
[Sponsors] 
April 18, 2005, 05:53 
Hi,
I want to calculate the

#1 
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 11 
Hi,
I want to calculate the airflow in a room with heated walls and a ventilation in and outlet. Do you have any hint, which solver I should use? I found 'turbfoam' for incompressible, turbulent flow, but it does not seem that it supports buoyancy. The other solver I found is 'buoyantFoam'. This one is for compressible flow and does not seem to be suitable either... Can you make a suggestion? Greetings! Fabian 

April 18, 2005, 06:18 
'buoyantFoam' is suitable, in

#2 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 14 
'buoyantFoam' is suitable, in fact it was developed for exactly this kind of flow. Why do you think it is unsuitable? There is also 'buoyantSimpleFoam' for steadystate buoyancydriven flows.


April 18, 2005, 06:55 
Hi,
because it is for compres

#3 
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 11 
Hi,
because it is for compressible flow!? And usually we use a incompressible solver. Fabian 

April 18, 2005, 07:03 
... but buoyancydriven flows

#4 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 14 
... but buoyancydriven flows are compressible; the density changes as a function of temperature and pressure!


April 19, 2005, 01:14 
...but the Manumber is smalle

#5 
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 11 
...but the Manumber is smaller than 0.3, so you should be able to use incompressible.
Actually I would be the first at our building technology institute who is using a compressible one. Doesn't it take longer to get convergence with a compressible solver? Greetings! Fabian 

April 19, 2005, 03:46 
You could make the assumption

#6 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 14 
You could make the assumption of incompressibility if it is appropriate for your problem but remember compressibility is not just about the Manumber, the density could significantly vary due to pressure changes as a consequence of bodyforces e.g. gravity in the atmosphere and I didn't want to limit the kind of buoyancydiven flows than buoyantFoam could be applied to.
If the assumption of incompressibility is important to you it would not be difficult to remove the compressibility effects from buoyantFoam but I doubt it will make much difference to the performance of the code because it already uses a lowManumber pressure solver and the compressibility effects make that slightly diagonally dominant which is beneficial to convergence. The only downside of maintaining compressibility effects is the possibility of the solution supporting waves which would not be present in a incompressible solution and which you may not be interested in. 

April 20, 2005, 01:29 
I think it is good that there

#7 
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 11 
I think it is good that there is no limit, but in a room it is possible to neglect the change of density due to pressure differences.
I will try the buoyantFoam, but maybe you can give me a hint, how to remove the compressibility effects. My Prof. wants to have incompressible. Greetings! Fabian 

April 20, 2005, 03:15 
I am not sure what approximati

#8 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 14 
I am not sure what approximations your Prof would like you to introduce but you have the source code for buoyantFoam and are free to change it in anyway he feels is appropriate.
Could you please explain why your Prof wants incompressible given that compressible is already implemenented and more realistic? What do you gain from the assumption of incompressibility? 

April 21, 2005, 01:23 
Hi,
he mentioned, that it w

#9 
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 11 
Hi,
he mentioned, that it won't converge as fast ... but I will try out compressible with the low Manumber pressure solver; I actually did not tell him about that. Changing it to incompressible, is it enought to take care about the files in : OpenFOAM1.1/applications/solvers/heatTransfer/buoyantFoam Greetings! Fabian 

April 21, 2005, 03:31 
> he mentioned, that it won't

#10 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 14 
> he mentioned, that it won't converge as fast ...
How does he know? You said that all the codes you have are incompressible or is there one in which he could have tried both compressible and incompressible? As I have said before running compressible will actually improve the convergence of the pressure solver but may affect the overall convergence by supporting pressure waves but give that your flow is lowMa and in a small domain I doubt there will be much difference. > Changing it to incompressible, is it enought to take care about the files in : OpenFOAM1.1/applications/solvers/heatTransfer/buoyantFoam Yes. 

