Hydrofoil exercise to validate CFD analysis

Discussion in 'Hydrodynamics and Aerodynamics' started by quequen, Oct 1, 2014.

  1. quequen
    Joined: Jul 2009
    Posts: 370
    Likes: 15, Points: 28, Legacy Rep: 199
    Location: argentina

    quequen Senior Member

    Mikko, about "Flying the Virtual Moth", this is what I've done so far.
    The hull is a HungryBeaver, it's pretty coarse, I hope it's enough for the run.
    Appendages are from the Vendor2, using airfoil data found on the web.
    The T-Foil flap is not deflected.
    About rig and sail, I think you will do a far better job than me ;)
    I'm sending the iges files by p.m.
    Let me know what you think...

    -
     

    Attached Files:

    • Moth.jpg
      Moth.jpg
      File size:
      101 KB
      Views:
      1,250
  2. Mikko Brummer
    Joined: May 2006
    Posts: 549
    Likes: 69, Points: 28, Legacy Rep: 258
    Location: Finland

    Mikko Brummer Senior Member

    Great, thank you. I don't know when I shall have the time to simulate, I have 2 sail designs, one mast & one centerboard that are more urgent...
     
  3. Mikko Brummer
    Joined: May 2006
    Posts: 549
    Likes: 69, Points: 28, Legacy Rep: 258
    Location: Finland

    Mikko Brummer Senior Member

    You are right - I was not thinking the motion is against the free surface, it will not work as Quequen's case shows, at least not if you treat free surface as a symmetry plane. It would depend on how your software treats moving walls or a morphing mesh, or free surface that matter. Filling the tank from the bottom would be quite a clever way to fool the motion into the software.
     
  4. Leo Lazauskas
    Joined: Jan 2002
    Posts: 2,696
    Likes: 151, Points: 63, Legacy Rep: 2229
    Location: Adelaide, South Australia

    Leo Lazauskas Senior Member

    For those interested in optimizing hydrofoil profiles, the following paper has
    just been published on-line.

    M.H. Djavareshkian and A. Esmaeili
    "Heuristic optimization of submerged hydrofoil using ANFIS–PSO",
    Ocean Engineering, 92 (2014) pp. 55-63.

    In this research, optimization of shape and operating conditions
    of a submerged hydrofoil is investigated by a heuristic optimization
    approach, been a combination of an adaptive network based fuzzy
    inference system model (ANFIS) and particle swarm optimization (PSO).
    The constrained discrete variables such as the thickness and camber of
    hydrofoil, angle of attack and submerge distance are clearly defined as
    design variables and the lift to drag ratio is selected as a nonlinear
    objective function, which is extracted from an accurate numerical
    procedure. The Navier-Stocks equation is numerically solved, and volume
    of fluid (VOF) method has been utilized to simulate two-phase fluid
    (water and air). The results demonstrate that the resulted body of the
    hydrofoil in the optimum operating conditions should reach a maximum
    value of lift to drag ratio.
     
  5. nico
    Joined: Jan 2003
    Posts: 190
    Likes: 6, Points: 0, Legacy Rep: 52
    Location: SF

    nico Senior Member

    Interesting topic! Based on my experience, here are some comments:

    On the meshing side: this geometry would require around 4-5 millions of cells to reach a descent accuracy. Y+ values between 30 and 100 are needed (low y+ < 1 would be great but not required). Refinements along the leading and trailing are required.
    The above is for meshes in polyhedras, a hexa mesh (~structured approach as in Pointwise or Icem) would require 1M cells less, a tetrahedra mesh 3-4M more (for a total around the 8M mark).

    On the solver side: a 2 equations turbulence model is the norm and will get you accurate results. Convergence is reached once residuals (momentum and continuity) go down by 3 or 4 orders of magnitude AND all forces are steady (good criteria is taking the last 200 iterations, computing min and max of those, difference should be lower than 1% of the mean).

    Finally, do not ever believe CFD results without being shown a mesh refinement study. This is something pretty basic; it involves checking numerical errors (google Roache and uncertainties in CFD for more).
    Such process involves running meshes of varying size (for the above it would typically be a 2M mesh, a 4M and a 8M mesh). Each variable of interest (e.g. lift and drag) are then plotted against mesh size. If you get convergence of results (i.e. error is getting smaller as you refine the mesh), great; you'll then be able to estimate numerical uncertainty (typically in the range of 1-3%).
    If you don't get any convergence (e.g. results keep changing while refining), your mesh or the solver is most probably wrong and you're in trouble!.

