|
|
|
|
|
|
|
|
Could you try with attached hack of mirrorMesh (mirrorMesh_with_maps)? Or upload a simple ready-made mesh to try it on. |
|
|
|
|
|
Have tried with your mirrorMesh_with_maps, but quits with error: /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 5.x | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 5.x-e4c205229198 Exec : mirrorMesh_with_maps -overwrite Date : Oct 09 2017 Time : 15:13:50 ... I/O : uncollated Case : .../testCase_ofFix nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Mirroring points. Old points: 13179 New points: 25995 Mirroring faces. Old faces: 33368 New faces: 66424 Mirroring patches. Old patches: 6 New patches: 5 Mirroring cells. Old cells: 10152 New cells: 20304 Mirroring cell shapes. Creating new mesh Reading hexRef8 data : cellLevel Reading hexRef8 data : pointLevel Reading hexRef8 data : level0Edge Writing mirrored mesh #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigSegv::sigHandler(int) at ??:? #2 ? in "/lib64/libc.so.6" #3 Foam::mapPolyMesh::mapPolyMesh(Foam::polyMesh const&, int, int, int, Foam::List<int> const&, Foam::List<Foam::objectMap> const&, Foam::List<int> const&, Foam::List<Foam::objectMap> const&, Foam::List<Foam::objectMap> const&, Foam::List<Foam::objectMap> const&, Foam::List<int> const&, Foam::List<Foam::objectMap> const&, Foam::List<Foam::objectMap> const&, Foam::List<Foam::objectMap> const&, Foam::List<Foam::objectMap> const&, Foam::List<int> const&, Foam::List<int> const&, Foam::List<int> const&, Foam::HashSet<int, Foam::Hash<int> > const&, Foam::List<Foam::List<int> > const&, Foam::List<Foam::List<int> > const&, Foam::List<Foam::List<int> > const&, Foam::List<Foam::List<int> > const&, Foam::List<Foam::List<int> > const&, Foam::Field<Foam::Vector<double> > const&, Foam::List<int> const&, Foam::List<int> const&, Foam::autoPtr<Foam::Field<double> > const&) at ??:? #4 ? at ??:? #5 __libc_start_main in "/lib64/libc.so.6" #6 ? at ??:? ./run_mesh: line 14: 47608 Segmentation fault mirrorMesh_with_maps -overwrite => I have used the uploaded case testCase_ofFix.tar.gz. It seems the error occurs after "mMesh.write();" in mirrorMesh.C |
|
|
|
|
|
It was accessing a zero-sized list since I'm creating the minimum mapping construct. Try above version 2. |
|
|
Version 2 generates the refinement files, but in an unexpected behaviour: 1. If the 0 folder exists (with or without any files), neither "mirrorMesh_with_maps" nor "mirrorMesh_with_maps -overwrite" generates the files, just the plain mesh is mirrored 2. If no 0 folder exists, "mirrorMesh_with_maps" results in the same situation as 1. 3. If no 0 folder exists, "mirrorMesh_with_maps -overwrite" generates the refinement files in 0/polyMesh rather than in constant/polyMesh The expected behaviour is: 1. The existence of a 0 folder should not be of importance, existing files should be overridden 2. "mirrorMesh_with_maps" should generate the refinement files in 0/polyMesh 3. "mirrorMesh_with_maps -overwrite" should generate the refinement files in constant/polyMesh |
|
|
This version (check size, should be 11925 bytes) writes correctly - with or without -overwrite - with or without 0 |
|
|
Files are written properly now, but the pointLevel is somehow messed up. If I start "pimpleDyMFoam" with "mirrorMesh_with_maps-3", the following error occurs: Create time Create mesh for time = 0 Selecting dynamicFvMesh dynamicRefineFvMesh --> FOAM FATAL ERROR: PointLevel is not consistent across coupled patches. point:25567 coord:(6.4 0.0939279 0) has level 1 whereas the coupled point has level 0 From function void Foam::hexRef8::checkRefinementLevels(Foam::label, const labelList&) const in file polyTopoChange/polyTopoChange/hexRef8/hexRef8.C at line 4923. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::error::abort() at ??:? #2 Foam::hexRef8::checkRefinementLevels(int, Foam::List<int> const&) const at ??:? #3 Foam::hexRef8::hexRef8(Foam::polyMesh const&, bool) at ??:? #4 Foam::dynamicRefineFvMesh::dynamicRefineFvMesh(Foam::IOobject const&) at ??:? #5 Foam::dynamicFvMesh::addIOobjectConstructorToTable<Foam::dynamicRefineFvMesh>::New(Foam::IOobject const&) at ??:? #6 Foam::dynamicFvMesh::New(Foam::IOobject const&) at ??:? #7 ? at ??:? #8 __libc_start_main in "/lib64/libc.so.6" #9 ? at ??:? Aborted I added a picture of the issue => "issue_pointLevel.png". It seems "mirrorMesh_with_maps-3" mirrors the pointLevel and then sets all old pointLevels to zero. With cellLevel everything seems to be correct. issue_pointLevel.png (78,721 bytes) |
|
|
Edit to picture "issue_pointLevel.png": Shown are inlet (left) and outlet (right) patches of the mirrored mesh. The top picture is the mesh produced with "mirrorMesh_with_maps-3" and the bottom is the one produced with "tfd_mirrorMesh", which mirrors "pointLevel" equal to "points". |
|
|
|
|
|
Would it be possible to test with the uploaded new mirrorMesh_with_maps_20171020.tgz? It was missing the map for the original points (so that is why you were seeing 0 level). |
|
|
The cell level and point level are being mirrored properly now. I am going to test the tool for more sophisticated test cases. There may some additional issues show up. In that case, I will open a new issue. For now I would mark the subject as solved |
|
|
Resolved in OpenFOAM-5.x by commit 28fdc3c4e851fd0f036676385592239f021da83f Resolved in OpenFOAM-dev by commit 19da21ed93703f2d94c3dacf81f85e076aaa86fc |
- Anonymous
