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

Defining boundary conditions on interior faces

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 3, 2006, 09:06
Default Hello, I'd like to add some
  #1
Member
 
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 8
melanie is on a distinguished road
Hello,

I'd like to add some boundary conditions on interior faces iimported from Fluent. I've tried splitMesh, but it creates only walls (I want to set a temperature condition and velocity direction on the interior face), and createPatch only operates on external faces... How can I handle my problem ?

Thanks!
melanie
melanie is offline   Reply With Quote

Old   August 8, 2006, 10:15
Default Hi, could anybody help me def
  #2
Member
 
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 8
melanie is on a distinguished road
Hi,
could anybody help me defining some boundary conditions on interior faces saved as faceSets ? I want to use it as a heating condition.
Thanks !
melanie
melanie is offline   Reply With Quote

Old   August 9, 2006, 18:05
Default Hi Melanie! If you want to
  #3
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Hi Melanie!

If you want to set a fixed temperature and a fixed velocity, a wall is perfect for you (both can be done on walls). If you want to transport anything (passive scalar, turbulence ...) through that wall: that's a bit more complicated.

I'm afraid (but that is out of my league), that setting boundary conditions on faces that are not on patches is not forseen in OF. Which means: it can be done, but it's going to get wild.

As I see it, the most elegant way is: use splitMesh and write your own BC for those "walls" (one that sets values for T and U and transports the rest through). But before that: what is the physical reality that you want to model?
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   August 10, 2006, 02:28
Default Hi Bernhard ! thanks fo r y
  #4
Member
 
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 8
melanie is on a distinguished road
Hi Bernhard !

thanks fo r your reply. The reason why I need this type of BC is that I'd like to model a heat exchanger in a duct; as a first approximation, a heat exchanger can be seen as introducing a heating condition, pressure drop condition and velocity condition (redressing and spreading velocity vectors) on a surface.

I didn't think about using the wall condition... I thought that the "wall" would always mean that nothing passes through this BC.

Is there a way to get OpenFOAM see faceSets and/or cellSets be seen as patches, apart from splitting the mesh ?

Thanks !
melanie
melanie is offline   Reply With Quote

Old   August 10, 2006, 03:48
Default faceSets as patches: not that
  #5
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
faceSets as patches: not that I'm aware of (but for a definite "No" you've got to aks someone with more knowledge about the OK-kernel - Henry, Hrv ...)

My best guess for your problem is to place at the right places in the solver forAll loops over the faceSet and adjust the values in the neighbouring cells according to your conditions (for velocity before or after solving the UEqn).

Or you introduce surfaceFields that act as source-Terms (only non-zero on the faceSets). But how to integrate them in the differential equations I'm not fully sure.
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   August 10, 2006, 03:58
Default Nope, not patches. Anyway, it
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Nope, not patches. Anyway, it is not done like that. You will need to end up with a cell based momentum sink and energy source because nothing is solved for on the faces anyway (they just handle the transport). Mesh zoning will help you define the location where the jump occurs, but the rest is just built into the equations.

Note that OpenFOAM looping in discretisation handles ALL internal faces in the same manner, even those created by, say, a sliding interfaces. This is critical for clean design, speed of execution, consistent discretisation and a bunch of other things that make OpenFOAM as good as it is.

BTW Bernhard, a surface field cannot appear as source in the cell-based equation - at the very least you need to hit it with a divergence operator, which will make a volume field out of it.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   August 10, 2006, 06:58
Default I'm a little bit confused now:
  #7
Member
 
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 8
melanie is on a distinguished road
I'm a little bit confused now: if I understand well, nothing can be done with either faceSets or cellSets ? and surfaceFields wouldn't either solve my problem ?
and what do you mean by:
Quote:
Mesh zoning will help you define the location where the jump occurs, but the rest is just built into the equations.
Could I define "mesh zoning" with cellSets and then apply my conditions on it ?
melanie is offline   Reply With Quote

Old   August 10, 2006, 08:44
Default Yes, you could. Take a look at
  #8
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Yes, you could. Take a look at addZones, faceZones, pointZones and cellZones functions in polyMesh.H.

An easier solution would however be to grab the existing porous media code from the wiki and build on that to implement your HE.
eugene is offline   Reply With Quote

Old   August 10, 2006, 09:42
Default I looked through the wiki but
  #9
Member
 
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 8
melanie is on a distinguished road
I looked through the wiki but I didn't found this porous media code... are you sure the code was posted there ? (and could you give me the link if yes ?)
thanks !
melanie
melanie is offline   Reply With Quote

Old   August 10, 2006, 09:52
Default Hmm, your right there is nothi
  #10
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Hmm, your right there is nothing there.

Just do a search for porous media on the forum. There have been a several discussions on the subject.
eugene 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
defining flux across face for interior boundary Sandilya Garimella FLUENT 2 October 10, 2009 00:05
Defining Boundary Conditions in GAMBIT Tim R FLUENT 3 April 14, 2008 04:30
Batch Mode : re-defining boundary conditions MaxiFLOW CFX 6 March 29, 2007 08:41
Defining Boundary conditions in gambit anthro FLUENT 2 February 14, 2007 10:17
'internal' and 'interior' boundary conditions Vishu FLUENT 0 January 28, 2004 22:25


All times are GMT -4. The time now is 20:37.