CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Meshing & Mesh Conversion

[mesh manipulation] more than two regions to join using stitchMesh partial or perfect option

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

Like Tree6Likes
  • 1 Post By Lada
  • 1 Post By jherb
  • 4 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 30, 2011, 14:05
Default more than two regions to join using stitchMesh partial or perfect option
  #1
New Member
 
vladimir krejci
Join Date: Mar 2009
Location: Czech Republic
Posts: 20
Rep Power: 14
Lada is on a distinguished road
It seems when attaching a mesh using partial option there can be only one such interface and it must be the last one in the joining sequence.
I have created a rather simple case made of three cylinders which I want to join to make a single pipe. The cylinders are meshed completely the same. The only difference is they are offset axially by their respective heights.
When I merge them and stitch them using perfect option, everything goes smoothly. When the first interface is stitched as perfect and the second one as partial, no problems rise. But when the first stitching is partial and the second one perfect, the second one is not performed resulting in an error:

--> FOAM FATAL ERROR:
Master or slave face zone contain no faces. Please check your mesh definition.

From function void slidingInterface::checkDefinition()
in file slidingInterface/slidingInterface.C at line 97.

Has anyone encountered this weird behaviour of stitchMesh utility when applied to join more than two meshes?
Is there a way out?

I hope the attached case might help to solve the puzzle. Just run the Allrun script to see the error in the log.stitchMesh_2 file.
Attached Files
File Type: gz join_three_meshes.tar.gz (3.3 KB, 70 views)
Zhiheng Wang likes this.
Lada is offline   Reply With Quote

Old   November 25, 2011, 13:09
Default bugreport
  #2
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 614
Rep Power: 18
jherb is on a distinguished road
I can reproduce this problem (with/without the -partial option) and have reported a bug at:
http://www.openfoam.com/mantisbt/view.php?id=347
Zhiheng Wang likes this.
jherb is offline   Reply With Quote

Old   October 20, 2013, 03:48
Default
  #3
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,962
Blog Entries: 45
Rep Power: 123
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Greetings to all!

I was browsing the list of bugs still open at OpenFOAM's bug tracker, when I spotted the bug report that points to this thread.

I gave the case a try and reproduced the same error. But I applied the solution I had found some time ago here: http://www.cfd-online.com/Forums/ope...tml#post433137 post #10 - and attached is the result.
It can stitch the 3 meshes just fine, as long as the file "constant/polyMesh/meshModifiers" is removed between stitches.

In addition, the attached case also demonstrates how to use my own little utility stitchMeshMultiPatch: https://github.com/wyldckat/stitchMeshMultiPatch

Best regards,
Bruno
Attached Files
File Type: gz join_three_meshes_fixed.tar.gz (3.8 KB, 59 views)
__________________
wyldckat is offline   Reply With Quote

Old   May 28, 2015, 09:52
Default
  #4
New Member
 
Join Date: May 2015
Posts: 2
Rep Power: 0
braker is on a distinguished road
@wyldckat
Thank you very much, that just solved the problem!
braker is offline   Reply With Quote

Old   April 12, 2017, 11:00
Default
  #5
New Member
 
Laszlo Barta
Join Date: Nov 2015
Posts: 8
Rep Power: 7
LaszloBarta is on a distinguished road
Hello,
I have a multiregion case, I would like to stitch or merge meshes of the regions into a single mesh. But I would like to retain the zones for defining porous zones. Could anyone tel me if that is possible and if yes, how?
Thanks
Laszlo
LaszloBarta is offline   Reply With Quote

Old   June 17, 2018, 16:29
Default
  #6
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,962
Blog Entries: 45
Rep Power: 123
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick note: As I've just indicated in report https://bugs.openfoam.org/view.php?id=347
Quote:
This issue was fixed back in April 2018, in commit 484c16a5da1896d1141f832aecfbfc0ce251f434 of OpenFOAM-dev.

The solution was to not write the mesh modifiers, therefore 'stitchMesh' would not load those modifiers the next time it is run.
@LaszloBarta: I hope you've solved your problem.
__________________
wyldckat is offline   Reply With Quote

Reply

Tags
stitchmesh

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wrong multiphase flow at rotating interface Sanyo CFX 14 February 7, 2017 17:19
Multiphase flow - incorrect velocity on inlet Mike_Tom CFX 6 September 29, 2016 01:27
Error - Solar absorber - Solar Thermal Radiation MichaelK CFX 12 September 1, 2016 05:15
sliding mesh problem in CFX Saima CFX 45 September 22, 2015 10:53
Waterwheel shaped turbine inside a pipe simulation problem mshahed91 CFX 3 January 10, 2015 11:19


All times are GMT -4. The time now is 06:44.