CAD Software Modeling an Airfoiled Fin in F360

Inspired by dr. Wogz Model a Fin tutorial, using the loft tool in Fusion 360 to model an airfoliled fin. The screen shots are from a part for an upscaled EAC Viper, and I modeled this to be milled on a CNC router -- but it doesn't matter except that the fin was milled in halves, which fit together like clam-shells. Dimensions are in millimeters.

1) Create a sketch and draw the fin. The body of the fin and the tab are are separated.




2 - Create a sketch plane at the root edge of the fin. rotate it 90° to the plane of the fin sketch.





3 - On the new sketch plane, draw the root profile -- the dashed line is a construction line placed as a guide, to mark the intended height (thickness) of the fin at the root. The conic section drawing tool in F360 is limited. You cannot (AFIK) enter an equation, so I played with the "rho" parameter to get a more-or-less parabolic profile. (To match a particular profile I'd've used the function plotting tool in Inkscape to create an SVG of the the curve, then imported that into F360. -- which would be a whole other thing to talk about)






4 - Repeat steps (2) and (3) at the fin tip. Note that the tip sketch-plane does not nave to be parallel to the root sketch plane. Note, also, that for this part the profile at the tip is shorter (thinner) than the root -- so that the fin will taper from root to tip.





5 - Use the loft tool to create a solid body between the two conic profiles.

6 - That's pretty much it for making the fin profle. The fin tab is extruded using the push-pull-tool -- which brings up the "extrude" dialog.


7 - The fin and the tab are two separate bodies. This doesn't matter for CNC machining, and I don't think it will matter if you export an STL for 3D printing. Thinking about making this a printable part, and worrying about the strength of a printed tab, I pulled the tab up past the top of the fin root

7.5 - I joined the bodies so that I could fillet the seam -- just because I think it might look cool.




Here is what the milled and assembled fins looked like (including some authentic field damage on the papered fin)

Why not import coordinates in (X,Y,Z) format then loft from plane to plane from real airfoil data?

Andrew_ASC said:

Why not import coordinates in (X,Y,Z) format then loft from plane to plane from real airfoil data?

Click to expand...

1) Partly because there is no "real airfoil" for the Estes Aerospace Club Viper, so that is not how I did it for this model.

2) Mostly because this is a "tricks and tips"/"quick start" kind of guide for folks who might be stumped for how to start a profiled fin model in F360 and I wanted to keep it simple.

2a) See the comment about plotting the profile and bringing in an SVG from Inkscape.

Cool. Very similar to what I'm doing. +1 for keeping it simple. Importing points for spline from CSV file is advanced topic (been there, done that). Anyhow, while there are free airfoil databases, different airfoils are optimized for different things, and unless you know exactly which airfoil shape you need, you are probably not much better than a simpler approach of drawing something airfoil-like yourself ;-)

lofting, or sweeps, or blends are powerful tools in CAD, but they do take time to master.

You should be able to enter in an equation for the line / curve. And, as Andrew pointed out, you should be able to have a p-line (or spline) pass thru a series of points, either entered manually, or driven from a spreadsheet.. The line/ curve could also be generated from an excel table..

dr wogz said:

lofting, or sweeps, or blends are powerful tools in CAD, but they do take time to master.

You should be able to enter in an equation for the line / curve. And, as Andrew pointed out, you should be able to have a p-line (or spline) pass thru a series of points, either entered manually, or driven from a spreadsheet.. The line/ curve could also be generated from an excel table..

Click to expand...

Yes you should be able to enter an equation but -- as of this writing -- Fusion 360 does not support plotting splines from equations (Autodesk Inventor, will do this). You can script it through the API, and you can import XYZ values into F360 from a .csv file (from a spreadsheet), but these techniques require deeper dives than seemed appropriate for a follow-on to your "how to model a fin" tutorial.

When I have needed a particular curve, I have used the function plotter in inkscape to create an SVG (with a lot of points), to be "inserted" into F360.



F360 treats the SVG as a series of splines -- segments connecting the points.





The SVGs sometimes come in with missing segments. To to avoid having to hunt down the open vertices, and to avoid faceting on the solid when I eventually get the the profile to close, I would probably trace the SVG profile with a bezier spline, rather than than lofting/revolving/extruding/etc. the SVG itself.

thank you. I stand corrected, or at least a little more educated! I knew Inventor did it, I assumed F360 would as well.