Sanity check of NACA 0012 gives wrong coefficient of lift

[BobHope]

Hi,

I am trying to teach myself to use CDdOF for aerodynamic design of remote piloted aircraft.

I am trying to validate my knowledge by creating a wind tunnel in which I can reproduce the NACA 0012 wing study and obtain accurate numbers for total lift, Cl, Cd, drag, etc from it.

My sanity check of NACA 0012 gives wrong coefficient of lift ( solves out to around 2.0 instead of 1.0 )

I picked NACA 0012 as it is a well studied aerofoil and there are pre existing simulations and NASA studies.

The example I picked was this one : https://help.sim-flow.com/validation/naca-0012-airfoil

A NACA 0012 at 10 degrees angle of attack. 1m chord.

Airflow at 52 M/S pressure at 101325 PA

As my work will deal with non symmetrical 3d objects, and I hope to to progress to building a more complicated model in an accurate wind tunnel, my test case is a complete wing in a 3D space. I do appreciate that this will alter the accuracy somewhat, and that building a 2D or symmetrical model would be faster, however my aim with this model is not the nth degree of accuracy or to validate the physics model, but rather to see if it is possible to build a test space in which I can get real world approximating results on a model - so within 10% is probably acceptable.

After reading a lot of tutorials and videos, I finally managed to produce something that seems like it should work :

I built a 1m chord wing 5M in length and placed in in a cube with a boolean XOR

I setup the inlet as uniform 52 M/S

Outlets are top and bottom and back of box with static pressure.

Sides of the tunnel as walls slip inviscid

Fluid to air.

PhysicsModel to steady, Single phase, incompressible, RANS model kOmegaSST ( I tried SpalartAllmaras as it says its designed for aerofoils and it did not seem to resolve )

There were a number of places in the setup I felt I did not have complete knowledge :
The CFD reporting function asks for reference pressure, I set this to 101325PA, and the freestream flow speed I did not fully understand, I set this to 52 M/S - matching my inlet speed.

However, when I run the Solver, the Freecad reports for Cl give a result of around 2.0 and the test report is 1.0.

I tried to refine the mesh over a few interations- however this did not seem to be having much of an effect, the solver still comes out at around Cl 2.0. I am not much of a mesh export , so I could be making an error here.

Could someone please take look at my windtunnel and advise if I have made an error or wrong assumption ?

I have seen references in the forums to the Freecad reports being incorrect - is this a known issue ?

An observation : the curling turbulent flow around the wingtips seems to be a real problem for the solvers and making the windtunnel longer seems to make it worse.

[BobHope]

NACA wingtip vortex.png (464.24 KiB) Viewed 2285 times

Naca 0012 test data.png (67.29 KiB) Viewed 2285 times

[BobHope]

I spotted a problem in my original file, the box for the windtunnel was rotated, not the part. I have sorted it so the wing is rotated and not the box.

I improved my boundary layer on the mesh to 150mm.

Added the forces to my case

Code: Select all

forces_all
    {
    type forces;
    libs ( "libforces.so" );
    patches
    (
    Wing002
    );
    rho rhoInf;
    rhoInf 1.2;
    log off;
    writeControl timeStep;
    writeInterval 1;
    CofR ( 0 0 0 );
}

however, it seems to be solving out at around the same value of 2.0

I will post the new file once I finish the simulation.

[BobHope]

1m chord wing 10 degrees improved fine mesh and rotation simulation converges mesh removed.FCStd

(112.23 KiB) Downloaded 47 times

Improved file

Simulation Residuals.png (206.4 KiB) Viewed 2210 times

force coefficients.png (27.12 KiB) Viewed 2210 times

force.png (34.84 KiB) Viewed 2210 times

[BobHope]

2D pressure slice.png (253.96 KiB) Viewed 2200 times

[BobHope]

Checking the file from lift and drag around a car, I see differences in my model.


To match that simulation I changed Inlet pressure to 0PA and Changed the initalise section from a set pressure to Potential Flow and Kinetic Values I copied from the lift and drag model.

Running the simulation now.

values from car simulation.png (40.71 KiB) Viewed 2173 times

[thschrader]

Here is a test case:

naca2412_2DplanarMesh.FCStd

(400.84 KiB) Downloaded 57 times

See also
https://forum.freecadweb.org/viewtopic. ... 12#p622724

and
http://www.ae.metu.edu.tr/tuncer/ae443/ ... All-Re.pdf

Thomas

[BobHope]

Hi Thomas,
Thanks for your tutorials, they have been very useful indeed.

However I don't see the force coefficient report in the examples. Is this a new feature ?

I thought I would try to add the force coefficient to your NACA 241_2d Planer mesh file.

I searched but could not find an explanation for the Free stream flow speed and and reference length.

They seem to be critical values :

The 55ms Value gave a 0.14 Cl
The 14 m/s value gave 6.5 Cl close to the reference 0.6 from the data - however I guessed that value I did not calculate it.

Freestream 14ms.png (230.75 KiB) Viewed 2048 times

[thschrader]

I ran your file with 33,4 m/s inlet speed, to match the Re-value in the NACA-report.
With the 100 mm base-mesh the p-residuals starts to vibrate a little, so I used a 50 mm base mesh.
Runtime approx 40 min on intel i7 all cpus. Convergence to 0,0001 after 2000 iterations.
Mesh-thickness is still 50 mm. AoA of wing is 4 degrees.

With the forces plot I get F-lift=29 N, F-drag=0,6 N, wich gives
c-lift=0,62
c-drag=0,013
This is equal to the NACA-investigation.
Nice, isnt it?

Every time you change the inlet-speed you must adjust the reference pressure and free-stream flow speed
to get the correct forces/coefficients.
Have a nice Christmas,
Thomas

file:

naca2412_BH.FCStd

(402.28 KiB) Downloaded 53 times

naca_report.JPG (121.59 KiB) Viewed 1969 times

forces_coefficients.JPG (60.85 KiB) Viewed 1969 times

[BobHope]

Thanks Thomas, these values finally start to make sense, very useful.