|
[Sponsors] |
|
October 24, 2007, 04:48 |
Import fluent mesh
|
#1 |
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 |
|
October 24, 2007, 07:46 |
If I understand right, you don
|
#2 |
New Member
Gabriel Barroso
Join Date: Mar 2009
Posts: 23
Rep Power: 17 |
If I understand right, you don't have the fluent.msh file in ascii?
|
|
October 24, 2007, 07:53 |
no
i only have .fvuns format
|
#3 |
Guest
Posts: n/a
|
no
i only have .fvuns format fieldview and .case and .geo format ensight |
|
October 24, 2007, 08:03 |
Do you have ICEM, can you read
|
#4 |
New Member
Gabriel Barroso
Join Date: Mar 2009
Posts: 23
Rep Power: 17 |
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 |
|
October 24, 2007, 08:09 |
no i don't have ICEM,i only go
|
#5 |
Guest
Posts: n/a
|
no i don't have ICEM,i only got fluent but i can't write .msh file
thank regards |
|
October 24, 2007, 08:11 |
Sorry, no idea :-(
|
#6 |
New Member
Gabriel Barroso
Join Date: Mar 2009
Posts: 23
Rep Power: 17 |
Sorry, no idea :-(
|
|
October 24, 2007, 08:14 |
Write the .cas file in ascii f
|
#7 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
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 |
|
October 24, 2007, 08:18 |
If your EnSight geo file is AS
|
#8 |
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,689
Rep Power: 40 |
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. |
|
October 24, 2007, 09:26 |
My file is ensight binary
i
|
#9 |
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 |
|
January 8, 2008, 16:27 |
Hi everybody,
i would like
|
#10 |
New Member
soufymer
Join Date: Mar 2009
Posts: 5
Rep Power: 17 |
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 |
|
January 8, 2008, 23:20 |
have you tried fluent3DMeshtoF
|
#11 |
Member
vof_user
Join Date: Mar 2009
Posts: 67
Rep Power: 17 |
have you tried fluent3DMeshtoFoam and checked.
|
|
January 9, 2008, 01:41 |
some important notes:
- wri
|
#12 |
Member
Christian Winkler
Join Date: Mar 2009
Location: Mannheim, Germany
Posts: 63
Rep Power: 17 |
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 |
|
August 29, 2008, 20:53 |
I need to know what you think
|
#13 |
Member
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 17 |
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 |
|
June 1, 2010, 15:32 |
fluentMeshToFoam
|
#14 |
New Member
sasan
Join Date: Feb 2010
Posts: 5
Rep Power: 16 |
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. |
|
October 10, 2010, 23:48 |
fluentmesh to foam
|
#15 |
Senior Member
Tarak
Join Date: Aug 2010
Location: State College, PA
Posts: 111
Rep Power: 15 |
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. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Mesh Changing When Importing from Fluent | russel60 | OpenFOAM Running, Solving & CFD | 0 | February 15, 2019 16:43 |
Transfer of mesh from Meshing to Fluent destroys the mesh | balrog_f | FLUENT | 9 | July 28, 2018 10:02 |
[ANSYS Meshing] Combine solid mesh generated in workbench mesh and fluid mesh in fluent meshing ? | RPjack | ANSYS Meshing & Geometry | 2 | August 27, 2015 09:33 |
[ANSYS Meshing] Import Plot3D mesh to fluent | nw_ds | ANSYS Meshing & Geometry | 0 | May 26, 2015 11:52 |
[Commercial meshers] Import mesh with internal face from Fluent to openfoam 2.1.1 | neeraj | OpenFOAM Meshing & Mesh Conversion | 1 | April 29, 2013 03:54 |