Dear all,

I have encountered a conjugate heat transfer problem in which the heat transfer in the air and a solid epoxy has to be simulated simultaneously. Due to the large ratio (about 180) of the thermal diffusivities for the air and the solid, it is found that the heat transfer process develops very slowly during the calculation.

In one paper, the author claimed that this ratio is equivalent to the characteristic time-scale ratio of the temperature evolution in the fluid and the solid. Can anyone tell me what does this "charateristic time-scale ratio" mean ?

Thank you very much in advance.

Li

heat diffusion has velocity. characteristic time scale means the time needed for heat to go a characteristic distance, say, thermal boundary thckness, grid size.

versi,

Thank you very much for your reply ! But why this makes the heat transfer between the air and fluid very slow ? Any references ? It is suggested that, during the calculation, the ratio of the thermal diffusivities should be set initially to a much smaller value and then gradually increased to the real value.

With best wishes,

Li

" ... heat transfer in the air and a solid epoxy has to be simulated simultaneously."

This suggests that you want the time-dependent solution (for the temperature changes in the epoxy?). In that case, modifying the natural diffusivities to obtain a "solution" is not a good idea.

Do you need to do a full CFD solution for the air flow, or will some sort of boundary layer approximation along the surface of the epoxy be adequate?

In any case, the nature of the flow will depend strongly on the orientation of that surface and whether your air is blown against/along the surface or moves only by natural convection (forced or free convection).

I assume that you aren't melting or freezing the epoxy at the surface. Then, at a point on the surface, the heat flux from the air (+ or -, depending on whether you're heating or cooling the epoxy) must equal the heat flux to the epoxy. Starting with this, a bit of analysis will suggest how the near-boundary mesh spacing in the air should relate to the near-boundary mesh spacing in the epoxy. Then the stability requirements for your particular numerical schemes will set the allowable time step.

You'll learn a lot by trying various meshing combinations and studying the resulting solutions.

This solution behaviour is a well known to those performing thermal analysis of forced convection cooled electronic systems. Flotherm by Flomerics for example has a solution acceleration technique called 'block correction' that accounts for the fact that the air flow settles down to steady state much earlier than the temperature field in a solid construction that has a heat source buried within it, i.e. an IC package.

The physical time scales are very different (the thermal time constant for the solid is much larger than that for moving air!). This physical behaviour is echoed in the numerics in the rate at which the solid settles down to steady state vs. the air.

Classical multi grid methods also resolve this issue. The 'block correction' method described above is a variant on an AMG method in that it corrects only amalgamated cell groups that require correction, not a grid uniform coarsening approach. Much more efficient.

Jim,

Thanks a lot for your reply. I want to simulate a fully unsteady turbulent air flow and would also like to investigate the conjugate heat transfer behaviour using a harmonic mean at the interfaces between the air and the epoxy. After a steady solution is obtained, the unsteady option will be switched on.

From what you said, I assume that the number of grid points used in the epoxy is also important for an accurate simulation of the heat transfer inside the epoxy. Any critirion ?

Best wishes

Li

Dear Harry,

Thanks a lot for your reply and those information provided.

I am doing an unsteady flow simulation. The air flow is coupled with the heat transfer within the epoxy. As the thermal conductivity of the epoxy is much larger than that of the air and the temperature on the epoxy surface is calculated through a harmonic mean, the surface temperature is dominated by the temperature inside the epoxy. I find that, although the unsteadiness in the air flow can be clearly identified,the surface temperature will not change much and appear to be quite steady. I wonder anyone out there has similar experience.

Kindest regards

Li

The thermal time constant of the epoxy is very high compared to that of moving air. As such its temperature will change little as a function of the rate of change of the air temperature at the surface. Calculate the time constant of the epoxy (theraml resistance x thermal capacitance) and compare it to say the fluid residency time as it passes over the epoxy (I think that's a good comparison).

This physical behaviour is echoed in the numerics of steady state solution I described earlier.

This reminds me of an ERCOFTAC test case based on the experimental work by E. Meinders.

Harry, thanks a lot for your knowledge regarding this. As a matter of fact, I am working on this ECROFTAC test case. I will check the block correction method you mentioned when necessary. Best wishes, Li