Sweep with Solid body

[Anonymous]

I am trying to sweep a profile to mimic the movement of a .125" ball endmill. 

I can just use trace in manufacture to get the shape I want, but I would really like to be able to model the part correctly. 

What is the best way to model this?

[jeff_strater]

unfortunately, there is no great way to do this in Fusion today.  I took a look at your model, but it was not immediately obvious what body you want to sweep along what path.  You can get a close approximation using silhouette edge projection and some clever copy/split/move of the body, but that is labor-intensive, and can fail for complex bodies.

[MRWakefield · Accepted solution]

Is this the kind of thing you're thinking of?

[Anonymous]

Yes that is what I am trying to model.

How did you accomplish this?

[etfrench · Accepted solution]

I would use two coils, one with a circular section to simulate the ball end, and one with a square section to simulate the shank.

[etfrench]

Adding the guide rail makes the sweep work. 

[Anonymous]

Got it, thanks!

[etfrench]

I think @MRWakefield post would be the preferred solution 😀

p.s. To see how it was done, use the Timeline play buttons in the lower left of the Fusion 360 window.  You can also use Edit Feature to see all of the settings.

[MRWakefield]

As @etfrench said; scroll through the timeline to see how I did it. You were close-ish, you just needed to have your profile perpendicular to the path and add a couple of revolves to model the ends of the slot/pocket. Oh yes, and use one of the paths as a guide rail for the sweep as per @etfrench's comment.

[jeff_strater]

all of those approaches will work in this case (simple body, simple path).  Here is a more general (not 100% general, just more so...) approach to the "sweep a solid body", just FYI.

start with the tool and the path:

create a second instance of the tool at the end of the path (removed at the end), using Pattern on Path:

copy/paste body at the start and end - creates two bodies at the root (could be in another component, I was too lazy to do that):

Create a Plane Along Path at the start:

sketch on that plane, project the tool silhouette into the sketch (Project, with selection set to "Bodies"):

sweep/join that profile along that path:

then you have a body that you can use to subtract against another body, or use as a keepout volume for a mechanism, etc...

As I said, a bit of effort, but fairly accurate...