// Herringbone Gear
// A herringbone, or double-helical gear, is a cylindrical gear type with angled teeth in opposing directions. This allows the quietness and smoothness of a helical gear, without applying a directional load while turning

// Set units
@settings(defaultLengthUnit = mm)

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

  // Define a function to create a rotated gear sketch on an offset plane
  fn herringboneGearSketch(offsetHeight) {
    // Calculate the amount to rotate each planar sketch of the gear given the gear helix angle and total gear height
    helixCalc = acos(offsetHeight * tan(helixAngle) / (tipDiameter / 2))

    // Using the gear parameters, sketch an involute tooth spanning from the base diameter to the tip diameter
    herringboneGearSketch = startSketchOn(offsetPlane(XY, offset = offsetHeight))
      |> startProfile(at = polar(angle = helixCalc, length = baseDiameter / 2))
      |> involuteCircular(
           startRadius = baseDiameter / 2,
           endRadius = tipDiameter / 2,
           angle = helixCalc,
           tag = $seg01,
         )
      |> line(endAbsolute = polar(angle = 160 / nTeeth + helixCalc, length = tipDiameter / 2))
      |> involuteCircular(
           startRadius = baseDiameter / 2,
           endRadius = tipDiameter / 2,
           angle = -(4 * atan(segEndY(seg01) / segEndX(seg01)) - (3 * helixCalc)),
           reverse = true,
         )

      // Position the end line of the sketch at the start of the next tooth
      |> line(endAbsolute = polar(angle = 360 / nTeeth + helixCalc, 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()
      // Create a center hole with an 8mm diameter
      |> subtract2d(tool = circle(center = [0, 0], radius = 4))
    return herringboneGearSketch
  }

  // Draw a gear sketch on the base plane
  gearSketch001 = herringboneGearSketch(offsetHeight = 0)

  // Draw a gear sketch that has been rotated by the helix angle
  gearSketch002 = herringboneGearSketch(offsetHeight = gearHeight / 2)

  // Draw a gear sketch at the total gear height that reverses the angle direction
  gearSketch003 = clone(gearSketch001)
    |> translate(z = gearHeight)

  // Loft each rotated gear sketch together to form a herringbone gear
  herringboneGear = loft(
    [
      gearSketch001,
      gearSketch002,
      gearSketch003
    ],
    vDegree = 1,
  )

  return herringboneGear
}

herringboneGear(
  nTeeth = 25,
  module = 1,
  pressureAngle = 14,
  helixAngle = 40,
  gearHeight = 8,
)