spur-reduction-gearset

// Spur Reduction Gearset
// A pair of spur gears meshed together, with an equal module and different number of teeth

// Set units
@settings(defaultLengthUnit = mm)

// Define a function to create a spur gear
fn spurGear(nTeeth, module, pressureAngle, gearHeight) {
  // Calculate gear parameters
  pitchDiameter = module * nTeeth
  addendum = module
  deddendum = 1.25 * module
  baseDiameter = pitchDiameter * cos(pressureAngle)
  tipDiameter = pitchDiameter + 2 * module

  // Using the gear parameters, sketch an involute tooth spanning from the base diameter to the tip diameter
  gearSketch = startSketchOn(XY)
    |> startProfile(at = polar(angle = 0, length = baseDiameter / 2))
    |> involuteCircular(
         startRadius = baseDiameter / 2,
         endRadius = tipDiameter / 2,
         angle = 0,
         tag = $seg01,
       )
    |> line(endAbsolute = polar(angle = 160 / nTeeth, length = tipDiameter / 2))
    |> involuteCircular(
         startRadius = baseDiameter / 2,
         endRadius = tipDiameter / 2,
         angle = -atan(segEndY(seg01) / segEndX(seg01)) - (180 / nTeeth),
         reverse = true,
       )
    // Position the end line of the sketch at the start of the next tooth
    |> line(endAbsolute = polar(angle = 360 / nTeeth, length = baseDiameter / 2))
    // Pattern the sketch about the center by the specified number of teeth, then close the sketch
    |> patternCircular2d(
         %,
         instances = nTeeth,
         center = [0, 0],
         arcDegrees = 360,
         rotateDuplicates = true,
       )
    |> close()
    // Subtract a 10mm diameter center hole from the gear
    |> subtract2d(tool = circle(center = [0, 0], radius = 5))
    // Extrude the gear to the specified height
    |> extrude(length = gearHeight)

  return gearSketch
}

// Model a small gear
spurGear(
  nTeeth = 17,
  module = 1.5,
  pressureAngle = 14,
  gearHeight = 9,
)

// Model a larger gear with the same module
spurGear(
       nTeeth = 51,
       module = 1.5,
       pressureAngle = 14,
       gearHeight = 7,
     )
  // Translate the larger gear by the combined pitch radius of both gears, plus a small gap
  |> translate(x = (51 + 17) / 2 * 1.5 + 1.3)

  // Rotate the gear so that the teeth mesh but do not intersect
  |> rotate(yaw = 3)