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

Icem CFD mesh grading issue

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

Like Tree1Likes
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   October 14, 2010, 11:40
Default Icem CFD mesh grading issue
  #1
Member
 
joegi
Join Date: Nov 2009
Location: genoa
Posts: 59
Rep Power: 6
joegi.geo is on a distinguished road
Hi,

I generated a volume mesh by using the Delaunay method. To generate the mesh I imposed the tetra sizes on the loops, but now I am wondering how can I get the same elements grading/distribution on the edge where the surfaces meet (see attached figures). In gambit you can use size function to control the mesh grading and get a uniform distribution, is there something similar in Icem CFD? (sorry for bringing gambit into an icem cfd discussion)

Cheers,

Joel
Attached Images
File Type: jpg f1.jpg (89.1 KB, 86 views)
File Type: jpg f2.jpg (89.3 KB, 80 views)
joegi.geo is offline   Reply With Quote

Old   October 19, 2010, 13:34
Default Options...
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
Gambit had some good stuff, so no need to apologize... Actually, those Gambit features, such as the sizing function, are now in the ANSYS Meshing application. That application will run with the ICEM CFD full or ICEM CFD Tetra license, so maybe try it out...

In the mean time, ICEM CFD has a Sizing function, but it doesn't work with patch dependent surface meshing... So two choices...

1) Switch to Octree Tetra. With ICEM CFD, you don't actually need to start with a surface mesh (common Gambit user problem). You can go into Global mesh params, turn on the curvature and proximity size function (and set what ever sizes you want on specific entities) and then run the Octree Tetra method directly (under compute mesh). You will probably find it saves a few clicks over Gambit. If you don't like the Octree mesh, you can run delaunay afterward (or run delaunay directly from geometry in one click if you setup PI as the surface mesh default).

2) If you really needed Shell meshing, you can set the number of nodes on those vertical curves (curve parameters)... You can also set the sizing at the ends and the growth laws and ratios... It is a lot more interactive than a Sizing function, but it gives you complete control. In the model tree, right click on "Curves => Curve node spacing" if you want to see the distribution before meshing.
PSYMN is offline   Reply With Quote

Old   October 19, 2010, 19:40
Default
  #3
Member
 
joegi
Join Date: Nov 2009
Location: genoa
Posts: 59
Rep Power: 6
joegi.geo is on a distinguished road
Hi Simon,

As usual, I found your comments extremely helpful. Now I manage to have a better control over the surface mesh, but I still see some problems. Take a look at the firsts two figures. Why the first rows do not respect the imposed spacing?.

Also, it seems that the volume mesh does not follows the same grading as the one imposed on the surface mesh (take a look at the last two figures, specially to the central area), correct me if I am wrong. How can I obtain a smoother transition from the surface mesh to the to the volume mesh?

It will made any sense to impose as well the surface parameters (such as growth rate and number of tetra elements)?.

Btw I am using delaunay method.


Regrads,

Joel
Attached Images
File Type: jpg ff1.jpg (91.6 KB, 63 views)
File Type: jpg ff2.jpg (93.4 KB, 60 views)
File Type: jpg ff3.jpg (97.3 KB, 72 views)
File Type: jpg ff4.jpg (96.1 KB, 56 views)
joegi.geo is offline   Reply With Quote

Old   October 20, 2010, 16:40
Default
  #4
Member
 
joegi
Join Date: Nov 2009
Location: genoa
Posts: 59
Rep Power: 6
joegi.geo is on a distinguished road
Hi Simon,

Forget the previous post. I found what was the problem. I was using different growth rates for the curves so that was messing around the mesh. Final question, Can I use density areas with Delaunay or AFT volume meshes?.

Joel
joegi.geo is offline   Reply With Quote

Old   October 22, 2010, 03:39
Default
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 33
PSYMN will become famous soon enoughPSYMN will become famous soon enough
Density will work with the Delaunay mesher, but the "width" setting, which I often use with Octree as a special kind of "surface aligned" density, won't.

The Advancing Front mesher (AKA the CFX Mesher or the GE Mesher) is smoother (more controllable growth ratio), but much much slower (6 times slower per element). It also doesn't respect controls like "density". Still, many of our customers really love that mesher, so to each his own.

If you have 12.1, I recommend the Delaunay with the TGlib AF option... Unless you have limited memory. It will give you a more advancing front like smoothness, but works with all the ICEM CFD controls.
Far likes this.
PSYMN is offline   Reply With Quote

Old   October 24, 2010, 14:49
Default
  #6
Member
 
joegi
Join Date: Nov 2009
Location: genoa
Posts: 59
Rep Power: 6
joegi.geo is on a distinguished road
Hi Simon,

I created a volume mesh using delaunay method and mesh density. The volume mesh obey the mesh density I imposed but the surface mesh doesn't. Is there a way to impose the mesh density on the surfaces as well?.


Regards,

Joel
joegi.geo is offline   Reply With Quote

Old   October 25, 2010, 07:12
Default
  #7
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 11
BrolY will become famous soon enough
I guess you created an Octree mesh, then deleted all the fluid elements and finally created the volume mesh with delauney?
If so, I think you can't modify the surface mesh with delauney. You have to do it when you created the Octree mesh (Mesh/Surface Mesh Setup). This is why the mesh density only changed the volume mesh, and not the surface mesh !
BrolY is offline   Reply With Quote

Old   March 8, 2011, 18:26
Default
  #8
New Member
 
shawlini
Join Date: Mar 2011
Location: hyd,india
Posts: 1
Rep Power: 0
shawlini is on a distinguished road
Simon sir,
I am working on the Fortran90 code that you submitted in the anti essays.com over supersonic flow past a blunt body...n i need your help on my project please...
shawlini 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
Future CFD Research Jas Main CFD Forum 10 March 30, 2013 13:26
Tri Mesh In ICEM CFD Mohammad Faridul Alam CFX 0 January 16, 2008 06:33
prob while exporting icem cfd hexa mesh to fluent mani CFX 4 March 7, 2007 03:41
ICEM CFD surface mesh Francesco CFX 1 May 31, 2006 11:09
importing mesh from ICEM CFD into CFX 5 Jay CFX 2 November 12, 2002 13:46


All times are GMT -4. The time now is 02:37.