drag and moment coefficient problem
I solved for the aerodynamic properties of a RAE2822 airfoil (hex meshed in ICEM) in fluent using the RANS density based solver and S-A model. Once the solution has converged 5e-6 i find through examining the force monitors that the lift is accuretly predicted within 1% but that the drag coefficient is over predicted by 20% and the moment coefficient is under predicted by 20%. I have refined the mesh however my answer does not change so i dont think this is to do with the grid refinement. For my turbulence specification ive used the viscosity ratio of 10. Ive tried playing with this and lowering it all the way to 1 but this has been no help.
Thanks for the help
Check to make sure your reference values are set correctly as these are used to calculate the force coefficients.
Although there appears to be alot of contradiction from what I've read in other posts the values to use seem to be with regards to aerofoils are:
Length = chord (usually 1)
Depth = 1 (unit measurement of Span)
Area = 1 (Chord*Span)
In another post someone said that for 2D the area is always equal to 1 and can be corroborated by the following books:
Milne - Theoretical Aerodynamics.
Anderson - Fundamentals of Aerodynamics.
As Fluent calculates the drag per unit area.
Length = Chord
Area = Chord*Span (Which I assume as the wetted area so just get Fluent to calculate it reports>surface integrals>area. Useful for complex geometries)
Someone else may have a different view but using the wetted area for 3D work has always give me decent results.
Hope this is of some help.
Thanks for the quick response I calculated the lift and drag coeficients as the components of the resultant aeordynamic force (i.e net effect of pressure and shear stress distribution) acting on the body. Therefore since my angle of attack was set to 3.22 degrees i have the force vector for my lift set to x=-0.0562 and Y=0.99842 and for my drag i have X=0.99842 and Y=0.05617. As well moment is calculated at the quarter chord. So my set up i feel is fine and ive checked my reference values which also appear to be ok. So i dont think the problem is in the set-up or maybee im missing something. Also, when i get fluent to print out the force report along the velocity direction vector i see that in adding the pressure coefficient and viscous coefficients to get the total drag, without the viscous coefficient the presssure coesfficeint is only 7% off of the actual value (7% lower) so does this mean my viscous contribution is too high? For the moment im still lost as to its 20% divergence from the accurate result
I would normally say adjust your turbulence parameters at the inlet to increase the turbulent dissipation but you have already done this. The same refining the grid as well to try and reduce the Cd. The only thing I can think of would be to check where you have applied grid refinement and make sure that the mesh resolution is sufficient. If you haven't tried it already you could refine the wake region by say 3-5 chord lengths.
The next thing would be to use a more complex turbulence model such as the k-w SST transition model to account for laminar to turbulent transition. Which should hopefully reduce the viscous contribution to drag and give you a more accurate result.
|All times are GMT -4. The time now is 04:01.|