[Tobermory]

I am going mad trying to generate a layered mesh at the interface between CHT solid/gas regions using the OF13 ... I have a simple rectangular block of metal surrounded by gas, with a basic hex mesh, (see pic 1, where the metal is the red block) and I just want to add layers at the interface to resolve the gradients in the gas and metal at the surface.

When I try run this in OF13, SHM tells me "No layers to generate ..." (it generates them fine if I only mesh the gas, or only mesh the metal, ie mesh as a single region). The same dictionary (attached) works fine in OF2506 - see picture 2. Note that it's not the naming of the layers (i.e. changing gas_to_metal to Ibeam has no effect - SHM still concludes that there are no layers to generate).

Following advice from earlier posts, I can wangjangle it by: meshing without layers; splitting the regions; meshing the layers in each region by moving the constant/{region}/polyMesh to constant/polyMesh, running SHM, and moving the resulting constant/polyMesh back to constant/{region}. So there's a work-around, but the basic point is that the Foundation version of SHM seems broken. EDIT: actually, thinking about this more, I am not certain that this is a guaranteed workaround ... does it preserve the correct face coupling between the gas and metal regions? I'll need to check
Indeed - it worked on a trivial test case, but failed on a more complex geometry.

Looking at the coding below from snappyLayerDriver.C, I am guessing that the Foundation version views the metal/gas interface as a coupled patch, and therefore assumes no layers are required ... whereas the COM version (which has the same coding below) does not make that assumption and correctly lines up the surface for layer generation. I don't understand why the two make different assumptions about the interface though ...

     label nFacesWithLayers = 0;
     forAll(numLayers, patchi)
     {
         if (numLayers[patchi] > 0)
         {
             const polyPatch& pp = mesh.boundaryMesh()[patchi];
  
             if (!pp.coupled())
             {
                 patchIDs.append(patchi);
                 nFacesWithLayers += mesh.boundaryMesh()[patchi].size();
             }
             else
             {
                 WarningInFunction
                     << "Ignoring layers on coupled patch " << pp.name()
                     << endl;
             }
         }
     }
     patchIDs.shrink();
  
     if (returnReduce(nFacesWithLayers, sumOp<label>()) == 0)
     {
         Info<< nl << "No layers to generate ..." << endl;
     }
     else
     {

Does anyone have any insights before I try logging as a bug?

[Yann]

Hello Tobermory,

I don't really have experience with multiregion meshing in the foundation branch but for what it's worth I remember this commit dating back to OpenFOAM-7 and mentioning layers on coupled interfaces:
https://github.com/OpenFOAM/OpenFOAM...c2d75980212a63

No idea how it evolved in the latest version but I'm dropping it here just in case it could be of any help.

[Tobermory]

Thanks Yann for the reply, but unfortunately that's not it. The output from the Foundation and COM versions is identical (in the layer addition phase) until it gets to the "Checking mesh manifoldness ..." part, at which point the COM version seems to convert the faceZoned faces on the CHT interface to temporary baffles and then continues to generate layers on either side of the baffles, before converting the baffles back to internal faces. The foundation version just says "Nah - there are no layers to add" and skips the layer addition.

I've tried changing the interface to a baffle, but that didn't work. Seems like the foundation version has broken the logic for CHT/internal faces?

I'll drop a bug report, but I usually get a pretty terse reply and so am not hopeful.

[Yann]

Yeah, the .com mechanism is pretty handy for layer addition.

I'd be interested to know if you find a solution, it could be useful to know how to handle it in .org.

[Tobermory]

I have given up for the moment and have just switched to the .com fork for this case ... I tried the following:

1. my suggested work-around above, i.e. mesh without layers, split the regions and then try add layers to each region individually; this worked on a simple test case, but failed in the real (more complex) case. Rats.

2. meshing with blockMesh and SHM in .com (v2506) and then passing that over to .org (v13) for splitting etc., and ofc the two forks are now so wide apart that they disagree on the file format of some of the mesh fundamentals, so that failed too.

I have logged a bug report, so let's see if that gets any attention, but in the meantime my suggestion is to use the .com fork for CHT, since otherwise you cannot add a layered mesh next to your surface (which is rather too restrictive). I'll update if there's any news.

[Tobermory]

Okay - a quick update (thanks to Will at openfoam.org, who gave me a very helpful response to my bug report). The TLDR is that "Putting layers into a face-zone is not supported by Foundation snappyHexMesh" (Will's words) ... in other words you cannot create the SHM mesh including layers all in one step, in the foundation version (unless you want a non-conformal mesh at the interface, which I will assume you don't).

However, Will did give me the correct 3 step approach, which is as follows (see also the multiRegion/CHT/shellAndTubeHeatExchanger tutorial):
1. Run SHM without layer addition, marking the cell zones for the different regions, and the face zones between them. Set the faceZone types to internal.
2. Disconnect the mesh at the faceZones by converting the faceZones to baffles using createBaffles and then running splitBaffles. This generates pairs of mappedWall boundary patches at each faceZone.
3. Run SHM again, with just layer addition this time, to add the layers on the above patches on either side of the faceZone. Ensure you add "mergeFaces false" to the layer definition.

This seems to work very nicely on my test case.

[Yann]

Thanks for your feedback Tobermory!

The workflow is slightly more complex than in the .com branch but it's good to know there is a way to add layers on the whole mesh while preserving a conformal mesh at the interfaces!

Will's answer is great to know how to add layers on both conformal and non conformal interfaces.
If you don't mind I'll leave the link to your bug report here: https://bugs.openfoam.org/view.php?id=4278#c13683