CFD Online Logo CFD Online URL
Home > Forums > ANSYS Meshing & Geometry

What's the correct unstructured mesh procedure

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Display Modes
Old   January 11, 2011, 07:17
Default What's the correct unstructured mesh procedure
Senior Member
Join Date: Nov 2010
Posts: 126
Rep Power: 8
Nick R is on a distinguished road

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.
Nick R is offline   Reply With Quote

Old   January 11, 2011, 11:28
Senior Member
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 521
Rep Power: 16
siw will become famous soon enough
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.
siw is offline   Reply With Quote

Old   January 12, 2011, 18:42
Retired from CFD Online
PSYMN's Avatar
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,665
Blog Entries: 1
Rep Power: 39
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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.
PSYMN is offline   Reply With Quote

Old   January 12, 2011, 19:40
Senior Member
Join Date: Nov 2010
Posts: 126
Rep Power: 8
Nick R is on a distinguished road
Thanks guys. You rock. I'll try your suggestions and get back to you if I have questions.
Nick R is offline   Reply With Quote


Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On

Similar Threads
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

All times are GMT -4. The time now is 15:46.