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

How can I save a mesh file in ANSYS Workbench V12 for standalone mode CFX-Pre?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 9, 2010, 12:13
Question How can I save a mesh file in ANSYS Workbench V12 for standalone mode CFX-Pre?
  #1
New Member
 
Join Date: Jul 2009
Posts: 6
Rep Power: 7
fkonias is on a distinguished road
So far in V11 I could use “Meshing” in a workbench project and create a mesh file in a *.gtm or *.cmdb form and use it separately in other projects or standalone CFX-Pre mode. Now in V12 I can not save separately the mesh files or any other file type. I can only save the whole project in workbench, which connects the various steps from geometry to post, automatically without intermediate save files from every step. How can I extract a mesh file from “Meshing” in *.gtm or *.cmdb form to use separately in CFX-pre standalone mode?

Thank you for your time
fkonias is offline   Reply With Quote

Old   April 12, 2010, 04:04
Default
  #2
New Member
 
Join Date: Jul 2009
Posts: 6
Rep Power: 7
fkonias is on a distinguished road
anyone???
fkonias is offline   Reply With Quote

Old   April 14, 2010, 01:10
Default Export Mesh
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
There is an export option...

In ANSYS Meshing, go to File => Export...

(sorry I don't have it up in front of me so I forget the exact wording of the option, but I recall there were lots of options in there including fluent.msh files, ICEMCFD.uns file, CGNS files, etc. I don't remember if CFX Mesh was an option, but it probably was...)

Simon
PSYMN is offline   Reply With Quote

Old   April 14, 2010, 03:31
Default
  #4
New Member
 
Join Date: Jul 2009
Posts: 6
Rep Power: 7
fkonias is on a distinguished road
I know about the export tool, but there is no CFX-Meshing option. Never mind though, I found a way to get a *.cmdb file and do my job. I am sure there is a more sophisticated way than mine, but I don’t mind at the moment because I am on hurry. Thanks
fkonias is offline   Reply With Quote

Old   July 22, 2010, 07:11
Default Export Mesh
  #5
New Member
 
Saravanakumar
Join Date: Apr 2010
Location: Bangalore
Posts: 9
Rep Power: 6
saravana is on a distinguished road
We can export mesh from workbench as Fluent msh file and can use the same in CFX stand alone.
That is how i have been doing so for.
saravana is offline   Reply With Quote

Old   September 30, 2010, 13:14
Default
  #6
Member
 
Join Date: Mar 2009
Location: Norway
Posts: 85
Rep Power: 7
kjetil is on a distinguished road
The Fluent mesh exporter in Ansys 12.1 is terribly bad, and cannot be read by "other" software as i.e OpenFOAM. Importing it into Gambit always means a whole lot of "auto repair", as it is stated from the command field - adding points, lines and volumes for the mesh to be valid. As for the cgns exporter in workbench - it doe not work either, so Ansys has made a pretty poor job in making clients able of testing simulations in other cfd environments.
kjetil is offline   Reply With Quote

Old   October 1, 2010, 23:04
Default News to me...
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Kjetil,

That is the first complaint I have ever heard about the Fluent mesh output (and you can imagine how many thousands of customers use it regularly). Certainly, I have had no problem getting the meshes to load in Fluent, TGrid or ICEM CFD.

I have heard a minor complaint about the CGNS format (that was easily worked around and has since been fixed).

I would like to get to the bottom of this. Can you send me more specific messages or perhaps the actual files?

I would like the Workbench Files as well as the fluent.msh files so I could see if the problem is in your setup.

As far as I know, it creates a perfect standard Fluent File. If there is a problem importing a Fluent mesh file into OpenFoam, I would assume that OpenFoam has trouble with the Fluent format rather than assuming the Fluent OEM doesn't know how to output their own format. On the other hand, if you know of other "Fluent" files that load properly into OpenFoam or if you know what is different in the file formats, I could take that to development and sort this out. Perhaps the Fluent format has been enhanced since the last version that OpenFoam was setup for?
PSYMN is offline   Reply With Quote

Old   October 2, 2010, 07:39
Default
  #8
New Member
 
wu ming
Join Date: Oct 2010
Posts: 2
Rep Power: 0
customer is on a distinguished road
PSYMN,

