|
[Sponsors] |
October 10, 2005, 07:24 |
Conversion problem
|
#1 |
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 20 |
Hello everybody,
I have a beginer's problem! I have generated a mesh using gambit 2.2.30. The mesh format is msh (for fluent). When I try to convert this to openfoam I get the following error: mshToFoam ~/ dragosica-foam test_gradient.msh ...cut... Exec : mshToFoam /home/dragos/ dragosica-foam test_gradient.msh Date : Oct 10 2005 Time : 13:00:48 Host : bobby PID : 28256 Root : /home/dragos/ Case : dragosica-foam Nprocs : 1 Create time --> FOAM FATAL IO ERROR : wrong token type - expected int found on line 1 the punctuation token '(' file: test_gradient.msh at line 1. From function operator>>(Istream&, int&) in file primitives/int/intIO.C at line 74. FOAM exiting Then I tried to import the mesh in neu format, but I get another error: dragos@bobby:~/work/test_gradients$ gambitToFoam ~/ dragosica-foam test_gradient.neu ...cut... Exec : gambitToFoam /home/dragos/ dragosica-foam test_gradient.neu Date : Oct 10 2005 Time : 13:04:03 Host : bobby PID : 28260 Root : /home/dragos/ Case : dragosica-foam Nprocs : 1 Create time Title: test_gradient Written by Gambit version 2.2.30 File written on 10 Oct 2005 12:10:57 number of points: 9181 number of cells: 7875 number of patches: 2 Reading nodal coordinates Reading cells Reading cell streams Reading cell stream labels Finished reading cell stream labels Reading patches patch 0: name: inlet --> FOAM FATAL IO ERROR : Attempt to get back from bad stream file: IStringStream.sourceFile at line 3. From function void Istream::getBack(token& t) in file db/IOstreams/IOstreams/Istream.C at line 44. FOAM exiting Anyone knows what is the problem? At least gambitToFoam reads one boundary condition (inlet), but still does not finish. Best regards, Dragos |
|
October 10, 2005, 09:07 |
@mshToFoam in your first examp
|
#2 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
@mshToFoam in your first example: the utility you wanted to use is fluentMeshToFoam. mshToFoam is for a completely different format (.msh seems to be a very popular extension for all kinds of mesh files)
__________________
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 |
|
October 10, 2005, 10:22 |
At least for the first problem
|
#3 |
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 20 |
At least for the first problem it was my fault. I should have used fluentMeshToFoam instead of mshToFoam. But it still remains the problem with gambitToFoam converter!
|
|
October 10, 2005, 10:26 |
Is your gambit file ascii or b
|
#4 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 |
Is your gambit file ascii or binary? Binary is not supported, try writing it out ascii and converting again. The Gambit converter works fine over here (and it was me who wrote it) :-)
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
October 11, 2005, 03:34 |
Yes, the gambit neutral file i
|
#5 |
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 20 |
Yes, the gambit neutral file is in ascii format. I wrote myself some converters (neu->tecplot) for it. Anyway I do not know how to create a neutral file format other than ascii (which should be ok).
