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

[Commercial meshers] Error in polyhedral-mesh (Fluent Meshing) conversion to OpenFOAM.

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

Like Tree5Likes
  • 1 Post By akidess
  • 4 Post By ACLT

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 27, 2018, 07:33
Angry Error in polyhedral-mesh (Fluent Meshing) conversion to OpenFOAM.
  #1
New Member
 
Adriana
Join Date: Feb 2015
Posts: 4
Rep Power: 11
ACLT is on a distinguished road
Hi everyone,

I am using the ACT extension* to convert ANSYS Meshing meshes to polyhedral meshes and everything seem to be ok in Fluent. Then, I tried to convert the mesh to OpenFOAM and after many errors the conversion was successful. However, when I visualized the mesh I realized that the polyhedrons were not well-converted. The polyhedrons seem to be divided and I don't know why can be the reason, or if I am missing some extra command needed.

Thanks in advance!




*When I used only FluentMeshing to generate the mesh and not ACT, the same occurs.
Attached Images
File Type: png OriginalMesh.PNG (42.0 KB, 98 views)
File Type: png OriginalMesh2.PNG (131.5 KB, 85 views)
File Type: png OF_mesh.PNG (44.0 KB, 117 views)
File Type: png OF_mesh2.PNG (36.8 KB, 82 views)
ACLT is offline   Reply With Quote

Old   July 27, 2018, 08:34
Default
  #2
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,377
Rep Power: 30
akidess will become famous soon enough
How to visualize polyhedron mesh in paraview
Tobi likes this.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
akidess is offline   Reply With Quote

Old   August 16, 2018, 02:45
Default
  #3
New Member
 
Adriana
Join Date: Feb 2015
Posts: 4
Rep Power: 11
ACLT is on a distinguished road
Thank you very much!
ACLT is offline   Reply With Quote

Old   October 27, 2018, 13:10
Default
  #4
New Member
 
Not applicable
Join Date: Sep 2018
Posts: 15
Rep Power: 7
kagen816 is on a distinguished road
Quote:
Originally Posted by ACLT View Post
Hi everyone,

I am using the ACT extension* to convert ANSYS Meshing meshes to polyhedral meshes and everything seem to be ok in Fluent. Then, I tried to convert the mesh to OpenFOAM and after many errors the conversion was successful. However, when I visualized the mesh I realized that the polyhedrons were not well-converted. The polyhedrons seem to be divided and I don't know why can be the reason, or if I am missing some extra command needed.

Thanks in advance!




*When I used only FluentMeshing to generate the mesh and not ACT, the same occurs.
Hi ACLT,

Could you tell me how you import the polyhedral mesh from fluent into openFoam? I am now straggling with it. thank you very much.
kagen816 is offline   Reply With Quote

Old   October 29, 2018, 02:50
Default
  #5
New Member
 
Adriana
Join Date: Feb 2015
Posts: 4
Rep Power: 11
ACLT is on a distinguished road
Hi kagen816!


Once you have the mesh in Fluent, you need to save the .cas with the "binary files" option deactivate. Then, in OpenFOAM use the command "fluent3DmeshToFoam your_name_case.cas" and now an error appears always to me. It says something like "Do not understand characters ; ", so you need to open the file with vim or another editor, then find the ";" character and delete it (In my meshes it appears always two times). Finally, another time with the command fluent3DmeshToFoam, it should work.


Hope it works for you! If you need more information, don't hesitate to tell me
rezaeimahdi, manuc, dyle and 1 others like this.
ACLT is offline   Reply With Quote

Old   October 29, 2018, 12:36
Default
  #6
New Member
 
Not applicable
Join Date: Sep 2018
Posts: 15
Rep Power: 7
kagen816 is on a distinguished road
Quote:
Originally Posted by ACLT View Post
Hi kagen816!


Once you have the mesh in Fluent, you need to save the .cas with the "binary files" option deactivate. Then, in OpenFOAM use the command "fluent3DmeshToFoam your_name_case.cas" and now an error appears always to me. It says something like "Do not understand characters ; ", so you need to open the file with vim or another editor, then find the ";" character and delete it (In my meshes it appears always two times). Finally, another time with the command fluent3DmeshToFoam, it should work.


Hope it works for you! If you need more information, don't hesitate to tell me
Hi ACLT,

It works very well! Thank you very much!

Best Regards.
kagen816 is offline   Reply With Quote

Old   June 22, 2022, 03:36
Default
  #7
Member
 
rezaeimahdi's Avatar
 
mahdi
Join Date: Nov 2015
Location: Paris, France
Posts: 32
Rep Power: 10
rezaeimahdi is on a distinguished road
Quote:
Originally Posted by ACLT View Post
Hi kagen816!


Once you have the mesh in Fluent, you need to save the .cas with the "binary files" option deactivate. Then, in OpenFOAM use the command "fluent3DmeshToFoam your_name_case.cas" and now an error appears always to me. It says something like "Do not understand characters ; ", so you need to open the file with vim or another editor, then find the ";" character and delete it (In my meshes it appears always two times). Finally, another time with the command fluent3DmeshToFoam, it should work.


Hope it works for you! If you need more information, don't hesitate to tell me
Hi,

I just posted it here for the guys working with Ansys 2021 R2 or newer versions:

In these versions, you don't have that binary option in saving mesh files as suggested by ACLT

Also, in "Behavioral Change Messages" it is mentioned that: "The default mesh file format is changed to the Common Fluids Format (CFF) with an extension of *msh.h5. "

To be able to write a file.cas in ASCII format in fluent:

First, you need to change as follow:

File-->Preferences-->Default Format for I/O--->Legacy


Then in fluent console, type:

Code:
/file> binary-legacy-files
Write binary files? [yes] no
/file> write-case
The rest of the process in OpenFOAM is same as ACLT suggested.

Also please note that if you don't need the polyhedral mesh generated in fluent and just want to export a mesh from Ansys Mesher, then:

Ansys mesher --> file --> options --> meshing --> export --> format of input file --> ASCII

Enjoy!

Last edited by rezaeimahdi; June 23, 2022 at 03:53.
rezaeimahdi is offline   Reply With Quote

Reply

Tags
act, fluent meshing, openfoam 5.0, polyhedral mesh

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Transfer of mesh from Meshing to Fluent destroys the mesh balrog_f FLUENT 9 July 28, 2018 10:02
Updating Fluent after meshing from Worbench Scripting, asks to update mesh again. UchihaMadara FLUENT 0 January 8, 2018 14:18
[mesh manipulation] Importing Multiple Meshes thomasnwalshiii OpenFOAM Meshing & Mesh Conversion 18 December 19, 2015 18:57
[snappyHexMesh] No layers in a small gap bobburnquist OpenFOAM Meshing & Mesh Conversion 6 August 26, 2015 09:38
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55


All times are GMT -4. The time now is 02:20.