I am a newer about the ansys workbench 12.1 and in a hurry for my project, may i ask some questions about how to make the workbench to read the mesh file from other thrid party ( i.e. the mesh files are generated by fortran). i mean i only want to use the mesh , boundarys ,loading and material information form this fotran generated files and want to convert this files to the workbech mesh file which the workbench can tell.

due i have a mesh generator code, it can generate the shell mesh, so i want to transfer this mesh file to workbench and use simulation to solve it. would you have some idea about it, i am in a very very hurry about it ,hope i can get some responses soon. anyway, thanks advance.
customer is offline   Reply With Quote

Old   October 2, 2010, 09:42
Default
  #9
Member
 
Join Date: Mar 2009
Location: Norway
Posts: 85
Rep Power: 7
kjetil is on a distinguished road
Simon,

I acknowledge the number of Ansys clients, and I'm equally surprised that this problem has not been addressed earlier.

To me, it seems like regardless the simplicity of the geometry, the Fluent file export from Ansys is possible to import into OpenFoam - at least for the past 1.5 years.

The .msh-files from Ansys are always significantly smaller than after being imported and re-saved in Gambit. Please see http://www.tadaa.no/pipetest.zip , which is a rather simple geometry - where the .msh-file ending in "_g" is the one repaired in Gambit. Do not misunderstand the 'helix' prefix of the files - this has to do with the flow characterstics.

When it comes to exporting to cgns, I simply get an error message saying that I should "contact vendor/supplier", can't quite recall the exact message. Though I have not tried to save this specific mesh to cgns.
kjetil is offline   Reply With Quote

Old   October 2, 2010, 14:52
Default Skin it...
  #10
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
To Customer,

WB needs to have a geometry to apply bocos, etc.

If you only have a mesh, you must first load it into FE Modeler (a free app on the workbench platform) and "skin" it. This creates a geometry from the surface of the mesh model. Then you can proceed to WB Simulation with the original mesh and the skinned geometry, apply boco's, etc.

Best regards,

Simon
PSYMN is offline   Reply With Quote

Old   October 2, 2010, 15:05
Default Ascii vs Binary...
  #11
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Kjetil,

It took looking at your files to remind me... The file that WB outputs by default is in a binary format. OpenFoam needs the older ASCII format (hasn't caught up in the past few years).

You can get ANSYS Meshing to output in the FLuent ASCII format with an environment variable (as shown in this thread)...

AWP_WRITE_FLUENT_MESH_ASCII=1

I am not sure what the Gridgen autorepair is about, probably just a conversion process, but I will pass your nicely bundled file set to development and ask them about it. It is most likely just a newer Fluent format than the Gambit reader.

Best regards,

Simon
PSYMN is offline   Reply With Quote

Old   October 2, 2010, 15:16
Default License for CGNS...
  #12
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Kjetil,

It just occurred to me what you were seeing with CGNS export. You are not complaining about the format, but rather that it didn't let you export at all...

There was a licensing bug where the CGNS export, which was originally part of the ICEM CFD code, was still looking for an ICEM CFD output license (aioutcfd). If you didn't have this key, it may have asked you to contact your ANSYS vendor. This was not intentional and has been fixed with 13.0, which is due out in November.

In the mean time, if you had contacted your vendor or tech support, they could have sent you the extra licensing increment.

Best regards,

Simon
PSYMN is offline   Reply With Quote

Old   October 2, 2010, 17:18
Default
  #13
New Member
 
wu ming
Join Date: Oct 2010
Posts: 2
Rep Power: 0
customer is on a distinguished road
PSYMN,

Thank you very much. may i ask another question, what kind of mesh file format can be read by ANSYS WORKBENCH .my mesh generator can generate three type of mesh file, one includes the nodes coordinate, one includes the elements information by nodes and material information for elements, last includes the loading information for nodes. how to conver these files to workbench, i know it need code a convertor, bur i don't know which file format can be read by workbench and how to do. sorry for a lot of questions, hope someone can response me early. thanks again.
customer is offline   Reply With Quote

Old   October 3, 2010, 15:07
Default standard formats.
  #14
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Customer,

The mesh formats for ANSYS (.in), Nastran (.nas) or Fluent (.msh) are all published and all can be read into FE modeler. You should look at these formats and decide which best suits your needs. There are others also, please check the full list of imports to FE modeler and then decide.

It could be that your mesh is already in what could be considered a standard format or at least once you identify the name of the format you currently have, you could look for a translator to one of the formats FE modeler can import.

Do some research before coding.

