAM/c1
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 polyMesh for time = 0

Time = 0

Mesh stats
    points:           1379889
    faces:            3754800
    internal faces:   3397200
    cells:            1192000
    faces per cell:   6
    boundary patches: 14
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     1192000
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
 ***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
   *Number of regions: 149
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    in_gora             400      441      ok (non-closed singly connected)  
    out_gora            400      441      ok (non-closed singly connected)  
    in_dol              400      441      ok (non-closed singly connected)  
    out_dol             400      441      ok (non-closed singly connected)  
    bloki_obliczeniowe  47200    52038    ok (non-closed singly connected)  
    podstawaDol1        400      441      ok (non-closed singly connected)  
    podstawaDol2        400      441      ok (non-closed singly connected)  
    metalStripDol       400      441      ok (non-closed singly connected)  
    metalStripGora      400      441      ok (non-closed singly connected)  
    metalStripS1        400      441      ok (non-closed singly connected)  
    metalStripS2        400      441      ok (non-closed singly connected)  
    podstawaGora1       400      441      ok (non-closed singly connected)  
    podstawaGora2       400      441      ok (non-closed singly connected)  
    defaultFaces        305600   310428   ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (0 0 0) (0.45 0.0115 0.14)
    Mesh (non-empty, non-wedge) directions (0 0 0)
    Mesh (non-empty) directions (0 0 0)
 ***Number of edges not aligned with or perpendicular to non-empty directions: 36118
  <<Writing 36321 points on non-aligned edges to set nonAlignedEdges
    Boundary openness (6.90913e-18 4.22973e-17 -7.64549e-19) OK.
    Max cell openness = 1.89637e-16 OK.
    Max aspect ratio = -1 OK.
    Minimum face area = 1.25e-08. Maximum face area = 0.0001575.  Face area magnitudes OK.
    Min volume = 1.395e-11. Max volume = 4.2e-09.  Total volume = 0.0007236.  Cell volumes OK.
    Mesh non-orthogonality Max: 0.572747 average: 0.0218034
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.000223949 OK.
    Coupled point location match (average 0) OK.

Failed 1 mesh checks.

End

simpleFoam:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : simpleFoam
Date   : May 29 2013
Time   : 18:01:17
Host   : "seav-eME730G"
PID    : 4263
Case   : /home/seav/Pulpit/mgr/mgr
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 RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    sigmaEps        1.3;
}

Creating finite volume options
No finite volume options present


SIMPLE: no convergence criteria found. Calculations will run for 100 steps.


Starting time loop

Time = 1

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8  Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#10  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#11  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#12  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#13  
 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#14  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#15  
 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
Błąd w obliczeniach zmiennoprzecinkowych (core dumped)

A.

Lieven · May 29, 2013, 12:23

Dear Arthur,

I still have the impressing a number of empty faces are defined in the blockMeshDict (based on the checkMesh output). Second, there is also the

Code:

The mesh has multiple regions which are not connected by any face.

warning which is not ok either. You can't expect simpleFoam to do anything usefull if the mesh doesn't make sense.
Therefore, I would recommend you to start from a simplified blockMeshDict and gradually introduce the more complex parts. Make it as simplified as needed for simpleFoam to run.

Cheers,

Lieven

seav · May 29, 2013, 15:47

Lieven, you have right.

I was so focused on initial and boundary conditions that I missed bugs in my blockMeshDict. I will fix this as fast as possible. If you are ok with that I am asking you to suscribe this thread. I dont want to create multiple threads. I just "smell" errors before they happened.

I am start fixing mesh. I will post the results.

A.

