CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

mesh quality measurement

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 31, 2009, 21:05
Default mesh quality measurement
  #1
New Member
 
Khosrow
Join Date: Aug 2009
Posts: 2
Rep Power: 0
khosrow1355 is on a distinguished road
Hello everybody,

As you know one of the parameters for measuring mesh quality is aspect ratio. I would be appreciated if any body can help me to know what is the optimum range for this parameter to have an appropriate quality for generated grid?
khosrow1355 is offline   Reply With Quote

Old   September 6, 2009, 17:23
Default
  #2
Senior Member
 
John Chawner
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 223
Rep Power: 9
jchawner is on a distinguished road
Hello khosrow.

There are no universal guidelines for mesh cell aspect ratio. In fact, a pessimist might say that the only universal guideline for mesh quality is positive volume.

Acceptable (forget optimum) aspect ratio will depend on your solver. If you're using a commercial CFD code, contact their tech support engineers and I'm certain they'll be able to provide you with recommendations.

But acceptable aspect ratio also depends on cell type. For example, a highly stretch quad with an aspect ratio of 100 could very well be acceptable. A triangle with an aspect ratio of 100 could be horrible or good (depending on the included angles).

Acceptability also depends on what you're trying to compute. For example, you might be able to get away with poor grid quality if you're only interested in wall pressure. But if you're trying to compute heat transfer or boundary layer transition, the same grid may fail miserably.

Finally, it depends on where the cell is. A crappy cell out in the farfield can be tolerated while one in the boundary layer probably can't be.

Sorry this isn't a very good answer.
__________________
John Chawner / jrc@pointwise.com / www.pointwise.com
Blog: http://blog.pointwise.com/
on Twitter: @jchawner
jchawner is offline   Reply With Quote

Old   September 7, 2009, 02:22
Default
  #3
New Member
 
Ertan Karaismail
Join Date: Apr 2009
Posts: 17
Rep Power: 8
ertan is on a distinguished road
I guess, fluent recommends a max aspect ratio of 5. However, sometimes it becomes very hard to satisfy this requirement. I generally try to keep it less than 15. It results in acceptable meshes for me. However, I totally agree with the previous reply. And as another point, that might be important, is that, different turbulence models (i.e. equations) have different mesh quality requirements. Especially, if you will use RSM, you should know that it is extremely sensitive to the mesh quality. It may not converge with the meshes acceptable for other model. There fore if you are gonna use RSM, you need to keep the mesh quality as high as you can, meaning that use of a low aspact ratio.
ertan is offline   Reply With Quote

Old   September 7, 2009, 11:09
Default
  #4
Senior Member
 
Ahmed
Join Date: Mar 2009
Location: NY
Posts: 250
Rep Power: 9
Ahmed is on a distinguished road
I quote this line from the GRUMMP UserGuide
http://tetra.mech.ubc.ca/GRUMMP/UserGuide.pdf
"There must be a balance between resolution of the boundary and surface features and
complexity of the problem. In addition, for problems with isotropic physics, element aspect ratio must be
small to minimize linear system condition number and interpolation error"

but they do not define how small the aspect ratio must be. or how small is small.
This is a question of getting experience by doing, i.e. meshing
Good Luck
Ahmed 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] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
basic of mesh refinement arya CFX 4 June 19, 2007 12:21
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
mesh quality julie FLUENT 5 July 26, 2004 05:31


All times are GMT -4. The time now is 18:45.