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

FluentMeshToFoam errorplease help me

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 1, 2006, 21:15
Default http://www.cfd-online.com/Open
  #1
New Member
 
Andy Cong
Join Date: Mar 2009
Posts: 17
Rep Power: 8
andycong is on a distinguished road

This is a 2D centeralpump model.
When simulate it in Fluent, I set with two fluid zones, one is stationary and the other is rotating(reference).
But when I import the mesh to OpenFOAM,
errors appears as following:
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.2 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : fluentMeshToFoam /home/andycong/OpenFOAM/andycong-1.2/run/tutorials/simpleFoam 2Dcenteralpump /home/andycong/2Dcenteralpump/pump_mesh.msh
Date : Mar 02 2006
Time : 09:09:01
Host : linux
PID : 10727
Root : /home/andycong/OpenFOAM/andycong-1.2/run/tutorials/simpleFoam
Case : 2Dcenteralpump
Nprocs : 1
Create time

Dimension of grid: 2
Number of points: 2567
Reading points
number of faces: 7263
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Number of cells: 4690
Reading uniform cells
Reading uniform cells
Reading zone data
Reading zone data
Reading zone data
Reading zone data
Reading zone data
Reading zone data
Reading zone data
Reading zone data


FINISHED LEXING


dimension of grid: 2
Grid is 2-D. Extruding in z-direction by: 14.4162
Creating shapes for 2-D cells
Creating patch for zone: 4 start: 1 end: 173 type: wall name: wall_3
Creating patch for zone: 5 start: 174 end: 263 type: wall name: wall_2
Creating patch for zone: 6 start: 264 end: 479 type: wall name: wall_1
Creating patch for zone: 7 start: 480 end: 498 type: outflow name: outlet
Creating patch for zone: 8 start: 499 end: 546 type: velocity-inlet name: inlet
Creating patch for zone: 10 start: 547 end: 7263 type: interior name: default-interior
Patch 10 contains solid or internal faces. Not added to boundary
Not adding to internal boundaries
Creating patch for front and back planes

Default patch type set to empty


--> FOAM FATAL ERROR : Trying to specify a boundary face 4(0 1 2568 2567) on the face on cell 399 which is either an internal face or already belongs to some other patch. This is face 0 of patch 1 named wall_2.

From function polyMesh::polyMesh
(
const IOobject& io,
const pointField& points,
const cellShapeList& cellsAsShapes,
const faceListList& boundaryFaces,
const wordList& boundaryPatchTypes,
const wordList& boundaryPatchNames,
const word& defaultBoundaryPatchType
)
in file meshes/polyMesh/createPolyMesh.C at line 375.

FOAM aborting

Aborted


Could anyone tell my what's the matter?
andycong is offline   Reply With Quote

Old   March 2, 2006, 06:42
Default I have the same problem. I thi
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
I have the same problem. I think it is related to the zone interfaces. Will be looking into it soon.
eugene is offline   Reply With Quote

Old   March 2, 2006, 14:37
Default Hi Andy, The only Fluent me
  #3
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Hi Andy,

The only Fluent mesh I have that has this problem consists of 13million cells. As you can imagine it is a bit hard to find the problem when the core dump takes 10 mins. Could I please have a copy of your mesh to do my testing on?
eugene is offline   Reply With Quote

Old   March 2, 2006, 20:46
Default Of cource it is OK. Now I wil
  #4
New Member
 
Andy Cong
Join Date: Mar 2009
Posts: 17
Rep Power: 8
andycong is on a distinguished road
Of cource it is OK.
Now I will attach it in this board.
Yestoday when I searched the messages before, I found it seemed that OpenFOAM does not support rotating machine, what do you think of that?

andycong is offline   Reply With Quote

Old   March 2, 2006, 20:51
Default Of cource it is OK. Now I wil
  #5
New Member
 
Andy Cong
Join Date: Mar 2009
Posts: 17
Rep Power: 8
andycong is on a distinguished road
Of cource it is OK.
Now I will attach it in this board.
Yestoday when I searched the messages before, I found it seemed that OpenFOAM does not support rotating machine, what do you think of that?
I have sent the mesh to your Email.
andycong is offline   Reply With Quote

Old   March 3, 2006, 08:27
Default Thanks, got it. Will post the
  #6
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Thanks, got it. Will post the fix when I find it.
eugene is offline   Reply With Quote

Old   March 7, 2006, 05:04
Default Hi Andy. As far as I can t
  #7
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,905
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi Andy.

