If you change to local time stepping from physical or vice versa you have to set a number of parameters correctly or it returns an error. Have a look at the CCL of a run set up for local time stepping and a run set for physical time stepping to see what parameters you need to set.

Problem solved. I used the default time stepping method, that is auto time scale. Just reduced the Timescale Factor by 10, so that my default time step of 5.5 * 10e-05 reduced to 5.5*10e-06. This incrased time steps, for converged solution, from 100-150 to 1000-1300 depending on the flow regime (choking, design or stall).

PS.

1.It is very important to note that, for using the SMC model you requrie patience and lot of patience. Many times when you look at the residual plot, you dont find any noticble improvment in solution, but it is ok.

2. Aspect ratio is around 1000-1300, and this should not be the problem after adopting above strategy.

Similar problem with RSM in transient
 

Hi Fellows,
let me open up this thread again as I have a similar problem, but couldn't solve it yet. I can't get convergence with BSL Reynolds Stress Model (RSM) in a transient simulation.
I am trying to simulate the flow in a small basin (2 x 0.8 x 0.4 m) with ANSYS CFX 14. Since I want to know about the evolution of the flow when the quiet basin is flooded, I am performing a transient simulation. The flow is basically a free stream; attachment to the wall is only in a small region. Flow velocities are small, about 5 cm/s (0.05 m/s).
I tried two equation models (k-e, k-o, sst, sst with curvature correction). Results in comparison with measurement are OK, although it's needless to say that two equation models don't capture fluctuations in the velocities. From a RSM I expect these fluctuations to be captured better, that's why i would like to use RSM.
To get the RSM simulation running, I use the results after the first two time steps of the k-epsilon simulation as initial conditions. Starting directly with RSM doesn't work.
My problem is I can't get convergence with RSM. Initially the residuals fall to 1e-5 within 10 coefficient loop iterations, but after a few seconds of simulation time they rise to about 2e-4 and remain there. Reducing the time step by a factor of 10 results in falling residuals to 1e-5 and then rising again to 2e-4. I did it several times to a time step of 0.0005 s (I started with 0.1 s), always the same effect. What's curious: each time I decrease time step, the velocity fluctuations become larger by a factor of approx. 10. This results in quite unrealistic velocity peaks, becoming even worse the lower the time step. Due to the rising velocities, I'm not able to reduce the max. Courant number below C_max=12, but C_RMS is reduced with a smaller time step (it's below 1).
Mesh quality is good (see below), although I'm not able to reach mesh independency, because of a lack of computational resources. With the two eq. models my yplus is below 5, but since its free stream it shouldn't have an influence. Due to fluctuations with RSM, yplus is higher with this model.
min. ortho. angle=29.4°
max expansion factor=3
max aspect ratio=5

Any ideas how to improve convergence and how to choose the right time step size?
CFX help tips don't work:
1. Reducing time step results in the above mentioned problem (no improvement in convergence, higher velocity fluctuations).
2. Obtaining two eq. model simulation first is not possible, because I want to simulate the evolution of the flow with changing BC.
3. It's already a transient simulation.

RSM models are very sensitive to mesh quality. Your mesh quality is probably fine for 2-eqn models, but inadequate for RSM. In my experience RSM runs fine when the mesh quality is very good.

But note my experience is with single phase RSM. Multiphase RSM could well be different.

It took a while, but I made several test with a high quality mesh (see below) without success. The behavior is still the same: reducing the time step decreases the residuals first, but after some iterations they rise again. With the velocities it's the same.
There seems to be a connection with the Courant Number. If max. Courant is around 1 (RMS Courant = 0.03!), residuals are good. But when max. Courant is getting higher, convergence stalls. I'm not sure if velocity (and hence Courant) is rising, resulting in bad convergence, or if the problems with convergence causes the increase in velocity. There is no obvious reason (like changing BC) that causes the change.
My mesh quality is now as follows:
min. ortho. angle = 74°
max. expansion factor = 2
max aspect ratio = 5
I will reduce the aspect ratio and see if there is any improvement, although I can't believe that an aspect ratio of 5 should be a problem. Any other suggestions which quality metrics are of importance?

An aspect ratio of greater than 1.2 results in significant errors in surface tension modelling. The only way to be sure on what mesh quality it requires is to test it and find out.

It may also be easier to draw a simple box where you deliberately generate meshes of various aspect ratios, expansion ratios and othogonality. This way you can generate meshes of any quality you like and run a RSM simulation on them and see how they go. If this goes well you will get a target mesh quality required to get a good result.

Sorry for answering late,
finaly I didn't get it running and I gave it up.
I did as you suggested and made a simple box test case with the same mesh quality. But I was not able to reproduce the the behavior of the full scale model.
Thanks for your help, anyway.

I'm guessing I'm too late here, but depending on your velocity scales 0.0005 s is not that small for a transient run. You also mentioned a Courant of 12. The Courant number isn't that import in one phase simulations for CFX, but since you're solving a free surface simulation if the volume fraction equation isn't coupled it could affect your solution. Either keep decreasing the timestep or try using the coupled volume fraction option (you might still need to decrease the timestep, though). You should have a timestep value that allows you to converge each timestep iteraion in 3-5 coefficient loops.

Good luck.

That's why I generally recommend doing transient runs with adaptive time stepping homing in on 3-5 coeff loops per iteration. Then the solver automatically takes care of the time step size.

In terms of automation, that really is the best option. The only thing I don't like about auto-timestepping is that is messes up with any type of animation you'll want to do at post-processing. There are some ways to decrease the effects, but they never completely go away.

Thanks for your suggestions.
It is not a multiphase flow, I'm modeling the water surface by a symmetry BC. But later I wan't to introduce a dispersed phase, so I'll keep your tip in mind.
Concerning time step size, it's not practicable for me to reduce it further, so I guess RSM won't help me.
But I tried a SAS with pretty good results compared to meassurements. It works fine with a much higher time step, although I haven't made a senstivity check on that, yet.

What are the requirements of SAS model?

SAS is similar to LES. In regions where your mesh resolves turbulent structures the turbulence model goes unsteady, don't ask me how. You should read the sections in the CFX Modeling Guide about LES, DES and SAS.
In my case SAS works fine with a rather coarse grid and a timestep with Courant between 0.5 and 1. But as I said, I haven't made a sensitivity check on that.

According to modeling guide :

1. SAS is improved URANS approach and gives you the LES like behavior in detached flow regions.

2. Contrary to DES (RANS/LES) SAS cannot be forced to go unsteady by grid refinement.

But I cannot find the exact requirements of meshing for SAS model, that's why I asked this. :eek: