
[Sponsors] 
October 1, 2005, 13:25 
Divergence detected in AMG Solver:TEMPERATURE

#1 
Guest
Posts: n/a

Hello all,
I am working on 3D, ROTATING/ SWIRL flow inside the pipe problem. Flow is compressible and turbulent. I started with Segregated and Implicit solver with underrelaxation factor for energy equation equal to 1. I am using RSM as a turbulence model. But after some iteration I have got the "Divergence detected in AMG Solver:TEMPERATURE" and then the iteration stop. Please help. Thanks in advance, best wishes, Sachin Nimbalkar 

October 2, 2005, 08:12 
Re: Divergence detected in AMG Solver:TEMPERATURE

#2 
Guest
Posts: n/a

Chech the boundary conditions . If it is ok so , you may reduce the URF. Wael


October 3, 2005, 08:49 
Re: Divergence detected in AMG Solver:TEMPERATURE

#3 
Guest
Posts: n/a

You should set your limits (Solve>Controls>Limits) pretty carefully when using high URF values and the segregated solver. This will help keep your model from getting too far out of the bounds of reality. You still need some margin so that the model can adjust as it approaches a converged solution, but the default values are rediculously broad.
Hope this helps, and good luck, Jason 

October 3, 2005, 12:28 
Re: Divergence detected in AMG Solver:TEMPERATURE

#4 
Guest
Posts: n/a

Thank you Wael and Jason.
I am still working on the problem. As soon as I figure out the solution I will let you guys know. Appreciate! 

October 4, 2005, 10:17 
Re: Divergence detected in AMG Solver:TEMPERATURE

#5 
Guest
Posts: n/a

Don't solve Energy Equation for the first 50 iterations, then turn it back on.
If it still fails, you have other issues. 

October 5, 2005, 22:49 
Re: Divergence detected in AMG Solver:TEMPERATURE

#6 
Guest
Posts: n/a

i solved this problem by "decreasing the relax factor to a low number"


October 16, 2005, 02:10 
Re: Divergence detected in AMG Solver:TEMPERATURE

#7 
Guest
Posts: n/a

Hi,
Try to change the multigrid cycle for pressure from "V" to "W". 

October 8, 2010, 04:08 

#8 
New Member
sunqiang
Join Date: Nov 2009
Posts: 23
Rep Power: 10 
I had the same problem, i used mass flow rate as intlet , after fews iterations,the error occured ,but if i changed the inlet BC to velocity inlet and maintained other BCs ,the problem was gone.


October 8, 2010, 04:14 

#9 
New Member
sunqiang
Join Date: Nov 2009
Posts: 23
Rep Power: 10 
I had the same problem, i used mass flow rate as intlet , after fews iterations,the error occured ,but if i changed the inlet BC to velocity inlet and maintained other BCs ,the problem was gone.


February 8, 2011, 08:58 
divergence detected in AMG solver: temperature

#10 
New Member
Amit Chauhan
Join Date: May 2010
Location: Chennai, India
Posts: 13
Rep Power: 9 
I too encountered the same problem.. and I tried to solve it by above methods. but sorry to say in my case it didnt work...
but I changed my time step size and it worked... what does it physically signifies??????? 

September 7, 2012, 07:11 
Re: Divergence detected in AMG Solver:TEMPERATURE

#11 
New Member
Orkun Temel
Join Date: Feb 2012
Posts: 13
Rep Power: 8 
Hi chauhanji,
As far as i know, there are many reasons causing the referred problem. I don't know your case, but as i understand from your solution, your problem seemed to be stability problem. Assuming that you're using explicit approach, you just need to provide that your time step size is under the limitation due to CFL condition. Probably, when you changed your delta_t, you provided this. And this is how your finite equations became stable and consistent. Physically, it is also wise to keep delta_t under the characteristic convective and diffusive time scale, so that you can obtain a numerical solution including the whole transport process. 

January 4, 2013, 06:21 

#12 
New Member
peyman
Join Date: Mar 2012
Posts: 8
Rep Power: 7 
I had a same problem and I changed the relaxation factor of energy from 1 to 0.9 and it didn't error anymore


January 5, 2013, 04:19 

#13 
Senior Member
SSL
Join Date: Oct 2012
Posts: 226
Rep Power: 8 
Are you using Coupled solver? else correct your mesh. You should use a finer mesh.


March 4, 2013, 12:02 

#14 
New Member
Fan He
Join Date: Jan 2013
Location: Virginia
Posts: 11
Rep Power: 7 
Hi all,
1 I also select this probelm by reducing UnderRelaxation Factors from Turbulent Kinetic Energy from 0.8 to 0.1. 2 I guess this problem may be caused by using a high inlet velocity (i.e. large Reynolds #), because when I use some much lower inlet velocities to run the model, I can get good results though the URF is 0.8. 3 This problem is solved, but my results in this high inlet velocity case still are not convergent (energy equation is convergent, while continuety equation and momentm equations are not convergent). I will work on this problem for some more time. Thank you for your suggestion here. 

March 4, 2013, 19:53 

#15 
New Member
sp
Join Date: Jul 2011
Posts: 23
Rep Power: 8 
In addition to what others have said, at your pressure/mass flow inlet boundary condition, you need to set the initial/supersonic pressure to a value close to your expected upstream pressure. If you initialize with default values, it will use 0 as the pressure at the inlet.
If you are using a pressure inlet and a pressure outlet, another thing that helps is to start with a lower pressure differential between your inlet and outlet, and then gradually decrease your exit pressure to the point that you need. Good luck. 

September 12, 2016, 13:38 

#16 
New Member
abhijeet jaiswal
Join Date: Sep 2016
Posts: 7
Rep Power: 3 
Thanks riaan i used your method and the problem is solved.


October 29, 2016, 16:08 

#17  
New Member
yes
Join Date: Oct 2016
Posts: 17
Rep Power: 3 
Quote:
please tell me because i have the same problem on the fuel cell PEMFC 

October 30, 2016, 00:02 

#18 
New Member
abhijeet jaiswal
Join Date: Sep 2016
Posts: 7
Rep Power: 3 
No need to initialize the solution...directly run the calculation...


October 30, 2016, 08:19 

#19 
New Member
yes
Join Date: Oct 2016
Posts: 17
Rep Power: 3 

November 17, 2016, 14:15 

#20 
New Member
yes
Join Date: Oct 2016
Posts: 17
Rep Power: 3 
thank you sir l tried and it worked .but I have another problem.when I draw the polarisation curve I have falling in curent density at the voltage 0.6v next it augment in 0.7 after that it work normally
it mean why the value of current density deacrease at 0.6 v after that increase thank you sir 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Error: Divergence detected in AMG solver  siri  FLUENT  7  February 12, 2018 19:35 
Divergence detected in AMG solver: ads0  Patrino  FLUENT  5  November 25, 2015 10:04 
Quarter Burner mesh with periosic condition  SamCanuck  FLUENT  2  August 31, 2011 11:34 
user subroutine error  CFDUSER  CFX  2  December 9, 2006 07:31 
user defined function  cfduser  CFX  0  April 29, 2006 10:58 