[gtg627e]

Hello everybody,

I am running some validation cases for a naca0012 at low angle of attack using simpleFoam and k-epsilon turbulence model. Airfoil chord 1 m, inlet velocity 50 m/s, free-stream viscosity 1.7894e-5.

I noticed that if I compile the liftDrag.C version from Vincent RIVOLA on Wednesday, September 19, 2007 - 09:36 am the results are quite good (if I multiply by density).

However, I tried using liftDrag.C posted by Vincent RIVOLA on Thursday, September 20, 2007 - 03:47 am and I get a drag coefficient which is 4 orders of magnitude lower.

I am checking these two files. I will keep you updated.

Thank you,

Alessandro

[gtg627e]

Sorry, I see you have to pass in Aref.

Howver comparing "Vincent RIVOLA on Wednesday, September 19, 2007 - 09:36 am" with "Vincent RIVOLA on Thursday, September 20, 2007 - 03:47 am " it seems like the values of turbulent and laminar drag coefficients get swapped.

Alessandro

[gtg627e]

Hello everybody,


using liftDrag.C from "Vincent RIVOLA on Wednesday, September 19, 2007 - 09:36 am" and my airfoil at 0-deg angle of attack I get:

total Turbulent drag coefficient: 0.00034
total laminar drag coefficient: 0.00116

which I cannot explain. Even if I multiply my density, say 1.225, the total drag is way too low, as it should be ~~ 0.0058 from "theory of wing sections".

I changed liftDrac.C as suggsted by " Rosario Russo on Monday, September 24, 2007 - 09:32 am" and now I get:

total Turbulent drag coefficient: 0.00198
total laminar drag coefficient: 0.001161


Still way off.
I will re-run my case with better schemes.

Any comments?

Thank you,

Alessandro

[gtg627e]

Ok, I give up.

Using the same mesh in fluent I get a drag coefficient of 0.0052 which is 10% away from the experimental value in "theory of wing sections."

OpenFoam gives me 0.00314.

Please help

Alessandro

[vinz]

Hi Alessandro,

I'm also interested in your computations since, I am still not sure that the liftDrag utility is computing the drag correctly.
To really compare the values from OpenFOAM and Fluent, I think it would be interesting to compare the Cp values found in fluent to the ones found in OpenFOAM. If these values are the same, the problem is coming from the liftdrag utility.
Otherwise, the problem is coming from the computation. The same can be done by comparing velocity fields.

Hope that helps.
Regards,

Vincent

[msrinath80]

liftDrag area calculation for force computation is non-trivial. Please make sure that if you are working on a 2D case, the domain length in the third direction is reasonable. See Hrv's comment here to follow what I'm referring to --> http://www.cfd-online.com/OpenFOAM_D...es/1/2726.html

[vinz]

Hi everybody,

I now manage to get some interesting results on Ahmed test case and on a real race car.
Pressure and velocity fields look not so bad and some vortices can be observed in some particular regions.
However I still have some doubts on my way to compute lift and drag coeffcients. Drag coefficient looks ok actually, for the ahmed body and for the race car as well.
But the lift coefficient is far from the results I should have.
By reading again this topic I see that some questions stayed without answer. Especially the doubts about the way to compute turbulent part.

Could someone point out what is actually the best liftDrag tool which could be used with simpleFoam?

Regards,

Vincent

[morfeus80]

Hi Vincent,
I ran a Ahmed body case with 4M cells for half car in SimpleFoam, but the results I managed weren't so good: the pressure and velocity fields were quite different from experimental data.
Can you describe what models and solvers you used, please?

[ceyrows]

Hey Mattia,

which slant angle did you run? Turbulence modelling is not capable for getting the correct results with 25°. Additionally the flow around the 25°-case is very instationary so simpleFoam has got some converging problems (at least in my calculations).
Apart from that the 35°-results with simpleFoam were pretty good, because the flow has got a stable character. I had positive experiences with the Realizable-k-epsilon model and the limitedLinear TVD-Interpolation.

Best regards,

Thomas

[louisgag]

Hi all,

I have been doing some Ahmed body drag and lift calculations and although I often get ok results for the drag coefficients, the lift coefficients I get are always in the range of 3-4.. Which is about 10 times too large.

