# Drag coefficient for aerfoil NACA0012

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

 February 3, 2010, 21:58 Drag coefficient for aerfoil NACA0012 #1 Member   thanos Join Date: Oct 2009 Posts: 30 Rep Power: 10 Hello to everyone! I try to simulate incompressible flow around a NACA0012 aerfoil. I have created a mess about 60.000 elements and y+ floats between 2 and 13. I have chozen the Spalart Allamaras Model. The problem is that although the calculated Cl is close to the experimental values (it's deviation is about up to 20%), the deviation of Cd is very large (about 60% or more). Is anything that i do wrong or is it more difficult to take from FLUENT a precise value of Cd? Thank you in advance.

 February 5, 2010, 13:17 #2 Senior Member   Join Date: Nov 2009 Posts: 411 Rep Power: 13 That is because you use a fully turbulent simulation, for a 0.2 Mach and a reasonable Re like 6*10^6 and for a 2 degree angle of attack you can have 60%-80% of the airfoil surface in laminar flow. This is the reason for which you have such a large discrepancy between your Cd and the experimental Cd. You have two options: 1. Split the mesh in two regions (a laminar and a turbulent region) http://pdf.aiaa.org/preview/2010/CDR...V2010_1469.pdf 2. Use Fluent 12 in which you should have a turbulence model that is capable to model the transition (a modification of the SST Menter model I think). Also your y+ must be lower then 1 or greater then 100 if you use Spalart-Allmaras, a y+ floating from 2 to 13 will give you a bad solution (see some theory of the boundary-layer). Do

 February 5, 2010, 13:24 #3 Member   thanos Join Date: Oct 2009 Posts: 30 Rep Power: 10 thanks a lot for your reply. i don't have fluent 12 but 6.2.16 which does not have this option about the laminar sublayer you say. 1) Is it possible with fluent 6.2.16 to find a good solution about the Cd? 2)If y+ is too small, in the order of 10^-2 or 10^-3 for instance, is it ok? Is the smaller y+ the better or it has o lower limit?

 February 5, 2010, 13:30 #4 Senior Member   Join Date: Nov 2009 Posts: 411 Rep Power: 13 An y+ lower then 1 will converge slower then a y+>100 but you will be able to better catch the physics. You can use Fluent 6.2.16 and have a good Cd (about 10-15% error) if you split your mesh in Gambit in two regions, then in Fluent you can define one of this as a laminar region (in this region Fluent will keep the turbulent viscosity zero) and use SA as turbulence model for the entire flow. You can do this even with Fluent 6.2. Do

 February 5, 2010, 13:35 #5 Member   thanos Join Date: Oct 2009 Posts: 30 Rep Power: 10 How can i do this in fluent 6.2.16? I haven't seen any tutorial doing that. can you show me the way? Also, how can i calculate the size of the laminar sublayer in order to create a right mesh for it?

 February 6, 2010, 09:11 #6 Senior Member   Jouke de Baar Join Date: Oct 2009 Posts: 126 Rep Power: 10 There is another option: use experimental data from a 'trip wire' setup. The foil has a wire along the leading edge that forces the flow to be fully turbulent. For example: W. J. McCroskey, A Critical Assessment of Wind Tunnel Results for the NACA 0012 Airfoil, NASA Technical Memorandum 10001 9 (1987) Still, if you decide to use a laminar region, do the following: Calculate the critical Reynold's point. You can start with the flat plate value Re = 5e5. In Gambit devide your domain in a part in front of this and behind this. Then go to zones, and next to 'specify boundary types' got to 'specify continuum types'. Here you can specify and name your laminar region. Export your mesh. In Fluent under boundary conditions you can select the laminar region and check the force laminar box. good luck!

 February 6, 2010, 09:23 #7 Member   thanos Join Date: Oct 2009 Posts: 30 Rep Power: 10 Thanks for your answer, Ihave two questions: If i separate my mesh to two parts, the turbulent region will be the right one? I can not understand why to divide my mess to two parts, right and left, and assume that the one is turbulent while the other is laminar will give me the correct results. Last edited by thanos; February 6, 2010 at 10:14.

