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

Fluent Adjoint Solver?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 25, 2013, 12:05
Default Fluent Adjoint Solver?
  #1
New Member
 
Malik
Join Date: Feb 2013
Posts: 4
Rep Power: 4
ex10148 is on a distinguished road
Hello Everyone!

Hope you are all doing good. I needed help regarding the functionalities in Ansys Fluent Adjoint Solver. I wanted to ask if any of you had any experience with the Adjoint Solver in Fluent? As for my final year project I am using lift constrained drag minimization approach for a formula one front wing and I have tried to find some material on how best to use adjoint solver inorder to get a converged solution. I am having trouble in settings of controls section in the adjoint solver module inside fluent as no information can be found for best setting for turbulence modelling I can't seem to get the right combination of settings and as a result my solution is diverging. The solver seems to converge perfectly alright for the conventional flow solver but its just the adjoint solver convergence I am having issues with. Any details on how to set the settings in adjoint flow solver for converged solution will be much appreciated.

Thank You. Have a nice day.

Best Regards,
Ahmed.
ex10148 is offline   Reply With Quote

Old   February 25, 2013, 13:06
Default
  #2
Member
 
Sheng
Join Date: Jun 2011
Posts: 58
Rep Power: 6
micro11sl is on a distinguished road
Hi,
As far as I know, the adjoint Fluent solver only allows you using k-epsilon with standard wall function turbulence model. A general step may be: run your case with the turbulence model you're preferred for accuracy, run adjoint solver with the k-epsilon with standard wall function turbulence model, after the done the mesh morpher, rerun the new case with your preferred turbulence model. In this way, the results of the adjoint solver is regarded as "guiding solutions".

I am not using the adjoint solver actually, so I can't guarantee my way can solve your problem. I am personally interested with it and I have attended an ANSYS Fluent webinar session talking about how to use the adjoint solver. Please check if you can have a customer account, so you can have access to those material as well. You can apply for a student account if you're eligible.

Regards,
Sheng

Quote:
Originally Posted by ex10148 View Post
Hello Everyone!

Hope you are all doing good. I needed help regarding the functionalities in Ansys Fluent Adjoint Solver. I wanted to ask if any of you had any experience with the Adjoint Solver in Fluent? As for my final year project I am using lift constrained drag minimization approach for a formula one front wing and I have tried to find some material on how best to use adjoint solver inorder to get a converged solution. I am having trouble in settings of controls section in the adjoint solver module inside fluent as no information can be found for best setting for turbulence modelling I can't seem to get the right combination of settings and as a result my solution is diverging. The solver seems to converge perfectly alright for the conventional flow solver but its just the adjoint solver convergence I am having issues with. Any details on how to set the settings in adjoint flow solver for converged solution will be much appreciated.

Thank You. Have a nice day.

Best Regards,
Ahmed.
micro11sl is offline   Reply With Quote

Old   February 25, 2013, 13:10
Default Reply: Fluent Adjoint Solver!
  #3
New Member
 
Malik
Join Date: Feb 2013
Posts: 4
Rep Power: 4
ex10148 is on a distinguished road
Thanks for your reply. Well I have attended the two webinars on the Adjoint Solver so far and I have read all the material available on Fluent Adjoint Solver. I know the steps that you have mentioned but I need some help in the control settings of Adjoint Solver where the stabilization schemes and preconditioning are set? Because with my current settings the solution tends to diverge? Any help on that will be much appreciated. Thanks again.
ex10148 is offline   Reply With Quote

Old   February 28, 2013, 05:19
Default
  #4
Member
 
Sheng
Join Date: Jun 2011
Posts: 58
Rep Power: 6
micro11sl is on a distinguished road
Hi,
Sorry to reply late. In my limited experience, I managed to converge by "uncheck" the "apply preconditioning" for my low Reynolds number aerofoil case. I find I can't replot the residual history, so I only upload the settings on the panel.

Regards,
Sheng

Quote:
Originally Posted by ex10148 View Post
Thanks for your reply. Well I have attended the two webinars on the Adjoint Solver so far and I have read all the material available on Fluent Adjoint Solver. I know the steps that you have mentioned but I need some help in the control settings of Adjoint Solver where the stabilization schemes and preconditioning are set? Because with my current settings the solution tends to diverge? Any help on that will be much appreciated. Thanks again.
Attached Images
File Type: png draw1.png (15.8 KB, 85 views)
micro11sl is offline   Reply With Quote

Old   February 28, 2013, 08:44
Default
  #5
New Member
 
Malik
Join Date: Feb 2013
Posts: 4
Rep Power: 4
ex10148 is on a distinguished road
Thanks a lot for your reply. As a test case I also did a 2D optimisation of NACA0012 using the Fluent Adjoint Solver and it did converge by turning off the preconditioning option. But I am doing optimisation of front wing of a formula one car with wheel aswell and that makes the mesh size pretty large with separation aswell at the trailing edge of the flaps and when I turned off the preconditioning option it diverged straight away as specifying the values of artificial compressibility and courant numbers is absiolutely necessary for stable operation of the adjoint solver and using low values of Artificial Compressibility(between 0-1) and Courant Number(0.1-2.5) aids in stabilizing the convergence.

