CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Very simple natural convection problem (http://www.cfd-online.com/Forums/fluent/93404-very-simple-natural-convection-problem.html)

Naseem October 14, 2011 03:10

Very simple natural convection problem
 
1 Attachment(s)
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

hariehkr October 14, 2011 21:25

Quote:

Originally Posted by Naseem (Post 327915)
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

LuckyTran October 14, 2011 22:26

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.

hariehkr October 15, 2011 06:31

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.

LuckyTran October 15, 2011 14:48

Quote:

Originally Posted by hariehkr (Post 328014)
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 October 15, 2011 15:02

Quote:

Originally Posted by LuckyTran (Post 328000)
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 October 15, 2011 15:17

Quote:

Originally Posted by hariehkr (Post 328014)
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?

LuckyTran October 15, 2011 15:22

Quote:

Originally Posted by Naseem (Post 328048)
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).

hariehkr October 15, 2011 18:58

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.

shubhankar.kulkarni55 October 15, 2011 22:56

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!

Naseem October 17, 2011 14:11

Quote:

Originally Posted by shubhankar.kulkarni55 (Post 328069)
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.

Naseem October 17, 2011 14:13

Quote:

Originally Posted by hariehkr (Post 328058)
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 October 17, 2011 14:25

Quote:

Originally Posted by LuckyTran (Post 328049)
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?

sofie1 October 18, 2011 02:14

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

Laci October 18, 2011 07:38

Settings
 
Try the further settings:
- pressure-velocity coupling: SIMPLEC
- pressure discretization: PRESTO!
- Momentum and Energy discretization: second-order upwind

These helped to me.

Naseem October 19, 2011 02:55

Quote:

Originally Posted by sofie1 (Post 328333)
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 October 19, 2011 02:57

Quote:

Originally Posted by Laci (Post 328392)
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?

rlahlou December 15, 2015 11:12

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 pressure-inlet at the bottom inlet, pressure-outlet at the top and walls at the sides of the doamin ( only one being heated and the other one far-away enough to have no impact on the boundary layer).

Thanks a lot for your (or anyone else's) feedback!


All times are GMT -4. The time now is 18:41.