|January 11, 2011, 07:17||
What's the correct unstructured mesh procedure
Join Date: Nov 2010
Posts: 125Rep Power: 7
I'm quite new to ICEM. I was wondering about the correct unstructured mesh procedure. I have a problem in this regard. Once I set curve nodes parameters and mesh the face everything looks neat. However when I use volume mesh and tick the use existing mesh option, the generated mesh looks distored and not orderly at all. What am I doing wrong? What's the right way to generate a mesh using an existing surface mesh. Thanks in advance.
|January 11, 2011, 11:28||
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 468Rep Power: 14
The way I make unstructured meshes in ICEM is after setting all the part, surface, density, curve sizings etc:
1. Make an octree mesh and delete the volume elements. Check and smooth the surface elements until they are a high quality.
2. Run Delaunay (with TGlib and AF) from the existing surface mesh. Check and smooth as mentioned above.
3. Run prism mesh. Check and smooth (careful with smoothing with PENTA_5 active though).
4. Export mesh to solver.
|January 12, 2011, 18:42||
Retired from CFD Online
Join Date: Mar 2009
Location: Ann Arbor, MI
Blog Entries: 1Rep Power: 38
The "Use existing mesh" option actually uses the "make consistent" command to make the octree volume mesh consistent with the previous surface mesh.
You would use that option if you had certain faces that you needed meshed in a certain way (such as fillets), perhaps to match up with another part or for some other reason.
Many users just go straight to Octree Tetra (as SIW suggested) and use the top down method. This approach first subdivides the volume and then fits to the surface to produce the surface mesh. It is very robust, patch independent and can walk over lots of problems (like a shrinkwrap). However, some people are looking for more patch aligned mesh.
If you want to start with a surface mesh, you could just use one of the other Tetra methods (such as Delaunay or Advancing Front Tetra). These start at the surface mesh boundary and fill the volume. They are faster than Octree mesh, and given a good surface mesh, will produce a better volume mesh.
You should only use the option to "Use existing Mesh" option if you want your model mostly patch independent but also have some parts with existing mesh. I don't know why it didn't work in your case. I would guess the problem was the selected part names, you must select the part names of the mesh you wish too keep.
|Thread||Thread Starter||Forum||Replies||Last Post|
|2D unstructured mesh||majidhojjat||OpenFOAM Meshing & Mesh Conversion||1||May 14, 2009 17:09|
|Structured and Unstructured mesh||Jingwei||FLUENT||0||March 2, 2009 22:29|
|Problem with solving for unstructured mesh||evgenii||OpenFOAM Running, Solving & CFD||5||November 27, 2006 05:37|
|Unstructured hex mesh||lr103476||OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...||12||November 24, 2006 06:56|
|2D Modelling using unstructured mesh||Yingchun||CFX||8||December 12, 2005 07:05|