 |
 |
 |
|
|
|
[Sponsors] | ||||
[Commercial meshers] Illegal cell label -1, error in mesh-conversion, icem |
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 2, 2014, 05:43
|
Illegal cell label -1, error in mesh-conversion, icem
|
#1 |
|
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 12  |
Zone: 19 name: INLET type: velocity-inlet. Reading zone data...done.
Zone: 20 name: TRAILING-EDGE type: wall. Reading zone data...done. FINISHED LEXING Creating patch 0 for zone: 15 name: OUTLET type: outlet-vent Creating patch 1 for zone: 16 name: SHROUD type: wall Creating patch 2 for zone: 17 name: NABE type: wall Creating patch 3 for zone: 18 name: BLADE type: wall Creating patch 4 for zone: 19 name: INLET type: velocity-inlet Creating patch 5 for zone: 20 name: TRAILING-EDGE type: wall patch 0 from Fluent indices: 0 to: 21355 type: outlet-vent patch 1 from Fluent indices: 21356 to: 24308 type: wall patch 2 from Fluent indices: 24309 to: 26339 type: wall patch 3 from Fluent indices: 26340 to: 212537 type: wall patch 4 from Fluent indices: 212538 to: 214840 type: velocity-inlet patch 5 from Fluent indices: 214841 to: 223233 type: wall --> FOAM FATAL ERROR: Illegal cell label -1 in neighbour addressing for face 0 From function polyMesh::initMesh() in file meshes/polyMesh/polyMeshInitMesh.C at line 65. [/CODE] Does anybody have some experience with this? I didnīt find this error in google, so I hope here is someone who can help me. Otherwise I just to do a new mesh with Icem. Thank you so far. Best regards Tobi |
|
|
|
|
|
June 2, 2014, 06:07
|
|
#2 |
|
Member
Tobias Adam
Join Date: Oct 2013
Location: Siegen
Posts: 55
Rep Power: 12 |
got it...
I simply forgot the volume mesh... Shame on me for this thread.... |
|
|
|
|
|
|
May 6, 2015, 02:59
|
i have the same problem
|
#3 | |
|
Member
behrouz
Join Date: Mar 2015
Posts: 34
Rep Power: 11 |
Quote:
|
||
|
|
|
||
|
May 6, 2015, 06:44
|
|
#4 | |
|
Member
behrouz
Join Date: Mar 2015
Posts: 34
Rep Power: 11 |
Quote:
oh oh,i forgot volum mesh to... shame on me too |
||
|
|
|
||
|
January 3, 2017, 08:11
|
|
#5 |
|
New Member
bart3000
Join Date: Nov 2016
Posts: 1
Rep Power: 0 |
Dear,
Is it possible to give a bit more explanation on how you solved this problem? I'm facing the exact same one. What do you exactly mean with the volume mesh? Thanks in advance, Bart Last edited by bart3000; January 4, 2017 at 01:55. |
|
|
|
|
|
|
May 11, 2018, 07:59
|
|
#6 | |
|
New Member
ashfaque
Join Date: Jul 2015
Posts: 1
Rep Power: 0 |
Quote:
Dear Bart I am also stuck at the exact problem with my mesh and completely lost  Did you manage to solve the problem and if yes how? It would be very kind if you could share the solution. Best regards Ashfaque |
||
|
|
|
||
|
January 12, 2021, 15:21
|
my solution
|
#7 |
|
New Member
Hui Zhang
Join Date: Jun 2020
Posts: 14
Rep Power: 5 |
In case of someone having same problem, I post my solution. When I copied and rotated the mesh, and output, this problem happened when I used fluent3DMeshToFoam. And I realized that I did not rotate and copy all substances of mesh. After selecting subsets, points, lines, shells and volumes, copied and rotated again, it was converted successfully. Thus, for this problem, I think that there are some missing lines, points or volumes causing this problem when you convert the mesh.
