Hi together !
I took notice of the revolve element command recently. Former, I tried to mesh my whole axisymmetrical body and applied load to the polygon edges/faces. A mesh of higher quality can be done with the revolve element command.
Unfortunately I have got two problems there and I would really like to ask you if you know a solution for that
First: When revolving the elements, I can't apply forces/loads to polygon edges anymore and so I've got to select all element edges/nodes etc. This is very unfortunate for later applications. The polygon edges are derived from the polygon bodies I think, and I can associate the mesh with the polygon body to have these edges. But that has to be done manually after the geometry part has changed.
Second: The "Revolved mesh" is not editable nor does it update if the original 1-D or 2-D mesh is updated (if the geometrical origin (sketch/face) is updated). Is an update of the revolved mesh simply impossible or am I too dumb to find a solution?
Thank you very much!
All of the mesh-based commands (i.e. pretty much everything on the "Nodes and Elements" ribbon tab) will not update when your geometry changes. Even if you associate your mesh back to the geometry, there is no geometry-based "recipe" for its creation, so it cannot update.
If your geometry is such that you can produce a suitable mesh by revolving elements, then I would expect you should be able to produce a similar result by using a 3D Swept Mesh, and this will be associated to your polygon geometry for future updates. Is there some reason why this doesn't work for you?
thank you for your quick response.
Ive got two setups for my model: Shell and Solid.
The shell body depicts problems anyway because the CAD environment is not able to combine more than 3 faces on one edge(connections similar to T-joints). Only stitchting is achieving the desired result but unfortunately, this method is not convincing utterly. The stitch edge command can't stitch edges which are closed (circumferential edges). I would have to split up the edges, stitch them, merge them afterwards. For the first model it is OK, but this does not necessarily depict an automatable stable solution. The meshes which are created when updated are OK but I would like to have more stable and consistent meshes in the Sheet setup.
For this reason, I tried to export the CAD sketch of the shell to the FEM environment and to revolve 1-D elements lying upon this sketch. But as you said, updating this template_FEM file is not really possible.
I already tried to split my solid body, 2D mesh the cross-section and 3D sweep the solid body. This works fine, but I don't know how to do that with a complete 360° solid body because there will be no cross section to 2D Mesh.
Do you know a solution for that?
I would be really really grateful
1. Split your solid body with a plane on the axis (e.g. use Split Body in the Idealized Part) so you have two 180 degree sections
2. In the FEM, create Mesh Mating Conditions on the two pairs of mating faces
3. Apply your 2D source mesh to one of the 2D faces
4. Apply 3D Swept Mesh (Multi-body infer target) to both of the solid bodies using the 2D mesh as the source
This should create a continuous 360 degree mesh which will update with geometry changes.
Although I was not able to create Mesh mating conditions between the two pairing faces. Either this was because the "View section" does not allow me to select 2 faces or because I already activated the "Create mesh mating conditions" in the split body dialog.
Do you perhaps know also a solution for my sheet body problem?
I'm not sure I understand the problem with the shell case. There is no 2D equivalent to the 3D Swept Mesh command, so you will always need to use a 2D surface mesh of some sort. Are you saying this doesn't give you a satisfactory mesh, so you need to split the surfaces?
For the creation of my template.fem, the geometry is derived from the idealized part.
Then I am stitching the edges to get one unique sheet body. The stitchting command, however, splits the circumferential edges. This leads to a very undesirable mesh.
Ergo, I am merging the edges afterwards, adding mesh controls (e.g. 50 elements on edge) to all circumferential edges and 2D mesh it. Then the mesh looks perfect. When I am changing geometrical dimensions of the underlying part, the FEM recognises the changes and automatically splits up the edges (which have been stitched and merged before) into two parts again. This can also be seen on the fact that the Mesh control on one edge is divided nto two mesh controls on the same but split edge (fortunately, NX tries to halve to amount of elements, but in many cases this is not exact. (instead of 25 numbers on one part of the edge and 25 on the other, 24-26 is applied). This distorts /rotates the mesh a little bit around the axis. For rough estimations the mesh is OK, but i don't know if there's a more sophisticated solution to this.
Is the problem now clearer to you? I try to take some pictures if not
I think I understand.
I would tend to avoid having 360 circumferential edges in the first place, then they shouldn't get split when you stitch. So if I was dealing with a simple cylinder, I would split it into two 180 degree segments in the Idealized Part (much the same as the solid example). This gives me two nice mappable 2D surfaces, and the mating edges should stitch in the FEM.
Thank you for your effort.
I've tried the approach with using two split bodies in the FEM already before but I was not able to get a nice mesh on it somehow. After you have suggested this here, I gave it another try and well..now the mesh looks superb and I am really really happy with it so far.
Unfortunately, I realized that the Mesh mating conditions didnt work when I have been running my first test case. I am not able to apply mesh mating conditions to the sheets somehow. What am I doing wrong? How can I apply mesh mating conditions onto my sheet bodies? Is this not possible? The mesh mating conditions function states "connects two seperate solid bodies ..."
Okay, I overread somehow that you don't use MMC but stitching. I will try that now