failed checkMesh after converting from .msh: non closed cells
 

HI,

I converted a .msh mesh using fluent3DMeshToFoam. When I did checkMesh, it failed with one error. I am wondering if someone can explain what might be wrong. Thanks!

Pei
----------------------------
*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.x-e8ca07322e45
Exec : checkMesh -constant
Date : Feb 02 2012
Time : 04:26:05
Host : "huwei"
PID : 6376
Case : /home/phsieh/OpenFOAM/phsieh-2.1.x/run/XPDuctReagentCompartmentTED-temp
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = constant

Time = constant

Mesh stats
points: 1584089
faces: 4490900
internal faces: 4370002
cells: 1453455
boundary patches: 19
point zones: 0
face zones: 10
cell zones: 5

Overall number of cells of each type:
hexahedra: 1392112
prisms: 10097
wedges: 0
pyramids: 3026
tet wedges: 0
tetrahedra: 2358
polyhedra: 45862

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
reagentboxwalls-coldfluiddomain-coldsink0 0 ok (empty)
reagentboxwalls-coldfluiddomain31793 33362 ok (non-closed singly connected)
reagentboxwalls-bottomplate-coldfluiddomain0 0 ok (empty)
reagentboxwalls-coldfluiddomain-intfan0 0 ok (empty)
reagentboxwalls-coldfluiddomain-gasket0 0 ok (empty)
reagentboxwalls-coldfluiddomain.10 0 ok (empty)
reagentboxwalls-bottomplate72221 73391 ok (non-closed singly connected)
reagentboxwalls-bottomplate-coldsink0 0 ok (empty)
reagentboxwalls-bottomplate-gasket0 0 ok (empty)
reagentboxwalls-bottomplate-intfan0 0 ok (empty)
reagentboxwalls-coldsink12233 13258 ok (non-closed singly connected)
reagentboxwalls-coldsink-gasket0 0 ok (empty)
reagentboxwalls-intfan3227 3448 ok (non-closed singly connected)
tec-aacoldside 240 284 ok (non-closed singly connected)
tec-abcoldside 240 284 ok (non-closed singly connected)
tec-bacoldside 234 269 ok (non-closed singly connected)
tec-bbcoldside 230 264 ok (non-closed singly connected)
tec-cacoldside 240 284 ok (non-closed singly connected)
tec-cbcoldside 240 284 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (0.01905 0.0011176 0.00339) (0.59944 0.174752 0.23876)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (-8.124018e-12 -3.083973e-10 1.897114e-10) OK.
***Open cells found, max cell openness: 1.975231e-05, number of open cells 327
<<Writing 327 non closed cells to set nonClosedCells
Minumum face area = 2.76708e-08. Maximum face area = 0.0003448002. Face area magnitudes OK.
Min volume = 6.216637e-12. Max volume = 5.605517e-06. Total volume = 0.02017582. Cell volumes OK.
Mesh non-orthogonality Max: 69.84655 average: 6.289126
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 1.21916 OK.
Coupled point location match (average 0) OK.

Failed 1 mesh checks.

End

Greetings Pei-Ying,

I saw that kind of error occur when we tried to manually fix a wrong oriented face that was created by snappyHexMesh. Basically, by right orienting the face, the cell that used it was then considered to be open.
So far, it looks to me that cells in OpenFOAM are inferred from faces and therefore one cannot simply change a couple of faces without having to affect all of the surrounding faces.

You can use foamToVTK to convert the set "nonClosedCells" to VTK files, so you can see where the troublesome cells are located. Standard fixing solution is to re-mesh it again in the troublesome area before converting once more.

Best regards,
Bruno

Hi, Bruno,

Thanks for the info. I did do a quick check of the nonClosedCells set in paraview, but, did not find anything obvious. This mesh was done in ANSYS Workbench using cutCell method. There are lots small gaps in the domain. I am not sure if cutCell allows me to just re-mesh the failed area.

Pei-Ying

Hi Pei-Ying,

Same problem as yours.

I have generated my mesh with ICEMCFD hexa. I also use the command fluent3DMeshToFoam to convert the mesh.

After checkMesh I get the same error message:
***Open cells found, max cell openness: 1, number of open cells 1110
<<Writing 1110 non closed cells to set nonClosedCells

Have you solved the problem ?

Best regards,
Stephane.

Hi, Stephane,

I ended up cleaning up the CAD geometries further and re-meshed the domain.

Pei-Ying

Hi,

I have solved my problem (nonClosedCells) by putting periodicity for verticies located on the axis. I have selected 2 times the same vertex.
The picture shows a blade (propeller has 5 blades), the shaft and a vertical cut in the wake.

Regards,

Stephane.

Hi Stephane,

I got the same problem here. Could you elaborate on how you solved the problem?

Really appreciate it.

Best,

Hang

Hi Hang,

I use ICEMCFD hexa to generate the mesh. Inside ICEMCFD you can check the mesh. If you have nonClosedCells you have to solve the problem before going ahead.

I have solved my problem (nonClosedCells) by putting periodicity for verticies located on the axis. I have selected 2 times the same vertex.

Regards,

Stephane.

I am having problems converting a mesh as well. I have a mesh generated with Tgrid 5.0.6. It's a hexcore mesh with prisms, and I have two copies: one with conformal pyramids on the tet-quad interface, and another with non conformal split tris on the interface. Both meshes are being read from a fluent 6.3.26 case file, written in ascii format.

When using fluent3DMeshToFoam, I get thousands of nonClosedCells, all of them occuring where a step is made in hex cell size. Does anyone have any tips here? Surely there are hexcore meshes from fluent that have been solved in FOAM.

yep!
try to convert your mesh with "tpoly"
http://aerojet.engr.ucdavis.edu/flue...238.htm#224889

I will give this a try, but currently I export from Tgrid with the "write as polyhedra" option. I thought this was the same thing? I will try it nonetheless and report back.

Yep, tpoly works. I guess as far as openFOAM goes, tpoly and "write as polyhedra" within tgrid are not equivalent, even though they are as far as fluent is concerned. Thanks for the tip!

Now time to get my CD down from 1e+7 down to less than 1....