Dear Sirs, I'm Dr. Laith K. Abbass from University of Technology- Baghdad, Iraq.I would like to ask a question which is problem for me in my research now.In my research dealing with the solution of the flow around an airfoil section using CFD in 2D by finding the pressure and shear for each node on the surface of the airfoil. If I want to compute the pressure coeff., lift and drag coefficients from the pressure and shear which I found. Can you assist me by sending mathematical relations of them because I don't depend on the relations of the academic (text) books? Thank you for corporation.

Dear Dr.Abbas,

Here are the relations you asked for

cli = ( fy * Dcos(alpha) - fx * Dsin(alpha) ) /&

(0.5d0*rhoinf*(uinf**2+vinf**2))

cdi = ( fy * Dsin(alpha) + fx * Dcos(alpha) ) /&

(0.5d0*rhoinf*(uinf**2+vinf**2))

clv = ( sfy * Dcos(alpha) - sfx * Dsin(alpha) ) /&

(0.5d0*rhoinf*(uinf**2+vinf**2))

cdv = ( sfy * Dsin(alpha) + sfx * Dcos(alpha) ) /&

(0.5d0*rhoinf*(uinf**2+vinf**2))

cl = cli +clv

cd = cdi + cdv

sfx = (touxx*sx(j)+touxy*sy(j))

sfy = (touxy*sx(j)+touyy*sy(j))

touwall = touxy*(tx**2-ty**2) - (touxx-touyy)*tx*ty sfc = touwall/(0.5d0*rhoinf*(uinf**2+vinf**2))

fy = fy +(-) p * sy(j)

fx = fx +(-) p * sx(j)

cp = (p - pinf)/(0.5d0*rhoinf*(uinf**2+vinf**2))

Note that cli,cdi coresspond to inviscid part and clv,cdv correspond to the viscous part. alpha is angle of attack and sx, sy represent the area normals, basically the product of face area and the normal component nx and ny. Note that in calculating sfx and sfy you need to integrate over all the points on the airfoil. inf refers to freestream conditions. Further in calculating the forces fx and fy you see that the proper sign must be used (+ or -) depending on conservation (flux leaves one cell and enters the other cell through a given face, so contribution to one cell is positive, while other is negative). Since you have the nodal values and you are concerned with only a specific boundary(here the airfoil), only one sign will come into picture. sfc represents the friction coefficient. Note that tx and ty are the tangential components and are given by

tx = -ny ty = nx

Note that nx,ny and facearea can be obtained by just knowing the nodes of the face, by

face_area = dsqrt(( x2- x1)**2)+(y2 - y1)**2)

nx = (y2-y1)/face_area

ny = -(x2-x1)/face_area

These relations can be derived from fundamental principles also, and you can check them for yourself to find if any error has crept in. Hope this helps.

Regards,

Ganesh

Dear Mr. Ganesh, Good Day to you,

I appreciate your mail and the related equations. Thank you so much. I've worked on Peric Code which solved 2D-Navier-Stokes equations with finite volume using k-w method. The results which I obtained for NACA 2412 using about 12000 elements with Re=3.1*10**6 are as follows: For angle of attack = 8 degree, Cli= 1.05, Clv=-0.00139, so CL=1.058, experimental result = 1.056. For the same angle of attack, Cdi=0.1812, Cdv=0.00708, so CD=0.1883, experimental result=0.0115. Pitching moment coeff Cm=-0.124 and experimental work=-0.15.

For angle of attack = 12 degree, Cli= 1.285, Clv=-0.001444, so CL=1.285, experimental result = 1.4. For the same angle of attack, Cdi=0.346, Cdv=0.00526, so CD=0.3517, experimental result=0.0172. Pitching moment coeff Cm=-0.14, experimental work=-0.1. As you see, the results for drag are too far. Would you please explain why? Thank you and looking forward to having your kindly reply, I remain. Dr. Laith K. Abbass

Dear Dr.Abbas,

It is nice to know that my mail was of some help to you. As for the problem you are facing regarding the mismatch in Cd, it is really surprising to me. This is because the inviscid part contributes to the lift and the viscous part contributes to the drag. Thus we would expect cli>>clv and cdi<<cdv. In short it is only practical to assume cl ~ cli and cd ~ cdv (unless inviscid drag components play a major role). However on the contrary, your cdi is 1000 orders larger than cdv, which indicates a problem. I have checked out the relationships I had mailed you and have found them correct, as you would have also verified. It is also difficult to think that getting cl right but cd wrong is fortunate.

I would therefore suggest that you try running the case just as an inviscid one and check the values of cl and cd. This could be possibly be one way of trying out if something has gone wrong at some point. I could also try the same with my code but I am at present only equipped with a Baldwin-Lomax model. If you could kindly wait for a day or two, I can try out your case and verify, provided I have the Mach number for the case. I however feel that there could have been a interplay of signs in your case, though I am not sure of the same.

Hope this helps. I can also try your case if you could kindly mail me the mach number.

Regards,

Ganesh

Dear Mr. Ganesh, Thank you for help. As I mail to you before, the Re=3.1*10**6, Mach Number= 0.13, Chord length =1. I will also send to you across your mail the some of results. Thank you again for assistance. Dr. Laith K. Abbass

Dear Dr.Abbas,

Thankyou for the information. I shall try out your test case and mail you the results in two days time. Hope that you will be able to resolve your problem by then.

Regards,

Ganesh

dear Mr. Ganesh, Thank you for your mail. I've sent to you a mail consists of some questions and results. I hope that you receive it. Thank you. Regards. Dr. Laith K. Abbass

Dear Dr. Laith, it seems to me that your mesh is not refine enough to capture with accuracy the drag coeficient (12000 elements only !). Usually, the capture the Cl with a reasonable accuracy is not a big deal, but to capture the Cd you really need to be careful. For example, with a Re of 3 millions and a Mach number of 0.20 the first point of the mesh outside the wall, would need to be around 10e-6 m to allow you to have an Y+ of 1. For an airfoil with a reference length of 1m the boundary layer thickness would be around 20 mm at the ending(more or less). To generate a quadrilateral mesh just to represent the boundary layer would lead you to something about 20.000 or 30.000 elements ! You also need to capture with accuracy the wake as well. Usually my 2D meshes are not lower than 200.000 elements.

Regards, Alexandre

Dear Alexandre,

It is true that the first spcaing shuld be of order 1e-6 to have a y+ close to 1 and get accurate results. However, I feel your grid is more fine than required for getting accurate results. You could always try a hybrid grid, or else you could go for mesh adaptation if necessary. However, even in the first case of suitably stretching a structured grid so that your grid is properly spaced near the body or using a hybrid mesh, with stretched quads near the airfoil, you can cut down your computations by a huge amount. In fact a standard test case of turbulent past RAE 2822 airfoil required only 25000 elements(All quads, C-grid) to give accurate results in my case.

If you feel that your computations are taking too much time and there is necessity to cut down time, you can try this suggestion.

Regards,

Ganesh