CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... (http://www.cfd-online.com/Forums/openfoam-meshing-other/)
-   -   Defining boundary conditions on interior faces (http://www.cfd-online.com/Forums/openfoam-meshing-other/61728-defining-boundary-conditions-interior-faces.html)

melanie August 3, 2006 09:06

Hello, I'd like to add some
 
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 August 8, 2006 10:15

Hi, could anybody help me def
 
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

gschaider August 9, 2006 18:05

Hi Melanie! If you want to
 
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?

melanie August 10, 2006 02:28

Hi Bernhard ! thanks fo r y
 
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

gschaider August 10, 2006 03:48

faceSets as patches: not that
 
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.

hjasak August 10, 2006 03:58

Nope, not patches. Anyway, it
 
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

melanie August 10, 2006 06:58

I'm a little bit confused now:
 
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 ?

eugene August 10, 2006 08:44

Yes, you could. Take a look at
 
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.

melanie August 10, 2006 09:42

I looked through the wiki but
 
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

eugene August 10, 2006 09:52

Hmm, your right there is nothi
 
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.


All times are GMT -4. The time now is 17:33.