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

Problem with Mesh conversion Gambit msh Foam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 22, 2005, 12:17
Default I have a problem to convert .
  #1
Rachid BANNARI (Bannari)
Guest
 
Posts: n/a
I have a problem to convert .msh file (obtained by
Gambit) to foam file. In fact the execution of the command
fluentMeshToFoam I obtained that the mesh created. when I chek, the file
blockMeshDict doasn't exist. with an other .msh file I did not have
this problem, but a FOAMFATAL ERROR... (problem in
Istream.C file). I hope know if somone
success this conversion, and how can I do that?
thanks
  Reply With Quote

Old   February 22, 2005, 12:39
Default You will not get a blockMeshD
  #2
Mattijs Janssens (Mattijs)
Guest
 
Posts: n/a
You will not get a blockMeshDict. A blockMeshDict is the input file for OpenFOAM's own block mesher.

The fluentMeshToFoam will have written the polyMesh files (points, faces, cells).

Mattijs
  Reply With Quote

Old   February 22, 2005, 14:13
Default indeed the changes had place i
  #3
BANNARI (Bannari)
Guest
 
Posts: n/a
indeed the changes had place in points, faces, cells but with the command I have
--> FOAM FATAL ERROR : Cannot find mesh description file
"constant/polyMesh/blockMeshDict" or
"constant/polyMesh/meshDescription" or
"constant/mesh/meshDescription"
thank you
  Reply With Quote

Old   February 22, 2005, 14:18
Default With what command?
  #4
Henry Weller (Henry)
Guest
 
Posts: n/a
With what command?
  Reply With Quote

Old   February 22, 2005, 14:37
Default Hi, Sorry if this sounds s
  #5
Niklas Nordin (Niklas)
Guest
 
Posts: n/a
Hi,

Sorry if this sounds stupid, but why are
you running the fluent converter on what I
understand is a gambit mesh?

How about using gambitToFoam instead?

N
  Reply With Quote

Old   February 22, 2005, 14:39
Default Easy Tiger, Fluent files w
  #6
Hrvoje Jasak (Hjasak)
Guest
 
Posts: n/a
Easy Tiger,

Fluent files will have the .msh and .cas extensions and you convert them with fluentMeshToFoam. Gambit files have the .neu extension and you use the gambitToFoam converter.

Hrv
  Reply With Quote

Old   February 22, 2005, 15:14
Default I have some results in Fluen
  #7
BANNARI (Bannari)
Guest
 
Posts: n/a
I have some results in Fluent. and I want to run the same problem in Foam to compare. To do that I want to transform my mesh file from fluent to Foam but unfortunately I do not succeeded that, even I follow the instructions in Foam manual

I convert this file (.msh) with:
>fluentMeshToFoamroot casename file.msh
after that
>blochMesh ...
in the points, faces, cells files I have the informations but I can't view the mesh in paraview

P.S. I'm new user of Foam
  Reply With Quote

Old   February 22, 2005, 15:50
Default >after that >>blochMesh ...
  #8
Henry Weller (Henry)
Guest
 
Posts: n/a
>after that
>>blochMesh ...

Why are you running blockMesh after fluentMeshToFoam? It makes no sense; blockMesh generates a mesh from a blockMeshDict mesh description file and has absolutely nothing to do with the mesh converters.
  Reply With Quote

Old   February 22, 2005, 15:56
Default ok so how can I visualise m
  #9
BANNARI (Bannari)
Guest
 
Posts: n/a
ok
so how can I visualise my converted mesh
thank you
  Reply With Quote

Old   February 22, 2005, 16:02
Default Use paraFoam
  #10
Henry Weller (Henry)
Guest
 
Posts: n/a
Use paraFoam
  Reply With Quote

Old   March 12, 2005, 02:54
Default Here is my issue with a mesh o
  #11
New Member
 
tchavdarov's Avatar
 
Join Date: Mar 2009
Posts: 19
Rep Power: 8
tchavdarov is on a distinguished road
Here is my issue with a mesh obtained by a third party from Gridgen, exported in Fluent .cas file (I was told that) and converted to polyMesh by fluentMeshToFoam:

No errors on outut from fluentMeshToFoam:

dimension of grid: 3
Creating shapes for 3-D cells
Creating patch for zone: 3 start: 1 end: 189360 type: interior name: interior-3
Patch 3 contains solid or internal faces. Not added to boundary
Creating patch for zone: 4 start: 189361 end: 190440 type: wall name: side1-4
Creating patch for zone: 5 start: 190441 end: 192240 type: wall name: side3-5
Creating patch for zone: 6 start: 192241 end: 194400 type: inlet-vent name: inlet-vent-6
Creating patch for zone: 7 start: 194401 end: 196560 type: pressure-outlet name: pressure-outlet-7
Creating patch for zone: 8 start: 196561 end: 198360 type: wall name: side4-8
Creating patch for zone: 9 start: 198361 end: 199440 type: wall name: side2-9

Default patch type set to empty
Checking mesh
Writing mesh

End
================================================

Then I made a LES case similar to channel395 and run it. The following error occurs :

Create database
Create mesh for time = 0

--> FOAM FATAL ERROR : face 0 and 540 areas do not match by 187.749% -- possible face ordering problem

Function: cyclicFvPatch::makeWeights(scalarField& w) const
in file: meshes/fvMesh/fvPatches/derivedFvPatches/cyclicFvPatch/cyclicFvPatch.Cat line: 62.