April 21, 2005, 04:10 
Sorry, I forgot to mention, th

#11 
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 11 
Sorry, I forgot to mention, that we use fluent and cfx.
As soon, as I get my fluent mesh into OpenFoam, I try out compressible and when I got the incompressible variant (if I can get done), I will compare both and let you know. Now, I'am actually curious about the differences. Greetings! Fabian 

April 21, 2005, 05:39 
FOAM has been compared with CF

#12 
Senior Member
Join Date: Mar 2009
Posts: 854
Rep Power: 14 
FOAM has been compared with CFX for buoyancydriven flows a few years ago and as far as I am aware the solution algorithms are very similar and CFX also includes the effect of pressure in density as in buoyantFoam. Either way the solutions were VERY similar.
Are you sure you are running CFX totally incompressible for your problems? What assumptions are being made for this? Is the density included in the transport equations but only adjusted as a function of temperature or is it assumed constant except for the buoyancy force? 

April 21, 2005, 06:28 
Boussinesq approximation is us

#13 
Senior Member
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 11 
Boussinesq approximation is used.


December 5, 2006, 07:45 
I would like to simulate buoya

#14 
Member
Tomislav Sencic
Join Date: Mar 2009
Posts: 42
Rep Power: 9 
I would like to simulate buoyancy driven convection in a Heavy Fuel Oil tank. Is buoyantFoam suitable for this kind of problems (Oil is incompressible, but viscosity and density change with temperature)?
How can I define the characteristics of Heavy Fuel Oil (density, specific heat, thermal conductivity, viscosity..)? 

December 5, 2006, 17:01 
You will need to write your ow

#15 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,789
Rep Power: 22 
You will need to write your own, probably using Bousinesq assumption. buoyantFoam solvers are all for compressible gasses really and you will want a compressible liquid.
Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

December 19, 2006, 07:08 
but at low mach cases wouldn't

#16 
Guest
Posts: n/a

but at low mach cases wouldn't compressible gases in buoyantFoam have the same behavior?


December 19, 2006, 07:27 
If I use buoyantFoam to simula

#17 
Guest
Posts: n/a

If I use buoyantFoam to simulate heating of a water mass which modifications would I do and where?
thanks! 

October 26, 2007, 04:11 
Hi
i would want to use buoy

#18 
Guest
Posts: n/a

Hi
i would want to use buoyantsimplefoam but for incompressible fluids which modifications i have to do and where? best regards 

March 31, 2008, 10:09 
I am developing a Simple based

#19 
Guest
Posts: n/a

I am developing a Simple based code suitable to study flames propagating in atmosphere. To do that I need to consider the effect of gravity, so I was looking to either "buoyantFoam" or "buoyantSimpleFoam" whose UEqns have something not straightforward to me. Indeed developing the RHS of the momentum equation one gets grad(p)rho*(grad(gh)), while
it should be grad(p)grad(gh*rho), does the lack of gh*grad(rho) rely on some semplications I am missing? 

April 1, 2008, 06:06 
Dear all!
I am about to loo

#20 
Senior Member
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 9 
Dear all!
I am about to look on fires in tunnels (low MachNumber, buoyant driven flow, radiation; LES) with the help of CFD and searched the web and this forum about information concerning solving this kind of flow in OF. I have the impression that Xoodles could be the most appropriate solver for that. Is this correct? Does this solver also handles the effects of smoke on radiation phenomena? Thanx for any comment! Mabinty 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
segregated solver vrs coupled solver  sm  FLUENT  0  November 6, 2007 02:24 
How to do it if i change the seregated finitevolume solver to segregated finiteelement solver  dandes  OpenFOAM PreProcessing  0  March 22, 2006 22:06 
AGMSOLVER  MANOJ  FLUENT  5  August 1, 2005 04:49 
solver  fuf  FLUENT  0  June 19, 2003 13:54 
coupled solver / uncoupled solver  Jaan Unger  Main CFD Forum  0  September 3, 2002 08:30 