How to center sketch on a slanted cylinder loft?

[harrison.friedes]

I created a slanted cylinder and then a sketch on a plane tangent to it. I'm trying to figure out how I can center a sketch between it's two filleted edges:

Projecting doesn't seem to create the correct outline I'm looking for, presumably because the plane distance interferes with properly replicating the 'edges'. Any idea what I can do instead? Fusion file attached below.

Also, if anyone has any suggestions on what I can do to better make the handle resemble that of the one I'm basing mine off of (it seems to add some nice little detail I can't quite conceptualize) I'd really appreciate it too:

[g-andresen]

Hi,

In principle, a projection of the body to which a feature is to be applied later is used for positioning sketches.
This projection, here especially the center points, orient the sketch.
Instead of the tangential sketch plane, I would just create the center of the profile with a line on an "origin plane" and project that line onto the body surface in another sketch.
The Pipe tool then creates the primary channel.

günther

[Ceecis · Accepted solution]

You used a rectangle and 2 arcs instead of a slot. You should use a slot instead.

You can project the lines that go around the top and the bottom of the cone. It will create ellipses that have a center point. Make them into construction lines.

Create a construction line that goes from the bottom arc of the top ellipse to the center point of the arc at the top of the slot. Make the construction line coincident with the center point of the top projected ellipse.

Create a construction line that goes from the bottom arc of the bottom ellipse to the center point of the bottom arc of the slot. Make the construction line coincident with the center point of the bottom projected ellipse.

Use equal constraints on each construction line. Use a vertical constraint on one of them.

Trace a normal (non-construction) line across the whole length of the slot so that the slot is split in 2.

Use the revolve feature to carve the shape of the slot into the part, rather than the emboss feature.

[harrison.friedes]

Thank you!