[Oleg V.]

Dear friends,
I want to solve a heating problem in Fluent. I have simple body of rotation, I want to make test calculations of heating this body in supersonic flow (Mach number M=3.0) using ANSYS Fluent. I made fine structural grid with y+ < 1 on the surface. Now my question is: what thermal boundary conditions should I use to calculate this problem? Heat flux = 0 doesn't work of course. What should I do? The materials are: air (ideal gas + sutherland's law viscosity) and solid material is steel.

[LuckyTran]

Use the coupled boundary condition.

When you import the grid, there should be a wall shadow-wall pair. One of these will be the BC for the fluid, the other will be the BC for the solid. Both should be coupled.

Also please be aware that if you are using the pressure-based solver, viscous heating is disabled by default. If you want to include viscous heating, then you have to enable it using:
define/models/energy? blah blah blah

[Oleg V.]

LuckyTran,
I used only 1 domain: Fluid. Do I have to make 2 domains: Fluid + Solid? If so then what kind of BC should I specify for inner edge of Solid?
For M=3 I use density-based solver, it's better for compressible flows (blah-blah-blah )

[LuckyTran]

For compressible solver, now you have the problem in that you cannot turn off viscous heating. So also be aware of that.

I'm not sure how you want to model the heating of this body. You could just do a fluid only simulation and get the heat transfer coefficient and adiabatic wall temperature. To me that gives you all the information you need. But it's up to you. If you want to solve for heat conduction throughout the solid body (i.e. a fluid + solid), then you need separate cell zones for each.

There should never be any doubt from the user what the boundary condition is because it's part of the problem definition. But some people like to use realistic boundary conditions and some people like to do funny things. I can't tell you what to do. It's up to you how you model your own problem.

[Oleg V.]

First of all I should notice that viscosity is a function of temperature, any supersonic calculation should consider it. For aerodynamic characteristics BC as adiabatic wall is enough, but not for heating! In my case I have to use "realistic BC" as you said, that's the problem.
Anyway right now I am making a new mesh for 2 domains: fluid and solid for shell. I'll see what will change.

[LuckyTran]

Sometimes you want to know what part of the adiabatic wall temperature is caused by the isentropic slowing down of the fluid (which has no viscosity contribution). If you are not able to turn off the viscous heating, then your adiabatic wall temperature always includes the isentropic slowing down part plus the viscous heating part.

Again, there are many non-realistic things you can do that can reveal useful information. In reality it's very tough to turn these settings on/off, but numerically it's much simpler and you can learn a lot of physics doing non-realistic things. It should not be overlooked.

Once you tell me the adiabatic wall temperature and heat transfer coefficient, what remains is a simple heat conduction problem in the solid. What you will miss from an adiabatic wall boundary condition is the conjugate part, the change in temperature field because heat is allowed to conduct along your body. But even without modelling the solid, you solve say 90% of the problem already. This is a typical approach. You rarely do 3D CFD of the entire universe, at some point you always say I cut-off the domain here and make it finite.

[vuongcongdat]

Originally Posted by LuckyTran

Use the coupled boundary condition.

When you import the grid, there should be a wall shadow-wall pair. One of these will be the BC for the fluid, the other will be the BC for the solid. Both should be coupled.

Also please be aware that if you are using the pressure-based solver, viscous heating is disabled by default. If you want to include viscous heating, then you have to enable it using:
define/models/energy? blah blah blah

Hi Lucky Tran, I am doing the exact simulation, I would like to know what is the best model to use: k-epsilon or STT or laminar or invisid and which near wall treament to use ? My simulation is the flow Mach =3 pass through a bullet shaped object. The object is hollow inside and there is air inside. I would like to know if the flow time is 50s then how the heat affects the air temperature inside the object.