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

Very simple natural convection problem

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

Like Tree1Likes
  • 1 Post By LuckyTran

Reply
 
LinkBack Thread Tools Display Modes
Old   October 14, 2011, 03:10
Default Very simple natural convection problem
  #1
New Member
 
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 5
Naseem is on a distinguished road
Hi guys,

I am trying to model natural convection in air-breathing PEM fuel cells. In order to better understand the physics of the problem, I have tried to simulate a very simple case: a vertical heated plate. I assigned a relatively high temperature for the plate (a wall), e.g. 320 K. As for the convection region adjacent to the plate, I tried several boundary conditions: pressure outlet, pressure inlet, outflow, but I have always had reversed flow. By the way, I have activated the gravity effect in order induce the natural convection. The temperature of the ambient air was assumed to be 298 K. I attached a schematic for the problem to illustrate the domain. Any input is highly appreciated.

Thanks,
Nassem
Attached Files
File Type: doc NaturalConvection.doc (49.0 KB, 105 views)
Naseem is offline   Reply With Quote

Old   October 14, 2011, 21:25
Default
  #2
New Member
 
hari
Join Date: Dec 2010
Posts: 3
Rep Power: 6
hariehkr is on a distinguished road
Quote:
Originally Posted by Naseem View Post
Hi guys,

I am trying to model natural convection in air-breathing PEM fuel cells. In order to better understand the physics of the problem, I have tried to simulate a very simple case: a vertical heated plate. I assigned a relatively high temperature for the plate (a wall), e.g. 320 K. As for the convection region adjacent to the plate, I tried several boundary conditions: pressure outlet, pressure inlet, outflow, but I have always had reversed flow. By the way, I have activated the gravity effect in order induce the natural convection. The temperature of the ambient air was assumed to be 298 K. I attached a schematic for the problem to illustrate the domain. Any input is highly appreciated.

Thanks,
Nassem
what about heat source
hariehkr is offline   Reply With Quote

Old   October 14, 2011, 22:26
Default
  #3
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 692
Rep Power: 13
LuckyTran will become famous soon enough
You can use pressure inlet / outlets with 0 pressure for your boundaries.

Reversed flow should not be a problem (if it is supposed to occur). It looks like you may have flow outward of the boundary near the top and inward from the bottom which would result in reversed flow at (at least one) on one of those regions.
LuckyTran is offline   Reply With Quote

Old   October 15, 2011, 06:31
Default
  #4
New Member
 
hari
Join Date: Dec 2010
Posts: 3
Rep Power: 6
hariehkr is on a distinguished road
Take top, bottom, sides boundary condition as symmetry (no net heat flow out) OR a constant temperature with zero heat flux. for natural convection you need to specify bounadry condtion as convection and you have to give heat transfer coeeficient value manually (it generally for natural covection 6-10 W/m2-K) and also out side air temperature.
hariehkr is offline   Reply With Quote

Old   October 15, 2011, 14:48
Default
  #5
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 692
Rep Power: 13
LuckyTran will become famous soon enough
Quote:
Originally Posted by hariehkr View Post
Take top, bottom, sides boundary condition as symmetry (no net heat flow out) OR a constant temperature with zero heat flux. for natural convection you need to specify bounadry condtion as convection and you have to give heat transfer coeeficient value manually (it generally for natural covection 6-10 W/m2-K) and also out side air temperature.
If top bottom and side boundary conditions are far enough away from the plate, then it is okay to use symmetry condition. Otherwise, this would place restrictions on the problem and likely produce incorrect results. Regardless, you cannot specify thermal boundary conditions on a symmetry boundary condition.

The specified temperature boundary condition is okay.
Naseem likes this.
LuckyTran is offline   Reply With Quote

Old   October 15, 2011, 15:02
Default
  #6
New Member
 
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 5
Naseem is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
You can use pressure inlet / outlets with 0 pressure for your boundaries.

Reversed flow should not be a problem (if it is supposed to occur). It looks like you may have flow outward of the boundary near the top and inward from the bottom which would result in reversed flow at (at least one) on one of those regions.
Thanks LuckyTran for the reply and the advice. I used pressure outlets for the boundaries and it sounds that the solution is realistic. What I made this different this time is that I have used Boussinseq approximation for the density.

As you mentioned, there were reversed flows at two of the boundaries. I will check what they are as soon as I go to office.

I am trying now to investigate the effect of the size of the natural convection region on the solution. It seem that the velocity profile get larger with the size of the region - it does not sound right, does it? I will give more description to the problem once I go to office. Thanks once again for your input.
Naseem is offline   Reply With Quote

Old   October 15, 2011, 15:17
Default
  #7
New Member
 
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 5
Naseem is on a distinguished road
Quote:
Originally Posted by hariehkr View Post
Take top, bottom, sides boundary condition as symmetry (no net heat flow out) OR a constant temperature with zero heat flux. for natural convection you need to specify bounadry condtion as convection and you have to give heat transfer coeeficient value manually (it generally for natural covection 6-10 W/m2-K) and also out side air temperature.
I did use the symmetry boundary condition but I did not get a converged solution. As for the constant temperature boundary condition, should I use a wall BC with a specified temperature?
Naseem is offline   Reply With Quote

Old   October 15, 2011, 15:22
Default
  #8
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 692
Rep Power: 13
LuckyTran will become famous soon enough
Quote:
Originally Posted by Naseem View Post
I did use the symmetry boundary condition but I did not get a converged solution. As for the constant temperature boundary condition, should I use a wall BC with a specified temperature?
Use the thermal boundary condition corresponding to the physics of your problem. The two you should look at are the specified temperature and specified heat flux. The simplest ones to implement are constant temperature or constant heat flux (although you can specify profiles).
LuckyTran is offline   Reply With Quote

