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/)
-   -   FluentMesh conversion problemwaiting for help (http://www.cfd-online.com/Forums/openfoam-meshing-other/61717-fluentmesh-conversion-problemwaiting-help.html)

waynezw0618 November 26, 2006 09:41

dear everyone, i have a flue
 
dear everyone,
i have a fluent .msh file when i use fluentMeshToFoam to change the mesh to Foam. it is said :



FINISHED LEXING


Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
Foam::sigSegv::sigSegvHandler(int)
/lib/tls/libpthread.so.0 [0x3dc8b8]
fluentMeshToFoam [0x8055421]
__libc_start_main
__gxx_personality_v0

what is problem?

hjasak November 26, 2006 11:21

Did you write out your Fluent
 
Did you write out your Fluent file in ascii?

Could you please produce a trace-back and post it here.

Hrv

waynezw0618 November 26, 2006 23:37

root@localhost ~]# fluentMeshT
 
[root@localhost ~]# fluentMeshToFoam OpenFOAM/root-1.3/run/tutorials/lesInterFoam/ hydrocylone /root/fluent-new.msh
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.3 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : fluentMeshToFoam OpenFOAM/root-1.3/run/tutorials/lesInterFoam/ hydrocylone /root/fluent-new.msh
Date : Nov 27 2006
Time : 11:45:05
Host : localhost.localdomain
PID : 21928
Root : OpenFOAM/root-1.3/run/tutorials/lesInterFoam/
Case : hydrocylone
Nprocs : 1
Create time

Dimension of grid: 3
Number of points: 356188
Reading points
Number of cells: 340982
Reading uniform cells
number of faces: 1038000
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading zone data
Reading zone data
Reading zone data
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


Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
Foam::sigSegv::sigSegvHandler(int)
/lib/tls/libpthread.so.0 [0xbf08b8]
fluentMeshToFoam [0x8055421]
__libc_start_main
__gxx_personality_v0

waynezw0618 November 27, 2006 00:05

Dear Hrv: i use ICEMcfd to cr
 
Dear Hrv:
i use ICEMcfd to creat mesh for fluent,what is wrong with it?
it is a mesh file for hydrocylone,could the OpenFoam do the Numerical simulation for both air-core and particle in the hydrocylone?

mattijs November 28, 2006 05:31

You can produce a more detaile
 
You can produce a more detailed traceback if you recompile fluentMeshToFoam with full debugging. Just add to EXE_INC in Make/options the compilation options

-DFULLDEBUG -g -O0

and recompile.

waynezw0618 November 30, 2006 02:53

Hi Hrv and Mattijs: i have do
 
Hi Hrv and Mattijs:
i have do the recompilation of fluentMeshToFoam,and here is the new trace back:
[root@localhost .OpenFOAM-1.3]# fluentMeshToFoam /root/OpenFOAM/root-1.3/run/tutorials/oodles hyrocylone /root/fluent-new.msh
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.3 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : fluentMeshToFoam /root/OpenFOAM/root-1.3/run/tutorials/oodles hyrocylone /root/fluent-new.msh
Date : Nov 30 2006
Time : 14:54:42
Host : localhost.localdomain
PID : 6299
Root : /root/OpenFOAM/root-1.3/run/tutorials/oodles
Case : hyrocylone
Nprocs : 1
Create time

Dimension of grid: 3
Number of points: 356188
Reading points
Number of cells: 340982
Reading uniform cells
number of faces: 1038000
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading uniform faces
Reading zone data
Reading zone data
Reading zone data
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




--> FOAM FATAL ERROR : index 6 out of range 0 ... 5

From function UList<t>::checkIndex(const label)
in file /root/OpenFOAM/OpenFOAM-1.3/src/OpenFOAM/lnInclude/UListI.H at line 107.

FOAM aborting

Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
Foam::error::abort()
fluentMeshToFoam [0x804da24]
fluentMeshToFoam [0x804e27c]
fluentMeshToFoam [0x804e2e2]
fluentMeshToFoam [0x8056d14]
__libc_start_main
__gxx_personality_v0
已放弃

please help me to solve the problem,and how to make simulation of aircore and particle in the hydrocylone by Foam?

hjasak November 30, 2006 04:48

Your mesh is invalid. Try run
 
Your mesh is invalid. Try running the attached version of fluentMeshToFoam and you will get a full error message. Of course, you need to compile it first.

Hrv

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif fluentMeshToFoam.L

waynezw0618 November 30, 2006 06:52

FINISHED LEXING --> F
 
FINISHED LEXING




--> FOAM FATAL ERROR : Trying to add 7th face to a cell with 6 faces. Face inde x: 1007892 Current faces: 6(35472 36212 36268 36269 36270 36271)

From function fluentMeshToFoam
in file fluentMeshToFoam.L at line 928.

FOAM aborting

Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
Foam::error::abort()
fluentMeshToFoam [0x804da74]
fluentMeshToFoam [0x80571da]
__libc_start_main
__gxx_personality_v0
已放弃

waynezw0618 November 30, 2006 07:03

Hi Hrv i use ICEMCFD to creat
 
Hi Hrv
i use ICEMCFD to creat this .msh file for fluent calculation. i am not quiet sure about my method of export the .msh file for fluent calculation in ICEM. i guess the problem may because of my operation. here is my operation:
1) make geo and premesh
2) right click the block tree and choose convert to unstructure mesh
3) choose fluent as solver
4) export msh
it that right?
i am not sure about "2)" ,but all my friends do it.
could you please help me?
thanks!

dmoroian November 30, 2006 07:49

I'm just curious: did you try
 
I'm just curious: did you try to read this mesh with fluent?

Dragos

hjasak November 30, 2006 08:02

Fluent will quietly fix the me
 
Fluent will quietly fix the mesh for you during the read. With all these broken meshes, if you can read them into Fluent and write them out again, the new case file will convert correctly.

In short, Icem, Gridgen and the like do not correctly adhere to Fluent mesh description and there isn't much I can do about it.

Hrv

waynezw0618 November 30, 2006 23:38

HI Dragos i have read this me
 
HI Dragos
i have read this mesh to fluent without any errors.
wayne

waynezw0618 December 1, 2006 00:12

Hi Hrv i use Tgrid to refine
 
Hi Hrv
i use Tgrid to refine the mesh.and now i can convert it to Foam!thanks!
by the way,it there any application in foam for the multiphase flow in hydrocyclone ?or i need to write the application for my simulation?


All times are GMT -4. The time now is 13:37.