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

[ICEM] CGNS output problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 2, 2011, 20:53
Default CGNS output problem
  #1
Member
 
Patrick Wollny
Join Date: Apr 2010
Posts: 58
Rep Power: 6
Pat84 is on a distinguished road
Hello again,

i am trying to mesh a litle laval nozzle with a unstruct mesh with a thickness of one cell. The goal is to compare the results of a compressible calculation (density based) from fluent with the results of the free cfd solver code saturne. For this reason i have tried to export the mesh to a cgns format, but for any reason the exported cgns mesh cannot be opened. neither in fluent nor in cfx. I have checked the mesh by icem, but itīs allright and when I export the mesh to a fluent or CFX fortmat, the mesh can be opened. I am sticking in the mud and need help to create succesfully a cgns mesh..
hope you can help me!
Attached Images
File Type: jpg ICEM_CGNS.jpg (94.7 KB, 52 views)
File Type: jpg FLU_CGNS.jpg (81.7 KB, 30 views)
File Type: jpg cfx_cgns2.jpg (72.5 KB, 32 views)
File Type: jpg FLU_msh.jpg (47.3 KB, 27 views)
Pat84 is offline   Reply With Quote

Old   January 3, 2011, 11:02
Default issues...
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
I think there may be some issue with the 2D CGNS output... Something to do with the upgrade to 3.0 libraries having issues with certain aspects in the earlier versions (such as 2D for CGNS 2.4). I am not exactly sure about all the issues, but development is working thru them.

Does this other program accept any other formats?

Do you have access to any older versions of ICEM CFD? (that don't have the CGNS 3.0 libraries)?

If not, I could quickly translate this for you using an older version, just so you can get going again while we figure out what the issue is.
PSYMN is offline   Reply With Quote

Old   January 3, 2011, 11:06
Default A fair benchmark would require a better mesh.
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Just a side issue, but for optimal results in fluent, assuming a viscous wall, you really need better boundary layer distribution and orthogonality... I have never heard of Saturne, but perhaps it would also appreciate the better grid.

This can be done with edge parameters and smoothing...

I recommend a better mesh before concluding your benchmark. Or perhaps the benchmark could include a variety of mesh types and densities.
PSYMN is offline   Reply With Quote

Old   January 3, 2011, 13:50
Default
  #4
Member
 
Patrick Wollny
Join Date: Apr 2010
Posts: 58
Rep Power: 6
Pat84 is on a distinguished road
Hi Simon,

thank you very much for your help. The grid is very coarse, especially in the near of the wall, but i will calculate a inviscid flow without shock and compare it with analytical results. I have calculated the case in fluent with this mesh (fluent v6 output of icem) and it agrees quiet well. Code Saturne also supports I-deas universal files and so i will try to use these output option in icem..

is there anything I should know about this format?

Enclosed:
I have the reason of the poor mesh quality. The grid appears to be localy shifted. I have attached 2 pictures. What can be the reason? The geometry is straight.
Attached Images
File Type: jpg Geom.jpg (85.8 KB, 28 views)
File Type: jpg Geom2.jpg (52.6 KB, 22 views)
Pat84 is offline   Reply With Quote

Old   January 3, 2011, 14:07
Default Edge distribution
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Your edge distributions are not well aligned... You could copy the one edge distribution to the other or you could set up periodicity...
PSYMN is offline   Reply With Quote

Old   January 3, 2011, 18:24
Default
  #6
Member
 
Patrick Wollny
Join Date: Apr 2010
Posts: 58
Rep Power: 6
Pat84 is on a distinguished road
Thank you Simon,

with the periodicity the edges are now straight. But I have no idea why they were shifted before. I have built the geometry nearly 10 times by creating one side and copying it in z-direction by the transform - translate tool. Then I have created a 3D block bounding box. I have cut it, I have associated the edges to curves and the vertices to points.. as always, but when I create a pre mesh, the two sides of the mesh are shifted!! That is so frustrating

As you have advised me in your post, I have tried to smooth the mesh orthogonal, but if i try to do this, icem crashes with the follow error message:
Attached Images
File Type: jpg orthoSmooth.jpg (88.9 KB, 12 views)
File Type: jpg parallel.jpg (94.6 KB, 6 views)

Last edited by Pat84; January 4, 2011 at 06:04.
Pat84 is offline   Reply With Quote

Old   January 3, 2011, 20:39
Default
  #7
Member
 
Patrick Wollny
Join Date: Apr 2010
Posts: 58
Rep Power: 6
Pat84 is on a distinguished road
After a renumbering the smoothing is now possible, but it makes nothing better. Maybe I donīt know how to perform the smoothing. Any tipps or tricks?

