Help with this break (line/sketch) feature

[Anonymous]

I'm trying to follow this tutorial, but they lose me when they start breaking their splines using intersection points. They are some how editing the sketch to add more lines, to use for breakpoints, without forcibly going back on the timeline. I tried to mimic this by just having the proper sketch that holds the intersection lines, which will be used for railing in future lofting, visible while editing the sketch which contains the spline i wish to break, but it doesn't have the same snapping that the normal intersection points have so I assume it's off. Also, when I attempt to loft after that approach it tend to error out so i assume it's not the proper method/approach. Can anyone help me with this?

Time he loses me : 6:12

https://knowledge.autodesk.com/search-result/caas/screencast/Main/Details/1d7370a2-67b2-438d-b75e-f2...

[etfrench]

I can see where that would be confusing   It looks to me like  about two minutes of random clicking about while trying to break the splines.  After the author started adding a line at the intersection point, the break command started to work.   It appears the main reason for breaking the splines is to create individual faces in the Patch workspace.

p.s. See post #2 in this thread.

There are quite a few more threads later than this on guitars.

[davebYYPCU]

That's an old version of Fusion, and he has no timeline, which would be confusing, to some, me especially.

That shape should loft without breaking the splines, with the current version of fusion, but would need the file to verify.

Loft Sketch 1 to Sketch 2 as profiles, and then the other two sketches are rails.  If your file errors then it is likely the rails are not connected to the profiles.  

Might help....

[TrippyLighting · Accepted solution]

as @davebYYPCU has already mentioned, breaking these splines is not needed and the shape will loft nicely. It will loft even better if you use a helper surface for the center profile instead of the sketched spline.

When going through the timeline, pay close attention to the loft options.

In general splitting splines is not a great technique as it'l kill the ability to modify a spline as a whole. It also often kills curvature quality. When lofting that last enter section, the author also makes the mistake of selecting sketched splines for rails, instead of selecting surface edges, which would allow him to define curvature continuity in the loft options. On second thought though, I don't think these options existed when that video was made.

[Anonymous]

Greatly appreciative of you and the others who've replied to my thread. Though, may i ask, what are helper surfaces and how to utilize them? 

[TrippyLighting]

If you go through the timeline of the design attached to my post you'll see that instead of using the center spline for lofting I am actually selecting a surface to loft towards that I extruded earlier in the timeline.

When you only use sketch geometry Fusion 360 will not offer you the ability to select curvature continuity settings for the start and end conditions of the loft. The reason is that you actually need a surface for the loft to be curvature continuous with.

That is what this helper surface is for. After the loft is completed it is not needed anymore and it can be removed (not deleted). In this design that's the only way to get (mostly) smooth curvature across the center of the object.