How to create sketch on shaft centerline?

[SherpaDoug]

I have a shaft extruded from a circle, with a number of radial features. Now I want to add some transverse features like a keyway. I can make a sketch on the YZ plane which bisects the shaft and shows a cross section lengthwise of the shaft, but it has few selectable lines. Specifically the shaft surface is not selectable. Is there some way to project the shaft features to the sketch plane?

 

[Ralf]

Hi SherpaDoug,

To get an idea, can you post a picture please?

 

[SherpaDoug]

This is the work in progress. I managed to get the chamfer on the square ends, but it was not graceful. There must be an easy way to do this simple task. I mention a keyway because that would be be a similar problem that many designers have to deal with.

 

[MilesH]

- You can simply recreate the section in the Sketch using the data from the Equation editor.

- You can Project from a 3D Section view (but you lose Associativity).

- You can Extrude Cut to the Plane, Project to Sketch and then Suppress the Extrude Cut.

 

[BernardK]

In the cross section plane, the end face appears as a line. This line can be projected to the sketch plane. Select create reference and maintain association to ensure this line remains associated with the end face. Create a centre line using a mid line constraint. The keyway cross section can then be drawn and constrained or dimensioned from the reference lines. Use a mid plane extrude cut and add fillets to create the rounded ends.

I would create a single tapered flat. Repeat the above to get the end face and centre line references. Create the cut profile and extrude cut through all. circular pattern for four flats and mirror for the other end.

 

[HaroldL]

Another method for placing a keyway is to insert a Plane offset from the default plane and tangent to the surface of the shaft. Click on the Reverse option to get it on the prefered side. Place your keyway sketch on the new plane, constrain it Symmetrical about the center axis of the shaft (when you select the axis for the Symetric constraint it will create a Reference line in the sketch) and dimension accordingly. Then Extrude Cut to your desired depth.

Hint: If this is going to be a common keyway that you will need on other projects/parts, it would be a good idea to save it as a Catalog Feature.

H.