
[Sponsors] 
Conjugate Heat Transfer: slow solid temperature convergence 

LinkBack  Thread Tools  Search this Thread  Display Modes 
February 2, 2016, 07:18 
Conjugate Heat Transfer: slow solid temperature convergence

#1 
New Member
Join Date: Sep 2015
Posts: 4
Rep Power: 10 
Hi!
I am currently running CHT simulations using chtMultiRegionSimpleFoam. My case is approximately 10 million cells, devidied to 8 million in a fluid region and the remaining 2 million cells is devided in over 60 different solid regions. The simulation runs smooth and fine, but my problem is that when convergence is achived in the fluid region, the temperatures in the solid region is not even close to converged. My question is if there is any option/setting availabe to speed up the simulation in the solid parts? As example I know that in CFX one can utulize a "solid time scale factor" which has a significant impact on the convergence time. Thank you! 

February 2, 2016, 13:31 

#2 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 21 
Hi Kocklauring!
This is a matter of great interest and in the following links you will find the answer to it: slowheattransfersolidregionschtmultiregionsimplefoam slowconvergencechtmultiregionsimplefoam What are your specifications in fvSolution for the solid regions? Hope it helps. Best regards, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

February 2, 2016, 14:42 

#3  
New Member
Join Date: Sep 2015
Posts: 4
Rep Power: 10 
Thank you for your answer!
Quote:
Thus, my fvSolution for the solid regions look something like below. So if I understand the threads right, simply setting the hrelaxation factor to 1 should severly decrease the number of iterations needed to convergence? I shall try this and come back with the results. solvers { h { solver PCG; preconditioner DIC; tolerance 1e06; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 0; } relaxationFactors { fields { } equations { h 0.7; } } 

February 2, 2016, 14:56 

#4 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 21 
First of all, what version of the software are you using? As per what I know chtMultiRegionSimpleFoam solves the energy equation for enthalpy not for temperature, I'm not aware if they changed it in the newest versions but I'm familiar with OF 2.3.x and in this version energy is solved for entalpy.
Besides that, I would recomend you to lower the relTol to 0.01 or even lower so that the solver will take more iterations in the first time steps. Maybe I would even lower the tolerance to 1e07 or 1e08. According to the links I gave you above, you should use some nNonOrthogonalCorrectors, maybe 2 or 3 would do the trick, I don't know, you should try it in order to find the proper amount of correctors. Finally, the relaxationFactor for T is exaggeratedly reduced, I recomend you to try with a value of 0.9 at least, being even advisable to use 0.95 or even 1. Best regards, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

February 2, 2016, 15:04 

#5  
New Member
Join Date: Sep 2015
Posts: 4
Rep Power: 10 
Quote:
Quote:


February 2, 2016, 16:16 

#6 
Senior Member
Join Date: Sep 2013
Posts: 353
Rep Power: 21 
As mentioned slow convergence is due to the relaxation factor of your energy equation. Set it to 1 if possible. From my experience the relaxation factor should only be used to stop crashes. If those happen remove it later on in the simulation. Other ways to achieve faster convergence is increasing nonOrthogonalCorrectors. However the relaxationfactor does the trick more efficiently. The standard relaxation factors for pressure and velocity however should stay in place.
Always check the residuals and make sure the solver is still solving. If the number of iterations becomes zero nothing will change anymore in that region. Because you have that many use minIter 1 for h in your fvSolution file to make sure the solver iterates even if the tolerance is reached. Often the tolerance of 1e6 is not enough to reach convergence. You could also simply lower it but this might increase your simulation time more. Convergence for heat transfer calculations should always be checked via temperature and heat flux values. Use the heatFlux utility and compare the fluxes between regions. They should be nearly identical. In addition if you want to speed up transient simulations and your flow pattern does not change use the frozenFlow option. This drastically reduces the computation time for chtMultiRegionFoam. I think this switch was implemented in V2.4.0. And can be activated in fvSolution. 

February 3, 2016, 04:32 

#7  
New Member
Join Date: Sep 2015
Posts: 4
Rep Power: 10 
Thank you zfaraday and Bloerb for your help.
Quote:
Additionally, is there an way to briefly explain what the relTol and nNonOrthogonalCorrectors options acctually do? Why does changing them increase the convergence speed? Also, to efficient monitor Temperatures I've been trying to use probes, but I can not get them to work. Do you know any "guide" or similar where it is explained how I can implement probes? 

February 3, 2016, 14:03 

#8  
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 21 
Hi Kockaluring,
Quote:
Code:
find $FOAM_APP iname "wallHeatFlux" Quote:
fvSolution Quote:
Code:
find $FOAM_TUTORIALS type f name controlDict  xargs grep l "probes"  xargs gedit& Hope it helps. Best regards, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

Tags 
conjugate heat transfer, convergence issues, openfoam 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Quenching simulation : how to set up a conjugate heat transfer between solid&liquid  Rockda  FLUENT  24  August 30, 2016 06:33 
Problem in setting Boundary Condition  Madhatter92  CFX  12  January 12, 2016 04:39 
Slow heat transfer in solid regions (chtMultiRegionSimpleFoam)  SvenH  OpenFOAM Running, Solving & CFD  2  July 23, 2014 18:05 
Enforce bounds error with heat loss boundary condition at solid walls  Chander  CFX  2  May 1, 2012 20:11 
Conjugate Heat Transfer between fluid and solid  Li Yang  Main CFD Forum  8  March 27, 2004 11:05 