|
[Sponsors] |
[Commercial meshers] Fluent Mesh into OpenFoam |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 8, 2014, 19:37 |
Fluent Mesh into OpenFoam
|
#1 |
Senior Member
Join Date: Jan 2012
Posts: 197
Rep Power: 14 |
Hi
I followed this link:http://openfoamwiki.net/index.php/Fluent3DMeshToFoam to convert the fluent mesh file into openfoam Once I ran this command: fluent3DMeshToFoam fluent.msh There is nothing in the polymesh file I wonder which step I did wrong or what I missed Thanks for your help Regards Ke |
|
January 9, 2014, 04:39 |
|
#2 |
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 22 |
Hi Ke,
Can you post the output of fluent3DMeshToFoam? Cheers, L |
|
January 9, 2014, 08:19 |
|
#3 |
Senior Member
Join Date: Jan 2012
Posts: 197
Rep Power: 14 |
Hi Lieven
Here is the outcome /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.2.2 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.2.2-9739c53ec43f Exec : fluent3DMeshToFoam cavity1 Date : Jan 09 2014 Time : 13:17:53 Host : "ke-wu" PID : 536 Case : /Volumes/OpenFOAM-v2.1/OpenFOAM-2.2.2/run/Elbowpipe nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time --> FOAM FATAL ERROR: Do not understand characters: n on line 1 From function fluentMeshToFoam::lexer in file fluent3DMeshToFoam.L at line 748. FOAM exiting |
|
January 9, 2014, 08:50 |
|
#4 |
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 22 |
Have a look at this post:
http://www.cfd-online.com/Forums/ope...eshtofoam.html My guess is that you didn't save the .msh-file in ascii format... Cheers, L |
|
January 9, 2014, 08:57 |
|
#5 | |
Senior Member
Join Date: Jan 2012
Posts: 197
Rep Power: 14 |
Quote:
I did actually First of all, I write the .msh file into Fluent and then save it in ascii format via following procedure File -> export -> solution data Once the mesh file is saved in ascii format, the file extension disappeared So I put command in fluent3dmeshtofoam cavity1 rather than fluent3dmeshtofoam cavity1.msh Any mistake in my steps? |
||
January 9, 2014, 09:02 |
|
#6 |
Senior Member
Onno
Join Date: Jan 2012
Location: Germany
Posts: 120
Rep Power: 15 |
Open the file using nano and make sure it is actually ascii.
Give fluentMeshToFoam (without 3D) a try. It converts 2D and 3D meshes. |
|
January 9, 2014, 09:08 |
|
#7 |
Senior Member
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 22 |
Hi Ke,
To export the mesh in ascii format you should go to (assuming you use workbench): Tools -> Options -> Meshing -> Export and set the export format to ASCII then your .msh file should automatically be in ascii-format. Let me know if this did the trick... Lieven |
|
January 9, 2014, 09:12 |
|
#8 |
Senior Member
Join Date: Jan 2012
Posts: 197
Rep Power: 14 |
||
January 9, 2014, 09:13 |
|
#9 | |
Senior Member
Join Date: Jan 2012
Posts: 197
Rep Power: 14 |
Quote:
See the pic I attached No option for export |
||
January 9, 2014, 17:16 |
|
#10 | |
Senior Member
Join Date: Jan 2012
Posts: 197
Rep Power: 14 |
Quote:
What you mean "open the file using nano" and what nano is I convert msh file into ascii file via fluent Once it was saved, the file extension disappeared, I'm not sure it's in ascii format And I tried the new command without 3D It seems better than what I have done pervasively, but still got error. This is what I got: /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.2.2 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.2.2-9739c53ec43f Exec : fluentMeshToFoam cavity1 Date : Jan 09 2014 Time : 22:03:27 Host : "ke-wu" PID : 1094 Case : /Volumes/OpenFOAM-v2.1/OpenFOAM-2.2.2/run/Elbowpipe nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time FINISHED LEXING dimension of grid: 0 Creating shapes for 3-D cells Building patch-less mesh...done. Building boundary and internal patches. Writing mesh... to "constant/polyMesh" done. End When I type checkMesh, I got these: /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.2.2 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 2.2.2-9739c53ec43f Exec : checkMesh Date : Jan 09 2014 Time : 22:06:56 Host : "ke-wu" PID : 1144 Case : /Volumes/OpenFOAM-v2.1/OpenFOAM-2.2.2/run/Elbowpipe nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 --> FOAM Warning : From function polyMesh(const IOobject&) in file meshes/polyMesh/polyMesh.C at line 306 no points in mesh --> FOAM Warning : From function polyMesh(const IOobject&) in file meshes/polyMesh/polyMesh.C at line 311 no cells in mesh Time = 0 Mesh stats points: 0 internal points: 0 faces: 0 internal faces: 0 cells: 0 faces per cell: 0 boundary patches: 0 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 0 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 0 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology Checking geometry... Overall domain bounding box (0 0 0) (0 0 0) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) Boundary openness (0 0 0) OK. Max cell openness = -1e+300 OK. Max aspect ratio = -1e+300 OK. Minimum face area = 1e+15. Maximum face area = -1e+15. Face area magnitudes OK. Min volume = 1e+15. Max volume = -1e+15. Total volume = 0. Cell volumes OK. Non-orthogonality check OK. Face pyramids OK. Max skewness = -1e+300 OK. Coupled point location match (average 0) OK. Mesh OK. End When I try to view the mesh in paraview, I got this message: Warning: In /Users/kitware/Dashboards/MyTests/NightlyMaster/ParaViewSuperbuild-Release/paraview/src/paraview/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 4749 vtkOpenFOAMReaderPrivate (0x115654190): The mesh contains no cells Can you help me further Thanks |
||
January 10, 2014, 01:57 |
|
#11 |
Senior Member
Onno
Join Date: Jan 2012
Location: Germany
Posts: 120
Rep Power: 15 |
nano is a text editor that can take on large files. Just enter "nano *meshfilename*". Ctrl+x to exit the editor.
