CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Drag predicion for a NACA 0012 airfoil

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   February 25, 2004, 19:57
Default Drag predicion for a NACA 0012 airfoil
  #1
Peter Giannakopoulos
Guest
 
Posts: n/a
Ladies & Gentlemen,

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????

Thanks in advance,

Cheers
  Reply With Quote

Old   February 26, 2004, 06:09
Default Re: Drag predicion for a NACA 0012 airfoil
  #2
Ugo
Guest
 
Posts: n/a
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
  Reply With Quote

Old   February 26, 2004, 10:44
Default Re: Drag predicion for a NACA 0012 airfoil
  #3
Peter Giannakopoulos
Guest
 
Posts: n/a
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
  Reply With Quote

Old   February 26, 2004, 14:40
Default Re: Drag predicion for a NACA 0012 airfoil
  #4
James Date
Guest
 
Posts: n/a
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
  Reply With Quote

Old   February 26, 2004, 16:51
Default Re: Drag predicion for a NACA 0012 airfoil
  #5
Peter Giannakopoulos
Guest
 
Posts: n/a
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
  Reply With Quote

Old   February 27, 2004, 12:54
Default Re: Drag predicion for a NACA 0012 airfoil
  #6
James Date
Guest
 
Posts: n/a
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
  Reply With Quote

Old   March 9, 2004, 16:27
Default Re: Drag predicion for a NACA 0012 airfoil
  #7
Xwang
Guest
 
Posts: n/a
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?
  Reply With Quote

Old   March 9, 2004, 16:32
Default Re: Drag predicion for a NACA 0012 airfoil
  #8
Xwang
Guest
 
Posts: n/a
I forgot to tell you that I have used a tethaedrical mesh (67000 cells).

P.S.:the radius is 50m not 100m
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Drag and Lift coefficient (NACA 0012) remi_fr STAR-CCM+ 17 March 2, 2015 17:23
Lift and Drag Coefficient data for NACA 2412 Airfoil mahbub03 Main CFD Forum 22 May 25, 2014 15:39
Symmetric NACA Airfoil Lift and Drag Data jrider22 Main CFD Forum 3 April 15, 2010 04:59
Drag prediction for Naca 23012 airfoil Ravel Bogatec CFX 17 February 15, 2008 01:21
analyzing NACA 0012 airfoil Hammam CFX 5 May 14, 2007 10:30


All times are GMT -4. The time now is 22:45.