Implicit supseronic flow simulations in flexi
1 Attachment(s)
Dear all,
I am trying to perform a Mach 2 supersonic flow simulation in flexi (https://www.flexi-project.org/) using implicit time stepping. Flexi user guide describes how to do implicit simulation for a Mach 0.2 RANS flat plate simulation. However, I am unable to obtain the correct solution with implicit time stepping in the supersonic case I am interested in. The simulation I am doing is of an impinging shock-boundary layer interaction. I am pasting my settings here and attaching the mesh file (degrez_corrected_mesh.h5) as a part of the zipped attachment to this post. Code:
!================================================================================== Code:
Attention: Timestep failed, repeating with dt/2! Code:
Timestep : 5.8680110E-07 My build settings: Code:
CMAKE_BUILD_TYPE Release Thanking in anticipation Vachan |
Dear vachan,
I will contact my FLEXI collegues. We're going to make this work! Regards |
Thanks a lot, Eifoehn4! I am truly grateful for your quick response and support!
|
Dear Vachan,
there was indeed a bug in the code that caused this behavior you observed. We fixed this and the updated version will be available on github after the weekend. So just pull the most recent version on Monday and you can run your simulation! What you observed was the following: the bug caused not choosing the shock-capturing scheme property. This then resulted in instabilities, so FLEXI tried to repeat the timestep but it was never stable. Though, I am not sure if implicit time discretization is the best choice for your setting. As the Mach number is quite high and the solution (especially in the beginning) changes rapidly, the implicit method is not able to use very large timesteps. So you maybe have to ramp your timestep to obtain a stable simulation. Kind regards, Jonas |
Dear Jonas,
Quote:
Quote:
Quote:
Thanks again for such a quick response! |
Still not working?
Dear Jonas,
As you said, I have noticed that a commit for the bug fix has been made to the github repo: https://github.com/flexi-framework/f...acaf6dd614ba21. I have compiled the latest version of flexi now. However, I am afraid this still didn't improve the performance of implicit stepping. This time, I started the implicit solution (with CFL 5 and the settings pasted below) with the solution at 1e-3 sec obtained through explicit stepping (standardrk3-3). By my estimate, the flow becomes steady in about 3e-3 sec. So at 1e-3 sec, most of the transients are gone, and it is only a matter of the separation region growing to its full size after this point. Code:
!========================================================================================= Code:
Attention: Timestep failed, repeating with dt/2! Thanking again, Vachan |
Dear Vachan,
I am not completely sure why this is happening in your case - there is something going wrong with the preconditioner. We probably will need some time to figure that out. In the meanwile I would suggest to use either fully explicit methods or implicit methods without preconditioning and additionally change your settings slightly: Code:
!========================================================================================= Kind regards, Jonas |
Dear Jonas,
Thanks for your response. It is indeed running fine without the preconditioner and your suggestions. I wish and hope that the issue in preconditioner will be sorted out soon! Thanking again, Vachan |
Dear Vachan,
I had a closer look on your problem and I think the main issue that causes bad convergence behaviors is the non-linearity of the slope limiting procedure (you selected "minmod" limiting). In this forum thread http://www.cfd-online.com/Forums/mai...d-limiter.html you find a related discussion and in the publications W. Gropp, D. Keyes, L. C. McInnes, M. D. Tidriri: Globalized Newton-Krylow-Schwarz algorithms and software for parallel implicit CFD. The International Journal of High Performance Computing Applications 14(2), 102-136 (2000) and P. A.Burton, P. K. Sweby: A Dynamical Approach Study of Some Explicit and Implicit TVD Schemes and Their Convergences to Steady-state Solutions. Numerical Analysis Report 5/95, University of Reading, Department of Mathematics, 1995. you find some investigations on this. I therefore recommend you to use the first order finite volume scheme for shock capturing, i.e. Code:
FV_LimiterType = 0 Moreover, it is recommendable to change your preconditioner settings as I observed that the accuracy of the preconditioner with ILU(0) inversion of the blocks is not sufficient for larger timesteps for your setting. Maybe you can try the following settings: Code:
PrecondType = 1 I hope that helps you! Kind regards Jonas |
Dear Jonas,
Sorry for such a late response! I am really grateful to you for your continuing engagement in this topic. I will try the settings you suggested and get back with my experience shortly. Thanks again! |
Dear Jonas,
As you mentioned, I confirm that I was able to use CFL=5 (which corresponds to dt ~ 1e-4) without any convergence issues. Thanks! |
All times are GMT -4. The time now is 05:55. |