[Gmsh] meshing partitions

Mon May 18 15:26:02 CEST 2020

> On 15 May 2020, at 15:04, Hansjoerg Seybold <hansjoerg at 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 <cgeuzaine at uliege.be> wrote:
>> 
>> 
>> 
>>> On 11 May 2020, at 16:32, Hansjoerg Seybold <hansjoerg at 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 <cgeuzaine at uliege.be> wrote:
>>>> 
>>>> 
>>>> 
>>>>> On 9 May 2020, at 18:09, Hansjoerg Seybold <hansjoerg at 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 at 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 at 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