Now the section has to be drawn. To do that select the sketch icon (The icon just above the options tab in the image above). Once you are inside sketcher, Use the edges of the features Outer_dia, Involute curves and the first extrude’s edge (root_dia). Trim all other entities except for the teeth section. (See the images below to understand) Use edge option is located in Sketch → Edge → Use from the sketcher main menu.
14. Now we just have to sweep the transverse gear tooth section along the helical path. To do that use Variable section sweep. In wildfire versions, it is located in Insert → Variable section sweep from the main menu. In Creo, select the Sweep option under layout tab. Pick the outer edge of helicoid as trajectory and select solid and the other options marked in red below.
In this case the root diameter is larger than the base diameter. So we directly use and the trim the edges. If the root diameter is smaller than the base diameter, a tangent line has to be drawn for the teeth profile. See Spur gear page to read about this.
16. Once variable section is completed the model will look shown below.
17. Create the chamfer and radius.
18. Group the variable section sweep, radius and the chamfer in model tree.
19. Pattern this group using the center axis of the gear. 32 teeth (No. Of teeth) for 360 degrees.
20. Add center hole, key way cut and chamfer to the teeth side faces (revolve cut). Hide the curves, surfaces etc directly or using layers. That's it we have a Helical gear now.
Multiple methods can be used to model the gear. Just understand the concept. You can also do it on your own way combining the steps. You can now change the input values from Tool → Parameters. The model will update automatically for new values. You may get regeneration failure on gear teeth profile depending on which value it was modeled at the first place. You will have to update the tooth profile to solve this. That's all for this topic. I hope this helped you.