CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

fluentMeshToFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 27, 2009, 11:21
Unhappy fluentMeshToFoam
  #1
Member
 
Stefan
Join Date: Jun 2009
Posts: 67
Rep Power: 8
preibie is on a distinguished road
Hallo,

I want to convert a Fluent msh File to OpenFoam. By using fluentMeshToFoam is a mistake (show below). Have anybody an Idea how I can concert a Fluent msh file to openFoam.

Thanks


/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : fluentMeshToFoam brick.msh
Date : Jul 27 2009
Time : 17:15:35
Host : Fluent64-2
PID : 29859
Case : /home/preibisch/OpenFOAM/preibisch-1.5/run/brick
nProcs : 1

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Dimension of grid: 3
Number of points: 15410
Reading points
number of faces: 155152
Reading mixed faces
Reading mixed faces
8(c6d 18d8 4 3Reading mixed faces
Reading mixed faces
Reading mixed faces
Number of cells: 74714
Other readCellGroupData: 2 1 123da 1 2
Reading uniform cells
Read zone1:2 name:fluid patchTypeID:fluid
Reading zone data
Read zone1:3 nameeriodic.1_shadow patchTypeID:shadow
Reading zone data
Read zone1:4 nameeriodic.1 patchTypeIDeriodic
Reading zone data
Read zone1:5 nameut patchTypeID:wall
Reading zone data
Read zone1:6 name:inner patchTypeID:wall
Reading zone data
Read zone1:8 name:default-interior patchTypeID:interior
Reading zone data


FINISHED LEXING


dimension of grid: 3
Creating shapes for 3-D cells
Building patch-less mesh...--> FOAM Warning :
From function polyMesh:olyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 576
Found 11448 undefined faces in mesh; adding to default patch.
done.

Building boundary and internal patches.
Creating patch 0 for zone: 3 start: 1 end: 3180 type: shadow name: periodic.1_shadow


fluent patch type shadow not recognised.#0 Foam::error:rintStack(Foam::Ostream&) in "/home/preibisch/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/preibisch/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 main in "/home/preibisch/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/fluentMeshToFoam"
#3 __libc_start_main in "/lib64/libc.so.6"
#4 __gxx_personality_v0 in "/home/preibisch/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/fluentMeshToFoam"


From function fluentToFoam::main(int argc, char *argv[])
in file fluentMeshToFoam.L at line 1337.

FOAM aborting
preibie is offline   Reply With Quote

Old   July 27, 2009, 11:38
Default
  #2
Member
 
Julien Schaguene
Join Date: Apr 2009
Location: France
Posts: 55
Rep Power: 8
Schag is on a distinguished road
Hi,

it seems that OpenFOAM doesn't recognize the type Shadow from Fluent (Gambit?).
You can have a look at lines 1260 to 1340 of fluentMeshToFoam.L (thank you Henrik to make me open this file earlier today), shadow is not an option for a patch from fluent to openFoam.
What does "shadow" means for you? Is it an internal face, a patch, fan, wall...?

Regards,

Julien
Schag is offline   Reply With Quote

Old   July 28, 2009, 02:54
Default
  #3
Member
 
Stefan
Join Date: Jun 2009
Posts: 67
Rep Power: 8
preibie is on a distinguished road
it is an internal wall i think, but how can I fix that problem?
preibie is offline   Reply With Quote

Old   July 28, 2009, 03:11
Default
  #4
Member
 
Julien Schaguene
Join Date: Apr 2009
Location: France
Posts: 55
Rep Power: 8
Schag is on a distinguished road
First, I don't think fluentMeshToFoam keeps internal faces (it didn't ever work for me, but I have to confess that I was not very persistent). Do you really need them?

Then, in Gambit, when creating boundary conditions, just choose another type than shadow (in this case, internal for example). If you don't need them, just don't mark them as boundary conditions.

Hope it helps...

Julien
Schag is offline   Reply With Quote

Old   July 28, 2009, 04:00
Default
  #5
Member
 
Stefan
Join Date: Jun 2009
Posts: 67
Rep Power: 8
preibie is on a distinguished road
I found the "mistake": when you define a pair of two walls for periodic boundary conditions on gambit one of this two walls is a shadow wall. I defined them to a simple wall and fluentMeshToFoam run without problems.

