
[Sponsors] 
Question about heat transfer simulation convergence 

LinkBack  Thread Tools  Search this Thread  Display Modes 
May 8, 2013, 16:04 
Question about heat transfer simulation convergence

#1 
Senior Member
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14 
Hi,
Heat transfer convergence usually takes much more time than the velocity convergence. For fluid dynamics simulation, when the velocity residual and mass flow residual is very small, then we can basically say that the simulation has already converged. But for heat transfer simulation, this convergence criteria may not work. I'm wondering what could be the convergence criteria for the heat transfer simulation?
__________________
Best regards, Meimei 

May 9, 2013, 11:52 

#2 
Member
Join Date: Jul 2011
Posts: 59
Rep Power: 13 
Transient or Steady State? How are the equations being solved? What exactly do you mean by convergence?
Are you using a commercial code or something you wrote youself? 

May 9, 2013, 12:38 

#3 
Senior Member
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14 
It's steady state conjugate heat transfer simulation. NS equations and total energy equations are solved by FVM. Convergence means the heat transfer rate doesn't change a lot anymore even thought the residual is still reduced. CFX is used.
__________________
Best regards, Meimei 

May 9, 2013, 15:14 

#4 
Member
Join Date: Jul 2011
Posts: 59
Rep Power: 13 
If the physical parameter you are interested in, ( a heat flux), is converged to a level that is good enough for you then stop there. There residual does not directly reflect how far your solution is from the correct solution, it tells you how accurately you are solving the equations. Also because the flow depends only weakly on the temperature it make sense that it will converge quickly, the temperature field depends strongly on the velocity field so that a small update to the velocity field can cause a large change to the convective terms in your heat equation. But I would say that if you flux is not changing by much then your answer is probably good enough and running the simulation for longer will not give you much more accuracy.


May 9, 2013, 18:11 

#5 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,372
Rep Power: 139 
CHT simulations commonly have this problem where the residuals are well converged but the imbalances are not and converge quite slowly. The problem is caused by the different time scales in the solid and fluid regions  the solid region is much slower than the fluid region, so a sensible time step for the fluid region only advances the solid region very slowly.
The answer is to use a solid time scale factor. This accelerates the time step in the solid region. As the equation solved in the solid region is just the heat equation and it is linear and wellbehaved you can accelerate it by a large amount  I typically use factors like 100 or 1000. This usually makes the solid region converge just as fast as the fluid region and speeds up CHT simulations many times. And this is also why it is vital that CHT simulations have convergence criteria on both residuals and imbalances. If you just use residuals or look at the convergence of parameters of interst you can get answers which are wrong by miles. 

May 10, 2013, 04:14 

#6  
Senior Member
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14 
Quote:
1) What do you mean by 'factors like 100 or 1000'? 2) Is there a way to setup to change the time step during the simulation running automatically? Then I can use large time step firstly then change to small step. I really need a automatic way to do this time step shifting. Because I have more than 300 this kind of simulations to run. I can't change the time step manually every time. 3) Could I setup a simulation stopping criteria like 'the outlet temperature doesn't change a lot anymore' in CFX? So that the simulation can be stopped by this criteria automatically and in this way the next simulation can be started earlier. This can save some computation time. 4) How to decide the length of the time step I need to use at the beginning to solve the solid temperature distribution?
__________________
Best regards, Meimei 

May 10, 2013, 04:48 

#7  
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 361
Rep Power: 13 
Quote:
I agree! Just compare solid time scales to fluid time scales and you quickly appreciate why the imbalances don't reduce as much as you want to! (And it's usually the energy equation  no suprises there!) However in transient simulations surely you can't set a timescale for the solid region, and a different time scale for the fluid region? Using your method described above (coincidentally is the same method I use) you're restricted to steady state calculations using "false" physical timesteps. 

May 10, 2013, 23:47 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,372
Rep Power: 139 
Yes, the solid time scale factor is only applicable to steady state runs. In transient runs you have to model it with the physical time step the same in both regions.
Shoushou: I mean set a solid time scale factor in the range of 1001000. You do not need to change the time step during a run. You can start it with this high factor. For CHT simulations I recommend using the residuals AND imbalances as convergence tolerances. Do a sensitivity study to check your settings are OK and then use that setting on all your runs. Setting time step size: Just try it out and see if it works. It is goes slow then make it bigger, If it diverges then make it smaller. 

