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

Import fluent mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 24, 2007, 04:48
Default Hi everybody i would like t
  #1
rengu
Guest
 
Posts: n/a
Hi everybody

i would like to import to OpenFOAM a mesh i've got in Fluent.
But i can only export Mesh to Ensight Case Gold,Fieldview Unstructured for 3d mesh
i can't export to 3D.msh ,only to 2D.msh for boundary and i don't know why
i can only export to this formats because there are polyhedral data
and if it's possible,will i get boundary conditions?
Anyone got an idea?

best regards
  Reply With Quote

Old   October 24, 2007, 07:46
Default If I understand right, you don
  #2
New Member
 
Gabriel Barroso
Join Date: Mar 2009
Posts: 23
Rep Power: 7
gabriel is on a distinguished road
If I understand right, you don't have the fluent.msh file in ascii?
gabriel is offline   Reply With Quote

Old   October 24, 2007, 07:53
Default no i only have .fvuns format
  #3
rengu
Guest
 
Posts: n/a
no
i only have .fvuns format fieldview and .case and .geo format ensight
  Reply With Quote

Old   October 24, 2007, 08:03
Default Do you have ICEM, can you read
  #4
New Member
 
Gabriel Barroso
Join Date: Mar 2009
Posts: 23
Rep Power: 7
gabriel is on a distinguished road
Do you have ICEM, can you read those formats into ICEM?

Sorry, but i usually write out a mesh from ICEM in Fluent format and then use fluentMeshToFoam or now new fluent3DMeshToFoam.

bests

Gabriel
gabriel is offline   Reply With Quote

Old   October 24, 2007, 08:09
Default no i don't have ICEM,i only go
  #5
rengu
Guest
 
Posts: n/a
no i don't have ICEM,i only got fluent but i can't write .msh file

thank regards
  Reply With Quote

Old   October 24, 2007, 08:11
Default Sorry, no idea :-(
  #6
New Member
 
Gabriel Barroso
Join Date: Mar 2009
Posts: 23
Rep Power: 7
gabriel is on a distinguished road
Sorry, no idea :-(
gabriel is offline   Reply With Quote

Old   October 24, 2007, 08:14
Default Write the .cas file in ascii f
  #7
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,733
Rep Power: 20
hjasak will become famous soon enough
Write the .cas file in ascii format and feed that into fluemtMeshToFoam. .msh file is a subset of the .cas but both should work fine with the converter I wrote.

Enjoy,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   October 24, 2007, 08:18
Default If your EnSight geo file is AS
  #8
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 774
Rep Power: 17
olesen will become famous soon enough
If your EnSight geo file is ASCII, it would be "fairly" easy (for you) to transform this into another ASCII mesh format.
The EnSight binary format would be more annoying.
olesen is offline   Reply With Quote

Old   October 24, 2007, 09:26
Default My file is ensight binary i
  #9
rengu
Guest
 
Posts: n/a
My file is ensight binary

i have writes a .cas file with fluent and convert it with fluent3DTofoam
i remove data unnecessary about the case that it don't recognyze and now i think it work
i can see my mesh in paraFoam

thanks a lot
best regards
  Reply With Quote

Old   January 8, 2008, 16:27
Default Hi everybody, i would like
  #10
New Member
 
soufymer
Join Date: Mar 2009
Posts: 5
Rep Power: 7
soufy is on a distinguished road
Hi everybody,

i would like to import to OpenFOAM a mesh that i have got in Fluent.
my file is in extetion .msh, i write the command ligne of fluemtMeshToFoam that's described in user's guide . by always i have problems. please i need a help to result this problem.

Where exactly i have to put the file .msh?

thanks a lot
soufy is offline   Reply With Quote

Old   January 8, 2008, 23:20
Default have you tried fluent3DMeshtoF
  #11
Member
 
a a saha
Join Date: Mar 2009
Posts: 67
Rep Power: 7
asaha is on a distinguished road
have you tried fluent3DMeshtoFoam and checked.
asaha is offline   Reply With Quote

Old   January 9, 2008, 01:41
Default some important notes: - wri
  #12
caw
Member
 
Christian Winkler
Join Date: Mar 2009
Location: Mannheim, Germany
Posts: 63
Rep Power: 7
caw is on a distinguished road
some important notes:

