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

selection of solver : buoayantBossinsqPisoFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 12, 2010, 04:53
Default selection of solver : buoayantBossinsqPisoFoam
  #1
Member
 
Dinesh Nath
Join Date: Dec 2009
Location: Kanpur, India
Posts: 39
Rep Power: 7
dinesh2n@gmail.com is on a distinguished road
Hi all,

Could anybody help me in selecting a correct solver. I have a vertical cylindrical annulus region filled with Argon. Its height is 1m and annulus region is 2cm wide. The bottom is at 803K and top at 303K with pressure 100 millibar above than atmospheric pressure. Using Argon properties in this temperature environment the Rayleigh Number is around Ra=10^7. My question is:
Is that correct to use buoayantBossinsqPisoFoam for solving this problem to see the natural convection. Or I shall have to write my own solver?. Also can I change g (gravity) to change the Rayleigh number to view the various temperature/velcoity profiles for different Rayleigh numbers.

thank you

regards
dinesh

Last edited by dinesh2n@gmail.com; June 12, 2010 at 06:15.
dinesh2n@gmail.com is offline   Reply With Quote

Old   June 16, 2010, 07:02
Default
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
The temperature difference is probably too big for the Bousinesq approximation. Try using the compressible solver buoyantPisoFoam instead.

Yes you can change gravity in the file - constant/g
eugene is offline   Reply With Quote

Old   June 16, 2010, 13:31
Default
  #3
Member
 
Dinesh Nath
Join Date: Dec 2009
Location: Kanpur, India
Posts: 39
Rep Power: 7
dinesh2n@gmail.com is on a distinguished road
Hello eugene
Thank you for your reply and helpful suggestion. I will try with buoyantPisoFoam. A little confusionis is that in the theory of this problem people have used incompressibility and Bousinesq approximation. So, if I use compressible solver, I may not follow the thoery. Could you tell me please how much max. temperature difference can be handled by buoayantBossinsqPisoFoam?
Second, I was trying to ask if I change gravity does it makes sense ? Since in nuclear reactor all the properties of Argon are fixed at those temperatures. So I can not alter Ra No.=g*beta*DetaT*L^3/nu^2)*Pr more. I can change L, but that have to be changed 10 orders of magnitude which is again impractical. So, I thought to change g just for simulation, since Bousinesq approximation involves g.

thanks you again for your valuable time.

dinesh
dinesh2n@gmail.com is offline   Reply With Quote

Old   June 17, 2010, 06:06
Default
  #4
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Check this paper on the Boussinesq approximation: (http://articles.adsabs.harvard.edu/c...MB&classic=YES)

It gives you everything you need to know about Boussinesq. In general the Boussinesq approx is valid if d(rho)/rho0 << 1 ~< 0.1. For an ideal gas with pressure ~constant, this can be expressed as d(rho)/rho0 = (T - T0)/T0.

Where T0 is something like the mean temperature. As you can see this does not leave a lot of room. For T0 = 300, the min max range of T is only 270 - 330 K. Not a lot at all.

The Boussinesq solver should still work, even with very high temperature differences, it just wont be very accurate.

You can certainly change g, as long as your dimensionless numbers all stay the same the results should be equivalent.
eugene is offline   Reply With Quote

Old   June 17, 2010, 06:46
Default
  #5
Member
 
Dinesh Nath
Join Date: Dec 2009
Location: Kanpur, India
Posts: 39
Rep Power: 7
dinesh2n@gmail.com is on a distinguished road
Thank you very much Eugene....
dinesh2n@gmail.com is offline   Reply With Quote

Reply

Tags
buoayantbossinsqpisofoam, cylindrical annulus

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
mach number and selection of the fluent solver turbinesv FLUENT 4 April 24, 2011 00:14
Working directory via command line Luiz CFX 4 March 6, 2011 21:02
why the solver reject it? Anyone with experience? bearcat CFX 6 April 28, 2008 14:08
Turbulent flow solver selection Jenner FLUENT 1 December 5, 2006 04:38
compressible two phase flow in CFX4.4 youngan CFX 0 July 1, 2003 23:32


All times are GMT -4. The time now is 02:14.