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I agree that this is not exactly obvious 😉
When projecting a sketch onto a curved surface you are creating a form of a 3D sketch. That is pretty obvious.
BUT once you are starting the Project to surface command it want's you to pick plane to sketch on, and that is not so obvious, because why would one need a plane for a non-flat sketch ?
A couple of good questions here:
- Why does Project Curve to Surface require two sketches?
- Why do I have to pick a sketch for the second sketch (the destination sketch)?
For the first, the reason is pretty internal to Fusion. This command establishes a dependency from one set of curves to another. To be perfectly honest, we don't have a mechanism to do this within a single sketch. It's no different than a normal Project from one sketch to another - you need two sketches there, as well.
For the second, this is just a general sketch requirement. Fusion does not differentiate between 2D and 3D sketches. Every sketch is inherently both 2D and 3D. This is why Fusion requires a plane to create any sketch. The sketch plane of the "target sketch" in this particular workflow is not being used at all. When you choose "Along Vector" as the "Project Type", the default vector that is chosen is the sketch plane normal of the sketch where the selected curves are owned. You can select a different vector, of course.
Hope this makes it a bit clearer for everyone
Jeff
Jeff Strater
Engineering Director
I am trying to visualize why you would want to project circles around a cylindrical surface. Once you have these circle projects, what would you want to do with them.
My suspicion is that you are attempting to do something that is possibly relatively simple to do when you use different tools in Fusion 360 and would possibly avoid having one or more sketches for projecting stuff.
Can you describe the end result, or provide a hand sketch or other image that shows something similar ?
There are probably lots of ways to do this that are simpler than projecting a curve to a surface. I would probably do something like create a tool body of a cylinder, then create a circular body pattern, and cut the holes by doing a subtract. Here is a very simple example that I hope is at least in the general right direction:
This would work in a general case, such as patterning around a cylinder. But, if you really have a 9-sided polygon shape, which is what I see in the picture, you can even just do a single cut, then pattern the cut.
Jeff
Jeff Strater
Engineering Director
Strange. I can see the screencast in my post. Not sure why you can't see it. Anyway, here is a link to the screencast: http://autode.sk/2bgTONE. Let me know if you cannot follow this link.
Jeff
Jeff Strater
Engineering Director
Hi @blacktip,
I apologize. This command is confusing. The problem in this screencast is that you are still editing the sketch which has the existing curves. For this command, you need two sketches. So, the steps would be:
- Click on "exit sketch" for the current sketch
- Start a new sketch, using the "Create sketch" command
- Pick a plane (it doesn't matter what plane)
- Then, use the Project to Surface command, select the surface, and the curves in the other sketch
Jeff
Jeff Strater
Engineering Director
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