Lift/Drag prediction Foil FX 78-PK-188-20
 

Hello,
currently I'am calculating the drag polar and the lift envelope for the aerofoil above. Even with intensive investigations I become not satisfying results.

I have done several calculations with different meshes to get the mesh independent solution. The calculation area is a 3d swept mesh with one element in dept.

First I tryed steady simulations with a unstructured mesh and changed the AOA in several design points for getting the fully polars in one run.
I obtain very better results when using the Gamma Theta Transition model. But then I have to do transient runs for the reason of laminar separation bubbles. For better results I also tryed a better mapped mesh where I change the angle of the incoming air.

When looking at the lift envelope there is a short lift drop between Zero degree AOA and the total separation. (laminar turbulent transition moves to leading edge) In the simulation this appears later and therefore to big lift is calculated for the AOA above this point.
-Avarage Yplus is about .5 (may plus <1) as in the limit for good boundary layer resolution neccesary.
-observed no deviation in results when using more than 300 knodes at the foil contour (in stream direction)
-The distance to the boundaries is about 20m.
-Tu is low <1%

Now I have absolutely no idea what else to change in the simulation, to get better results. Thanks for every helpful advice!

Your results are close - so you know you have the basics set up correctly. But to get the result accurate to those last few percent requires careful work.

* You have done a mesh sensitivity check (excellent) but the quality of your mesh is not great. There are several high aspect ratio elements I can see. Have a look how other researchers mesh airfoils, especially the C grid method.
* You need to check some of your other assumptions with sensitivity analysis: boundary proximity, convergence tolerance, time step size (for the transient runs).
* Also check how sensitive your simulation is to inlet turbulence levels and surface roughness on the airfoil.
* Are you using a second order advection scheme?

Hello Glenn,
fast answer, that is fantastic! :)
I will try to improve the mesh when all other suggestions will not help. So I have to reach lower AR right?

* Are you using a second order advection scheme?

" SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Maximum Number of Coefficient Loops = 5
Minimum Number of Coefficient Loops = 1
Timescale Control = Coefficient Loops
END
CONVERGENCE CRITERIA:
Residual Target = 1e-06
Residual Type = MAX
END
TRANSIENT SCHEME:
Option = Second Order Backward Euler
TIMESTEP INITIALISATION:
Option = Automatic"

Thank you very much!

Yes, you want the aspect ratio to approach 1. The C grid is good here because if you expand the radial mesh spacing in proportion to the radius then you get approximately aspect ratio 1 elements all the way out.

* The hires advection scheme will revert to upwinding (ie first order) in some areas. Check the velocity.beta variable in the post processor to see where it has gone first order. In your case I would suggest using a purely second order system like hybrid with the blend factor=1.0.
* Make the max number of coefficient loops larger, 10 is a good number.
* Your convergence tolerance is very tight. Are you sure you need it that tight?

Hello Glenn,

I have tryed a better mesh qualtity but the results will not improve.

A only second order advection scheme neither.

Wall roughness will not have much influence because the surface of aerofoils is very smooth, so that it can be managed as hydraulical smooth.

Wall proximity has a large influence for my drag values but they will not reduce the lift. - thats the point, it looks like cfx is overshooting lift for the reason of delayed separation or specific the laminar transition.
There is the typical buckle in the lift envelope, where the transition onset is equal to the leading edge. Then only turbulent boundary layer covers the suction side till separation, which declares the fast increase of drag.
For that reason I thougt my results are strongtly dependent on inlet turbulence but even when changing the intesity I have no remarkable changes.

Additional I have observed that the staedy state runs give nearly the same results, even when theire convergence did not fall below max Resi 1e-2! (transient: max Resi stable 1e-4, total time 4s, TS = 0.001s...0.01 s)

Now I have absolutely no idea what I can change. :(
In the some papers from ansys I have seen they have gained very reliable drag polars and lift envelopes.

Thank you very very much!

Have you looked at upstream turbulence levels? Also I have had some success in the past by applying wall roughness in excess of what the physical model actually had. Worth a try at least.

Your mesh does look higher quality but you still have some high aspect ratio elements near the trailing edge. But this is probably not contributing much to the problem.

Do the papers you have describe what they did in detail?

Well in one paper they also recognized this lift overshoot, they fixed it with an "in-house existent" correction implementation for the SST model. I have read the location of transition may be strongly dependent of Inlet viscosity ratio. For now I did not varied this value because in post, it seems that the free stream is very laminar, which I classified appropriate.

Using 1st order turbulence numerics instead of HiRes gives more unrealistic results althoug better convergence can be observed.

I will now try several roughness values and also use some other fixed inlet viscosity ratios. Is there a different to enter the roughness by wall-boundary or by transition model options?

I do not understand this question.

Sry I was not reading correcticly. At boundary condition "rough-wall" you have to enter the equivalent sandgrain roughness and when setting a roughness at the wall you have to enable the roughness correlation for Gamma Theta Transition by entering the geometric roughness - as said in the ansys manual.

Unfortunately this did not reduce my lift prediction. Maybe I have chosen the wrong values.

In some literature I found possible roughness values for wing surfaces about ks=0.002mm. As far as I understood the different notes and indices this must be the equivalent sand grain roughness right? But how can I determine the geometric roughness then? ... I have read the chapter in Schlichting (boundary layer theory) about this, anyhow I can not figure it out.

I have also changed the Inlet turbulence and eddy viscosity ratio so that a min. turbulence > 0.1% around the profile is ensured. (belonging to ansys manual) Nevertheless lift prediction gives an overshoot. Higher free stream turbulences will give correctly lift reduction but for the cost of strong drag increase.

Hello matmax, I am trying to do a similar approach as yours for a whole glider I am using inflation techniques and proximity curvature method, my mesh looks fine I'm getting values of y plus lowers than one but I am interested to learn how you set up your mesh? Also can you teach me how you set up your solver and your approach to get polars in one single run?