How to create this curve and adjust it?

[matthewpolack]

Hi,

I'm learning Fusion 360 and trying to create a simple trampoline spacer...it has a curved inner section.

I'm getting there...but am struggling with the easiest way to create the curved inner cut I need:

Specific struggles:

How do I create the inner arc cut? (Have tried creating an offset plane..then clumsily drawing a curve..)..but finding it a bit tough...

How do I set the dimension of the arc?

How do I repeat the arc symetrically on both sides?

How would you make this? Thanks so much. - MattHow do I cut this?

[davebYYPCU]

Like this?

Use Origin Planes, Extrude the Donut.

Then with mirrored circles, that are pipe diameters, Symmetric cut the scallop.

[TheCADWhisperer]

Can you post an image looking directly down from top?

Can you File>Export your *.f3d file of your attempt to your local drive and then Attach it here to a Reply?

A view directly from the side would help too.

[Anonymous]

Thanks so much for the replies...that replication you've made their CADwhisperer is very impressive!

My question was a little bit more beginner...my approach was to just to make a 3 point arc on the side...and then cut through the cylinder...but I wasn't sure how I could adjust the dimension of the curve here. I was also struggling to 'snap' the sketch to the edge of the cylinder..couldn't figure out how to get the constraint working. Thanks!

I've attached my go at this..very basic by comparison with yours! Thank you!

[Anonymous]

Thanks for this...at this point I don't quite understand all of this...so will keep watching tutorials! Thanks!

[davebYYPCU]

Where are you stuck?  Do you have the part to measure in person?

Fusion works best with dimensioned sketches to make the parts in material as a result.

Might help...

[chrisplyler]

Let's assume you made the cylinder by Extruding up a circle. You'll need a second sketch that is perpendicular to that circle sketch. On this second sketch, you Project the cylinder body(I use the Intersect option because I placed my sketch right through the center of the cylinder) into this sketch, which gives you purple lines/points. Then you sketch your arcs such that their ends are coincident to the corners of that purple projection.

The Project tool, and it's variant options, are a powerful method of "relating" sketch elements to either other sketches or to actual body geometry. In this case, it lets you ensure that the ends of your arcs are always exactly on the edges of the cylinder.

Of course, you might have made the cylinder with a Revolve instead of an Extrude...in which case your first sketch would have been vertical, and you could put the arcs right into that sketch without needing a second sketch, and without projecting anything. And of course, instead of connecting the arcs to the corners, you could connect them to the upper and lower surfaces of the cylinder and define a distance in from the edges. And of course you could sketch a shape more complex than just arcs, if you wanted to more accurately duplicate the real original part.

https://knowledge.autodesk.com/community/screencast/de89a3a4-cd50-4228-b013-9e5e7283b220

[chrisplyler]

Let's assume that you made the cylinder by Extruding the profile of a sketch with two circles. Then you'll need a second sketch to define the arcs. Use the PROJECT tool in that second sketch to capture an outline of the cylinder, which will give you purple lines/points representing the cross section of the cylinder. Then you can sketch the arcs with their ends coincident to the purple corners. Define the radius of the arcs with dimensions, as I have done, OR define the midpoint depth of the arcs using construction lines with dimensions.

https://knowledge.autodesk.com/community/screencast/de89a3a4-cd50-4228-b013-9e5e7283b220

[chrisplyler]

Of course you might have made the cylinder with a Revolve, in which case you could put the arcs right into the same sketch. Watch me edit the sketch and change the ends of the arcs from the edges of the cylinder to a defined distance inside the edges.

https://knowledge.autodesk.com/community/screencast/12bb8a0e-f5e6-4d30-b88e-7e01869a2561

[Anonymous]

Thank you so much for this extremely comprehensive reply Chris...apologies it has taken me a while to jump back in the forum and check for further replies. The detailed videos and explanations are absolutely excellent and I really appreciate your time in preparing this. Thank you so much. I will work my way through step by step with these exercises to get a solid understanding...their are some great new concepts you have included here that are extremely helpful.

I did indeed use the extrude method as shown in the first video...but have never seen that intersect option..that is a very handy way of doing what I was trying to achieve. Thank you!

[chrisplyler]

I'm glad to help when I can.

My advice:

When I first started using Fusion, I spend thirty minutes just looking in every single menu, hovering over every single tool item, reading every single Preference setting, activating a tool and looking at all the options/settings available for it, etc. Trying to get to know the UI and what was available within it. Didn't make me instantly understand everything, but just gave me a clue so that when later I was wondering, "Hmmm, I wonder if Fusion can do the thing I've just thought of," my brain answers, "You know, I think I saw something that might be that thing."

[chrisplyler]

Also...

You don't HAVE to make your sketch right through the center and Project>Intersect it. You could Construct>Offset Plane out to one side, and regular Project>Project it. Can achieve exactly the same results. I just figure why make an extra plane if I don't need it.