Hi,I am trying to calculate lift,drag and moment coefficient for a NACA0012 at different AOA.I ve runned the simulation and post processed the results in CFX.Apparently i ve got very good results.My problem is that i dont know which variable correspond to the lift and drag forces.I though it was 'Force Y' for lift and 'Force X' for drag,but I ve got very small values....E-7 order...definetly too small.Can anyone suggest a proper way to find out my lift and drag forces? Thank you.

Franny

Hi, ForceY and ForceX (normalised by projected areas should give you Lift and Drag coefficients. I assume that your freestream flow is along X axis. If you are giving an angle of attack by changing the flow direction, you then need to take components perpendicular to and along flow direction respectively. Alternatively, you can extract the pressure values around the airfoil and integrate them to get the lift and drag forces. This will however not give you viscous drag. So the best option is still to use the ForceX and ForceY from CFX post. If you want to see viscous and pressure drag breakups, you can use Normal and Tangential ForceX and ForceY.

Shastri

Hi thank you for your message.Yes, the free stream is along the X direction and the angle of attack is given by changing the flow direction and not the wing position in the fluid domain. I ve extracted teh force in the X and Y direction by postprocessing my results and then i ve calculated the relative components along and perpendicular to the flow direction.Lift and Drag founded for each value of force X and Y as L=-Fxsin(a0a)+Fycos(a0a) and D=Fxcos(a0a)+Fysin(a0a),integrated all over the airfoil but Cl is still very small(10-7 order). About the other method, using pressure distribution,to calculate Cl and Cd i assume i need to distinguish between lower and upper surface right? And finally,in the variable selection in CFX i ve decided for 'Force X' and 'Force Y',but you mention 'Normal and Tangential ForceX and ForceY'...do i have to try with that ones?

Hi, the method of calculation seems alright. I would first check the units. You might have accidentally imported the mesh in mm or inches instead of meters. To calculate using pressure, yes, you need to distinguish between upper and lower surfaces. You can actually create a polyline that passes through the airfoil profile and export pressures on that polyline. You can later split the data in Excel/Matlab at points with Min and Max X for leading and trailing edges respectively. You can calculate the forces Fy and Fx and proceed to calculate as before. The normal and tangential components wont give you answers different than the regular ForceY and ForceX so that wont solve your problem if something is basically wrong in simulation itself. But you can use them to do a detailed study of your errors. I remember that you can extract them by choosing particular plot lines in the solver manager.

My first doubt would be on units so just check lengths, velocities etc are all as they should be. Hope this helps. Shastri

BTW, I hope you are deviding the Fy and Fx values by normalising factor (0.5* rho* u^2*chord*span). THAT gives the value of Cl and Cd, not the forces themselves.

Hi Shastri,thank you very much for your help.Off course i m dividing the aerodynamic forces by the dynamic pressure,not problem about that.I will chech this morning about the unit of measure,but the value i ve got for the pressure on the polyline are reasonable,the plot as well and most important the boundary layer that i see above the wing is amazingly good....i can see all the velocity profile evolution along the surface till the small separation bubble.This is for me was a good sign that the simulation was right.I will check the units and i will let you know.Thank you again. Ciao

Franny

Guys,

I ran into an issue with the CFX POST function "Force", it only calculates the pressure forces (isotropic) and not the normal component of the viscous stress. This can give considerable errors. Use the .out file to get your results.

Hi Anil, thank you for your advise.This is what i ve found out yesterday.From my results file at the end of the simulation,i summed the pressure force to the viscous one and i ve obtained reasonable values for Cl and Cd.Unfortunately they looks like the half of what they should be.For a Naca0012 at 15 deg theory sais Cl=0.8, I ve got Cl=0.4.What do you think?

Franny

Franny,

As the factor is a round number like "2", do you have a factor 0.5 in the dynamic pressure, basically 0.5*rho*u*u? I would suggest use 'xfoil' results to compare your pressure distribution, if they match then you know it is the lift calculation formula.

Anil

hi,will u please give me the exact procedure to find the drag in CFX post using pressure-distance graph.

[hari.poudyal47@gmail.com]

Hello everyone,

I am now trying to calculate drag coefficient using Meshless MPS method.
I am now using Pressure for calculating drag coefficient but the result
is not good. So, if anyone has idea about calculating drag coefficient,please share with me too.

Your sincere
Hari

[ghorrocks]

This is the CFX forum. No meshless MPS methods are being used here.

[hari.poudyal47@gmail.com]

Dear ghorrocks sir,

Thank you very much for your response.
Do you know any reference or any other MPS related papers about drag
coefficient.

I will be really thankful for your kindness.

Your sincere
Hari Poudyal

[ghorrocks]

http://www.lmgtfy.com/?q=Moving+Part...mplicit+Method

[hari.poudyal47@gmail.com]

Dear ghorrocks sir,

I am working in MPS method since 1 year.
I know MPS method ( but not too much). So, I am facing problem
for calculating force from pressure distribution. ( just P = F /A is not sufficient.)

Any way, thank you very much for your link.

your sincere
Hari Poudyal

[hari.poudyal47@gmail.com]

Hello Everyone,
I am calculating drag coefficient. I found a fluent guide to calculate the drag coefficient.

https://confluence.cornell.edu/displ...irfoil-+Step+7

But I have a confusion about unit vector in drag force calculation.
It has been written as "ed is the unit vector parallel to the flow direction".

If the flow direction is along X axis, then can I use "ed" = (1,0,0) or should I calculate the instantaneous velocity component along X direction?

If anyone has any idea, please share with me.

Yours sincere
Hari

[esha]

Hi, I am trying to calculate Cd and Cl for 3D airfoil having dimension 4c in spanwise direction, and free stream is in x direction . As I know, in Fluent I need to just select the direction vector as x=1 y=0 z=0 for drag coefficient and x=0, y=1 and z=0 for lift coefficient. I already have selected area in reference values. But in a video I have seen, it was changing the z value also. If I am wrong please correct me because I do not know much about 3D simulation. I t is my first 3D simulation.
Thank you!