As far as I can tell the problem seems to be that you have an 'interior wall' (see http://www.cfd-online.com/OpenFOAM_D...ges/1/364.html)

What you have to do is define it as INTERNAL in Gambit and export the mesh again. The wall becomes a faceSet. Then use splitMesh to construct two walls from that faceSet (there is a reference to a more detailed description in the thread I referenced above)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   March 7, 2006, 09:46
Default Thank you, I will try it.
  #8
New Member
 
Andy Cong
Join Date: Mar 2009
Posts: 17
Rep Power: 8
andycong is on a distinguished road
Thank you, I will try it.
andycong is offline   Reply With Quote

Old   March 7, 2006, 12:48
Default http://www.cfd-online.com/Ope
  #9
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
fluentMeshToFoam.L

This is still work in progress, but if you compile this instead of the default it will basically ignore internal boundaries (it will however writes them as faceSets). Should take care of all the problems posted above.
eugene is offline   Reply With Quote

Old   March 7, 2006, 12:52
Default Forgot to mention, this is for
  #10
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Forgot to mention, this is for 1.3, don't know if it will work for 1.2.
eugene is offline   Reply With Quote

Old   March 8, 2006, 04:14
Default Hi Eugene, I tried compilin
  #11
Member
 
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 8
melanie is on a distinguished road
Hi Eugene,

I tried compiling your file with 1.2.1, but I miss the repatchPolyTopoChanger.H file:

fluentMeshToFoam.L:56:36: error: repatchPolyTopoChanger.H: No such file or directory.
melanie is offline   Reply With Quote

Old   October 2, 2006, 10:50
Default Hi, I have read several for
  #12
Member
 
anne dejoan
Join Date: Mar 2009
Location: madrid, spain
Posts: 66
Rep Power: 8
anne is on a distinguished road
Hi,

I have read several forum messages about fluenMeahToFoam, and I am still quite confused.

I have a mesh created with fluent (.msh file)
with some of the boudaries declared as "interior".
Is is the first time I am using such
complex grid and I couldn't well understand the
steps to correctly apply fluentMeshToFoam.

First, compiling the above FluentMeshToFoam.L,
with OpenFoam 1-3 gives me the following error compilation:

----
fluentMeshToFoam.L: In function 'int main(int, char**)':
fluentMeshToFoam.L:1506: error: 'repatchPolyTopoChanger' was not declared in this scope
fluentMeshToFoam.L:1506: error: expected `;' before 'repatcher'
fluentMeshToFoam.L:1509: error: 'repatcher' was not declared in this scope
make: *** [Make/linuxGcc4DPOpt/fluentMeshToFoam.o] Error 1
----


Then, reading older forum messages I could
see that this could be dealt with splitMesh, but
it is still very confusing for me the steps to follow.


Thanks you if you could help,

PS: I have also simply applied the original version of the fluentMeshToFoam application and have the following message:

------------------------
Patch 23 contains solid or internal faces. Not added to boundary
Not adding to internal boundaries

Default patch type set to empty
Checking mesh
Writing mesh
Only one cell group: no set written


Anne
anne is offline   Reply With Quote

Old   October 3, 2006, 04:17
Default Hello again, Well I have fo
  #13
Member
 
anne dejoan
Join Date: Mar 2009
Location: madrid, spain
Posts: 66
Rep Power: 8
anne is on a distinguished road
Hello again,

Well I have found on wiki server the
information for dealing with interior cell.

