Involute gear (Wildfire 3.0 to Creo 4.0)

[mholst]

I have an old 2008 tutorial on how to create an involute gear in Pro/ENGINEER Wildfire 3.0 which is very easy to follow and use (see attached).
However it is long since last time I have used it and my current employer is using Creo 4.0 and this is where the problem starts.
I can follow the steps until task 6 as the difference between Wildfire and Creo are small until this step but in task 6 it says to go to  >Insert, Model Datum, Evaluate. This feature is not available (or it is moved and renamed) in Creo 4.0. Also in task 7 it says to use >Edit, Copy. This feature is also unavailable in Creo 4.0...

Can anyone tell me how to do these features in Creo 4.0?

I know there is other guides on how to create involute gears but I really like this one. If anyone has a similar version for Creo however it will be most welcome.

[KenFarley]

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.

[rreifsnyder]

Looks great but I would suggest trying to use Geometry Pattern rather than a regular Pattern. I would expect significant performance improvement.

One of the longest steps in regenerating a feature is the checks to ensure that good solid geometry is being created. A regular pattern has to do this for the first half tooth and then again for the mirror again and again. The geometry pattern patterns surface copies of the finished geometry of the tooth and only solidifies it at the end so it only has to go through the geometry verification once.

[KenFarley]

I had not heard of the Geometry Pattern, probably because forever (at least since Creo) I've defaulted to the right mouse click plain old Pattern, not the dropdown menu Patterns. Seems to be significantly faster, and doesn't cause any curvature irregularities. I'm going to have to try that on some other CPU-hogging patterns we occasionally need to make (arrays of rectangular holes)...

[Patriot_1776]

I typically use geometry patterns as well, and for those reasons, but I was disappointed to see the geometry pattern didn't reduce the file size nearly as much as I'd hoped.  Sometimes it doesn't reduce it much at all.  Still a good idea to use them, especially since it's much easier to use now.

Honestly, it'd be awesome to have the macro inside Creo to just be able to pick a toothform (in sketch mode) from, say, the pallet, be able to modify the pressure angle etc., and get the curve without having to set up the equation blahblahblah.  Just for fun, I was able to create both a true epicycloid and involute curve without using an equation.  It's possible, but make for a large file.  My mind doesn't work well with equations, so I thought I'd see if I could do it with geometry.  Fun side exercise...

[tbraxton]

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.

[mholst · Accepted solution]

Thank you all for your solutions.
I have found that the command >Insert>Model Datum>Evaluate that I was missing in taks 6 in the guide could be substituded with using >Measure (the ruler symbol) and then saving the measure as a feature.

The >Edit>Copy feature I was missing in task 6 was simply done by right clicking a feature and using copy and paste - doh!
With these features I could follow the rest of the guide and create my gears just like I used to again.