Dragos |
|
February 10, 2007, 21:28 |
dear
itry to convert mesh fr
|
#6 |
New Member
mohamed
Join Date: Mar 2009
Posts: 1
Rep Power: 0 |
dear
itry to convert mesh from .neu to openfoam but i am faild i donot know why please help me their another thing i have cenataur in any format that i should get the mesh to put it in openfoam gambitToFoam ~/OpenFOAM/mhalima-1.3/run/tutorials/icoFoam/ halima testfeb09.neu /*---------------------------------------------------------------------------*\ | ========= | | | \ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \ / O peration | Version: 1.3 | | \ / A nd | Web: http://www.openfoam.org | | \/ M anipulation | | \*---------------------------------------------------------------------------*/ Exec : gambitToFoam /home/mhalima/OpenFOAM/mhalima-1.3/run/tutorials/icoFoam/ halima testfeb09.neu Date : Feb 11 2007 Time : 03:01:34 Host : mhalima PID : 7205 Root : /home/mhalima/OpenFOAM/mhalima-1.3/run/tutorials/icoFoam/ Case : halima Nprocs : 1 Create time Finished lexing gambitToFoam: Gambit file format does not provide information about the type of the patch (eg. wall, symmetry plane, cyclic etc). All the patches have been created as type patch. Please reset after mesh conversion as necessary. Default patch type set to empty --> FOAM FATAL ERROR : points deallocated From function const pointField& polyMesh::allPoints() const in file meshes/polyMesh/polyMesh.C at line 642. FOAM aborting Foam::error::printStack(Foam:stream&) Foam::error::abort() Foam::polyMesh::allPoints() const Foam::polyMesh::cellShapePointCells(Foam::List<foa m::cellshape> const&) const Foam::polyMesh::polyMesh(Foam::IOobject const&, Foam::Field<foam::vector<double> > const&, Foam::List<foam::cellshape> const&, Foam::List<foam::list<foam::face> > const&, Foam::List<foam::word> const&, Foam::List<foam::word> const&, Foam::word const&, Foam::List<foam::word> const&) gambitToFoam [0x8050b70] __libc_start_main __gxx_personality_v0 Aborted thanks alot yours m.halima |
|
May 10, 2007, 09:09 |
Hi everybody,
I have a small
|
#7 |
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Nantes, France
Posts: 195
Rep Power: 17 |
Hi everybody,
I have a small problem with FluentMeshToFoam. I have generated a mesh using gambit 2.3.16. The mesh format is msh (for fluent). I've got periodic faces in this file. (cyclic in Foam) so I choose PERIODIC in gambit,and named it CYCLIC1. When I try to convert it to Foam mesh, I got this error: ... FINISHED LEXING dimension of grid: 3 Creating shapes for 3-D cells Creating patch for zone: 3 start: 1 end: 5925 type: shadow name: CYCLIC1_shadow --> FOAM FATAL ERROR : fluent patch type shadow not recognised. From function fluentToFoam::main(int argc, char *argv[]) in file fluentMeshToFoam.L at line 1258. FOAM aborting I don't know why this "shadow" is coming ... Anyone knows what is the problem? Best regards, Cedric |
|
May 10, 2007, 10:37 |
Hi Cedric,
If I remember core
|
#8 |
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 20 |
Hi Cedric,
If I remember corectly, you cannot use the PERIODIC boundary condition! So, why don't you just set those faces as wall and then change the patch type in the boundary file that you get after the conversion? Dragos |
|
May 10, 2007, 11:01 |
Hi Dragos,
Thank's for the ti
|
#9 |
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Nantes, France
Posts: 195
Rep Power: 17 |
Hi Dragos,
Thank's for the tips, it works correctly now. I did't know that PERIODIC boundary condition doesn't work in conversion and I was a little bit ...suprised ;o) Cedric |
|
May 10, 2007, 11:02 |
Dragos is right. But make sure
|
#10 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
Dragos is right. But make sure that you have exactly the same meshes on both "walls" (there are ways to do that in Gambit, but don't ask me). Plus they should be in the same patch (use couplePatches afterwards to make sure that the faces are correctly ordered - see figure 6.4 in the UserGuide)
__________________
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 |
|
May 10, 2007, 11:45 |
hi Bernhard,
Thank you for th
|
#11 |
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Nantes, France
