Problem with energy imbalance
 

Hello,

I have a simple fluid domain which contains a small solid domain. A volume heat source is defined in the solid domain. The simulation type is steady state. The inlet velocity is very small (0.001m/s).

Based on the convergence history, the energy imbalance will be ok after some iterations in the solid domain but it doesn’t converge in the fluid field. Value of the energy imbalance is ~ 80-100% after 200-300 iterations too. Is it because of the heat source? What can I do in the interests of faster convergence?

Regards
Roland

the velocity is 1mm/s? this is really low speed. maybe this sould cause problems. is the flow driven also by buoyancy?what about mesh for such low Re?

Hello,

Is it an closed room? Describe your problem better, maybe some details would make the difference for us to help.

Hello Everybody

Yes, this velocity is very low. The reason is the next:
The solid domain is a disc which is rotating. I would like to investigate the effect of the rotation on the air domain. I would like to realize the case when the air is in rest. If the air velocity is higher than I can not investigate only the rotating effect.

The room is not closed. Naturally it is closed in the reality and this phenomenon is transient. But this simulation is steady state therefore it has to contain inlet and outlet or else the thermal balance can not occur because of the heat source. (At least I think this.)

Regards
Roland

You could specify a wall with a fixed temperature for the boundary conditions.
This will solve the problem of energy imbalance in the closed domain.

How do you model the rotation of the solid body? Do you have a moving mesh or some kind of rotor-stator-interface?

This is a common problem for CHT simulations. The problem is the thermal time scale is massively slow compared to the fluid time scale, so once the fluid flow is converged the thermal field still has a long way to go.

The way to resolve this in a steady state simulation is to use a solid time scale factor. Usually some pretty big numbers (like 1000) work fine. This accelerates convergence in the solid region.

[ The simulation type is steady state. The inlet velocity is very small (0.001m/s). ]
You velocity is too small, this might be a buoyant dominant flow. It might be more appropriate to run it in transient mode.

[Based on the convergence history, the energy imbalance will be ok after some iterations in the solid domain but it doesn’t converge in the fluid field. Value of the energy imbalance is ~ 80-100% after 200-300 iterations too. Is it because of the heat source? What can I do in the interests of faster convergence?]

You can do few things:
1. You can increase time scale for energy
2. You should try to achieve tighter convergence for energy - you might need to run your simulation much longer
3. You can run energy only at the end of the simulation (once your velocities have converged) to reach energy imbalance you need
4. Check that the mesh is good enough to resolve the heat transfer around the solids.

Hello,

Thanks for your quick help.
I have increased the Solid Timescale Factor to 1000. After that the Energy Timescale Factor has been increased to 10 and 100. Decreasing of Energy Imbalance was faster but it fluctuated between -20 and 20% in case of every solution. The RMS H-Energy is not adequate; it is ~3e-2.

Regards
Roland

If you are not getting the heat residuals down and the imbalances are fluctuating then you have too much solid acceleration. You should reduce it. You probably have other convergence problems as well, which are discussed here http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Hello,

I generated two new models with a higher quality mesh. In the first model the settings of time scale factor were default. Everything was OK but the T-energy imbalance converged in the rotating disc solid very slowly (about 6000 iterations). In the second model the solid physical timescale was 100s. The T-energy imbalance converged in the rotating disc very quickly (about 800 iterations) but all residuals started to fluctuate in the fluid domain. Though its value was ok; 1e-4, 1e-5.

I don’t understand the reason of fluctuation of residuals in the fluid. I changed only the solid physical time scale.

Regards
Roland

The FAQ I linked to explains the fluctuations - either some issue is stopping tighter convergence, or the flow is transient and the steady state run cannot converge becuase it is not appropriate. If you work through the issues on the FAQ it will guide you to a solution.

Hi Roland


Just found your thread and noticed that I have a very similar issue. In my case, there is a plate rotating in an air domain and a piston presses axially on that plate which leads to heat generation. During the simulation, every imbalance is fine except the T Energy in the plate. How did you solve the problem?


Thx in advance


Benni