CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...

failed checkMesh after converting from .msh: non closed cells

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 2, 2012, 05:43
Default failed checkMesh after converting from .msh: non closed cells
  #1
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 271
Rep Power: 9
phsieh2005 is on a distinguished road
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
phsieh2005 is offline   Reply With Quote

Old   February 2, 2012, 06:07
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
wyldckat is offline   Reply With Quote

Old   February 2, 2012, 17:29
Default
  #3
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 271
Rep Power: 9
phsieh2005 is on a distinguished road
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
phsieh2005 is offline   Reply With Quote

Old   March 9, 2012, 09:38
Default
  #4
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
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.
openfoam_user is offline   Reply With Quote

Old   March 9, 2012, 14:21
Default
  #5
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 271
Rep Power: 9
phsieh2005 is on a distinguished road
Hi, Stephane,

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

Pei-Ying
phsieh2005 is offline   Reply With Quote

Old   March 12, 2012, 04:51
Default
  #6
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
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.
Attached Images
File Type: jpg screen.jpg (103.2 KB, 131 views)
openfoam_user is offline   Reply With Quote

Old   June 3, 2012, 17:36
Default
  #7
Member
 
HD
Join Date: Jul 2011
Posts: 56
Rep Power: 6
Rebecca513 is on a distinguished road
Hi Stephane,

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

Really appreciate it.

Best,

Hang
Rebecca513 is offline   Reply With Quote

Old   June 4, 2012, 02:43
Default
  #8
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 300
Rep Power: 9
openfoam_user is on a distinguished road
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.
openfoam_user is offline   Reply With Quote

Old   September 19, 2012, 06:55
Default
  #9
Member
 
Join Date: Mar 2009
Posts: 72
Rep Power: 8
aerogt3 is on a distinguished road
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.
aerogt3 is offline   Reply With Quote

Old   September 19, 2012, 07:12
Default
  #10
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,972
Rep Power: 30
-mAx- will become famous soon enough
yep!
try to convert your mesh with "tpoly"
http://aerojet.engr.ucdavis.edu/flue...238.htm#224889
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   September 19, 2012, 07:16
Default
  #11
Member
 
Join Date: Mar 2009
Posts: 72
Rep Power: 8
aerogt3 is on a distinguished road
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.
aerogt3 is offline   Reply With Quote

Old   September 20, 2012, 08:51
Default
  #12
Member
 
Join Date: Mar 2009
Posts: 72
Rep Power: 8
aerogt3 is on a distinguished road
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....
aerogt3 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Import netgen mesh to OpenFOAM hsieh Open Source Meshers: Gmsh, Netgen, CGNS, ... 32 September 13, 2011 05:50
ParaView/Parafoam error when making animation Disco_Caine OpenFOAM Paraview & paraFoam 6 September 28, 2010 09:54
user subroutine error CFDUSER CFX 2 December 9, 2006 07:31
user defined function cfduser CFX 0 April 29, 2006 10:58
physical boundary error!! kris CD-adapco 2 August 3, 2005 00:32


All times are GMT -4. The time now is 14:58.