[ehrenwirth]

Hi there!

Once again, i have a problem with simulating thermal radiation. Below you can see the assembly i want to simulate:



As you can see, there are 3 Domains. They are called "Plate", "Cube" and "Air". The plate-material is steel, the cube-material is copper and air is made of air ;-). Below you can see an exploded view, where the interfaces "Plate-Cube" (between Plate and Cube) and "Cube-Air" (between Cube and Air) are drafted.



As you can see, the backside of the plate is given a temperature of 100°C. All remaining sides of the Domain "Air" are defined as an opening. In the screenshot below you can see all assumptions. All domains have the thermal option "thermal energy". The domain "air" has the monte-carlo-radiation-option activated.



When i start to solve this, the solver finishes within 40sec and no monitor-plots are shown!

In CFX-Post, following screen is shown (i added a plane and made a contour-plot of temperature on this plane):

In my opinion, the plot itselfs doesn´t look that bad, but the values of 100°C everywhere are suprising me. Maybe you can help me with this simulation and tell me what to change in CFX-Pre.

Thanks a lot!

[bharath]

Is there any interface between plate and air?

[ehrenwirth]

Hi!

No there isn´t. I already tried to define such a interface, but ANSYS tells me that the surface is already used. Is this neccesary?

Thanks for your reply!

[ckleanth]

i think i know what you did wrong and yes the interface is nessesary as the information between the domains wont be passed over to the adjacent domains otherwise

one possible problem is that the solid solid interface between the plate and cube does not exist as you missed to imprint the cube face on the plate (as a modeling aproach you dont need the plate anyway if you dont care about the temperature dissipation in the plate. you could simply set a contstant temperature on the outer air and cube domain faces.)

also if you meshed each volume as a separate part dont be suprised if you cant chose a 1:1 mesh connection method (might not be relevant to your current physics setup but you might find this problem in the future)

[ehrenwirth]

Hi again and thanks for your reply!

I think you where right with your suggestions. There was no "Plate-Air"-Interface, and the "Plate-Cube"-Interface did not include the surface where the cube stands normal to the plate. I startet a solver run and voila, the solver calculated some time ;-). After 50 iterations, i broke up to check the result. It really makes sense now. But i how can i connect the plate with the cube AND the air? Is there any option to do this?

Another question ist what will happen if i put an isolator between plate and cube. In my opinion the temperature should decrease or am i wrong with this suggestion?

Thanks a lot so far!

[ghorrocks]

Hi,

You cannot connect a single interface surface to two separate interface surfaces. You need to split the surface as suggested above and have one interface plate to cube and another one plate to air.

Also for this type of simulation you should also use imbalances as a convergence critereon. This means the overall heat balance will be converged to the level you specify.

Glenn Horrocks

[ehrenwirth]

Hi again!

I realized your suggestions and changed my modell, you can see the result below:



Like before, the temperature is 100°C at the left side of the plate. In this simulations i did not set the "opening" boundary at the outer air-surfaces. In my opinion they are not really needed, but please let me know if i´m wrong!

Now here´s a picture from the solver-run in the end. Actually there is no concergence...




At last, here is a screenshot from CFX-Post:



Again, this doesn´t make sense to me....

I would be very glad if you can help me again!

Thanks a lot!

[ckleanth]

have a read through the tutorials for conjugate heat transfer problems. and do a search in this forum. and in the ansys customer support website >technical tips > Converging CHT Simulations

once you include solid domains in your problem you need to calculate what timestep to use for solids as this is many times bigger than fluid domain timesteps. if you are lazy use a factor of 100 for automatic timestep for solids

also you overcomplicate your problem; with your current setup you could easily cut it in half and add symetry relation where you places your viewing plane

[ehrenwirth]

Hi again ckleanth!

Thanks for your reply! You are completely right, i could cut this modell twice to get only a forth of the actual problem.

I didn´t find "technical tips" in the ansys customer portal. Can you please give me a link or something?

Do you mean the timescale with timesteps?

Does the shown temperature-plot make sense in your opinion?

Thanks a lot!

[ckleanth]

lazy example with fluid and solid domains

CONVERGENCE CONTROL:
Length Scale Option = Conservative
Maximum Number of Iterations = 1000
Solid Timescale Control = Auto Timescale
Solid Timescale Factor = 500
Timescale Control = Auto Timescale
Timescale Factor = 1.0
END

plots mean nothing if your solution is not converged. as a small advice simplify your problem and don't use solid domains unless you are interested on how the heat flux flows though them. if you use solid domains it will take ages for the problem to converge.

technical tips link

[ghorrocks]

Hi,

Also: Are you expecting buoyancy effects to create a convective heat loss? If this is significant then this will change the simulation setup. If no then you don't need to model flow in the air at all and you might as well model it as a solid too.

Also also: If you are only doing simple radiative heat transfer between some simple surfaces then consider using the Discrete transfer model. It is much simpler than Monte Carlo and much faster.

Glenn Horrocks

[ehrenwirth]

Hi again!

I switched the radiation method from monte-carlo to discrete-transfer and got a much better and faster convergence:



Here you can see CFX-Post:



Would be very nice if you can comment this!

[ckleanth]

nice picture?

[ehrenwirth]

Nice comment . But i was interessted about your opinion to this plot...does this make sense? Thanks!

[ghorrocks]

Hi,

Whether it makes sense depends on what you are trying to model. Air with the sort of temperature gradients you have there would normally create a buoyancy driven flow and that would create additional convection. If this is important you will need to fundamentally change your model to account for buoyancy effects.

Glenn Horrocks