Simulation heat transfer
 

Hi guys,
I'm trying to simulation the air through the reactangular duct which has 4 cylinder inside. My boundary condition is velocity inlet 9.45(Re=15000), pressure outlet =0, lower wall is heat wall, heat flux is changed from 500 to 5000. But when i changed heat flux, my result Nusselt number on heat wall and cylinder absolutely didn't change. Just temperature change. I don't know why. Please someone help me
The second problem is when heat flux from 1000 to 5000, fluent notify " temperature limited to 1.000000e+00/5.00000e+003 in X cells on zone X" at the both first and second iteration . I searched in forum and they said because of grid. I use ICEM and qualify determinant 2x2x2 is around 0.9-1. y+<1 for using kw SST. Anyone met this problem before can help me understand ?
Thanks all.

If you change the heat flux and only see that only the temperature changes, this is absolutely correct! Heat transfer coefficient and Nusselt number is a property of the flow, it should not change with heat flux except due to non-linearities. By non-linearities, we mean that the heat flux changes the local fluid properties enough to change the flow. Otherwise, for relatively small changes in heat flux, the flow is unaffected and the Nusselt number should not change.

A better mesh always helps but if your solution converged for a heat flux of 1000 and only crashed when you changed the heat flux to 5000, then it can also just be an initialization problem. Have you tried using the converged solution with a heat flux of 1000 and then changing the heat flux instead of re-initializing?

u're right, just temperature change. Because i multiply heat flux 500 by 10 but Nu didn't change, I concern about it.
About the error temperature limited, we are the same way. Because my document i using to simulation don't have the quality of heat flux, they just said that heat wall is assigned with constant heat flux so i'm finding the value consistent with their result. It's document from turbo expo 2019.
u said try using the converged solution with heat flux 1000 and then changing the heat flux instead of re'initializing. I dont understand. why can i calculate if we don't re-initialize when heat flux change. I think it's wrong. Can u explain. Thanks

That's not necessarily something to worry about. Especially if the warning goes away after the first few iterations, and doesn't cause the simulation to diverge.
What's most likely happening in your simulation: For the first few iterations, the fluid velocity near some parts of the heated wall is very low. Yet the boundary dumps a lot of heat into it. That can cause very high temperature in some of the cells near the heated wall. There are ways to fix this, like initializing the velocity field differently, lowering under-relaxation for energy equation, disabling energy altogether for the first few iterations etc. But if the simulation does not blow up, and continues to converge normally afterwards, you don't really have to do anything about it.

Just to be clear. Temperature can change. Heat transfer coefficient and Nusselt number will not change. That is Newton's law of cooling. Nusselt number should depend only on Reynolds number and Prandtl number (and other dimensionless groupings), it should not depend on the wall temperature setting or the heat flux setting unless those are large enough to change the Reynolds number and so on.

You always need an initialization. I am just proposing that you use the converged solution with heat flux of 1000 as your new initialization. You are likely using a constant temperature field and zero velocity everywhere as your initial guess. The converged solution for a heat flux of 1000 will have a much better temperature field and velocity field, it might help with your convergence issues if that's what is happening.

If the warning goes away after some iterations that's fine too, that's normal.

I am trying a case with a 2d rectangular channel having a supersonic flow (pressure inlet and pressure outlet boundary condition). The lower wall is set with a heat flux value of 5000W/m^2. Mine is a very simple case - compressible flow with heat addition. But the heat provided from the bottom wall does not have a noticeable effect on the flow. Can someone suggest an alternative method or explain my mistake.