// Brake Caliper
// Brake calipers are used to squeeze the brake pads against the rotor, causing larger and larger amounts of friction depending on how hard the brakes are pressed.

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import caliperTolerance, caliperPadLength, caliperThickness, caliperOuterEdgeRadius, caliperInnerEdgeRadius, rotorDiameter, rotorTotalThickness, yAxisOffset from "parameters.kcl"

// Sketch the brake caliper profile
brakeCaliperSketch = startSketchOn(XY)
  |> startProfile(at = [
       rotorDiameter / 2 + caliperTolerance,
       0
     ])
  |> line(end = [
       0,
       rotorTotalThickness + caliperTolerance - caliperInnerEdgeRadius
     ])
  |> tangentialArc(angle = 90deg, radius = caliperInnerEdgeRadius)
  |> line(end = [
       -caliperPadLength + 2 * caliperInnerEdgeRadius,
       0
     ])
  |> tangentialArc(angle = -90deg, radius = caliperInnerEdgeRadius)
  |> line(end = [
       0,
       caliperThickness - (caliperInnerEdgeRadius * 2)
     ])
  |> tangentialArc(angle = -90deg, radius = caliperInnerEdgeRadius)
  |> line(end = [
       caliperPadLength + caliperThickness - caliperOuterEdgeRadius - caliperInnerEdgeRadius,
       0
     ])
  |> tangentialArc(angle = -90deg, radius = caliperOuterEdgeRadius)
  |> line(end = [
       0,
       -2 * caliperTolerance - (2 * caliperThickness) - rotorTotalThickness + 2 * caliperOuterEdgeRadius
     ])
  |> tangentialArc(angle = -90deg, radius = caliperOuterEdgeRadius)
  |> line(end = [
       -caliperPadLength - caliperThickness + caliperOuterEdgeRadius + caliperInnerEdgeRadius,
       0
     ])
  |> tangentialArc(angle = -90deg, radius = caliperInnerEdgeRadius)
  |> line(end = [
       0,
       caliperThickness - (2 * caliperInnerEdgeRadius)
     ])
  |> tangentialArc(angle = -90deg, radius = caliperInnerEdgeRadius)
  |> line(end = [
       caliperPadLength - (2 * caliperInnerEdgeRadius),
       0
     ])
  |> tangentialArc(angle = 90deg, radius = caliperInnerEdgeRadius)
  |> close()

// Revolve the brake caliper sketch
revolve(brakeCaliperSketch, axis = Y, angle = -70)
  |> appearance(color = "#c82d2d", metalness = 90, roughness = 90)


brake-caliper

// Wheel rotor
// A component of a disc brake system. It provides a surface for brake pads to press against, generating the friction needed to slow or stop the vehicle.

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import rotorDiameter, rotorInnerDiameter, rotorSinglePlateThickness, rotorInnerDiameterThickness, lugHolePatternDia, lugSpacing, rotorTotalThickness, spacerPatternDiameter, spacerDiameter, spacerLength, spacerCount, wheelDiameter, lugCount, yAxisOffset, drillAndSlotCount from "parameters.kcl"

rotorSketch = startSketchOn(XZ)
  |> circle(center = [0, 0], radius = rotorDiameter / 2)
rotor = extrude(rotorSketch, length = rotorSinglePlateThickness)
  |> appearance(color = "#dbcd70", roughness = 90, metalness = 90)

rotorBumpSketch = startSketchOn(rotor, face = END)
  |> circle(center = [0, 0], radius = rotorInnerDiameter / 2)
rotorBump = extrude(rotorBumpSketch, length = rotorInnerDiameterThickness)

lugHoles = startSketchOn(rotorBump, face = END)
  |> circle(center = [-lugSpacing / 2, 0], radius = 0.315)
  |> patternCircular2d(
       arcDegrees = 360,
       center = [0, 0],
       instances = lugCount,
       rotateDuplicates = true,
     )
  |> extrude(length = -(rotorInnerDiameterThickness + rotorSinglePlateThickness))
  |> appearance(color = "#dbcd70", roughness = 90, metalness = 90)