 February 6, 2010, 10:03 #8 Senior Member   Jouke de Baar Join Date: Oct 2009 Posts: 126 Rep Power: 10 That's correct, on the left you have your inflow and laminar region, on the right the turbulent region and outflow. The thing is that the turbulence model will generate a turbulent flow right from the leading edge of your foil. You can check this by plotting the Turbulent Intensity along the chord, under XY plot. In reality the flow will be laminar for the first part of the flow and then become turbulent. Fluent is unable to capture this transition. That is why you have to force this transition by hand. Therefore: a laminar region in front of the hand-calculated transition point. The drag of a completely turbulent foil is higher than of an partly laminar, partly turbulent foil. This might explain why your drag coefficients are to high. Hope it works! Last edited by jack1980; February 6, 2010 at 10:04. Reason: clearify

 February 6, 2010, 10:10 #9 Member   thanos Join Date: Oct 2009 Posts: 30 Rep Power: 10 is it easy to calculate by hand the critical point on the airfoil that i have to separate the mesh?

 February 6, 2010, 13:03 #10 Senior Member   Jouke de Baar Join Date: Oct 2009 Posts: 126 Rep Power: 10 Start out with Re = 5e5 (for the flat plate). So you have: Re = u_in * x_cr / viscosity = 5e5 => x_cr = 5e5 * viscosity / u_in

 February 6, 2010, 13:23 #11 Member   thanos Join Date: Oct 2009 Posts: 30 Rep Power: 10 by telling flat plate you mean the area is (chord)*(depth) ?

 February 6, 2010, 15:44 #12 Senior Member   Jouke de Baar Join Date: Oct 2009 Posts: 126 Rep Power: 10 sorry I didn't explain well. A flat plate is just a fysically flat plate at zero AoA. If you want: a 'naca 0000 at zero AoA' In a flow this flat plate will create a boundary layer. First the flow is laminar. At the transition point it becomes turbulent. The location x_cr of this transition point depends on the velocity u_in, the viscosity, the roughness of the plate etc. Define the critical Reynolds number: u_in * x_cr / visc. It turns out that for a smooth plate Re_cr is around 5e5. Of course you could say "this is all just baloney". The naca 0012 is not a flat plate. The transition point will depend on the section's thickness, the angle of attack etc. This is true, the flat plate transition point will only give a first guess. However it might improve your results. Of course there are alternatives. Like: - more simply: forget about the laminar region and compare your fully turbulent simulations to experimental results with a 'trip wire' - more complicated: calculate the transition points with xfoil, or use results of people who have done this, like in the rightmost figure on page 3 of http://www.basiliscus.com/ProaSectio.../AppendixD.pdf hope it helps, good luck!

 February 6, 2010, 20:27 #13 Member   thanos Join Date: Oct 2009 Posts: 30 Rep Power: 10 thanks a lot! One last question, how can i find data about the ''trip wire'' ? I can not find anything in google with that name.

 February 7, 2010, 04:22 #14 Senior Member   Jouke de Baar Join Date: Oct 2009 Posts: 126 Rep Power: 10 For example in W. J. McCroskey, A Critical Assessment of Wind Tunnel Results for the NACA 0012 Airfoil, NASA Technical Memorandum 10001 9 (1987) http://www.csc.kth.se/~jhoffman/wiki/archive/papers/McCroskey87.pdf They give experimental results for zero AoA, for 2e6 < Re < 2e7, with and without tripwire. The data are shown in Figs 4 and 5. Formulas 1 to 3 give fits to this data.

 February 7, 2010, 14:13 #15 Member   thanos Join Date: Oct 2009 Posts: 30 Rep Power: 10 nasa has also data about more angles of attack? thanks very much, I really appreciate your help.

 February 8, 2010, 09:01 #16 Senior Member   Jouke de Baar Join Date: Oct 2009 Posts: 126 Rep Power: 10 I'm afraid I don't know, sorry ...

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post John FLUENT 16 September 4, 2009 02:44 sebastian_vogl OpenFOAM Running, Solving & CFD 5 December 31, 2008 13:19 vinz OpenFOAM Running, Solving & CFD 98 October 27, 2008 09:43 Freeman Main CFD Forum 10 January 27, 2006 08:42 Noé Siemens 5 July 13, 2004 10:21

All times are GMT -4. The time now is 11:56.