I am working in 2D with simpleFoam and RealizableKE, komegaSST, and SA models.

Has anyone experienced difficulties with computing the lift? I would appreciate some pointers!

Thank you,

-Louis

[madad2005]

From reading some articles, it seems a few people have. How are you calculating the lift coefficient?

[louisgag]

Hi Adriano,

I use the forceCoefficients function included in OF 1.5. Also, I verify the results obtained from that with the patchIntegrate on pressure and I get values that correspond (viscous lift excluded) to what forceCoefficients gives.

Aref= frontal projected area

I assume there is something wrong in my pressure field but I find strange that drag forces are still reasonable.

Have a good day,

-Louis

[madad2005]

What is your frontal area value? What are your minimum values of surface pressure on the upper surface? Have you tried looking at the velocity fields and comparing it to the experimental data?

[louisgag]

Aref=0.00288 (my mesh is 0.01 m thick); min pressure on upper surface is [-1.5,-2.08] (the lowest pressure is proportional to the drag coefficient I get); and my velocity fields look somewhat like the experimental data: two recirculation zones at the vertical back plane (and on the slant plane when slant angle is large enough), very thin B.L. on top surface, acceleration zone on the top leading edge.
The acceleration zone on the leading edge goes all the way to the wall of the vehicle and the velocity is >1 until it reaches the wall where it suddenly becomes 0.

(Longitudinal vortices are excluded since Im in 2D).

Also, another strange trend I noticed is that when drag is overestimated, the value of lift reduces (usually not enough to get appropriate results and the trend is not always respected).

thanks for your help! (I am doing this project for my Master's thesis)

-Louis

[madad2005]

Is that your minimum pressre coefficient? The velocity at the wall should be zero due to the no-slip condition.

Do all your results converge ok? If so, how long do you run them for? Finally, what is the first wall spacing you are using (or y+ would be better)?

-Adriano

[louisgag]

the [-1.5,-2.08] is actually the pressure "p" value (using a 0 reference pressure), so I assume it is in (Pa *m^3/kg). ( I wrote lowest upper surface pressure proportional to drag coefficient but I meant lowest upper surface pressure proportional to lift coefficient...)

I use the no-slip condition (fixedValue velocity, value = uniform 0 on the vehicle wall) and still get velocity >1 on the cell/point next to the wall; also, pressure is zeroGradient on the vehicle wall.

My results converge very well, except in a few rare cases.

As for my y+ value, it is not consistent through the whole wall and I have a hard time getting it outsite of the "intertide" zone of 1<yplus<30. (Allthough Im not sure this is an issue with models other than SA)

Here are a few Yplus values I get:

min: 6.9669 max: 90.5637 average: 59.6992 (SA)
min: 0.418455 max: 18.4831 average: 8.81904 (SA)
min: 12.8556 max: 334.043 average: 155.761 (RKE)
min: 12.0163 max: 301.83 average: 144.64 (RKE)

Also, convergence is not a good (or maybe just very slow) when I try to lower my value of Yplus by refinement at the wall.

min: 0.128637 max: 18.1411 average: 6.55086 (komegaSST, with pretty fine mesh)


Have a good day!

-Louis

[louisgag]

Forgot to add...

It is my minimum pressure, yes.

And i run the calculation until drag is constant (at least to the 10^-4), when possible; at that point there are no more iterations per "timestep" on velocities and sometimes 1 on pressure. (Thats usually 20000-30000 iterations.

But again, with the smaller y+ it is not as obvious to run the simulations until convergence!

Also, concerning the velocity field, the velocity near the bottom leading edge of the vehicle lower than on the upper leading edge.

-Louis

[louisgag]

Hi Adriano,

Do you have any hints to help me get better lift coefficients?

I am currently trying to see if changing the bottom surface to a fixed one, as in the experiments, will help. So far my results still have a very high lift coefficient.

regards,

-Louis

[madad2005]

Hi Louis,

What boundary condition did you apply to the lower surface wall previously?

If possible, would you be able to e-mail me your mesh and I can run it myself and take a look at it?

In the meantime, I'd try, if possible, to get a mesh with a y+ of between 30 (abs. min) and 300 and re-run with the k-e model, and have a look at the results. It will give you a better idea before you attempt a more challenging y+=1 mesh.