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

SU2 Transonic Flow simulations bad results

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 16, 2014, 12:19
Default SU2 Transonic Flow simulations bad results
  #1
New Member
 
Spyros
Join Date: Mar 2014
Posts: 15
Rep Power: 3
S.Kontogiannis is on a distinguished road
Hello everyone,

As a part of my master thesis i will be using SU2 to simulate transonic flow around a wing and a complete aircraft configuration with long term goal to use the adjoint optimizer for optimizing the airfoil shape (and maybe the wing planform).

As a starting validation case I am considering the RAE 2822 case described in http://www.grc.nasa.gov/WWW/wind/val.../raetaf04.html (M=0.729, a=2.31 deg). However my results are not good.

I have tried JST method for the convective fluxes as well as the 2nd order ROE Method and the 2nd order HLLC Method (S-A used for modelling turbulence). All of these methods produce bad quality results in both structured grids I have used. I have used a coarse grid of y+~10 and another intermediate grid of y+~1.

HLLC is diverging and ROE and JST converge in non physical results after many iterations. I should also point out that when I use multi-grid every method diverges. Another "strange" fact is that the coarse mesh produces slightly better results.

I have uploaded a photo of my intemediate grid and some figures showing the results and a typical convergence behaviour.

I would appreciate any help, thanks.
Spyros


(This is a re-posted thread from SU2 Transonic Flow simulations bad results)
Attached Images
File Type: jpg Coarse_grid_Comparison.jpg (67.7 KB, 21 views)
File Type: jpg Convergence.jpg (49.0 KB, 18 views)
File Type: jpg JST_Comparison.jpg (67.8 KB, 19 views)
File Type: jpg structured_mesh.jpg (95.6 KB, 26 views)
Attached Files
File Type: txt turb_SA_RAE2822_2ndUpwind.txt (15.0 KB, 11 views)
S.Kontogiannis is offline   Reply With Quote

Old   May 18, 2014, 21:39
Default
  #2
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 S.Kontogiannis View Post
Hello everyone,

As a part of my master thesis i will be using SU2 to simulate transonic flow around a wing and a complete aircraft configuration with long term goal to use the adjoint optimizer for optimizing the airfoil shape (and maybe the wing planform).

As a starting validation case I am considering the RAE 2822 case described in http://www.grc.nasa.gov/WWW/wind/val.../raetaf04.html (M=0.729, a=2.31 deg). However my results are not good.

I have tried JST method for the convective fluxes as well as the 2nd order ROE Method and the 2nd order HLLC Method (S-A used for modelling turbulence). All of these methods produce bad quality results in both structured grids I have used. I have used a coarse grid of y+~10 and another intermediate grid of y+~1.

HLLC is diverging and ROE and JST converge in non physical results after many iterations. I should also point out that when I use multi-grid every method diverges. Another "strange" fact is that the coarse mesh produces slightly better results.

I have uploaded a photo of my intemediate grid and some figures showing the results and a typical convergence behaviour.

I would appreciate any help, thanks.
Spyros


(This is a re-posted thread from SU2 Transonic Flow simulations bad results)

Hi, interesting... this problem should work without problem, unless there is an issue with the grid or the non-dimensionalization. I would like to propose some changes in your configuration file.

To avoid any kind of problems with the non-dimensionalization, be sure that the chord of the airfoil in your mesh is 1... if that is the case then
REYNOLDS_LENGTH= 1.0

On the other hand, let's run the simulation dimensional

% Reference pressure (101325.0 N/m^2 by default, only for compressible flows)
REF_PRESSURE= 1.0
%
% Reference temperature (273.15 K by default, only for compressible flows)
REF_TEMPERATURE= 1.0
%
% Reference density (1.2886 Kg/m^3 by default, only for compressible flows)
REF_DENSITY= 1.0

with respect to the numerical methods...
CONV_NUM_METHOD_FLOW= ROE-2ND_ORDER
SLOPE_LIMITER_FLOW= VENKATAKRISHNAN

and

CONV_NUM_METHOD_TURB= SCALAR_UPWIND-1ST_ORDER

anyway, in the TestCases folder you will find a RAE2822 simulation.

/TestCases/rans/rae2822/turb_SA_RAE2822.cfg

Please note that the latest version in the git repository has introduced some changes in some tags of the config file.

Best,
Francisco
fpalacios is offline   Reply With Quote

Old   May 19, 2014, 11:47
Default
  #3
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 448
Rep Power: 9
Martin Hegedus is on a distinguished road
I'm definitely not an SU2 expert but this caught my attention when first posted in the Main section.

If the path that Francisco outlined doesn't work out, another thought is to remove the grid clustering where the shock is or to use dual time stepping. The reason I suggest this is that when using local time stepping, and the grid clustering is reduced, the smaller delta dt in the refined area does not allow the solution to work it's way through very well. In other words, the flow views the area as a type of not very porous wall.
Martin Hegedus is offline   Reply With Quote

Old   May 19, 2014, 12:08
Default
  #4
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 448
Rep Power: 9
Martin Hegedus is on a distinguished road
Oh, I want to mention that grid clustering's effect on delta t will not affect the converged steady state solution, it only affects convergence. If the feeling is that the solution is converged, then this is not the issue.
Martin Hegedus is offline   Reply With Quote

Old   June 5, 2014, 06:17
Default
  #5
New Member
 
Spyros
Join Date: Mar 2014
Posts: 15
Rep Power: 3
S.Kontogiannis is on a distinguished road
Dear fpalacios and Mr Hegedus,

Thank you for your reply and I am sorry for my late response.

