Exception en virgule flottante

taalf · January 16, 2011, 09:13

Hello everybody,

I'm proud to post my first comment in this forum

. I don't speak English so good so I apologize for every English mistakes

.

And, to show how much I am motivated, I will put pictures in my post : I set a good example, isn't it

?

Ok, I'm a false beginner in OpenFOAM that I study for my Final Project and it happens something that I don't understand and that I very would like to solve.

My problem is that when I make a coarse blockMesh geometry for a own icoFoam case, it works, but when I use a finer mesh, it makes an "Exception en virgule flottante" during calculation after very few first iterations.

Here is my coarse case (a 2D case with 2 "empty" boundary conditions and only one cell in the z direction) :

with, in my transportProperties file :

Code:

transportModel  Newtonian;

nu              nu [0 2 -1 0 0 0 0] 1e-06;

and, in my controlDict file :

Code:

application     icoFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         1;

deltaT          0.001;

writeControl    timeStep;

writeInterval   100;

and the results :

Pretty good, isn't it ?

Then, I tried to use a finer mesh by only modifying the simpleGrading values in the blockMeshDict:

but this happens when I launch icoFoam after deleting the old time directories (0 0.1 0.2 etc.) :

Code:

Time = 0.011

Courant Number mean: 1.01727e+34 max: 7.44368e+37
DILUPBiCG:  Solving for Ux, Initial residual = 5.77125e-09, Final residual = 5.77125e-09, No Iterations 0
DILUPBiCG:  Solving for Uy, Initial residual = 2.41172e-09, Final residual = 2.41172e-09, No Iterations 0
#0  Foam::error:: printStack(Foam::Ostream&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#1  Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#2  Uninterpreted: 
#3  Foam:: DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#4  Foam:: DICPreconditioner:: DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#5  Foam::lduMatrix:: preconditioner::addsymMatrixConstructorToTable<Foam:: DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#6  Foam::lduMatrix:: preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#7  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#8  Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam171/lib/linuxGccDPOpt/libfiniteVolume.so"
#9  
 in "/opt/openfoam171/applications/bin/linuxGccDPOpt/icoFoam"
#10  __libc_start_main in "/lib/libc.so.6"
#11  
 in "/opt/openfoam171/applications/bin/linuxGccDPOpt/icoFoam"
Exception en point flottant

Even if I reduce the time between iterations :

Code:

deltaT          0.0000001;

it stops after few iterations with the same error.

My extraordinary happiness when I computed my first case totally collapsed when I realized I wasn't able to redo it with fine mesh !

Does somebody have an idea ?

olivierG · January 17, 2011, 06:47

hello,

Check your Co number:1e34 max !
My guess i a bad boundary condition: give boundary + fvSchemes for more info.
regards,
olivier

taalf · January 17, 2011, 07:44

Hello,

Yes, the curent number is awesome ! But I think it is due to a solver problem because my theoretical curent number should be very low, as the max velocity is around 0.025 m/s and the size of my cells is about 0.025 m, so :

C0 = dt * |U| / dx => C0 = 0.001 * 0.025 / 0.025 = 0.001 = C0

Here are my files :

constant/polyMesh/blockMeshDict :

Code:

/*--------------------------------*- C++ -*----------------------------------*\                                    
| =========                 |                                                 |                                    
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |                                    
|  \\    /   O peration     | Version:  1.7.1                                 |                                    
|   \\  /    A nd           | Web:      http://www.OpenFOAM.com               |                                    
|    \\/     M anipulation  |                                                 |                                    
\*---------------------------------------------------------------------------*/                                    
FoamFile                                    
{                                    
    version     2.0;                                    
    format      ascii;                                    
    class       dictionary;                                    
    object      blockMeshDict;                                    
}                                    
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //                                    
                                    
convertToMeters    1    ;                            
                                    
vertices (                                    
(    0    0    0    )    //    0            
(    2    0    0    )    //    1            
(    3    0    0    )    //    2            
(    3    0.5    0    )    //    3            
(    2    0.5    0    )    //    4            
(    0    0.5    0    )    //    5            
(    0    1    0    )    //    6            
(    2    1    0    )    //    7            
(    0    0    0.1    )    //    8            
(    2    0    0.1    )    //    9            
(    3    0    0.1    )    //    10            
(    3    0.5    0.1    )    //    11            
(    2    0.5    0.1    )    //    12            
(    0    0.5    0.1    )    //    13            
(    0    1    0.1    )    //    14            
(    2    1    0.1    )    //    15            
                                    
