Keel profiles, blunt trailing edge and xfoil/XFLR5

I plan to fair the lead keel of my 35' C/R sailboat from 2005. The chord is about 1 m, the trailing edge is now 14-17 mm thick and the span is 1.53 m. Also the profile is not that fair. I don't know the profile the keel is supposed to have (both the designer and the yard refused to answer that), but it seems to be something like NACA 64A-015, which should be OK. I'm trying to minimize the work needed for fairing.

I have simulated some profiles with XLFR5 (should be identical to XFOIL, which I have used earlier), but I'm wondering how well does it predict the trailing edge effects.

I can't reproduce these measurements: http://ntrs.nasa.gov/archive/nasa/casi.ntrs.nasa.gov/19930082748_1993082748.pdf They show a huge additional resistance at low Cl values for 4% (40 mm) and also rather clear for 1.4% (14 mm) trailing edge. The XLFR5 prediction shows about the same Cd change at high Cl values, but not at all the clearly bigger change at low Cl values, which are the most important ones to sailing.

Are there other measurements for blunt trailing edges? For 6-series?

 

There are two issues here, both of which effect the "real" hydrodynamic answer. First, XLFR5 and XFOIL are not vortex solvers, which is needed for a problem like this. Second, do not expect aero data to be replicated by hydro data when it comes to sharp trailing edges. The extreme mass to kenetic viscosity difference for similiar Rn makes water behave very differently than air. Depending on speed, AoA changes, etc, it is often advantageous to cut the TE off sharp and form a "bound" closed vortex flow which fills in the streamlines generating an "apparent" cord length and a smoother seperation point.

 

Yes I know XFOIL is a panel code and full Navier Stokes would be better at this, but it is much more time consuming and there is a model for blunt trailing edges in XFOIL, thus I thought it may be able to reproduce the results.

Can you be more specific about the the differences between water and air at the same Rn? I have never seen them unless there is free surface, cavitation or compressibility effects.

 

By "vortex solver" do you mean a vortex lattice method?

 

No, it's not about method, it's about the equations you solve. XFOIL is a panel method software and panel method assumes non-viscid streamwise flow. It also has a correction for boundary layer, which a pure panel method doesn't care about.

Panel methods do not see viscous effects, which are very important for flows around bluff bodies like blunt trailing edges. Thus XFOIL has a correction for blunt trailing edges, but it doesn't seem to capture the measured effect for NACA 0012 at Rn 3-6e6.

There are many ways to take the viscous effects into account. The most used one would be a CFD software with a turbulence model, but it is not easy to get accurate Cd values (and Cl, but that is easier) for different profiles with them, especially for cases with partially laminar boundary layer and transition and separation somewhere during the profile. It's all about minor details in the boundary layer flow, which will depend much on the grid and turbulence model used.

XFOIL is a more accurate tool for normal profiles, since it is specially tailored just for those.

 

My question was intended for jehardiman, and was about method. He was the person I quoted.

 

I wouldn't count on CFD giving good results for drag or lift with a blunt trailing edge. I don't think most CFD codes with turbulence models work particularly well in predicting the pressure behind the blunt trailing edge.

 

The large drag increase around zero AoA is almost certainly due to unsteady vortex shedding which occurs with a sufficiently large blunt TE. A nonzero AoA will tend to quash this shedding, which is why you see the drag minimum for nonzero AoA.

To properly capture the vortex shedding with a Navier-Stokes code, you will have to run it in time-accurate mode and with an extremely fine grid which is fine "everywhere" in the wake where the vortices occur (not just near the x axis). The result will be extremely long calculation times, which you will then have to post-process to do the necessary time averaging to get the time-average forces. About 8 years ago a PhD student working for Jake Kerwin here did something like this for a "cupped" 2D hydrofoil section which was known to shed vortices. A typical run for one AoA required something like a week of CPU time to get a grid-independent and statistically-steady shedding solution. Might take "only" 1-2 days with today's machines. Still, it's not for the impatient.

 

So the blunt trailing edge model in XFOIL does not take into account vortex shedding at all?

Yes a grid that is fine everywhere is needed for vorticies. I did a lot of CFD modelling for impellers in mixing tanks during 90's and it was the same thing. You needed a fine grid everywhere in order to capture tip vorticies and thus correct turbulence levels and velocity profiles. It was better to use overall fine grid and wall functions than a one with fine grid at the walls for the low reynolds number model.

