Community
Fusion Design, Validate & Document
Stuck on a workflow? Have a tricky question about a Fusion (formerly Fusion 360) feature? Share your project, tips and tricks, ask questions, and get advice from the community.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Any way to revolve on path?

8 REPLIES 8
SOLVED
Reply
Message 1 of 9
nkloski
2100 Views, 8 Replies

Any way to revolve on path?

Let's say I want to create a lid (which I do).  The easiest way would be to have a "revolve on path" or "revolve with rails".  But there is no easy way to do this.  There is a harder way with surface lofts, then thickenings, then combines, but if there was a "revolve on rails/path" that would solve it.

 

Here is a simple fusion file showing this:

 

RevolveOnPath.PNG

 

Any ideas on how to do this easily?

 

Thanks!


Nick Kloski
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


8 REPLIES 8
Message 2 of 9
TrippyLighting
in reply to: nkloski

I don't think the sweep tool as currently implemented would to this, but it is imaginable as it has a "stretch" option that can be enabled if you make a sweep with path and rail.

What you're asking for is really that "rail" to be a point and the porofile to stretch beween the path ahd the rail as it is being swept.

 

I just don't thing that the sweep tool would allow a point as a "rail" equivalent to how you can loft between a profile and a point. Might be worth trying out.

 

 

 

 

Peter Doering
Message 3 of 9
nkloski
in reply to: TrippyLighting

Yeah, I tried sweeping...it works until the profile gets to the first corner bend, but then the profile starts to intersect itself at the center, and the command fails 😞

 

Ha!  Additionally, if you choose to sweep that profile in the file I attached, using the outer line as the path and the inner line as the guide rail, Fusion hangs forever 🙂


Nick Kloski
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 4 of 9
HughesTooling
in reply to: nkloski

If you can create 4 cross section one at every 90° loft will work. You can mirror the cross section you have but I think you'll need it in another sketch so it doesn't get selected as one.

 

Mark

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 5 of 9
nkloski
in reply to: HughesTooling

Yep...that is the "harder" way, but one that works.  Creating a 1/4 surface loft then mirroring to get half, then mirroring to get full, then thickening.  but that takes a long time...and in the file I attached, the top edge has spline-ripples in them, which I loft would not be able to do. 

 

I mean the loft "could" do those ripples, but the profile changes between the long and short sides (because the rail on the two sides would be different, and it would not be what I am envisioning a "revolve on path with scaling" to produce.

 


Nick Kloski
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 6 of 9
HughesTooling
in reply to: nkloski

I changed your rectangles to squares just to see if it would work and in the patch workspace I can get a surface like this.

logo.png

 

Don't know if you could copy your sketch 90° the use a non uniform scale to resize. I've attached the file in case it might be of some use.

 

Mark

 

Edit. Just looked and there's no non uniform scale option in the sketch workspace so that's a dead end.

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 7 of 9
nkloski
in reply to: HughesTooling

Thanks for trying!  Surprisingly, the sweep works without using a rail (just a profile and path) but creates a super-weird result:

 

sweep.PNG

 

Hence the request to see if there is a "revolve with guide rails" function.


Nick Kloski
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 8 of 9
HughesTooling
in reply to: nkloski

I think there's a request on the ideastation for rail revolve. For now how about the attached file.

I managed to make it work as 2 halves, i needed to make a new sketch with just half of the rectangular base profile.

Clipboard01.png

Mark

Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Message 9 of 9
nkloski
in reply to: HughesTooling

Aha!  That works...great solution!  You mad mirrored the quarter-sketch-profile, and then lofted one side to the other side, using the outer bottom edge/line as the rail.

 

I wold never have thought about lofting to mirrored profiles because there is NO way to loft to profiles that are exactly planar with each other....UNLESS you use a rail which solves that planar problem...awesome!


Nick Kloski
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report