CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...

Conversion Fluent cas and dat file to OpenFoam

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

Like Tree1Likes
  • 1 Post By fra76

Reply
 
LinkBack Thread Tools Display Modes
Old   January 24, 2008, 10:00
Default Hi to all, sorry for my engli
  #1
matteo_gautero
Guest
 
Posts: n/a
Hi to all,
sorry for my english; I am a newbie of OpenFoam. I have obtained several results for my problem with Fluent and now I want to work with OpenFoam using intermediate results obtained in Fluent so I want to convert .cas and .dat files to Openfoam files. I tried to use fluentMeshToFoam: it works very well with .msh file but it doesn't work with .cas and .dat files. Is it possible? Do you know some utility which do that?

I want to use OpenFoam because I have the possibility to exploit a linux based pc with more RAM and so I can refine the mesh and I hope to obtain better results. So,is the tool to refine the mesh present in OpenFoam good? Is there an open source or freeware program for linux that do a refine of the mesh with a GUI?

Thaks in advance,
Matteo Gautero.
  Reply With Quote

Old   January 24, 2008, 11:00
Default Hi Matteo, I've used fluent
  #2
Member
 
Francesco Boschetto
Join Date: Mar 2009
Location: Italy
Posts: 56
Rep Power: 8
francesco_b is on a distinguished road
Hi Matteo,

I've used fluentMeshToFoam with some .cas files and everything was ok. Which kind of errors do you have?

Regards

Francesco
francesco_b is offline   Reply With Quote

Old   January 24, 2008, 11:28
Default Hi Matteo, when I use fluen
  #3
Senior Member
 
Florian Krause
Join Date: Mar 2009
Location: Munich
Posts: 103
Rep Power: 8
florian_krause is on a distinguished road
Hi Matteo,

when I use fluentMeshToFoam to convert a fluent .cas file (only mesh information) I have no problems.

But as I understand you correct, you want to convert your results (.cas and .dat files), than refine the mesh and run the job with OF?

This conversion would be a result and mesh conversion but fluentMeshToFoam only works for mesh conversion.

Somebody might correct me if I am worng regarding the fluentMeshToFoam converter

Regards,
Flo
florian_krause is offline   Reply With Quote

Old   January 24, 2008, 11:30
Default Hi Matteo, you must save case
  #4
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 215
Rep Power: 9
fra76 is on a distinguished road
Hi Matteo,
you must save case as ascii to let the compiler work. And if the mesh is 3D, my suggestion is to use fluent3DMeshToFoam.
About data file, I'm not aware about a converter... You can do the other way round, with foamDataToFluent (and foamMeshToFluent for the mesh).

Regards,

Francesco
solefire likes this.
fra76 is offline   Reply With Quote

Old   January 24, 2008, 11:46
Default Hi to all, thanks for your an
  #5
matteo_gautero
Guest
 
Posts: n/a
Hi to all,
thanks for your answers. Yes Florian, I want to convert my results and than refine the mesh and run the case with OF. When I try to do this, the message error is:

Embedded blocks in comment or unknown:
(
Found end of section in unknown

for several lines and then OF print this message:

Number of cells: 736991
number of faces: 1524374
Number of points: 148787
0Dimension of grid: 12
(Dimension of grid: 2
Dimension of grid: 1
bDimension of grid: 3
edfDimension of grid: 1
Dimension of grid: 2
0Dimension of grid: 13
(Dimension of grid: 3
Dimension of grid: 1
Dimension of grid: 622
Dimension of grid: 24
Dimension of grid: 3

after this, OF stops. I think it's not possible to convert a .cas file after some iterations. So I will redo the itereations with the refined grid obtained by the first mesh used in Fluent. Anyway, I will try to convert the first .cas file containing the boundary conditions imposed in Fluent without iterations.

Thanks,
Matteo Gautero.
  Reply With Quote

Old   January 24, 2008, 11:59
Default No, that's not true. There is
  #6
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 215
Rep Power: 9
fra76 is on a distinguished road
No, that's not true.
There is no conceptual difference between a Fluent cas file at "0" iterations and another one saved after a while.
With respect to the .msh file, the .cas file contains some extra fields that the converter usually skips.
As I wrote before, you MUST save your .cas file in ASCII, otherwise the converter doesn't work, and sometimes remains blocked without giving any outoput...

Francesco
fra76 is offline   Reply With Quote

Old   January 25, 2008, 03:49
Default Hi Francesco, you're right. I
  #7
matteo_gautero
Guest
 
Posts: n/a
Hi Francesco,
you're right. I tried to do what you said and it worked very well. The first messages were errors, i.e.

Embedded blocks in comment or unknown (
Found end of section in unknown )
Found end of section in unknown )

but then OF read the grid and I visualized it, it was ok.

Thanks to all for these explanations,
Matteo.
  Reply With Quote

Old   April 2, 2008, 10:36
Default I'm having problems processing
  #8
Member
 
Michael Rangitsch
Join Date: Mar 2009
Location: Midland, Michigan, USA
Posts: 31
Rep Power: 8
mrangitschdowcom is on a distinguished road
I'm having problems processing a .cas file that I had run fluent on and then did a grid refinement to tighten up the grid in the boundary layer (it resulted in hanging grids). fluent3dmeshtoFoam won't process it at all -- gives me an illegal block type 37 -- that's the label on a block of text in the case file which describes the fluent models used... Any ideas?
mrangitschdowcom is offline   Reply With Quote

Old   April 2, 2008, 10:59
Default As far as I know, grid refinem
  #9
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
As far as I know, grid refinement in fluent means hanging nodes, which fluent3DMeshToFoam doesn't know how to interpret.

Dragos
dmoroian is offline   Reply With Quote

Old   April 3, 2008, 02:32
Default fluent3DMeshToFoam is able to
  #10
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 215
Rep Power: 9
fra76 is on a distinguished road
fluent3DMeshToFoam is able to handle hanging nodes (fluentMeshToFoam isn't).
If it finds an unknown block, try to open the .cas file with a text editor end remove the corresponding lines. In a fluent mesh file, each block is enclosed by ( ).

Good luck!
fra76 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
PLOT3D file conversion Achilleas Main CFD Forum 4 February 2, 2011 21:32
Conversion file ideasToFoam georgette OpenFOAM Meshing & Mesh Conversion 0 August 8, 2006 20:18
PLOT3D file conversion Achilleas FLUENT 1 November 10, 2005 10:47
conversion of geo file from CFX-4 to fluent Min-Hua Wang FLUENT 2 January 26, 2000 18:01
Graphics File Conversion Christian Tollschein Main CFD Forum 3 May 5, 1999 03:02


All times are GMT -4. The time now is 23:32.