// Spur Gear
// A rotating machine part having cut teeth or, in the case of a cogwheel, inserted teeth (called cogs), which mesh with another toothed part to transmit torque. Geared devices can change the speed, torque, and direction of a power source. The two elements that define a gear are its circular shape and the teeth that are integrated into its outer edge, which are designed to fit into the teeth of another gear.

// Set units
@settings(defaultLengthUnit = mm)

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

  // Define the constants of the keyway and the bore hole
  keywayWidth = 2
  keywayDepth = keywayWidth / 2
  holeDiam = 5
  holeRadius = holeDiam / 2
  startAngle = asin(keywayWidth / 2 / holeRadius)

  // Sketch the keyway and center hole
  holeWithKeyway = startSketchOn(XY)
    |> startProfile(at = [
         holeRadius * cos(startAngle),
         holeRadius * sin(startAngle)
       ])
    |> xLine(length = keywayDepth)
    |> yLine(length = -keywayWidth)
    |> xLine(length = -keywayDepth)
    |> arc(angleStart = -1 * startAngle + 360, angleEnd = 180, radius = holeRadius)
    |> arc(angleStart = 180, angleEnd = startAngle, radius = holeRadius)
    |> close()

  // 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 the keyway sketch from the gear sketch
    |> subtract2d(tool = holeWithKeyway)
    // Extrude the gear to the specified height
    |> extrude(length = gearHeight)

  return gearSketch
}

spurGear(
  nTeeth = 21,
  module = 1.5,
  pressureAngle = 14,
  gearHeight = 6,
)