Hello, Thanks a lot for the support. Meshing in two steps and noting the NbNodes and elements (NbTriangles, Nbquads) worked. I get a correct mesh in gmsh and also saving the result is correct. I still have some problems importing the final BDF mesh into ansys fluent (gmsh reads and displays the BDF correctly)
The BDF contains the diagonal edges twice although I use Coherence Mesh. after deleting CBAR 1 ... ... CBAR 16 ... by hand I can read the combined BDF mesh into ansys. I attached all three sample geo files for all three steps (mesh_1.geo, mesh_2.geo and mesh_combined.geo) for reference Thanks a lot again. Cheers, hj On Mon, May 11, 2020 at 5:30 PM Christophe Geuzaine <cgeuza...@uliege.be> wrote: > > > > > On 11 May 2020, at 16:32, Hansjoerg Seybold <hansjo...@fisica.ufc.br> wrote: > > > > Hello, > > Thanks a lot for the reply. Using the visibility filter worked. I > > created a simple test case (attached) > > which creates the two mesh pieces. So now I have two meshes > > multizone_1.msh and multizone_2.msh > > which I can load in a geo file > > -------------------------------------- > > Merge "multizone_1.msh"; > > Merge "multizone_2.msh"; > > Coherence Mesh; > > Save "multizone_merged.msh"; > > Save "multizone_merged.bdf"; > > Exit; > > -------------------------------------- > > I understood that the coherence mesh removes the duplicate nodes on > > the common edge and the above > > script displays the mesh in the gui correctly. > > However the export is distorted as the node ordering is not updated. > > I would get the development snapshot to try to use the mesh tag > > suggestion, but how would I do the reordering > > starting from the script above? > > > > You would do: > > Mesh.FirstNodeTag=1; > Mesh 2; > Save "multizone_1.msh"; > > ... > > Mesh.FirstNodeTag=Mesh.NbNodes + 1; > Mesh 2; > Save "multizone_2.msh"; > > > > regarding openmp: > > > > We (the IT cluster staff at ETH Zurich and myself) tried to get the > > openmp version of gmsh running on the cluster (CentOS 6), but without > > success. > > I managed to compile and run it on my ubuntu PC, but with very little > > speedup for the selected meshing algorithm. > > I tested openmp with two physical groups active and -nt 2, on a finer > > LC as in the attached geo for speed measurements and Mesh.Algorithm = > > 9; gmsh-4.4.1, > > a significant speedup could only be observed for del2d, but quality > > tests showed that the 'pack' algorithm gave the best meshing result > > Ok I see. The "pack" algorithm has not been worked on for a while and is > indeed currently sequential. We are working on updating this algorithm, so > hopefully it will get much faster (and parallel) soon. > > > BTW, is it possible to apply different meshing algorithms to different > > physical groups? > > > > Yes. In .geo files: MeshAlgorithm Surface {...} = ...; > > Christophe > > > > Regarding the 5 days meshing: I am using quad meshing (algo 9) with a > > not too sophisticated sizing function but with a very large domain, > > del2d is orders > > of magnitudes faster. > > > > Thanks a lot for the help. > > > > Hansjoerg > > > > > > > > > > > > > > > > On Sun, May 10, 2020 at 9:05 AM Christophe Geuzaine <cgeuza...@uliege.be> > > wrote: > >> > >> > >> > >>> On 9 May 2020, at 18:09, Hansjoerg Seybold <hansjo...@fisica.ufc.br> > >>> wrote: > >>> > >>> Hello, > >>> I am trying to mesh a model consisting of several physical groups each > >>> group at a time and then merge the meshes for the different physical > >>> groups afterwards. The reason why I am trying to perform this "domain > >>> decomposition" is that the meshing of the full model takes over 5 days > >>> and exceeds the runtime limit of the queuing system. > >>> > >>> However I could not find a simple way to apply the "Mesh 2" to a > >>> specific physical group. Gmsh always tries to mesh the whole model. > >>> > >> > >> You could either delete the parts you don't want to mesh; or hide the > >> parts you don't want to mesh (cf. the `Show` and `Hide` commands in .geo > >> script, or `setVisibility()` in the api) and use the > >> `Mesh.MeshOnlyVisible` option. > >> > >>> My question would be if anybody has a hint how to perform this meshing > >>> in parts and how to combine the resulting meshes into a single final > >>> model. > >>> > >> > >> That's trickier as each mesh will be independent. The development snapshot > >> allows you to set the starting node/element tag (Mesh.FirstNodeTag, > >> Mesh.FirstElementTag), which will help. Removing duplicate nodes when you > >> merge things together can be done with Coherence Mesh (in .geo files) or > >> removeDuplicateNodes() in the api. > >> > >> PS: 5 days to perform a 2D mesh ? Anything special in the geometry/size > >> field? If you don't do this already at least recompile Gmsh with OpenMP > >> enabled, and mesh in parallel? > >> > >> Christophe > >> > >>> Thank you very much. > >>> > >>> Best, > >>> hansjoerg > >>> > >>> _______________________________________________ > >>> gmsh mailing list > >>> gmsh@onelab.info > >>> http://onelab.info/mailman/listinfo/gmsh > >> > >> — > >> Prof. Christophe Geuzaine > >> University of Liege, Electrical Engineering and Computer Science > >> http://www.montefiore.ulg.ac.be/~geuzaine > >> > >> > >> > > <multizone_1.geo>_______________________________________________ > > gmsh mailing list > > gmsh@onelab.info > > http://onelab.info/mailman/listinfo/gmsh > > — > Prof. Christophe Geuzaine > University of Liege, Electrical Engineering and Computer Science > http://www.montefiore.ulg.ac.be/~geuzaine > > >
mesh_1.geo
Description: Binary data
mesh_2.geo
Description: Binary data
mesh_combined.geo
Description: Binary data
_______________________________________________ gmsh mailing list gmsh@onelab.info http://onelab.info/mailman/listinfo/gmsh