CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Naca airfoil with too high drag

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

Like Tree5Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 15, 2006, 12:13
Default Hi! I try to calculate a f
  #1
Member
 
Andreas Hauffe
Join Date: Mar 2009
Location: Dresden, Germany
Posts: 36
Rep Power: 7
andimb is on a distinguished road
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
andimb is offline   Reply With Quote

Old   March 15, 2006, 13:10
Default Whats your y+?
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 11
eugene is on a distinguished road
Whats your y+?
eugene is offline   Reply With Quote

Old   March 15, 2006, 15:02
Default Hi! The y+ is something aro
  #3
Member
 
Andreas Hauffe
Join Date: Mar 2009
Location: Dresden, Germany
Posts: 36
Rep Power: 7
andimb is on a distinguished road
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
andimb is offline   Reply With Quote

Old   March 15, 2006, 15:47
Default Hi andreas the y+ can be ca
  #4
Senior Member
 
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 7
kumar2 is on a distinguished road
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
kumar2 is offline   Reply With Quote

Old   March 16, 2006, 07:58
Default If you use a low-Re turbulence
  #5
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 11
eugene is on a distinguished road
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.
eugene is offline   Reply With Quote

Old   March 16, 2006, 10:27
Default Hi! Right now I'm useing th
  #6
Member
 
Andreas Hauffe
Join Date: Mar 2009
Location: Dresden, Germany
Posts: 36
Rep Power: 7
andimb is on a distinguished road
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!
andimb is offline   Reply With Quote

Old   March 16, 2006, 10:57
Default Hi sorry, I found answers o
  #7
Member
 
Andreas Hauffe
Join Date: Mar 2009
Location: Dresden, Germany
Posts: 36
Rep Power: 7
andimb is on a distinguished road
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.
andimb is offline   Reply With Quote

Old   May 3, 2007, 22:20
Default Andreas, I have only just seen
  #8
Member
 
Shaun Darmody
Join Date: Mar 2009
Posts: 36
Rep Power: 7
shaun is on a distinguished road
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
shaun is offline   Reply With Quote

Old   June 6, 2007, 17:42
Default Andreas- Would you be willi
  #9
Member
 
Doug Hunsaker
Join Date: Mar 2009
Location: Logan, UT
Posts: 57
Rep Power: 7
doug is on a distinguished road
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
doug is offline   Reply With Quote

Old   August 14, 2008, 06:16
Default Hi all I am trying to solve
  #10
Senior Member
 
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 7
mgz1985 is on a distinguished road
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
mgz1985 is offline   Reply With Quote

Old   August 14, 2008, 08:04
Default Hello Mayank, Could you giv
  #11
Member
 
Kevin Maki
Join Date: Mar 2009
Location: Ann Arbor, MI, USA
Posts: 38
Rep Power: 7
kjmaki is on a distinguished road
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
kjmaki is offline   Reply With Quote

Old   August 15, 2008, 02:28
Default Hi Kevin, I m simulating a
  #12
Senior Member
 
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 7
mgz1985 is on a distinguished road
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
mgz1985 is offline   Reply With Quote

Old   August 15, 2008, 02:29
Default http://www.cfd-online.com/Ope
  #13
Senior Member
 
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 7
mgz1985 is on a distinguished road
p

controlDict
mgz1985 is offline   Reply With Quote

Old   August 17, 2008, 22:14
Default Dear Mayank, If you are usi
  #14
Member
 
Kevin Maki
Join Date: Mar 2009
Location: Ann Arbor, MI, USA
Posts: 38
Rep Power: 7
kjmaki is on a distinguished road
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
kjmaki is offline   Reply With Quote

Old   August 18, 2008, 02:31
Default hi Kevin, I had already tri
  #15
Senior Member
 
mayank gupta
Join Date: Mar 2009
Posts: 110
Rep Power: 7
mgz1985 is on a distinguished road
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
mgz1985 is offline   Reply With Quote

Old   September 16, 2009, 20:20
Default
  #16
Senior Member
 
Steve Hansel
Join Date: Jun 2009
Location: Colorado, USA
Posts: 112
Rep Power: 7
hansel is on a distinguished road
Quote:
Originally Posted by mgz1985 View Post
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?
hansel is offline   Reply With Quote

Old   November 6, 2009, 05:45
Red face Reynold number
  #17
New Member
 
kapten_alieph
Join Date: Jul 2009
Posts: 1
Rep Power: 0
kapten_alieph is on a distinguished road
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
kapten_alieph is offline   Reply With Quote

Old   November 6, 2009, 12:58
Default
  #18
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 10
sega is on a distinguished road
Quote:
Originally Posted by kapten_alieph View Post
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!"
sega is offline   Reply With Quote

Old   January 3, 2010, 01:27
Default Problem with Drag force!
  #19
Member
 
nguyen van trieu
Join Date: Jul 2009
Posts: 64
Rep Power: 7
nvtrieu is on a distinguished road
Quote:
Originally Posted by andimb View Post
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!
nvtrieu is offline   Reply With Quote

Old   January 27, 2010, 05:05
Default
  #20
Senior Member
 
MadsR's Avatar
 
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 8
MadsR is on a distinguished road
Hi.

Any progress here?

/Mads
__________________
Online free airfoil-mesher for OpenFOAM here
MadsR is offline   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
Lift and drag coefficient with strange values for NACA airfoil antonio_ing OpenFOAM Running, Solving & CFD 16 September 13, 2012 13:21
NACA 23020 airfoil drag and lift calculation. Zmur CFX 2 December 23, 2008 17:35
Drag prediction for Naca 23012 airfoil Ravel Bogatec CFX 17 February 15, 2008 01:21
Naca airfoil with to much drag Andreas CFX 6 March 17, 2006 07:13
Drag predicion for a NACA 0012 airfoil Peter Giannakopoulos FLUENT 7 March 9, 2004 16:32


All times are GMT -4. The time now is 15:27.