BUT, the problem I have is that fluentMeshToFoam
does not create any faceSet, which means no
subdirectory sets in the constant/polyline/
so that when running splitMesh the name of the interior BC from Gambit is not given.


I have OpenFoam 1.3 from a linux binary package.


Why the subdirectory is not created ?
n my previous mail I made a copy of the
.msh file and there is one interior BC.


Thanks if you can help with this,


anne
anne is offline   Reply With Quote

Old   October 5, 2006, 05:05
Default What is the output of fluentMe
  #14
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,905
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
What is the output of fluentMeshToFoam?

In the distributed version if your "interior wall" has been set in Gambit to one of the types "interior", "internal", "solid", "fan", "radiator" or "porous-jump" a faceSet should be generated.

The last few lines of the MSH-file would be helpful to diagnose the problem(the ones starting with '(0 "Zones:")')
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   October 5, 2006, 08:28
Default Hello Bernhard, I have now
  #15
Member
 
anne dejoan
Join Date: Mar 2009
Location: madrid, spain
Posts: 66
Rep Power: 8
anne is on a distinguished road
Hello Bernhard,

I have now fixed the problem.
Having seen zones declared as "interior" in my .msh
I have read all th threat around.
However, they were not wall BC but, a zone that
is created by default with Gambit (it was the first I used it).

This zone is actually ignored by fluentMeshToFoam and I could run my job .


Thanks you for anser,


Anne
anne is offline   Reply With Quote

Old   November 3, 2007, 10:28
Default I use a membrane in my reactor
  #16
Member
 
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 8
danielle is on a distinguished road
I use a membrane in my reactor. It is an internal wall declared as INTERNAL, because I know that Foam don't accept a internal wall. In Fluent my mesh "reactor.msh" with two different zones is good. But when I convert it by fluentMeshToFoam I can't see the membrane (it is an internal wall
declared as INTERNAL). when I check for
faceSet in order to make the steps written
by "Bernhard Gschaider", I don't find it.
Please can you tel me what should I do step
by step?
1) fluentMeshToFoam . reactor reactor.msh (no problem)
2)??
3)??
Thanks
danielle is offline   Reply With Quote

Old   November 4, 2007, 11:05
Default Is it a 3D mesh? If so, set u
  #17
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 213
Rep Power: 9
fra76 is on a distinguished road
Is it a 3D mesh?
If so, set up as usual the Fluent case (with shadow surfaces), save the case in ascii and use the new "fluent3DMeshToFoam" (OpenFOAM 1.4.1) instead.
It should cope with this kind of meshes, now...

Francesco
fra76 is offline   Reply With Quote

Old   November 5, 2007, 05:47
Default Hi Danielle! In recent vers
  #18
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,905
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi Danielle!

In recent versions of fluentMeshToFoam you have to trigger the writing of sets (or zones) with the option -writeSets (or -writeZones). Have you done that? (It's usually a good idea to have a look at the available options with -h if a command does not behave as expected)

Bernhard

PS: liked the quotes around my name which suggest that I'm a fictitious person. Damn, my secret has been revealed ;)
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   November 5, 2007, 17:43
Default Hi Bernhard and Francesco, Th
  #19
Member
 
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 8
danielle is on a distinguished road
Hi Bernhard and Francesco,
Thank you for yours answers.
IT WORK NOW!
to Bernhard you are the real one in the Matrix :-)
danielle 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
Problems with fluentMeshToFoam su_junwei OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 1 February 25, 2010 09:40
Help Error fluentMeshToFoam loneboard OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 26 February 6, 2009 11:20
Problems with fluentMeshToFoam su_junwei OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 0 January 15, 2009 21:01
FluentMeshtoFoam error sukratu OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 4 March 7, 2008 23:54
FluentMeshToFoam no set written kian OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 May 25, 2007 12:04


All times are GMT -4. The time now is 21:36.