Old   October 15, 2011, 18:58
Default
  #9
New Member
 
hari
Join Date: Dec 2010
Posts: 3
Rep Power: 6
hariehkr is on a distinguished road
Can u tell briefly are u taking single cell OR stack?. ur considering 2D or 3D problem? if possible send me mesh file to me.
hariehkr is offline   Reply With Quote

Old   October 15, 2011, 22:56
Post
  #10
New Member
 
Shubhankar
Join Date: Jul 2011
Posts: 7
Rep Power: 6
shubhankar.kulkarni55 is on a distinguished road
I have also had the reversed flow problem in the natural convection analysis. Please try using incompressible-ideal gas instead Boussinesq model and use 'Body force weighted' solution method for pressure. Works fine. I am a bit doubtful about specifying the heat flux or source terms as they may not give you accurate temperatures. The temperature values come up to be very high. So I would prefer to give constant temperatures if they are known. Hope this helps. Thanks!
shubhankar.kulkarni55 is offline   Reply With Quote

Old   October 17, 2011, 14:11
Default
  #11
New Member
 
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 5
Naseem is on a distinguished road
Quote:
Originally Posted by shubhankar.kulkarni55 View Post
I have also had the reversed flow problem in the natural convection analysis. Please try using incompressible-ideal gas instead Boussinesq model and use 'Body force weighted' solution method for pressure. Works fine. I am a bit doubtful about specifying the heat flux or source terms as they may not give you accurate temperatures. The temperature values come up to be very high. So I would prefer to give constant temperatures if they are known. Hope this helps. Thanks!
I used what you suggested. From velocity and temperture contorus, it seems that the model does not work as good as that with Boussinseq model. I have a word file that contains some contours that have been generated using Fluent. I wonder if it is legal to post it here.

Last edited by Naseem; October 17, 2011 at 14:27.
Naseem is offline   Reply With Quote

Old   October 17, 2011, 14:13
Default
  #12
New Member
 
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 5
Naseem is on a distinguished road
Quote:
Originally Posted by hariehkr View Post
Can u tell briefly are u taking single cell OR stack?. ur considering 2D or 3D problem? if possible send me mesh file to me.
I have not built the model yet. It is meant to be for a 2D PEM fuel cell. I have started off with this simple case just to have a feeling of how natural convection is treated in Fluent.
Naseem is offline   Reply With Quote

Old   October 17, 2011, 14:25
Default
  #13
New Member
 
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 5
Naseem is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
Use the thermal boundary condition corresponding to the physics of your problem. The two you should look at are the specified temperature and specified heat flux. The simplest ones to implement are constant temperature or constant heat flux (although you can specify profiles).
It looks that for such a small ambient region, the pressure inlet/outlet BCs are the best options. However, I have increased the size of the ambient region and it appears that the case works better with wall BC (with either constant temperature or zero flux). I think one of the problems with Wall BC (as opposed to pressure BCs) is that it controls the size of the recirculations that occur as a result of natural convection. In other words, the size of recirculation proportionally increases with the size of the ambient and this may not be realistic. You may would like to comment on this?
Naseem is offline   Reply With Quote

Old   October 18, 2011, 02:14
Default
  #14
New Member
 
sofia
Join Date: Apr 2010
Location: world
Posts: 19
Rep Power: 7
sofie1 is on a distinguished road
try to boussinesq approximation with giving a small velocity at inlet BC and at outlet BC pressure outlet and use body force weighted and power law,the reversed flow is not aproblem

i hope that can help you
sofie1 is offline   Reply With Quote

Old   October 18, 2011, 07:38
Default Settings
  #15
Member
 
anonym
Join Date: Mar 2009
Posts: 65
Rep Power: 8
Laci is on a distinguished road
Try the further settings:
- pressure-velocity coupling: SIMPLEC
- pressure discretization: PRESTO!
- Momentum and Energy discretization: second-order upwind

These helped to me.
Laci is offline   Reply With Quote

Old   October 19, 2011, 02:55
Default
  #16
New Member
 
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 5
Naseem is on a distinguished road
Quote:
Originally Posted by sofie1 View Post
try to boussinesq approximation with giving a small velocity at inlet BC and at outlet BC pressure outlet and use body force weighted and power law,the reversed flow is not aproblem

i hope that can help you
Thanks for the advice. Would you please briefly explain the case you were working on? Did you use a mix of pressure inlet and outlet BCs? Have you validated it against experimental data? Thanks
Naseem is offline   Reply With Quote

Old   October 19, 2011, 02:57
Default
  #17
New Member
 
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 5
Naseem is on a distinguished road
Quote:
Originally Posted by Laci View Post
Try the further settings:
- pressure-velocity coupling: SIMPLEC
- pressure discretization: PRESTO!
- Momentum and Energy discretization: second-order upwind

These helped to me.
I used these setting but not that much improvement I have got. Was your case similar to the current case?
Naseem 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
Natural Convection Simulation - buoyantSimpleRadiation - Convergence Problem msarkar OpenFOAM 32 June 16, 2010 06:27
Flow is not converging in natural convection problem of boussinesq model for air rahulsharma FLUENT 0 January 25, 2010 02:16
Natural convection - Inlet boundary condition max91 CFX 1 July 29, 2008 20:28
Natural convection problem in CFX 11 Willy CFX 2 May 23, 2008 23:12
Transient natural convection problem Ravi Main CFD Forum 2 January 30, 2000 13:08


All times are GMT -4. The time now is 10:05.