Export/import issues format Salome/gmsh/OpenFOAM [solved]

1

Hello,
I am trying to import my meshes generated in salome to OpenFOAM.
the meshes have different type of cells (including pyramids, so I can not use the UNV format), therefore I try to export the mesh generated in salome to gmsh, and from gmsh export it to OpenFOAM. Nevertheless, I have not successfully got a ‘working’ mesh.
I have tried different possible exporting formats from salome to then import them into gmsh:
med 4.1, 4.0, 3.3, 3.2
CGNS (wich gave an error in gmsh 4.11.1)
GMF ASCII, binary (binary gave an error in gmsh 4.11.1)
when I import it to gmsh I don’t get any error message (with exception of the CGNS and GMF binary. then I export from there into .msh version 4.1 and then import it into OpenFOAM using gmshToFoam. this “works” but when I look at the mesh in paraview it is wrongly connected. It might be a stretch but depending in the format I exported in salome, I get different results in the end that’s why I am publishing here among the gmsh bug issues (not sure if the issue comes from the writing or reading this formats)
gmshBugReport
any insight in this issue or how to solve it would be appreciated

Edit:
the correct workflow for importing a med file to Openfoam (in case that anyone finds with similar issue) would be: In Salome

  1. Create the 2D groups for patches and at least one 3D group that contains all the cells, also it is important to delete all 1D groups (not sure if the 0D also) of the mesh, so only have surface and volumetric groups.
  2. Export it in med file format, from my tests whatever version is ok
  3. Import the mesh in gmsh by open/select the med file
  4. Go to file export
  5. Export it using following parameters ASCII 2.1 format, and all options set to off
  6. Use gmshToFoam without any flag. This will allow to conturnate the issue of not being able to export directly meshes with pyramids from Salome in a format that is importable to openfoam
1 Like
2

Hi franco.ota, thank you for the workflow reported. It also worked for me using SALOME 9.14, OpenFOAM 13 and Gmsh 4.12.

To follow your workflow I needed, previously, to add MED support to Gmesh as follows (done by IA, with corrections):

Update & install build deps (first block installs MED & HDF5 dev packages)
sudo apt update
sudo apt install -y build-essential cmake git pkg-config
libmed-dev libmedc-dev libmed11 libhdf5-dev
libx11-dev libxext-dev libgl1-mesa-dev

(Optional extras you may need for full Gmsh features)
sudo apt install -y libglu1-mesa-dev libfltk1.3-dev libjpeg-dev libpng-dev

2) Download Gmsh 4.12 source (pick 4.12.2 or 4.12.1 if you prefer)
cd /tmp
wget https://gmsh.info/src/gmsh-4.12.2-source.tgz
tar xzf gmsh-4.12.2-source.tgz
cd gmsh-4.12.2-source

3) Create build dir and run CMake enabling MED
mkdir build && cd build

Try a normal configure first — MED is an optional CMake option named “MED”
cmake .. -DMED=ON

4) Build & install
make -j$(nproc)
sudo make install

After it finishes, test MED support with:
gmsh -help | grep med

P.S.: In my case, I created a mesh in SALOME 9.14 that included pyramids. I then used the “Split Volumes” tool to split these pyramids into tetrahedra for export as a .unv file. Unfortunately, this splitting process causes ideasUnvToFoam to create a defaultPatch in OpenFOAM (which is not visible in SALOME) at the locations where the pyramids were split. In my case, the pyramids were formed at the interface between the hexahedral and tetrahedral cells.**