> On 15 May 2020, at 15:04, Hansjoerg Seybold <hansjo...@fisica.ufc.br> wrote: > > 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.
Ok that's normal: currently we only remove duplicate nodes, not elements (cf. https://gitlab.onelab.info/gmsh/gmsh/-/issues/19 for tracking this.) Christophe > > 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><mesh_2.geo><mesh_combined.geo> — Prof. Christophe Geuzaine University of Liege, Electrical Engineering and Computer Science http://www.montefiore.ulg.ac.be/~geuzaine _______________________________________________ gmsh mailing list gmsh@onelab.info http://onelab.info/mailman/listinfo/gmsh