CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [Other] ANSYS to Fluent mesh export in ASCII format (http://www.cfd-online.com/Forums/ansys-meshing/72929-ansys-fluent-mesh-export-ascii-format.html)

johannes February 22, 2010 08:31

ANSYS to Fluent mesh export in ASCII format
 
Hi all,

I have a short question regarding mesh transfer from ANSYS Workbench to Fluent. This is usually done by creating named sections as boundary conditions and exporting the mesh as a binary .msh file.

I sometimes need the mesh as input for another software which cannot read binary files, so the question is:
Is there any possibility to export the mesh as ASCII file, maybe using some kind of APDL macro or script?

Many thanks in advance!

Best regards,
Johannes

PSYMN March 1, 2010 10:24

Environment Variable...
 
I asked the developer and she said...

You can set an environment variable to get the mesh in ASCII:

AWP_WRITE_FLUENT_MESH_ASCII=1

I haven't had time to try it out myself, so let us know how it works. ;)

johannes March 1, 2010 14:21

Simon, you're the man! It works like a charm! Yeah! :D

Thank you very much for taking your time to forward my question.

Best regards,
Johannes

JasonG June 4, 2010 08:51

Is this environment variable only applicable if Ansys Fluent is loaded? I have access to the CFX mesher from within the Ansys 11.0 Workbench environment, and it appears to only have the ability to write a binary Fluent inport file.

I was hoping to find a flag or setting somewhere to make it write the ascii file, but so far no luck :(.

Any help is greatly appreciated.

PSYMN June 6, 2010 07:31

newer version...
 
It probably only works with 12.0 o 12.1 and was not available with 11.0.

Simon

JasonG June 27, 2010 13:08

I finally got 12.1 installed on my work desktop, and it works as described :). I was then able to import the mesh file to OpenFOAM.

kingjewel1 September 10, 2010 08:03

Are you saying you export the mesh from within FLUENT? I'm using Gambit...

JasonG September 10, 2010 08:18

I only have the Ansys Mechanical package, but it allows use of the CFX/Fluent mesher. I was able to export the mesh in a Fluent format with BCs, and then run the conversion to OpenFoam once on my Linux desktop.

Now if I could just figure out an easy way to get an inverted volume from cavities and fluid passages.

phsieh2005 February 17, 2011 11:10

more details?
 
Hi, Jason,

can you send me more detailed steps on how you use name selection, mesh it, specify BCs in workbench, then, export to fluent ascii?

I have both WB 12.1 and 13 under Windows 7. Which (and where) file to edit?

Thanks!

Pei

PSYMN February 17, 2011 12:14

JasonG, use DM, Tools => Enclosure.

Phsieh, This link should help...

http://www.youtube.com/user/ansysinc#p/u/6/-6Z2v8geroQ

JasonG February 17, 2011 12:26

Pei,

Here are some quick steps I followed to setup my computer, hopefully this will assist you:

Step 1: Right click on "My Computer" icon from desktop, click on "Properties", click on the "Advanced" tab, and then click on "Environment Variabls".

Step 2: Under "User Variables for __" click "New", a box should pop up. Fill out the following:

Variable name: AWP_WRITE_FLUENT_MESH_ASCII
Variable value: 1

Step 3: Click "ok" on all the windows to close out of the system properties.

Step 4: Once in the meshing applet of workbench, go to "File" -> "Export", and then select the ".msh" option.

This should export the fluent file in the correct format, and should translate all components (as long as none are overlapping).

JasonG February 17, 2011 12:30

Quote:

Originally Posted by PSYMN (Post 295746)
JasonG, use DM, Tools => Enclosure.

Phsieh, This link should help...

http://www.youtube.com/user/ansysinc#p/u/6/-6Z2v8geroQ


I keep discovering that Ansys has removed a lot of boolean functionality in Workbench (unless you purchase DM) that is still available in Classic. For now I have had decent success with getting my cavities from the Pro/Engineer, and it allows me to easily simplify some structures that I suspect to have little flow impact but will result in increased mesh size.

