Alright, apologies for some assumptions here! Let me jot down what I know. Feel free to take a dig at it so I can correct my approach
First of all, when I run full RNG/ADV5, I disable (unclick) the intelligent solution control. This is to avoid the timestep sizes being automatically set to too small values which aids in stability. I understand with this control enabled, the Solver runs pseudo-transiently using only one inner loop for every time step. Thus, logically, smaller time step values may result in longer convergence times (though Autodesk documentation contradicts this view).
I have a basic question here. If I keep values of 0.4 and enable the intelligent control, you say it will use these values though they are greyed. But won't these values keep changing for every iteration as the time-step changes? And if this is true, then what is the point in keeping it as 0.4 as it will eventually decrease? I would rather disable the intelligent control and force the Solver to use 0.4 (or any) value so the convergence proces is not unnecessarily longer.
Hope the post addresses your question?
Correction to earlier post:
You mention the pressure/velocity values are not changed if intelligent control is enabled.
Then this only changes the time step values. So it doesnt this affect the time for convergence?
Additionally, I would like to explain my motivation for switching the intelligent control off.
Generally, I use many monitor points in the flow domain. My definition of "convergence" is the flatness of these monitor point plots (for velocity/pressure/temperature etc.) and not only the flatness of global average values. I have observed that with intelligent control enabled, the convergence occurs even when these monitors are not flat and I don't want that.
Our steady state solver is a pseudo-transient. However, we do not run just 1 loop. You can see in the convergence monitor (on the right there is a drop down to look rather than AVG to Solv Iter), this is the solver iterations per global iteration.
While we do not typically recommend making wild adjustments within the Solution Control dialog, adjustments to Velocity and Pressure do not tend to make a very large impact on overall convergence time. As I mentioned in one of the previous notes, there are models (Data Centers, or complex electronics) where we might set Pressure to ~0.25, however we will run with Solution Control Enabled.
While Solution control can adjust the timestepping, typically it wil not impeded the solutions progress or time to convergence. If your goal is to allow for an extended run and not prematurely stopping due to Auto-Convergence assessment, you can go in to the Advanced dialog (next to the Enable check box) and set this to "Tight" to tighten the convergence assessment. We do this often for external aerodynamic models. If you like you can even disable our Convergence Assessment from that dialog while keeping Solution Control enabled for stability purposes.
I would suggest (in order to try first)
Run ADV5/RNG with Velocity/Pressure relaxation to 0.4 (or even 0.3) with Solution Control ON (and Convergence Assessment OFF)
If you still see some divergences in this, try the previous recommendation or Switching the Turbulence Startup to Extend
Or increase the Turb/Lam ratio to 1000
Thanks Apollo, that was an elaborate and comprehensive discussion.
I now understand that intelligent solution control doesn't stop the solution process with premature convergence, but the automatic convergence assessment does, which I can always turn off and judge conergence on my monitor plots! Nor does it change the under-relaxation factors too much to affect ETA for convergence.
Concludingly, I would like to ask one question:
Is there any side effect if I start with "Extend" setting and Turb/Lam ratio of 1000 every time to minimise any divergence risk? I generally run the simulations overnight on cluster and any diverged simulation affects my timeline. FYI, I typically run upto 1500 iterations for every simulation, which is more than minimum 400 iterations recommended for the "Extend."
Additionally, I would like to point out that generally, I observe that in the event of divergence, the unphysical results are seen at pressure outlet boundary. e.g. velocities as high as 5000 m/s while the general velocity is upto 40 m/s.
Any thoughts on why these unphysical results exist near outelt and any suggestions for mitigating the same?
No, there shouldn't be any negative impact running Extend on your models if you are running them out as you mention.
As far as the divergence, typically with a divergence you will get impractical / non-physical resutls.
As for the reason behind it, sometimes it can be mesh related. If a gradient develops that is steeper than the mesh can capture there is a potential for some of this. Otherwise, without looking at this through a Support case, I couldn't specifically mentioned why it would diverge.