CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Divergence detected in AMG Solver:TEMPERATURE (http://www.cfd-online.com/Forums/fluent/38074-divergence-detected-amg-solver-temperature.html)

Sachin Nimbalkar October 1, 2005 13:25

Divergence detected in AMG Solver:TEMPERATURE
 
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


Wael October 2, 2005 08:12

Re: Divergence detected in AMG Solver:TEMPERATURE
 
Chech the boundary conditions . If it is ok so , you may reduce the URF. Wael

Jason October 3, 2005 08:49

Re: Divergence detected in AMG Solver:TEMPERATURE
 
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

Sachin Nimbalkar October 3, 2005 12:28

Re: Divergence detected in AMG Solver:TEMPERATURE
 
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!

Riaan October 4, 2005 10:17

Re: Divergence detected in AMG Solver:TEMPERATURE
 
Don't solve Energy Equation for the first 50 iterations, then turn it back on.

If it still fails, you have other issues.

ztdep October 5, 2005 22:49

Re: Divergence detected in AMG Solver:TEMPERATURE
 
i solved this problem by "decreasing the relax factor to a low number"

Sachin Kulkarni October 16, 2005 02:10

Re: Divergence detected in AMG Solver:TEMPERATURE
 
Hi,

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


matthewsun October 8, 2010 04:08

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 October 8, 2010 04:14

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.

chauhan February 8, 2011 08:58

divergence detected in AMG solver: temperature
 
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???????

Orkun September 7, 2012 07:11

Re: Divergence detected in AMG Solver:TEMPERATURE
 
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.

pzahedi January 4, 2013 06:21

I had a same problem and I changed the relaxation factor of energy from 1 to 0.9 and it didn't error anymore

msaeedsadeghi January 5, 2013 04:19

Are you using Coupled solver? else correct your mesh. You should use a finer mesh.

caitoc March 4, 2013 12:02

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.

chaosh March 4, 2013 19:53

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.

abhijeet September 12, 2016 13:38

Thanks riaan i used your method and the problem is solved.


All times are GMT -4. The time now is 17:36.