May 14, 2013, 06:52 

#9  
Senior Member
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14 
Quote:
I didn't find the answers of it on the user manual. Thanks.
__________________
Best regards, Meimei 

May 14, 2013, 08:07 

#10 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,372
Rep Power: 139 
No, I mean using the global imbalances as an additional convergence critereon. This is described in the documentation. It does not mean RMS TEnergy or HEnergy, it is a global imbalance.


May 14, 2013, 10:15 

#11 
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 19 
In your case, Glenn is talking about the balances of all the heat. For example when you stop a run, CFX will report out in tablular format TENERGY*** for each of your solid domains. It will also report out HENERGY*** for each of your fluid domains.
It also tells you what the balance (or imbalance) is (for a SS run Heat in should = Heat out). All of your boundarys and sources are listed in this table. If you desire, during a run, you could monitor all of your heat (make sure you include the fluid inlets and outlets and losses), see what is going where, and determine from that whether your heat solution is converged. 

May 14, 2013, 11:23 

#12  
Senior Member
lnk
Join Date: Feb 2011
Location: Switzerland
Posts: 118
Rep Power: 14 
Quote:


May 14, 2013, 11:32 

#13 
Senior Member
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14 
What documentation is the global imbalances defined? I searched for it in the Ansys help but found only very limited information about it. What is the definition of the 'global imbalances'?
__________________
Best regards, Meimei 

May 14, 2013, 11:43 

#14 
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 19 
See attached Picture. The arrows point to the imbalance. The items above are all the heat sources for your each of your domains. All of those numbers are in watts.
I assume you put in heat as either a surface flux, or volume generation. You know the watts of your imposed sources. You can check the balances for all locations using this information. Adding up all the numbers should be about 0 (give or take a resonable variance). 

May 14, 2013, 12:13 

#15  
Senior Member
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14 
Quote:
And how is HEnergy and TEnergy defined?
__________________
Best regards, Meimei 

May 14, 2013, 13:27 

#16 
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 19 
You first question answer is correct.
By HEnergy and TEnergy, I assume you mean the Solver Manager convergence RMS (or MAX) plot that you see when the job is running? That is just the residual of the Energy Equation. If you mean HEnergy and TEnergy precisely then that is the energy equation: Energy In  Energy Out + Energy Stored = Total Energy. In simple terms Energy In would be: Volume Intergal of all your volumetric heat generation+surface integral of All your heat fluxes+mdot_fluid_in*enthalpy You can do the other terms in similar manner. If this is not what you mean, I do not understand the question. 

May 14, 2013, 14:04 

#17  
Senior Member
Meimei Wang
Join Date: Jul 2012
Posts: 494
Rep Power: 14 
Quote:
__________________
Best regards, Meimei 

May 14, 2013, 18:34 

#18  
Senior Member
lnk
Join Date: Feb 2011
Location: Switzerland
Posts: 118
Rep Power: 14 
Quote:
Which of them is the residual of energy equation? HEnergy or TEnergy? What is the difference between them? 

May 15, 2013, 09:20 

#19 
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 511
Rep Power: 19 
One pertains to a fluid domain, the other a solid domain.
If you run just fluids you will only see HEnergy. 

May 22, 2013, 01:59 

#20  
Member
Ben B. Huang
Join Date: Oct 2012
Posts: 54
Rep Power: 12 
Quote:
I have convergence problems too in my singlephase simulation with thermally stratified tank which has an inlet, three outlets, free slip surface and other noslip walls. Water flow into the domain having a varying density with temperatue (temperature changing with depth). Considering temperature transport, Henergy RMS reduces very slowly, even increases somewhere. The Imbalance is strange too. what's the problem? Could you give some suggestions for this? Thank you so much. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Transient heat transfer simulation with variable heat source  rdr  CFX  3  July 31, 2015 04:33 
Question about fluidsolid conduction heat transfer contact resistance  Anna Tian  Main CFD Forum  1  May 7, 2013 10:39 
Heat Transfer mechanisms  tafaugl  CFX  1  November 7, 2012 18:46 
increasing mesh quality is leading to poor convergence  tippo  CFX  2  May 5, 2009 10:55 
Heat transfer convergence problem  kam  FLUENT  0  February 26, 2007 12:32 