[Flexi1095]

Hi everyone,
I'm currently working on a calculation with OpenFoam and have a problem with simpleFoam.

First of all I have to say that I'm only 19 years and started working with OF half a year ago. In the beginning I got some help, but most of it I have learned on my own (mainly because it really makes fun ). So I'm not extreme high experienced.^^ But during the time, the work with OF works quite well.

At the time I'm trying to simulate a litte car.
"BlockMesh" & "snappyHexMesh -overwrite" worked both without any problems and according to checkMesh the mesh is ok. In addition at the begining I reduce the scale of the imported .stl with

surfaceTransformPoints AutoWF2014.stl AutoWF2014-m.stl scale '(0.001 0.001 0.001)'

because the CAD program exports in mm.
After doing these steps it looks like this:
https://www.dropbox.com/s/bt3n4x6njz...Bild1.jpg?dl=0
https://www.dropbox.com/s/k65hvf9opy...Bild2.jpg?dl=0

But when I start "simpleFoam", I recive an error right away:
https://www.dropbox.com/s/wonrsug9u6...Bild3.jpg?dl=0
https://www.dropbox.com/s/9g8fgj5i7t...Bild4.jpg?dl=0
https://www.dropbox.com/s/mscaxrcaua...Bild5.jpg?dl=0

Any ideas what I can change? Thank you in advance!
Best regards, Michael

[RodriguezFatz]

Hi,

First of all: If you want to post code, click on the "Go Advanced" button and for code click on the "#"-wrap code button. Put your code / log files between the "CODE" tags. No pictures from suspicious places...

Anyway
It looks like the pressure solver doesn't work. Can you post the fvSolution and fvSchemes files (as I wrote above).

[Flexi1095]

Hi RodriguezFatz,
thanks for your reply.
The fvSolution file looks like this.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    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-06;
        relTol          0.1;
        smoother        GaussSeidel;
        nPreSweeps      0;
        nPostSweeps     2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    U
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-08;
        relTol          0.1;
    }

    nuTilda
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps         2;
        tolerance       1e-08;
        relTol          0.1;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
//    pRefCell        0;
//    pRefValue       0;

    residualControl
    {
        p               1e-3;
        U               1e-4;
        nuTilda         1e-4;
    }
}

relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.7;
        nuTilda         0.7;
    }
}


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

and the fvSchemes.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    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 linearUpwind grad(U);
    div(phi,nuTilda) bounded Gauss linearUpwind grad(nuTilda);
    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(DnuTildaEff,nuTilda) Gauss linear corrected;
    laplacian(1,p)  Gauss linear corrected;
}

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

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}


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

[alexeym]

Hi,

Also please post your:

1. checkMesh output
2. Initial and boundary conditions (archive of 0 folder)

As the error happens during solution of pressure equation, you can start by changing GAMG solver to PCG (or play with GAMG settings).

[Flexi1095]

Hi alexeym,

1. checkMesh output:

michael@michael-Lenovo-G510:~/OpenFOAM/michael-2.3.0/run/AutoWF2014$ checkMesh
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  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   : checkMesh
Date   : Jan 14 2015
Time   : 12:08:31
Host   : "michael-Lenovo-G510"
PID    : 4300
Case   : /home/michael/OpenFOAM/michael-2.3.0/run/AutoWF2014
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:           334778
    faces:            873257
    internal faces:   808366
    cells:            270441
    faces per cell:   6.21808
    boundary patches: 7
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     240837
    prisms:        5194
    wedges:        13
    pyramids:      0
    tet wedges:    104
    tetrahedra:    0
    polyhedra:     24293
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            4   841
            5   1398
            6   5988
            7   138
            8   72
            9   11293
           10   27
           11   13
           12   2772
           14   9
           15   1497
           17   1
           18   241
           21   3