);                                    
                                    
blocks (                                    
hex (    0    1    4    5    8    9    12    13    )
(    80    20    1    )                    
simpleGrading (    1    1    1    )                    
hex (    5    4    7    6    13    12    15    14    )
(    80    20    1    )                    
simpleGrading (    1    1    1    )                    
hex (    1    2    3    4    9    10    11    12    )
(    40    20    1    )                    
simpleGrading (    1    1    1    )                    
);                                    
                                    
Edges (                                    
);                                    
                                    
patches (                                    
empty                                    
frontAndBack (                                    
(    0    1    4    5    )                
(    5    4    7    6    )                
(    1    2    3    4    )                
(    8    9    12    13    )                
(    13    12    15    14    )                
(    9    10    11    12    )                
)                                    
wall                                    
walls (                                    
(    0    8    9    1    )                
(    1    9    10    2    )                
(    6    7    15    14    )                
(    4    3    11    12    )                
(    12    15    7    4    )                
)                                    
patch                                    
inlet (                                    
(    0    5    13    8    )                
(    5    6    14    13    )                
)                                    
patch                                    
outlet (                                    
(    10    11    3    2    )                
)                                    
);                                    
                                    
mergePatchPairs (                                    
);                                    
                                    
// ************************************************************************* //

0/p:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.4                                   |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

// Field Dictionary

FoamFile
{
    version         2.0;
    format          ascii;

    root            "/home/william";
    case            "default";
    instance        "0";
    local           "";

    class           volScalarField;
    object          p;
}

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


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

internalField   uniform 0;

boundaryField
{
    walls           
    {
        type            zeroGradient;
    }

    frontAndBack           
    {
        type            empty;
    }

    inlet           
    {
        type            zeroGradient;
    }
    
    outlet           
    {
        type            fixedValue;
        value            uniform 0;
    }
}


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

0/U:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.4                                   |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

// Field Dictionary

FoamFile
{
    version         2.0;
    format          ascii;

    root            "/home/william";
    case            "default";
    instance        "0";
    local           "";

    class           volVectorField;
    object          U;
}

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


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

internalField   uniform (0.01 0 0);

boundaryField
{
    walls           
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    
    frontAndBack           
    {
        type            empty;
    }
    

    inlet           
    {
        type            fixedValue;
        value           uniform (0.01 0 0);
    }

    outlet           
    {
        type            zeroGradient;
    }
}


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

system/fvSchemes :

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.4                                   |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

// FoamX Case Dictionary.

FoamFile
{
    version         2.0;
    format          ascii;

    root            "/home/william";
    case            "default";
    instance        "system";
    local           "";

    class           dictionary;
    object          fvSchemes;
}

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

ddtSchemes
{
    default         steadyState;
}

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

divSchemes
{
    default         Gauss upwind;
    div(phi,U)      Gauss upwind;
    div(phi,k)      Gauss upwind;
    div(phi,epsilon) Gauss upwind;
    div(phi,R)      Gauss upwind;
    div(R)          Gauss linear;
    div(phi,nuTilda) Gauss upwind;
    div((nuEff*dev(grad(U).T()))) Gauss linear;
}

laplacianSchemes
{
    default         none;
    laplacian(nu,U) Gauss linear corrected;
    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;
    laplacian(DREff,R) Gauss linear corrected;
    laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

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

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p;
}


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

And, just in case :

constant/TransportProperties:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.4                                   |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

// FoamX Case Dictionary.

