[lejonetfrannorden]

Hello everyone,

I am a newbie in SU2. I created an airfoil mesh in 2D without a problem in coordinate axes (e.g. Normal and Axial directions). Then I set the Freesream velocity equal to (39.780000, 4.180000, 0.000000) which results in 6 degrees of angle of attack as expected.

Definition of my coordinate axes are as follows in Pointwise:
x-axis: parallel to chordline, downstream direction
y-axis: normal to chordline, lift direction
z-axis: port side of the wing
They form a right handed coordinate system.


However, when I use the same freestream velocity in the SU2 config file, SU2 interprets this as 6 degrees of sideslip angle. I am very confused about this topic, and hope you guys can enlighten me!
Hence I guess due to this sideslip angle I get very low CL values such as 0.007. Does this indicate that there really is a sideslip and no angle of attack? I have NACA0015 with AR=1 and c=1 m, due to symmetry there should be little to none lift at zero degrees of angle of attack. Additionally, I am in an early phase of the solution (~1100 iterations) should I expect dramatic changes in CL then?

Regards,
LejonetFranNorden

[LaurentvdB]

What kind of simulation are you doing (RANS/Euler/Compressible/Incompressible/?)? Is your SU2 mesh 2D or 3D?

In case of compressible flow, there is a parameter AOA (Angle of Attack) that you can use to directly set the angle. I am not sure whether the compressible solver uses the FREESTREAM_VELOCITY at all (see config_template.cfg in the root folder).

[lejonetfrannorden]

Originally Posted by LaurentvdB

What kind of simulation are you doing (RANS/Euler/Compressible/Incompressible/?)? Is your SU2 mesh 2D or 3D?

In case of compressible flow, there is a parameter AOA (Angle of Attack) that you can use to directly set the angle. I am not sure whether the compressible solver uses the FREESTREAM_VELOCITY at all (see config_template.cfg in the root folder).

Hello Laurent,

Sorry, I was not clear enough. My mesh is 3D and I am using incompressible solver with RANS - SA turbulence model, hence the freestream velocity. I do not experience the aformentioned problem in 2D case.

Regards,
LejonetFranNorden

[hlk]

From your description, I'm not sure if you mean that it is printing out text saying that the sideslip is 6 degrees, or if the resulting velocity vectors have a sideslip angle in the resulting volume solution. If the former, it sounds like you probably have it set up correctly and it's just a terminology difference.


The assumed coordinate system for wings has the y direction pointing along the span ("port" in your description), with the z direction up and the x in the streamwise direction. This is an industry convention, it's pretty much arbitrary (like how sometimes we joke that the 0th law of fluid dynamics is that flow goes from left to right).



Since the code has no way of differentiating what orientation your wing is in, or even that it is a wing, the print-out of whether it is a sideslip or angle of attack is likely based on the standard aviation coordinate system, which would assume that the 2nd coordinate is along the direction of the wing span. This would not effect the eventual volume solution, just which word is used in the text output.



If this is what the problem is, then your Cl, Cd, and Csideforce will be correspondingly flipped around to different axes.

Note that if the reference area is being automatically computed, it is the projection in the z axis for 3D geometries, so to get the correct nondimensionalization for lift/drag coefficients you will need to either input the reference area manually or reorient your mesh.