Best regards,

Simon
PSYMN is offline   Reply With Quote

Old   October 4, 2010, 19:19
Default Old version...
  #15
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
kjetil,

Acording to the headder at the top of your fluent.msh file, it was output by WB version 11.0.7 (a version from 3 years ago).

Since version 12.0, we have used a different output interface. (Not sure why you thought you were using 12)

Please try a more recent version and let us know if it works any better for you.
PSYMN is offline   Reply With Quote

Old   October 5, 2010, 00:17
Default How do I export a workbench mesh file of "axisymmetric" model to "standalone" Fluent?
  #16
Member
 
Join Date: Oct 2010
Posts: 44
Rep Power: 6
siri is on a distinguished road
Hi Simon.

I have read thru your replies in this post and thought you would be of help in this case ?!?

I am having problem in setting up the 2D axisymmetric analysis in "stand alone" Ansys Fluent after importing a pure quad mesh generated using Ansys Mesh (Workbench 12).

I am suspecting a conflict going on between the two with respect to coordinate system orientation here - while workbench export requires the axis along Y; Fluent searches for axial along X. Am I right to say so?

Now the issue I face is that Fluent is unable to initialize the solution using velocity inlet boundary condition (i want to specify axial velocity and i tried doing it along X or Y, neither is working). In the velocity and density boxes on the Solution initialization tab, it computes them from Inlet as #.IND
What does it mean?

Lastly, I couldn't find any better than this post on the whole webpages about this ..... this post was the closest I could read on such an axisymmetric model.

Has anyone done anything like it before, plz respond if anyone did.


P.S: Don't have the license to run Fluent in workbench, hence the situation


Thanks to everyone here.
siri is offline   Reply With Quote

Old   October 5, 2010, 01:16
Default
  #17
Member
 
Join Date: Mar 2009
Location: Norway
Posts: 85
Rep Power: 7
kjetil is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
kjetil,

Acording to the headder at the top of your fluent.msh file, it was output by WB version 11.0.7 (a version from 3 years ago).

Since version 12.0, we have used a different output interface. (Not sure why you thought you were using 12)

Please try a more recent version and let us know if it works any better for you.
Simon,
thanks for your effort. I have not spent awfully lot of time on trying to export to the cgns format - it just occured to me that OpenFoam hadde import capabilites from it, as I at that point still couldn't get the Ansys .msh exporter to work (as we all know now - to get it to output to ascii). As you can see the content of "pipetest" zip file originates 9 months back in time, which happens to be the time I was working on my thesis. I picked this bundle due to the specific geometry simplicity, and I have, nor had, no control of what licenses or software versions the university department could access. As of today, I do have access to a 12.1 workbench - but I didn't want to publish here my most recent works
kjetil is offline   Reply With Quote

Old   October 5, 2010, 18:51
Default new topic.
  #18
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,661
Blog Entries: 1
Rep Power: 34
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Siri, sorry I don't really know about that issue. I would suggest starting a new thread for it.
PSYMN is offline   Reply With Quote

Old   January 31, 2011, 22:31
Default
  #19
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,891
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Hi PSYMN ,

you said formats are published, but where could we find the binary format specifications of .msh? FLUENT documentation seems to include only the "old" ASCII format.

Thanks,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   October 24, 2011, 19:40
Default
  #20
Member
 
Nathan
Join Date: Aug 2010
Posts: 64
Rep Power: 6
natantyt is on a distinguished road
Hi

I have two .msh files for Fluent one is a random packing of particles and one is the pore network between them. These are created and meshed with OpenFoam separately. Is it possible to merge them together?I would like to analyze the whole pore/solid geometry in Fluent. Is it possible to merge the original stl. files?
natantyt 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
Ansys workbench CFX Mesh Tom ANSYS Meshing & Geometry 22 December 1, 2010 22:34
Version 15 on Mac OS X gschaider OpenFOAM Installation 120 December 2, 2009 11:23
Compiling gmshFoam with OpenFOAM-1.5 BlGene Open Source Meshers: Gmsh, Netgen, CGNS, ... 10 August 6, 2009 05:26
Compiling OpenFOAM13 on AMD64 with Redhat Enterprise mbeaudoin OpenFOAM Installation 20 June 17, 2008 07:43
error while compiling the USER Sub routine CFD user CFX 3 November 25, 2002 16:16


All times are GMT -4. The time now is 08:16.