FOAM aborting.

I apreaciate if someone can help. Could email the original .cas mesh file if let me know how to do so.

Thanks,
Boyko
tchavdarov is offline   Reply With Quote

Old   March 12, 2005, 03:55
Default Your cyclic faces are out of o
  #12
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Your cyclic faces are out of order - this is not picked up from the fluent file.

Mattijs has written a tool which automatically reorders cyclic patches - he'll probably be able to give you more detail...

Enjoy,

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

Old   March 12, 2005, 05:18
Default It is called couplePatches. It
  #13
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
It is called couplePatches. It does not need a dictionary and you can run it with just the root and case. It should either tell you that the 'coupled patch face ordering ok' or something about morphing the mesh and will write the new mesh to a new time directory.

Just move that polyMesh/ directory back to constant/ (and check by running couplePatches again that the faces are now correctly ordered)

Mattijs
mattijs is offline   Reply With Quote

Old   May 30, 2006, 06:30
Default Hello, I am trying to use a
  #14
Member
 
anne dejoan
Join Date: Mar 2009
Location: madrid, spain
Posts: 66
Rep Power: 8
anne is on a distinguished road
Hello,

I am trying to use a pipe line mesh (theadres) created from fluent. It is a .msh extension mesh file.

The converter fluenttofoam works apparently ok
(when I use checkMesh, nothing wrong is noticed).

However I have a problem with the cyclic
condition:

When I run icoFoam on my case I have the following error:

------------------------
-> FOAM FATAL ERROR : face 0 and 216 areas do not match by 3.49993% -- possible face ordering problem
From function cyclicFvPatch::makeWeights(scalarField& w) const
in file fvMesh/fvPatches/derivedFvPatches/cyclicFvPatch/cyclicFvPatch.C at line 58.
----------

So, after having consulted the forum I applied
the command couplePatches to my case BUT it doen't create any new correct time polymesh directory. I have the following message from couplePatches:


-----------------------------
Create time

Create polyMesh for time = 0

Using geometry to calculate face correspondence across coupled boundaries (processor, cyclic)
This will only work for cyclics if they are parallel or their rotation is defined across the origin

Mesh has coupled patches ...

Doing dummy mesh morph to correct face ordering ...
--> FOAM Serious Error :
From function cyclicPolyPatch::geometricOrder
in file meshes/polyMesh/polyPatches/derivedPolyPatches/cyclicPolyPatch/cyclicPolyPatch.C at line 541
patch:inlet : Patch inlet gets decomposed in two zones ofinequal size: 432 and 0
This means that the patch is either not two separate regions or one region where the angle between the different regions is not sufficiently sharp.
Please use topological matching or adapt the featureCos() setting
Continuing with incorrect face ordering from now on!
--> FOAM Serious Error :
From function cyclicPolyPatch::geometricOrder
in file meshes/polyMesh/polyPatches/derivedPolyPatches/cyclicPolyPatch/cyclicPolyPatch.C at line 541
patch:outlet : Patch outlet gets decomposed in two zones ofinequal size: 432 and 0
This means that the patch is either not two separate regions or one region where the angle between the different regions is not sufficiently sharp.
Please use topological matching or adapt the featureCos() setting
Continuing with incorrect face ordering from now on!
Mesh ordering ok. Nothing changed.
End
-------------------------------------


Thanks if someone can help me,

Anne
anne is offline   Reply With Quote

Old   February 12, 2008, 00:54
Default Yes, I got the same message. H
  #15
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
Yes, I got the same message. How could I fix it?

/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4.1 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : couplePatches . cylinder
Date : Feb 12 2008
Time : 03:38:18
Host : daniel-desktop
PID : 12053
Root : /home/daniel/OpenFOAM/daniel-1.4.1/run/tutorials/icoFoam
Case : cylinder
Nprocs : 1
Create time

Create polyMesh for time = 0

Using geometry to calculate face correspondence across coupled boundaries (processor, cyclic)
This will only work for cyclics if they are parallel or their rotation is defined across the origin

Mesh has coupled patches ...

Doing dummy mesh morph to correct face ordering ...
cyclicPolyPatch::order : Number of faces per zone71 71)
--> FOAM Serious Error :
From function cyclicPolyPatch::order(const primitivePatch&, labelList&, labelList&) const
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 726
patch:walls : Cannot match vectors to faces on both sides of patch
half0Ctrs[0]12.733 -15.2763 5)
half1Ctrs[0]0.407746 0.272448 5)
Please use topological matching or adapt the featureCos() setting
Continuing with incorrect face ordering from now on!
Mesh ordering ok. Nothing changed.
End
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   February 12, 2008, 01:50
Default I've got it working now. Fo
  #16
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 12
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
I've got it working now.

