Hi,

I am currently trying to run a case on CFX with a solid copper plate with hot air below and cool air above. I have enabled buoyancy and have all the domain interfaces set up. However, when the model runs the results show that very little heat is transferred to the solid (Rise of about 0.3 of a degree) from the fluid. Even after a transient time of 500 secs. The lower fluid is at 300 degrees Celsius, while the solid is at 25 degrees.

I have even tried impinging the flow directly onto the plate, but still the heat transfer is minimal, which is unlikely.

Has anyone got any ideas why this might be the case?

Thanks

Charles.

Hi,

Some things to check: Near wall mesh resolution, convergence on both residuals and imbalances, correct model specification with heat transfer model.

Glenn Horrocks

Try import the CAD model to DesignModeler-->do the whole assembly a "from new part" (from tools menu) for creating the appropriate contact region between fluid-solid....re-mesh...after try the analyses

I think in this case the FSI will work the heat transfer between the boundary of fluid and solid

Best...

Hi,

You should be able to do the analysis Charles describes entirely in CFX, so no need for FSI. Also as he is getting some heat flow but an accurate amount of heat flow I suspect the problem is in the simulation physics/numerics and not the geometry.

The most likely cause of the problem is there is a large difference between fluid timescales and solid heat transfer time scales so even though the residuals indicate convergence the heat equation has not converged enough to conserve heat accurately. This shows itself by heat not being conserved. You can check this by looking at the imbalances in the solver manager. If they are larger than 1% you are not achieving good heat conservation.

Generally the fix is to add a convergence check on imbalances as well as residuals for CHT simulations (conjugate heat transfer - heat transfer in both fluid and solid regions), and possibly making the imbalance check finer than the default of 1% (this is problem dependant, need to do a sensitivity analysis).

Glenn Horrocks

Thanks,

I have already done what you suggested with DesignModeler and have formed a new part. This was the fix of one of the problems I was having earlier, in that the domain interfaces were not being created as it did not recognise the shared boundary.

I will try to refine the mesh futher and see what happens...

Thanks

Charles.

Hi Glenn,

Thank you for the advice. I will experiment with the solid and fluid timescales and try to add a convergence check on imbalances.

I am fairly new to CFX (Just started using it at university) and am not fully aware of its capabilities yet. I am assuming that I don't have to apply my own expressions to the fluid/solid boundary to allow heat transfer? (An academic I know said he had to do this when he used Fluent).

Kind Regards

Charles

Hi,

When you set up the fluid/solid boundary as an interface it includes heat transfer. No need for special modifications in most circumstances.

Glenn Horrocks