CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Divergence detected in AMG Solver:TEMPERATURE

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree8Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 1, 2005, 13:25
Default Divergence detected in AMG Solver:TEMPERATURE
  #1
Sachin Nimbalkar
Guest
 
Posts: n/a
Sponsored Links
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 under-relaxation 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

zxgdey likes this.
  Reply With Quote
Sponsored Links

Old   October 2, 2005, 08:12
Default Re: Divergence detected in AMG Solver:TEMPERATURE
  #2
Wael
Guest
 
Posts: n/a
Chech the boundary conditions . If it is ok so , you may reduce the URF. Wael
  Reply With Quote

Old   October 3, 2005, 08:49
Default Re: Divergence detected in AMG Solver:TEMPERATURE
  #3
Jason
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
ambrish4u, caitoc and alex_gtz like this.
  Reply With Quote

Old   October 3, 2005, 12:28
Default Re: Divergence detected in AMG Solver:TEMPERATURE
  #4
Sachin Nimbalkar
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!
  Reply With Quote

Old   October 4, 2005, 10:17
Default Re: Divergence detected in AMG Solver:TEMPERATURE
  #5
Riaan
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.
ambrish4u and abhijeet like this.
  Reply With Quote

Old   October 5, 2005, 22:49
Default Re: Divergence detected in AMG Solver:TEMPERATURE
  #6
ztdep
Guest
 
Posts: n/a
i solved this problem by "decreasing the relax factor to a low number"
  Reply With Quote

Old   October 16, 2005, 02:10
Default Re: Divergence detected in AMG Solver:TEMPERATURE
  #7
Sachin Kulkarni
Guest
 
Posts: n/a
Hi,

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

  Reply With Quote

Old   October 8, 2010, 04:08
Default
  #8
New Member
 
sunqiang
Join Date: Nov 2009
Posts: 23
Rep Power: 9
matthewsun is on a distinguished road
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.
pk_bd likes this.
matthewsun is offline   Reply With Quote

Old   October 8, 2010, 04:14
Default
  #9
New Member
 
sunqiang
Join Date: Nov 2009
Posts: 23
Rep Power: 9
matthewsun is on a distinguished road
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.
matthewsun is offline   Reply With Quote

Old   February 8, 2011, 08:58
Exclamation divergence detected in AMG solver: temperature
  #10
New Member
 
Amit Chauhan
Join Date: May 2010
Location: Chennai, India
Posts: 13
Rep Power: 9
chauhan is on a distinguished road
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???????
chauhan is offline   Reply With Quote

Old   September 7, 2012, 07:11
Default Re: Divergence detected in AMG Solver:TEMPERATURE
  #11
New Member
 
Orkun Temel
Join Date: Feb 2012
Posts: 13
Rep Power: 7
Orkun is on a distinguished road
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.
Orkun is offline   Reply With Quote

Old   January 4, 2013, 06:21
Default
  #12
New Member
 
peyman
Join Date: Mar 2012
Posts: 8
Rep Power: 7
pzahedi is on a distinguished road
I had a same problem and I changed the relaxation factor of energy from 1 to 0.9 and it didn't error anymore
behzzad93 likes this.
pzahedi is offline   Reply With Quote

Old   January 5, 2013, 04:19
Default
  #13
Senior Member
 
SSL
Join Date: Oct 2012
Posts: 226
Rep Power: 7
msaeedsadeghi is on a distinguished road
Are you using Coupled solver? else correct your mesh. You should use a finer mesh.
msaeedsadeghi is offline   Reply With Quote

Old   March 4, 2013, 12:02
Smile
  #14
New Member
 
Fan He
Join Date: Jan 2013
Location: Virginia
Posts: 11
Rep Power: 6
caitoc is on a distinguished road
Hi all,
1 I also select this probelm by reducing Under-Relaxation 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.
caitoc is offline   Reply With Quote

Old   March 4, 2013, 19:53
Default
  #15
New Member
 
sp
Join Date: Jul 2011
Posts: 23
Rep Power: 8
chaosh is on a distinguished road
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.
chaosh is offline   Reply With Quote

Old   September 12, 2016, 13:38
Default
  #16
New Member
 
abhijeet jaiswal
Join Date: Sep 2016
Posts: 7
Rep Power: 2
abhijeet is on a distinguished road
Thanks riaan i used your method and the problem is solved.
abhijeet is offline   Reply With Quote

Old   October 29, 2016, 16:08
Default
  #17
New Member
 
yes
Join Date: Oct 2016
Posts: 17
Rep Power: 2
abir dz is on a distinguished road
Quote:
Originally Posted by Riaan
;124738
Don't solve Energy Equation for the first 50 iterations, then turn it back on.

If it still fails, you have other issues.
sir please tell me when i solve the problem after 50 iteration and turn back on i do inisialise or i run the calculation directly
please tell me because i have the same problem on the fuel cell PEMFC
abir dz is offline   Reply With Quote

Old   October 30, 2016, 00:02
Default
  #18
New Member
 
abhijeet jaiswal
Join Date: Sep 2016
Posts: 7
Rep Power: 2
abhijeet is on a distinguished road
No need to initialize the solution...directly run the calculation...
abhijeet is offline   Reply With Quote

Old   October 30, 2016, 08:19
Default
  #19
New Member
 
yes
Join Date: Oct 2016
Posts: 17
Rep Power: 2
abir dz is on a distinguished road
Quote:
Originally Posted by abhijeet View Post
No need to initialize the solution...directly run the calculation...
thank you sir l'll try and I tell you
abir dz is offline   Reply With Quote

Old   November 17, 2016, 14:15
Default
  #20
New Member
 
yes
Join Date: Oct 2016
Posts: 17
Rep Power: 2
abir dz is on a distinguished road
Quote:
Originally Posted by abir dz View Post
thank you sir l'll try and I tell you
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
abir dz is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Error: Divergence detected in AMG solver siri FLUENT 5 November 21, 2016 07:50
Divergence detected in AMG solver: ads-0 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

Sponsored Links


All times are GMT -4. The time now is 10:47.