CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Naca airfoil with too high drag (http://www.cfd-online.com/Forums/openfoam-solving/58641-naca-airfoil-too-high-drag.html)

andimb March 15, 2006 12:13

Hi! I try to calculate a f
 
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

eugene March 15, 2006 13:10

Whats your y+?
 
Whats your y+?

andimb March 15, 2006 15:02

Hi! The y+ is something aro
 
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

kumar2 March 15, 2006 15:47

Hi andreas the y+ can be ca
 
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

eugene March 16, 2006 07:58

If you use a low-Re turbulence
 
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.

andimb March 16, 2006 10:27

Hi! Right now I'm useing th
 
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 March 16, 2006 10:57

Hi sorry, I found answers o
 
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

shaun May 3, 2007 21:20

Andreas, I have only just seen
 
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

doug June 6, 2007 16:42

Andreas- Would you be willi
 
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

mgz1985 August 14, 2008 05:16

Hi all I am trying to solve
 
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

kjmaki August 14, 2008 07:04

Hello Mayank, Could you giv
 
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

mgz1985 August 15, 2008 01:28

Hi Kevin, I m simulating a
 
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.

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif U

mgz1985 August 15, 2008 01:29

http://www.cfd-online.com/Ope
 
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif p

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif controlDict

kjmaki August 17, 2008 21:14

Dear Mayank, If you are usi
 
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

mgz1985 August 18, 2008 01:31

hi Kevin, I had already tri
 
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

hansel September 16, 2009 19:20

Quote:

Originally Posted by mgz1985 (Post 197332)
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?

kapten_alieph November 6, 2009 05:45

Reynold number
 
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 :confused:

sega November 6, 2009 12:58

Quote:

Originally Posted by kapten_alieph (Post 235322)
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 :confused:

I don't know how this question is related to airfoils (which is the topic of this discussion)?

nvtrieu January 3, 2010 01:27

Problem with Drag force!
 
Quote:

Originally Posted by andimb (Post 197318)
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!

MadsR January 27, 2010 05:05

Hi.

Any progress here?

/Mads


All times are GMT -4. The time now is 08:51.