
[Sponsors] 
October 14, 2011, 03:10 
Very simple natural convection problem

#1 
New Member
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 13 
Hi guys,
I am trying to model natural convection in airbreathing 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 

October 14, 2011, 21:25 

#2  
New Member
hari
Join Date: Dec 2010
Posts: 3
Rep Power: 14 
Quote:


October 14, 2011, 22:26 

#3 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,490
Rep Power: 64 
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. 

October 15, 2011, 06:31 

#4 
New Member
hari
Join Date: Dec 2010
Posts: 3
Rep Power: 14 
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 610 W/m2K) and also out side air temperature.


October 15, 2011, 14:48 

#5  
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,490
Rep Power: 64 
Quote:
The specified temperature boundary condition is okay. 

October 15, 2011, 15:02 

#6  
New Member
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 13 
Quote:
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. 

October 15, 2011, 15:17 

#7  
New Member
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 13 
Quote:


October 15, 2011, 15:22 

#8 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,490
Rep Power: 64 
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).


October 15, 2011, 18:58 

#9 
New Member
hari
Join Date: Dec 2010
Posts: 3
Rep Power: 14 
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.


October 15, 2011, 22:56 

#10 
New Member
Shubhankar
Join Date: Jul 2011
Posts: 7
Rep Power: 14 
I have also had the reversed flow problem in the natural convection analysis. Please try using incompressibleideal 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!


October 17, 2011, 14:11 

#11  
New Member
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 13 
Quote:
Last edited by Naseem; October 17, 2011 at 14:27. 

October 17, 2011, 14:13 

#12 
New Member
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 13 
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.


October 17, 2011, 14:25 

#13  
New Member
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 13 
Quote:


October 18, 2011, 02:14 

#14 
Member
sofia
Join Date: Apr 2010
Location: world
Posts: 30
Rep Power: 15 
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 

October 18, 2011, 07:38 
Settings

#15 
Member
anonym
Join Date: Mar 2009
Posts: 65
Rep Power: 16 
Try the further settings:
 pressurevelocity coupling: SIMPLEC  pressure discretization: PRESTO!  Momentum and Energy discretization: secondorder upwind These helped to me. 

October 19, 2011, 02:55 

#16 
New Member
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 13 
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


October 19, 2011, 02:57 

#17 
New Member
Naseem
Join Date: Oct 2011
Posts: 11
Rep Power: 13 
I used these setting but not that much improvement I have got. Was your case similar to the current case?


December 15, 2015, 10:12 

#18 
New Member
Radia
Join Date: Feb 2015
Posts: 2
Rep Power: 0 
Hi Naseem,
did you finally solve your issue? What do you mean by reversed flow that you obtained? Is it part of the flow on the top that recirculates and comes down (which could be a physically acceptable solution if the width of your domain is to small such a way that it simulates a channel), or is it the whole flow that is coming downwards instead of upwards as expected? I tried to simualte the same problem as you to understand BCs behavior in natural convection, and I'm getting the whole flow downwards although the gravity direction is the right one (along the negative vertical direction). I used pressureinlet at the bottom inlet, pressureoutlet at the top and walls at the sides of the doamin ( only one being heated and the other one faraway enough to have no impact on the boundary layer). Thanks a lot for your (or anyone else's) feedback! 

December 2, 2020, 18:16 

#19 
New Member
DB
Join Date: Jan 2019
Posts: 28
Rep Power: 6 
The domain is too small. It should extend out enough to be at the freestream, near zero velocity, on the sides. On top it should be at least the height of the surface, better to be twice the height. On bottom it can be the height of the surface.
It is also necessary to apply pressure potential function as BC rather than fixed pressure at the top. Reference pressure at the bottom. 

December 17, 2020, 16:00 

#20 
New Member
Obii300
Join Date: Dec 2020
Posts: 2
Rep Power: 0 
HI can anyone help me out I am facing problem in doing simulation in ansys fluent for thermally driven flow. I have 3d pipe tilted at 45* and I have chose water as a working fluid. I want to know how much water rises and its temperature and velocity contour If localized heating of pipe wall is done. I want to know proper boundary conditions. What I want to consider is a natural flow keeping gravity and buoyancy factors. Also. I want to give zero velocity at inlet and want to find out if fluid will flow or not and if it does its velocity contour.
Kindly help me in this regard. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Flow is not converging in natural convection problem of boussinesq model for air  rahulsharma  FLUENT  4  December 2, 2020 21:07 
Natural Convection Simulation  buoyantSimpleRadiation  Convergence Problem  msarkar  OpenFOAM  32  June 16, 2010 06:27 
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 12:08 