- write your fluent mesh as ascii (not binary. uncheck this in tgrid for export)!
- if you did that under windows you have to use dos2unix on that file
- as mentioned above, use fluent3DMeshtoFoam

regards
Christian
caw is offline   Reply With Quote

Old   August 29, 2008, 20:53
Default I need to know what you think
  #13
Member
 
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 7
danielle is on a distinguished road
I need to know what you think about my mesh. because I got the
good result by Fluent but don't work with O.F (very BAD
results)
Thanks
======================

Create time

Create polyMesh for time = constant

Time = constant

Mesh stats
points: 314704
edges: 1088715
faces: 1277556
internal faces: 1211202
cells: 492171
boundary patches: 13
point zones: 0
face zones: 0
cell zones: 2

Number of cells of each type:
hexahedra: 257595
prisms: 0
wedges: 0
pyramids: 4884
tet wedges: 0
tetrahedra: 229692
polyhedra: 0

Checking topology...
Boundary definition OK.
Point usage OK.
Upper triangular ordering OK.
Topological cell zip-up check OK.
Face vertices OK.
Number of identical duplicate faces (baffle faces): 11380
Face-face connectivity OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface
wall_cylin_int_Pied 22752 10349 multiply connected surface (shared edge)
wall_cylin_ext_G 8448 8624 ok (not multiply connected)
wall_capt_inlet_G 960 980 ok (not multiply connected)
inlet3 142 76 ok (not multiply connected)
inlet2 140 75 ok (not multiply connected)
outlet 25 33 ok (not multiply connected)
Wall_top 2653 2755 ok (not multiply connected)
inlet1 78 43 ok (not multiply connected)
wall_buttom 2669 1406 ok (not multiply connected)
wal_capt_inlet_F 873 685 ok (not multiply connected)
wall_cylin_inter 809 420 multiply connected surface (shared edge)
wall_cylin_ext_F 24925 19277 ok (not multiply connected)
wall_disc_inlet 1880 949 ok (not multiply connected)
<<Writing 10349 conflicting points to set nonManifoldPoints

Checking geometry...
Domain bounding box: (-0.139998 -0.139998 -8.61533e-16) (0.139998 0.139997 0.99)
Boundary openness (-1.08376e-17 2.8904e-17 -1.39722e-16) OK.
Max cell openness = 1.66038e-15 OK.
Max aspect ratio = 21.4331 OK.
Minumum face area = 1.22452e-07. Maximum face area = 8.99153e-05. Face area magnitudes OK.
Min volume = 2.74672e-11. Max volume = 2.55601e-07. Total volume = 0.0347228. Cell volumes OK.
Mesh non-orthogonality Max: 84.9996 average: 12.6589
*Number of severely non-orthogonal faces: 49.
Non-orthogonality check OK.
<<Writing 49 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 1.33507 OK.
Min/max edge length = 0.000218421 0.0171268 OK.
All angles in faces OK.
Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 0.995346
All face flatness OK.

Mesh OK.

End
danielle is offline   Reply With Quote

Old   June 1, 2010, 15:32
Default fluentMeshToFoam
  #14
New Member
 
sasan
Join Date: Feb 2010
Posts: 5
Rep Power: 6
ali805509 is on a distinguished road
Hi everyone,

I imported my mesh file to a FOAM mesh successfully using fluentMeshToFoam command.
I was wondering if there is any way to visualize the mesh file using Paraview. The problem I have is that after converting the mesh, blockMeshDict is not generated (all the other files like points and boundary are generated though) and therefore, bolckMesh command does not work.
ali805509 is offline   Reply With Quote

Old   October 10, 2010, 23:48
Default fluentmesh to foam
  #15
Senior Member
 
Tarak
Join Date: Aug 2010
Location: State College, PA
Posts: 105
Rep Power: 6
Tarak is on a distinguished road
hii Ali,

I think the BlockmeshDict file is for writing the code to generate the grids. But since have already generated the grid using other grid generator, blockmesh is not needed.
Tarak 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
Import cfx mesh into fluent Michele CFX 0 March 22, 2006 08:43
Import of Fluent Mesh jemteo CFX 1 February 19, 2006 19:33
Import ICEM Mesh to Fluent Fluent Beginner FLUENT 5 June 23, 2004 00:27
Mesh Import from Fluent to CFX sam CFX 3 July 2, 2003 10:26
Import 2D-3D mesh into FLUENT. vincent Main CFD Forum 3 April 12, 1999 04:31


All times are GMT -4. The time now is 01:50.