[nomad]

Hi,
I'm trying to calculate forces on a symmetric airfoil. I've set lref to the chord length and Aref to the reference area based on the span (these have been converted from imperial to metric units). I also have two separate patches, one for the top surface and one for the lower surface.
However, i get high Cl values (which should be zero) and Cd values that don't really make sense. here's my last time step:

Time = 2

DILUPBiCG: Solving for Ux, Initial residual = 0.0209504, Final residual = 2.13957e-07, No Iterations 9
DILUPBiCG: Solving for Uy, Initial residual = 0.0586488, Final residual = 3.39781e-07, No Iterations 9
DILUPBiCG: Solving for Uz, Initial residual = 0.0873523, Final residual = 4.68623e-07, No Iterations 9
DICPCG: Solving for p, Initial residual = 0.213432, Final residual = 9.62741e-10, No Iterations 296
DICPCG: Solving for p, Initial residual = 0.368842, Final residual = 9.65877e-10, No Iterations 284
DICPCG: Solving for p, Initial residual = 0.118823, Final residual = 9.0931e-10, No Iterations 278
DICPCG: Solving for p, Initial residual = 0.0732968, Final residual = 9.25933e-10, No Iterations 258
time step continuity errors : sum local = 6.07097e-11, global = 5.91392e-19, cumulative = 2.59606e-18
smoothSolver: Solving for nuTilda, Initial residual = 0.0120958, Final residual = 0.00101485, No Iterations 2
ExecutionTime = 23.62 s ClockTime = 31 s

forces output:
forces(pressure, viscous)((-8026.46 0 0) (11.1053 -7.92581 -8.84242))
moment(pressure, viscous)((0 -10186.1 112963) (974.88 -3443.99 426.025))

forces output:
forces(pressure, viscous)((-1910.11 0 0) (1.60656 0.792914 21.378))
moment(pressure, viscous)((0 -2420.21 -39146.1) (-301.654 -1457.53 38.3032))

forceCoeffs output:
Cd = -1308.63
Cl = -1.29401
Cm = 0

forceCoeffs output:
Cd = -12267.4
Cl = 5.09667
Cm = -0

End


Any help would be highly appreciated.
Thanks.

[hansel]

I was doing some experiments on a cylinder and getting forces that were in the wrong direction. Then I made my mesh finer (I went from 1cm to 3mm) and it completely changed the forces.

I was thinking since the cylinder was 1m in diameter I didn't need such a fine mesh, but the boundary layer is on the order of 7mm so I guess even with big objects you need a fine mesh. I'm using icoFoam. Maybe turbFoam would be more forgiving.

[hansel]

By the way, even with the finer mesh I have not managed to get results that agree with what the text books say the drag on a cylinder should be.

[walex]

Hi,

I have the same problems. I made simulations of a NACA64-418 and a NACA0012 airfoil (simpleFOAM and turbFOAM). Each for different angles of attack. CL is always to high. Around 4.4 till 4.9 times too high to be precisely. In case of the NACA64-418 it is strange that the cp plot is nearly the same like from another CFD solver we use. I have not checked it for the NACA0012 yet. As the cp distribution is the same lift should also be the same. Therefore something must be wrong with the forces determination. I really dont know where this problem comes from.

The drag problem could maybe occur because of the slowly development of k and epsilon. Even after 8000 iteration my absolute k values are comparable to other results but k decreases very fast going away from the wall (TM: LienCubicKELowRe). This definitely will lead to wrong drag results. But it does not explain the wrong CL results.

Regards
Alex

[hansel]

Walex, if you make any progress please post what you did here. What are you using for your transport properties? This is what I'm using, do these look right for air?

transportModel Newtonian;

nu nu [0 2 -1 0 0 0 0] 1.5E-5;


CrossPowerLawCoeffs
{
nu0 nu0 [0 2 -1 0 0 0 0] 1e-06;
nuInf nuInf [0 2 -1 0 0 0 0] 1e-06;
m m [0 0 1 0 0 0 0] 1;
n n [0 0 0 0 0 0 0] 1;
}

BirdCarreauCoeffs
{
nu0 nu0 [0 2 -1 0 0 0 0] 1e-06;
nuInf nuInf [0 2 -1 0 0 0 0] 1e-06;
k k [0 0 1 0 0 0 0] 0;
n n [0 0 0 0 0 0 0] 1;
}

RAS Properties:
RASModel kEpsilon;

turbulence on;

printCoeffs on;

laminarCoeffs
{
}

kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
alphaEps 0.76923;
}

RNGkEpsilonCoeffs
{
Cmu 0.0845;
C1 1.42;
C2 1.68;
alphak 1.39;
alphaEps 1.39;
eta0 4.38;
beta 0.012;
}

realizableKECoeffs
{
Cmu 0.09;
A0 4.0;
C2 1.9;
alphak 1;
alphaEps 0.833333;
}

kOmegaSSTCoeffs
{
alphaK1 0.85034;
alphaK2 1.0;
alphaOmega1 0.5;
alphaOmega2 0.85616;
gamma1 0.5532;
gamma2 0.4403;
beta1 0.0750;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
c1 10;

Cmu 0.09;
}

NonlinearKEShihCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
alphak 1;
alphaEps 0.76932;
A1 1.25;
A2 1000;
Ctau1 -4;
Ctau2 13;
Ctau3 -2;
alphaKsi 0.9;
}

LienCubicKECoeffs
{
C1 1.44;
C2 1.92;
alphak 1;
alphaEps 0.76923;
A1 1.25;
A2 1000;
Ctau1 -4;
Ctau2 13;
Ctau3 -2;
alphaKsi 0.9;
}

QZetaCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
alphaZeta 0.76923;
anisotropic no;
}

LaunderSharmaKECoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
alphaEps 0.76923;
}

LamBremhorstKECoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
alphaEps 0.76923;
}

LienCubicKELowReCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
alphak 1;
alphaEps 0.76923;
A1 1.25;
A2 1000;
Ctau1 -4;
Ctau2 13;
Ctau3 -2;
alphaKsi 0.9;
Am 0.016;
Aepsilon 0.263;
Amu 0.00222;
}

LienLeschzinerLowReCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
alphak 1;
alphaEps 0.76923;
Am 0.016;
Aepsilon 0.263;
Amu 0.00222;
}

LRRCoeffs
{
Cmu 0.09;
Clrr1 1.8;
Clrr2 0.6;
C1 1.44;
C2 1.92;
Cs 0.25;
Ceps 0.15;
alphaEps 0.76923;
}

LaunderGibsonRSTMCoeffs
{
Cmu 0.09;
Clg1 1.8;
Clg2 0.6;
C1 1.44;
C2 1.92;
C1Ref 0.5;
C2Ref 0.3;
Cs 0.25;
Ceps 0.15;
alphaEps 0.76923;
alphaR 1.22;
}

SpalartAllmarasCoeffs
{
alphaNut 1.5;
Cb1 0.1355;
Cb2 0.622;
Cw2 0.3;
Cw3 2;
Cv1 7.1;
Cv2 5.0;
}

wallFunctionCoeffs
{
kappa 0.4187;
E 9;
}

[walex]

Hi Steve,

nu looks good for air. Of course it depends on your temperature. For T=288.15K nu is 1.46e-05. But I never played with the CrossPowerLawCoeffs and the BirdCarreauCoeffs. In my case they are all set to zero. What's your opinion/experience?

Looking on your turbulence model I would suggest that you use the standard settings. But remember that the k-epsilon model implemented in OF is a highRe model. That means it uses wall functions to simulate the boundary layer. For an accurate simulation I would recommend a lowRe model. But this depends on what you are interested in.

Alex

[hansel]

Thanks for the reply. Just before you replied I found that I was using the high Re model. Since my wings are only 10cm across and the air is 6m/s I think I'm definitely should be using the low Re model. I'm trying the LaunderSharmaKE now. I have no experience in this. I'm an EE who just wanted to simulate wind turbines. I've learned more about fluid dynamics in the last 4 months than I ever knew even existed. :-)

[walex]

HI Steve,

low Reynoldsnumber model does not mean that your Reynoldsnumber based on the chord lenght is low. It means that the Re number based on the height of your first cell row in your boundary layer should be low. So for lowRe models your yplus should be 1 and for highRe models it should larger than 30 I think.

Which values for k and epsilon do you use? In case of the lowRe model is was said somewhere here in the forum that it should be set to 10e-05 to reach convergence.

[hansel]

Originally Posted by walex

HI Steve,

low Reynoldsnumber model does not mean that your Reynoldsnumber based on the chord lenght is low. It means that the Re number based on the height of your first cell row in your boundary layer should be low. So for lowRe models your yplus should be 1 and for highRe models it should larger than 30 I think.

Which values for k and epsilon do you use? In case of the lowRe model is was said somewhere here in the forum that it should be set to 10e-05 to reach convergence.

Thanks Walex, you seem to be onto something here. I changed my initial value of K from .017 to .00017 and it came out completely different. In fact now the drag is too low and the K settled out in most areas at 1E-9.

It seems that it's not right to have a value so dependent on only it's initial conditions? Should I have k fixed at my inlet or at a wall? What's a reasonable number for k or the wind? Do I need to do the same thing with epsilon or is that driven by K?

Thanks for the help.

[walex]

Steve,

how many iterations did you run? In my opinion k and epsilon should settle at reasonable results independend from your initial conditions as long as your simulation converges.

Alex

[jploz]

Hi,

yes, you should set k and epsilon to a fixed value at your inlet since this are properties of the incoming fluid. The values depend on your environmental conditions. Look for 'turbulence parameters' in the cfd wiki. In general, k is the turbulent kinetic energy and can be calculating from the turbulence intensity of the incoming fluid. When isotropic turbulence is assumed k can be calculated by k=3/2(I*mag(u))^2 where I is the turbulence intensity. Values from 0.01 to 0.1 for I (according to 1% .. 10% turbulence intesity) are typical but this depends on your case. For strong wind a higher value is maybe suitable. Epsilon is the dissipation rate and is related to the turbulence model you use and the length scale of the turbulence.

HTH,
Jean-Peer

[hansel]

Originally Posted by walex

Steve,

how many iterations did you run? In my opinion k and epsilon should settle at reasonable results independend from your initial conditions as long as your simulation converges.

Alex

I'm keeping the courant number < 0.2. This means I'm using about 0.1ms steps and I let the simulation run for about 2 seconds. I guess that's approximately 20,000 iterations.

[walex]

Instead of taking very small values for k and epsilon you could also determine them by following equations:

k/U^2 = 1*10^-6 -------> Tu=0.08%

epsilon*c/U^3 = 4.5*10^-7

nut/nu=0.2 for Re=10^6

I am testing these settings right now and the simulation is at least stable.

BTW: Is there anyone who can help you with the mesh? Maybe there is a problem, too.

Alex

[walex]

Hi,

just read something about an tutorial in OF for a 2D airfoil called airFoil2D. Does anybody know where it can be downloaded? It is not part of my OF installation.

Thanks
Alex