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 e05 to 5.55 e10 (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 turbomachinery 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 kε or kω based model solution be obtained first and then a Reynolds stress model solution can be attempted from the converged twoequation solution. 3. It is frequently observed that Reynolds Stress models produce unsteady results, where twoequation 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 2eqn 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. 
Quote:

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 underrelaxation 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 underrelaxation 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.cfdonline.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 1e5 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 flowthrough 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 
All times are GMT 4. The time now is 22:07. 