Lieven · May 29, 2013, 17:30

Ok, have fun

seav · June 1, 2013, 07:00

blockMesh

Code:

Creating block mesh topology
--> FOAM Warning : 
    From function polyMesh::polyMesh(... construct from shapes...)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 901
    Found 4 undefined faces in mesh; adding to default patch.

checkMesh

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : checkMesh
Date   : Jun 01 2013
Time   : 12:46:19
Host   : "seav-eME730G"
PID    : 6380
Case   : /home/seav/oFOAM/c1
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 polyMesh for time = 0

Time = 0

Mesh stats
    points:           296329
    faces:            770700
    internal faces:   663300
    cells:            239000
    faces per cell:   6
    boundary patches: 16
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     239000
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
 ***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
   *Number of regions: 59
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    in_gora             100      121      ok (non-closed singly connected)  
    out_gora            100      121      ok (non-closed singly connected)  
    in_dol              100      121      ok (non-closed singly connected)  
    out_dol             100      121      ok (non-closed singly connected)  
    face_plyn           58000    63844    ok (non-closed singly connected)  
    face_plyn_zewnetrzne11800    14278    ok (non-closed singly connected)  
    face_przeszkody     36000    39600    ok (non-closed singly connected)  
    podstawaDol1        100      121      ok (non-closed singly connected)  
    podstawaDol2        100      121      ok (non-closed singly connected)  
    metalStripDol       100      121      ok (non-closed singly connected)  
    metalStripGora      100      121      ok (non-closed singly connected)  
    metalStripS1        100      121      ok (non-closed singly connected)  
    metalStripS2        100      121      ok (non-closed singly connected)  
    podstawaGora1       100      121      ok (non-closed singly connected)  
    podstawaGora2       100      121      ok (non-closed singly connected)  
    defaultFaces        400      484      ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (0 0 0) (0.45 0.0115 0.14)
    Mesh (non-empty, non-wedge) directions (0 1 1)
    Mesh (non-empty) directions (0 1 1)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (-1.83771e-19 4.61985e-18 1.2634e-18) OK.
    Max cell openness = 1.65436e-16 OK.
    Max aspect ratio = 280 OK.
    Minimum face area = 4e-08. Maximum face area = 0.00063.  Face area magnitudes OK.
    Min volume = 1e-11. Max volume = 3.36e-08.  Total volume = 0.0007245.  Cell volumes OK.
    Mesh non-orthogonality Max: 0 average: 0
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.000249975 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

Hello,
I did reduce the number of undefined faces, but still there are four which I`ve missed. Is there any possibility to check which faces are undefined ?

Cheers,
Arthur

seav · June 4, 2013, 04:50

simpleFoam:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : simpleFoam
Date   : Jun 04 2013
Time   : 10:40:17
Host   : "seav-eME730G"
PID    : 7212
Case   : /home/seav/oFOAM/c1
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 RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    sigmaEps        1.3;
}

Creating finite volume options
No finite volume options present


SIMPLE: no convergence criteria found. Calculations will run for 100 steps.


Starting time loop

Time = 1

smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.0710741, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.0699946, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 0.0723841, No Iterations 2
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4  Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5  Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8  Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#9  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#10  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#11  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#12  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#13  
 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"
#14  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#15  
 in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/simpleFoam"

checkMesh

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : checkMesh
Date   : Jun 04 2013
Time   : 10:43:13
Host   : "seav-eME730G"
PID    : 7444
Case   : /home/seav/oFOAM/c1
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 polyMesh for time = 0

