Import to OpenFoam / patch creation fails
COmputational fluid dyNamics STRUctured grid CreaTor for 2D airfoils
Brought to you by:
montagdp
Menu
▾
▴
Hello,
I've created a number of O-meshes for the DU91-W2-250 and the NACA0012 airfoil (the one provided as an example) which I want to use in OpenFoam. Mesh creation works, plot3dToFoam fails so I opened them in GMSH, clicked on "create mesh" to convert the file format to GMSH format, gmshToFoam works, checkMesh is happy, now it's time to create the boundary patches: autoPatch -overwrite 59 (or other angles < 90°) always create 6 instead of the expected 4 (airfoil, front, back, farfield) boundary patches. (angles > 90° result in just one patch). The other two patches are strips (very close together) of faces which connect the trailing edge with the farfield. A check in Engrid identifies "overlapping cells" in that area.
How can I use a mesh created with construct2d in OpenFoam? (All the meshes I created are well within the parameters described in the manual which should be ok)
T.
here is the fix:
1: open mesh.p3d file in GMSH and click save mesh, then close GMSH
2: import mesh.msh file into OpenFoam: gmshToFoam mesh.msh (in an OF case directory)
3: autoPatch -overwrite 69
4: stitchMesh -overwrite auto0 auto5
5: open boundary file, remove patches with size 0, rename patches
point 4 reintegrates two patches usually connecting the trailing edge with the farfield boundray of the o-mesh which is a technical issue typical for o-meshes.