CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Meshing & Mesh Conversion

[Salome] ideasUnvToFoam Error: Assertion `nouveau > -1' failed

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

Like Tree2Likes
  • 2 Post By GerhardHolzinger

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 29, 2019, 11:23
Default ideasUnvToFoam Error: Assertion `nouveau > -1' failed
  #1
Senior Member
 
Gerhard Holzinger
Join Date: Feb 2012
Location: Austria
Posts: 287
Rep Power: 23
GerhardHolzinger will become famous soon enoughGerhardHolzinger will become famous soon enough
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:
  • Keep several OpenFOAM and foam installations on your system, they might turn out to be handy
  • The [CODE]Assertion `nouveau > -1' failed/CODE] error might be caused by duplicate face group membership
dokeun and vince_cfd like this.
GerhardHolzinger is offline   Reply With Quote

Reply

Tags
ideasunvtofoam, mesh conversion, salome

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Foam::error::printStack(Foam::Ostream&) with simpleFoam -parallel U.Golling OpenFOAM Running, Solving & CFD 45 September 26, 2020 15:57
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


All times are GMT -4. The time now is 14:48.