Hydrofoil exercise to validate CFD analysis

The foil is an asymmetric section, thus it will produce a considerable sideforce at zero AoA, which may or may not be equal to leeway depending on the angle of the foil. So all the simulations shown contain both lift and sideforce.

 

As the vertical fin is asymmetric, too, there is actually plenty of lift against leeway already (the lateral or horisontal lift in the calcs).

What Quequen ought to do is find out the righting moment of his dinghy, calculate the sail/wingmast sideforce that produces that righting= heeling moment, and then with his estimated boatspeed see what leeway angle would match that sideforce.

 

You should set k and epsilon or watherever your turbulence models needs to the values observed in sea. They do not change with the speed the foil travels, thus it is not sensible to describe the turbulence intensity at the inlet, since that would means k depends on the square of that speed. So defining 1% at 8 m/s is equal to 4% at 4 m/s.

I once found a good article about measured k in an ocean at different depths, but I have lost it.

Also depending on epsilon and your domain you may get very much different turbulence values near the foil. There is no production of k before the foil. If you have a huge domain before the foil, you will have very low turbulence level once the flow gets to the foil. Setting epsilon too high "eats" all the k very rapidly.

 

Mikko, if you remember my paper on turbulence levels, 0.1% to 0.2% would be an appropriate value for inshore waters below the surface. In the surface layer the TKE is much higher, depending on wind forces and fetch.

 

Good info, but what depths are we talking about? These hydrofoils work on average at less than 0.5-0.6 meters below the surface.

 

Attached.

 

FWIW, everyone I've talked to about transition in water indicates that it happens earlier than in air. Turbulence may be part of it, but also biomass, sediment, dissolved air, etc.

In the e^n method of predicting transition, an ncrit value of 1 - 3 appears to be be appropriate.

 

The value of leeway will depend on the aerodynamic side loads from the rig. So it's not possible to set a leeway angle when analyzing the foil alone. One needs to run a range of leeway angles, then include the forces vs leeway in a VPP to see what leeway angle settles out.

 

Besides the leeway angle, there is the angle of attack in the vertical plane to consider, too. A range of rake angles should be run to vary the vertical force. And because leeway affects the vertical force, there should be combinations of leeway and rake added to the matrix.

All of that is fine if one is only interested in performance, where the velocity vector can be assumed to be parallel to the water surface. However, if one wants to consider dynamic situations, such as takeoff or maneuvers, then the velocity vector will not be parallel to the surface, but have a vertical component. For example, a dagger foil that is descending will have a larger angle of attack on its wing than a foil flying level with the same rake angle.

How can this be handled in a RANS calculation? Is it as simple as adding a vertical component to the boundary conditions on the foil surface instead of zero slip?

 

The boundary condition on the foil is still zero slip (wall), but you simply add a velocity component in the Y-direction at the inlet (assuming that the sea surface is in x-z plane). The most advanced CFD-codes with motion capabilities can do this through real physical simulation, including gravity, inertia etc., up to 6 degrees of freedom (DOF). Like the Star sailing in the attachment under real sail forces, finding its leeway angle after some initial sideslip, and pitching & heaving in the simulated waves.

If somebody gives me a moth-model, I will make it fly - or a AC-62 will do just as well ;-).

 

Now that you mention it, I vaguely remember... so many things I forget these days. Perfect, thank you. I include the paper here, if I may, for those who missed it.

 

Interesting paper, also giving food for thought regarding internal flows; thanx Uli and Mikko for producing and sharing!

 

That's really great - thanks! It explains a lot of the difference observed between aeronautical results and sailing tests.

 

Changing the inflow boundary condition was the first thing I thought of, but is there an effect on the free surface? Or is the free surface undisturbed but moving upward (like a large tank being filled from the bottom)?

Is a quasi-steady simulation valid under such conditions?

 

More or less: where I work they have 30 full SWpro network licences and I access one of them when possible. I also have access to the free academic version of Autodesk Simulation CFD, which should be better than FS, but is too difficult to use, I simply don't get it.

I must say thankyou to all the contributors to this threat, it has become awesome! I will print it, frame and put it on the wall