CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   A simple problem about Adaptive Time steps (http://www.cfd-online.com/Forums/cfx/110418-simple-problem-about-adaptive-time-steps.html)

sakurabogoda December 10, 2012 22:34

A simple problem about Adaptive Time steps
 
I am using adaptive time steps for a simulation.

Min. time step= 0.0001S
Max. time step= 0.05S

My problem is, now the simulation is running around 5000 time steps, but it uses only 0.0001S for all steps.

Why the solver does not change the time step (its own time step)?

(I used this much of smaller time step as always solver diverged with larger time steppes, even for 0.001S)

ghorrocks December 11, 2012 03:57

Assuming you are using adaptive time steps homing into 3-5 coeff loops per iteration (which is the general recommendation), then if it keeps making the time step size smaller and smaller you have some issues to consider:
1) Is this just an initial transient thing, which has no bearing on the overall simulation accuracy? If so then you can just use the lower time step limit to stop it going too far, converge loosely through this bit and it is OK providing the convergence recovers as the simulation progresses.
2) Is your convergence critereon too tight? Do a convergence sensitivity check to see if you need a convergence tolerance as tight as you currently have. Looser convergence = bigger time steps = faster simulation = happy boss.

Lance December 11, 2012 03:58

Well, what is your critera for adaptive stepping? Max Courant number or specified coefficient loops? For example, if the solver cannot converge within the max coeff loops it will try to decrease the timestep until the min allowed time step.

sakurabogoda December 11, 2012 04:27

Dear Glenn and Lance,
Many many thanks...

Glenn:
01. This is for overall simulation. I am working with cyclone flow.
02.Actually I am using 3 coeff loops per iteration and convergence tolerance is e-6.

Lance:
Though CFX is implicit I used courant no. 0.1 and 0.5 to lower and upper limits because I am using LES. Also 3 coeff loops per iteration.

*Thanks again for your advises and I will do a sensitivity analysis by adjusting coeff loops and convergence criteria.

Lance December 11, 2012 04:34

Ok, max courant at 0.5 and residuals at 1e-6 might be too tight to get convergence within 3 coeff loops with a time step at 1e-4 s, which explains why the solver stays at the minimum allowed time step.

sakurabogoda December 11, 2012 06:02

Dear All, I have tried the simulation again with following adjustments, but solver diverged. :(

max. courent no. = 1.0, min. courent no. =0.5
convergent criteria = e-5
max. coeff. loops per iteration = 5
time step = 0.001S

the problem is, all simulations ran correctly with inlet velocities of 5m/s and 10m/s and the solver diverges with 15m/s inlet velocity.

As the expectation is highly turbulent flow, is it possible to increase courant no and convergence criteria?

Lance December 11, 2012 06:27

Quote:

Originally Posted by sakurabogoda (Post 396876)
As the expectation is highly turbulent flow, is it possible to increase courant no and convergence criteria?

why not test and find out for yourself?
However, LES often requires a very fine time step to resolve the scales accurately and it could be that 0.001 s is not sufficient.

ghorrocks December 11, 2012 17:01

The general recommendation is to use adaptive time stepping homing in on 3-5 coeff loops per iteration. Courant number adaptive time steps are not generally recommended. And as suspected your convergence toelrance is very tight for a transient run and can almost certainly be relaxed. You need to do a sensitivity analysis to determine what the correct convergence tolerance for your case is.

sakurabogoda December 11, 2012 21:00

Dear All,
Thank you very much.
I used adaptive time stepping with 1e-4 convergence and there too, time steps did not change. Simulation runs with time step=0.0001s only.
The problem is then the simulation takes too much time but I think this is the max time step that I can choose. :(
Thanks a lot for your kind helps again.

ghorrocks December 12, 2012 05:22

Welcome to CFD :), this is why people use super computers for CFD.

Did you do a sensitivity study of did you just try 1e-4? Unless you actually determine what you need you are guessing. And you could save your self a lot of time and effort by just drawing the results you want to see in photoshop.

But do not compromise the accuracy of your simulation by setting a big minimum time step. Rather get a more powerful computer or more parallel power. And don't forget to do sensitivity checks on mesh, time step and convergence tolerance so you do not set them too coarse or fine.


All times are GMT -4. The time now is 07:53.