CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Meshing & Mesh Conversion

Hypermesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 3, 2006, 10:00
Default Hello everybody, Is it poss
  #1
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello everybody,

Is it possible to read in a mesh generated by Hypermesh? Hypermesh is from Altair part of the hyperworks package.
I've tried several outputs, Among which Ideas and Ansys, but they do not work. They all give the same error:

--> FOAM FATAL ERROR : points deallocated

From function const pointField& polyMesh::allPoints() const
in file meshes/polyMesh/polyMesh.C at line 656.

FOAM aborting

Has anybody got an idea? If not I will contact hyperworks and ask them for different mesh outputs.

regards
Guido
guido_adriaensen is offline   Reply With Quote

Old   January 4, 2006, 15:49
Default The message comes from the mes
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
The message comes from the mesh being empty so it looks like the conversion has failed.

The ideasToFoam was written some time ago to convert a mesh input file coming from Ansys. We only tested it on flange.ans from the laplacianFoam tutorial.
mattijs is offline   Reply With Quote

Old   January 13, 2006, 05:54
Default We managed to convert a hyperM
  #3
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
We managed to convert a hyperMesh file.

- export to Ansys
- if nessecary replace all DOS linefeeds with Unix ones (e.g. with dos2unix)
- use ideasToFoam
mattijs is offline   Reply With Quote

Old   January 13, 2006, 07:02
Default Hello Mattijs, Thanks for t
  #4
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello Mattijs,

Thanks for the update. I also just received a message from hypermesh-people that it should work. I believe they have contacted you for this. :-) I just tested it myself and it works indeed, thanks for your help!

Guido
guido_adriaensen is offline   Reply With Quote

Old   March 17, 2006, 12:19
Default Hello Guido, Hello Mattjis, I
  #5
Member
 
Vivek Kumar
Join Date: Mar 2009
Location: Switzerland
Posts: 34
Blog Entries: 1
Rep Power: 8
vivekcfd is on a distinguished road
Hello Guido, Hello Mattjis,
I tried to read an IDEAS file generated by ICEM
with ideasToFoam and I got exactly the same error message as Guido.

--------------------

--> FOAM FATAL ERROR : points deallocated

From function const pointField& polyMesh::allPoints() const
in file meshes/polyMesh/polyMesh.C at line 656.

FOAM aborting

Aborted
--------------

I then executed dos2unix (since I generated the file on a windows machine) but still
no success. Can anybody help?

Regards and thanks
Vivek
vivekcfd is offline   Reply With Quote

Old   March 17, 2006, 14:23
Default - check the file for DOS linef
  #6
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
- check the file for DOS linefeeds.
- check the contents of the file. Compare to the flange.ans file in the laplacianFoam tutorial. Do you have 'N' (nodes), 'EN' (elements) and 'SFE' (boundary faces)? (all the other fields are discarded)
mattijs is offline   Reply With Quote

Old   March 20, 2006, 03:54
Default Hello, If you have created
  #7
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello,

If you have created the mesh with hypermesh you indeed will have to use something like dos2unix, since hypermesh writes out the mesh-files in dos-format.
I've spoken to some people from hypermesh last week. They are now working on a conversion from hypermesh directly to openFOAM. I've provided them with some examples of the mesh-files from openFOAM and they will create either a conversion tool or maybe even a direct export option inside hypermesh. The more people that ask hypermesh for a port to openfoam, the more likely that they will built it in to their next release.

kind regards
Guido
guido_adriaensen is offline   Reply With Quote

Old   March 20, 2006, 06:47
Default Mattijs: My IDEAS file diffe
  #8
Member
 
Vivek Kumar
Join Date: Mar 2009
Location: Switzerland
Posts: 34
Blog Entries: 1
Rep Power: 8
vivekcfd is on a distinguished road
Mattijs:
My IDEAS file differ comopeletly from what lies in the .ans file from the laplacianFoam tutorial. I have checked my IDEAS file, it has no N, EN and SFE flags.
Guido:
I have not generated the IDEAS file with hypermesh but with another grid generation tool known as ICEM.

I am still not finding a way to export my mesh from ICEM to OpenFOAM. From ICEM, I can export my grid file to the follwoing unstructured grid formats:
ANSYS, ANSYS-CFX, IDEAS and PATRAN

Can you help?

regards
Vivek
vivekcfd is offline   Reply With Quote

Old   March 20, 2006, 09:21
Default export to fluent, you'll get a
  #9
Member
 
nicolas
Join Date: Mar 2009
Location: Glasgow
Posts: 42
Rep Power: 8
nico765 is on a distinguished road
export to fluent, you'll get a *.cas file. Then you can use fluentToFoam utility.

Nico
nico765 is offline   Reply With Quote

Old   March 20, 2006, 19:23
Default Nicolas As I wrote in my prev
  #10
Member
 
Vivek Kumar
Join Date: Mar 2009
Location: Switzerland
Posts: 34
Blog Entries: 1
Rep Power: 8
vivekcfd is on a distinguished road
Nicolas
As I wrote in my previous mail, I can only export my mesh in the follwoing formats as per output module of ICEM:
ANSYS, ANSYS-CFX, IDEAS and PATRAN

Other exports require an additional ICEM license which I do not have at the moment.

