|
[Sponsors] |
[Salome] ideasUnvToFoam Error: Assertion `nouveau > -1' failed |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 29, 2019, 11:23 |
ideasUnvToFoam Error: Assertion `nouveau > -1' failed
|
#1 |
Senior Member
Gerhard Holzinger
Join Date: Feb 2012
Location: Austria
Posts: 342
Rep Power: 28 |
This is more an answer, than a question.
I have created a geometry with Salome, and created a tet mesh, which I exported in the UNV format. The next step was to convert the mesh using the converter ideasUnvToFoam. However, I only got this far: Code:
/*---------------------------------------------------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 6 \\/ M anipulation | \*---------------------------------------------------------------------------*/ Build : 6-4086512c6910 Exec : ideasUnvToFoam cfdTetMesh.unv Date : Jan 29 2019 Time : 16:07:14 Host : "userWork" PID : 63105 I/O : uncollated Case : /home/user/OpenFOAM/user-6.0/geometries/myCaseFullGeometry/CFD_tetMesh nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Processing tag:164 Starting reading units at line 3. l:1 units:" SI: Meter (newton)" unitType:2 Unit factors: Length scale : 1 Force scale : 1 Temperature scale : 1 Temperature offset : 273.15 Processing tag:2420 Skipping tag 2420 on line 9 Skipping section at line 9. Processing tag:2411 Starting reading points at line 20. Read 187382 points. Processing tag:2412 Starting reading cells at line 374787. First occurrence of element type 11 for cell 1 at line 374788 First occurrence of element type 41 for cell 3529 at line 385372 First occurrence of element type 111 for cell 85459 at line 549232 Read 983696 cells and 81930 boundary faces. Processing tag:2467 Starting reading patches at line 2516626. For group 1 named banana trying to read 556 patch face indices. For group 2 named apple trying to read 556 patch face indices. For group 3 named orange trying to read 424 patch face indices. For group 4 named gasOutlet trying to read 76 patch face indices. For group 5 named bottom trying to read 50 patch face indices. Sorting boundary faces according to group (patch) 0: banana is patch 1: apple is faceZone 2: orange is patch 3: gasOutlet is patch 4: bottom is patch Constructing mesh with non-default patches of size: banana 556 orange 424 gasOutlet 76 bottom 50 --> FOAM Warning : From function Foam::polyMesh::polyMesh(const Foam::IOobject&, const Foam::Xfer<Foam::Field<Foam::Vector<double> > >&, const cellShapeList&, const faceListList&, const wordList&, const wordList&, const Foam::word&, const Foam::word&, const wordList&, bool) in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 595 Found 80824 undefined faces in mesh; adding to default patch. Adding cell and face zones Face Zone apple 556 ideasUnvToFoam: ideasUnvToFoam.C:1277: int main(int, char**): Assertion `nouveau > -1' failed. Abgebrochen (Speicherabzug geschrieben) I tried various versions of OpenFOAM, to no avail. However, when I tried using my foam-extend-4.0 installation, the error message contained the vital hint Code:
/*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | foam-extend: Open Source CFD | | \\ / O peration | Version: 4.0 | | \\ / A nd | Web: http://www.foam-extend.org | | \\/ M anipulation | For copyright notice see file Copyright | \*---------------------------------------------------------------------------*/ Build : 4.0-246a172c9d9e Exec : ideasUnvToFoam cfdTetMesh.unv Date : Jan 29 2019 Time : 16:07:59 Host : userWork PID : 63112 CtrlDict : "/home/user/OpenFOAM/user-6.0/geometries/myCaseFullGeometry/CFD_tetMesh/system/controlDict" Case : /home/user/OpenFOAM/user-6.0/geometries/myCaseFullGeometry/CFD_tetMesh nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Processing tag:164 Starting reading units at line 3. l:1 units:" SI: Meter (newton)" unitType:2 Unit factors: Length scale : 1 Force scale : 1 Temperature scale : 1 Temperature offset : 273.15 Processing tag:2420 Skipping tag 2420 on line 9 Skipping section at line 9. Processing tag:2411 Starting reading points at line 20. Read 187382 points. Processing tag:2412 Starting reading cells at line 374787. First occurrence of element type 11 for cell 1 at line 374788 First occurrence of element type 41 for cell 3529 at line 385372 First occurrence of element type 111 for cell 85459 at line 549232 Read 983696 cells and 81930 boundary faces. Processing tag:2467 Starting reading patches at line 2516626. For group 1 named banana trying to read 556 patch face indices. For group 2 named apple trying to read 556 patch face indices. For group 3 named orange trying to read 424 patch face indices. For group 4 named gasOutlet trying to read 76 patch face indices. For group 5 named bottom trying to read 50 patch face indices. Sorting boundary faces according to group (patch) Constructing mesh with non-default patches of size: banana 556 apple 556 orange 424 gasOutlet 76 bottom 50 --> FOAM FATAL ERROR: Trying to specify a boundary face 3(33 782 6589) on the face on cell 321448 which is either an internal face or already belongs to some other patch. This is face 0 of patch 1 named apple. From function polyMesh::setTopology ( const cellShapeList& cellsAsShapes, const faceListList& boundaryFaces, const wordList& boundaryPatchNames, labelList& patchSizes, labelList& patchStarts, label& defaultPatchStart, label& nFaces, cellList& cells ) in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 357. FOAM aborting Abgebrochen (Speicherabzug geschrieben) It turned out, that I messed up my definition of face groups in Salome. Thus, the converter tried and failed to assign the same boundary face to more than one patch. The error message of the ideasUnvToFoam converter of my foam-extend installation actually reports this error. The ideasUnvToFoam converter of the (foundation) OpenFOAM installations fail with no hint in that regard. Lessons learned:
|
|
November 7, 2024, 07:49 |
|
#2 |
New Member
Akshay Mani
Join Date: Oct 2022
Posts: 1
Rep Power: 0 |
Yes. This is true. It happened with me when I had grouped the same patch under two different names.
|
|
Tags |
ideasunvtofoam, mesh conversion, salome |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Foam::error::printStack(Foam::Ostream&) with simpleFoam -parallel | U.Golling | OpenFOAM Running, Solving & CFD | 52 | September 23, 2023 04:35 |
Initial conditions for uniform flow | andreas | OpenFOAM | 5 | November 16, 2012 16:00 |
[OpenFOAM] ParaView/Parafoam error when making animation | Disco_Caine | ParaView | 6 | September 28, 2010 10:54 |
user subroutine error | CFDUSER | CFX | 2 | December 9, 2006 07:31 |
user defined function | cfduser | CFX | 0 | April 29, 2006 11:58 |