[jferrari]

I'm looking to model a NACA0012 airfoil using simpleFOAM. Abbot and Von Doenhoff (p462) report a lift coefficient of about 0.9 and a drag coefficient of about 0.01. I am calculating a lift coefficient of 0.710 and a drag coefficient of 0.0242 - values that are significantly off, especially the drag. I get the same results when I double the cells in the x and y directions. My y+ on the finer of the two meshes is about 6.5. I'm not really sure what to look for to debug this - can anyone point me in the right direction?

[kid]

Hi,
Which turbulence model are you using?
And what are the values of epslion and k you have used if using RANs?

NOTE: pasting the patch of epslion and k would give a clear idea.

Regards
CFDkid

[jferrari]

Thanks for the reply CFDkid. I'm using the Spalart-Allmaras turbulence model, so I'm specifying boundary conditions for nuTilda and nut.


My nut boundary conditions are:
boundaryField
{
frontAndBack
{
type empty;
}

topAndBottom
{
type advective;
}

left
{
type inletOutlet;
inletValue uniform 1e-06;
}

right
{
type advective;
}

airfoil
{
type nutUSpaldingWallFunction;
value uniform 1e-10;
}
}

nuTilda:

boundaryField
{
frontAndBack
{
type empty;
}

topAndBottom
{
type advective;
}

left
{
type inletOutlet;
inletValue uniform 3e-06;
}

right
{
type advective;
}

airfoil
{
type nutUSpaldingWallFunction;
value uniform 1e-10;
}
}

pressure:

boundaryField
{
frontAndBack
{
type empty;
}

topAndBottom
{
type outletInlet;
outletValue uniform 0;
}

left
{
type outletInlet;
outletValue uniform 0;
}

right
{
type outletInlet;
outletValue uniform 0;
}

airfoil
{
type zeroGradient;
}
}

velocity:

boundaryField
{
topAndBottom
{
type inletOutlet;
inletValue uniform (29.7081 4.1751 0);
}

frontAndBack
{
type empty;
}

left
{
type inletOutlet;
inletValue uniform (29.7081 4.1751 0);
}

right
{
type inletOutlet;
inletValue uniform (29.7081 4.1751 0);
}

airfoil
{
type fixedValue;
value uniform (0 0 0);
}
}

[jferrari]

http://www.cfd-online.com/Forums/ope...-get-help.html


Just saw this thread. When I get home this evening I'll post everything to do with my case.

[jferrari]

CheckMesh output: http://dl.dropbox.com/u/62138912/checkMeshLog
fvSchemes: http://dl.dropbox.com/u/62138912/fvSchemes
fvSolution: http://dl.dropbox.com/u/62138912/fvSolution


Complete mesh:


Zoomed in some:


I'm a bit concerned about this - the gridlines aren't really normal to the surface and I'm getting cells with very large aspect ratios near the surface.



Thanks again.

[jferrari]

Long story short - I was looking at a NACA 0020 airfoil and comparing the results to those published for a NACA 0012 airfoil. I'm very embarassed by this. My advisor made me aware of this yesterday evening. I will rerun with the correct geometry this afternoon.

[kid]

Hello,
Can you share the NACA0012 paper with me. I was doing NACA4412, the one validation study that comes with Fluent.
https://confluence.cornell.edu/displ...ver+an+Airfoil

But it would be better doing NACA0012.
Please help regarding the resources to carry out this study.

Regards
CFDkid

[jferrari]

Can you share the NACA0012 paper with me

I'm comparing to Abbot and Von Doenhoff's Theory of Wing Sections (page 462-463, reproduced below).




After fixing my geometry (NACA 0012 vs 0020), I reran under the same conditions. I'm calculating lift that's slightly higher, but my drag is still double what it should be. I may still have something fishy going on with my mesh - I'm using a rounded trailing edge who's radius looks to be too large, so my trailing edge isn't tangent to the rest of the airfoil. I would expect this to cause my drag to increase, but would this make it double what it should be?

[mihaipruna]

I have a similar problem, I am trying to analyze the NACA 5012 airfoil and getting a Cl of 0.52 at 0 degrees AOA and 15 at 5 degrees AOA! I am hoping that with the low airspeed we are still in the laminar regime.

Here are my forcecoeffs


Airfoil 5 degree:

forces
{
type forceCoeffs;
functionObjectLibs ( "libforces.so" );
outputControl timeStep;
outputInterval 1;
patches (
"vol1face1"
"vol1face2"
"vol1face3"
"vol1face4"
);
pName p;
UName U;
rhoName rhoInf; // Indicates incompressible
log true;
rhoInf 1; // Redundant for incompressible
liftDir (-0.087 0.996 0);
dragDir (0.996 0.087 0);
CofR (0.72 0 0); // Axle midpoint on ground
pitchAxis (0 0 1);
magUInf 20.0;
lRef 1.0;
Aref 10.0;
}


0 degrees:

forces
{
type forceCoeffs;
functionObjectLibs ( "libforces.so" );
outputControl timeStep;
outputInterval 1;
patches (
"vol1face1"
"vol1face2"
"vol1face3"
"vol1face4"
);
pName p;
UName U;
rhoName rhoInf; // Indicates incompressible
log true;
rhoInf 1; // Redundant for incompressible
liftDir (0 1 0);
dragDir (1 0 0);
CofR (0.72 0 0); // Axle midpoint on ground
pitchAxis (0 0 1);
magUInf 20.0;
lRef 1.00;
Aref 10.0;
}

[jferrari]

Mikhail, the first thing to catch my attention is that you are looking at a 5012 airfoil. This could just be a typo, but if your point of maximum camber is at your leading edge that would be an awkward airfoil. What kinematic viscosity are you using? I see you have a reference length of 1 and reference area of 10. From this is see that your chord is 1 m and your span (even if this is 2D) is 10 m. Is this the case in your geometry? If not this could cause your results to off by an order of magnitude. Also, one of your notes States that the density is not needed for incompressible flow - I'm not sure if this is true because to get the lift and drag coefficients you would need to get the force then divide by the area (like I mentioned earlier) and the dynamic pressure (where density shows up).