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
   *Number of regions: 9
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"
  <<Writing region 0 with 270433 cells to cellSet region0
  <<Writing region 1 with 1 cells to cellSet region1
  <<Writing region 2 with 1 cells to cellSet region2
  <<Writing region 3 with 1 cells to cellSet region3
  <<Writing region 4 with 1 cells to cellSet region4
  <<Writing region 5 with 1 cells to cellSet region5
  <<Writing region 6 with 1 cells to cellSet region6
  <<Writing region 7 with 1 cells to cellSet region7
  <<Writing region 8 with 1 cells to cellSet region8

Checking patch topology for multiply connected surfaces...
                   Patch    Faces   Points                  Surface topology
                   inlet      225      256  ok (non-closed singly connected)
                  outlet      225      256  ok (non-closed singly connected)
                    left     8619     9630  ok (non-closed singly connected)
                   right     1125     1216  ok (non-closed singly connected)
                   floor     7641     8119  ok (non-closed singly connected)
                    roof     1125     1216  ok (non-closed singly connected)
                fahrzeug    45931    48597  ok (non-closed singly connected)

Checking geometry...
    Overall domain bounding box (-1 0 -0.0055) (0.5 0.3 0.3)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (3.20843e-16 -1.31603e-14 5.93089e-15) OK.
    Max cell openness = 3.37423e-16 OK.
    Max aspect ratio = 20.9569 OK.
    Minimum face area = 6.90304e-09. Maximum face area = 0.00040934.  Face area magnitudes OK.
    Min volume = 8.46529e-13. Max volume = 8.1737e-06.  Total volume = 0.137385.  Cell volumes OK.
    Mesh non-orthogonality Max: 55.9442 average: 9.03408
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 2.4256 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

[1]+  Exit 1                  paraFoam

2. Files in 0 folder (exept cellToRegion):
- nut:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.6                                   |
|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 0.006;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           $internalField;
    }
    outlet
    {
        type            zeroGradient;
    }

    right
    {
        type            slip;
    }

    left
    {
        type            symmetryPlane;
    }

    floor
    {
        type            slip;
    }

    roof
    {
        type            slip;
    }

    "fahrzeug.*"
    {
        type            nutUSpaldingWallFunction;
        value           uniform 0;
    }
}

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

- nuTilda:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.6                                   |
|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      nuTilda;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 0.011;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           $internalField;
    }
    outlet
    {
        type            zeroGradient;
    }

    right
    {
        type            slip;
    }

    left
    {
        type            symmetryPlane;
    }

    floor
    {
        type            slip;
    }

    roof
    {
        type            slip;
    }

    "fahrzeug.*"
    {
        type            zeroGradient;
    }
}

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

- p:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.6                                   |
|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet
    {
        type            zeroGradient;
    }
    outlet
    {
        type            fixedValue;
        value           $internalField;
    }

    right
    {
        type            slip;
    }

    left
    {
        type            symmetryPlane;
    }

    floor
    {
        type            slip;
    }

    roof
    {
        type            slip;
    }

    "fahrzeug.*"
    {
        type            zeroGradient;
    }

}

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

- U:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.6                                   |
|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (-33.333 0 0);

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           $internalField;
    }
    outlet
    {
        type            zeroGradient;
    }

    right
    {
        type            slip;
    }

    left
    {
        type            symmetryPlane;
    }

    floor
    {
        type            slip;
    }

    roof
    {
        type            slip;
    }

    "fahrzeug.*"
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
}

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

[RodriguezFatz]

Hi,
Ok, can you try:

p
{
        solver           GAMG;
        tolerance        1e-12;
        relTol           0.1;

        maxIter         20;    

        smoother         DIC;
    
        nPreSweeps       1;
        nPostSweeps      1;
        nFinestSweeps    2;

        cacheAgglomeration true;

        nCellsInCoarsestLevel 1000;
        agglomerator     faceAreaPair;
        mergeLevels      1;
     }

Why do you use an old version of openFOAM? Edit: Ok, it's just the file...

