The following tutorial outlines a sequence of steps that may be used to create diamond knurls in SpaceClaim 2009+ SP1.
Create a chamfered cylinder. The dimensions of the puck below are 0.125″ x 0.500″ x 0.010″.
Switch to Sketch Mode and create a “comb” that defines knurl depth and spacing. The sample below has a tooth depth of 0.005″ and a tooth spacing of 0.010″.
Back to 3D mode.
Create a surface from the comb profile.
Pull a helical solid from the comb surface. Taper angle should always be zero. Pitch is shown to be 0.500″ with a height of 1″. The pitch may be varied to affect the geometry of the knurl diamonds.
If the pull is successful, a solid helical comb is created.
Using the Combine Tool, subtract the helical comb from the cylinder to begin the knurl. Since there are so many resultant solids to get rid of, I escape out of the combine operation after the second click and just use the Structure Tree to quickly get rid of the “groovy” solids.
Note that both right-handed (red) and left-handed (blue) helical cutters are required.
The beginning of the diamond knurl is shown where the right handed and left handed cuts overlap. Although the picture below shows one right-handed cut and one left handed cut, in practice I would do all of the right handed cutting first followed by all of the left handed cutting (or vice-versa) as I think it’s easier to keep track of one’s place that way.
To complete the knurl treatment, the helical solids must be moved up or down along the z-axis in order to cover the entire diameter of the puck. The movement distance must be in increments of the tooth spacing as defined above in order for the grooves to align.
Once that process is complete, the knurl should look like this. Do note that the subtraction process is computationally expensive, especially towards the end. For example, on my older, single core machine, the very last cut took well over twenty minutes.
If anyone has an alternative methodology for knurling in SpaceClaim, be sure to drop a note in the comments.