# Naca airfoil with too high drag

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

 March 15, 2006, 12:13 Hi! I try to calculate a f #1 Member   Andreas Hauffe Join Date: Mar 2009 Location: Dresden, Germany Posts: 36 Rep Power: 8 Hi! I try to calculate a flow around some Naca 4 digit airfoils. In my calculation the lift is nearly right, but the drag is much too high. I'm comparing the calculated values with the book "theory of wing sections". Can you give me a reason or advice? I use a wall as boundary condition for a profil and the calculations are done with the standard k-epsilon turbulence model. Thank you Andreas

 March 15, 2006, 13:10 Whats your y+? #2 Senior Member   Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 12 Whats your y+?

 March 15, 2006, 15:02 Hi! The y+ is something aro #3 Member   Andreas Hauffe Join Date: Mar 2009 Location: Dresden, Germany Posts: 36 Rep Power: 8 Hi! The y+ is something around 40. This is to high, right? Is there a way to calculate the y+ with OpenFOAM or how do I by hand? I did it with CFX this time. What turbulence model should I use? Thanks for the responce. Andreas

 March 15, 2006, 15:47 Hi andreas the y+ can be ca #4 Senior Member   kumar Join Date: Mar 2009 Posts: 112 Rep Power: 8 Hi andreas the y+ can be calculated with the checkYPlus command ( this is in utilities .) you can also calculate the lift and drag with the liftDrag command . i am also working with foils and am very curious to know the y+ range best for OpenFoam regards kumar

 March 16, 2006, 07:58 If you use a low-Re turbulence #5 Senior Member   Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 12 If you use a low-Re turbulence model a y+ = 1 is best. If you use a high-Re turbulence model a 30 < y+ < 100 is preferred. If you have high streamwise pressure gradients and or weak seperation, a low-Re model will do better than the high-Re model. For aerofoils you should be using a low-Re model. Search the forum for a post by Hrv about what kinds are available.

 March 16, 2006, 10:27 Hi! Right now I'm useing th #6 Member   Andreas Hauffe Join Date: Mar 2009 Location: Dresden, Germany Posts: 36 Rep Power: 8 Hi! Right now I'm useing the standart k-epsilon-tubulence model. I know that it is thought for near wall problems, but I unable to get another model calculating. Could someone give me some advice? - Which schemes should I use? - Which model? - Which relaxations factor in simpleFoam? I'm calculating a Re=6 Mio and an speed of Ma 0.25. Thanks Andreas Sorry for my Englisch!

 March 16, 2006, 10:57 Hi sorry, I found answers o #7 Member   Andreas Hauffe Join Date: Mar 2009 Location: Dresden, Germany Posts: 36 Rep Power: 8 Hi sorry, I found answers of my question in older posts. 1. start by running potentialFoam, this is a good way of checking the BCs as well as generating a sensible starting U field. 2. start the simpleFoam run with very low under-relaxation on these fields, 0.05 or even lower. 3. after a few iterations this can be raised to a normal level Sorry, Andreas Alhasan likes this.

 May 3, 2007, 21:20 Andreas, I have only just seen #8 Member   Shaun Darmody Join Date: Mar 2009 Posts: 36 Rep Power: 8 Andreas, I have only just seen this post. Your drag is too high because you have turbulent flow everywhere. The boundary layer is more than likely transitioning from laminar to turbulent flow. Hence your drag value would be incorrect for a RANS simulation that assumes turb flow throughout the domain. Use XFOIL or if you can get a copy try MSES. Both codes are from Marc Drela and take into account boundary layer transition. regards Shaun.D

 June 6, 2007, 16:42 Andreas- Would you be willi #9 Member   Doug Hunsaker Join Date: Mar 2009 Location: Logan, UT Posts: 63 Rep Power: 8 Andreas- Would you be willing to send me a zipped file of your input parameters for your potential foam case? I've been trying to get an airfoil case running in potential foam, but have an error in my boundary conditions. I haven't been able to locate the error. Would you mind sending me your files so I can compare my BCs to yours? Thanks. -Doug

 August 14, 2008, 05:16 Hi all I am trying to solve #10 Senior Member   mayank gupta Join Date: Mar 2009 Posts: 110 Rep Power: 8 Hi all I am trying to solve a laminar flow over an airfoil in a 2-D case with icoFoam as it is an incompressible flow. I am facing a problem with the Cd and Cl values. they are vey low with a reference area of 1 to the order of 1e-07. can some one help me? regarding the potentialFoam, I want to try it but need help in setting up the case as I can't understand it in my tutorials (it does not have reynold's number definition, and even if i change my end time, my solution stops after one second in the example of pitzDaily) thanks a lot

 August 14, 2008, 07:04 Hello Mayank, Could you giv #11 Member   Kevin Maki Join Date: Mar 2009 Location: Ann Arbor, MI, USA Posts: 41 Rep Power: 8 Hello Mayank, Could you give more details about the particular foil that you are using, and the angle of attack you are simulating? Perhaps the lift-curve slope will be the quantity that interests you most for validation. Also, without turbulence, your drag coefficient may be very low, especially if it is a thin foil at a small angle of attack. About potentialFoam, I understand that this can be used to generate more realistic initial conditions for the Navier-Stokes solver, but be careful about the velocity at the trailing edge. I don't see how you can impose the Kutta-condition when solving the full Navier-Stokes equations for a case that is not at the angle of zero lift, and therefore with non-zero angle of attack the continuous solution will have infinite velocity at the trailing edge. If it were me, I would just start from uniform i.c.'s for this problem. Kind regards, Kevin

 August 15, 2008, 01:28 Hi Kevin, I m simulating a #12 Senior Member   mayank gupta Join Date: Mar 2009 Posts: 110 Rep Power: 8 Hi Kevin, I m simulating a NACA 63A41 air foil at dynamic pressure fo 120 km/m/s and Reynold's Number of 1.67 million. I have to solve at various angles of attack but I first tried 0 degree and it is giving me errors in Cd and Cl. The problem is not only the low value of CD but also the low value of Cl. I am attaching my boundary conditions file alongwith controlDict here. If you could take a look. U

 August 15, 2008, 01:29 http://www.cfd-online.com/Ope #13 Senior Member   mayank gupta Join Date: Mar 2009 Posts: 110 Rep Power: 8

 August 17, 2008, 21:14 Dear Mayank, If you are usi #14 Member   Kevin Maki Join Date: Mar 2009 Location: Ann Arbor, MI, USA Posts: 41 Rep Power: 8 Dear Mayank, If you are using icoFoam, and your body resides entirely inside the flow domain, then you do not need to specify pressure. I had a glance at the new forces postProcessing tool, and the c++ is a little too heavy for me to comment on your choice of rho, I would check this and the reference length. But, as I was trying to get at in my earlier reply, if you are simulating an angle near the angle of zero-lift, you should have very small forces, right? The lift should be close to zero and the drag will be small anyway, cd~10e-(3-4), but you have no turbulent viscosity, so it can even be much smaller than that! Have you tried an angle that is larger so that you can compute the lift-curve slope? Regards, Kevin

 August 18, 2008, 01:31 hi Kevin, I had already tri #15 Senior Member   mayank gupta Join Date: Mar 2009 Posts: 110 Rep Power: 8 hi Kevin, I had already tried with 0 pressure also but without any success. My drag forces are of the order of 10e-04 and cd is of 10e-07 with reference area of 1 but if i reduce the reference area by the order I get the Cd of the correct order but Cl is a order less. yes my airfoil is inside the whole domain. My cells near the airfoil (in the boundary layer) are smaller than the boundary layer thickness (0.1/Re^0.5) The only option I think left to try is make the upstream and downstream region very high or use another solver. I have already tried simpleFoam with turbulence off but no success there too. I am making a better mesh today and running the solver. Shall let you know if there is any improvement. The important thing is I am comparing these results with the actual wind-tunnel results. So the problem is in my CFD. I know this message is long but it has everything I believe relevant to my problem. Thanx a lot

September 16, 2009, 19:20
#16
Senior Member

Steve Hansel
Join Date: Jun 2009
Posts: 112
Rep Power: 8
Quote:
 Originally Posted by mgz1985 hi Kevin, I had already tried with 0 pressure also but without any success. My drag forces are of the order of 10e-04 and cd is of 10e-07 with reference area of 1 but if i reduce the reference area by the order I get the Cd of the correct order but Cl is a order less. yes my airfoil is inside the whole domain. My cells near the airfoil (in the boundary layer) are smaller than the boundary layer thickness (0.1/Re^0.5) The only option I think left to try is make the upstream and downstream region very high or use another solver. I have already tried simpleFoam with turbulence off but no success there too. I am making a better mesh today and running the solver. Shall let you know if there is any improvement. The important thing is I am comparing these results with the actual wind-tunnel results. So the problem is in my CFD. I know this message is long but it has everything I believe relevant to my problem. Thanx a lot
Did you have any luck getting reasonable numbers?

 November 6, 2009, 05:45 Reynold number #17 New Member   kapten_alieph Join Date: Jul 2009 Posts: 1 Rep Power: 0 Hai Guys, i'm a new member...please help me,, i want to know Reynold number for standart air flow for air conditioning of building ?? thanks for help

November 6, 2009, 12:58
#18
Senior Member

Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
Quote:
 Originally Posted by kapten_alieph Hai Guys, i'm a new member...please help me,, i want to know Reynold number for standart air flow for air conditioning of building ?? thanks for help
I don't know how this question is related to airfoils (which is the topic of this discussion)?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"

January 3, 2010, 01:27
Problem with Drag force!
#19
Member

nguyen van trieu
Join Date: Jul 2009
Posts: 69
Rep Power: 8
Quote:
 Originally Posted by andimb Hi! I try to calculate a flow around some Naca 4 digit airfoils. In my calculation the lift is nearly right, but the drag is much too high. I'm comparing the calculated values with the book "theory of wing sections". Can you give me a reason or advice? I use a wall as boundary condition for a profil and the calculations are done with the standard k-epsilon turbulence model. Thank you Andreas
Hello Andimb,

I've been doing simulation on NACA 4 digits in Star-CCM+. I still got the problem as yours before. The lift force is ok, but the drag is higher than experimental data, especially, when increase the attack angle. Have you fixed your problem yet? then could you show me in very detail how to correct the drag force? I still confuse how to determine "y+", "testing grid independence".
It should better for me if you can send me an email: trieuckgt@gmail.com
Thanks you so much!

 January 27, 2010, 05:05 #20 Senior Member     Mads Reck Join Date: Aug 2009 Location: Copenhagen, Denmark Posts: 175 Rep Power: 8 Hi. Any progress here? /Mads __________________ Online free airfoil-mesher for OpenFOAM here

 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 antonio_ing OpenFOAM Running, Solving & CFD 16 September 13, 2012 12:21 Zmur CFX 2 December 23, 2008 17:35 Ravel Bogatec CFX 17 February 15, 2008 01:21 Andreas CFX 6 March 17, 2006 07:13 Peter Giannakopoulos FLUENT 7 March 9, 2004 16:32

All times are GMT -4. The time now is 09:23.