// (update when boolean is available)
centerSpacer = startSketchOn(rotor, face = START)
  |> circle(center = [0, 0], radius = .25)
  |> extrude(length = spacerLength)

secondaryRotorSketch = startSketchOn(centerSpacer, face = END)
  |> circle(center = [0, 0], radius = rotorDiameter / 2)
secondRotor = extrude(secondaryRotorSketch, length = rotorSinglePlateThickness)

lugHoles2 = startSketchOn(secondRotor, face = END)
  |> circle(center = [lugSpacing / 2, 0], radius = 0.315)
  |> patternCircular2d(
       arcDegrees = 360,
       center = [0, 0],
       instances = lugCount,
       rotateDuplicates = true,
     )
  |> extrude(length = -rotorSinglePlateThickness)

spacers = startSketchOn(rotor, face = START)
  |> circle(center = [spacerPatternDiameter / 2, 0], radius = spacerDiameter)
  |> extrude(length = spacerLength)
  |> patternCircular3d(
       arcDegrees = 360,
       axis = Y,
       center = [0, 0, 0],
       instances = spacerCount,
       rotateDuplicates = true,
       useOriginal = true,
     )

rotorSlottedSketch = startSketchOn(rotor, face = START)
  |> startProfile(at = [2.17, 2.56])
  |> xLine(length = 0.12)
  |> yLine(length = 2.56)
  |> xLine(length = -0.12)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()
  |> patternCircular2d(
       center = [0, 0],
       instances = drillAndSlotCount,
       arcDegrees = 360,
       rotateDuplicates = true,
     )
rotorSlotted = extrude(rotorSlottedSketch, length = -rotorSinglePlateThickness / 2)

secondRotorSlottedSketch = startSketchOn(secondRotor, face = END)
  |> startProfile(at = [-2.17, 2.56])
  |> xLine(length = -0.12)
  |> yLine(length = 2.56)
  |> xLine(length = 0.12)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()
  |> patternCircular2d(
       center = [0, 0],
       instances = drillAndSlotCount,
       arcDegrees = 360,
       rotateDuplicates = true,
     )

carRotor = extrude(secondRotorSlottedSketch, length = -rotorSinglePlateThickness / 2)
  |> appearance(color = "#dbcd70", roughness = 90, metalness = 90)


car-rotor

// Tire
// A tire is a critical component of a vehicle that provides the necessary traction and grip between the car and the road. It supports the vehicle's weight and absorbs shocks from road irregularities.

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import tireInnerDiameter, tireOuterDiameter, tireDepth, bendRadius, tireTreadWidth, tireTreadDepth, tireTreadOffset from "parameters.kcl"

// Create the sketch of the tire
tireSketch = startSketchOn(XY)
  |> startProfile(at = [tireInnerDiameter / 2, tireDepth / 2])
  |> line(
       endAbsolute = [
         tireOuterDiameter / 2 - bendRadius,
         tireDepth / 2
       ],
       tag = $edge1,
     )
  |> tangentialArc(angle = -90deg, radius = bendRadius)
  |> line(endAbsolute = [
       tireOuterDiameter / 2,
       tireDepth / 2 - tireTreadOffset
     ])
  |> xLine(length = -tireTreadDepth)
  |> yLine(length = -tireTreadWidth)
  |> xLine(length = tireTreadDepth)
  |> line(endAbsolute = [
       tireOuterDiameter / 2,
       -tireDepth / 2 + tireTreadOffset + tireTreadWidth
     ])
  |> xLine(length = -tireTreadDepth)
  |> yLine(length = -tireTreadWidth)
  |> xLine(length = tireTreadDepth)
  |> line(endAbsolute = [
       tireOuterDiameter / 2,
       -tireDepth / 2 + bendRadius
     ])
  |> tangentialArc(angle = -90deg, radius = bendRadius)
  |> line(endAbsolute = [tireInnerDiameter / 2, -tireDepth / 2], tag = $edge2)
  |> close()

// Revolve the sketch to create the tire
carTire = revolve(tireSketch, axis = Y)
  |> appearance(color = "#0f0f0f", roughness = 80)


car-tire

// Car Wheel
// A sports car wheel with a circular lug pattern and spokes.

