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

Which solver

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 18, 2005, 05:53
Default Hi, I want to calculate the
  #1
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
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
braennstroem is offline   Reply With Quote

Old   April 18, 2005, 06:18
Default 'buoyantFoam' is suitable, in
  #2
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
'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 steady-state buoyancy-driven flows.
henry is offline   Reply With Quote

Old   April 18, 2005, 06:55
Default Hi, because it is for compres
  #3
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Hi,
because it is for compressible flow!? And usually we use a incompressible solver.

Fabian
braennstroem is offline   Reply With Quote

Old   April 18, 2005, 07:03
Default ... but buoyancy-driven flows
  #4
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
... but buoyancy-driven flows are compressible; the density changes as a function of temperature and pressure!
henry is offline   Reply With Quote

Old   April 19, 2005, 01:14
Default ...but the Ma-number is smalle
  #5
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
...but the Ma-number 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
braennstroem is offline   Reply With Quote

Old   April 19, 2005, 03:46
Default You could make the assumption
  #6
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
You could make the assumption of incompressibility if it is appropriate for your problem but remember compressibility is not just about the Ma-number, the density could significantly vary due to pressure changes as a consequence of body-forces e.g. gravity in the atmosphere and I didn't want to limit the kind of buoyancy-diven 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 low-Ma-number pressure solver and the compressibility effects make that slightly diagonally dominant which is beneficial to convergence. The only down-side 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.
henry is offline   Reply With Quote

Old   April 20, 2005, 01:29
Default I think it is good that there
  #7
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
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
braennstroem is offline   Reply With Quote

Old   April 20, 2005, 03:15
Default I am not sure what approximati
  #8
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
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?
henry is offline   Reply With Quote

Old   April 21, 2005, 01:23
Default Hi, he mentioned, that it w
  #9
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Hi,

he mentioned, that it won't converge as fast ...
but I will try out compressible with the low Ma-number pressure solver; I actually did not tell him about that.

Changing it to incompressible, is it enought to take care about the files in :

OpenFOAM-1.1/applications/solvers/heatTransfer/buoyantFoam

Greetings!
Fabian
braennstroem is offline   Reply With Quote

Old   April 21, 2005, 03:31
Default > he mentioned, that it won't
  #10
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
> 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 low-Ma 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 : OpenFOAM-1.1/applications/solvers/heatTransfer/buoyantFoam

Yes.
henry is offline   Reply With Quote

Old   April 21, 2005, 04:10
Default Sorry, I forgot to mention, th
  #11
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
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
braennstroem is offline   Reply With Quote

Old   April 21, 2005, 05:39
Default FOAM has been compared with CF
  #12
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
FOAM has been compared with CFX for buoyancy-driven 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?
henry is offline   Reply With Quote

Old   April 21, 2005, 06:28
Default Boussinesq approximation is us
  #13
Senior Member
 
Fabian Braennstroem
Join Date: Mar 2009
Posts: 407
Rep Power: 10
braennstroem is on a distinguished road
Boussinesq approximation is used.
braennstroem is offline   Reply With Quote

Old   December 5, 2006, 07:45
Default I would like to simulate buoya
  #14
Member
 
Tomislav Sencic
Join Date: Mar 2009
Posts: 42
Rep Power: 8
tsencic is on a distinguished road
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..)?
tsencic is offline   Reply With Quote

Old   December 5, 2006, 17:01
Default You will need to write your ow
  #15
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
hjasak is offline   Reply With Quote

Old   December 19, 2006, 07:08
Default but at low mach cases wouldn't
  #16
guilherme
Guest
 
Posts: n/a
but at low mach cases wouldn't compressible gases in buoyantFoam have the same behavior?
  Reply With Quote

Old   December 19, 2006, 07:27
Default If I use buoyantFoam to simula
  #17
guilherme
Guest
 
Posts: n/a
If I use buoyantFoam to simulate heating of a water mass which modifications would I do and where?

thanks!
  Reply With Quote

Old   October 26, 2007, 04:11
Default Hi i would want to use buoy
  #18
rengu
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
  Reply With Quote

Old   March 31, 2008, 10:09
Default I am developing a Simple based
  #19
diego_n
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?
  Reply With Quote

Old   April 1, 2008, 06:06
Default Dear all! I am about to loo
  #20
Senior Member
 
Aram Amouzandeh
Join Date: Mar 2009
Location: Vienna, Vienna, Austria
Posts: 186
Rep Power: 8
mabinty is on a distinguished road
Dear all!

I am about to look on fires in tunnels (low Mach-Number, 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
mabinty 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
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 Pre-Processing 0 March 22, 2006 22:06
AGM-SOLVER 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


All times are GMT -4. The time now is 13:54.