For i made a mistake in my *.geo file like this,
// Walls
Physical Surface("walls wall") = {98,186,216,296,516,494,480,450,146,344,370,388,40 6,252,234,172};

and now I modified it to:
// cylinder
Physical Surface("cylinder wall") = {146,344,370,388,406,252,234,172};

// Walls
Physical Surface("walls cyclic") = {98,186,216,296,516,494,480,450};

It works!
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   May 28, 2008, 00:49
Default i'm also geeting this message.
  #17
New Member
 
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8
yousuf is on a distinguished road
i'm also geeting this message. Can anyone help please


/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4.1 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : couplePatches /home/admin/intern/project cyclic_igv_case
Date : May 28 2008
Time : 10:00:49
Host : BGR-SW-99GML02
PID : 8679
Root : /home/admin/intern/project
Case : cyclic_igv_case
Nprocs : 1
Create time

Create polyMesh for time = 0

Using geometry to calculate face correspondence across coupled boundaries (processor, cyclic)
This will only work for cyclics if they are parallel or their rotation is defined across the origin

Mesh has coupled patches ...

Doing dummy mesh morph to correct face ordering ...
cyclicPolyPatch::order : Number of faces per zone15174 0)
cyclicPolyPatch::order : Writing half0 faces to OBJ file "wall1_periodic_half0_faces.obj"
cyclicPolyPatch::order : Writing half1 faces to OBJ file "wall1_periodic_half1_faces.obj"
cyclicPolyPatch::order : Writing half0 face centres to OBJ file "wall1_periodic_half0.obj"
cyclicPolyPatch::order : Writing half1 face centres to OBJ file "wall1_periodic_half1.obj"
--> FOAM Serious Error :
From function cyclicPolyPatch::order(const primitivePatch&, labelList&, labelList&) const
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 596
patch:wall1_periodic : Patch wall1_periodic gets decomposed in two zones ofinequal size: 15174 and 0
This means that the patch is either not two separate regions or one region where the angle between the different regions is not sufficiently sharp.
Please use topological matching or adapt the featureCos() setting
Continuing with incorrect face ordering from now on!
cyclicPolyPatch::order : Number of faces per zone15158 0)
cyclicPolyPatch::order : Writing half0 faces to OBJ file "wall2_periodic_half0_faces.obj"
cyclicPolyPatch::order : Writing half1 faces to OBJ file "wall2_periodic_half1_faces.obj"
cyclicPolyPatch::order : Writing half0 face centres to OBJ file "wall2_periodic_half0.obj"
cyclicPolyPatch::order : Writing half1 face centres to OBJ file "wall2_periodic_half1.obj"
--> FOAM Serious Error :
From function cyclicPolyPatch::order(const primitivePatch&, labelList&, labelList&) const
in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 596
patch:wall2_periodic : Patch wall2_periodic gets decomposed in two zones ofinequal size: 15158 and 0
This means that the patch is either not two separate regions or one region where the angle between the different regions is not sufficiently sharp.
Please use topological matching or adapt the featureCos() setting
Continuing with incorrect face ordering from now on!
Mesh ordering ok. Nothing changed.
End


Thanx in advance
yousuf is offline   Reply With Quote

Old   January 15, 2009, 03:28
Default I am wondering if the couplePa
  #18
Member
 
John Wang
Join Date: Mar 2009
Location: Singapore
Posts: 71
Rep Power: 8
cwang5 is on a distinguished road
I am wondering if the couplePatches command is included in the OF 1.5. I received the message "command not found" when I typed in couplePatches
cwang5 is offline   Reply With Quote

Old   January 15, 2009, 05:28
Default couplePatches has been integra
  #19
Member
 
Kati Laakkonen
Join Date: Mar 2009
Location: Espoo, Finland
Posts: 36
Rep Power: 8
kati is on a distinguished road
couplePatches has been integrated into createPatch, I think. Check release notes and/or User Guide, if I remember correctly there was some information about this issue.

Regards,
Kati
kati is offline   Reply With Quote

Old   January 15, 2009, 05:40
Default Thanks Kati, I checked the
  #20
Member
 
John Wang
Join Date: Mar 2009
Location: Singapore
Posts: 71
Rep Power: 8
cwang5 is on a distinguished road
Thanks Kati,

I checked the release note and found out about the integration, although the User guide still listed couplePatches as a separate function. I will look around the forum and see if I can get the createPatch to work correctly. Thanks

John
cwang5 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
Problem in running mesh imported from fluent to foam vishal OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 February 6, 2009 11:05
Problem converting gambit mesh to foam quartzian OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 1 September 29, 2008 18:29
Help: mesh conversion from Gambit to ICEM sarah_ron2002 FLUENT 2 April 5, 2008 01:53
Mesh Conversion Problem ms903 OpenFOAM Running, Solving & CFD 0 October 16, 2006 13:39
gambit icem conversion Tomasz Ochrymiuk FLUENT 2 March 14, 2000 04:02


All times are GMT -4. The time now is 03:40.