[reyeszjj]

i'm using CFD-ACE to model flow over airfoil(naca0012) and compare them with experiment data (http://www.cyberiad.net/library/airf...ta/n0012cd.htm)

the reynolds number i used is 5e+006 and attached is the data i got compared with experiment data

anyone has any idea about what the problem might be?

Thanks in advance

[pavitran]

1. How you are calculating your lift and drag coefficients. ?
cl = [Force_normal*cos(AOA)-Force_axial*sin(AOA)]/(0.5*density*V^2*S)
cd = [Force_normal*sin(AOA)+Force_axial*cos(AOA)]/(0.5*density*V^2*S)

S-> surface area
V-> velocity

2. If your using the above equations, then I guess your simulation is overpredicting the forces.

3. If your using k-w SST turbulence model with average y-plus < 2, then you will get a good matching of cl & cd with experiments till cl-max AOA ( provided your mesh quality is good).

[reyeszjj]

Originally Posted by pavitran

1. How you are calculating your lift and drag coefficients. ?
cl = [Force_normal*cos(AOA)-Force_axial*sin(AOA)]/(0.5*density*V^2*S)
cd = [Force_normal*sin(AOA)+Force_axial*cos(AOA)]/(0.5*density*V^2*S)

S-> surface area
V-> velocity

2. If your using the above equations, then I guess your simulation is overpredicting the forces.

3. If your using k-w SST turbulence model with average y-plus < 2, then you will get a good matching of cl & cd with experiments till cl-max AOA ( provided your mesh quality is good).

1. I set the parameter of AOA in geometry and mesh, so the geometry includes the AOA, thus my equation is
cl = [Force_y]/(0.5*density*V^2*S)
cd = [Force_x]/(0.5*density*V^2*S)

2. my guess is that i need to split the mesh on the airfoil into laminar and turbulent domains

3. I used the default k-epsilon model for turbulent, I will try others to see if there's any improvement

Thanks pavitran

[pavitran]

Could you tell me how your defining your velocity at the inlet?

[dominic]

I guess your grid is already rotated to account for angle of attack, so you do not have to add any contribution of angle of attack or axial contribution of lift. The forces Fx and Fy that you obtain represent Drag and Lift respectively. Between 8 and 18 degrees, you can see that your lift is under-predicted by a large amount. Similarly, your drag is over-predicted. I believe this should be related to your grid resolution ? Check your grid quality and try refining it.

-Dominic

[reyeszjj]

Originally Posted by pavitran

Could you tell me how your defining your velocity at the inlet?

HI pavitran

I refined my mesh, now yplus is well below 1, but the results did not improve a lot, the drag is still miles away, though lift is, as before, acceptable

for inlet, I defined
pressure:73048
temperature:283
velocity:236(which is mach number 0.7)
and i used standard k-epsilon model, using turbulence intensity 0.01 and length scale 0.02, kinetic energy 8.52

I tried to switch to SST, but it diverged, must be wrong with the parameters

I'm very frustrated about the drag results

Any idea?

Thanks in advance

[pavitran]

Originally Posted by reyeszjj

HI pavitran

I refined my mesh, now yplus is well below 1, but the results did not improve a lot, the drag is still miles away, though lift is, as before, acceptable

and i used standard k-epsilon model, using turbulence intensity 0.01 and length scale 0.02, kinetic energy 8.52

I tried to switch to SST, but it diverged, must be wrong with the parameters

1. Standard k-epsilon model is not used for resolving viscous boundary layer(yplus below 1) , unless until you have some low Re modifications to the model. Usually k-epsilon model is used along with wall functions.

2. When you have yplus below 1, use the SST model.

The reasons for divergence may be?

a. What type of domain you used, I guess it is a C-domain? and how far is your outlet boundary? Usually it should be 15 to 20 chords away. How did you resolve your wake region.?
b. What type of numerical scheme are you using for discretization?
c. And also try to check with your solver manual about the allowed aspect ratio of cells and also check for orthoganility? I guess your using quad cells(for 2D)?
d. From my experience I have seen the convergence problems ( especially when you have separation) because of cell aspect ratios in the wake region, just behind the trailing edge (ofcourse it also depends on what solver your using).

e. My advice is, try to keep the average y-plus below 2 and avoid below 1, because more cells ends up in viscous boundary layer than required(This also helps in in decreasing the aspect ratio) and in the outer part of turbulent boundary layer the number of cells will decrease?

Regarding the Turbulence parameters(length scale and Turbulent Kinetic energy) you used. Please refer the following webpage for further guidance.
http://support.esi-cfd.com/esi-users/turb_parameters/

I hope this will help you

[reyeszjj]

Originally Posted by pavitran

1. Standard k-epsilon model is not used for resolving viscous boundary layer(yplus below 1) , unless until you have some low Re modifications to the model. Usually k-epsilon model is used along with wall functions.

2. When you have yplus below 1, use the SST model.

The reasons for divergence may be?

a. What type of domain you used, I guess it is a C-domain? and how far is your outlet boundary? Usually it should be 15 to 20 chords away. How did you resolve your wake region.?
b. What type of numerical scheme are you using for discretization?
c. And also try to check with your solver manual about the allowed aspect ratio of cells and also check for orthoganility? I guess your using quad cells(for 2D)?
d. From my experience I have seen the convergence problems ( especially when you have separation) because of cell aspect ratios in the wake region, just behind the trailing edge (ofcourse it also depends on what solver your using).

e. My advice is, try to keep the average y-plus below 2 and avoid below 1, because more cells ends up in viscous boundary layer than required(This also helps in in decreasing the aspect ratio) and in the outer part of turbulent boundary layer the number of cells will decrease?

Regarding the Turbulence parameters(length scale and Turbulent Kinetic energy) you used. Please refer the following webpage for further guidance.
http://support.esi-cfd.com/esi-users/turb_parameters/

I hope this will help you

Thanks for your reply

I attached my grid here

I didn't pay attention to wake before, I will look for some reference about that

[pavitran]

1. Increase the number of cells around the airfoil(about 500) and try to have a uniform cell size in the mid part of suction and pressure side.

2. Extend your outlet boundary further (approximately 4 to 5 chords). If possible, try to relax the clustering of the wake near the outlet boudary(I mean refine the wake region only upto 3 to 4 chords from the trailing edge).