> On 28 Aug 2016, at 13:57, andrew <armit...@gmail.com> wrote:
>
> Hi,
>
> Thank you for your response.
>
> I have tried the suggestion you made but this way I don't get the internal
> surfaces which I need. The surface mesh is constructed correctly but as you
> can see from the first image I don't have the internal regions. I do get the
> points but openfoam does not understand them no matter what I do. In the
> second image is the mesh that I want with the internal surfaces.
>
> In the third image is a mesh I get with the loops but without the 'Line In
> Surface' set of commands where you can see that I get a bad mesh near the
> narrow areas where the mesh crosses the boundaries of the loop lines. I would
> expect that since I construct the surface with the loops, even if they were
> of zero width, they would be embedded in the surface since its creation
> making the need for the 'Line In Surface' commands obsolete.
>
I see; indeed this is a valid approach.
I have recoded the "Coherence Mesh;" function to make it much faster. Could you
download the next build and give it a try?
Thanks for the detailed feedback,
Christophe
> Anyway I found a workaround but it involves the Salome mesh generator.
>
> In the first step I create the mesh in Gmsh without the coherence function. I
> save it in unv format. I reload it in Salome and I remove the duplicate nodes
> there with 'merge nodes'. I delete the 'vol' since I don't need it and I save
> the mesh with only the surfaces I need again in unv format.
>
> It sounds cybersome but all these are done by scripts and Salome needs a few
> minutes to load a 3+ million cells mesh and save it back and less than a
> minute to remove the duplicates. Gmsh needs a few minutes for the mesh and
> 2+hrs for the removal so the procedure through Salome is way faster.
>
> Salome is written in python which is no faster than C++ so I guess the
> coherence routine in gmsh could take a refinement to a faster way.
>
> Kind regards
>
> Andrew Tsiantis
>
>
> 2016-08-28 12:10 GMT+03:00 Christophe Geuzaine <cgeuza...@ulg.ac.be>:
>
> Andrew,
>
> The problem actually seems to come from the way you define the surface: can
> you regenerate your geometry script after
>
> - removing all the zero-area line loops (e.g. "Line Loop(6) = {5, -5};")
> - removing these loops from the definition of the main surface (i.e. simply
> have "Plane Surface(1) = {205};")
>
> With this you should not have duplicate vertices anymore, which should make
> "Coherence Mesh" unnecessary.
>
> Let us know,
>
> Christophe
>
>
> > On 21 Aug 2016, at 17:33, andrew <armit...@gmail.com> wrote:
> >
> > hi,
> >
> > Thank you for the response. The file I submitted was a small one and the
> > problem was not so obvious. I am attaching a 'real' file that I use on my
> > simulations. It has 3000 cuts in it. This takes 2 hours on a quad core and
> > 1+ hour on a i7 @4ghz. I am using the version 2.13.1.
> >
> > Kind regards
> >
> > Andrew Tsiantis
> >
> >
> > 2016-08-21 17:50 GMT+03:00 Christophe Geuzaine <cgeuza...@ulg.ac.be>:
> >
> > > On 19 Aug 2016, at 21:34, andrew <armit...@gmail.com> wrote:
> > >
> > > Hi,
> > >
> > > I try to create a 3d mesh from an extruded 2d mesh. The mesh is a simple
> > > box but with cuts in it of zero width. The geometry is created ok and the
> > > meshing even when I have 2000-3000 cuts is done in less than a few
> > > minutes. However when I convert the mesh for use with openfoam I was
> > > getting errors. By adding the command 'Coherence mesh;' after the
> > > creation of the mesh, the mesh is converted correctly for use with
> > > openfoam by using the ultility 'gmshToFoam'.
> >
> > Indeed, it's a limitation of our extrusion algorithm with embedded curves
> > ("Line In Surface"): it currently creates duplicate vertices. The real fix
> > is thus for us to enhance extrusion of embedded curves, but it's not
> > trivial due to the way extruded meshes are generated.
> >
> > > The problem is in the use of the 'Coherence Mesh'. It takes almost two
> > > hours to execute while the meshing takes a few minutes. Is there a way to
> > > improve the Coherence command or to make the same geometry without the
> > > duplicate nodes that need so much time to be removed?
> > >
> > > I attached a file that needs 2.5 minutes on a quad core for meshing and
> > > more than ten minutes to remove 1600 duplicates.
> > > I have to create thousands of these meshes so a speedup would be welcomed.
> > >
> >
> > That seems a bit slow: on my laptop meshing and duplicate removal take
> > about the same time (2 minutes each). Which version of Gmsh do you use?
> >
> > > kind regards
> > >
> > > Andrew tsiantis
> > >
> > > <se.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
> >
> > Tetrahedron V, July 4-5 2016: http://tetrahedron.montefiore.ulg.ac.be
> > Free software: http://gmsh.info | http://getdp.info | http://onelab.info
> >
> >
> > <3k_cuts.zip>_______________________________________________
> > 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
>
> Free software: http://gmsh.info | http://getdp.info | http://onelab.info
>
>
> <gmsh-1.jpg><gmsh-2.jpg><gmsh-3.jpg><se.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
Free software: http://gmsh.info | http://getdp.info | http://onelab.info
_______________________________________________
gmsh mailing list
gmsh@onelab.info
http://onelab.info/mailman/listinfo/gmsh
