[Chander]

Hi,

This is related to my previous thread:
http://www.cfd-online.com/Forums/cfx...nds-error.html

As I explained already in that thread, I am solving a conjugate heat transfer problem of flow through a microchannel heat sink. The heat sink receives heat flux at the bottom solid surface.
The same heat sink has been analysed experimentally and the heat loss from the rest of the solid surface to environment is known. This loss is significant under some operating conditions. I impose this loss as an average negative heat flux on rest of the outer solid walls and fluid walls.
Now the error occurs when I use Standard option for Output and it occurs AFTER the simulation has converged and BEFORE the result file is created. The error notice is:
+--------------------------------------------------------------------+
| ****** Notice ****** |
| While evaluating Static Entropy, |
| Temperature on boundary IPO Inlet manifold top adiabatic wall |
| went outside of its lower limit. Its minimum value was |
| -9.5381E+05. The bounds error was handled by clipping. |
| If this situation persists, consider increasing the table range. |
+--------------------------------------------------------------------+
Following the previous thread, I contacted Ansys support and they pointed out that the negative heat loss boundary condition at outer solid walls and outer fluid walls is the cause of this error. If one uses heat transfer coefficient instead of heat flux option for the outer walls, this error disappears. I found out that the error also disappears if one uses adiabatic boundary conditions on the outer walls. However, I do not have the heat transfer coefficient values from experiments and that is why I use the heat flux values so that the total heat loss is model is same as that in experiments.
Why does using the heat flux boundary condition instead of specifying the heat transfer coefficient at outer walls cause this error?
I am posting this again thinking that the new info may help in someone pointing the actual cause. Is the negative heat flux boundary condition wrong in some way? Any inputs will be highly welcome.

I am sorry for posting this again. But just hoping for any new suggestions. Otherwise, I will have to reduce the accuracy of the model by neglecting the heat loss from heat sink to environment which is not exactly desirable for my project.

[ghorrocks]

I suspect the negative heat flux then causes the fluid somewhere to get very cold. As heat flux boundaries are unbounded (ie they keep cooling with nothing to stop them) you can get unphysically cold areas.

So I suspect your error is because the negative heat flux boundary is not appropriate. Some ideas:
1) Switch to a convective BC. Sure, you do not know the HTC, but hopefully you know the ambient temperature and the total heat flux so you can work the coefficient out from that.
2) Put a CHT solid and apply the neg heat flux to the outside of the solid. The solid will allow a bit of conduction and thermal inertia which might just fix the problem.
3) Look at a results file (you might have to do a special partial run to get a results file) and see where the error is occuring and just remove that bit of boundary. If you have specified a total heat flux the rest of the boundary will have slightly greater heat flux to account for it so the total effect will still be the same.

[Chander]

Thanks Glen for ur reply and help.
Replacing heat flux with HTC boundary condition does work though I have to do some work to find an approximate value for HTC.
However, I still wonder why specifying a heat flux instead of HTC leads to problems.
Anyway I keep keep looking for any plausible reasons for this though my problem is solved for the moment.