Add channel-transport transport OpenFOAM

[fsimonis]

This PR adds an OpenFOAM variant of the transport participant of the channel-transport tutorial.

The case uses a modified version of the scalarTransportFoam application. Main difference is that we assume U to change every timestep. Therefore we need to recompute $\phi$ every timestep.

@MakisH Can you give this PR a thorough review to make it as easy to use as possible?

Result:

Screencast_20251210_145936.webm

Checklist:

• I added a summary of any user-facing changes (compared to the last release) in the changelog-entries/<PRnumber>.md.
• I will remember to squash-and-merge, providing a useful summary of the changes of this PR.

edit: updated to the working state

[MakisH]

Besides the fact that solver and config are in the same directory, it looks good overall. I have not yet tried to run it.

[MakisH]

@fsimonis this seems to be close to merging. Does this need more work from your side, or just a new review iteration?

edit: Actually, no. There is still a blocking modeling issue.

[MakisH]

Just finished a co-working session with @fsimonis. I pushed some new commits, which make the custom solver work with dynamic meshes and adjusts the case to apply dynamic mesh refinement with dynamicRefineFvMesh, based on the magnitude of the gradient of the transported value.

The settings are in constant/dynamicMeshDict and are currently rather arbitrary. Next step would be to refine these. We worked with an uncoupled scalar transport case based on the pitzDaily tutorial. Here is the draft (also with arbitrary settings):

adaptivePitzDaily.tar.gz

Run with: rm -rf 0.* && blockMesh && dynamicScalarTransportFoam.

The next step would be to further understand and adjust the mesh refinement settings.

The coupled case currently fails, but this is expected since the adapter does not yet support remeshing (precice/openfoam-adapter#382). I can start an implementation of that.

The accumulation of T at the outlet remains. Making the channel longer and refining the mesh showed that the accumulation is really on the last 2-3 layers of the mesh. Changing the system/fvSchemes strongly affected the behavior (to the worse):

divSchemes
{
    default         none;
-    div(phi,T)      Gauss linearUpwind grad(T);
+    div(phi,T)      Gauss linear grad(T);
}

However, the numerics and the boundary conditions are the same as in the pitzDaily case, so this might be unrelated. I would look next if the changes from the standard scalarTransportFoam have any effect (but I would expect not).

Some URLs for reference:

• https://precice.org/couple-your-code-moving-or-changing-meshes.html
• https://api.openfoam.com/2506/classFoam_1_1dynamicRefineFvMesh.html#details
• https://openfoamwiki.net/index.php/Parameter_Definitions_-_dynamicRefineFvMesh

[fsimonis]

I got the non-AMR version running. I moved the AMR specific changes to #689 and will revert this PR to the non-AMR version.
Let's then first merge it and continue from there.

[fsimonis]

@MakisH I think I implemented all suggestions. Could you review again?

[MakisH]

I applied a few more changes directly, and in terms of usability and integration to the rest of the tutorials, the case is ready. It still needs reference results for the system tests (I can add them).

I still have doubts about the outlet conditions and the space integration of T. But I am also still confused.

[MakisH]

I see the trick with the grading, it is already much better, but I am not yet sure that the case is correctly configured. The accumulation at the outlet is gone, but if I just change the mesh (I apply the same blockMeshDict from fluid-openfoam), I still see some accumulation at the outlet and an unphysical jump on the second-last layer:

channel-transport-openfoam.mp4

While I could accept that the origin of the issue is related to the mesh, I would like to better understand it.

Nutils

The combination fluid-openfoam/transport-nutils does not show this issue (solution available on mesh nodes only, Paraview interpolates):

transport-nutils.mp4

Fine grid

Even the fine grid case still shows some temporary accumulation near the center of the outlet when T first reaches the outlet:

channel-transport-openfoam-fine.mp4

If I restrict the value range to 0-0.2, some cells near the corner also look a bit strange, as the values at the last layer of cells are getting smaller than the values in the layer before:

channel-transport-openfoam-fine-range.mp4

Monolithic

To check the monolithic case, I removed the function object from the controlDict, I applied a similar initial condition as in the fluid-openfoam in U: internalField uniform (10 0 0);, and I used the same blockMeshDict as in the fluid-openfoam.

I observe the same "jump" before the obstacle (the accumulation is expected, since the flow field is constant and fully horizontal), but no issue with the outlet:

monolithic-DynamicScalarTransportFoam.mp4

Same with the standard scalarTransportFoam:

monolithic-ScalarTransportFoam.mp4

Conclusions

From this, I converge to:

• The issue at the outlet must be related to the combination of the volume coupling and the update of the outlet boundary, since it does not appear in the monolithic cases. But the issue is observed on the T, not on the U, which is the one being read. I am confused.
• The integration scheme of T could still be improved, as the monolithic simulation shows discontinuities.