Applying convection as internal boundary condition?

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

November 3, 2016, 11:10
Applying convection as internal boundary condition?
#1
New Member

Evan Johnson
Join Date: Jun 2016
Posts: 6
Rep Power: 10
Hello CFD Community,

I am dealing with a conjugate heat transfer problem, and I am having trouble when specifying a boundary condition between the solid and fluid zones.

My problem is essentially a fluid flowing along a fin. In the attached image, the metal fin is gray, the fluid zone is brown, and fluid is flowing downward along the fin. Heat is applied to the base of the fin via radiation, and there are convective and emissive losses to the outside (no problem here). At the interface between the fin and fluid, I would like to specify a convection boundary condition, by specifying a convection coefficient I have found experimentally, so the heat flux from the solid to the fluid should be calculated as: q = h*(T_wall-T_inf).

Since this is a Two-Sided wall, Fluent only gives the options of "coupled", "temperature", and "heat flux" for the boundary conditions of the wall (and its shadow), so convection is not an option. If the BC is "coupled" then heat flows, but not at the rate I would like with my known h value. If "coupled" is NOT chosen, then (according to the user guide, and my own trials) the two sides of the wall are essentially insulated and don't communicate heat.

I have read other threads with similar questions, and the advice is essentially "don't specify an internal boundary because it's not physically realistic to impose such a condition" but in this case I think it IS physically realistic since the external losses are temperature dependent (please correct me if I'm wrong!) In fact, I would like to impose this convection boundary condition specifically in order to solve for the temperatures of the fin and the external losses!

So, how do I apply an boundary condition at the interface such that the heat is specified by my heat transfer coefficient? Can Fluent even do this?

Thank you very much - I truly appreciate the help! And if I find a solution, I'll happily post the details for future modelers.
Attached Images
 fin_picture.JPG (18.8 KB, 56 views)

 November 7, 2016, 14:36 #2 Senior Member   Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,735 Rep Power: 66 Indeed if coupled is not selected then you have isolated domains and it is no longer a conjugate heat transfer problem. Indeed the problem is non-sensical if you want to specify the htc and I am super glad Fluent does not give this option. The htc is a property of the fluid flow, if you specify the htc then you have already implicitly specified the fluid flow. You should simulate the fluid by itself with a wall and the htc given or the fin by itself with the desired htc. If you know the htc, then you do not have a conjugate heat transfer problem.

 January 6, 2017, 02:08 #3 New Member   Evan Johnson Join Date: Jun 2016 Posts: 6 Rep Power: 10 Thanks for your response. I do understand now why I was trying to do something incorrectly! I'm trying to model something where I do NOT know the fluid properties (conductivity, viscosity), though I have experimentally measured the heat transfer to the fluid. Fluent must know these properties and then it calculates the heat transfer, so applying a the properties and simultaneously requiring a heat transfer condition does indeed over-define the problem. Ignoring for a moment the way the CFD problem is solved, I would like to impose a heat transfer coefficient and leave the properties undefined, thus not over defining the problem. (I realize this sounds odd, but I don't care about the exact heat distribution in the flow, as it will all be mixed later.) In reality, this isn't the way CFD software works, but I could write some type of energy balance code that could work this way. To your last point, even if I know the heat transfer coefficient, this still ends up being a conjugate heat transfer problem because it is internal flow (so T_bulk changes down the length and a simple q" = h*(T-T_inf) is not correct), and the base of the fin has a complex radiation + emission + convection boundary, which is highly temperature dependent. I can't model the fin without modeling the fluid's increase in bulk temperature, and I can't model the fluid by itself without the geometry and heat transfer properties of the fin taken into account - so modeling them simultaneously is sill necessary in my opinion. As a work-around, instead of applying the htc directly, I have chosen the thermal conductivity value that produces the htc that I need, and I am proceeding to model in this way. Thanks for your help and ideas! Best -

 January 28, 2019, 03:57 #4 Senior Member   vidyadhar Join Date: Jul 2016 Posts: 138 Rep Power: 10 Hello Lucky Tran, I am working on interfacial flows, in which evaporation should take place at the interface of liquid and vapor. If I assume that the interface between liquid and vapor is stationary or fixed, then Can I apply a convection boundary condition on the interface in Fluent? If so, can you let me know how to apply? Thanks in advance!

January 28, 2019, 09:49
#5
Senior Member

Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,735
Rep Power: 66
Quote:
 Originally Posted by evanJ To your last point, even if I know the heat transfer coefficient, this still ends up being a conjugate heat transfer problem because it is internal flow (so T_bulk changes down the length and a simple q" = h*(T-T_inf) is not correct),

You can never say you know the heat transfer coefficient without knowing the reference temperature. The heat flux q" is invariant to the definition of heat transfer coefficient and selection of the reference temperature.

I don't disagree that this is a conjugate heat transfer problem, but then that means you should not be imposing any heat flux internally. My original point was that if you truly knew the heat transfer coefficient and are trying to impose it, then it is a decoupled problem.a

Quote:
 Originally Posted by vidyadhar Hello Lucky Tran, I am working on interfacial flows, in which evaporation should take place at the interface of liquid and vapor. If I assume that the interface between liquid and vapor is stationary or fixed, then Can I apply a convection boundary condition on the interface in Fluent? If so, can you let me know how to apply? Thanks in advance!

Yes & No. Same as the problem in the original post. You can only apply boundary conditions at boundaries. It is an internal interface regardless of whether it moves or is stationary if you treat it as an internal internal interface. Either decouple your problem or let the physics do physical things.