Time = 0

Mesh stats
    points:           296329
    faces:            770700
    internal faces:   663300
    cells:            239000
    faces per cell:   6
    boundary patches: 16
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     239000
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
   *Number of regions: 59
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    in_gora             100      121      ok (non-closed singly connected)  
    out_gora            100      121      ok (non-closed singly connected)  
    in_dol              100      121      ok (non-closed singly connected)  
    out_dol             100      121      ok (non-closed singly connected)  
    face_plyn           58000    63844    ok (non-closed singly connected)  
    face_plyn_zewnetrzne11800    14278    ok (non-closed singly connected)  
    face_przeszkody     36000    39600    ok (non-closed singly connected)  
    podstawaDol1        100      121      ok (non-closed singly connected)  
    podstawaDol2        100      121      ok (non-closed singly connected)  
    metalStripDol       100      121      ok (non-closed singly connected)  
    metalStripGora      100      121      ok (non-closed singly connected)  
    metalStripS1        100      121      ok (non-closed singly connected)  
    metalStripS2        100      121      ok (non-closed singly connected)  
    podstawaGora1       100      121      ok (non-closed singly connected)  
    podstawaGora2       100      121      ok (non-closed singly connected)  
    defaultFaces        400      484      ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (0 0 0) (0.45 0.0115 0.14)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-1.83771e-19 4.61985e-18 1.2634e-18) OK.
    Max cell openness = 1.65436e-16 OK.
    Max aspect ratio = 900 OK.
    Minimum face area = 4e-08. Maximum face area = 0.00063.  Face area magnitudes OK.
    Min volume = 1e-11. Max volume = 3.36e-08.  Total volume = 0.0007245.  Cell volumes OK.
    Mesh non-orthogonality Max: 0 average: 0
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.000249975 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

blockMesh

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : blockMesh
Date   : Jun 04 2013
Time   : 10:46:09
Host   : "seav-eME730G"
PID    : 7636
Case   : /home/seav/Pulpit/mgr/mgr
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

Creating block mesh from
    "/home/seav/Pulpit/mgr/mgr/constant/polyMesh/blockMeshDict"
Creating curved edges
Creating topology blocks
Creating topology patches

Creating block mesh topology
--> FOAM Warning : 
    From function polyMesh::polyMesh(... construct from shapes...)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 901
    Found 4 undefined faces in mesh; adding to default patch.
--> FOAM Warning : 
    From function polyMesh::polyMesh(... construct from shapes...)
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 919
    Reusing existing patch 15 for undefined faces.

Check topology

	Basic statistics
		Number of internal faces : 180
		Number of boundary faces : 1074
		Number of defined boundary faces : 1074
		Number of undefined boundary faces : 0
	Checking patch -> block consistency

Creating block offsets
Creating merge list .

Creating polyMesh from blockMesh
Creating patches
Creating cells
Creating points with scale 0.001

Writing polyMesh
----------------
Mesh Information
----------------
  boundingBox: (0 0 0) (0.45 0.0115 0.14)
  nPoints: 296329
  nCells: 239000
  nFaces: 770700
  nInternalFaces: 663300
----------------
Patches
----------------
  patch 0 (start: 663300 size: 100) name: in_gora
  patch 1 (start: 663400 size: 100) name: out_gora
  patch 2 (start: 663500 size: 100) name: in_dol
  patch 3 (start: 663600 size: 100) name: out_dol
  patch 4 (start: 663700 size: 58000) name: face_plyn
  patch 5 (start: 721700 size: 11800) name: face_plyn_zewnetrzne
  patch 6 (start: 733500 size: 36000) name: face_przeszkody
  patch 7 (start: 769500 size: 100) name: podstawaDol1
  patch 8 (start: 769600 size: 100) name: podstawaDol2
  patch 9 (start: 769700 size: 100) name: metalStripDol
  patch 10 (start: 769800 size: 100) name: metalStripGora
  patch 11 (start: 769900 size: 100) name: metalStripS1
  patch 12 (start: 770000 size: 100) name: metalStripS2
  patch 13 (start: 770100 size: 100) name: podstawaGora1
  patch 14 (start: 770200 size: 100) name: podstawaGora2
  patch 15 (start: 770300 size: 400) name: defaultFaces

End

Greetings,

I did a little trick. In my blockMeshDict file I added:

Code:

defaultFaces
    	{
        	type wall;
       		faces ();
    	}

However it didnt help me much. Error is different and I dont know if its still mesh problem.

Arthur.

Lieven · June 4, 2013, 05:15

Arthur, the blockMesh setup of the mesh is still not ok.
If everything is ok, it should not give any warning or error.
Applying tricks like the defaultFaces-entry probably will change something but if you don't understand what it changes you should not apply it.