I am suprised fluentMeshToFoam didn't prompt some error message. Obviously something is wrong with the mesh. |
|
January 29, 2014, 06:51 |
fluentMeshToFoam
|
#12 |
New Member
sangram
Join Date: Jan 2014
Posts: 17
Rep Power: 12 |
Hello,
I just joined this forum....feeling excited to learn new things.... I am trying to import fluent mesh file (.msh) in openFOAM. I am not getting any error msg till i go in the paraview......but once I click on apply to see mesh in paraview.....it is showing me following msg....can any body please help me solve this issue...... -->FOAM FATAL IO ERROR: Cannot find patchField entry for velocity-inlet-5 file: /home/sandeep/OpenFOAM/sandeep-2.2.2/run/tutorials/zfluent/bubble/0/U.boundaryField from line 26 to line 40. From function GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::readField(const DimensionedField<Type, GeoMesh>&, const dictionary&) in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.2/src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 206. FOAM exiting |
|
January 29, 2014, 13:22 |
|
#13 |
Senior Member
Onno
Join Date: Jan 2012
Location: Germany
Posts: 120
Rep Power: 15 |
Try renaming 0/ to 0.org. You probably forgot to set your boundary conditions.
|
|
January 29, 2014, 23:55 |
|
#14 |
New Member
sangram
Join Date: Jan 2014
Posts: 17
Rep Power: 12 |
Thanks Kaskade for the immediate reply...
|
|
January 30, 2014, 00:14 |
fluentMeshToFoam
|
#15 | |
New Member
sangram
Join Date: Jan 2014
Posts: 17
Rep Power: 12 |
Hello,
Quote:
Then I tried renaming 0 with 0.org......Now I am getting following error message... --> FOAM FATAL IO ERROR: cannot find file file: /home/sandeep/system/controlDict at line 0. From function regIOobject::readStream() in file db/regIOobject/regIOobjectRead.C at line 73. FOAM exiting I am just 3 weeks older in CFD and OF......Guys please help me to learn..... |
||
January 30, 2014, 01:20 |
|
#16 |
Senior Member
Onno
Join Date: Jan 2012
Location: Germany
Posts: 120
Rep Power: 15 |
Have you done any of the tutorials? Maybe you should start with that, in order to learn about the OpenFOAM case structure and the required files.
|
|
January 30, 2014, 01:49 |
|
#17 | |
New Member
sangram
Join Date: Jan 2014
Posts: 17
Rep Power: 12 |
Quote:
Actually I have read basics of openFOAM and done Cavity tutorial....now I am trying to import fluent (.msh) file.....I think I have problem with selection of solver....can you please guide me on solver selection..... |
||
January 30, 2014, 02:05 |
|
#18 |
Senior Member
Onno
Join Date: Jan 2012
Location: Germany
Posts: 120
Rep Power: 15 |
What are you trying to simulate?
|
|
January 30, 2014, 04:19 |
|
#19 |
New Member
sangram
Join Date: Jan 2014
Posts: 17
Rep Power: 12 |
I am trying to import fluent (dam break) tutorials .msh file in openFOAM and trying to solve it using interfoam solver.......
When I am typing InterFoam in terminal window it is showing following error.... --> FOAM FATAL IO ERROR: cannot find file file: /home/sandeep/OpenFOAM/sandeep-2.2.2/run/tutorials/zfluent/Multiphase/dambreak/0/p_rgh at line 0. From function regIOobject::readStream() in file db/regIOobject/regIOobjectRead.C at line 73. FOAM exiting |
|
January 30, 2014, 04:45 |
|
#20 |
Senior Member
Onno
Join Date: Jan 2012
Location: Germany
Posts: 120
Rep Power: 15 |
1. copy the OpenFOAM dam break tutorial to your run directory
2. rename 0 to 0.org 3. rename constant/polyMesh/boundary to constant/polyMesh/boundary.org 4. delete the other files in constant/polyMesh 5. move the .msh-file to the case directory 6. convert it (-scale 0.001 if it's in mm instead of m) 7. run paraFoam and check the mesh 8. run checkMesh -constant 9. if everything checks out, rename 0.org back to 0 10. set your boundary conditions a. open constant/polyMesh/boundary, to see what boundaries need to be set b. open each file under 0 and edit it, so that the correct boundary names and conditions are set |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Running UDF with Supercomputer | roi247 | FLUENT | 4 | October 15, 2015 13:41 |
Suggestion for a new sub-forum at OpenFOAM's Forum | wyldckat | Site Help, Feedback & Discussions | 20 | October 28, 2014 09:04 |
[Commercial meshers] Fluent case to openfoam mesh | Mat_fr | OpenFOAM Meshing & Mesh Conversion | 8 | August 29, 2012 08:10 |
[Gmsh] 2D Mesh Generation Tutorial for GMSH | aeroslacker | OpenFOAM Meshing & Mesh Conversion | 12 | January 19, 2012 03:52 |
fluent add additional zones for the mesh file | SSL | FLUENT | 2 | January 26, 2008 11:55 |