Fluent3DMeshToFoam
Convert a mesh generated by Fluent/Gambit to OpenFOAM.
1. Save the file in Fluent/Gambit in ASCII format (uncheck the "Write Binary Files" option)
2. Create a new case (e.g. Beispiel) for OpenFOAM (easy option: copy the following files from a comparable tutorial, e.g. icoFoam)
a. Create case directory: mkdir Beispiel b. Create the following directories inside Beispiel folder (or copy from the icoFoam tutorial) mkdir Beispiel/system mkdir Beispiel/constant mkdir Beispiel/constant/polymesh mkdir Beispiel/0 c. Create the following files: (or copy from icoFoam tutorial) Beispiel/system/controlDict Beispiel/system/fvScheme Beispiel/system/fvSolution Beispiel/constant/transportProperties
3. Copy the fluent.msh file into Beispiel folder.
4. Run the fluent3DMeshtoFoam converter (within the Beispiel folder)
without scaling: fluent3DMeshtoFoam fluent.msh OR with appropriate scaling if required (e.g. from meters to millimeters): fluent3DMeshtoFoam fluent.msh -scale 0.001
4. Edit the Beispiel/constant/polyMesh/boundary file and set proper names. Typically every surface might be a wall. If one needs inlet, outlet, etc as boundary condition, change wall to patch.
5. Run checkMesh(from Beispiel root folder) to check if the mesh has been converted properly.
checkMesh OR checkMesh -allTopology -allGeometry
6. Copy the initial/boundary condition files into Beispiel/0 folder and edit them appropriately.
e.g. Beispiel/0/U and Beispiel/0/p from icoFoam tutorial.
7. Make further appropriate changes (e.g. nu in Beispiel/constant/transportProperties )
8. The case is ready to run (from Beispiel root folder):
icoFoam or foamJob icoFoam