Exercise: Formed Curve on Cylinder

• Create an extruded surface cylinder
  Feature > Create > Surface > Extruded > Done
• Sketch a circle 1" diameter
  Extrude it 2" deep
• Create a Formed Datum Curve
  Select Datum Curve icon > Formed > Done > Quilt Surface > Done
• Create a sketching plane that is offset 1" from the RIGHT datum plane.
• Note: Cylindrical surfaces are comprised of 2 halves - and the formed curve will fail to be created if it's vertex falls on the seam. (Offsetting from the FRONT datum will have that problem)
• Sketch a line as shown below -

• Align the bottom of the line to the 2 datum planes (or the edge of the surface cylinder and it's axis)
• Align the top vertex of the line to the top edge of the surface.
• Place a "sketch coordinate system" as shown
• Create just one dimension for the length of the line.

This provides the following helical curve:

Sweep a solid down the outer edge of the resulting surface feature.

• Feature > Create > Solid > Protrusion > Sweep > *Solid > Done
     * Use Thin if the sweep is hollow
• Choose Select Sec
• Choose One by One, query select and select the whole curve.
• Done > OK
• Sketch the sweep's profile
• Done > OK

You now have a coil driven with the desired dimensioning scheme: