What's the easiest way to create the shaft in this sketch?

[banshee10]

There's an interesting article about sketches at http://forums.autodesk.com/t5/Design-Differently/The-Power-of-Top-Down-Design-in-Fusion-360/bc-p/517...

But there's some features of the sketch that are non-obvious.

1.  If you've got the two circles for the pins on the shaft, how do you create the shaft itself?  Is there a simple way to do it, or is a muti-step process involving intermediate circles that get deleted?

2.  What's the dotted line in the circle?  The inner and outer circle seem obvious (they're just circles), but that dotted thing seems to be some sort of joint or constraint.

3.  How do you get a dimension that's just the distance between the two pins?  It seems like creating dimensions always wants to draw at 90 degree angles, never just the distance between two points.

[TheCADWhisperer]

I can walk you through this design step-by-step.

Start a new design.

1. Change the Units to inch

2. Start a new sketch on the XY plane and then select the Project Geometry tool and project the Origin.

3. Sketch a circle centered at the origin.  Dimension the circle 1".  Right click on the circle and select Construction.

Indicate here when you have finished these 3 steps and I will explain the next few steps.

[TheCADWhisperer · Accepted solution]

Sketch 2 more circles at the origin as shown.

(You can see that the dotted linetype circle is construction linetype.)

Add the rectangle and dimension as shown.

Add this construction line (you know how to create a construction line now, this step is not shown in the original sketch).

Sketch small circle at intersection of the construction line and construction circle.

Sketch small circle to left as in image.

Sketch construction line between the two small circles.

Dimension the length of the 3" construction line by Right Mouse Button - Aligned.

Add an Equal (=) constraint between the two small circles that we you just created.

Sketch 2 larger circles at the centerpoints of the 2 smaller circles.

Sketch lines connecting them together (Tip: If you click and drag - Fusion will automatically add the Tagent Constraints.  If you don't get the automatic Tangents, add them yourself).

Trim the two arcs.

Add an = constraint between the two arcs.

Dimension one of the arcs.

Stop Sketch

Export Archive.

Right click on the exported archive file and select Send to Compressed (zipped) Folder.

Attach the resulting *.zip file here (or the *.f3d if the forum will allow).

[banshee10]

Thanks, that was extremely useful.

[TheCADWhisperer]

Post back if you have any trouble completing the rest of the tutorial.