Airfoil Coefficient of Lift and Drag - Published Data vs CFD Results
 

Hi, I’m looking for some advice about how to generate more agreeable results for lift and drag coefficient from my CFD CFX simulation of air flow across an airfoil. I’m fairly new to CFD, but have some experience in basic CFD analysis.

I have created a C-grid style mesh around my airfoil using ICEM and established appropriate boundary conditions in CFX-Pre. I’ve set my turbulence model to SST and aimed for a Y+ max < 1 across my airfoil.
I’ve performed a steady state simulation, checked residuals are converging to at least e-5 at both low and high angles of attack (AoA), and checked that monitor points for lift and drag appear to steady out with time steps. I’ve managed to roughly capture the trend of published data, but my coefficient of lift (CL) is still pretty different. As my CL results appear to get worse around stall (~14°), I thought maybe I needed to run a transient analysis for higher AoA’s, however, residuals at 14° AoA still appear to show reasonable convergence, so I’ve stuck with steady state analysis.

I’ve tried increasing mesh element count, reducing/increasing y+, reducing RMS target, and using different turbulence models (SST, k-ω, SA). No matter what changes I make, I can’t seem to achieve better results. I’m a bit stumped. As I’m fairly new to CFD, I was wondering if anyone could give me advice to improve my CL results. Thanks.

Attachment 76814

Attachment 76815

Attachment 76816

Attachment 76819

Attachment 76820

You appear to have missed two fundamental physics issues:

1) Your Re appears to be 128k. For most aerofoils this is a transitional Re number where there is a large laminar section and turbulence transition somewhere near mid-chord. You cannot model this with a standard 2 eqn turbulence model, these models all assume fully turbulent conditions. You will probably need to use a turbulence transition model to capture this.

2) Getting accurate results around stall is much more challenging than for other sections of the lift vs AOA curve. What generally happens is you start getting transient large vortex shedding, and again a traditional 2 eqn turbulence model cannot capture these sort of large scale transient features. You will need to consider LES, SAS or DES approaches to model this.

Note that you will be limited in options which cover both turbulence transition AND large scale vortex shedding. You may well find that you cannot model both of these physics at the same time. But hopefully you have a happy adventure trying them all out and finding out which one works good enough for you :)

Thanks very much for your quick response! I'll do some more research into the physics of flow separation and appropriate turbulence models.

I've done some further reading on low-Re flow characteristics and updated my turbulence model to transitional SST using the gamma-theta model.

I'm now struggling to reach convergence with my residuals, and my CL & CD appear to just oscillate. I've been analysing flow behaviour at an AoA of 5 degrees, and I think I can spot the point of separation and reattachment of flow around the mid-point of the airfoil, which I didn't notice before using just a 2 equation model - so I suppose this is probably a good thing.

Is there any advice you may give for achieving convergence? I've attempted refining my mesh by increasing element count, reducing my nodal growth rate to 1.01, and fiddling with time steps.

With turbulence transition at mid chord as I expected that means you definitely need a turbulence transition model.

I can also see that you have a classic laminar separation bubble - where the laminar boundary layer detaches from the surface, goes turbulent and reattaches. This attachment/reattachment forms a laminar separation bubble. So far so good.

But laminar separation bubbles are usually transient. They like to jiggle about, which means steady state convergence is challenging. While it is theoretically possible to damp this out in my experience the best way is just to use a steady state run to get close to converged, then switch to a transient simulation and run for long enough to get a few cycles so you can get a reasonable average CL or CD.

Comments on your attempts at convergence so far:
* finer mesh will make it harder to converge steady state, not easier (as the finer mesh has reduced dissipation). But the finer mesh should be more accurate.
* reduced growth rate will be useful as the laminar separation bubble happens a distance off the surface, so this means you will have better resolution of the bubble.
* Time steps - you probably won't get this to converge steady state regardless of time step size. When you do a transient run you should expect to need very fine time steps to get good convergence. But you only need to run a short amount of physical time so hopefully it is manageable.