    Hope this helps,
    Nico.
     
  6. daiquiri
    Joined: May 2004
    Posts: 5,373
    Likes: 255, Points: 93, Legacy Rep: 3380
    Location: Italy (Garda Lake) and Croatia (Istria)

    daiquiri Engineering and Design

    Do not believe the CFD results even if the mesh refinement study shows convergence. This analysis only tells you whether the numerical solution converges to a well-defined value as the mesh gets denser. But it won't tell how far is the converged result from the true value. In order to get that, you need to compare the results with reliable experimental data. ;)

    Cheers
     
  7. Mikko Brummer
    Joined: May 2006
    Posts: 549
    Likes: 69, Points: 28, Legacy Rep: 258
    Location: Finland

    Mikko Brummer Senior Member

    Agree with you in general, but in this case I believe Quequen can pretty much rely on these numbers for preliminary design, considering how close several different software and even basic hand calc all agree. Except that free surface is ignored.
     
  8. Mikko Brummer
    Joined: May 2006
    Posts: 549
    Likes: 69, Points: 28, Legacy Rep: 258
    Location: Finland

    Mikko Brummer Senior Member

    The software Quequen is learning here (Solidworks Flowsim) differs from traditional CFD in that it utilises a cartesian grid and relies heavily on a two scale wall function, as explained in the paper referred in post 21 by Joakim. Refining the mesh close to the wall therefore only helps that much, and on the other hand you get reasonable result with even less than 1 million cells.

    I actually did an ad-hoc grid sensitivity test on the results I had, but didn't have the time to post it. If you look at the attachment below, in terms of L/D something like 750 000 cells will give results for preliminary study of forces. I didn't do more than 2 million cells, maybe 3 million or so cells would still influence the result, but you have the time explore so many more variations if you contend with less, working on a desktop PC.

    Definitely agree that any serious CFD project starts with a mesh refinement study. Saves you plenty of time in the end, too.

    The other attachment shows the boundary layer with the mesh 2 million cells, you can see that there's barely one or two cells within the boundary layer. The wall functions handle this.

    For more realistic results allowing for the free surface piercing, you should at least give up symmetry at the surface, and maybe submerge the foil a bit. I did a run with the foil submerged 10% of the vertical strut height, see 3rd attach. The vertical lift changed little, but about 13% of the lateral force was lost, you can see the effect in the velo distribution in the upper strut and the isolines of relative pressure.

    Nico, what about the ambient turbulence in the sea? What value of inflow turbulence intensity do you think would be appropriate for a foil at this submergence? Relatively little turbulence will prevent most laminar flow on the foil.
     

    Attached Files:

  9. quequen
    Joined: Jul 2009
    Posts: 370
    Likes: 15, Points: 28, Legacy Rep: 199
    Location: argentina

    quequen Senior Member

    This Flow Simulation technical paper explains some of the virtues (beyond simplicity and rapidity) of cartesian grids.

    -
     
  10. Mikko Brummer
    Joined: May 2006
    Posts: 549
    Likes: 69, Points: 28, Legacy Rep: 258
    Location: Finland

    Mikko Brummer Senior Member

    A question that comes to mind, why are these L-foils always directed inwards? One would think that outwards they would give you a large gain in righting moment? A collision hazard with outwards directed foils? Or something else I've missed,
     
  11. daiquiri
    Joined: May 2004
    Posts: 5,373
    Likes: 255, Points: 93, Legacy Rep: 3380
    Location: Italy (Garda Lake) and Croatia (Istria)

    daiquiri Engineering and Design

    The main reason is hydrodynamic one. You have to think about how lift force and induced drag are related to each other. If you recall the lifting-line theory (LLT), it essentially tells you these important things to know:
    1. the local circulation around the wing section at a given spanwise point of the wing is directly proportional to the lift coefficient at that spanwise point;
    2. the local vortex strength in the wake at a given spanwise point of the wing is proportional to the spanwise rate of change of the circulation at that spanwise point of the wing;
    3. the induced drag is proportional to the cumulative strength of the vortices making the wake.
    Now, an inwards-bent L-foil set at a positive angle of attack and subject to a leeway, has a pressure system which sees all the points of low pressure placed on the inwards surfaces (both horizontal and vertical). Hence, the local lift coefficients will be of the same sign along the entire span of the foil. It means (see the above extracts from the LLT) that the circulation around L-foil sections will gradually change from the root to the tip of the foil, with a single peak. A gradually changing circulation in the spanwise direction translates into low-energy trailing vortex sheet. Hence, low induced drag.

