Curve from equation with part parameters

Just type part parameter names to equation?

Say you have part level parameter called DIAMETER (Real Number), then one can create curve from equation; Cylindrical.

r =diameter/2
theta = t * 360
z = 0

I've built a few gears with involute curves and what Mikko suggests is exactly what I did. You define your parameters, then use them to define the parametric equations defining the three spacial coordinates for your curve. I don't think I was able to look at the part parameters as I defined the curve driven equation. I had to bounce out of the curve definition, make sure of what my desired parameter was, then plug that into the equations.

I found that the equations are much simpler if I use r, theta and z rather than x, y, and z. The curve definition from one of my parts is:

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

Also, a big tip. I found that I had to define a half tooth, then mirror it, then pattern it around the axis of the gear. My initial attempt at this was to use the involute curve as a reference of a full tooth sketch. One side of the tooth was a direct "use curve" that used the equation driven curve. The other side was a mirror of the first about the center of the tooth. This seemed to work, looked okay, etc. But, what I found later was that if I had to change the definition (i.e. I wanted 42 teeth instead of 44) the teeth were no longer perfectly symmetric. The mirrored side would vary, particularly in curvature, from the side driven directly by the equations. My theory is this is because Creo is using a spline for the mirrored side that is an approximation. When I change dimensions, it's not like the program is "re-mirroring" the equation driven curve, but somehow adjusting that approximation to suit the situation. In other words, there doesn't seem to be a mathematical "link" between the mirrored curve and the driven one. Thus, I found that mirroring a half tooth was the only way I could have perfectly symmetric teeth in my gear.

Another thing I learned along the way is to define all the driving dimensions of the gear using parameters. Name them with easy to understand names, like numTeeth, etc. Thus, when I wanted to make another gear (and another, etc.) it was much easier to go into the parameters and change all the pertinent values rather than editing all the features.