|
[Sponsors] |
[Commercial meshers] FluentMesh conversion problem |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
November 26, 2006, 09:41 |
FluentMesh conversion problem
|
#1 |
Senior Member
|
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? |
|
November 26, 2006, 11:21 |
Did you write out your Fluent
|
#2 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
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 |
|
November 26, 2006, 23:37 |
root@localhost ~]# fluentMeshT
|
#3 |
Senior Member
|
[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 |
|
November 27, 2006, 00:05 |
Dear Hrv:
i use ICEMcfd to cr
|
#4 |
Senior Member
|
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? |
|
November 28, 2006, 05:31 |
You can produce a more detaile
|
#5 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
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. |
|
November 30, 2006, 02:53 |
Hi Hrv and Mattijs:
i have do
|
#6 |
Senior Member
|
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? |
|
November 30, 2006, 04:48 |
Your mesh is invalid. Try run
|
#7 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
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 |
|
November 30, 2006, 06:52 |
FINISHED LEXING
--> F
|
#8 |
Senior Member
|
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 |
|
November 30, 2006, 07:03 |
Hi Hrv
i use ICEMCFD to creat
|
#9 |
Senior Member
|
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! |
|
November 30, 2006, 07:49 |
I'm just curious: did you try
|
#10 |
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 20 |
I'm just curious: did you try to read this mesh with fluent?
Dragos |
|
November 30, 2006, 08:02 |
Fluent will quietly fix the me
|
#11 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
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 |
|
November 30, 2006, 23:38 |
HI Dragos
i have read this me
|
#12 |
Senior Member
|
HI Dragos
i have read this mesh to fluent without any errors. wayne |
|
December 1, 2006, 00:12 |
Hi Hrv
i use Tgrid to refine
|
#13 |
Senior Member
|
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? |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[Commercial meshers] Problem In conversion From Fluent to Foam | aks017 | OpenFOAM Meshing & Mesh Conversion | 0 | April 15, 2019 07:12 |
BuoyantBoussinesqSimpleFoam_Facing problem | Mondal131211 | OpenFOAM Running, Solving & CFD | 1 | April 10, 2019 20:41 |
Mesh& steptime independant: conduction-convection problem | Fati1 | Main CFD Forum | 1 | October 28, 2018 14:52 |
CFD by anderson, chp 10.... supersonic flow over flat plate | varunjain89 | Main CFD Forum | 18 | May 11, 2018 08:31 |
Unit Conversion Problem | lambuhere | CFX | 0 | August 20, 2004 05:49 |