    In case of an outwards-bent L-foil working under the same conditions, things are very different. The horizontal part of the foil would see low-pressure points on the upper surface, while the vertical part would see it on the inwards surface. Hence, starting from the root and moving towards the tip, there would be a point where the sign of the lift coefficient changes, and hence the sign of the circulation too. For the same overall foil length, it implies two spanwise peaks (one high and one low) in the distribution of circulation and hence a much higher values of its spanwise rate of change. Which in turn means a stronger wake vortex system - hence, a higher induced drag.

    So, resuming it all: an inwards-bent L-foil has a much lower drag than an outwards-bent foil, for the same lift and leeway force. It was seen in practice that the drag penalty of the outwards-bent L-foil outweighs the gains due to higher righting moment.

    Hope it was clear enough. If it wasn't, I suggest you to go through the LLT equations, and it will be all much clearer. :)

    Cheers
     
  12. Mikko Brummer
    Joined: May 2006
    Posts: 549
    Likes: 69, Points: 28, Legacy Rep: 258
    Location: Finland

    Mikko Brummer Senior Member

    Totally clear, thanks. Has it been seen indeed in practice, that the drag penalty outweighs the RM advantage? Actually, this would drive you to the DSS foil, where the vertical & the lateral forces are kept all separate.
     
  13. daiquiri
    Joined: May 2004
    Posts: 5,373
    Likes: 255, Points: 93, Legacy Rep: 3380
    Location: Italy (Garda Lake) and Croatia (Istria)

    daiquiri Engineering and Design

    A quick search returned me this post by D. Lord: http://www.boatdesign.net/forums/mu...trimaran-test-model-36058-115.html#post704177 in which he reports a testimony by Greg Ketterman, the boss of Hobie Cat Co. Check it out! ;)

    Cheers
     
  14. Doug Lord
    Joined: May 2009
    Posts: 16,680
    Likes: 346, Points: 93, Legacy Rep: 1362
    Location: Cocoa, Florida

    Doug Lord Flight Ready


  15. daiquiri
    Joined: May 2004
    Posts: 5,373
    Likes: 255, Points: 93, Legacy Rep: 3380
    Location: Italy (Garda Lake) and Croatia (Istria)

    daiquiri Engineering and Design

    In that particular case (Open 60), the things change because vertical lift and sideways force have been physically decoupled, just like in the case of DSS. Vertical lift force is produced by the L-foil, while the biggest part of side force comes from the keel. The vertical strut of the L-foil works at a much smaller leeway AoA, because the main keel makes it possible, being a much more efficient producer of sideways force. So the L-foil experiences much smaller variations in spanwise pressure field, regardless of the direction it is bent into (inwards or outwards).
    And besides all that, when compared to a monohull with no lifting appendages, it is imo pretty clear that any solution which provides the vertical lift with a good L/D ratio at high speeds plus an additional righting moment, will be beneficial.
    Cheers
     
Loading...
Similar Threads
  1. S V
    Replies:
    0
    Views:
    639
  2. Eytan Levi
    Replies:
    0
    Views:
    790
  3. container
    Replies:
    7
    Views:
    2,627
  4. vejas
    Replies:
    34
    Views:
    7,764
  5. revintage
    Replies:
    8
    Views:
    1,695
  6. revintage
    Replies:
    14
    Views:
    11,586
  7. rallyhybrid
    Replies:
    39
    Views:
    4,361
  8. optiwings
    Replies:
    1
    Views:
    1,635
  9. Tommifin
    Replies:
    5
    Views:
    1,949
  10. Ittiandro
    Replies:
    2
    Views:
    4,891
Forum posts represent the experience, opinion, and view of individual users. Boat Design Net does not necessarily endorse nor share the view of each individual post.
When making potentially dangerous or financial decisions, always employ and consult appropriate professionals. Your circumstances or experience may be different.