I still stick to my initial advise, simplify the geometry, bring it back to the most basic setup you can think of (only a few blocks) and take that as a starting point for the further development.

Good luck,

Lieven

seav · June 4, 2013, 05:24

Thank you Lieven for fast replay.

I have found those undefined faces.

blockmesh

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : blockMesh
Date   : Jun 04 2013
Time   : 11:18:15
Host   : "seav-eME730G"
PID    : 9839
Case   : /home/seav/Pulpit/mgr/mgr
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

Creating block mesh from
    "/home/seav/Pulpit/mgr/mgr/constant/polyMesh/blockMeshDict"
Creating curved edges
Creating topology blocks
Creating topology patches

Creating block mesh topology

Check topology

	Basic statistics
		Number of internal faces : 180
		Number of boundary faces : 1074
		Number of defined boundary faces : 1074
		Number of undefined boundary faces : 0
	Checking patch -> block consistency

Creating block offsets
Creating merge list .

Creating polyMesh from blockMesh
Creating patches
Creating cells
Creating points with scale 0.001

Writing polyMesh
----------------
Mesh Information
----------------
  boundingBox: (0 0 0) (0.45 0.0115 0.14)
  nPoints: 296329
  nCells: 239000
  nFaces: 770700
  nInternalFaces: 663300
----------------
Patches
----------------
  patch 0 (start: 663300 size: 100) name: in_gora
  patch 1 (start: 663400 size: 100) name: out_gora
  patch 2 (start: 663500 size: 100) name: in_dol
  patch 3 (start: 663600 size: 100) name: out_dol
  patch 4 (start: 663700 size: 58000) name: face_plyn
  patch 5 (start: 721700 size: 11800) name: face_plyn_zewnetrzne
  patch 6 (start: 733500 size: 36000) name: face_przeszkody
  patch 7 (start: 769500 size: 300) name: podstawaDol1
  patch 8 (start: 769800 size: 100) name: podstawaDol2
  patch 9 (start: 769900 size: 100) name: metalStripDol
  patch 10 (start: 770000 size: 100) name: metalStripGora
  patch 11 (start: 770100 size: 100) name: metalStripS1
  patch 12 (start: 770200 size: 100) name: metalStripS2
  patch 13 (start: 770300 size: 300) name: podstawaGora1
  patch 14 (start: 770600 size: 100) name: podstawaGora2
  patch 15 (start: 770700 size: 0) name: defaultFaces

End

checkMesh gives me the same error:

Code:

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
   *Number of regions: 59
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"

However the same error occured.

This case demands such many blocks.. it sounds crazy but its the simplest form of this geometery.

Arthur.

seav · June 4, 2013, 08:18

Lieven, I think I`ve found solution for my problem.

1. I did define all faces in my mesh.
2. I switched solver in my pressure, GAMG to PCG. I did try even on smoothSolver.

Seems all works fine. I need to change my initial conditions and boundaries once again to solve this for proper values.

I will post here the results when my calculations over.

Cheers,
A.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Transient simulation not converging	skabilan	OpenFOAM Running, Solving & CFD	14	December 16, 2019 23:12
Unable to get converged solution using SimpleFoam	jr33	OpenFOAM Running, Solving & CFD	6	December 12, 2016 04:48
pisoFoam with k-epsilon turb blows up - Some questions	Heroic	OpenFOAM Running, Solving & CFD	26	December 17, 2012 03:34
plot over time	fferroni	OpenFOAM Post-Processing	7	June 8, 2012 07:56
Orifice Plate with a fully developed flow - Problems with convergence	jonmec	OpenFOAM Running, Solving & CFD	3	July 28, 2011 05:24

May 28, 2013, 12:49		#2
Lieven Senior Member Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 299 Rep Power: 22	Hello Arthur, Welcome to the forum! You will need to post a bit more information about your case before anyone can really help you out. Else it will be just guessing for the cause of the error (boundary conditions, initial conditions, mesh quality, ...) So briefly explain what you are simulating, give a description of the mesh (e.g. using checkMesh-output), summarize your boundary conditions and initial conditions, ... Cheers, Lieven