I have tried your proposed solutions but unfortunately with no success. The weird thing is that in these last attempts I do not alter any of the default setups (from the Stanford test case), but still I have very bad results especially in the suction side. Also, I do not understand why multi-grid leads to divergence, and so quickly.

From what I understand, the only difference between my case and the Stanford test case is the grid. My grid is structured instead of hybrid and if I am not mistaken more fine near the wall. I do not know if that creates issues in the code but it does not make sense to be the source of the problem since the same mesh is of good quality and has worked nicely in commercial codes.

Thank you very much,
Spyros
S.Kontogiannis is offline   Reply With Quote

Old   June 5, 2014, 14:48
Default
  #6
Super Moderator
 
Francisco Palacios
Join Date: Jan 2013
Location: Stanford, CA
Posts: 301
Rep Power: 5
fpalacios is on a distinguished road
Could you please share the grid that you are using, we should like to take a look at it.

Cheers,
Francisco
fpalacios is offline   Reply With Quote

Old   June 5, 2014, 15:43
Default
  #7
New Member
 
Spyros
Join Date: Mar 2014
Posts: 15
Rep Power: 3
S.Kontogiannis is on a distinguished road
Dear Mr. Palacio,

Thank you very much for your superfast reply. Of course. I am uploading you a coarse and an intermediate grid (cgns files) in a zip folder.
https://www.dropbox.com/s/y02kwj3m8eksdey/RAE_2822.zip

Thanks,

Spyros
S.Kontogiannis is offline   Reply With Quote

Old   June 6, 2014, 01:55
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 S.Kontogiannis View Post
Dear Mr. Palacio,

Thank you very much for your superfast reply. Of course. I am uploading you a coarse and an intermediate grid (cgns files) in a zip folder.
https://www.dropbox.com/s/y02kwj3m8eksdey/RAE_2822.zip

Thanks,

Spyros
Hi, the case is working for me... just two small comments:
- The y+ of the coarse grid is not appropriate for the SA model.
- In order to run the intermediate mesh, could you create a new mesh with chord = 1.0 .

Attached a config file that is working for me (using a grid with a chord= 1.0)

Cheers,
Francisco
Attached Files
File Type: txt turb_SA_RAE2822.txt (15.1 KB, 12 views)
fpalacios is offline   Reply With Quote

Old   June 6, 2014, 04:15
Default
  #9
New Member
 
Spyros
Join Date: Mar 2014
Posts: 15
Rep Power: 3
S.Kontogiannis is on a distinguished road
Dear Mr Palacio,

Thank you very much for your help.
The grid was initially created with not a c=1 value in order to be exact to the NASA test case #4 (http://www.grc.nasa.gov/WWW/wind/val.../raetaf04.html) where the Re number led to a chord of 0.3048. Do you believe this was the problem? I will try it with a chord of 1.

The coarse grid was deliberately not appropriate as to be the first mesh of a grid convergence study.

Thank you very much,
I will create the mesh again, run the simulation and let you know.

Spyros
S.Kontogiannis is offline   Reply With Quote

Old   June 6, 2014, 17:47
Default
  #10
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 S.Kontogiannis View Post
Dear Mr Palacio,

Thank you very much for your help.
The grid was initially created with not a c=1 value in order to be exact to the NASA test case #4 (http://www.grc.nasa.gov/WWW/wind/val.../raetaf04.html) where the Re number led to a chord of 0.3048. Do you believe this was the problem? I will try it with a chord of 1.

The coarse grid was deliberately not appropriate as to be the first mesh of a grid convergence study.

Thank you very much,
I will create the mesh again, run the simulation and let you know.

Spyros
Hi Spyros,

Thanks to your feedback we have detected a bug in the CGNS reader, could you please try again with the latest version in GitHub.
https://github.com/su2code/SU2

Cheers,
Francisco
fpalacios is offline   Reply With Quote

Old   June 6, 2014, 18:08
Default
  #11
New Member
 
Spyros
Join Date: Mar 2014
Posts: 15
Rep Power: 3
S.Kontogiannis is on a distinguished road
Dear Mr Palacio,

Thanks for the reply. Does this mean that the mesh was ok, but the problem was created from transforming the cgns file into su2 file? (or running the simulation with the cgns file?)

It is good if I help even implicetely with your development of the code!

Thank you very much,
Spyros
S.Kontogiannis is offline   Reply With Quote

Old   June 6, 2014, 18:47
Default
  #12
Super Moderator
 
Francisco Palacios
Join Date: Jan 2013
Location: Stanford, CA
Posts: 301
Rep Power: 5
fpalacios is on a distinguished road
Thanks Spyros,

Still my two previous comments apply… the coarse grid was too coarse, and be careful with the non-dimensionalization… it is based on the chord so you should use
REYNOLDS_LENGTH= 0.3048
or… change the chord to 1, and maintain REYNOLDS_LENGTH= 1.0 (this is probably the most intuitive solution).

Best,
Francisco
fpalacios is offline   Reply With Quote

Reply

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
combustion simulations from cmcPimpleFoam results openfoammaofnepo OpenFOAM 0 July 9, 2013 07:05
Solver for transonic flow? Martin Hegedus OpenFOAM 20 February 22, 2012 12:29
Bad Cd results applying k-ε models to hydrofoil spk FLUENT 1 December 10, 2011 09:27
How to do simulations for pressible flow Gaurav FLUENT 3 October 9, 2003 16:20
Total pressures; Transonic flow Louwrens CFX 9 April 19, 2003 18:01


All times are GMT -4. The time now is 19:44.