CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

cyclic boundary with same geometric size but different number of faces?

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

Like Tree1Likes
  • 1 Post By strikeraj

Reply
 
LinkBack Thread Tools Display Modes
Old   April 17, 2012, 21:53
Default cyclic boundary with same geometric size but different number of faces?
  #1
New Member
 
Tom Li
Join Date: Aug 2011
Posts: 16
Rep Power: 6
strikeraj is on a distinguished road
Hi

I am just wondering if this is possible.
I have a 3D rectangular domain. It is meshed in ICEM with unstructured grid, save to fluent .msh and converted in openfoam using fluent3DMeshToFoam.
But when I try to run it, it says the number of faces does not match on the two patches that I set as cyclic. Is there a way to work this out without remeshing the faces with a structured grid? If not, does my way of generating and exporting mesh works when I put a structured surface mesh on both sides?

Thanks in advance

Cheers,
Tom
strikeraj is offline   Reply With Quote

Old   May 6, 2012, 16:16
Default
  #2
New Member
 
Tom Li
Join Date: Aug 2011
Posts: 16
Rep Power: 6
strikeraj is on a distinguished road
sorry to bump this up but can anyone give me an idea on how to put on cyclic BC on an unstructured mesh?

Many thanks
strikeraj is offline   Reply With Quote

Old   May 7, 2012, 10:50
Default
  #3
New Member
 
Michael Ahlmann
Join Date: Feb 2010
Posts: 27
Rep Power: 7
danishdude is on a distinguished road
The original cyclic condition requires point matched faces. However, the cyclicAMI condition allows you to use a cyclic condition without point matching. It's available in OF 2.1.
danishdude is offline   Reply With Quote

Old   May 8, 2012, 12:44
Default
  #4
New Member
 
Bruno
Join Date: Apr 2011
Posts: 2
Rep Power: 0
brunotojo is on a distinguished road
Yes, it is possible. In ICEM you need to define the mesh as periodic in Mesh>Global Mesh Setup>Set up periodicity.

And then, after converting to OpenFoam format, you will need to use createPatch (there are a lot of post about this here) to define your periodic boundary.

I am also new to OpenFoam so, I am not sure if this will work for every case, but for me it did.

Best regards,
Bruno
brunotojo is offline   Reply With Quote

Old   May 8, 2012, 12:46
Default
  #5
New Member
 
Tom Li
Join Date: Aug 2011
Posts: 16
Rep Power: 6
strikeraj is on a distinguished road
Thanks Michael and Bruno for your reply.
I will take a look into both methods after I finish my work on hand and I will let you know how it works out
strikeraj is offline   Reply With Quote

Old   May 15, 2012, 18:58
Default
  #6
New Member
 
Tom Li
Join Date: Aug 2011
Posts: 16
Rep Power: 6
strikeraj is on a distinguished road
Quote:
Originally Posted by danishdude View Post
The original cyclic condition requires point matched faces. However, the cyclicAMI condition allows you to use a cyclic condition without point matching. It's available in OF 2.1.
Hi Michael

I have just tried my case with the cyclicAMI BC and it works if i run it serial.
But when I try to use decomposePar and run in parallel with mpirun, error occurs. Do you have clue on what might be wrong?

Thanks very much for your time

Cheers,
Tom

attached is the error log file
Attached Files
File Type: zip log.1.1.0.zip (2.5 KB, 21 views)

Last edited by strikeraj; May 15, 2012 at 19:09. Reason: attach log
strikeraj is offline   Reply With Quote

Old   May 16, 2012, 11:10
Default
  #7
New Member
 
Michael Ahlmann
Join Date: Feb 2010
Posts: 27
Rep Power: 7
danishdude is on a distinguished road
Any chance you can upload the case somewhere so I can take a closer look? If it's not too big, you can e-mail it to me at mahlmann@ucdavis.edu
danishdude is offline   Reply With Quote

Old   May 21, 2012, 07:02
Default
  #8
Member
 
Join Date: Apr 2010
Posts: 61
Rep Power: 7
alquimista is on a distinguished road
Hello,

I had the same questions months ago and in my opinion the best option was to use the extend version of OpenFOAM. It has General Interface Grid implemented. There's more information available on internet.

https://cmg.soton.ac.uk/community/at...LloydAug11.pdf
http://www.tfd.chalmers.se/~hani/kur...dy_2010_OP.pdf

Good luck.
alquimista is offline   Reply With Quote

Old   May 21, 2012, 10:43
Default
  #9
New Member
 
Tom Li
Join Date: Aug 2011
Posts: 16
Rep Power: 6
strikeraj is on a distinguished road
Update:

I have posted this on the bug tracker and got a reply with working solution:

Quote:
The AMI assumes the patches are collocated - if not you have to specify the 'transform' type. (This does not affect serial running since it uses a different code path).

Add transform=translational and a separationVector to your constant/polyMesh/boundary file and it should work:

CYCLIC1
{
type cyclicAMI;
neighbourPatch CYCLIC2;
transform translational;
separationVector (0 0 -0.0914);
nFaces 9824;
startFace 593664;
}

CYCLIC2
{
type cyclicAMI;
neighbourPatch CYCLIC1;
transform translational;
separationVector (0 0 0.0914);
nFaces 11028;
startFace 615000;
}
Thoma likes this.
strikeraj is offline   Reply With Quote

Old   December 13, 2013, 13:35
Default decompose par for cyclicAMI bc
  #10
New Member
 
swapnil
Join Date: Jun 2013
Posts: 1
Rep Power: 0
swapnilsalokhe is on a distinguished road
Hi Tom Li,

When you are using any cyclic boundary in decomposePar you have to set both cyclic planes on one processor then only it will work on parallel processors.


Quote:
Originally Posted by strikeraj View Post
Hi Michael

I have just tried my case with the cyclicAMI BC and it works if i run it serial.
But when I try to use decomposePar and run in parallel with mpirun, error occurs. Do you have clue on what might be wrong?

Thanks very much for your time

Cheers,
Tom

attached is the error log file
swapnilsalokhe 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
Problem with parallel run Hisham OpenFOAM Running, Solving & CFD 9 March 13, 2012 09:31
critical error during installation of openfoam Fabio88 OpenFOAM Installation 21 June 2, 2010 03:01
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 00:55.