Hi all! I want to calculate lift and drag coefficient on a naca 23012 airfoil at different angle of attack (from 0 to 10 degrees). I've created different type of 2D extruded mesh (one for wall function models and one for low-re models) with blocking in Icem, quad (structured block) all around the airfoil and tria elsewhere (unstructured blocks). The airfoil chord is 1 m long, the domain is 15x14m, the Reynolds number is 3*10^6. y+ is about 60 for coarse mesh and <1 for fine mesh (with 20 nodes in the boundry layer). I run the solver in double-precision mode and I leave the solver running until the lift and drag forces (which i monitor) stabilize and until the convergence (1e-9) is reached . The results is in very good agreement with experimental data (from Abbott) for lift (error < 1%), but the drag coefficient is too high (+55%). I've tried two different models, SST and BSL-Reynolds Stress. What should I do for better drag prediction? How can I justify, to my course professor, this divergence from experimental data? Thank you in advance! Ps. sorry for my "english"!

Hi Bogatec

What type of typology did you use. Can i have a look at your mesh. You can e-mail it to on cfd.student@gmail.com. Drag is difficult to predict. You have to have very fine mesh for it.

Simon

Hi,

I agree with Simon. You will need to be very careful with your boundary layer mesh for accurate drag prediction. Do a sensitivity study of the boundary layer mesh parameters.

Glenn Horrocks

I've sended the Icem project file and the CFX def file to cfd.student; I think it is possible to obtain better results with smoother and more relaxed mesh, but I dont know how do that in Icem... with use of pre-mesh smoother I can't get a relaxed mesh

For a sensitivity study you mean, in practice, grid indipendence analysis?

Hi Ravel i have received your files but there was no mesh. Try using o-grid, make y+=1 in the boundary layer region and make it close to 20 for overall domain. Also have at least 20 cells across the boundary layer region. Use SST turbulence model. This should give you the drag coefficient.

Simon

You have to open the .prj file in icem and select pre-mesh under blocking to see it. Or open the def file in cfx-pre or post. The mesh is C-type, there is 20 nodes in the boundary layer, and y+ is about 1 with max value=2 in just few points.

What is your angle of incidence? If there is flow separation in your flow try LES. Flow separation problems are often poorly predicted by RANS models. I will look at your mesh tomorrow.

Simon

Different angles, from 0 to 10, there is no separation, and the drag prediction is wrong also at 0 degrees

Your mesh looks fine. It has to be turbulence model. Try using different turbulence models and see what comes out of it. Also you have to divide your Cd with dynamic pressure. Dont forget to do that.

Simon

The best turbulence Model for this case I think is SST. If your y+ = 1, the drag should be near the experimental data. As Simon said, you must take the force that is parallel to the wind and divided it by air density, square of free velocity, wing area and multiply by 2. Make sure your calculations are correct, cause sometimes the error are much more simple than you expected.

Ravel, Check you inlet boundary. Make sure that viscosity ratio is very very low at inlet. Two high a viscosity ration means you are flowing numeric mud over the wing and the wall shear drag can be grossly over predictied. I learned this the hard way my self.

If data on the wind tunnel test is not available assume a free stream turbulence intensity of one one tenth of a parcent ie .001 Set the length scale to be small enough to give a viscosity ratio of less than .01

If inlet is OK ie viscosity ratio less than .01 then check coefficient of pressure at front of air foil.

Physically it should be identically 1.000 Numerically you can expect a slight over or under prediction but not by much. A larger over prediction would logically lead to an over prediction of drag. This can be caused by insufficient grid in front of the air foil. Do a one d stream calc assuming a cylinder and solve for pressure on the stagnation stream line. make sure you have lots of grid out to the point where the pressure curve begins to rise. In subsonic flow that can be very far in front of the leading edge.

Good Luck - Andy R

If you look at .def file you will see all the expressions for the Cd and Cl monitoring, it's all correct. Angle = 6 [deg] Chord = 1 [m] Span = 0.1 [m] SectionArea = Chord*Span FreeStreamVel = 2.678 [m s^-1] FluidDensity = 997 [kg m^-3] Drag = ((force_x()@WING)*cos(Angle))+((force_y()@WING)*si n(Angle)) Lift = (-1.0*(force_x()@WING)*sin(Angle))+((force_y()@WING) *cos(Angle)) TrqQuarterCford = torque_z()@WING - ((0.25 * Chord) * force_y()@WING) CD = Drag/(0.5*FluidDensity*SectionArea*FreeStreamVel^2) CL = Lift/(0.5*FluidDensity*SectionArea*FreeStreamVel^2) TrqQuarterChord/(0.5*FluidDensity*SectionArea*Chord*FreeStreamVel^ 2) TargetCD = 0.0078 TargetCL = 0.76 TargetCM = -0.07 RelErrCD = (CD / TargetCD) - 1 RelErrCL = (CL / TargetCL) - 1 RelErrCM = (CM / TargetCM) - 1

For inlet turbulence intensity I assume .0001 (from Naca-TN-1283, for the Langley 2D low-turbulence pressure tunnel, which is indicated in Abbott like the wind tunnel where the experiments were conducted). What you mean for viscosity ratio? Is the ratio between the turbulent viscosity and the fluid viscosity, or something like that? How can I evaluate it? Ok, I think I understand, with the only assumption of the turbulence intensity at the inlet, the turbulence is not yet defined, the "epsilon" or "omega" is still missing. But how is the viscosity ratio related to lenght scale? I mean, is there some semi-empiric expression, or should I just check the results to see if the value of the turbulent viscosity respect this criteria?

I checked the results: the max eddy viscosity at the inlet is 8.9e-5 [Pa s], where the dynamic viscosity is 8.899e-4 [Pa s], thus the ratio is about 0.1, too high then.. Now I try to change the lenght scale and will tell you tomorrow.. Thank you very much for your help!

At the stagnation point the Pressure is 3595.93 [Pa] and the Total Pressure is 3596.06 [Pa], where the expression 0.5*Density*FreeStreamVel^2 give 3599 [Pa]. Now the solver is running with SST model and Eddy Viscosity Ratio = 0.01 (there is an option Eddy Viscosity Ratio at the Inlet Boundary Condition in CFX!), but for what I see the drag error is costant at +58%, and the lift is perfect (-0.9%)! Maybe shold I use some transition model?

The solution lies in the laminar-turbulence transition model, because there is a large portion of laminar region on the airfoil! I tried to use the Gamma-Theta Model, but now there's no convergence..

hi Ravel,

i am new to Cfd, however i feel density value cannot be 997 kg m^-3.

This value is generally taken for water.

for air density = pressure/ ( Gas constant * temperature )

Example: 101325 / ( 287 * 300 )

P = 101325 pa

R = 287 J / kg K

T = 300 Kelvin

and density value will be 1.17682

If Possible can you give some details on why you have considered Naca 23012 & how to generate the profile for this, it will be helpfull.

Thanks & regards raj