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

Beginner needs help with BCs and solver

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 4, 2011, 18:23
Question Beginner needs help with BCs and solver
  #1
New Member
 
Join Date: Jun 2011
Posts: 12
Rep Power: 6
homerun4711 is on a distinguished road
Hello!

I am quite new to OpenFOAM and trying to figure out if OpenFOAM
could be used for a project my company is working on. I personally like
the program because of its clear and simple syntax and its configuration
via human-readable text files.
And I would like to use it for our calculations if it fits our needs.

Till now I finished some tutorials I found in the users guide and in the
internet. I found only little information on heat transfer and heat
conduction and I am a bit confused of all the solvers around.

I attached a picture showing our system and the BCs we need.
It is a 2D cut through a cooling tower.

Is there a solver that fits all my needs or do I have to start a new one?
And which border conditions will fit our needs?

You don´t have do write long explanations, I would be thankful if you
could just push me in the right directions. Any information is welcome.

Kind regards,
Walter
Attached Images
File Type: jpg mesh_tower.jpg (48.2 KB, 74 views)
homerun4711 is offline   Reply With Quote

Old   June 5, 2011, 16:06
Default
  #2
Senior Member
 
Join Date: Mar 2011
Posts: 155
Rep Power: 6
tH3f0rC3 is on a distinguished road
Hi,

I now that I have read about the Solver chtMultiRegionRadFoam. Someone has added radiation to chtMultiRegionFoam-Solver.
The chtMultiRegionFoam-Solver is a transient solver for heat transfer. -> ChtMultiRegionFoam and P1 radiation model

I think you can use the solver chtMultiRegionRadFoam for your problem. But I don't know if this solver is used for complex geometries because I know that this solver was tested only to simple geometries.

I hope my response was helpful,

Best Regards,
tH3f0rC3
tH3f0rC3 is offline   Reply With Quote

Old   June 6, 2011, 03:14
Default
  #3
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
I don't think chtMultiRegionFoam is the right tool for this purpose. The way I understand it you only want to simulate the heat transfer within the wall, and use special boundary conditions on the surface. Is that right? In that case the solver you want is just scalarTransportFoam, and add the right BCs. groovyBC is always worth a look if the built in BCs aren't enough, as it might be the case for your radiation + convection boundary.
akidess is offline   Reply With Quote

Old   June 6, 2011, 04:15
Default
  #4
New Member
 
Join Date: Jun 2011
Posts: 12
Rep Power: 6
homerun4711 is on a distinguished road
Hi!

Thanks for your answers.

I guess chtMultiRegionRadFoam is for solids in contact with fluids.
This is not neccessary so far.
Our first model should only include a fixed heat flux to the air
inside the tower. Maybe later we will include that, too.

I had a look into scalarTransportFoam and laplacianFoam and the difference
between them is that laplacianFoam misses

+ fvm::div(phi, T)

in the equation definition.

I looked it up in my heat transfer text book, but could not find it.
What does this part of the heat equation stand for?

Is it possible to add multiple boundary conditions to the same border
in OpenFOAM or is it neccessary to use the mentioned groovyBC in
that case?
homerun4711 is offline   Reply With Quote

Old   June 6, 2011, 04:27
Default
  #5
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
Very good - the term div(phi,T) is the convective term of the transport equation, and since you are looking at a solid laplacianFoam is indeed what you need! (phi is a flux obtained by multiplying the fluid velocity with a cell face area).

You can only specify one boundary condition per variable and border.

By the way, you can mesh your geometry with hexahedral cells without too much effort, and it will improve the convergence of your calculations. It won't make a huge difference because this problem is fairly easy to solve, but it might come in handy if you want to do a big batch of calculations.
akidess is offline   Reply With Quote

Old   June 6, 2011, 11:23
Default
  #6
New Member
 
Join Date: Jun 2011
Posts: 12
Rep Power: 6
homerun4711 is on a distinguished road
Ok, so I can only specify one bc per boundary. Argh.
I am a bit lost right now, because I do not know if it
is possible at all to set all three BCs using groovyBC.
Is it?
So far I only read about people using it to set convection
of heat to the ambient temperature...

In principle all BCs I need are heat fluxes (solar in, convection out, radiation out). And I guess we do not need a complicated radiation model
like P1 or DOM. Just adding a heat flux like

P = sigma_Boltzmann * ViewFactor * (T_inf - T_surface)

would do the trick.(In our case the viewfactor would be 0.5)

Also convection would be a constant factor in the first case.
Just some value from a lookup-table (10 W/m^2).

Any ideas what I could do?
homerun4711 is offline   Reply With Quote

Old   June 7, 2011, 03:59
Default
  #7
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
It should be possible to do this with groovyBC. Just take a sheet of paper and write down all contributions to the wall heat flux (q = q_sun - q_conv - q_rad). Once you have a nice formula for the total heat flux, have a look at how people write a convection BC with groovyBC and it should be straightforward to extend that with the other two fluxes.
akidess is offline   Reply With Quote

Old   June 7, 2011, 04:28
Default
  #8
New Member
 
Join Date: Jun 2011
Posts: 12
Rep Power: 6
homerun4711 is on a distinguished road
Ok, sounds good

But there is still the problem that one of the heat fluxes, the sun irradiation,
is trasient and written in a text file. So far I could not figure out
if groovyBC can deal with this. Can you tell me if this is possible?
homerun4711 is offline   Reply With Quote

Old   June 7, 2011, 04:50
Default
  #9
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
You could certainly approximate your datapoints by a polynomial function and then put it into groovyBC, but I think the BC can also read timelines from a file - see http://openfoamwiki.net/index.php/Co...oovyBC#wobbler.

I've never used that particular functionality so I can't help you much on how to use it, but maybe the example on the wiki is enough to get you started.
akidess is offline   Reply With Quote

Old   June 7, 2011, 08:22
Default
  #10
New Member
 
Join Date: Jun 2011
Posts: 12
Rep Power: 6
homerun4711 is on a distinguished road
Ok, that looks good.
One must have eagle eyes to find that
Thank you very much!
homerun4711 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
Dealing with BC's in OF 1.6 vkrastev OpenFOAM Running, Solving & CFD 5 September 4, 2012 11:58
[GAMBIT] BC's value assignment in Gambit Vs. Fluent (solver) hadikhayyamian ANSYS Meshing & Geometry 5 December 21, 2010 13:28
Periodic BC's and Stone SIP Solver ilyasy Main CFD Forum 0 August 14, 2009 06:04
Need Assistance: BCs for k-e model implementation Dean Schrage Main CFD Forum 3 August 11, 2001 01:02
Wall BC's for a NS solver André Burdet Main CFD Forum 6 December 8, 2000 22:45


All times are GMT -4. The time now is 11:23.