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

SU2 v.7.0.8 cannot solve expansion region that was solved by using v.6.1.0

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 16, 2021, 08:42
Question SU2 v.7.0.8 cannot solve expansion region that was solved by using v.6.1.0
  #1
New Member
 
Hüseyin Emre
Join Date: Mar 2017
Location: Istanbul
Posts: 8
Rep Power: 7
aeronautics is on a distinguished road
Dear all,

I have been trying to solve a supersonic flow domain around an aircraft with SU2 v.7.0.8 that was solved before with SU2 v6.1.0 and results were validated. I have adapted the .cfg file from v6 to v7 without any change in solvers, multigrid etc.. However, the solution I have obtained by using v7 has yielded non-physical points at the downstream of the aft where Mach number goes up to 1800. The region behind this non-physical region has been solved almost the same as in v6.

This is the non-physical solution I've got. The aircraft is attached to wind tunnel sting. I've rescaled the Mach interval as 1.6-1.8 in the image. Freestream Mach is 1.7.
wrong_solution.jpg

This is the mesh around the region. Aft of the aircraft (has relatively higher diameter) and sting (has relatively lower diameter) can be seen.
mesh.png

I'm appending the .cfg file.
config_fluid_v7.txt

What am I doing wrong? What could be the possible problem(s) and solution(s)? Any kind of help is appreciated. Thank you all in advance.

Huseyin Emre
aeronautics is offline   Reply With Quote

Old   February 16, 2021, 10:36
Default
  #2
pcg
Senior Member
 
Pedro Gomes
Join Date: Dec 2017
Posts: 428
Rep Power: 11
pcg is on a distinguished road
Some of the things that changed:
Implementation of Euler and Symmetry boundaries, to improve them for viscous flows.
How the CFL adaption works.
And I believe the reference length for limiters was fixed at one, so you might need to multiply the Venkat constant by the reference length manually.
I recommend using the adaptive CFL strategy, even if you don't go higher than 15 it can reduce CFL in more challenging regions and possibly improve stability.
With multigrid I never use damping factors higher than 0.75.
pcg is offline   Reply With Quote

Old   February 16, 2021, 11:40
Smile
  #3
New Member
 
Hüseyin Emre
Join Date: Mar 2017
Location: Istanbul
Posts: 8
Rep Power: 7
aeronautics is on a distinguished road
Quote:
Originally Posted by pcg View Post
Some of the things that changed:
Implementation of Euler and Symmetry boundaries, to improve them for viscous flows.
How the CFL adaption works.
And I believe the reference length for limiters was fixed at one, so you might need to multiply the Venkat constant by the reference length manually.
I recommend using the adaptive CFL strategy, even if you don't go higher than 15 it can reduce CFL in more challenging regions and possibly improve stability.
With multigrid I never use damping factors higher than 0.75.
Thank you Pedro for your answer! I will try your suggestions and then let you know results.

Edit:

I've used adaptive CFL, multigrid damping factors of 0.75 and different limiter coefficients. Despite residuals has decreased about 0.7, I couldn't avoid non-physical solutions.

Last edited by aeronautics; February 17, 2021 at 11:19. Reason: Update about new solutions
aeronautics is offline   Reply With Quote

Old   February 18, 2021, 07:43
Default
  #4
New Member
 
Hüseyin Emre
Join Date: Mar 2017
Location: Istanbul
Posts: 8
Rep Power: 7
aeronautics is on a distinguished road
I've overcome the issue with non-physical points. I don't know exactly why yet I think the problem was aroused from Roe scheme. I changed convective scheme to AUSM, adjusted multigrid damping factors to 0.75 and activated adaptive CFL then I could be able to get an accurate result.
aeronautics is offline   Reply With Quote

Reply

Tags
expansion, non-physical, su2 v7, supersonic

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
Can I use fvOptions to couple a solid region and a fluid region? titanchao OpenFOAM Running, Solving & CFD 4 January 14, 2022 08:55
How to let the mesh motion solver just solve a small region near a moving boundary? zhajingjing OpenFOAM Running, Solving & CFD 9 April 28, 2016 05:15
Define velocity profile in fully develpoed region to solve energy equation haghgoo_reza OpenFOAM Programming & Development 0 September 22, 2013 21:19
Can SU2 solve the blast wave problem? newmancfd SU2 2 May 13, 2013 04:33
How can I solve at the interface region K. Baker FLUENT 0 April 3, 2007 04:39


All times are GMT -4. The time now is 20:52.