CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Drag predicion for a NACA 0012 airfoil (http://www.cfd-online.com/Forums/fluent/33119-drag-predicion-naca-0012-airfoil.html)

 Peter Giannakopoulos February 25, 2004 19:57

Drag predicion for a NACA 0012 airfoil

I am trying for some time now to calculate the Cd and Cl for a NACA 0012 with FLUENT 6.0. It's an incompressible flow (M=0.15), Hi Re number, and results for Cd are poor at best!!!

I am using the Spalart-Allmaras model.

Has anybody ever managed to get any decent results with FLUENT????

Cheers

 Ugo February 26, 2004 06:09

Re: Drag predicion for a NACA 0012 airfoil

Could you provide me more informations on your problem setup? I need to know: 1) first cell height; 2) reference values; 3) BCs,wall treatment and so on... bye

 Peter Giannakopoulos February 26, 2004 10:44

Re: Drag predicion for a NACA 0012 airfoil

I am using my finest grid, C-type, hyperbolic, generated in GRIDGEN, about 90,000 cells, with a value of (y+)=1.

Reference values from the velocity inlet ( U=43.81m/s, density, pressure are the default)

Op. Conditions, Pressure=0, Temp=288.16K

I am using the Spalart-Allmaras model, with a Prandtl Number of 0.72.

Hope that helps!

Thanks for the fast response!!!

Cheers

 James Date February 26, 2004 14:40

Re: Drag predicion for a NACA 0012 airfoil

The usual things to check are; not specifically in this order mind:

1) Ensure the first grid point location is in correct Y+ range

2) Make sure you have enough cells to resolve the boundary layer above the first grid point location

3) Make sure the wake grid is of adequate resolution

4) Make sure outer boundaries are far enough away from to section > 10 chord lengths should do it

5) Ensure inlet and outlet/pressure boundaries are correctly prescribed

6) Use a second order differencing scheme

7) Make sure the solution has fully converged, i.e. mass source residual (mass conservation) is low say < 1.0x10^4

8) Remember looking at force convergence can be misleading if convergence is very slow

9) Make sure inlet turbulence parameters are set to those off your comparison experimental data

This should help to get you on track, although there are a few various other things which could also be the source of your problem.

Although this might seem like a simple problem to solve, getting accurate results is very difficult. I've had a lot of fun in my time trying to solve exactly the same flow problem over a NACA0012 section using finite volume CFD methods.

Regards James

 Peter Giannakopoulos February 26, 2004 16:51

Re: Drag predicion for a NACA 0012 airfoil

Thanks James!!!

The problem is that the NACA 0012 exp. data i've been using is from Abbott(1959), where no turbulence data is shown.

I've been thinking that it's most likely a problem of the S-A model within FLUENT, since NOBODY seems to be getting any reasonable results with it.

Other than that, I did all the things you mentioned plus a few of my own, and although i get some good predictions for Cl, the results for Cd are rubbish...

Cheers

 James Date February 27, 2004 12:54

Re: Drag predicion for a NACA 0012 airfoil

The turbulence intensity is quoted in Abbott if you check closely. 10% i think.

You need good exp data to compare. Check the pressure distribution if you can.

Try the k-e model also. A good high quality grid is needed. Avoid using a tet mesh to begin with.

James

 Xwang March 9, 2004 16:27

Re: Drag predicion for a NACA 0012 airfoil

I'm doing the same test. I'm studying an incompressible flow (M=0.12) on a airfoil of unitary chord lenght with Re=3000000. I used a circle of 100m to set a Velocity inlet boundary condition (so I impose the velocity components far from the airfoil) and I obtain a good result for Cd and a poor one for Cl (20% less then experimental data). I use k-e model with the standard parameter for the bondary condition (namely unitary ones). What can I modify?

 Xwang March 9, 2004 16:32

Re: Drag predicion for a NACA 0012 airfoil

I forgot to tell you that I have used a tethaedrical mesh (67000 cells).

P.S.:the radius is 50m not 100m

 All times are GMT -4. The time now is 01:03.