SMC models Convergence
 

Dear Fellows

I am trying to simulate the rotor 37 transonic rotor. I have completed the mesh independence study, y plus independence study, made compresion between wall function and yplus 1 meshes for the one equation (SA) and two equation models (KE, BSL, SST).

I have also successfully used the SSG Reynolds Stress model (second moment closure <SMC> model) and BSL RSM model using the wall function mesh. I have also used yplus 1 mesh for SSG model,

But I am unable to get the convergence for the BSL Reynolds stress model with yplus 1 mesh

I tried the following but no success

1. used the BSL results for the same mesh as initial guess for the RSM BSL model

2. used the low rpm at first and then gradually increased to higher values.

3. Used the first order upwind scheme

4. used the double precision solver.

5. reduced the time step from 5.55 e-05 to 5.55 e-10 (physical time scale)

6. multiplied the auto time scale with 0.1 and 0.01 (default value is 1)

6. all of the above steps simultaneously

I am looking forward for your help

Best Regards
Far

PS. I have very good results with same mesh and eddy viscosity models and most of the time error is less than 1% with experimental results. These results are even better than I have found on the NASA and journal of turbo-machinery with LES and two equation models

Reynolds stress models are hard to converge so it is not a surprise that it has caused problems. They are often very sensitive to mesh quality.

which mesh parameter is most impotant ? my minimum angle is 28 deg (far from the wall surface) and maximum aspect retio is 8000. I believe that after selecting the double precision solver aspect retio should not be the problem.

Aspect ratio of 8000 is pretty huge. You will need to get that down for a RSM.

should it be less than 1000? or even less!

It should be low enough to make it converge :)

Aspect ratio of 1000 is still huge so I doubt that will work. 100 is still large but might be OK. Just keep improving it until it works.

This is very much diffult, I would rather say impossible to get the aspect ratio 100 in boundary layer.

CFD was never meant to be easy. This is why most people do not use RSM turbulence models.

This is what I got from CFX help

1. In principle, the same time step can be used for all turbulence model variants, but pragmatically the time step should be reduced for the Reynolds Stress Model due to the increased complexity of its equations and due to numerical approximations made at general grid interfaces (GGI) and rotational periodic boundary conditions.

2. If convergence is difficult, it is recommended that a k-ε or k-ω based model solution be obtained first and then a Reynolds stress model solution can be attempted from the converged two-equation solution.

3. It is frequently observed that Reynolds Stress models produce unsteady results, where two-equation models give steady state solutions. This can be correct from a physical standpoint, but requires the solution of the equations in transient mode.

What should be done: Meshing quality or above steps?

Well, we are both right. Both my comments and support's comments are generalisations and I have no idea what is happening in your specific case. RSM is very sensitive to mesh quality, and RSM often needs a small time step, good initial conditions and can be transient when a 2-eqn model is steady.

So I would try them all until it starts working.

Your first post suggests you have already tried the initial condition and small time step approaches. So you only have transient and better mesh quality left to try. Both of them will result in long simulation times so I hope you have a big computer available.

I have only 4 GB RAM and DELL 670 workstation with duel xeon 3.4 Ghz processora

This is from the fluent help about RSM models

Using the RSM creates a high degree of coupling between the momentum equations and the turbulent stresses in the flow, and thus the calculation can be more prone to stability and convergence difficulties than with the - models. When you use the RSM, therefore, you may need to adopt special solution strategies in order to obtain a converged solution. The following strategies are generally recommended:

1. Begin the calculations using the standard - model. Turn on the RSM and use the solution data as a starting point for the RSM calculation.
2. Use low under-relaxation factors (0.2 to 0.3) and (for the coupled solvers) a low Courant number for highly swirling flows or highly complex flows. In these cases, you may need to reduce the under-relaxation factors both for the velocities and for all of the stresses.


Instructions for setting these solution parameters are provided below. If you are applying the RSM to prediction of a highly swirling flow, you will want to consider the solution strategies discussed in Section 8.4 as well.

The under relaxation factor comments are not relevant to CFX. The other comments are relevant, but only repeat what support said in your post yesterday.

Problem is solved by using the yplus 10 mesh (to lower the aspect ratio in boundary layer) and double precision solver (further relaxing the aspect ratio problem.

Shall share the complete updates with forum soon.

As far as the validation of yplus 10 mesh is concered reader is reffered to following post (2nd image in pdf format)
http://www.cfd-online.com/Forums/cfx...machinery.html

You can also get the same aspect ratio by staying at y+=1, but using 10 time more elements along the chord. Of course this results in a 10x larger mesh which only makes run times even longer.

Local time stepping
 

Is local time stepping useful for stiff numerics ?

Yes, I find it very useful for getting tricky steady state simulations on the way to convergence. But you need to run physical timestepping for a while afterwards before declaring it converged, you cannot run the entire way with local time stepping.

I have made another mesh with aspect ratio of 1000 (yplus = 10, double precision solver) and used the SSG RSM model. This time again I had hard time in converging the solution, but due to higher quality and use of local time stepping I am able to reduce the residuals by order of 1e-5 and still converging (although five to six times more time steps needed than two equation models)

It was previously suggested on this forum and user guide that the last few iterations should be run with physical time step, now my questions are:

1. what is the current time step for all variables of my simulation, as scale varies for all variables. As in auto time scale, solver displays the time scale after few iteration whereas in physical time step we know in advance the time step.

2. What should be time step size of last few iterations using the physical time step

3. I guess I should modify current pre file and specify the physical time scale and use the converged solution using local time stepping as initial values. Am I right?

4. It is mentioned that last few iterations should be run with physical time step, how to determine the few iterations, should it be 10, 20, 100 or as per requirement

5. If the solution diverges in physical time scale what should be done?


Best Regards
Far

1 - there is no single timescale as it varies across the domain.
2 - running for about 1 time scale sounds sensible (1 flow-through time, 1 eddy turnover time etc)
3 - yes, you can also do the change over with edit run in progress then you do not need to stop and restart.
4 - see 2
5 - Make the time step smaller

Thanks ghorrocks

I cant understand how to change the time scale from local to physcial, becuase when I try to change it by edit run in progress it gives me error.

and what should be the time step for physical time scale for last few iteration, or I have to find it by hit and trial?

Best Regards

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: