 |
 |
 |
|
|
|
[Sponsors] | ||||
January 3, 2006, 10:00
|
Hypermesh
|
#1 |
|
Member
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 17  |
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 |
|
|
|
|
|
January 4, 2006, 15:49
|
The message comes from the mes
|
#2 |
|
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
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. |
|
|
|
|
|
|
January 13, 2006, 05:54
|
We managed to convert a hyperM
|
#3 |
|
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
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 |
|
|
|
|
|
|
January 13, 2006, 07:02
|
Hello Mattijs,
Thanks for t
|
#4 |
|
Member
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 17 |
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 |
|
|
|
|
|
|
March 17, 2006, 12:19
|
Hello Guido, Hello Mattjis,
I
|
#5 |
|
Member
|
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 |
|
|
|
|
|
|
March 17, 2006, 14:23
|
- check the file for DOS linef
|
#6 |
|
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
- 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) |
|
|
|
|
|
|
March 20, 2006, 03:54
|
Hello,
If you have created
|
#7 |
|
Member
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 17 |
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 |
|
|
|
|
|
|
March 20, 2006, 06:47
|
Mattijs:
My IDEAS file diffe
|
#8 |
|
Member
|
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 |
|
|
|
|
|
|
March 20, 2006, 09:21
|
export to fluent, you'll get a
|
#9 |
|
Member
nicolas
Join Date: Mar 2009
Location: Glasgow
Posts: 42
Rep Power: 17 |
export to fluent, you'll get a *.cas file. Then you can use fluentToFoam utility.
Nico |
|
|
|
|
|
|
March 20, 2006, 19:23
|
Nicolas
As I wrote in my prev
|
#10 |
|
Member
|
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 |
|
|
|
|
|
|
March 21, 2006, 05:04
|
Try the Ansys format. See if i
|
#11 |
|
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
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)
|
|
|
|
|
|
|
March 21, 2006, 05:11
|
Actually Mattijs, that one is
|
#12 |
|
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
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 |
|
|
|
|
|
|
January 14, 2008, 12:51
|
Hi all, which is the actual si
|
#13 |
|
Member
Francesco Boschetto
Join Date: Mar 2009
Location: Italy
Posts: 56
Rep Power: 17 |
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 |
|
|
|
|
|
|
January 15, 2008, 04:34
|
Hello Francesco,
I'm using
|
#14 |
|
Member
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 17 |
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 |
|
|
|
|
|
|
January 15, 2008, 05:25
|
Hi Guido and Francesco,
For
|
#15 |
|
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,714
Rep Power: 40 |
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 |
|
|
|
|
|
|
January 15, 2008, 05:30
|
Hi Guido,
I've changed fro
|
#16 |
|
Member
Francesco Boschetto
Join Date: Mar 2009
Location: Italy
Posts: 56
Rep Power: 17 |
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 |
|
|
|
|
|
|
January 15, 2008, 06:19
|
Hi all!
sounds good, that y
|
#17 |
|
Senior Member
Florian Krause
Join Date: Mar 2009
Location: Munich
Posts: 103
Rep Power: 17 |
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 |
|
|
|
|
|
|
January 15, 2008, 06:27
|
Hello Francesco and Mark,
W
|
#18 |
|
Member
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 17 |
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 |
|
|
|
|
|
|
January 15, 2008, 06:48
|
Hello,
The update I was spe
|
#19 |
|
Member
Guido Adriaensen
Join Date: Mar 2009
Posts: 56
Rep Power: 17 |
Hello,
The update I was speaking about is the same as the one from Florian. It works perfectly for us. :-) kind regards Guido |
|
|
|
|
|
|
January 15, 2008, 07:16
|
Hi,
This patch is the actua
|
#20 |
|
Senior Member
Florian Krause
Join Date: Mar 2009
Location: Munich
Posts: 103
Rep Power: 17 |
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 |
|
|
|
|
|
 |
| Thread Tools | Search this Thread |
| Display Modes | |
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| HyperMesh for Mesh Generation for SU-2 | MM711 | SU2 | 0 | June 22, 2018 10:12 |
| Hypermesh Exporting | eishinsnsayshin | FLUENT | 8 | November 29, 2012 01:29 |
| Hypermesh Exporting | eishinsnsayshin | ANSYS | 0 | April 3, 2012 19:16 |
| Hypermesh file to Fluent | Logesh | FLUENT | 1 | November 30, 2011 14:46 |
| Volume mesh for Fluent.. Hypermesh or TGrid?? | mayur | FLUENT | 5 | June 25, 2010 02:45 |
Linear Mode
