I’m trying to generate a structured mesh for a pipe. I’ve chosen wire discretisation, Quadrangle Mapping and Hexahedron for 1,2 and 3D respectively. I’m able to get a good enough mesh, however when I add Viscous layer hypothesis to size the boundary layer 2 things happen,
If viscous layer thickness is too high then. Then the mesher throws “Unknown Exception” error. It might be because the viscous layers are encroaching the subdomains used for meshing.
If the viscous layer is too small, the volume meshing is successful however it appears to have a discontinuity in the domain as shown. Note that the face meshing is perfect, the 3D mesh is what is messed up.
Hello,
pretty sure that your issue is coming from double nodes, you can check this by going in mesh/controls/node controls/double nodes. if you have, then that’s your problem, and this comes from having double faces in the interfaces of the cylinder. if that’s the case, you can use glue faces in geom to correct the cad
you dont have internal faces, your geometry is a solid, when it should be a compound of solids, where each solid is a block, sharing the corresponding faces.
Correct, and I presume that Salome subdivides the domain into hex meshable volumes automatically, doesn’t it? Thats why I stuck with having a single body.
I was working on subdividing the domain manually right now. If I were to use that on Salome,
Would I need to do something to connect the nodes on the adjacent inner surfaces together? Or would it do automatically - say based on tolerance?
How would I create the groups for inlet, outlet & wall? Salome only lets you create groups of faces of a single body together, doesn’t it? So do I have to create groups with the same names on each of the bodies?
lol, if salome would do that it would solve hex meshing for everything… today you can not achieve a 3D hex mesh, from a 2D quad divided solid it does not exist a solution for this, not in salome nor in other softwares.
you need to divide manually your geometry in 3D not only the surface.
you need to create a solid for each block, then create a compound body of all your solids, and use glue faces to remove the internal double faces. then you can surface groups on it.
check in geome/new entry/blocks/divided cylinder. you will get a body that looks like what you need.
I’ve tried to glue the faces, explode the solids again, assign the group names and tried meshing individual bodies. However, I’m getting the same error, “Unknown Exception”.
each block should have only 6 faces, your blocks have more, for your geometry, it should be 15 blocks in total, 5 for straight section, 5 for the angle, and 5 for the other straight section. like this one Part Studio 2.step (128,5 KB)
I’ve tried to mesh with 15 bodies, with 2 different mesh for the 3 cuboid like bodies in the middle and for the rest. This time the mesh doesn’t fail, however there are double nodes. I’ve rechecked the connection between the faces in geom (repair >> glue faces >> Detect) but there are no faces available for gluing.
your geometry is still wrong. you have some over lapping parts between each block. I don’t know where you draw the CAD model, but it is a cad/geometry related issue. when you use partition over the geometry itself, there are some ‘solids’ that appear that are the internal faces (or at least they look like they might be really thins solids) in any case you are bringing problems from the geometry. the rest is correct.
I used the STEP file that you sent me. I am able to do the meshing if I don’t have viscous layers (both your as well as my STEP file). However if I add a viscous layers the program crashes when I used your file. And when I use mine, it has those disjointed mesh that I’ve shown you earlier. I’m inclined to think that I messed up something while defining the viscous layer.
Here is the study that I have created using your STEP file. Study1.hdf (600.2 KB)
Yep, the geometry works on 9.12. However my geometry (made from freecad) still has double nodes. Can I use the merge nodes function to join these double nodes automatically? After merging, visually it looks like the regions are separated,
However, running checkMesh tool in openFoam only reports one single region. Opening the exported mesh in paraview also shows that the mesh is well connected. So I am inclined to believe that the mesh is good and the merge tool worked.
I’ve also attached the link to the github issue - for anyone following along.
well… yes the merge nodes will work, it is the function, but the thing is, that why solving the result of the issue when you can solve the root of the problem on the geometry? it is like increasing the non ortho correctors in OF when you can improve the orthogonality of the mesh instead… I don’t use freecad, you can create it in shaper quite easily this geometry and will not have this issue for sure. also for sure that you can do it ‘correctly’ in freecad but as mentioned I don’t know too much about it. from what it looks in my tests of your geometry, it looked like the solids overlapped more than the face itself but for a small volume, I would say that this comes from the use of a second sketch that is not equal to the first one or extra lines in the first one…but again, I don’t use freecad I just have experience in cad in general. you can visualize what I am mentioning by partitioning the geometry by itself, and then exploding the geometry into solids, you will see some reaaaally thin volumes
regards
,
