Hello! I have created my mesh in .med format and uploading it fails. I got an internal-error message (Error Id: 2c22a49a).
Mesh does have groups of faces and volumes and it is saved in 3.3 version.
Here is the link to my mesh file: https://drive.google.com/file/d/1Qd0UVQkqQijMQFUEurflGtigEi4NX9bG/view?usp=sharing
Hi, thanks for posting!
Having a look at the mesh, I can see a group of volumes, but I cannot see groups for the faces (which is necessary when uploading .med meshes):
Could you double check on your side?
PS: are you using Salome or a different tool to generate the mesh?
Cheers
I do have groups of faces, maybe the file I uploaded on Google Drive was old.
Could you refresh it from this link: https://drive.google.com/file/d/1Qd0UVQkqQijMQFUEurflGtigEi4NX9bG/view?usp=sharing ?
Yes, I use Salome.
To add here, you need to add one face group for each face of the model, so as many face groups as faces in the geometry, even if you are not going to assign them to boundary conditions. Same applies for volumes.
Thanks! It is interesting.
I made groups for all external faces of the model, but there are more than one face in one of the groups. To simplify, if model was a box there would be Group 1 for one face, Group 2 for second face and Group 3 for the rest of the faces. Is it possible to do it this way?
Speaking of volumes, there is one volume in my geometry and all the volumetric elements belong to one group.
I’m also a bit suspicious of the detailed topology on the bottom of the “walls” face group:
We have some weird patterns - looks like multiple cells are stacked?
It is possible because of the complexity of this surface in Geometry. Let me try to fix it. So it means that if mesh has some irregularities or faults it wouldn’t even be uploaded?
Very likely. And it definitely would not run a simulation successfully with overlapping cells.
On a side note: is there a particular reason for not meshing the geometry in SimScale?
My main aim was to succeed in uploading .med file, before I start to work with simulation. So, continuing the discussion of the uploading problem: I made a coarse mesh based on same geometry and, as far as I can see, with no overlapping cells. Could you please check this one https://drive.google.com/file/d/1SHN8q2MgjpxtLlG1cAW0iuKuj-gY-ept/view?usp=sharing?
As I said, the geometry is complicated and it didn’t work for me to mesh it in SimScale. I’m not familiar with built-in meshing tool of SimScale and it seemed easier for me to mesh geometry by Salome. I could share the SimScale project with my uploaded geometry and maybe you can give me a hint what is possible to do to get a proper mesh.
I still think there is something weird with the groups. If I try to create the groups on my side, the geometry gets super weird.
I’m trying to select some faces, but a face far away from the mouse pointer gets selected. Perhaps I can share the way how I usually create groups, to see if it helps?
Usually I start by creating groups for the geometry, and not for the mesh:
Nothing fancy here - I just created one “inlet”, one “outlet”, “side_walls” and one group for the volume.
Then I will mesh the geometry and create groups from Geometry:
So you just click on the groups you created on the geometry (one by one) and apply:
This will give you the groups for the mesh automatically. Then it’s just a matter of saving the mesh in the 3.2 or 3.3 versions and importing:
In short, I still think there is something weird with the groups. The way that I described above is more consistent.
Speaking of my geometry, I created groups in a similar way, but using filter “Belong to Geom”. For Inlet and Outlet I used side faces of my geometry and for the Wall I made a logical filter "NOT Belong to Geom AND NOT Belong to Geom " (to choose everything on external borders but Inlet and Outlet) because of the same reason - geometry on the bottom is complicated and mesh is an approximation of this geometry thus face elements could not be chosen by geometrical border.
I tried your tutorial just to check of the simpliest geometry works and it worked - I uploaded simple box with mesh. So it means that the problem is in the complexity of my geometry.
Is it possible that SimScale does not support polygons and polyhedrons among mesh elements?
By the way, have you tried to check Mesh_3 which I uploaded in my last message?
Hey, yes I did have a look at mesh_3 (which was quite simple). This was the mesh that I was trying to manually re-create the contacts using the mesh, but failed to do so, as the group selection looked a bit buggy.
Polyhedron are supported - there’s actually a log showing the element types once you run a hex-dominant mesh in the platform
As a FYI, I also tried one alternative workflow for taking mesh_3 into SimScale. Basically saving it as a UNV mesh and converting it to the foam format using OpenFOAM’s ideasUnvToFoam utility.
It was the same error message discussed in this thread. This also points to issues with mesh groups.
Quick update:
I’ve corrected mesh_3 - splitted hexahedra and polyhedra to tetrahedra and it worked! So maybe hexa- and polyhedra are not the best choice particularly for importing mesh.
Hello! I cleaned my geometry on the bottom - excluded weird angles and overlapping surfaces, and I tried to mesh it with standard SimScale Mesh tool (Hex-dominant parametric option).
It worked for the curved bottom surface without holes (can provide a link to that project too), but when it comes to small extra volumes which cut the volume on the bottom, the algorithm fails. I tried to work with surface and region refinements, but it seems that I do something wrong. Could you please take a look at my geometry and mesh parameters and maybe give me any hint what could be done to mesh this complex volume?
Here is the link to my project: SimScale
Hi! I see what you are trying to do, but I’m afraid that this level of geometry complexity is too much for the community plan.
This kind of simulation (specially with a complex terrain) is more fitting for PWC/Incompressible LBM (e.g. this project 1).
Both of these solvers are only available on-demand, so they require a subscription.
Cheers
Do these solvers provide other meshing algorithms?
Both LBM and PWC use their own meshing algorithm - the meshes consist exclusively of hex cells (it’s basically a perfect, 100% orthogonal mesh). The algorithms are also quite tolerant with not-100%-clean CAD models, which is a plus.
If you follow the steps in this article, you will get an idea of the resulting mesh in PWC simulations (e.g. this project)
This one from the image above has around 60M cells 
Cheers