Export to fluent: is it fluent_V4 or fluent_V6 export?

Can anyone give me a solution? I am getting very frustated with the very first step of getting aquianted with OpenFOAM.

thanks
VK
vivekcfd is offline   Reply With Quote

Old   March 21, 2006, 05:04
Default Try the Ansys format. See if i
  #11
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Try the Ansys format. See if it is similar to that flange.ans one. If so try the ideasToFoam (in the new version it has been renamed to ansysToFoam)
mattijs is offline   Reply With Quote

Old   March 21, 2006, 05:11
Default Actually Mattijs, that one is
  #12
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Actually Mattijs, that one is very problematic: it reads the Ansys input file (creating vertices etc as an Ansys script) rather than the actual mesh. It came as a way of getting a mesh from Ideas and we didn't have a sensible export format. I'm not sure we've got a converter that can read the ansys mesh.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   January 14, 2008, 12:51
Default Hi all, which is the actual si
  #13
Member
 
Francesco Boschetto
Join Date: Mar 2009
Location: Italy
Posts: 56
Rep Power: 8
francesco_b is on a distinguished road
Hi all, which is the actual situation with Hypermesh? I tried to use ideasUnvToFoam to convert files but I still got some problems. Is there someone who succeeded in solving it?

Thank you in advance

Francesco
francesco_b is offline   Reply With Quote

Old   January 15, 2008, 04:34
Default Hello Francesco, I'm using
  #14
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello Francesco,

I'm using Hypermesh to create my mesh-files and import them into OF. Which version are you using? We have had an update to write native fluent / star, etc formats. I'm using the fluent format, which I convert by using fluentMeshToFoam. This works perfectly. The problem with the current release is that they write nastran files, even though it says write fluent or whatever.

Guido Adriaensen
guido_adriaensen is offline   Reply With Quote

Old   January 15, 2008, 05:25
Default Hi Guido and Francesco, For
  #15
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Hi Guido and Francesco,

For the STAR-CD export, they're exporting Nastran solids as well. The boundary condition definitions are a bit of a hack: they define shells and then use the pro-STAR functionality to change these into boundary patches.

How are the boundary conditions being defined for the Fluent and unv outputs?

/mark
olesen is offline   Reply With Quote

Old   January 15, 2008, 05:30
Default Hi Guido, I've changed fro
  #16
Member
 
Francesco Boschetto
Join Date: Mar 2009
Location: Italy
Posts: 56
Rep Power: 8
francesco_b is on a distinguished road
Hi Guido,

I've changed from version 7.1 to 8.0 RS1 only some days ago, I also downloaded the patches from the Altair site, but I'm quite new to this version. I tried to export a mesh with the "CFD/general" template but I could only write a Nastran file. Where can I find your update? Is it available somewhere?

Thank you in advance

Francesco
francesco_b is offline   Reply With Quote

Old   January 15, 2008, 06:19
Default Hi all! sounds good, that y
  #17
Senior Member
 
Florian Krause
Join Date: Mar 2009
Location: Munich
Posts: 103
Rep Power: 8
florian_krause is on a distinguished road
Hi all!

sounds good, that you use HM for meshing

We have an CFD Update for HM80SR1 which should solve your problem.

ftp://ftp.altair.de/outgoing/hyperwo...80/CFD_Updates

You will find the packed files and a readme with the install introductions

In the Utility Browser you will get a CFD I/O menu where you can export a "real" Fluent *.cas file, so no problem to use fluentMeshToFoam ;)

a positive feedback would be nice!

Regards,
Flo
florian_krause is offline   Reply With Quote

Old   January 15, 2008, 06:27
Default Hello Francesco and Mark, W
  #18
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello Francesco and Mark,

We have had an update from Altair. If you send me an email I will send you the files, you need to extract them in your install directory of HW and it will create the correct translators. Or you could contact Altair and request this update from them, it was an unofficial update from the USA department of Altair.

kind regards
Guido Adriaensen
guido_adriaensen is offline   Reply With Quote

Old   January 15, 2008, 06:48
Default Hello, The update I was spe
  #19
Member
 
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 8
guido_adriaensen is on a distinguished road
Hello,

The update I was speaking about is the same as the one from Florian. It works perfectly for us. :-)

kind regards
Guido
guido_adriaensen is offline   Reply With Quote

Old   January 15, 2008, 07:16
Default Hi, This patch is the actua
  #20
Senior Member
 
Florian Krause
Join Date: Mar 2009
Location: Munich
Posts: 103
Rep Power: 8
florian_krause is on a distinguished road
Hi,

This patch is the actual one, but it will be updatet from time to time.
So I can let you know if we have a new cfd update with significant changes on our ftp site...

Regards,
Flo
florian_krause 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 To Fluent Raghu FLUENT 12 December 12, 2013 02:26
hypermesh. Venkata Satyanand Main CFD Forum 0 February 21, 2008 14:49
Hypermesh and Fluent carno FLUENT 1 September 8, 2007 23:29
hypermesh-splin guang ai FLUENT 0 February 18, 2006 00:24
hypermesh and CFX garywang CFX 2 April 24, 2005 20:20


All times are GMT -4. The time now is 05:16.