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Lofting problem wing with gurney flap

robert_horton034robert_horton034 Member Posts: 6
I'm creating a wing shape that will be 3d printed. It helps a lot to have a flat edge which will be the side that lies down on the bed of the printer. I've lofted the wing shape and I'm using the trailing edge of the wing to be the edge that lays on the bed. This way the entire wing can be printed without support. So far so good.

A print needs a decent surface area to successfully print; something for that first layer to attach to the bed. Since the trailing edge of the wing is very thin, I'm adding a sizable gurney flap onto that wing trailing edge so that the print has a decent-sized contact with the bed.

Where I run into a problem is in lofting the gurney flap so that it matches and connects to the lofted wing profile. 

https://cad.onshape.com/documents/79305a673201200f8bc2a108/v/2f456a921951e6c48334788d/e/87dce962878413a7ad0544d6

I've been through the reference guides, the tutorials, and a variety of videos. The loft of the wing works fine but connecting it to the gurney flap has me stumped. I can't find any way to make the wing profile include the gurney flap. I spent several weeks on that attempt. 2d drawings can't be merged into a part. Every time I attempt to loft either the wing profile or the gurney flap as separate lofts that I will then use binary to merge fails because I can't get any lofts to follow a guide or a path. I created a 3d spline that matches the trailing edge but it refuses to use the spline as the path. 
Above is the wing profile with the gurney flap.



And this is where I get stuck attempting to loft the flap.

Comments

  • glen_dewsburyglen_dewsbury Member Posts: 77 ✭✭
    I think I see what your looking for. I use 2 profiles as expected then added a 3D fit spline to force the trailing edge straight. Followed with a box shape sketched on the same planes as profile sketches to loft the gurney flap. Make sure the top of the box shape is inside of the original profiles to avoid non manifold condition when you use add for the second loft.
    https://cad.onshape.com/documents/12b0679a712bc6f544f72c07/w/67e973d9c8c7d9393a467fa0/e/966b75c44db58304ecde3538
  • robert_horton034robert_horton034 Member Posts: 6
    Glen, yours looks like the simplified version of exactly what I'm attempting. I just haven't been successful at getting the second loft to follow the 3D fit spline. I'll play with it some more.
  • glen_dewsburyglen_dewsbury Member Posts: 77 ✭✭
    The simplified sample doesn't need to follow the curve for the second loft because the first loft did and already has a straight edge.
  • robert_horton034robert_horton034 Member Posts: 6
    Glen, yours looks like the simplified version of exactly what I'm attempting. I just haven't been successful at getting the second loft to follow the 3D fit spline. Looking at yours gave me the idea to make a simplified part studio.

    https://cad.onshape.com/documents/582ef5bc0951a193050d44af/w/a2d2f9dbc29bf56356973493/e/ccc3374051443f8eb3b5b6d2

    What I learned in that play area was that line or spline for the path must be a real line, not a construction line. I'm not sure why that restriction but that solved most of the problem. That solved it in the test drawing but not in the complex drawing I was working on. I'm going to try again to create a 2D profile with the gurney flap included since I know that works.

  • glen_dewsburyglen_dewsbury Member Posts: 77 ✭✭
    I got rid of the draw down on the inboard section to get a smoother blend into the tip. How ever when trying to make the gurney flap on the tip I ran into the same problems you did. If I get a chance over the weekend I'll have another look.
    https://cad.onshape.com/documents/3adda7bee6878142e772d11e/w/8b312ac02139b14f7d8a1779/e/4bf239e7e1293ba383ac7073
  • glen_dewsburyglen_dewsbury Member Posts: 77 ✭✭
    edited November 13
    I figured out why this wasn't behaving as I expected. Option in the profile generator to use a single spline seemed to leave a radius on the trailing edge of at lease one of the profiles but not on all. That means the loft is not seeing a consistent number of divisions on the profiles which can cause twisting of the loft. It wasn't a lot so not so easy to notice. When making the gurney strut for outboard end I noticed a very small gap between the profile and a guide curve that was not expected. Went back to the profile generator and made a change to the option for spline/s and the rest of the model began to start working as expected.
    Change profile generator to upper & lower splines.
    The gurney strut on outboard end is now a simple sweep. This sketch shows the difference between tailing edge profiles.
    https://cad.onshape.com/documents/3adda7bee6878142e772d11e/w/8b312ac02139b14f7d8a1779/e/4bf239e7e1293ba383ac7073


  • leonid_raizleonid_raiz Member Posts: 9
    I think the bulletproof way to get what you want is to create 3 straight lines; one along trailing edge of the blade and two along desired bottom of gurney flap. Then make a single loft that includes both blade and the flap. Use predefined lines as guide curves. 
  • leonid_raizleonid_raiz Member Posts: 9
    There are several approaches to get what you want.
    1. Include outline of gurney flap in your loft profiles. This way you will avoid the necessity to attach flap to a blade and make all in one loft.
    2. Make a straight line along trailing edge and use it as guide in blade loft. When defining gurney flap assure that its edge with be exactly along blade trailing edge and make it so its body sufficiently embedded inside the blade. This will guarantee flap to blade attachment.  
  • robert_horton034robert_horton034 Member Posts: 6

    What I did, in the end, is to trace the profile with the spline tool including the gurney flap that I wanted; as leonid_raiz suggested. Maybe there is something in the UI that I am missing but there is a serious lack of error message feedback to the user. I would not accept a code compiler rejecting my code with the only clue being "error". At the minimum, I would expect an error code I have to go look up in a book. I don't see why a CAD tool should be much different. Getting a clue as to what the problem seems to be the number one stumbling block to many operations.
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