CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] how to realize smooth transition of volume mesh?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 11, 2009, 00:05
Thumbs down how to realize smooth transition of volume mesh?
  #1
New Member
 
Bo Yang
Join Date: Dec 2009
Posts: 3
Rep Power: 7
yangboMAE is on a distinguished road
Firstly, I generated the volume mesh around a car using the Octree method. Then, I tried to re-generate the mesh using Delaunay method based on existing mesh. But I noticed that the volume mesh sizes around the car were still increased very quickly (not smoothly) in space. So could we generate smooth changing mesh using Delaunay method based on the mesh generated using Octree method in ICEM-CFD? And if we could, how to do that?
Thanks indeed.
yangboMAE is offline   Reply With Quote

Old   December 11, 2009, 15:32
Default
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Delaunay is a more sudden transition than the advancing front method (it started life as an FEA algorithm, where as the advancing front algorithm started life at GE specifically designed for fluids). Personally, I find that method to be too slow to generate.

I prefer the Delaunay method in 12.1 with the TGlib and AF options...

I made a post recently where I showed images of these various methods for comparison.
PSYMN is offline   Reply With Quote

Old   December 11, 2009, 16:02
Default Thank you. Could you please illustrate in detail?
  #3
New Member
 
Bo Yang
Join Date: Dec 2009
Posts: 3
Rep Power: 7
yangboMAE is on a distinguished road
hi Simon,

Could you please illustrate it in detail? or could you paste the link of your post for me?

Maybe the original Octree volume mesh is not smooth enough for Fluent solution, I guess. So I would like to use Delaunay based on the existing Octree mesh. But I don't find options about how to control the tetra mesh size increasing rate.

What do you recommend? By the way, I am using the ICEM-CFD 12.0.1.
Thanks indeed.
yangboMAE is offline   Reply With Quote

Old   December 11, 2009, 16:16
Default
  #4
Super Moderator
 
Ryne Whitehill
Join Date: Aug 2009
Posts: 313
Rep Power: 9
rwryne is on a distinguished road
Quote:
Originally Posted by yangboMAE View Post
hi Simon,

Could you please illustrate it in detail? or could you paste the link of your post for me?

Maybe the original Octree volume mesh is not smooth enough for Fluent solution, I guess. So I would like to use Delaunay based on the existing Octree mesh. But I don't find options about how to control the tetra mesh size increasing rate.

What do you recommend? By the way, I am using the ICEM-CFD 12.0.1.
Thanks indeed.
domain interface in ICEM for fluent
rwryne is offline   Reply With Quote

Old   December 11, 2009, 22:27
Default
  #5
New Member
 
Bo Yang
Join Date: Dec 2009
Posts: 3
Rep Power: 7
yangboMAE is on a distinguished road
domain interface?
what does it mean?
Now I set up some density regions around and in the wake of the car to obtain refined Octree volume mesh firstly. Then, re-generate Delaunay volume mesh on the existing Octree volume mesh. It seems better. But I think the volume mesh transition is still not smooth enough. Because the car is a blunt body near road. And tyres contact road. So the Delaunay volume mesh depends on the surface mesh on the road, I think.
Simon, how could we obtain smooth transition surface mesh on the road (or the floor of wind tunnel)??
Thanks indeed.
yangboMAE is offline   Reply With Quote

Old   December 14, 2009, 13:45
Default
  #6
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
You could use some options in the Part Mesh Setup menu such as Tetra Size Ratio and Tetra Width (look at the user manual to explain how it works).
BrolY is offline   Reply With Quote

Old   December 15, 2009, 20:24
Default Tips for smoother tetra mesh
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You are right in that these bottom up tetra methods are very dependent on the surface mesh. So you should always smooth the surface mesh with the Laplace algorithm before running Delaunay. This algorithm is particularly good at smoothing transitions.



Of course there is also the “Spacing scaling factor” to roughly control the expansion with the Delaunay method. (Width and Tetra Size Ratio are for Octree and don’t yet work with Delaunay (but may at 13.0 )). For Advancing front, you can set the Expansion Factor to control the rate of expansion. There is a similar Expansion Factor for the TGrid method, but I think the TGLib AF method uses the Spacing Scaling factor (I will have to test to confirm).

Another tip would be to "nest" density regions. You can put a size 1 right behind the vehicle, then a larger density box with size 1.5 would extended beyond that one up and down stream, outside of that, you could put another density box with size 2, etc. (the smaller size density box is nested within the larger). Then when you run Delaunay (or Delaunay with TGlib AF) it will respect these and slow down even further.



The final suggestion is to use the Laplace Volume smoother now available in 12.1.
PSYMN is offline   Reply With Quote

Reply

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
[ICEM] negative mesh volume problem (icem-cfd/cfx) adam2008 ANSYS Meshing & Geometry 5 April 16, 2010 12:21
[TGrid] Tgrid hybrid mesh pyramid transition tony00 ANSYS Meshing & Geometry 4 November 26, 2009 05:36
On the damBreak4phaseFine cases paean OpenFOAM Running, Solving & CFD 0 November 14, 2008 22:14
Interpolating volume data onto quad surface mesh N.R. CFX 6 June 7, 2007 08:15
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 12:27.