CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

SMC models Convergence

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 21, 2011, 12:39
Default SMC models Convergence
  #1
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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
Far is offline   Reply With Quote

Old   July 21, 2011, 19:21
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,823
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   July 21, 2011, 23:55
Default
  #3
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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.
Far is offline   Reply With Quote

Old   July 22, 2011, 00:00
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,823
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Aspect ratio of 8000 is pretty huge. You will need to get that down for a RSM.
ghorrocks is offline   Reply With Quote

Old   July 22, 2011, 02:41
Default
  #5
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
should it be less than 1000? or even less!
Far is offline   Reply With Quote

Old   July 22, 2011, 07:10
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,823
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   July 22, 2011, 08:21
Default
  #7
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
This is very much diffult, I would rather say impossible to get the aspect ratio 100 in boundary layer.
Far is offline   Reply With Quote

Old   July 22, 2011, 08:26
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,823
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
CFD was never meant to be easy. This is why most people do not use RSM turbulence models.
ghorrocks is offline   Reply With Quote

Old   July 23, 2011, 05:29
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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?
Far is offline   Reply With Quote

Old   July 23, 2011, 06:25
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,823
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   July 23, 2011, 06:41
Default
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by ghorrocks View Post
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
Far is offline   Reply With Quote

Old   July 24, 2011, 04:18
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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.
Far is offline   Reply With Quote

Old   July 24, 2011, 06:33
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,823
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   July 25, 2011, 05:46
Default
  #14
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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)
Comparison of fluent and CFX for turbomachinery
Far is offline   Reply With Quote

Old   July 25, 2011, 08:12
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,823
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   July 26, 2011, 14:16
Default Local time stepping
  #16
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Is local time stepping useful for stiff numerics ?
Far is offline   Reply With Quote

Old   July 26, 2011, 18:47
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,823
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   August 5, 2011, 07:34
Default
  #18
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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
Far is offline   Reply With Quote

Old   August 5, 2011, 18:16
Default
  #19
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,823
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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
ghorrocks is offline   Reply With Quote

Old   August 6, 2011, 02:16
Default
  #20
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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
Far is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Convergence Centurion2011 FLUENT 24 May 9, 2015 08:02
convergence of Spalart-Allmaras and k-w(SST) turbulence models smartdingo Main CFD Forum 0 July 14, 2010 11:03
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
increasing mesh quality is leading to poor convergence tippo CFX 2 May 5, 2009 10:55
Defect correction and convergence ganesh Main CFD Forum 4 June 30, 2006 14:20


All times are GMT -4. The time now is 15:42.