|
[Sponsors] |
[Commercial meshers] Defining boundary conditions on interior faces |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
August 3, 2006, 10:06 |
Defining boundary conditions on interior faces
|
#1 |
Member
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
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 |
|
August 8, 2006, 11:15 |
Hi,
could anybody help me def
|
#2 |
Member
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
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 |
|
August 9, 2006, 19:05 |
Hi Melanie!
If you want to
|
#3 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
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 |
|
August 10, 2006, 03:28 |
Hi Bernhard !
thanks fo r y
|
#4 |
Member
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
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 |
|
August 10, 2006, 04:48 |
faceSets as patches: not that
|
#5 |
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 |
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 |
|
August 10, 2006, 04:58 |
Nope, not patches. Anyway, it
|
#6 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 |
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 |
|
August 10, 2006, 07:58 |
I'm a little bit confused now:
|
#7 | |
Member
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
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:
|
||
August 10, 2006, 09:44 |
Yes, you could. Take a look at
|
#8 |
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 |
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. |
|
August 10, 2006, 10:42 |
I looked through the wiki but
|
#9 |
Member
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 17 |
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 |
|
August 10, 2006, 10:52 |
Hmm, your right there is nothi
|
#10 |
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 |
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. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Centrifugal fan | j0hnny | CFX | 13 | October 1, 2019 14:55 |
CFD analaysis of Pelton turbine | amodpanthee | CFX | 31 | April 19, 2018 19:02 |
Velocity vector in impeller passage | ngoc_tran_bao | CFX | 24 | May 3, 2016 22:16 |
Difficulty In Setting Boundary Conditions | Moinul Haque | CFX | 4 | November 25, 2014 18:30 |
Low Mixing time Problem | Mavier | CFX | 5 | April 29, 2013 01:00 |