But how I define a periodic boundary condition?
preibie is offline   Reply With Quote

Old   July 28, 2009, 04:02
Default
  #6
Member
 
Julien Schaguene
Join Date: Apr 2009
Location: France
Posts: 55
Rep Power: 8
Schag is on a distinguished road
Are you speaking about cyclic BC?
Schag is offline   Reply With Quote

Old   July 28, 2009, 04:19
Default
  #7
Member
 
Stefan
Join Date: Jun 2009
Posts: 67
Rep Power: 8
preibie is on a distinguished road
I think yes. When a fluid element fly out of the domain by crossing one of this two walls. He comes in the domain again by crossing the other wall. Is this the definition for cyclic BC?
preibie is offline   Reply With Quote

Old   July 28, 2009, 04:31
Default
  #8
Member
 
Julien Schaguene
Join Date: Apr 2009
Location: France
Posts: 55
Rep Power: 8
Schag is on a distinguished road
I'm not familiar with cyclic BC, but I think this is the definition yes.

Maybe you should take a look there:
http://www.cfd-online.com/Forums/ope...-boundary.html

This topic seems to deal with your problem. I cannot do much more, sorry, I did not use cyclic BC yet. Good luck.
Schag is offline   Reply With Quote

Old   October 4, 2012, 15:13
Default
  #9
Senior Member
 
sivakumar selvaraju
Join Date: Mar 2009
Location: Cape Town - South Africa
Posts: 186
Rep Power: 8
sivakumar is on a distinguished road
Send a message via Skype™ to sivakumar
Hi there,
I am trying to mesh the fan passage in gambit.
I dont know what is the problem in the mesh, its giving the following error.

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Dimension of grid: 3
Number of points: 808911
Reading points
number of faces: 2358500
Reading mixed faces
Reading mixed faces
8(fa1 1f40 4 3Reading mixed faces
Reading mixed faces
8(4651 6d60 6 5Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Reading mixed faces
Number of cells: 775000
Other readCellGroupData: 2 1 bd358 1 4
Reading uniform cells
Read zone1:2 name:fluid patchTypeID:fluid
Reading zone data
Read zone1:3 nameeriodic_1_shadow patchTypeID:shadow
Reading zone data
Read zone1:4 nameeriodic_1 patchTypeIDeriodic
Reading zone data
Read zone1:5 nameeriodic_2_shadow patchTypeID:shadow
Reading zone data
Read zone1:6 nameeriodic_2 patchTypeIDeriodic
Reading zone data
Read zone1:7 name:top_3 patchTypeID:wall
Reading zone data
Read zone1:8 name:top_2 patchTypeID:wall
Reading zone data
Read zone1:9 name:top_1 patchTypeID:wall
Reading zone data
Read zone1:10 name:center_2 patchTypeID:wall
Reading zone data
Read zone1:11 name:center_1 patchTypeID:wall
Reading zone data
Read zone1:12 name:fan patchTypeID:fan
Reading zone data
Read zone1:13 nameutlet patchTypeIDressure-outlet
Reading zone data
Read zone1:14 name:inlet patchTypeID:velocity-inlet
Reading zone data
Read zone1:16 name:default-interior patchTypeID:interior
Reading zone data


FINISHED LEXING


dimension of grid: 3
Creating shapes for 3-D cells
Building patch-less mesh...--> FOAM Warning :
From function polyMesh:olyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 614
Found 67000 undefined faces in mesh; adding to default patch.
done.

Building boundary and internal patches.
Creating patch 0 for zone: 3 start: 1 end: 4000 type: shadow name: periodic_1_shadow


--> FOAM FATAL ERROR:
fluent patch type shadow not recognised.

