Conjugate Heat Transfer- Radiation
 

I am modelling a part being heated via radiation. This is performed in a vacuum. My model has the following characteristics:

-solid domain: this is the part. Monte Carlo, surface to surface specified
-fluid domain: air at 25oC, vacuum, Monte Carlo, surface to surface specified (created using enclosure tool in geometry)
-fluid domain, boundary- Temperature; there is a heating element at 700oC which is the radiation source (created by imprinting faces tool onto the enclosure in geometry).
-interfaces; these are the default interfaces (don't have a problem with these).
-I am not solving for turbulance or fluids as it is assumed there is no convection due to radiation

In CFX- Solver:

-RMS H-Energy diverged (was just above 1.0e-3 then went up to 1.0e-2)
-RMS T-Energy converged (<1.0e-3)
-following summary results:

-------------------------------------------------------------------+
| I-Radiation |
+--------------------------------------------------------------------+
Boundary : Fluid Domain Default -2.3380E+00
Boundary : Flux 1 -5.8078E+01
Boundary : Flux 2 7.5831E+01
Boundary : Solid Domain Default -1.5414E+01
-----------
Global Imbalance : 2.0218E-04
Global Imbalance, in %: 0.0003 %
+--------------------------------------------------------------------+
| H-Energy-Fluid Domain |
+--------------------------------------------------------------------+
Boundary : Fluid Domain Default 1.9116E+00
Boundary : Flux 1 -2.0170E+00
Boundary : Flux 2 2.6976E+00
Domain Interface : Default Fluid Solid Interface -2.7985E+00
-----------
Domain Imbalance : -2.0624E-01
Domain Imbalance, in %: -1.3132 %
+--------------------------------------------------------------------+
| T-Energy-Solid Domain |
+--------------------------------------------------------------------+
Boundary : Solid Domain Default 1.5705E+01
Domain Interface : Default Fluid Solid Interface 2.7985E+00
-----------
Domain Imbalance : 1.8504E+01
Domain Imbalance, in %: 117.8191 %


*****

What can I do to reduce this imbalance? Have I incorrectly defined something in the Solid Domain?

Hi,

The fact that the solution has not converged suggests that there is something wrong.
But for the imbalances, as I had such a problem before, when you have heat flux in as a boundary condition, I think CFX doesn't calculate the imbalances right. In CFXpost use function calculator, and calculate area integral of heat flux on those two boundaries, and compare them to see exactly how much imbalance there is in the solution.
Again 10e-2 is not a good convergence, if you can consider it a convergence at all, so you need to work more on your mesh, or mathematical modeling of the physical problem, or ...

I can not agree more.

For the radiation with Monte carlo method, it is difficult to reach a good convergence or take a much longer time. As triple_r said, you need to make sure the model is physically right, and then optimize the meshing. If the problem exists, you can simply your model to test your cfx-pre setup.

Please let us know when you get a satisfied solution.
:D:D:D

I will try your suggestion in CFX-Post.

I know its a terrible convergence, but this was a quick first pass to see if the solution worked.

I know I have to work on my mesh (a lot).

But such a large imbalance and divergence suggested to me it was more that I was incorrectly defining some parameter.

I have stipulation Temperature=500K, in a boundary condition, in the fluid domain (rather than flux).

Another question I had was in the Solid Domain I can only select Monte Carlo method, and was hoping to use P1 and Monte and compare them. Whereas in the fluid I can specify a number of radiation methods. Is there a reason for this?

Simple, so simple!

I do not need a radiation model for the Solid domain as this domain as the radiation is either converted to heat or bounces off when it hits the solid domain. It is not travelling through it like in the fluid domain.

So I changed the fluid to discrete ordinate and it converged! There are a few other spots that were a bit dodgy- but mesh is dodgy so I will fix that up.

Now, I have to make this a transient problem in CFX;

The temperature starts at 20oC then goes to 70oC in 30sec, then over the next 5mins to 200oC. This is all in ramp (ie it takes 30sec to raise the temp of the heaters 40oC), and there is no time where the temp is constant.

I have changed the simulation type in the Simulation Time to transient and specified timesteps.

Does anyone know of an appropriate tutorial I would be able to look at? I can only find ones relating to velocity, and I do not know how to define the expression. (Or put the expression into the temp boundary condition)

Thanks guys!

Hi,

I'm really happy that you found the problem with your mathematical model.
I don't know if I understood the problem exactly, but everywhere in CFX-pre when you need to provide a numerical value (not everywhere actually but most of the places) there is a button with an alpha on it, which allows you to provide an expression for that box.
First you need to define an expression for the temperature vs time for your boundary condition, and then provide that expression as the temperature on that boundary.
I can't think of the exact tutorial that has the temperature versus time variation for a boundary condition, but you can find all the information you need in the CEL related help topics. btw t is the variable that CFX uses for time, and be careful with the units.
I hope these can help you.

For those playing at home- I thought my problem was fixed. The transient simulation was running. The conduction through the solid looked ok... Then I looked at my temperature values.

Scenario:
The whole furnace starts at 295.25K at time zero. The temperature of the heaters increases. The temperature of the solid increases due to conduction with the outside temp being greater than the temp at the bottom (tick).

However, the air above the solid DECREASES in temperature. That is, it goes down to 235K while the solid slowly heats up with the heaters. And the air at the top is also heating up.

ALL domains are set to 295.15K to start

I am presuming it is a numerical problem.

What I have tried:

-not solving for fluids, P= 4 torr (this is valid as my model is in a vaccum)
-Discrete transfer (fluid domain); surface to surface and participating media
-Monte carlo (fluid domain); surface to surface and participating media.

Any ideas?

Found the tutorial
Put a user function
and then a user expression: function(Accumulated Time Step)


I am getting RMS values of less than 10^-5; however my T-Energy and I-radiation imbalances are 100%. Any clues?