Forgive any grammatical errors, I'm typing on my cell phone so it's tough to gather my thoughts properly. Also forgive if I'm flat out wrong, I'm still very new to openFOAM.

[kid]

Jferrari,
Thank you for sharing those plots. I came across this paper which seems to be good,
"Evaluation of the turbulence models for the simulation of the flow over a National Advisory Committee for Aeronautics (NACA) 0012 airfoil "
Douvi C. Eleni*, Tsavalos I. Athanasios and Margaris P. Dionissios

Would follow this to run a case. Also, i will look at your plots and get back with some results if possible.

Regards,
CFDkid

[vkrastev]

If you are interested in NACA0012 validation, just take a look at this:

http://turbmodels.larc.nasa.gov/naca0012_val.html

There you can find also some indications for useful experimental databases.

Regards

V.

[kid]

True, had gone to that site before. thanks even the paper we discussed have Aboot's experimental data. But yes the link of naca has around 4 to 5 experimental data, which is good.

Can you help me on how to calulate Lift Force and Drag Force . Which i suppose
could be implemented directly in OpenFOAM, but i do not no the implementation. How to
go about it?

Regards
CFDkid

[vkrastev]

Originally Posted by kid

True, had gone to that site before. thanks even the paper we discussed have Aboot's experimental data. But yes the link of naca has around 4 to 5 experimental data, which is good.

Can you help me on how to calulate Lift Force and Drag Force . Which i suppose
could be implemented directly in OpenFOAM, but i do not no the implementation. How to
go about it?

Regards
CFDkid

The calculation of aerodynamic forces or force coefficients in OF is quite straightforward. You just have to add at the end of your controlDict file something like this:

functions
{
totalDrag
{
// rhoInf - reference density
// CofR - Centre of rotation
// dragDir - Direction of drag coefficient
// liftDir - Direction of lift coefficient
// pitchAxis - Pitching moment axis
// magUinf - free stream velocity magnitude
// lRef - reference length
// Aref - reference area
type forceCoeffs;
functionObjectLibs ("libforces.so");
patches (nose body slant back);
rhoName rhoInf;
rhoInf 1.184;
CofR (0 0 0);
liftDir (0 1 0);
dragDir (1 0 0);
pitchAxis (0 0 1);
magUInf 40;
lRef 0.288;
Aref 0.0561;

outputControl timeStep;
outputInterval 50;
}
}

The above syntax allows the code to activate force coefficients calculation at run time and to print the values every 50 steps. The same syntax applies for the forces, but in that case the type should be forces instead of forceCoeffs. Just some additional details:

1) This EXACT syntax applies to the OF-1.7.x family: there could be some small formal differences for the 2.x.x releases which I'm not aware of;

2) For incompressible runs, the rhoInf value is used for absolute forces calculation (not for force coefficients), while for compressible runs you have to use the actual rho value (rhoName becomes rho)

3) For an airfoil, lref is the chord length, while Aref should be the actual spanwise section (remember that in OF 2D grids are physically 3D), which is the chord length multiplied by the grid width.

Hope this helps

V.

[mihaipruna]

Originally Posted by jferrari

Mikhail, the first thing to catch my attention is that you are looking at a 5012 airfoil. T

Hi Joe, I used the example here:
http://www.dur.ac.uk/g.l.ingram/down...ofoilGuide.pdf

I was assuming that since the static pressure is set to 0 and the flow is incompressible, the value of the density doesn't matter as it factors out.

Indeed,I have a 10m wing span and 1 m chord.

Thanks for the feedback.

I am mainly concerned about the discrepancy that a 5 degrees angle of attack seems to cause in Cl.

[vkrastev]

Originally Posted by mihaipruna

I was assuming that since the static pressure is set to 0 and the flow is incompressible, the value of the density doesn't matter as it factors out.
.

It doesn't matter for force coefficients (adimensional), as OF solves incompressible flows directly for p/rho, but it do matters if you need forces (dimensional).

Regards

V.

[mihaipruna]

Originally Posted by vkrastev

It doesn't matter for force coefficients (adimensional), as OF solves incompressible flows directly for p/rho, but it do matters if you need forces (dimensional).

Regards

V.

That is understood, and I'm only looking for a reasonably accurate Cl and Cd.

[jferrari]

Mihai, you mentioned that you were looking to stay in the laminar flow regime, but you're posting in this thread about simpleFoam. This is a turbulent solver. The laminar solver is icoFoam. Which solver are you using? What Reynolds number are you using? If you're using simpleFoam, what turbulence model are you using?

[kid]

Hi jferrari,

SimpleFOAM is turbulent solver, but we can use it for laminar flow calculation with little modification. One needs to edit RASProperties file and switch off turbulence (control/RASProperties).

icoFoam: Transient solver for incompressible, laminar flow of Newtonian fluids.( PISO algorithm)
simpleFoam: Steady-state solver for incompressible, turbulent flow. (SIMPLE algorithm).

Hope the difference is clear now.

regards,
CFDkid.

[kid]

Vesselin Krastev,
Thanks, will share results after i am done.

regards
CFDkid