[ngj]

Hi all

I am solving an advection-diffusion equation for suspended sediment transport (variable c). The physical models describe the boundary condition to be set some distance from the bed, say 2d_50 (d_50 being median grain diameter), hence I will use fvMeshSubset to get the computational domain on which I will solve for c.

The sediment transport results in bed level changes and it is being moved using the moving mesh capabilities on the entire mesh.

My question/confirmation quest is:

The fvMesh obtained using fvMeshSubset (local mesh) is a reference to the global fvMesh, so please confirm that moving the pointField on the global mesh carries over to the local mesh?

Thank you very much for your time,

Niels

[ngj]

Hi all

To follow up on my questions, I have come closer to an answer. First of all, it is possible to do what I described (thanks to the OpenFOAM for a very flexible mesh handling). However, there is a little twist in the mesh handling, as the points in the submesh is not updated automatically. Therefor, this is a small guide to how I handled the coupling (everything is based on 1.5, where the fvMeshSubset is constructed differently as in 1.7!):

1. Create the submesh:

fvMeshSubset submesh( c, mesh ); // c is in this case a volScalarField

cellSet cCells(mesh, "cCells");

submesh.setLargeCellSubset(cCells, patchID, true); // patchID is the patch number, which the previously internal faces must adopt.

fvMesh & cMesh = submesh.subMesh();

2. How to move cMesh when mesh has been moved (using the movePoints interface in fvMesh):

const labelList & pointMap_(submesh.pointMap());
const pointField & pp(mesh.points());

pointField cpp(pointMap_.size(), vector::zero);

forAll ( pointMap_, pointi )
{
    cpp[pointi] = pp[pointMap_[pointi]];
}

cMesh.movePoints(cpp);

I hope the above can help someone.

Have a nice weekend,

Niels