And is there any reason why the I-deas mesh works in fluent with all areas but not in cfx? (pic 2)

Does ICEM not support the GAMBIT neutral output?
Attached Images
File Type: jpg smoothing.jpg (92.3 KB, 23 views)
File Type: jpg I-deas.jpg (88.6 KB, 15 views)

Last edited by Pat84; January 4, 2011 at 09:56.
Pat84 is offline   Reply With Quote

Old   January 4, 2011, 10:07
Default
  #8
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You can see that the smoother is trying to make things orthogonal and trying to smooth out volume transitions, etc. It is just tough to do with such a coarse mesh... That mesh you showed is still probably better than your original. Remember, individual quality may go down, but the solver is actually more concerned about orthogonality and transition between elements. You could try a lot more iterations, you could fix (Freeze) the initial height on the curving wall... 13.0 works much better than 12.1 and there is also a beta option for structured smoothing that I really prefer.

The ICEM CFD output to ANSYS CFX should work... But once in CFX, you say you are importing from ICEM CFD.

ICEM CFD does not support the Gambit neutral output, but it does output in Fluent v6 *.msh format, and both Fluent and CFX will read that in no problem.

The I-DEAS product (Masters Series) is really out of date. We have almost no customers working in that format and ICEM CFD stopped selling our IDEAS CAD reader years ago. The IDEAS output is still there because there is no pressure to remove it, but it is not receiving much attention. You could submit a defect for the CFX team, but I doubt (just my guess) they would would be too worried about issues with reading the rarely used IDEAS format when you have the option of using the Fluent msh or CFX formats...
PSYMN is offline   Reply With Quote

Old   January 4, 2011, 10:34
Default
  #9
Member
 
Patrick Wollny
Join Date: Apr 2010
Posts: 58
Rep Power: 6
Pat84 is on a distinguished road
Ok.. but i am searching for a compatible format for code saturne and the I-deas mesh does not work with code saturne,too. There is a failure with the mesh while the pre procress is running. When I was working for the german aerospace center, I used GAMBIT with code saturne and it worked very fine. Now with ICEM there seems to be no way to export a mesh to code saturne..

I will send you an email with the mesh in fluent v6 format. Please convert it to cgns 2.4

Is ANSYS 13 already out? What are the innovations?

Last edited by Pat84; January 4, 2011 at 11:09.
Pat84 is offline   Reply With Quote

Old   January 4, 2011, 17:14
Default
  #10
Member
 
Patrick Wollny
Join Date: Apr 2010
Posts: 58
Rep Power: 6
Pat84 is on a distinguished road
Problem is solved!

ICEM 12.1 has a bug with earlier cgns formats, but with ICEM 11 it is no problem to export a cgns mesh to code saturne. You only have to create default BC patches and use face elements for BC patch.

Thank you for the support Simon!
Pat84 is offline   Reply With Quote

Old   January 6, 2011, 14:14
Default
  #11
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,650
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Just to be clear, the bug was with the CGNS 3.0 libraries we included with 12.1 and 13.0. They have trouble when exporting Hexas in CGNS V2.4 or 2.5. There is some other workaround that can be done to fix the files, but we are working to update the library for the next release. I expect to have a patch sooner or later. Let me know if you need it.
PSYMN is offline   Reply With Quote

Old   May 1, 2013, 20:56
Default
  #12
New Member
 
Eric
Join Date: Jan 2011
Location: Beijing,China
Posts: 9
Rep Power: 5
sstemptation is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
Just to be clear, the bug was with the CGNS 3.0 libraries we included with 12.1 and 13.0. They have trouble when exporting Hexas in CGNS V2.4 or 2.5. There is some other workaround that can be done to fix the files, but we are working to update the library for the next release. I expect to have a patch sooner or later. Let me know if you need it.
hi, Simon,

The exporting problem about ICEM to CGNS is due to the version of FLUENT?

I met the same problem right now.
sstemptation 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
2 Way FSI Problem alialibas CFX 16 May 5, 2014 08:34
Can I solve this problem by Fluent? Kai_kc FLUENT 1 October 27, 2010 05:29
Velocity profiles problem behind the elbow (3D problem) kabat73 FLUENT 8 May 9, 2010 04:26
CFX-5.7 MPICH Parallel Problem (Output of Results) James Date CFX 7 February 15, 2005 16:03
ICEM5 Hexa output problem Pete CFX 9 September 16, 2004 18:33


All times are GMT -4. The time now is 16:31.