[RodriguezFatz]

Dear all,

I am trying to get a turbulent pipe profile using the cyclic boundary condition on a short piece of pipe.
I use the settings of the "channel395" tutorial and I get the error message:

--> FOAM FATAL ERROR: 
Coupled patches with transformations not supported.
Problematic patch IN

    From function extendedCellToCellStencil::extendedCellToCellStencil(const polyMesh&)
    in file fvMesh/extendedStencil/cellToCell/extendedCellToCellStencil.C at line 50.

FOAM exiting

I don't understand the message. Can someone help me?
BTW: this is an ICEM mesh, that I converted via "Fluent3dMeshtoFoam". I did not set any periodic stuff in ICEM.

boundary file:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.2                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      binary;
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

3
(
    IN
    {
        type            cyclic;
    inGroups        1(cyclic);
        nFaces          7605;
    startFace       2243358;
    matchTolerance  0.0001;
    neighbourPatch  OUT;
    }
    OUT
    {
        type            cyclic;
    inGroups        1(cyclic);
        nFaces          7605;
        startFace       2250963;
    matchTolerance  0.0001;
    neighbourPatch  IN;
    }
    PIPE_WALL
    {
        type            wall;
        nFaces          15444;
        startFace       2258568;
    }
)

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

fvOptions:

/*--------------------------------*- 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      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

momentumSource
{
    type            pressureGradientExplicitSource;
    active          on;            //on/off switch
    selectionMode   all;       //cellSet // points //cellZone

    pressureGradientExplicitSourceCoeffs
    {
        fieldNames  (U);
        Ubar        ( 0 0 10 );
    }
}


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

All boundary files looks like this (U):

/*--------------------------------*- 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       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0 0 10);

boundaryField
{
    IN
    {
    type cyclic;
    }

    OUT
    {
    type cyclic;
    }

    PIPE_WALL
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

}


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

[RodriguezFatz]

Ok, I got it: after trying to understand what the CellToCell... files do, I changed the gradient scheme from
"grad(U) faceLimited pointCellsLeastSquares 1;"
to Gauss linear. Now it works.
So no edgeCellLeastSquares with cyclic boundary conditions? I also see this in the chanell395 tutorial.

[loreasr]

Hello,
I'm experiencing the same problem with my case. I have a cyclic BC and I would like to use The CubicUpwindFit scheme but I get the same error. Any idea of how make it works?

Best wishes

Lorenzo

[ykanani]

Originally Posted by loreasr

Hello,
I'm experiencing the same problem with my case. I have a cyclic BC and I would like to use The CubicUpwindFit scheme but I get the same error. Any idea of how make it works?

Best wishes

Lorenzo

Hello Lorenzo,

I am trying to do the same thing. Did you find any solution?
I need to try higher order upwind scheme in my simulations and it seems this is the only available option in the OpenFOAM which unfortunately does not support the cyclic boundary conditions.

I appropriate if you let me know if you already figured this out.

Thanks,
Yousef