Problem with energy imbalance

Roland R · July 25, 2012, 11:19

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

keeper · July 25, 2012, 11:59

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?

Felggv · July 25, 2012, 13:09

Hello,

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

Roland R · July 25, 2012, 18:17

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

flotus1 · July 25, 2012, 18:28

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?

ghorrocks · July 25, 2012, 19:24

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.

Shljuki · July 25, 2012, 21:40

[ 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.

Roland R · July 26, 2012, 04:40

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

ghorrocks · July 26, 2012, 08:38

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

Roland R · July 27, 2012, 08:28

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

ghorrocks · July 28, 2012, 08:52

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.

bemomb · November 8, 2019, 04:47

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

July 25, 2012, 11:19	Problem with energy imbalance	#1
Roland R Senior Member Roland Rakos Join Date: Mar 2009 Posts: 131 Rep Power: 17	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

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Energy Balance problem	masud	STAR-CCM+	1	May 23, 2012 11:15
volumetric reaction and energy balance?	m.beh	FLUENT	1	October 17, 2011 18:21
energy source problem	fluboy	Fluent UDF and Scheme Programming	2	January 10, 2010 09:56
Convergence problem of the energy equation	Woo Meng Wai	FLUENT	2	May 13, 2008 04:06
SIMPLE and energy equation convergence	Fabio	Main CFD Forum	0	June 1, 2007 07:06

July 25, 2012, 11:59		#2
keeper Senior Member Join Date: Jul 2010 Posts: 152 Rep Power: 16	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?

July 25, 2012, 13:09		#3
Felggv Member Felipe Gobbi Join Date: Apr 2012 Location: Brazil Posts: 76 Rep Power: 14	Hello, Is it an closed room? Describe your problem better, maybe some details would make the difference for us to help.

July 25, 2012, 18:17		#4
Roland R Senior Member Roland Rakos Join Date: Mar 2009 Posts: 131 Rep Power: 17	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

July 25, 2012, 18:28		#5
flotus1 Super Moderator Alex Join Date: Jun 2012 Location: Germany Posts: 3,427 Rep Power: 49	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?

July 25, 2012, 19:24		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	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.

July 25, 2012, 21:40		#7
Shljuki New Member Join Date: Jun 2012 Location: Melbourne Posts: 14 Rep Power: 14	[ 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.

July 26, 2012, 04:40		#8
Roland R Senior Member Roland Rakos Join Date: Mar 2009 Posts: 131 Rep Power: 17	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

July 26, 2012, 08:38		#9
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	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

July 27, 2012, 08:28		#10
Roland R Senior Member Roland Rakos Join Date: Mar 2009 Posts: 131 Rep Power: 17	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

July 28, 2012, 08:52		#11
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	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.

November 8, 2019, 04:47		#12
bemomb Member Benni Join Date: Oct 2019 Location: Germany Posts: 33 Rep Power: 7	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