Posts: 195
Rep Power: 17 |
hi Bernhard,
Thank you for the adding comments, I will check my mesh again in Gambit. I'm sure that the mesh's parameters are the same for the two side of the "wall" but for the order of the faces, ... I'll check again. Cedric |
|
August 6, 2007, 05:54 |
hello everybody,
I also have
|
#12 |
Senior Member
Cedric DUPRAT
Join Date: Mar 2009
Location: Nantes, France
Posts: 195
Rep Power: 17 |
hello everybody,
I also have a beginer's problem! but I can't find the mistake ... I have generated a mesh using gambit The mesh format is neu. When I try to convert this to openfoam I get the following error: " Default patch type set to empty Foam::error::printStack(Foam:stream&) Foam::sigSegv::sigSegvHandler(int) /lib/tls/libpthread.so.0 [0xa75898] Foam::polyMesh::polyMesh(Foam::IOobject const&, Foam::Field<foam::vector<double> > const&, Foam::List<foam::cellshape> const&, Foam::List<foam::list<foam::face> > const&, Foam::List<foam::word> const&, Foam::List<foam::word> const&, Foam::word const&, Foam::List<foam::word> const&) gambitToFoam [0x8051911] __libc_start_main __gxx_personality_v0 Segmentation fault" So before this message, OF read correctly my 4 empty patchs (2 inlet, 1 outlet, 1 wall). Because there is no tips in the OF's message, ....I don't know what to do. Anyone knows what is the problem, any advice? Best regards, Cedric |
|
September 13, 2007, 16:35 |
Dear all,
I generated a fl
|
#13 |
Member
Quinn Tian
Join Date: Mar 2009
Posts: 62
Rep Power: 17 |
Dear all,
I generated a fluent mesh with Gridgen. I am trying to convert fluent mesh to openFOam. For some reason, I am keep geting this warning message during "checking mesh" process. It seems like non-orthogonality problem in the element, but I don't know how to solve this problem. I recheck mesh and did not see any place suspicious. Can anyone give me some help and advise? Thank you very much. --> FOAM Warning : From function primitiveMesh::checkFaceDotProduct(const bool report, labelHashSet* setPtr) const in file meshes/primitiveMesh/primitiveMeshCheck.C at line 534 Severe non-orthogonality detected for face 31089 between cells 10443 and 10444: Angle = 176.177 deg. --> FOAM Warning : From function primitiveMesh::checkFaceDotProduct(const bool report, labelHashSet* setPtr) const in file meshes/primitiveMesh/primitiveMeshCheck.C at line 534 Severe non-orthogonality detected for face 31090 between cells 10443 and 10626: Angle = 174.315 deg. |
|
September 13, 2007, 19:18 |
E.g. use setSet to pick up the
|
#14 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
E.g. use setSet to pick up the cells using these faces:
setSet <root> <case> faceSet f0 new labelToFace (31089) cellSet c0 new faceToCell f0 any quit This will write a VTK file for f0 (which now cotains that face label) and for (the outside faces of) c0 (which contains owner and neighbour of f0). |
|
September 13, 2007, 19:47 |
Mattijs,
Could you please g
|
#15 |
Member
Quinn Tian
Join Date: Mar 2009
Posts: 62
Rep Power: 17 |
Mattijs,
Could you please give more explanation about your solution? I think I don't even quite understand what causes my problem. Thank you for your help. QT |
|
September 14, 2007, 05:44 |
It was not a solution, just a
|
#16 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
It was not a solution, just a way of visualising the problematic cell(s).
Your mesh as generated by Gridgen is incorrect. The maximum non-orthogonality for a mesh is 90 degrees, for it also to be 'runnable' quite a bit lower than that. |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Mesh& steptime independant: conduction-convection problem | Fati1 | Main CFD Forum | 1 | October 28, 2018 13:52 |
CFD by anderson, chp 10.... supersonic flow over flat plate | varunjain89 | Main CFD Forum | 18 | May 11, 2018 07:31 |
[ICEM] Problem with 2D to 3D block conversion using Multizone | Arvind_CFD | ANSYS Meshing & Geometry | 0 | March 12, 2015 23:02 |
Problem in implementing new sgs model | zoptirik | OpenFOAM Programming & Development | 0 | January 29, 2015 05:35 |
Unit Conversion Problem | lambuhere | CFX | 0 | August 20, 2004 04:49 |