FoamFile
{
    version         2.0;
    format          ascii;

    root            "/home/william";
    case            "default";
    instance        "constant";
    local           "";

    class           dictionary;
    object          transportProperties;
}

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

transportModel  Newtonian;

nu              nu [0 2 -1 0 0 0 0] 1e-06;

CrossPowerLawCoeffs
{
    nu0             nu0 [0 2 -1 0 0 0 0] 1.48e-05;
    nuInf           nuInf [0 2 -1 0 0 0 0] 1.48e-05;
    m               m [0 0 1 0 0 0 0] 1.225;
    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;
}


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

system/controlDict:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.4                                   |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

// FoamX Case Dictionary.

FoamFile
{
    version         2.0;
    format          ascii;

    root            "/home/william";
    case            "default";
    instance        "system";
    local           "";

    class           dictionary;
    object          controlDict;
}

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

application     icoFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         1;

deltaT          0.001;

writeControl    timeStep;

writeInterval   100;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression uncompressed;

timeFormat      general;

timePrecision   6;

graphFormat     raw;

runTimeModifiable yes;

functions       
(
);


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

system/fvSolution:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.4                                   |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

// FoamX Case Dictionary.

FoamFile
{
    version         2.0;
    format          ascii;

    root            "/home/william";
    case            "default";
    instance        "system";
    local           "";

    class           dictionary;
    object          fvSolution;
}

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

solvers
{
     p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-06;
        relTol          0;
    }

    U
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0;
    }
    k               PBiCG 
    {
        tolerance       1e-05;
        relTol          0;
        preconditioner  DILU;
    };

    epsilon         PBiCG 
    {
        tolerance       1e-05;
        relTol          0;
        preconditioner  DILU;
    };

    R               PBiCG 
    {
        tolerance       1e-05;
        relTol          0;
        preconditioner  DILU;
    };

    nuTilda         PBiCG 
    {
        tolerance       1e-05;
        relTol          0;
        preconditioner  DILU;
    };
}

PISO
{
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
}

relaxationFactors
{
    p               0.2;
    U               0.2;
    k               0.7;
    epsilon         0.7;
    R               0.7;
    nuTilda         0.7;
}


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

Chris Lucas · January 17, 2011, 08:08

Hi,

you use a transient solver with a steady state ddt scheme.

Either use a different ddt scheme (e.g. Euler) or a steadyState solver (e.g. simpleFoam)

Regards,
Christian

taalf · January 17, 2011, 08:25

Hello,

Thank you very much, guys ! It works perfectly !

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
MPI Error - simpleFoam - Floating Point Exception	scott	OpenFOAM Running, Solving & CFD	3	April 13, 2012 17:34
reactingFoam floating point exception	pajofego	OpenFOAM	0	November 6, 2010 18:29
Cannot Open .sim (Floating Point Exception)	trex930	STAR-CCM+	1	July 30, 2010 07:51
turbFoam floating point exception and k-epsilon	Hectux	OpenFOAM Running, Solving & CFD	4	April 28, 2009 08:10
"exception : return code 139"	june	Siemens	0	January 8, 2008 21:20

January 17, 2011, 06:47		#2
olivierG Senior Member Olivier Join Date: Jun 2009 Location: France, grenoble Posts: 272 Rep Power: 18	hello, Check your Co number:1e34 max ! My guess i a bad boundary condition: give boundary + fvSchemes for more info. regards, olivier

January 17, 2011, 08:08		#4
Chris Lucas Senior Member Christian Lucas Join Date: Aug 2009 Location: Braunschweig, Germany Posts: 202 Rep Power: 18	Hi, you use a transient solver with a steady state ddt scheme. Either use a different ddt scheme (e.g. Euler) or a steadyState solver (e.g. simpleFoam) Regards, Christian

January 17, 2011, 08:25		#5
taalf Member William Tougeron Join Date: Jan 2011 Location: Czech Republic Posts: 70 Rep Power: 15	Hello, Thank you very much, guys ! It works perfectly !