Bad convergence
 

Hi friends.
I use ANSYS CFX.I have a serious problem in converging. Mesh quality is good:
Orthogonality Angle:36.9 ok
Expansion Factor: 13 ok
Aspect Ratio: 8 OK
My model has very large size.(Tunnel with diameter 8 m and length 100 m )
I use teta mesh.Also I use k-e model with free surface flow(standard).
By the way, y plus in my simulation is 100,000! I can reduce this to 8000 with inflation and I can not reduce this any way. Is there any relation between slow convergence and y plus?
After two step, error 1 appears whereas any F in monitor. (All of them are ok!)
I reduced timescale factor to .1 but convergence become very slow!
Is there any solution for this problem?
Best regards
ali

You cannot say mesh quality is good simply by quoting the OK/ok/! factors. This is case dependant and some simulations are MUCH more sensitive to mesh quality than others. The output file is just a guide.

If the tunnel is 8x100 metres, how big is the object inside it you are modelling? Are you using double precision numerics?

This sounds like an FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Thanks for your response ghorrocks.
I asked my problems before and you answer my questions kindly.
http://www.cfd-online.com/Forums/cfx...om-outlet.html

I used double precision but my result did not changed.

I run this model in transient state last night and saw surprisingly it is converged well. (After 100 time step RMS is 1e-5):):):)
My important parameters particularly vent air velocity is logical and constant.
I your opinion my mistake had been steady state?

Total time:10s
Time step:.001s
So number of time step is 10000!
I have to wait 25 day for finishing this time. In time step 200 I stopped solver and checked my simulation but there is still no water in the tunnel. After which time step I can stop this simulation and Compare with physical model?

Thanks in advance.
ali

It is quite possible your flow is transient so steady state was never going to converge. This is quite common, especially with bluff bodies or jet flows (you have both).

If you do not care about the time evolution of the flow and only care about the pseudo-steady state result then do not worry too much about tight convergence in the time steps, just run lots of time steps to get to what might be a psuedo-steady state, then tighten the convergence to get you answer.

If you care about the time evolution then you need to do a convergence critereon sensitivity study to correctly set your convergence critereon.

And I recommend you use adaptive time stepping, homing in on 3-5 coeff loops per iteration, with max and min time step sizes wide enough that you never reach them.

Thanks alot. But one question:
MAX residuals are 100 times larger RMS residuals! What do you think? Is it a problem?

Probably not a problem.

You are not using adaptive time stepping - you should.

I am using adaptive time stepping, this way convergence is improved, but I think there is a oscillation behavior. Is it right? Is this behavior a problem?
Inlet data are as follow:
Total time: 5 s
initial time step: .005 s
max time step: .01
min time step: .00001
max coeff loops per iteration: 3
In follow you can see convergence monitor.

With regards
ali

Make sure you never reach the min and max time steps. Also make the max coeff loops per iteration 10.

Sorry.I forgot put picture:

How can I check this?

I think I make a mistake. I set 5 for max number of coeff loops in solver control, but set 3 for target max coeff loops in analyse type.
Which of these should be 10?

If you are using adaptive time stepping and it is not converging to your criteria then you probably set the limits too tight or put a maximum number of iterations on. As I said in my previous post I suspect you did all of these things.

And if the result is it does not reach steady state (as it appears this does not) then your simulation is not steady but transient so no wonder it did not converge. Run it for long enough that the periodic pattern is consistent, then look at the cycle. You can probably do a time average to get a representative single number, but you should check first.

I think my solution in #5 which is indicated was correct. RMS 1e-5 is sufficient for me. In that solution air velocity was about 37 that was sensible(Of course this decrease gradually with time)whereas in this solution air velocity is about 10!
What do you think? Do you agree with me?

At this stage I would not trust any result you have posted so far. You have not shown either result is reliable.

Dear Glenn
Thanks for your advice.

Unfortunately My time for this project is over. Transient sate take long time and I have to try various time step. But how can I make sure never reach the min and max time steps is my problem. In addition, I do not know what initial time step should be use.

In your opinion is there any way that I use steady state instead transient? Otherwise how can I reach appropriate response with at least possible time?

By the way, What do you mean by the following statement?
"If you are using adaptive time stepping and it is not converging to your criteria then you probably set the limits too tight or put a maximum number of iterations on."

Regards
ali

Set the min to 1e-20 and the max to 1e20 and it will never reach them.

Work out the initial time step by doing an initial run and see what time step it settles on. Then do another simulation using that timestep as the initial time step.

If the flow is transient then there is no way of running it steady state.

Adaptive time stepping should adjust the time step to a value which converges to your tolerance. So in difficult to converge sections you get small time steps.

Thanks a lot for your good advice.:)