gear

// 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 = in, kclVersion = 1.0)

// Define parameters
nTeeth = 21
module = 0.5
pitchDiameter = module * nTeeth
pressureAngle = 20
addendum = module
deddendum = 1.25 * module
baseDiameter = pitchDiameter * cos(pressureAngle)
tipDiameter = pitchDiameter + 2 * module
gearHeight = 3

// Interpolate points along the involute curve
cmo = 101
rs = map(
  [0..cmo],
  f = fn(@i) {
    return baseDiameter / 2 + i / cmo * (tipDiameter - baseDiameter) / 2
  },
)

// Calculate operating pressure angle
angles = map(
  rs,
  f = fn(@r) {
    return units::toDegrees(acos(baseDiameter / 2 / r))
  },
)

// Calculate the involute function
invas = map(
  angles,
  f = fn(@a) {
    return tan(a) - units::toRadians(a)
  },
)

// Map the involute curve
xs = map(
  [0..cmo],
  f = fn(@i) {
    return rs[i] * cos(invas[i]: number(rad))
  },
)

ys = map(
  [0..cmo],
  f = fn(@i) {
    return rs[i] * sin(invas[i]: number(rad))
  },
)

// Extrude the gear body
body = startSketchOn(XY)
  |> circle(center = [0, 0], radius = baseDiameter / 2)
  |> extrude(length = gearHeight)

toothAngle = 360 / nTeeth / 1.5

// Plot the involute curve
fn leftInvolute(@i, accum) {
  j = 100 - i // iterate backwards
  return line(accum, endAbsolute = [xs[j], ys[j]])
}

fn rightInvolute(@i, accum) {
  x = rs[i] * cos(-toothAngle + units::toDegrees(atan(ys[i] / xs[i])))
  y = -rs[i] * sin(-toothAngle + units::toDegrees(atan(ys[i] / xs[i])))
  return line(accum, endAbsolute = [x, y])
}

// Draw gear teeth
start = startSketchOn(XY)
  |> startProfile(at = [xs[101], ys[101]])
teeth = reduce([0..100], initial = start, f = leftInvolute)
  |> arc(angleStart = 0, angleEnd = toothAngle, radius = baseDiameter / 2)
  |> reduce([1..101], initial = %, f = rightInvolute)
  |> close()
  |> extrude(length = gearHeight)
  |> patternCircular3d(
       axis = [0, 0, 1],
       center = [0, 0, 0],
       instances = nTeeth,
       arcDegrees = 360,
       rotateDuplicates = true,
     )

// Define the constants of the keyway and the bore hole
keywayWidth = 0.250
keywayDepth = keywayWidth / 2
holeDiam = 2
holeRadius = 1
startAngle = asin(keywayWidth / 2 / holeRadius)

// Sketch the keyway and center hole and extrude
keyWay = startSketchOn(body, face = END)
  |> startProfile(at = [
       holeRadius * cos(startAngle),
       holeRadius * sin(startAngle)
     ])
  |> xLine(length = keywayDepth)
  |> yLine(length = -keywayWidth)
  |> xLine(length = -keywayDepth)
  |> arc(angleStart = -1 * units::toDegrees(startAngle) + 360, angleEnd = 180, radius = holeRadius)
  |> arc(angleStart = 180, angleEnd = units::toDegrees(startAngle), radius = holeRadius)
  |> close()
  |> extrude(length = -gearHeight)