CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Adjoint convergence on race-car

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

Like Tree1Likes
  • 1 Post By jabeken

LinkBack Thread Tools Search this Thread Display Modes
Old   May 9, 2018, 12:10
Default Adjoint convergence on race-car
New Member
Jonas Abeken
Join Date: Apr 2018
Location: Zurich
Posts: 10
Rep Power: 6
jabeken is on a distinguished road

I am currently trying to set up an adjoint simulation-workflow for a closed-wheel race-car. However, the convergence of the adjoint-solver is very unstable and minor changes of the geometry and/or mesh can lead to divergence.
My current model-setup includes:
- Polyhedral mesh, with high-y+ prism layers (3 layers)
- Coupled Implicit 2nd order
- realizable k-e with two-layer all y+ wall-treatment
- AMG-solver set to W-cycle with a tolerance of 1e-5 and 2 pre- and post-sweeps (for both coupled and adjoint)
- Adjoint solver at 1st-order, with a CFL of 40 (reducing the CFL to 20 had no effect on convergence)

Looking at the location of the highest residuals of the diverged adjoint-solver, the divergence always starts somewhere in the prism-layers, most of the time at the start of a separation or some other area where oscillating flow-behavior can be expected. Also, due to the velocity change in these areas, they often show y+ values in the unfavorable region of 5<y+<30. This can hardly be avoided due to the wide range of present velocities over the whole car.
As the adjoint-solver in Star-CCM+ operates with frozen turbulence, I assume that I have to achieve a better convergence of the turbulence-properties before attempting to go over to the adjoint-solver.
Attempting to switch to a k-omega SST with high resolution prism-layers in my experience leads to very slow convergence of the coupled solver and additional instabilities in "transient" areas due to the high resolution, which is why I would like to avoid this.
I also already tried to switch on the GMRES Acceleration for Adjoint which slowed the convergence to a crawl, making it not a valid option.

Has anybody some experience with the adjoint-solver on oscillating flows or hard to converge geometries? I appreciate any input!

I attached the current develpment of residuals, the first two steps show the switch from segregated to 1st-order coupled and then 2nd-order coupled, which I need to achieve a good initial condition for the 2nd-order coupled.

Thanks and best regards,
Attached Images
File Type: jpg Diverging.jpg (120.4 KB, 48 views)
jabeken is offline   Reply With Quote

Old   February 13, 2019, 05:16
Default Solved
New Member
Jonas Abeken
Join Date: Apr 2018
Location: Zurich
Posts: 10
Rep Power: 6
jabeken is on a distinguished road
So, I basically found a "brute-force" method suggested by Star which is in fact the GMRES solver (acceleration method in adjoing solver).
It is computationally VERY costly per iterations but takes very little iterations to converge which makes the overall cost to convergence acceptable.
For hard to converge cases the Krylov-spaces have to be increased (in my case it achieved stable convergence at around 40 Krylov spaces).
More Krylov spaces mean more memory requirement and time per iterations but for me it was the only way to achieve convergence.

Maybe this helps some other struggling soul in the future.
addis likes this.
jabeken is offline   Reply With Quote


adjoint, convergence, coupled, oscillating residuals

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
problem with Min/max rho tH3f0rC3 OpenFOAM 8 July 31, 2019 09:48
Problems launching adjoint max_ SU2 2 March 12, 2016 11:32
2d ffd Luca B SU2 Shape Design 6 September 19, 2015 23:46
Race car Edu Main CFD Forum 0 September 29, 2005 11:22
CFD for a Soap Box Derby car Dean Christakis Main CFD Forum 0 July 6, 1999 01:09

All times are GMT -4. The time now is 12:44.