Adaptive Timestep and Residuals
I'm running a transient external aero simulation around some bluff bodies (ICEM hybrid mesh ~20 million elements - on my 8 core PC takes ages to run). Re = 6 million.
I did the usuall steady state simulations (SST k-omega) to determine mesh and physcial time scale sensitivity in order to get a flowfield to initialise the transient run.
I expect a turbulent flowfield behind the bluff bodies with a range of scales - not a periodic shedding of vortices. So I don't know what transient time set-up to use. Therefore, following Glenn's reply (http://www.cfd-online.com/Forums/cfx...e-problem.html) I'm using the adaptive timestepping to CFX can work it out it self.
But I've found the RMS residuals have increased greatly (see image of the run in progress). In using the SAS-SST with Bounded CD advection scheme following the ANSYS SRS Best Practice document. I could not get the residuals any lower in the steady state run as the mesh size was getting far too large (however, the steady state monitor points became constant and the imbalances were all 0%).
Should I let this simulation to continue (it'll take ages) or does anyone known how to improve things. I'm also watching the monitor points which are starting to oscillate (which I expect was they are points in the turbulent wake).
You cannot do time scale sensitivity on a steady state run. It has to be done on a transient run. Doing mesh sensitivity on a steady state run sounds OK. But if you use adaptive time stepping that avoid the problem - but you still need to define a convergence criteria and that requires a sensitivity analysis.
You cannot directly compare residuals from steady state and transient runs. They are normalised differently.
So do a sensitivity analysis on your convergence criteria on the transient run and if that shows it is OK then you are fine.
Since a timescale (in my case a physical timescale) is needed for a steady state simulation I always thought it a good idea to do a sensitivty test on that parameter. Do you consider that pointless?
With regards to a sensitivity analysis on the convergence criteria. The images shows from the CFX-Solver Manager Out File (the run is still going) the Timestep and Solver Controls I set. BTW the 1 second limit was arbitary and I'll end up stopping the run before then.
So which input parameter would I need to change? I guess it must be the Coeff Loops because since the RMS residuals (mass and momemtum) are not even getting close to 1e-06 then any change to that would, surely, not make any difference.
Sensitivity analysis on physical time step size for a steady state run is pointless. The only thing which matters is how tight the convergence is. The time step is just a means to achieve convergence.
You have specified a very tight convergence. Are you sure you need to be that tight?
Why are you using a central difference advection scheme (very accurate), second order time differencing (very accurate) but only first order turbulence numerics? This is not necessarily wrong, just that it is unusual.
My reason for setting a target residual = 1e-06 was because I thought the solver would never get to that level and so the solver would not stop running until it got the the specified number of iterations - which I set to 200 to ensure all the monitor points became flat for a good handful of iterations. I'm looking through the CFX guides about the transient residuals are normalized differently but I'm not seeing anything to say it's a different method to steady state residuals.
I was under the impression from reading through the CFX guides that because I'm not using LES (or a RANS-LES) model I should leave the turbulence numerics to 1st-order as with a RANS simulation. Do you recommend changing it for SAS-SST? Again the ANSYS SRS Best Practice gude says nothing with that respect.
So for a sensitivty test on the convergence, what parameter(s) do you suggest I change?
OK, you are just running it until it converges as far as it can.
The transient residual contains a transient term which obviously the steady state one does not.
The SAS-SST model is a transient model. You cannot run it steady state.
For sensitivity on convergence, the main parameter is the residual tolerance, but for some models the imbalance is important.
I know SAS-SST is transient only so cannot be run in steady state - I'm not sure where in the topic I gave the impression that I was trying to run it as steady state.
Anyway, the simulation crashed last night. Not 100% why but it did have a high Mach number notice (M ~ 8) which is completely none physical for this simulation. So I've set a fixed timestep and try again. If that fails I'll try SST-URANS instead of SAS-SST although that's not the preferred model.
|All times are GMT -4. The time now is 04:01.|