Involute gear (Wildfire 3.0 to Creo 4.0)

There's been a lot of discussion in the past about this, with examples, etc. A Google of "Creo involute" brings up lots of stuff, like the following:

Previous Involute Discussion on PTC Community

I've had the task of defining some toothed wheels with involute shapes and it's a fun mathematical adventure, for sure. Creo is very different from Wildfire in terms of the commands available, some things are easier (I feel) than it was in the old days.

The basic steps to create the gear that I've found works well is:

(1) Create the standard set of planes, an axis defined as the intersection of the "X" and "Y" planes, and a coordinate system.

(2) Define the geometric parameters that will govern the tooth shape, things like pitch diameter, number of teeth, pressure angle, etc.

(2) Define the involute curve via the Model->Datum->Curve->Curve Through Points. I've found that using cylindrical coordinates makes the definition less complicated. The "t" value is set to a range of 0.0 to 90.0, and the equations end up being:

r = diabase * sqrt ( 1.0 + ( PI * t / 180.0 )^2 ) / 2.0
theta = t - atan ( PI * t / 180.0 )
z = 0.0

(3) I use this curve to define a half tooth, along with a couple of circles at the root and tip diameters. This half tooth is the first solid feature in the model. I learned, the hard way, not to define a full tooth. I thought I'd be able to do this by using mirrored curves in the tooth sketch, but that didn't come out too well. It looked okay at first, but when I tweaked any of the dimensions, the mirrored geometry would deviate from being an accurate mirror of the involute curve. The curvature on the mirrored side would vary wildly from the original. There is some sort of disconnect between the mirrored geometry and the original when the entities are splines, I think.

(4) Once I've built the first half tooth, I mirror the solid geometry to create the first full tooth. This, unlike sketch geometry, maintains curvature equivalence. I group the half tooth and the mirror, naming it something like "single-tooth".

(5) Using the number of teeth parameter, I pattern this single tooth about the central axis to create the complete gear.

(6) Add the necessary bore hole, keyway, chamfers, etc.

I've found that root and tip fillets are best added in the sketch for the half tooth.

Look in the upper right side of the ribbon in Creo for the magnifying glass icon. It is a command search that will allow you to search for commands and guide you to them graphically in the UI. It does not have 100% coverage of commands that work but should point you to most of what you need.

Click the icon and then enter the name of the command and it will return results if they are found and show you where the commands are in the UI.