CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... (http://www.cfd-online.com/Forums/openfoam-meshing-other/)
-   -   Problem with Mesh conversion Gambit msh Foam (http://www.cfd-online.com/Forums/openfoam-meshing-other/61679-problem-mesh-conversion-gambit-msh-foam.html)

Rachid BANNARI (Bannari) February 22, 2005 11:17

I have a problem to convert .
 
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

Mattijs Janssens (Mattijs) February 22, 2005 11:39

You will not get a blockMeshD
 
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

BANNARI (Bannari) February 22, 2005 13:13

indeed the changes had place i
 
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

Henry Weller (Henry) February 22, 2005 13:18

With what command?
 
With what command?

Niklas Nordin (Niklas) February 22, 2005 13:37

Hi, Sorry if this sounds s
 
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

Hrvoje Jasak (Hjasak) February 22, 2005 13:39

Easy Tiger, Fluent files w
 
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

BANNARI (Bannari) February 22, 2005 14:14

I have some results in Fluen
 
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

Henry Weller (Henry) February 22, 2005 14:50

>after that >>blochMesh ...
 
>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.

BANNARI (Bannari) February 22, 2005 14:56

ok so how can I visualise m
 
ok
so how can I visualise my converted mesh
thank you

Henry Weller (Henry) February 22, 2005 15:02

Use paraFoam
 
Use paraFoam

tchavdarov March 12, 2005 01:54

Here is my issue with a mesh o
 
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

hjasak March 12, 2005 02:55

Your cyclic faces are out of o
 
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

mattijs March 12, 2005 04:18

It is called couplePatches. It
 
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

anne May 30, 2006 06:30

Hello, I am trying to use a
 
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

lakeat February 11, 2008 23:54

Yes, I got the same message. H
 
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 zonehttp://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif71 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]http://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif12.733 -15.2763 5)
half1Ctrs[0]http://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif0.407746 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

lakeat February 12, 2008 00:50

I've got it working now. Fo
 
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!

yousuf May 28, 2008 00:49

i'm also geeting this message.
 
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 zonehttp://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif15174 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 zonehttp://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif15158 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

cwang5 January 15, 2009 02:28

I am wondering if the couplePa
 
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

kati January 15, 2009 04:28

couplePatches has been integra
 
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

cwang5 January 15, 2009 04:40

Thanks Kati, I checked the
 
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


All times are GMT -4. The time now is 04:38.