But does it really have to be that fine? 8 days? Was that for a single processor or parallel? Or was it LES? I would think you could capture the vorticies with a much smaller computing time, but not as accurately. Or will a turbulence model dampen out the vortex shedding and fail to capture its effect on drag?

 

In the broad sense no, not the vortex lattice method used for wings, but rather similiar but not on a marco scale; i.e. a specific portion of the flow is modeled as a vortex.

There are situations were we know from flow evidence that bound vorticity is present. Rather than use an ultra fine grid as markdrela stated (in which you can never be sure if the vorticity is just a grid artifact), significant computational time can be saved by injecting a "known" vortex into the solution, similiar to what Joakim proposed. The problem with such solutions is what happens when the vortex doesn't form? I know of a "Multi-Vortex" CFD program developed over 10 years ago for a particular application. It works very well in certian flow conditions, and totally fails in others. In my experience, the bound vortex flow in truncated symetrical foils falls into the arena.

 

I did a quick test and was able to capture the lift quite well even with a very course grid.

Measurements for NACA 0012 at Rn 3-6e6 are at zero angle Cd ~0.006 (smooth) or 0.008-0.01 (tripped) and at 8 degree Cd is 0.009 (smooth) or 0.01-0.018 (tripped) and Cl a bit under 0.9.

With only 14 000 cells and standard k-e turbulence model with wall functions I got at zero angle Cd=0.0196 and at 8 degree Cd=0.053 and Cl=0.746. Thus very bad for Cd, but "only" ~15% wrong Cl.

With 38 000 cells and k-w SST turbulence model without wall functions I got at zero angle Cd=0.00926 and at 8 degree Cd=0.0168 and Cl=0.868. Thus now Cd's are close to tripped values and Cl is very accurate.

With much denser grid (230 000) and bigger modeled area you can get even better results: http://turbmodels.larc.nasa.gov/naca0012_val_sst.html

For the cut version of NACA 0012 cut at 0.875 chord (4% thick te) the measured values show at zero angle Cd=0.019 and at 8 degree Cd=0.014 and Cl~0.95 (all for the cut chord length).

With the course grid and standard k-e I got at zero angle Cd=0.0278 and at 8 degree Cd=0.0616 and Cl=0.810. Thus even the course grid shows the added Cl and Cd compared to normal NACA 0012, but Cd's are clearly too high and the low value for Cd at 8 degree is not predicted. Both show signs of instability possible due to vortex shedding.

With the denser grid and k-w SST I got at zero angle Cd=0.0114 and at 8 degree Cd=0.0179 and Cl=0.914. Thus Cl is accurate again and Cd's are similar to what XFOIL shows. Thus they show just a slight increase from normal NACA 0012, not the huge increase at zero angle. This simulation (when run time dependent) shows clear signs of vortex shedding at ~20 Hz, but probably the grid is not dense enough to really capture it and the added resistance. The frequency equals to strouhal number of 0.27 for the trailing edge, which seems to be the right order of magnitude.

The measurement had a much higher frequency due to different fuild and scale at the same Rn. Probably around 1000 Hz. Is this why they had no idea about the reason for the increased drag? Or is it even the cause?

Will vortex shedding occur at the same Rn or will it also depend on scale or fluid?

Attached are some pictures from the simulations.

 

This link isn't about keel trailing edges, it's about prop nozzle trailing edges. Apparently a rounded over trailing and leading edges have benefits in hydrodynamics.
http://www.olds.com.au/marine/maximizing_propulsion_efficiency/

 

I run just one simulation more. The 4% thick case with zero angle with a 64 700 cell grid that was denser than before behind the trailing edge. I first started as steady state, then with 0.01 s time steps and the solution converged nicely to Cd=0.0128. Then I just left it running over night with 0.0001 s time steps (from about 41 s). And there it was! Nice cyclical pattern for Cl and Cd with vortex shedding. The Cl varies +-0.07 with an zero average and Cd varies 0.025-0.029 with an average of 0.0234, thus somewhat higher than the measured ~0.019. The simulation was done with water and Rn=3e6 (1 m chord 3 m/s) and the measurement with air at Rn=6e6. The grid is certainly not dense enough to accurately predict added resistance from the vortex shedding. The frequency is 16.7 Hz which means the strouhal number is 0.195.

Here are some pictures near the maximum and zero lift.

 

Very nice work. I assume these are "two dimensional" calculations.

 

Thanks! And yes.