[LThomes]

Hello,
I'm simulating a flow inside a tube, and the boundary condition at the wall is "Heat Transfer Coefficient", i.e, the thermal conductivity of the material of the tube (I will call it k from now on) over the wall thickness.
The problem is that k is a function of the wall temperature (k = f(T)). Is there anyway I could get the temperature at each cell face of the wall to write an expression at the "Setup", e.g.,

k = const x Temperature@wall

P.S.: I will also need the rate of heat transfer or heat flux at each cell face of the wall.

Could anybody help me?
Thanks in avance.

[ghorrocks]

Heat transfer coefficient is not usually defined from the conductivity and thickness of the wall material. The HTC is usually defined as the heat transfer due to fluid motion next to a wall. The wall conductivity and thickness are usually accounted for differently. Are you sure you are talking about the right thing?

[LThomes]

I'll try to make myself more clear. As you can see from the attached figure, I need the Heat Flux (q") to calculate the temperature at the outside surface of the tube (T2) and the Temperature T1 to calculate my heat transfer coefficient.
The tube walls are not part of the computational domain.
Capturar.PNG

[ghorrocks]

Is this steady state or transient?

[LThomes]

Originally Posted by ghorrocks

Is this steady state or transient?

It's a steady state regime

[ghorrocks]

In steady state you can combine the convective outer boundary and the conduction in the tube to a combined boundary on the fluid domain. One approach could be to add the thermal resistance of the convective section and the conduction in the pipe, and apply that as a heat flux boundary condition to the fluid. You can do this using CEL expressions and you will be able to variable k (or anything else for that matter).

[LThomes]

Originally Posted by ghorrocks

In steady state you can combine the convective outer boundary and the conduction in the tube to a combined boundary on the fluid domain. One approach could be to add the thermal resistance of the convective section and the conduction in the pipe, and apply that as a heat flux boundary condition to the fluid. You can do this using CEL expressions and you will be able to variable k (or anything else for that matter).

I know that, but the problem is that I don't have the temperature at the inside surface of the wall (T1) , it's calculated by the numerical solution. I would like to know if I could get this temperature to calculate k and the HTC at each iteration. So that the HTC boundary condition would change according to each iteration.

[urosgrivc]

And what is your boundary condition at your most outer wall?
I dont understand, do you just want (T) dependant material properties?
if so you can do it via user function create a table of T and conductivity than set it in material properties as a form of expresion conductivity(T)

[ghorrocks]

You don't need to calculate T1, the solver does it. If you need T1 to evaluate material properties then just use a CEL expression/interpolation function which evaluates material properties as a function of T - it will use T from the previous coefficient loop, so will converge on the correct value of T as your simulation converges.

[LThomes]

Originally Posted by ghorrocks

You don't need to calculate T1, the solver does it. If you need T1 to evaluate material properties then just use a CEL expression/interpolation function which evaluates material properties as a function of T - it will use T from the previous coefficient loop, so will converge on the correct value of T as your simulation converges.

That's exactly what I want. But how do I do that? Could you please post some pictures or write step by step?

[ghorrocks]

I don't normally do this but I was in the mood for a bit of light entertainment so here goes:

Let the temperature at the inside of the wall be T1, outside T2 and ambient air temp T3. The wall is thickness L, thermal conductivity k and the heat transfer coefficient from T2 to T3 is h.

In the wall, q"=k dT/dX which we will approximate as = k (T1-T2)/L

In the convection q"=h dT = h(T2-T1).

Equate the T2 terms and write in terms of q" and you get

q" = k (T1 - T3)/(L + k/h)

Now you have a function for heat flux at the inside wall as a function of T1 and known variables. You can use this as the heat flux for the wall boundary condition and it will model a combined conducting wall and convection. You can make any of the constants functions of temperature, time, position or anything.

I recommend you check my maths, but that's the general idea.

[LThomes]

ghorrocks, thank you so much for your attention, but I think I didn't make myself clear yet.
The point is that I don't know how to tell CFX that I want the value of T1. If I create an expression named "T1", I'll just have to type

T

? Is T the value of the temperature in each wall cell? Or am I only able to get the average temperature at the wall? Just like

areaAve(T)@wall

[ghorrocks]

Yes, for the variable T1 just use the "T" variable in CFX. This will get the local wall temperature.

[LThomes]

Thanks. And is there anyway I could get the q" on each cell face? I just managed to get the area average, using

areaAve(Wall Heat Flux)@wall

[ghorrocks]

The variable Wall Heat Flux is the local q".