[GM_XIII]

Hi mates,

I am trying to initalize my simplefoam problem with potentialfoam and now i am getting this error:

--> FOAM FATAL ERROR: 

    request for surfaceScalarField phi from objectRegistry region0 failed
    available objects of type surfaceScalarField are

0
(
)


    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 131.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::Ostream& Foam::operator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/opt/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/bin/potentialFoam"
#3  Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> >(Foam::word const&) const in "/opt/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#4  Foam::surfaceInterpolationScheme<Foam::Vector<double> >::addMeshConstructorToTable<Foam::upwind<Foam::Vector<double> > >::New(Foam::fvMesh const&, Foam::Istream&) in "/opt/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5  Foam::surfaceInterpolationScheme<Foam::Vector<double> >::New(Foam::fvMesh const&, Foam::Istream&) in "/opt/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/bin/potentialFoam"
#6  
 at potentialFoam.C:0
#7  
 in "/opt/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/bin/potentialFoam"
#8  __libc_start_main in "/lib/libc.so.6"
#9  
 in "/opt/OpenFOAM/OpenFOAM-2.1.1/platforms/linux64GccDPOpt/bin/potentialFoam"
Aborted

Seems it is looking for the surfaceField phi. Could someone help me with this? Thanks in advance.

I post my fvsolution:

/*--------------------------------*- 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      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
p
{
    solver          GAMG;
    tolerance       1e-06;
    relTol          0.01;
    smoother        DIC;
    cacheAgglomeration true;
    nCellsInCoarsestLevel 500;
    agglomerator    faceAreaPair;
    mergeLevels     1;
}

U
{
    solver          PBiCG;
    preconditioner  DILU;
    tolerance       1e-06;
    relTol          0.0;
}

k
{
    solver          PBiCG;
    preconditioner  DILU;
    tolerance       1e-06;
    relTol          0.0;
}

epsilon
{
    solver          PBiCG;
    preconditioner  DILU;
    tolerance       1e-06;
    relTol          0.0;
}

}
//version OF 1.7.1:
//SIMPLE
//{
//    nNonOrthogonalCorrectors 6;
//    convergence 5e-3;
//}
//version OF 2.1.1:
SIMPLE
{
    nNonOrthogonalCorrectors 8;

    residualControl
    {
        p               5e-3;
        U               1e-3;
        "(k|epsilon)"   1e-3;
    }
}
//version OF 1.7.1:
//relaxationFactors
//{
//    p               0.05;
//    U               0.05;
//    k               0.01;
//    epsilon         0.01;
//}
//version 2.1.1:
relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.7;
        k               0.1;
        epsilon         0.1;
    }

}
potentialFlow
{
    nNonOrthogonalCorrectors 10;
}
// ********************1***************************************************** //

and fvschemes

/*--------------------------------*- 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      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default steadyState;
}

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

divSchemes
{
    default         Gauss linear;
    div(phi,U)      Gauss upwind;
    div(phi,k)      Gauss upwind;//Gauss vanLeer;
    div(phi,epsilon) Gauss upwind;//Gauss vanLeer;
// version 1.7.1:
//   div((nuEff*dev(grad(U).T()))) Gauss linear;
// version 2.1.1:
    div((nuEff*dev(T(grad(U)))))  Gauss upwind phi;
}

laplacianSchemes
{
    default         Gauss upwind phi corrected;
    //laplacian(nuEff,U) Gauss linear corrected;
    //laplacian(1,p) 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         upwind phi;
    interpolate(U)  upwind phi;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p;
}



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

[Bernhard]

I think you should change this

 interpolate(U)  upwind phi;

To something like this

 interpolate(U)  linear;

The problem is that simpleFoam will try to create phi from U by an interpolation. Because you want to discretize it using an upwind scheme, you need phi again. By a linear scheme, that is not necessary. I don't think the interpolate(U) is used anywhere else in the code.

[GM_XIII]

Originally Posted by Bernhard

I think you should change this

 interpolate(U)  upwind phi;

To something like this

 interpolate(U)  linear;

The problem is that simpleFoam will try to create phi from U by an interpolation. Because you want to discretize it using an upwind scheme, you need phi again. By a linear scheme, that is not necessary. I don't think the interpolate(U) is used anywhere else in the code.

Seems logic, thank you mate. I didn't realize that simplefoam take the same shemes in case you dont specify them