May 28, 2013, 14:01		#4
Lieven Senior Member Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 299 Rep Power: 22	Hi Arthur, There is something strange going on in your mesh. The checkMesh-utility reports that the mesh is 3D (i.e. not 1D or 2D), yet you define an empty patch somewhere... This is only used for 2D cases (maybe it also works for 1D, don't know, anyway not the point). So could be post your blockmesh-file and a sketch of the geometry you want to draw cause I have the strong impression it is a mesh-related issue. Cheers, L

May 28, 2013, 18:28		#5
seav Member Join Date: May 2013 Posts: 51 Rep Power: 12	Hi Leiven, thank you for your response. My blockMeshDict file is heavy one and excceds line limit. Sketch won`t show main problem with geometry, I mean the geometery is "sticky". I will try to show this file. I do define empty patch. I looked up into pitzDaily tutorial from simpleFoam tutorials folder. Cheers, Arthur.

May 29, 2013, 08:32		#6
Lieven Senior Member Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 299 Rep Power: 22	Normally you should be able to attach the file to the post without having to embed it in the text. Can you explain a bit why you define the empty patch? It is indeed done in the simpleFoam tutorial but this is simply cause the tutorial is 2D. Cheers, L

May 29, 2013, 10:12		#8
Lieven Senior Member Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 299 Rep Power: 22	That's a very big blockMeshDict file But this confirms a bit my suspicion, the empty-patch should be defined for a 3D mesh. So I would recommend you to read the manual and try to correct the file. Good luck, Lieven

May 29, 2013, 10:44		#10
Lieven Senior Member Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 299 Rep Power: 22	This is no problem Code: No finite volume options present SIMPLE: no convergence criteria found. Calculations will run for 100 steps. I'm more curious for the output of checkMesh. Could you post this again? Cheers, L

May 29, 2013, 12:23		#12
Lieven Senior Member Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 299 Rep Power: 22	Dear Arthur, I still have the impressing a number of empty faces are defined in the blockMeshDict (based on the checkMesh output). Second, there is also the Code: The mesh has multiple regions which are not connected by any face. warning which is not ok either. You can't expect simpleFoam to do anything usefull if the mesh doesn't make sense. Therefore, I would recommend you to start from a simplified blockMeshDict and gradually introduce the more complex parts. Make it as simplified as needed for simpleFoam to run. Cheers, Lieven

May 29, 2013, 15:47		#13
seav Member Join Date: May 2013 Posts: 51 Rep Power: 12	Lieven, you have right. I was so focused on initial and boundary conditions that I missed bugs in my blockMeshDict. I will fix this as fast as possible. If you are ok with that I am asking you to suscribe this thread. I dont want to create multiple threads. I just "smell" errors before they happened. I am start fixing mesh. I will post the results. A. Last edited by seav; May 29, 2013 at 20:24.

May 29, 2013, 17:30		#14
Lieven Senior Member Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 299 Rep Power: 22	Ok, have fun

June 4, 2013, 05:15		#17
Lieven Senior Member Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 299 Rep Power: 22	Arthur, the blockMesh setup of the mesh is still not ok. If everything is ok, it should not give any warning or error. Applying tricks like the defaultFaces-entry probably will change something but if you don't understand what it changes you should not apply it. I still stick to my initial advise, simplify the geometry, bring it back to the most basic setup you can think of (only a few blocks) and take that as a starting point for the further development. Good luck, Lieven

June 4, 2013, 08:18		#19
seav Member Join Date: May 2013 Posts: 51 Rep Power: 12	Lieven, I think I`ve found solution for my problem. 1. I did define all faces in my mesh. 2. I switched solver in my pressure, GAMG to PCG. I did try even on smoothSolver. Seems all works fine. I need to change my initial conditions and boundaries once again to solve this for proper values. I will post here the results when my calculations over. Cheers, A.