[batdan]

Hi everyone!

I am working on a multiphase problem using overset meshes with OpenFOAM v2012 and I'm trying to follow the advise of putting the overset type patches first in the boundary file. So, in the blockMeshDict of the background mesh, I have add the dummy overset boundary:

boundary
(
	oversetPatch
	{
		type overset;
		faces ();
	}
...
);

The output on the boundary file is the following. It surprises me that it does not include the line with the inGroups and it has de line with faces ();.

(
    oversetPatch
    {
        type            overset;
        nFaces          0;
        startFace       2518708;
        faces           ( );
    }
...
);

Then, in the overset mesh, the overset faces are in the same patch with the same previous name:

(
    oversetPatch
    {
        type            overset;
        inGroups        1(overset);
        nFaces          44287;
        startFace       3677752;
    }
...
);

The unexpected behaviour comes when running the mergeMeshes utility, because the following message appears: label patchIndex(const polyPatch& p) : Patch 0 named oversetPatch in mesh XXXX already exists, but patch types do not match. So the oversetPatch remains with zero faces and a new oversetPatch_XXXX is created with the overset faces.

Has anyone faced this problem and know how to solve it? Many thanks in advance!!

[batdan]

Is it possible that the problem is related with the fact that the background mesh is obtained with blockMesh and the overset mesh with snappyHexMesh?
I've seen that the grammar of the boundary file generated with each utility is different, I mean:

Background mesh

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

7
(
    oversetPatch
    {
        type            overset;
        nFaces          0;
        startFace       4172730;
        faces           ( );
    }
...
);

Overset mesh

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

4
(
    oversetPatch
    {
        type            overset;
        inGroups        1(overset);
        nFaces          44512;
        startFace       3823684;
    }
...
);

[gcampana]

Hi,

I believe the problem is that you are not loading up the overset library when you are creating the mesh.

Try to add:

libs            ("liboverset.so");

at the beggining of your controlDict file.

[batdan]

Yes, adding that line has solved the problem. Thank you very much!

[PC6823]

so useful!!!!!