|
[Sponsors] |
[Commercial meshers] Error in polyhedral-mesh (Fluent Meshing) conversion to OpenFOAM. |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Adriana
Join Date: Feb 2015
Posts: 4
Rep Power: 11 ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Adriana
Join Date: Feb 2015
Posts: 4
Rep Power: 11 ![]() |
Thank you very much!
|
|
![]() |
![]() |
![]() |
![]() |
#4 | |
New Member
Not applicable
Join Date: Sep 2018
Posts: 15
Rep Power: 8 ![]() |
Quote:
Could you tell me how you import the polyhedral mesh from fluent into openFoam? I am now straggling with it. thank you very much. |
||
![]() |
![]() |
![]() |
![]() |
#5 |
New Member
Adriana
Join Date: Feb 2015
Posts: 4
Rep Power: 11 ![]() |
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 ![]() |
|
![]() |
![]() |
![]() |
![]() |
#6 | |
New Member
Not applicable
Join Date: Sep 2018
Posts: 15
Rep Power: 8 ![]() |
Quote:
It works very well! Thank you very much! Best Regards. |
||
![]() |
![]() |
![]() |
![]() |
#7 | |
Member
mahdi
Join Date: Nov 2015
Location: Paris, France
Posts: 32
Rep Power: 10 ![]() |
Quote:
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 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. |
||
![]() |
![]() |
![]() |
Tags |
act, fluent meshing, openfoam 5.0, polyhedral mesh |
|
|
![]() |
||||
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 |