[S.Kontogiannis]

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 http://www.cfd-online.com/Forums/mai...tml#post492407)

[fpalacios]

Originally Posted by S.Kontogiannis

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 http://www.cfd-online.com/Forums/mai...tml#post492407)

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

[Martin Hegedus]

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]

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.

[S.Kontogiannis]

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

[fpalacios]

Could you please share the grid that you are using, we should like to take a look at it.

Cheers,
Francisco

[S.Kontogiannis]

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

[fpalacios]

Originally Posted by S.Kontogiannis

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

[S.Kontogiannis]

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

[fpalacios]

Originally Posted by S.Kontogiannis

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

[S.Kontogiannis]

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

[fpalacios]

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

[msahin.ae00]

I have just uploaded the RAE2822 airfoil geometry from UICC web site and AGARD-AR-138 report and the meshes at \TestCases-6.2.0.tar\TestCases-6.2.0\rans\rae2822\ don't coincide with these geometries.