Worm gears

Intro

▶ 0:00

Worm gears transmit power between non-intersecting shafts, and achieve a very high gear reduction ratio in a very compact space.

Modeling the worm

▶ 0:15

Think of the worm as a rack that has been revolved around an axis, except the teeth are revolved around in a helix instead of in circles.

Parameters

▶ 0:45
 
\(module\) 2mm
\(length\) (in teeth) 10
\(pressure angle\) 20°
\(starts\) 4
\(diameter\) 40mm

New component: worm

▶ 1:06

New sketch on the vertical (xz) plane

▶ 1:14

This sketch looks much like the sketch in the rack video:

diameter 2 length × module × π

Sweep

▶ 1:45

Surface → Sweep, of type “Single Path”

 
profile horizontal line
path vertical line
twist angle \( length / starts \times 360° \)

The only part we’re interested in is that outer helical path. Since we want to have a total length of 10 teeth, and four starts, each start will twist 2½ times.

Tooth profile

▶ 2:38

Create a sketch on the vertical (xz) plane, and project in the horizontal line we used for the sweep profile, so we can align the tooth profile with it.

▶ 2:57

The tooth profile itself is just a trapezoid drawn with lines and several constraints.

1.5 × module 1 × module pi × module/2 90° - pressure angle pitch line

Helical sweep

▶ 3:50

Solid → Sweep → “path + guide rail sweep”

The profile is the tooth profile we just drew, the path is the vertical line, and the guide rail is the helix. (Make sure “chain selection” is off when selecting these.)

This gives us a single start for the worm gear:

Go into the worm gear, and hide the unneeded surface body.

Circular pattern

▶ 4:23

Select our sweep and do a circular pattern with Object type Bodies, around the central axis, with Quantity \( starts \):

Worm gear body

▶ 4:46

Create a sketch on the horizontal (xy) plane:

diameter - 2½ ✕ module

Extrude → Two Sides:

 
Above: \( (length\_in\_teeth + 1) \times module \times \pi \)
Below: \( module \times \pi \)

End