[Dilu]

Hi,

I am trying to solve how the heat is transferred in as Solid body with multiple layers (pls see attached image). The small layer seen is the heat source and the other layers have different materials. I am new to Ansys fluent and I have researched that the heat transfer problem could be solved in fluent by using Conjugate heat transfer model or shell conduction,
My Question is can I use both the methods for this problem? if so how could I use shell conduction method? Is there any resources I could read and look into to learn how to use the above 2 methods other than Ansys user guide?
Thank you for your time.

[LuckyTran]

There appears to be only a solid? Then this can't be a conjugate heat transfer model (there's no fluid). Shell conduction model isn't even applicable either.


In this scenario, you just mesh the solid and solve the heat equation in the solid by brute force.

[Comi]

I have a question: what if a solid covered with another material is inserted into a air volume? How should I define the boundary conditions? In my case the energy residuals are very high and I'm using a density base solver with k-e model and s2s radiative model.
It has been hunting me for days, usually my residuals are very low but this time I cannot reach a satisfing solution.

Thanks everybody

[vinerm]

Conjugate Heat Transfer is meant to be used if the objective is to predict thermal field inside the solid domain. If that is not the objective and only the effect of solid needs to be included on the thermal field in the fluid zone, either shell conduction or thin wall model can be used. Of course, CHT can still be used but would be an overkill. Thin wall to be used only if thermal diffusivity is high enough. Usually, it is mentioned that thin wall is to be used for thin walls but that is incorrect notion. If the thin wall is made of insulation material with very low thermal diffusivity or anisotropic thermal conductivity then thin wall as well as shell conduction model is invalid.

Could not understand the statement below

what if a solid covered with another material is inserted into a air volume?

Do you mean something like a projectile or reentry vehicle? And do you have very high Mach number flow? If the flow is hypersonic, as in reentry vehicle do note that S2S is invalid for the scenario.

[Comi]

It is actually simper than that. I'm simulating a boiler filled with hot water, covered with an insulating material, into a closed space. my big problem is the energy residual which looks very High. however the energy conservation is verified.

[vinerm]

I am afraid that I could not really understand the setup. So, I have a few questions.

Is it the boiler that is covered by an insulating material? If yes, is it covered on all sides?

And are you trying to model the boiling phenomenon as well?

Do not use density based solver. It is meant to be used with flow having Mach number higher than 2.

[Comi]

I assumed the temperature of the water inside as a constant. The tank is covered almost completely, only the hydraulic connections are in contact with the air volume

[vinerm]

If the objective is to predict the thermal energy transfer through the insulation and thermal field within the insulation, then you have to use CHT with natural convection simulation of the surrounding air. If the objective is to predict the flow of the air around the boiler due to natural convection, then shell conduction will do the job.

[Comi]

Thank you very much for your answer I'm actually trying to predict the thermal energy transfer inside the insulator, the doublt regarding my action are given by the high residuals but I guess that I'll need to revisit the BCs and the mesh.

[vinerm]

The most important point is to look at the flow. Since the flow of air around the boiler is most likely incompressible, use Boussinesq approximation or incompressible ideal gas. If you are not modeling the natural convection of air, then it is not really a CFD scenario since there is only thermal energy transfer by conduction and/or by radiation. Then, you just need to solve energy equation. Disable Flow equation in that case.