[robyTKD]

Hi developers,

I have a problem related to shape optimization(objective function DRAG and contraint on LIFT). After one step of optimization, the drag coefficient of modified airfoil is higher than the undeformed case. Attached below you can find the picture of the deformed surface.

I think this is caused by wrong shape sensitivities, actually, performing deformation following the gradients (the first with DRAG objective function, the second with LIFT), aerodynamics coefficients are not reduced as you can see:

• undeformed Cl = 1.0903975881, Cd = 0.0144672429
• deformed(DRAG) Cl = 1.0913637969, Cd = 0.0144798238
• deformed(LIFT) Cl = 1.0835264954, Cd = 0.0150110962

Configuration file and mesh: https://dl.dropboxusercontent.com/u/...ile%26Mesh.zip

[rktchip]

Originally Posted by robyTKD

Hi developers,
I have a problem related to shape optimization(objective function DRAG and contraint on LIFT).

Hi roby, can you please describe your shape optimization case? Makes it easier to interpret the config file..

[robyTKD]

Yes.

OPT_OBJECTIVE= DRAG*0.001

OPT_CONSTRAINT= ( LIFT>1.09 )*0.001

Design variables are Hicks-Henne function on top and bottom of the airfoil.

DEFINITION_DV= ( 1, 1.0 | AIRFOIL | 0, 0.05 ); ( 1, 1.0 | AIRFOIL | 0, 0.10 ); ( 1, 1.0 | AIRFOIL | 0, 0.15 ); ( 1, 1.0 | AIRFOIL | 0, 0.20 ); ( 1, 1.0 | AIRFOIL | 0, 0.25 ); ( 1, 1.0 | AIRFOIL | 0, 0.30 ); ( 1, 1.0 | AIRFOIL | 0, 0.35 ); ( 1, 1.0 | AIRFOIL | 0, 0.40 ); ( 1, 1.0 | AIRFOIL | 0, 0.45 ); ( 1, 1.0 | AIRFOIL | 0, 0.50 ); ( 1, 1.0 | AIRFOIL | 0, 0.55 ); ( 1, 1.0 | AIRFOIL | 0, 0.60 ); ( 1, 1.0 | AIRFOIL | 0, 0.65 ); ( 1, 1.0 | AIRFOIL | 0, 0.70 ); ( 1, 1.0 | AIRFOIL | 0, 0.75 ); ( 1, 1.0 | AIRFOIL | 0, 0.80 ); ( 1, 1.0 | AIRFOIL | 0, 0.85 ); ( 1, 1.0 | AIRFOIL | 0, 0.90 ); ( 1, 1.0 | AIRFOIL | 0, 0.95 ); ( 1, 1.0 | AIRFOIL | 1, 0.05 ); ( 1, 1.0 | AIRFOIL | 1, 0.10 ); ( 1, 1.0 | AIRFOIL | 1, 0.15 ); ( 1, 1.0 | AIRFOIL | 1, 0.20 ); ( 1, 1.0 | AIRFOIL | 1, 0.25 ); ( 1, 1.0 | AIRFOIL | 1, 0.30 ); ( 1, 1.0 | AIRFOIL | 1, 0.35 ); ( 1, 1.0 | AIRFOIL | 1, 0.40 ); ( 1, 1.0 | AIRFOIL | 1, 0.45 ); ( 1, 1.0 | AIRFOIL | 1, 0.50 ); ( 1, 1.0 | AIRFOIL | 1, 0.55 ); ( 1, 1.0 | AIRFOIL | 1, 0.60 ); ( 1, 1.0 | AIRFOIL | 1, 0.65 ); ( 1, 1.0 | AIRFOIL | 1, 0.70 ); ( 1, 1.0 | AIRFOIL | 1, 0.75 ); ( 1, 1.0 | AIRFOIL | 1, 0.80 ); ( 1, 1.0 | AIRFOIL | 1, 0.85 ); ( 1, 1.0 | AIRFOIL | 1, 0.90 ); ( 1, 1.0 | AIRFOIL | 1, 0.95 )

If you need somethin more just ask.

Roberto

[rktchip]

ah i meant more of the physical case. what conditions, geometry etc?

[robyTKD]

Airfoil NACA0012, Navier-Stokes with Spalart-Allmaras turbulence model.
Flow conditions are the following:

• M = 0.15
• Re = 6E6
• AoA = 10 deg
• T = 300 K

[economon]

Hi Roberto,

One thing we have seen in the past is that the ordering of the line elements making up the airfoil in the mesh file can be reversed (depends on the mesh generator, since there is no standard), and this causes the direction of the gradient/deformation to be reversed. One thing that you can try in order to fix this is to simply flip the connectivity in the mesh file for the airfoil marker. For example, if the first line element in the airfoil is

MARKER_TAG= airfoil
MARKER_ELEMS=200
3 199 0

try changing it to

MARKER_TAG= airfoil
MARKER_ELEMS=200
3 0 199

and perform this change for the rest of the line elements making up the airfoil marker as well. We will implement an automatic fix for this soon.

Hope this helps,
Tom

[robyTKD]

Thank you Tom, this seems to be one of the problems related to my "bad" shape optimization.
Elements on the airfoil were non-uniformly oriented, then a simply change of orientation was not enough. But giving them the same orientation things seems to work (in laminar regime).

I am trying to set the turbulent case on the new mesh to see if things work with the introduction of Spalart-Allmaras model.

I will post news as soon as possible.

Best regards,
Roberto

[hoyos98]

You can find the optimal airfoil shape (minimizing the drag) but fulfilling a target lift coefficient on this website: https://aeroptimal.com/airfoil . The methodology is under review in journals. The CFD method employs OpenFOAM.