[Arne Voß]

Hello everyone,

I would like to calculate an aircraft during pitch-up as a steady Euler simulation. Looking at the config template and some examples, I figured out the following parameters:

AOA= 0.0
GRID_MOVEMENT= ROTATING_FRAME
MOTION_ORIGIN= 4.83 0.0 0.0 <-- CG of the aircraft
ROTATION_RATE= 0.0 0.1 0.0 <-- pitch velocity q = 0.1 rad/s

Expected results: An induced velocity pointing downward at the aircraft nose and a upward velocity at the tail, linear changing in between with 0 induced velocity at the motion origin. The lift coefficient CL may change slightly comparing q=0.0 and q=0.1 but should stay close to Cl~=0.0 due to AoA=0.

What I get: When plotting the Grid_Velocity_xyz as vectors, everything looks as expected, see figure attached. BUT: the flow field does not correspond to the grid velocity. For example, I get a significant additional lift. Looking at the momentum_z, it looks like I have a rotation about the left side of the mesh instead of the center.

Where is my mistake or is this a bug?

I found a similar discussion from two years ago here: Rotating frame does not rotate about the center of rotation

[Arne Voß]

I testet the rolling motion as well: With a spherical farfield with radius of 200 m and p=0.1/rad/s, I would expect a flow velocity of +/-20m/s at the farfield. Again, the grid velocity vectors show the intended behavior, but for the flow quantities the distribution looks different and I get much smaller values, see figure attached.

Do you have any ideas?

Thank you very much in advance,
Arne Voß

[pcg]

As a quick sanity check can you try setting up the simulation with inlets and outlets?

[Arne Voß]

Hello Pedro,

thank you for your suggestion. I generated a mesh with the aircraft in a cylindrical control volume, see figure attached. The walls of the cylinder are euler walls (like the aircraft itself), for the inlet and the outlet I used the following parameters:
INLET_TYPE= MASS_FLOW
MARKER_INLET= ( in, 1.224999036598556, 136.118, 1.0, 0.0, 0.0 )
MARKER_OUTLET= ( out, 101325.0 )

For the rolling motion (I guess pitch makes no sense with the cylindrical control volume) I used the following parameters:
GRID_MOVEMENT= ROTATING_FRAME
MOTION_ORIGIN= 4.83 0.0 0.0
ROTATION_RATE= 0.1 0.0 0.0

The results look very similar compared to the approach with the farfield, see figure attached.

Do you have any ideas? To me it looks like the solver does not apply the grid velocity properly to the flow field... Is that possible?

Arne

[pcg]

In the rolling case that looks fine because SU2 solves on the absolute frame. To "see" the flow rotating you need to compute the velocity in the frame relative to the aircraft.

[Arne Voß]

Hi Pedro,

a) Here comes the pitching motion (q=0.1 rad/s) with inlet and outlet conditions. I used a spherical control volume with the front semi-sphere as inlet and the rear semi-sphere as outlet. However, the results are very similar compared to the farfield results in my first post, see figure attached. Also, the lift coefficient increases to CL=0.25, which shouldn't be the case.

b) I had a second look at the rolling motion: I can see a slightly asymmetrical pressure distribution comparing the left and right wing and the Cmx is close to what I get from a vortex lattice method.

c) From your last comment I understood that the rotational velocities are not included in the momentum / flow velocities. To me, this is confusing but I can live with that as long as the results are correct
BUT: Why is there a momentum / flow velocity in z-direction for the pitching motion?

Arne

[pcg]

Hi Arne,
I'm also more used to looking at relative velocities for moving frame simulations, but the transformation is fairly simple to apply in paraview.

If the results are similar with farfield and in/out that is good (I did not expect exactly the same due to backflow treatment) thanks for checking.

As I mentioned in the other thread I don't have a good feel for how to simulate a constant pitch rate.
Imagining that we were actually moving the domain, i.e. fixed observer, we would translate at the farfield speed and rotate at the pitch rate, which would make the aircraft loop around some point located at Uinf / q (far from the aircraft).
Now, the equivalent of this for a moving (with the plane) observer would be a rotating frame with origin at the center of the loop / circular trajectory described by the aircraft.

Let me stress again that I don't know if that is the right way of doing it, but somehow it feels closer to the real world than farfield + rotating about the CG.

[Arne Voß]

Hello Pedro,

as discussed yesterday, I tried to use only the rotational frame with the farfield mach number = 0.0. I am happy to say that the results look good to me - thank you for this suggestion!

However, I came across a new problem: When reading the nodal forces f_xyz on the surface via pysu2 and GetFlowLoad(), I now receive NaNs...

My first idea was that maybe the forces are calculated from the pressure coefficients, which show "strange" values in Tecplot, probably due to the division by V_inf. Can we fix that? I have no idea where to start looking...

Arne

[pcg]

Hi Arne,
I'm glad that seems to work. Yep... I can see why the forces could go wrong. Can you create a simple problem that reproduces this? Maybe a circle, with a python script for the python wrapper. If you open a github issue with that I can have a look.

The python wrapper tries to return dimensional forces (even if the simulation is nondimensional) and so the nans might be because of 0/0, in which case even a farfield Mach of 1e-9 would solve the problem.

[Arne Voß]

Pedro, If you could fix this, that would be great!

For anyone else reading/following this thread, I opened an issue here: https://github.com/su2code/SU2/issues/1588

Arne

[jdp810]

Hi Arne,

I just saw this

Originally Posted by Arne Voß

as discussed yesterday, I tried to use only the rotational frame with the farfield mach number = 0.0. I am happy to say that the results look good to me - thank you for this suggestion!

and it is a coincidence because I am having problems like the ones you are reporting. I am calculating the dynamic stability derivatives and they are too high as well. I'm right now trying to set the MACH_NUMBER option to 0.0 and the MACH_MOTION to the value that I want to see if the values are correct.

I'll let you know if it works for me too!

Thanks!

[jdp810]

Hi Arne,

Could you post the cfg file that worked for you for ROTATING_FRAME? I am still having a similar problem...

What I am seeing is that the farfield boundaries have zero velocity, even though the rest of the field has the velocity that is expected...

Thanks!

[pcg]

Hi Jose,
The extra detail is that you need to set the center of rotation away from the CG of the aircraft. Such that "radius x omega" gives you the grid velocity you want at the CG. This grid velocity defines the Mach number and AoA.
Then in postprocessing you'll want to plot "Momentum/Density - GridVelocity".