From function fluentToFoam::main(int argc, char *argv[])
in file fluentMeshToFoam.L at line 1344.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/cerecam/OpenFOAM/OpenFOAM-2.0.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/cerecam/OpenFOAM/OpenFOAM-2.0.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2
in "/home/cerecam/OpenFOAM/OpenFOAM-2.0.1/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
#3 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#4
in "/home/cerecam/OpenFOAM/OpenFOAM-2.0.1/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
Aborted (core dumped)

I dont know what is the shadow, I didnt define anything like that.

can you please help me sort out this issue.

thanks and regards,
Siva
sivakumar is offline   Reply With Quote

Old   October 4, 2012, 18:02
Default
  #10
New Member
 
Francesco
Join Date: Jun 2012
Location: Rome, Italy
Posts: 23
Rep Power: 5
Bombolati is on a distinguished road
Hi Siva, in my mesh the shadow patch was a patch that was coupled with an other one. For example you design a cylinder,to reduce the dimension of the file you do a clove of this cylinder. Now you have two sides that were the same surface before you do the clove,for example L1. In the mesher (as gambit) you assign a periodic boundary condition to L1 and its "brother". When you convert the mesh, OF sees L1 and L1_shadow. I hope that this hint will be useful.
Bombolati is offline   Reply With Quote

Old   October 5, 2012, 03:44
Default
  #11
Senior Member
 
sivakumar selvaraju
Join Date: Mar 2009
Location: Cape Town - South Africa
Posts: 186
Rep Power: 8
sivakumar is on a distinguished road
Send a message via Skype™ to sivakumar
Hi Bombolati,
Thanks for your reply, i got the information regarding the shadow.
If it gives the full converted mesh then, i can edit the necessary files. but now its not converting the whole mesh, its giving the fatal error in between and it stopped converting the mesh.

see the message,

--> FOAM FATAL ERROR:
fluent patch type shadow not recognised.

From function fluentToFoam::main(int argc, char *argv[])
in file fluentMeshToFoam.L at line 1344.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/home/cerecam/OpenFOAM/OpenFOAM-2.0.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/cerecam/OpenFOAM/OpenFOAM-2.0.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2
in "/home/cerecam/OpenFOAM/OpenFOAM-2.0.1/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
#3 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#4
in "/home/cerecam/OpenFOAM/OpenFOAM-2.0.1/platforms/linux64GccDPOpt/bin/fluentMeshToFoam"
Aborted (core dumped)

what should i do now? please give me your idea.

Thanks and regards,
Siva
sivakumar is offline   Reply With Quote

Old   October 5, 2012, 03:54
Default
  #12
Member
 
Join Date: Jun 2011
Posts: 52
Rep Power: 6
blacksquirrel is on a distinguished road
Hello Siva,

You can try to simplify your boundary conditions in gambit, like using only velocity inlet, pressure outlet and wall for everything else (e.g. periodic boundarys).

And after you converted the mesh with Fluent(3D)MeshToFoam you can use the createPatch utility to create the patches you need from your "walls".
blacksquirrel is offline   Reply With Quote

Old   October 5, 2012, 04:01
Default
  #13
Senior Member
 
sivakumar selvaraju
Join Date: Mar 2009
Location: Cape Town - South Africa
Posts: 186
Rep Power: 8
sivakumar is on a distinguished road
Send a message via Skype™ to sivakumar
Hi,
Thanks, nice idea. i will try now, then i will post result

thanks.

Siva
sivakumar is offline   Reply With Quote

Old   October 5, 2012, 06:47
Default
  #14
Senior Member
 
sivakumar selvaraju
Join Date: Mar 2009
Location: Cape Town - South Africa
Posts: 186
Rep Power: 8
sivakumar is on a distinguished road
Send a message via Skype™ to sivakumar
Hi blacksquirrel,
As per you idea, I have generated the mesh with wall boundary condition.
Now i wan to use the createPatch utility, can you please explain it.
In which folder i need to execute the command?
sivakumar is offline   Reply With Quote

Old   October 5, 2012, 07:18
Default
  #15
Member
 
Join Date: Jun 2011
Posts: 52
Rep Power: 6
blacksquirrel is on a distinguished road
Hello Siva,

You execute createPatch from your "case" folder. It reads everything from the createPatchDict (http://openfoamwiki.net/index.php/CreatePatch) in the "case"/system folder.

