[mirko]

Hi,

I have a geometry that consists of two blocks that I build and mesh using blockMesh. I have defined two interface patches, and merged them.

I want to solve for the temperature distribution using laplaceFoam.

I get an error because laplaceFoam needs a boundary condition on the interface patch. I typed in `xyz' in the 0/T boundaryField dictionary, and I saw a list of available boundary conditions. I did not see anything that would give me a continuous heat flux across the boundary.

Do I need to implement my own boundary condition, or am I missing a boundary that can do the job?

Thanks,

Mirko

[boger]

Do you need the interface? In other words, having "merged" the two blocks together (using stitchMesh or mergeMesh), shouldn't the interface patches vanish altogether?

[mirko]

Originally Posted by boger

Do you need the interface? In other words, having "merged" the two blocks together (using stitchMesh or mergeMesh), shouldn't the interface patches vanish altogether?

I use mergePatchPairs in the blockMeshDict. I was following the discussion in Section 5.3.2 of the user manual.

Mirko

[boger]

The discussion in 5.3.2 says "if all the faces of a patch are merged, then the patch itself will contain no faces and is removed", so it sounds to me like something went wrong with the merge.

[mirko]

Originally Posted by boger

The discussion in 5.3.2 says "if all the faces of a patch are merged, then the patch itself will contain no faces and is removed", so it sounds to me like something went wrong with the merge.

Hm, you are right. Not sure where my mistake is. Here are parts of the file.

here are the point definitions for the internal patches. They are identical:

    (0 0 4.0) // 4
    (1 0 4.0) // 5
    (1 1 4.0) // 6
    (0 1 4.0) // 7
    (0 0 4.0) // 8
    (1 0 4.0) // 9
    (1 1 4.0) // 10
    (0 1 4.0) // 11

The block definitions:

blocks          
(
    hex (0 1 2 3 4 5 6 7) (1 1 20) simpleGrading (1 1 1)
    hex (8 9 10 11 12 13 14 15) (1 1 100) simpleGrading (1 1 1)
);

The patch definitions:

   patch interface1
    (
        (4 5 6 7)
    )
    patch interface2
    (
        (11 10 9 8)
    )

and the merging:

mergePatchPairs
(
    (
        interface1
        interface2
    )
)

No idea where the error would be. I've attached the full blockMeshDict file.

Thanks,

Mirko

[mirko]

I am adding the mesh view.

One block is with a coarse mesh, and the other with a fine mesh along z
(this is a 1D geometry)

The merged patch is shown by the diagonal lines. Not sure why that is so.

I also built the mesh with the blocks not touching, and faces unmerged, to make sure that the blocks are defined OK. Things looked fine.

Mirko

[boger]

Without having checked the rules, what if you specify interface2 as (8 11 10 9), so that both interfaces begin from the same point in space?

[mirko]

No difference.

For what it's worth, I think that the mesh is valid. If I specify the slip boundary condition on the interface, the calculation runs, and I get an answer that makes sense: the temperature is uniform in each block, the value corresponding to the boundary condition on the far wall.

See attached picture.

[mirko]

I think I found the problem:

I am solving a 1D problem and I set the mesh size in the ignored directions to be 1x1. If I change that to 1x2, 2x1, or 2x2, the internal patch is removed, and I get a temperature ramp as expected.

Mirko