|
[Sponsors] |
[Technical] checkMesh states that faces do not form a cell, mesh appears correct |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
March 18, 2014, 06:33 |
checkMesh states that faces do not form a cell, mesh appears correct
|
#1 |
New Member
Richel Bilderbeek
Join Date: Nov 2013
Posts: 14
Rep Power: 13 |
I try to create the mesh of a cube consisting of two adjacent prisms, using the points, faces, boundary, owner and neighbour files. It should be easy, but checkMesh states:
Code:
The mesh has multiple regions which are not connected by any face. Code:
***Boundary openness (0 0.171573 0) possible hole in boundary description. ***Open cells found, max cell openness: 1, number of open cells 1 Although my research appears thorough to me, I appear to overlook something. I am pretty sure the windings are correct, as this was the previous aspect checkMesh made me correct. The files used and generated, of which I think of to be most important, I paste below, all and the compete files can be viewed at http://www.richelbilderbeek.nl/ToolO...CellsFound.htm . I have tried hard to make it clear to deduce what I overlooked, so I am very curious what it is. Thanks, Richel Bilderbeek checkMesh output: Code:
Build : 2.1-88b2f2ae3a0b Exec : checkmesh Date : Mar 18 2014 Time : 08:52:39 Host : "AIRBEAR-W7-I5" PID : 1524 Case : D:/Projects/Tools/build-ToolTestTriangleMeshConsole-Desktop_Qt_5_1_1_Mi nGW_32bit-Debug nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMas ter allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 8 internal points: 0 faces: 9 internal faces: 0 cells: 2 boundary patches: 6 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 0 prisms: 1 wedges: 0 pyramids: 0 tet wedges: 1 tetrahedra: 0 polyhedra: 0 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. *Number of regions: 2 The mesh has multiple regions which are not connected by any face. <<Writing region information to "0/cellToRegion" Checking patch topology for multiply connected surfaces ... Patch Faces Points Surface topology back 1 4 ok (non-closed singly connected) bottom 2 4 ok (non-closed singly connected) front 1 4 ok (non-closed singly connected) left 1 4 ok (non-closed singly connected) right 1 4 ok (non-closed singly connected) top 2 4 ok (non-closed singly connected) Checking geometry... Overall domain bounding box (-1 -1 0) (1 1 1) Mesh (non-empty, non-wedge) directions (1 1 1) Mesh (non-empty) directions (1 1 1) ***Boundary openness (0 0.171573 0) possible hole in boundary description. ***Open cells found, max cell openness: 1, number of open cells 1 <<Writing 1 non closed cells to set nonClosedCells Minimum face area = 1. Maximum face area = 2. Face area magnitudes OK. Min volume = 0.722222. Max volume = 1. Total volume = 1.72222. Cell volume s OK. Non-orthogonality check OK. Face pyramids OK. Max skewness = 0.421474 OK. Coupled point location match (average 0) OK. Failed 2 mesh checks. End Code:
FoamFile { version 2.0; format ascii; class polyBoundaryMesh; location "constant\polyMesh"; object boundary; } 6 ( back { type zeroGradient; nFaces 1; startFace 0; } bottom { type zeroGradient; nFaces 2; startFace 1; } front { type zeroGradient; nFaces 1; startFace 3; } left { type zeroGradient; nFaces 1; startFace 4; } right { type zeroGradient; nFaces 1; startFace 5; } top { type zeroGradient; nFaces 2; startFace 6; } ) Code:
FoamFile { version 2.0; format ascii; class faceList; location "constant/polyMesh"; object faces; } 9 ( 4(0 2 6 1) 3(5 6 4) 3(4 6 2) 4(1 6 5 3) 4(4 7 3 5) 4(0 7 4 2) 3(3 7 1) 3(1 7 0) 4(1 7 4 6) ) Code:
FoamFile { version 2.0; format ascii; class labelList; note "nPoints: 8 nCells: 2 nFaces: 9"; location "constant/polyMesh"; object neighbour; } 9 ( -1 -1 -1 -1 -1 -1 -1 -1 1 ) Code:
FoamFile { version 2.0; format ascii; class labelList; note "nPoints: 8 nCells: 2 nFaces: 9"; location "constant/polyMesh"; object owner; } 9 ( 1 0 1 0 0 1 0 1 0 ) Code:
FoamFile { version 2.0; format ascii; class vectorField; location "constant/polyMesh"; object points; } 8 ( (0 1 1) (-1 0 1) (0 1 0) (0 -1 1) (1 -0 0) (0 -1 0) (-1 0 0) (1 -0 1) ) Code:
FoamFile { version 2.0; format ascii; class cellSet; location "constant/polyMesh/sets"; object nonClosedCells; } 1 ( 1 ) Code:
FoamFile { version 2.0; format ascii; class labelList; location "0"; object cellToRegion; } 2(0 1) |
|
March 20, 2014, 05:46 |
A non-solution
|
#2 |
New Member
Richel Bilderbeek
Join Date: Nov 2013
Posts: 14
Rep Power: 13 |
I noted that after doing a renumberMesh and zipUpMesh I get a 'correct' mesh (that is: a mesh in which checkMesh does find errors in).
What is strange, it has two bent pentagons in: I posted the question http://www.cfd-online.com/Forums/ope...tml#post481044 , with a lot more detail. How can my -as far as I can see- correct mesh be labeled incorrect? How can my -as far as I can see- incorrect mesh be labeled correct? |
|
March 24, 2014, 10:08 |
Solved
|
#3 |
New Member
Richel Bilderbeek
Join Date: Nov 2013
Posts: 14
Rep Power: 13 |
I found out what caused the error: in the file 'boundary', the (unnamed) internal faces must be put first. Modifying 'boundary', reordering the files 'faces', 'neighbour' and 'owner' resulted in checkMesh reporting no errors. Below an image with face indices.
Complete files can be found at http://richelbilderbeek.nl/ToolOpenF...FoundFixed.htm
__________________
I will never accept a 'Friend' request, I will always accept beer |
|
December 7, 2015, 12:14 |
|
#4 | |
Senior Member
Join Date: Mar 2015
Posts: 250
Rep Power: 12 |
Hello Richel,
thanks for this interesting topic! What do you mean with internal faces in the boundary file? My boundary file usually only consists of my defined patches. Best regards, Kate Quote:
|
||
Tags |
boundary openness, checkmesh, mesh, open cells found, regions not connected |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Foam::error::PrintStack | almir | OpenFOAM Running, Solving & CFD | 92 | May 21, 2024 08:56 |
[snappyHexMesh] Layers not growing at all | zonda | OpenFOAM Meshing & Mesh Conversion | 12 | June 6, 2020 12:28 |
[snappyHexMesh] sHM layer process keeps getting killed | MBttR | OpenFOAM Meshing & Mesh Conversion | 4 | August 15, 2016 04:21 |
SigFpe when running ANY application in parallel | Pj. | OpenFOAM Running, Solving & CFD | 3 | April 23, 2015 15:53 |
Moving mesh | Niklas Wikstrom (Wikstrom) | OpenFOAM Running, Solving & CFD | 122 | June 15, 2014 07:20 |