A herringbone planetary gearset is a type of planetary gear system where the teeth of the sun gear, planet gears, and/or ring gear are herringbone rather than straight. This design allows for smoother, quieter operation, greater load-carrying capacity, and more flexible shaft alignment.

// Herringbone Planetary Gearset
// A herringbone planetary gearset is a type of planetary gear system where the teeth of the sun gear, planet gears, and/or ring gear are herringbone rather than straight. This design allows for smoother, quieter operation, greater load-carrying capacity, and more flexible shaft alignment.
// Categories: Automotive, Aerospace

// 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 = 160deg / 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 = 360deg / 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 = 360deg,
           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
}

// Define a function to create a ring gear
fn ringGear(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 ringGearSketch(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
    ringTeeth = 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 = 220deg / 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 = 360deg / 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 = 360deg,
           rotateDuplicates = true,
         )
      |> close()

    // Create a circular body that is larger than the tip diameter of the gear, then subtract the gear profile from the body
    ringGearSketch = startSketchOn(offsetPlane(XY, offset = offsetHeight))
      |> circle(center = [0, 0], radius = tipDiameter / 1.8)
      |> subtract2d(tool = ringTeeth)
    return ringGearSketch
  }

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

  // Draw a rotated gear sketch on a middle interstitial plane
  gearSketch002 = ringGearSketch(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 ring gear
  ringGear = loft(
    [
      gearSketch001,
      gearSketch002,
      gearSketch003
    ],
    vDegree = 1,
  )

  return ringGear
}

// Create the outer ring gear for the planetary gearset
ringGear(
  nTeeth = 58,
  module = 1.5,
  pressureAngle = 14deg,
  helixAngle = -35deg,
  gearHeight = 8,
)

// Create a central sun gear using a small herringbone gear
herringboneGear(
  nTeeth = 18,
  module = 1.5,
  pressureAngle = 14deg,
  helixAngle = 35deg,
  gearHeight = 8,
)

// Create the herringbone planet gears
numPlanetGears = 4
herringboneGear(
       nTeeth = 18,
       module = 1.5,
       pressureAngle = 14deg,
       helixAngle = -35deg,
       gearHeight = 8,
     )
  |> translate(y = 18 * 1.5 + 1.95)
  |> patternCircular3d(
       instances = numPlanetGears,
       axis = [0, 0, 1],
       center = [0, 0, 0],
       arcDegrees = 360deg,
       rotateDuplicates = false,
     )


Geometry Engine

Zoo CAD Engine Overview

KCL: A Programming Language for Parametric CAD

File Formats

A Practical Overview of CAD File Formats

Text-to-CAD

Text-to-CAD: Generating Editable, Parametric B-Rep CAD Models from Natural Language

Automation

Automating Your Workflow

herringbone-planetary-gearset