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

FluentMesh conversion problemwaiting for help

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 26, 2006, 09:41
Default dear everyone, i have a flue
  #1
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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:stream&)
Foam::sigSegv::sigSegvHandler(int)
/lib/tls/libpthread.so.0 [0x3dc8b8]
fluentMeshToFoam [0x8055421]
__libc_start_main
__gxx_personality_v0

what is problem?
waynezw0618 is offline   Reply With Quote

Old   November 26, 2006, 11:21
Default Did you write out your Fluent
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
Did you write out your Fluent file in ascii?

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

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

Old   November 26, 2006, 23:37
Default root@localhost ~]# fluentMeshT
  #3
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
[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:stream&)
Foam::sigSegv::sigSegvHandler(int)
/lib/tls/libpthread.so.0 [0xbf08b8]
fluentMeshToFoam [0x8055421]
__libc_start_main
__gxx_personality_v0
waynezw0618 is offline   Reply With Quote

Old   November 27, 2006, 00:05
Default Dear Hrv: i use ICEMcfd to cr
  #4
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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?
waynezw0618 is offline   Reply With Quote

Old   November 28, 2006, 05:31
Default You can produce a more detaile
  #5
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
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.
mattijs is offline   Reply With Quote

Old   November 30, 2006, 02:53
Default Hi Hrv and Mattijs: i have do
  #6
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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:stream&)
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?
waynezw0618 is offline   Reply With Quote

Old   November 30, 2006, 04:48
Default Your mesh is invalid. Try run
  #7
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
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

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

Old   November 30, 2006, 06:52
Default FINISHED LEXING --> F
  #8
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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:stream&)
Foam::error::abort()
fluentMeshToFoam [0x804da74]
fluentMeshToFoam [0x80571da]
__libc_start_main
__gxx_personality_v0
已放弃
waynezw0618 is offline   Reply With Quote

Old   November 30, 2006, 07:03
Default Hi Hrv i use ICEMCFD to creat
  #9
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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!
waynezw0618 is offline   Reply With Quote

Old   November 30, 2006, 07:49
Default I'm just curious: did you try
  #10
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
I'm just curious: did you try to read this mesh with fluent?

Dragos
dmoroian is offline   Reply With Quote

Old   November 30, 2006, 08:02
Default Fluent will quietly fix the me
  #11
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   November 30, 2006, 23:38
Default HI Dragos i have read this me
  #12
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
HI Dragos
i have read this mesh to fluent without any errors.
wayne
waynezw0618 is offline   Reply With Quote

Old   December 1, 2006, 00:12
Default Hi Hrv i use Tgrid to refine
  #13
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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?
waynezw0618 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
conversion hari Main CFD Forum 0 December 6, 2007 00:26
Conversion 13 14 of dynamicBodyFvMesh lr103476 OpenFOAM Running, Solving & CFD 2 June 19, 2007 05:38
FluentMesh conversion problemwaiting for help waynezw0618 OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 0 November 26, 2006 23:27
FoamtoFluent conversion mer OpenFOAM Post-Processing 0 January 8, 2006 01:43
tet to hex conversion? Henry Main CFD Forum 10 June 8, 2001 07:03


All times are GMT -4. The time now is 11:39.