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

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

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

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!

Don't solve Energy Equation for the first 50 iterations, then turn it back on.

If it still fails, you have other issues.

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

Hi,

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

[matthewsun]

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]

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]

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]

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]

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]

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

[caitoc]

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]

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]

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

[abir dz]

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

[abhijeet]

No need to initialize the solution...directly run the calculation...

[abir dz]

Originally Posted by abhijeet

No need to initialize the solution...directly run the calculation...

thank you sir l'll try and I tell you

[abir dz]

Originally Posted by abir dz

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