PSYMN February 17, 2011 12:38

I wasn't there for the decision, but I suspect that you have given the reason why...

Many users have access to CAD tools which can extract the flow volume, simplify it and send it to ANSYS Meshing as a solid. So it probably didn't seem necessary to complicate the mesher (and use up our meshing team resources and probably increase the price of ANSYS Meshing) to replicate this same functionality.

For those who want to pay for this sort of development, we have DM. It is designed for users (mostly analysts) who would prefer a specialist tool because they either don't have access (or don't want to pay for something like Pro/E), or don't want to learn a professional CAD system.

The tools that were in classic are still there (and Mechanical APDL is available in WB). DM and CAD tools (connected with direct CAD interfaces) just do it better.

JasonG February 17, 2011 12:50

I just get that "nickle and dimed" feeling from Ansys :). At this time time the only reason I use workbench is for the experimenting I am doing with OpenFOAM. All of my structural analyses will remain in the Classic environment unless there is a better hybird made of the two.

PSYMN February 17, 2011 13:05

Don't think of it as nickel and dimming. It is more like not charging you for stuff you don't want. The alternative is to just include it and raise the price and complexity for everyone... Oh well, not up to me, but that is how I look at it.

As for Classic functionality moving over to WB, it is a continuous process. The hard part is balancing the functionality of Classic with the Ease of Use of WB. They have to be careful to do it right.

You can now run APDL snipits in ANSYS Mechanical. Plus ANSYS Mechanical APDL (aka ANSYS Classic) is actually on the workbench project page now so you can connect it to DM and/or ANSYS Meshing or automatically parse the APDL for variables which become parameters and can be controlled by DX, etc. This combo lets you take advantage of the easy parts of WB while still having the solver flexibility and scritability of classic. The plans for the next few releases should take care of the rest.

Just keep checking back. They are working hard to win you over eventually :cool:

JasonG February 17, 2011 14:00

Ah, but don't fix what isn't broken! I am happpy with my APDL and classic lol.

phsieh2005 February 17, 2011 18:36

Thanks a lot Jason!

This is what I have been looking for for a long time.

Pei

Quote:

Originally Posted by JasonG (Post 295748)
Pei,

Here are some quick steps I followed to setup my computer, hopefully this will assist you:

Step 1: Right click on "My Computer" icon from desktop, click on "Properties", click on the "Advanced" tab, and then click on "Environment Variabls".

Step 2: Under "User Variables for __" click "New", a box should pop up. Fill out the following:

Variable name: AWP_WRITE_FLUENT_MESH_ASCII
Variable value: 1

Step 3: Click "ok" on all the windows to close out of the system properties.

Step 4: Once in the meshing applet of workbench, go to "File" -> "Export", and then select the ".msh" option.

This should export the fluent file in the correct format, and should translate all components (as long as none are overlapping).


PSYMN February 17, 2011 22:02

Quote:

Originally Posted by JasonG (Post 295771)
Ah, but don't fix what isn't broken! I am happpy with my APDL and classic lol.

Yea, I am pretty sure they know not to wreck that... They are just exposing its functionality thru the new interface... No worries ;)

Alynx June 10, 2011 06:05

Quote:

Originally Posted by PSYMN (Post 247917)
I asked the developer and she said...

You can set an environment variable to get the mesh in ASCII:

AWP_WRITE_FLUENT_MESH_ASCII=1

I haven't had time to try it out myself, so let us know how it works. ;)


Hello,
I try it with WB 13.0 and it works fine :D
Thanks a lot

JasonG June 10, 2011 08:16

This feature is also working for me in R13.0. I have discovered that the file export will always be in Metric units regards of the current project setting in Workbench. I spoke with Ansys support, and they said the Fluent export will only write the file in Metric and allow the user to convert to different units once in Fluent.

The industry I work in is largely based around standard units (unfortunately), so I will need to figure out a way to scale everything around in the pre-solution or in the post processing. For now I have added a few lines to my controlDict that will compute Pstatic, and I added a factor to my density such that I end up with units of Psi.


All times are GMT -4. The time now is 15:36.