Hi Aziz,

You do not have to define any interface in Fluent to simulate this Conjugate Heat Transfer problem.

Considering the symmetries, you can only simulate one eighth of your geometry to reduce the CPU time. Due to the temperature differences, you should account not only for convection but also for radiation.

Dear Abdulaziz Abutunis

Please choose "coupled" as the "Thermal condition" for boundaries between the two walls, and for the boundary between the outer wall and air choose "convection" and determine a value for "h_air". Some references are allocated to determining "h_air" that you can use. We used one of those references to determine h_air for our latest published article, which can be found here.

Good Luck.

Philippe Béard : If there is influence of buoyancy, than there is - for a transient flow - no symmetry at all. The flow will show some non-symmetric vortex shedding.

Otherwise it is a Fluent-only conjugate heat transfer prediction. If the walls are properly resolved by the mesh, i.e. the thermal boundaries on walls, then the distribution of (h) in spce and time is the result of the CFD/CHT prediction.

Regards,

Dr. Th. Frank.

Philippe Béard,

Thank you for your comment. You are right if the geometry is symmetric I should consider that yet this geometry was a simplified one. Regarding the interface, I am usually running fluent to calculate the hydro/aerodynamic forces and I used interfaces for that I will consider your suggestion. but what if i am running FSI for that I think then I need interface if I am not wrong.

Thank you again

Aziz

Dear Mojtaba Bezaatpour,

Thank you for your comment. I am looking for temperature distribution, do you think during the transient simulation it is okay to use one fixed h_air. shouldn't h_air be a function of time and local temperature if I am not wrong.

The

Can you please include the reference that reports the h_air?

Thank you

Aziz

Thomas Frank,

Thank you for your elaboration. I agree with you, I am considering the refining the mesh to resolve the thermal boundary layer and find h(r,x,y,z) because I am interested in the variation in the temperature distribution within the solid bodies. do you have any suggestions either to solve the problem in a one-way FSI or two-way FSI.. or in other words, how to import the transient thermal properties into the solid model to find this variation over time in the temperature distribution.

Thank you again,

Aziz

Dear Abdulaziz Abutunis

Partially yes. You assume "h" as a constant value for the bulk air around the outer walls, but remember that it is a temperature-dependent parameter near the boundary, and if the temperature difference between the initial and final times is considerable, you should use a UDF code and define an equation for "h" based on boundary' temperature.

Dear Mojtaba Bezaatpour,

Thank you again for your valuable suggestion. The outer air temperature is the same but the surface of the outer wall has a different temperature 2D profile that varies with time as it cools down. and I am wondering if this h would also be affected by the very inner body since it has a different temperature and different thermal conductivity. I think it is better to couple the 2 models.

Best regards

Aziz

Dear Abdulaziz Abutunis

To get a suitable temperature distribution transient behavior for your problem statement. It's better to add an air zone to it and couple the three zones together during the solution. In this case you should calculate the minimum far away distance for the air zone that not effected by the heat zone i.e. free convection streams. This is a simple free convection problem to find out these distances around the materials zones.

So that 'h' will be calculated internally during the transient solution till steady state situation achieved. In addition it will give you a simulation for the built-ed free convection streams around the materials.

Regards.

Thank you Alaa for your suggestion,

Yes, I am aware that I need the far air BC with zero heat transfer. The challenge I see is how to communicate this varied h with calculating the temp profile of the internal walls. Again I will try to couple the two, the fluid and solid models.

Best regards,

Aziz

Dear Abdulaziz Abutunis

When you add this air zone, h will be calculated by fluent directly.

Regards.

Abdulaziz Abutunis : It is a bit confusing me, that you are talking about an FSI simulation. Are you interested in resulting stresses within the solid body (e.g. due to differences in the temperature distribution and thermal expansion of the solid material)?

If not, than this simulation is not a FSI simulation at all. It is a pure ANSYS Fluent CHT simulation, where the solid material properties are getting assigned to the solid domain inside of Fluent material properties selector.

Could you please clarify the final goal of the intended simulation?

Regards,

Dr. Th. Frank.

Hi Thomas Frank,

Thank you for your comment. My main concern is the temperature distribution through the inner walls and I am using fluent just to account for the transient heat convection. For now, I am not considering any stresses or thermal expansion in solid materials. As far as I know fluent will deal with solid materials as a thin wall and solve for the heat and forces on it. However, I am really interested in the temperature profile through the thickness of the walls. Your suggestions are highly appreciated.

Best regards

Aziz

Dear Abdulaziz Abutunis

Another question, the inner solid temperature is 200 C.

Did you looking for cooling it by air convection through the outer solid?, or its at constant temperature?

If its at constant temperature, you can neglect it from the model and set the inner faces of the outer solid at constant temp. of 200 C. This will reduce model mesh elements and leads to faster transient calculations.

Regards.

Abdulaziz Abutunis : Your statement about how ANSYS Fluent treats solids in terms of heat conduction is so not correct. Fluent can solve an energy equation in the interior of a solid material domain, if this domain is provided with its own mesh. Spatial resolution of any temperature distribution just depends on the applied mesh resolution. Just define for each solid its own body / domain and mesh it. Than you can select this as a volumetric zone in Fluent, assign a solid material and solve for 3d temperature distribution. Absolutely no need then to involve any different solver than just Fluent (or ANSYS CFX, if you like this more for its superior stability as a CFD solver, like I do).

Regards,

Dr. Th. Frank.

Thank you Thomas Frank for your precious clarification. You are right my understood of how fluent deals with solids is very limited to the hydro/aerodynamics. I usually do the heat transfer in Ansys solids or Abaqus if solid is defined and when convective heat transfer coefficient or heat flux are steady and defined. It has been a while since I worked with CFX but as you recommended if the convergence is not achieved by fluent, I may go to CFX.

My final question is do you have any recommendation if either conformal or nonconformal interface would be better for heat transfer between the fluid and the solid.

It is really great information, thanks again

Aziz

Abdulaziz Abutunis : Conformal or Non-Conformal mesh.

A conformal mesh is of course better, since it avoids any kind of interpolation on the domain / mesh interfaces. But sometimes it is hard or nearly impossible to create such a conformal mesh everywhere it might be needed. If your case is really as rectangular domain like shown, than it would be easy and beneficial to create such conformal meshes at interfaces.

Otherwise if that is not possible, than use non-conformal interfaces, but make the spatial mesh resolution on both sides of the interface as identical as possible (approx. same dx). And with a non-conformal interface you might want to spent a couple of more mesh cells in comparison with a nice hexahedral and conformal mesh interface. Than it should be enough to compensate for the interpolation errors, which are then non-avoidable. In my experience the usage of non-conformal interfaces has almost no impact on solver stability or computational time.

Regards,

Dr. Th. Frank.

Thank you, Dr. Thomas Frank. I will consider your valuable suggestions.

Best regards

Aziz

Dear Mr. Abdulaziz Abutunis

Heat transfer coefficient value depending to the

1- temperature difference between the object and the wall (walls)

2- air gap distance (if it is contain air) if there is no air it is the best heat insulation when there is a vacuumed.

If the gap contained air so you can calculate the Nu number value if its more then 3 ( Nu>3), so there is a convection heat transfer else if Nu