CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...

Hypermesh Update????

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 26, 2012, 10:10
Default Hypermesh Update????
  #1
Senior Member
 
n/a
Join Date: Sep 2009
Posts: 198
Rep Power: 7
deji is on a distinguished road
Hello Foamers. I am in the process of creating my 3D meshes with hypermesh, and need to know if there is any update regarding converting these hypermesh files into OpenFOAM? I did see a couple of threads regarding this same topic, but they are quite old. Can anyone please give me some feedback on this?

Cheers,
Deji
deji is offline   Reply With Quote

Old   January 26, 2012, 10:13
Default
  #2
Senior Member
 
n/a
Join Date: Sep 2009
Posts: 198
Rep Power: 7
deji is on a distinguished road
I think I've found the answer to my question,

Deji
deji is offline   Reply With Quote

Old   January 30, 2012, 05:26
Default
  #3
Senior Member
 
BastiL
Join Date: Mar 2009
Posts: 471
Rep Power: 11
bastil is on a distinguished road
Quote:
Originally Posted by deji View Post
I think I've found the answer to my question,

Deji
And what is the answer, please?
bastil is offline   Reply With Quote

Old   January 30, 2012, 08:47
Default
  #4
New Member
 
Slawek
Join Date: Feb 2010
Posts: 1
Rep Power: 0
slawekchr is on a distinguished road
Hi,

you can export your mesh from Hypermesh directly to OpenFoam
(it is possible from Hypermesh version 10.0).
Or you can export from HM to fluent and then use fluentMeshToFoam.

Slawek
slawekchr is offline   Reply With Quote

Old   May 3, 2013, 07:51
Default
  #5
Senior Member
 
Rishi .
Join Date: Mar 2009
Posts: 138
Rep Power: 8
hellorishi is on a distinguished road
Although there is a direct way to export from HyperMesh to OpenFOAM, exporting via Fluent remains the most robust method (as of HyperMesh 12.0).
hellorishi is offline   Reply With Quote

Old   May 3, 2013, 08:14
Default
  #6
Member
 
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5
billie is on a distinguished road
Currently exporting to fluent mesh is the more robust method as hellorishi already mentioned.

This is especially true for multi-region cases and if internal faces are required which is because the direct export from Hypermesh to Openfoam does not distinguish between internal and external faces. Everything is exported as a boundary. Exporting to fluent format first and using fluent*MeshToFoam creates boundaries for external faces and faceZones for internal faces if the recommended naming scheme is used in Hypermesh (i. e. prefixing internal faces with inte_).

There are also some face ordering problems which can occur when using the direct export method. This however can be fixed by using renumberMesh.

I have reported this issues to Altair and maybe this will be fixed eventually.
billie is offline   Reply With Quote

Old   May 14, 2013, 07:08
Default
  #7
Member
 
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5
billie is on a distinguished road
Quote:
Originally Posted by billie View Post
I have reported this issues to Altair and maybe this will be fixed eventually.
Today I received an email from the Altair support. The issues I have reported will be fixed in the next Update which will be Hyperworks 12.0-110. Lets see if this improves direct export to OpenFOAM from Hyperworks.
billie is offline   Reply With Quote

Old   October 3, 2013, 04:45
Default
  #8
Member
 
Daniel Pielmeier
Join Date: Apr 2012
Posts: 96
Rep Power: 5
billie is on a distinguished road
Quote:
Originally Posted by billie View Post
Currently exporting to fluent mesh is the more robust method as hellorishi already mentioned.

This is especially true for multi-region cases and if internal faces are required which is because the direct export from Hypermesh to Openfoam does not distinguish between internal and external faces. Everything is exported as a boundary. Exporting to fluent format first and using fluent*MeshToFoam creates boundaries for external faces and faceZones for internal faces if the recommended naming scheme is used in Hypermesh (i. e. prefixing internal faces with inte_).

There are also some face ordering problems which can occur when using the direct export method. This however can be fixed by using renumberMesh.

I have reported this issues to Altair and maybe this will be fixed eventually.
The Hyperworks 12.0 SA Update which includes Hypermesh 12.0.110.40 fixes the above mentioned issues. Direct export to OpenFOAM significantly improved with this version.
billie 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
Hypermesh file to Fluent Logesh FLUENT 1 November 30, 2011 14:46
HyperMesh x ProStar Vinicius CD-adapco 2 January 21, 2009 16:30
Hypermesh used for Fluent ?? Boris FLUENT 2 January 27, 2003 22:05
Imprting HYPERMESH Mesh file in Gambit Atul T. Shinde FLUENT 1 December 31, 2002 12:39
Exporting HyperMesh file to fluent 5 Ricardo FLUENT 0 July 6, 2000 04:18


All times are GMT -4. The time now is 23:30.