CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > SU2

Problem with Discrete adjoint based on RANS

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 18, 2018, 05:30
Default Problem with Discrete adjoint based on RANS
  #1
New Member
 
Suman Vajjala
Join Date: Jun 2014
Posts: 4
Rep Power: 7
SumanVajjala is on a distinguished road
Hi. I am using SU v 6.1 to extract adjoints for a simple onera M6 wing (mesh provided in the SU2 Testcases suite) using discrete adjoint for RANS and the simulations are blowing-up when the solver starts the AD part after I get the direct solution. However, the same simulation does not blow when running Euler simulation instead of RANS. I have tried many options- reducing CFL no, changing the flux calculation (Least squares and Green-Gauss) but none worked. Can you please suggest what to do in this regard.

Best
Suman
SumanVajjala is offline   Reply With Quote

Old   July 4, 2018, 04:36
Default
  #2
Zen
Member
 
Zeno
Join Date: Sep 2013
Location: Delft, The Netherlands
Posts: 60
Rep Power: 8
Zen is on a distinguished road
Hi Suman,

Can you attach your config file?

Zen
Zen is offline   Reply With Quote

Old   July 12, 2018, 02:37
Default
  #3
New Member
 
Suman Vajjala
Join Date: Jun 2014
Posts: 4
Rep Power: 7
SumanVajjala is on a distinguished road
Hi Zen!

Quote:
Originally Posted by Zen View Post
Hi Suman,

Can you attach your config file?

Zen
Sorry for the late reply. I have attached the config file. Please let me know if there are any issues with it.

Thanks
Suman
Attached Files
File Type: txt turb_ONERAM6_cfg.txt (9.9 KB, 13 views)
SumanVajjala is offline   Reply With Quote

Old   July 31, 2018, 06:36
Default
  #4
pcg
Member
 
Pedro Gomes
Join Date: Dec 2017
Posts: 81
Rep Power: 4
pcg is on a distinguished road
Hi Suman,

The universal advise with discrete adjoint is that you should converge the direct solver very well. Do note that the turbulence residuals usually take longer to drop, I usually use a much larger CFL for the turbulence equations (by setting CFL_REDUCTION_TURB > 1).

With regards to solver settings you can try:
MGLEVEL= 2 or 3

LINEAR_SOLVER= BCGSTAB
LINEAR_SOLVER_PREC= ILU
LINEAR_SOLVER_ERROR= 1E-3
LINEAR_SOLVER_ITER= 1000 (just to make sure the linear solver converges)
DISCADJ_LIN_SOLVER= BCGSTAB
DISCADJ_LIN_PREC= ILU

I suggest the switch to BiCGSTAB because that way you can increase the number of iterations to make sure the linear solver converges during the first iterations without increasing memory usage (that would happen with FGMRES). If BiCGSTAB fails (it should not with the CFL you have) switch back to FGMRES, keep ILU and reduce the number of iterations to the 10-100 range.

You mentioned that Euler works fine, keep in mind that SU2 does not have wall functions, therefore you need y+ around 1. If your wall cell size is already that small be careful with very high edge ratios (1000:1 is as far as I would go for testing).

If all this fails there is always the option to freeze the turbulence in the adjoint solver (I do not recall the name but you can check the template config file).

Cheers,
Pedro
pcg is offline   Reply With Quote

Reply

Tags
su2 ad

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
the gradients calculated through discrete adjoint are near zero Haowang SU2 9 October 17, 2019 23:53
SU2 LES, discrete adjoint testcase SU2 1 July 27, 2017 05:46
Problem with Application based on a faceZone in parallel psilkeit OpenFOAM Programming & Development 2 April 28, 2016 10:47
SQP method for adjoint based aerodynamic shape optimization cfdbooks Main CFD Forum 2 May 26, 2009 11:40
steady RANS for flow problem with unsteady inlet? kat Main CFD Forum 0 February 16, 2009 11:24


All times are GMT -4. The time now is 15:33.