Best, Hui |
|
|
|
|
|
|
July 31, 2021, 05:36
|
|
#8 | |
|
Senior Member
CFD_Lovers
Join Date: Mar 2015
Posts: 168
Rep Power: 11 |
Quote:
Can you just leave u some hints on how you solve it? Thank you |
||
|
|
|
||
|
October 19, 2021, 15:45
|
|
#9 |
|
New Member
Balaji
Join Date: May 2013
Posts: 21
Rep Power: 12 |
Hi guys,
I am using commercial software to create mesh for openfoam (Ansa HeXtreme) I am getting the same error, I have made sure to include the Volume region. What might be the issue, how did you guys solve the issue? My mesh size is around 144M elements, external aerodynamics Any inputs/methods will be appreciated Code:
[0] [0] [0] --> FOAM FATAL ERROR: (openfoam-2012) [0] Illegal cell label -1 in neighbour addressing for face 411208890 [0] [0] From void Foam::polyMesh::initMesh() [0] in file meshes/polyMesh/polyMeshInitMesh.C at line 77. [0] FOAM parallel run exiting [0] -------------------------------------------------------------------------- MPI_ABORT was invoked on rank 0 in communicator MPI_COMM_WORLD with errorcode 1. |
|
|
|
|
|
|
October 20, 2021, 03:12
|
|
#10 | |
|
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,684
Rep Power: 40 |
Quote:
Making some guesses here. The OpenFOAM meshes are assembled from faces, not primitive cell shapes. This means that the mesh connectivity is given by the face owner/neighbour relationship. Each face will have a "owner" cell, all internal mesh faces have a "neighbour" cell, but the faces on the domain boundary do not have a "neighbour". Thus the number of neighbours will be less than the number of owners. In very versions (old even as "FOAM" before it became "OpenFOAM") the neighbour list was padded to the same length with -1 values. It could be that your commercial mesher is generating these old formats and they are triggering a problem? Things to check. Do the list sizes mentioned in polyMesh/{owner,neighbour} files make sense? Is the owner < neighbour, any -1 values to be seen? What does checkMesh tell you? Run in serial to rule out problems there. |
||
|
|
|
||
|
October 20, 2021, 11:09
|
|
#11 | |
|
New Member
Hui Zhang
Join Date: Jun 2020
Posts: 14
Rep Power: 5 |
Quote:
Check two lines cross the vertice that you want them to cross. I used ICEM to generate mesh, and sometimes can not make the nearby lines cross same points or vertices automatically. this kind of mistakes can be ignored easily, because only zoom in, to some extent, this error can be seen. So please check carefully your basic elements. |
||
|
|
|
||
|
October 21, 2021, 04:41
|
Solution Found
|
#12 |
|
New Member
Balaji
Join Date: May 2013
Posts: 21
Rep Power: 12 |
Hi Guys,
So I found out the solution to the issue which I was facing. For anyone who is interested, the below method maybe helpful. The commercial software programs (ANSA) sometimes create huge mesh 144M elements, but sometimes the volumes meshes are penetrating with some shell meshes. In my case the HeXtreme mesh was getting penetrated with 2 Trias surfaces, which should normally not happen after auto quality improvement. Luckily there is an option in ANSA, where one can find out the penetrated regions. I then manually deleted the two unreferenced Trias surfaces and then re-exported the Volume mesh in openFoam format. So basically, there should not be any hanging unreferenced surfaces other than the main mesh and boundaries. The checkMesh unfortunately didn't capture this detail. Hence the confusion  So the solution is to re-verify the mesh on commercial software packages for intersection or penetration, then either Auto-fix or remove them manually. Cheers Neal 
|
|
|
|
|
|
|
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| [snappyHexMesh] problems generating clean mesh | Christian_tt | OpenFOAM Meshing & Mesh Conversion | 2 | June 20, 2019 05:39 |
| CFD by anderson, chp 10.... supersonic flow over flat plate | varunjain89 | Main CFD Forum | 18 | May 11, 2018 07:31 |
| [mesh manipulation] Importing Multiple Meshes | thomasnwalshiii | OpenFOAM Meshing & Mesh Conversion | 18 | December 19, 2015 18:57 |
| Inner geometry gets lost exporting mesh from ICEM CFD to CFX-Pre | powpow | CFX | 3 | December 20, 2012 09:14 |
| [Commercial meshers] ansys icem tetra mesh to fluent_v6 conversion problems | milleniumrider | OpenFOAM Meshing & Mesh Conversion | 3 | May 13, 2010 14:54 |
3Likes
Linear Mode