What kind of boundaries do you want to create? Cyclic boundaries? I explained it in this thread:
http://www.cfd-online.com/Forums/ope...patchdict.html
blacksquirrel is offline   Reply With Quote

Old   October 5, 2012, 08:34
Default
  #16
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!
Quote:
Originally Posted by blacksquirrel View Post
What kind of boundaries do you want to create? Cyclic boundaries? I explained it in this thread:
http://www.cfd-online.com/Forums/ope...patchdict.html
FYI, I've moved that thread to here: Usage of createPatchDict - I think it's easier to find it in the future, if it's located in the right sub-forum

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   October 5, 2012, 10:28
Default
  #17
Senior Member
 
sivakumar selvaraju
Join Date: Mar 2009
Location: Cape Town - South Africa
Posts: 186
Rep Power: 8
sivakumar is on a distinguished road
Send a message via Skype™ to sivakumar
Hi there,
I have converted the .msh in to foam.
I got 2 errors,
firstly as follows,

--> FOAM FATAL ERROR:
face 6439 area does not match neighbour by 0.0103693% -- possible face ordering problem.
patch:OLR0 my area:0.000199448 neighbour area:0.000199427 matching tolerance:0.0001
Mesh face:1370739 fc0.0966635 -0.0215988 0.729129)
Neighbour fc0.0967883 -0.5304 0.500736)
If you are certain your matching is correct you can increase the 'matchTolerance' setting in the patch dictionary in the boundary file.
Rerun with cyclic debug flag set for more information.

then I have increased the matchTolerance 0.0001 to 0.001
then executed paraFoam

after that I am getting the error as follows,



--> FOAM FATAL ERROR:
More than six unsigned transforms detected:
6(((0 0 0) (1 1.57813e-06 -0.000193506 -0.000137946 0.707107 -0.707107 0.000135714 0.707107 0.707107) 1) ((0 0 0) (0.999999 3.64383e-05 -0.00152133 -0.00110151 0.707109 -0.707104 0.00104998 0.707105 0.707108) 1) ((0 0 0) (0.999996 7.7863e-05 -0.00275828 -0.00200544 0.707113 -0.707098 0.00189536 0.7071 0.707111) 1) ((0 0 0) (0.999992 0.000140037 -0.00401223 -0.00293604 0.70712 -0.707087 0.00273811 0.707093 0.707115) 1) ((0 0 0) (1 -0.000137946 0.000135714 1.57813e-06 0.707107 0.707107 -0.000193506 -0.707107 0.707107) 1) ((0 0 0) (0.999999 -0.00110151 0.00104998 3.64383e-05 0.707109 0.707105 -0.00152133 -0.707104 0.707108) 1))

From function void Foam::globalIndexAndTransform::determineTransforms ()
in file primitives/globalIndexAndTransform/globalIndexAndTransform.C at line 225.

can you guys help me.

Thanks,
Siva
sivakumar is offline   Reply With Quote

Old   October 8, 2012, 03:40
Default
  #18
Member
 
Join Date: Jun 2011
Posts: 52
Rep Power: 6
blacksquirrel is on a distinguished road
hello Siva,

I assume these errors occur while using the createPatch utility?

Then look in your createPatchDict. What is written in the "transform" options?
(e.g.
transform rotational;
rotationAxis (1 0 0);
rotationCentre (0 0 0); )

You maybe don't need to transform anything, so you can delete/comment the transform options.
blacksquirrel is offline   Reply With Quote

Old   October 8, 2012, 07:10
Default
  #19
Senior Member
 
sivakumar selvaraju
Join Date: Mar 2009
Location: Cape Town - South Africa
Posts: 186
Rep Power: 8
sivakumar is on a distinguished road
Send a message via Skype™ to sivakumar
Dear blacksquirrel,
I am giving you the createPatchDict and my boundary file.
please have a look.
my createPatchDict :

// Patches to create.
patches
(
{
// Name of new patch
name ILR0;

// Dictionary to construct new patch from
patchInfo
{
type cyclic;
neighbourPatch ILR1;

// Optional non-default tolerance to be able to define cyclics
// on bad meshes
matchTolerance 1E-3;
}

