Hello

I am studying the drag-lift coefficient of an airfoil NACA 23012, and don't worry, my question is different than the ones you can find on the whole forum...

Is the "section drag coefficient" (found in books such as "Theory of wing sections") the same than the "drag coefficient" (calculated, with CFX for example, on a 3D airfoil) ? (And in fact I have the same question for the lift coefficient...)

Any idea?

Many thanks in advance

Mary

As far as I remember in CFX Post there's not the "drag coefficient" variable. The drag coefficient of CFX should be for the particle tracking... The drag coefficient of the books for an airfoil should be calculated from the Drag (1/2rhov2CdA) and the Drag is the Force of CFX. Be careful if your airfoil is not aligned with the X and Y axis, you have to project the Force. Is the simulation of CFX done considering only one cell in the 3rd direction? The Naca airfoil is 2D, while CFX needs at least one element in the 3rd direction. Hope this helps!

Section drag coefficient is the drag coefficient calculated for a 2d cross-section of infinite span. In essence, it is a drag/span type number.

You have understood that I have a bad drag coefficient

In CFX I can calculate the forces on X and Y axis for the whole airfoil... my airfoil is well aligned... I use your formula, I obtain a Cd : different from the Cd of the book..And I haven't understood in your answer whether they should be equal...

I use a good mesh, a good turbulence model, so a good Y+, a good Re...I don't know how to find a good Cd.. In fact I don't know which is the good Cd

My lift coefficient, and pressure distribution are almost perfect...

Any idea?

Thanks Ag

So you mean that if my span is 1meter : Cd Cfx = Cd book * 1meter ?? ouinnnnnn it changes nothing

One question: you say that your airfoil is aligned with X and Y. And your wind? The Drag is the force in the direction of the wind and the lift is perpendicular to it. Is your wind aligned with one of the axis?

I don't use CFX, so I don't know what CFX is giving you. I just gave the definition of section drag. If you are performing a simulation of a L-meter section of airfoil, with suitable end conditions to simulate an infinitely long airfoil (or alternatively a 2d flow) then the section drag would be the total drag (evaluated over the entire surface) divided by the L-meter span. If you are not in agreement with the experimental values, make sure you are comparing apples to apples. Total drag is composed of the pressure drag and viscous drag - make sure that you're not computing pressure drag in the solver and comparing to total drag in a report, for example.

don't worry my wind is on the X axis (like my chord) and it is Y for my lift force

Thanks, Like that I have checked that

Thanks for your time, and your interesting answer...

yes I have a simulation of a 1-meter section of an airfoil with suitable end conditions to simulate an infinitely long airfoil (function of CFX: Symmetry plane at the end of the airfoil)

and I am sure that I compute pressure+viscous drag on CFX, and I can check tomorrow in the book if it is really the total drag, but I think so..

I find Cd=0.13 instead of 0.65

Any other ideas ?

If your lift and pressure distribution look good, but drag is not correct, then my first guess would be that the viscous contribution is not correct. This could be due to having a grid that is too coarse at the wall, incorrect turbulence modeling (are you comparing laminar results to turbulent data, for example), etc. Or there could be an error in the formula you are using to compute drag. Those are the things I would look at first.

Check up! :

I use the SST model, automatic wall treatment

Y+ ~1

I think this is the problem : Reynolds number : -when I calculate it manually, I have a result around 3.10^6 (charateristic length:chord, Reynolds used in the book) -but CFXsolver use an other length and so find Re=1.10^7... The difference shall come from here, no?? If you think so, I am going to ask in the CFX-forum how to change it because I don't know...

Thank you very much to give me so much possible error!!!

As far as I know CFX calculates the Re number considering the inlet velocity, the inlet width, and the average density over the inlet area and the result may be different from the Re number indicated for the airfoil in the book. Regarding the mesh (Hexa or Tetra?) it is important to have 10 nodes in the boundary layer. Hope this helps!

Ok for the Reynolds number... I use the Hexa-mesh (it is a good choice?) And I have refined my mesh (my BL is very fine), and now I have a Cd of 0.007 instead of 0.006... It is enough for me

Thank you!!

Marion i had the answer to your question why did you not ask me. Anyways its too late now! You should work on your dam!

Usman