[Flexi1095]

Hi RodriguezFatz,
thanks for your help, but I still get an error.

michael@michael-Lenovo-G510:~/OpenFOAM/michael-2.3.0/run/AutoWF2014$ simpleFoam
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  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   : simpleFoam
Date   : Jan 14 2015
Time   : 13:45:09
Host   : "michael-Lenovo-G510"
PID    : 6967
Case   : /home/michael/OpenFOAM/michael-2.3.0/run/AutoWF2014
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 SpalartAllmaras
SpalartAllmarasCoeffs
{
    sigmaNut        0.66666;
    kappa           0.41;
    Cb1             0.1355;
    Cb2             0.622;
    Cw2             0.3;
    Cw3             2;
    Cv1             7.1;
    Cv2             5;
}

    Employing Ashford correction
No finite volume options present


SIMPLE: convergence criteria
    field p	 tolerance 0.001
    field U	 tolerance 0.0001
    field nuTilda	 tolerance 0.0001


Starting time loop


Time = 1

smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 0.0330649, No Iterations 4
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.0883086, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 0.0976873, No Iterations 2
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) at ??:?
#4  Foam::DICSmoother::DICSmoother(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) at ??:?
#5  Foam::lduMatrix::smoother::addsymMatrixConstructorToTable<Foam::DICSmoother>::New(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) at ??:?
#6  Foam::lduMatrix::smoother::New(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::dictionary const&) at ??:?
#7  Foam::GAMGSolver::initVcycle(Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::lduMatrix::smoother>&, Foam::Field<double>&, Foam::Field<double>&) const at ??:?
#8  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#9  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
#10  Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
#11  
 at ??:?
#12  
 at ??:?
#13  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#14  
 at ??:?
Gleitkomma-Ausnahme (Speicherabzug geschrieben)

I use OpenFoam 2.3.0. I know that 2.3.1 was published in December, but had no time to install the new version. Are there so many advantages that I should do it immediately?

[alexeym]

Hi,

as GAMG fails try PCG, i.e.

    p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-8;
        relTol          1e-2;
    }

Also you've got 55 degree of maximum non-orthogonality, increase number of nNonOrthogonalCorrectors, start with 1-2.

[Flexi1095]

Hi alexeym,
thanks for your idea with PCG, but the error occures at the same time.
Also to increase the numbers of nNonOrthogonalCorrectors doesn't helps.

Another idea: Could the error come from the possibility that the stl file has somewhere a little hole and is not completely closed?

[RodriguezFatz]

Flexi, checkMesh says that mesh openness is not a problem...
But what does that mean:

The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"
  <<Writing region 0 with 270433 cells to cellSet region0
  <<Writing region 1 with 1 cells to cellSet region1
  <<Writing region 2 with 1 cells to cellSet region2
  <<Writing region 3 with 1 cells to cellSet region3
  <<Writing region 4 with 1 cells to cellSet region4
  <<Writing region 5 with 1 cells to cellSet region5
  <<Writing region 6 with 1 cells to cellSet region6
  <<Writing region 7 with 1 cells to cellSet region7
  <<Writing region 8 with 1 cells to cellSet region8

Can you post a picture of your domain?

[betakv]

Dear Flexi1095,

the error is in your mesh. You have there a 8 regions with 1 cell. Please try to create another mesh.

VB

[Flexi1095]

Hi RodriguezFatz & betakv,

@RodriguezFatz: see attachment
So if I understand correctly, the problem comes with snappyHexMesh, which creates the 8 regions with only 1 cell. I have repeated the same process, but there are again these 9 regions.
Do you have an ideas what could cause this problem?

Thanks for your help so far!

[hokhay]

Originally Posted by Flexi1095

Hi RodriguezFatz & betakv,

@RodriguezFatz: see attachment
So if I understand correctly, the problem comes with snappyHexMesh, which creates the 8 regions with only 1 cell. I have repeated the same process, but there are again these 9 regions.
Do you have an ideas what could cause this problem?

Thanks for your help so far!

Hi Rodriguez,

Have you managed to find a solution for this problem?

Sorry to bring this post back. I am now facing the exact same problem with you. I have posted the problem in the forum for 2 weeks but with no single response. It seems the problem has been here for more than at least 2 years but no one has seems to know why.

Could anyone help me with this problem please?

Jason