// How to construct: either from 'patches' or 'set'
constructFrom patches;

// If constructFrom = patches : names of patches. Wildcards allowed.
patches (ILR_shadow);

}
{
// Name of new patch
name ILR1;

// Dictionary to construct new patch from
patchInfo
{
type cyclic;
neighbourPatch ILR0;

// Optional non-default tolerance to be able to define cyclics
// on bad meshes
matchTolerance 1E-3;
}

// How to construct: either from 'patches' or 'set'
constructFrom patches;

// If constructFrom = patches : names of patches. Wildcards allowed.
patches (ILR);

}
{
// Name of new patch
name OLR0;

// Dictionary to construct new patch from
patchInfo
{
type cyclic;
neighbourPatch OLR1;

// Optional non-default tolerance to be able to define cyclics
// on bad meshes
matchTolerance 1E-3;
}

// How to construct: either from 'patches' or 'set'
constructFrom patches;

// If constructFrom = patches : names of patches. Wildcards allowed.
patches (OLR_shadow);

}
{
// Name of new patch
name OLR1;

// Dictionary to construct new patch from
patchInfo
{
type cyclic;
neighbourPatch OLR0;

// Optional non-default tolerance to be able to define cyclics
// on bad meshes
matchTolerance 1E-3;
}

// How to construct: either from 'patches' or 'set'
constructFrom patches;

// If constructFrom = patches : names of patches. Wildcards allowed.
patches (OLR);

}
);

// ************************************************** *********************** /

my boundary file is:

FoamFile
{
version 2.0;
format ascii;
class polyBoundaryMesh;
location "1/polyMesh";
object boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

12
(
fan
{
type wall;
nFaces 2800;
startFace 1357300;
}
top2
{
type wall;
nFaces 5600;
startFace 1360100;
}
top1
{
type wall;
nFaces 800;
startFace 1365700;
}
top0
{
type wall;
nFaces 2800;
startFace 1366500;
}
center1
{
type wall;
nFaces 5600;
startFace 1369300;
}
center0
{
type wall;
nFaces 2800;
startFace 1374900;
}
outlet
{
type patch;
nFaces 2000;
startFace 1377700;
}
inlet
{
type patch;
nFaces 2000;
startFace 1379700;
}
ILR0
{
type cyclic;
nFaces 3500;
startFace 1381700;
matchTolerance 0.001;
neighbourPatch ILR1;
}
ILR1
{
type cyclic;
nFaces 3500;
startFace 1385200;
matchTolerance 0.001;
neighbourPatch ILR0;
}
OLR0
{
type cyclic;
nFaces 7000;
startFace 1388700;
matchTolerance 0.001;
neighbourPatch OLR1;
}
OLR1
{
type cyclic;
nFaces 7000;
startFace 1395700;
matchTolerance 0.001;
neighbourPatch OLR0;
}
)

// ************************************************** *********************** //

please help me to sort out this problem,

And what are the further steps I need to follow?

Thank you,
Siva
sivakumar is offline   Reply With Quote

Old   October 8, 2012, 07:41
Default
  #20
Member
 
Join Date: Jun 2011
Posts: 52
Rep Power: 6
blacksquirrel is on a distinguished road
I'm sorry, for me those two files look fine. Can you post a picture of your gambit mesh? Your error message said, that ILR and ILR_shadow (or OLR with shadow) doesn't match exactly. I had a similar error once and had to rotate one patch to match the other one.
blacksquirrel 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
FluentMeshToFoam segmentation fault gtg627e OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 6 June 27, 2011 10:34
Converting a mesh with splitted cells using fluentMeshToFoam jlpelerin OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 4 April 25, 2011 16:56
a probem with fluentMeshToFoam wei_wu OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 3 June 13, 2009 10:22
Z direction thickness control when using fluentMeshToFoam to extrude 2D mesh wei_wu OpenFOAM Running, Solving & CFD 2 February 1, 2009 05:15
Z direction thickness control by using fluentMeshToFoam wei_wu OpenFOAM Running, Solving & CFD 0 January 31, 2009 14:51


All times are GMT -4. The time now is 16:14.