CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Pointwise & Gridgen

mismatch between faces of periodic domains

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 16, 2014, 13:31
Default mismatch between faces of periodic domains
  #1
Member
 
Jace
Join Date: Oct 2012
Posts: 77
Rep Power: 6
zhengzh5 is on a distinguished road
Hi,

I created a structured domain, and used it to create a periodic domain with a rotation of 40 degrees in my mesh. It all seems to be going well until I exported the mesh to OpenFOAM and performed a checkMesh. It essentially complains about the faces not matching each other. I did a quick visualization in paraview using the labelID specified by the checkMesh error and found that the 2 faces that are supposed to be matched in the cyclic BC are completely off. They are located on the opposite end of the periodic domain....

Does anyone know what's going on there?

Thanks,

Jason
zhengzh5 is offline   Reply With Quote

Old   April 16, 2014, 16:59
Default
  #2
Member
 
Payam D.
Join Date: Aug 2011
Posts: 83
Blog Entries: 3
Rep Power: 7
pdp.aero is on a distinguished road
Quote:
Originally Posted by zhengzh5 View Post
Hi,

I created a structured domain, and used it to create a periodic domain with a rotation of 40 degrees in my mesh. It all seems to be going well until I exported the mesh to OpenFOAM and performed a checkMesh. It essentially complains about the faces not matching each other. I did a quick visualization in paraview using the labelID specified by the checkMesh error and found that the 2 faces that are supposed to be matched in the cyclic BC are completely off. They are located on the opposite end of the periodic domain....

Does anyone know what's going on there?

Thanks,

Jason
Hi Jason,

Can you please attach your grid's picture? your axis along with your periodic domains.
My first suggestion is make sure that your axis is perfectly straight and horizontal (depends on your axis direction though.)
pdp.aero is offline   Reply With Quote

Old   April 17, 2014, 10:56
Default
  #3
Senior Member
 
David Garlisch
Join Date: Jan 2013
Location: Pointwise HQ
Posts: 138
Rep Power: 5
dgarlisch is on a distinguished road
This is a known limitation (bug) in the Pointwise OpenFOAM (OF) exporter.

The faces on matched periodic/cyclic boundaries are not numbered in the correct order.

The only workaround is to adjust the exported grid with OF tools. Someone else with OF skills will need to give you details on how to run these tools.

Please submit a bug report to Pointwise support.
dgarlisch is offline   Reply With Quote

Old   April 17, 2014, 15:32
Default
  #4
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 387
Rep Power: 13
cnsidero is on a distinguished road
Quote:
Originally Posted by zhengzh5 View Post
Hi,

I created a structured domain, and used it to create a periodic domain with a rotation of 40 degrees in my mesh. It all seems to be going well until I exported the mesh to OpenFOAM and performed a checkMesh. It essentially complains about the faces not matching each other. I did a quick visualization in paraview using the labelID specified by the checkMesh error and found that the 2 faces that are supposed to be matched in the cyclic BC are completely off. They are located on the opposite end of the periodic domain....

Does anyone know what's going on there?

Thanks,

Jason
The matching of periodic domains created in Pointwise is lost when exported to OpenFOAM. Geometrically the points and faces are periodic but the face ordering - as you've found out - is not guaranteed.

You can however recreate the periodic coupling, called cyclic in OpenFOAM-speak, using the createPatch utility. Refer to the location of the createPatch utility

Code:
$FOAM_UTILITIES/mesh/manipulation/createPatch/
for an example createPatchDict that is set up to recreate cyclic coupling between patches.

-Chris
cnsidero is online now   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
Foam::error::PrintStack almir OpenFOAM Running, Solving & CFD 62 June 16, 2016 03:01
No layers in a small gap bobburnquist OpenFOAM Native Meshers: snappyHexMesh and Others 6 August 26, 2015 09:38
snappyhexmesh remove blockmesh geometry philipp1 OpenFOAM Running, Solving & CFD 2 December 12, 2014 11:58
Add Mesh Layers doesnt work on the whole surface Kryo OpenFOAM Native Meshers: snappyHexMesh and Others 8 September 13, 2012 09:28
[Other] Mesh Importing Problem cuteapathy ANSYS Meshing & Geometry 1 June 7, 2012 13:39


All times are GMT -4. The time now is 15:24.