Do you know anyone who might know how to set the right values for adjoint controls inorder to get a converged solution? As the only problem I am facing is adjoint convergence. Thanks a lot.

Quote:
Originally Posted by micro11sl View Post
Hi,
Sorry to reply late. In my limited experience, I managed to converge by "uncheck" the "apply preconditioning" for my low Reynolds number aerofoil case. I find I can't replot the residual history, so I only upload the settings on the panel.

Regards,
Sheng
ex10148 is offline   Reply With Quote

Old   March 14, 2014, 05:03
Default adj solver diverges
  #6
New Member
 
metu_aee's Avatar
 
Ali Yıldırım
Join Date: Jul 2013
Location: Ankara/Turkey
Posts: 6
Rep Power: 4
metu_aee is on a distinguished road
Dude can I ask to share your NACA0012 profile adjoint solution and control settings since I am working on it but solution diverges somehow. I am stuck!




Quote:
Originally Posted by ex10148 View Post
Thanks a lot for your reply. As a test case I also did a 2D optimisation of NACA0012 using the Fluent Adjoint Solver and it did converge by turning off the preconditioning option. But I am doing optimisation of front wing of a formula one car with wheel aswell and that makes the mesh size pretty large with separation aswell at the trailing edge of the flaps and when I turned off the preconditioning option it diverged straight away as specifying the values of artificial compressibility and courant numbers is absiolutely necessary for stable operation of the adjoint solver and using low values of Artificial Compressibility(between 0-1) and Courant Number(0.1-2.5) aids in stabilizing the convergence.

Do you know anyone who might know how to set the right values for adjoint controls inorder to get a converged solution? As the only problem I am facing is adjoint convergence. Thanks a lot.
metu_aee is offline   Reply With Quote

Old   May 1, 2014, 09:48
Default
  #7
New Member
 
caphfa
Join Date: Apr 2014
Posts: 1
Rep Power: 0
caphfa is on a distinguished road
Hello people!
Maybe somebody find out the way to overcome divergence problems in adjoint solution? It seems I have tried almost all possible variants of adjoint solver settings and also I tried different “high quality” grids, but results are still far from converged solution. So, if it is impossible to obtain fully converged adjoint solution, can I use calculated gradient for optimization purposes? If somebody has similar experience I’ll be very thankful for any advice.

Thanks
caphfa is offline   Reply With Quote

Old   September 5, 2014, 12:35
Default
  #8
Super Moderator
 
Francisco Palacios
Join Date: Jan 2013
Location: Stanford, CA
Posts: 301
Rep Power: 5
fpalacios is on a distinguished road
Quote:
Originally Posted by caphfa View Post
Hello people!
Maybe somebody find out the way to overcome divergence problems in adjoint solution? It seems I have tried almost all possible variants of adjoint solver settings and also I tried different “high quality” grids, but results are still far from converged solution. So, if it is impossible to obtain fully converged adjoint solution, can I use calculated gradient for optimization purposes? If somebody has similar experience I’ll be very thankful for any advice.

Thanks
Have you tried SU2 (su2.stanford.edu) ?

Cheers,
fpalacios is offline   Reply With Quote

Old   January 30, 2015, 08:33
Default
  #9
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 4
revilo82 is on a distinguished road
In order to get good convergence with the Adjoint you have to check the following steps:
  1. CFD convergence
  2. Mesh quality (Ortho>0.05)
  3. Start with default Adjoint setup (Activate Preconditioning and stabilization)
  4. Check the AMG iterations --> if they converged within 10 iteration, all is fine. If not, decrease the CFL# until 1, decrease AC to 0.05 and 0.01, if the flow rate diverges, then increase / decrease
  5. Check outer iterations --> oscillations can be handles with URF and stabilization
  6. Dissipation scheme: increase the damping factor, reduce the damping order to 1
revilo82 is offline   Reply With Quote

Old   January 30, 2015, 08:34
Smile
  #10
New Member
 
Join Date: May 2013
Posts: 7
Rep Power: 4
revilo82 is on a distinguished road
last point: use R16!
revilo82 is offline   Reply With Quote

Old   Yesterday, 16:36
Default
  #11
Senior Member
 
Syavash
Join Date: Apr 2010
Location: Tehran, Karaj
Posts: 202
Rep Power: 8
syavash is on a distinguished road
Not quite a solution, but lowering mesh number can possibly lead to convergence!
syavash is offline   Reply With Quote

Reply

Tags
fluent, fuent adjoint solver, turbulence modelling

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
Fluent IcePak - AMG Solver Russ FLUENT 1 December 25, 2013 09:26
Multiphase modelling using Fluent VOF: Solver settings akash FLUENT 0 February 22, 2013 07:29
Compressible flow solver in Fluent jwillie2000 FLUENT 4 May 25, 2012 09:58
help required in using six dof solver in fluent Shah FLUENT 1 February 25, 2006 12:31
Viscous adjoint solver Steve Main CFD Forum 1 March 7, 2002 06:05


All times are GMT -4. The time now is 04:18.