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import lugCount, lugSpacing, offset, backSpacing, wheelWidth, wheelDiameter, spokeCount, spokeGap, spokeAngle, spokeThickness from "parameters.kcl"

// Create the wheel center
lugBase = startSketchOn(XZ)
  |> circle(center = [0, 0], radius = (lugSpacing + 1.5) / 2)
  |> subtract2d(tool = circle(center = [0, 0], radius = (lugSpacing - 1.5) / 2))
  |> extrude(length = wheelWidth / 20)

// Extend the wheel center and bore holes to accomidate the lug heads
lugExtrusion = startSketchOn(lugBase, face = END)
  |> circle(center = [0, 0], radius = (lugSpacing + 1.5) / 2)
  |> subtract2d(tool = circle(center = [0, 0], radius = (lugSpacing - 1.5) / 2))
  |> extrude(length = wheelWidth / 10)

// Create the circular pattern for the lugs
lugClearance = startSketchOn(lugExtrusion, face = END)
  |> circle(center = [lugSpacing / 2, 0], radius = 1.2 / 2)
  |> patternCircular2d(
       arcDegrees = 360,
       center = [0, 0],
       instances = lugCount,
       rotateDuplicates = true,
     )
  |> extrude(length = -wheelWidth / 10)

// Create the circular pattern for the lug holes
lugHoles = startSketchOn(lugBase, face = END)
  |> circle(center = [lugSpacing / 2, 0], radius = 16mm / 2)
  |> patternCircular2d(
       arcDegrees = 360,
       center = [0, 0],
       instances = lugCount,
       rotateDuplicates = true,
     )
  |> extrude(length = -wheelWidth / 20)
  |> appearance(color = "#ffffff", metalness = 0, roughness = 0)

// Add detail to the wheel center by revolving curved edge profiles
wheelCenterInner = startSketchOn(XY)
  |> startProfile(at = [(lugSpacing - 1.5) / 2, 0])
  |> yLine(length = -wheelWidth / 10 - (wheelWidth / 20))
  |> bezierCurve(control1 = [-0.3, 0], control2 = [0, 0.3], end = [-0.4, 0.3])
  |> yLine(endAbsolute = 0)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()
  |> revolve(axis = Y)
  |> appearance(color = "#ffffff", metalness = 0, roughness = 0)

wheelCenterOuter = startSketchOn(XY)
  |> startProfile(at = [(lugSpacing + 1.5) / 2, 0])
  |> yLine(length = -wheelWidth / 10 - (wheelWidth / 20))
  |> bezierCurve(control1 = [0.3, 0], control2 = [0.2, -0.3], end = [0.4, -0.1])
  |> yLine(endAbsolute = -wheelWidth / 20)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()
  |> revolve(axis = Y)
  |> appearance(color = "#ffffff", metalness = 0, roughness = 0)

// Write a function that defines the spoke geometry, patterns and extrudes it
fn spoke(spokeGap, spokeAngle, spokeThickness) {
  // Seperating the spoke base planes
  plane001 = {
    origin = [0.0, 0.0, spokeGap / 2],
    xAxis = [1.0, 0.0, spokeAngle],
    yAxis = [0.0, 1.0, 0.0]
  }

  // Spoke cross sections
  spokeProfile = startSketchOn(plane001)
    |> startProfile(at = [(lugSpacing + 2) / 2, -0.7])
    |> bezierCurve(
         control1 = [
           (wheelDiameter - lugSpacing - 2.9) / 3.5,
           offset / 7
         ],
         control2 = [
           (wheelDiameter - lugSpacing - 2.9) / 4,
           offset / 1.5
         ],
         end = [
           (wheelDiameter - lugSpacing - 2.9) / 2,
           offset
         ],
       )
    |> yLine(length = -wheelWidth / 15)
    |> bezierCurve(
         control1 = [
           -(wheelDiameter - lugSpacing - 2.9) / 5,
           -offset / 7
         ],
         control2 = [
           -(wheelDiameter - lugSpacing - 2.9) / 5,
           -offset / 1.5
         ],
         end = [
           -(wheelDiameter - lugSpacing - 2.9) / 2,
           -offset
         ],
       )
    |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
    |> close()

  // Circular pattern spokes
  spokePattern = extrude(spokeProfile, length = spokeThickness)
    |> patternCircular3d(
         axis = [0, 1, 0],
         center = [0, -2000, 0],
         instances = spokeCount,
         arcDegrees = 360,
         rotateDuplicates = true,
       )
    |> appearance(color = "#ffffff", metalness = 0, roughness = 0)
  return spokePattern
}

spoke(spokeGap = spokeGap, spokeAngle = spokeAngle, spokeThickness = spokeThickness)
spoke(spokeGap = -spokeGap, spokeAngle = -spokeAngle, spokeThickness = -spokeThickness)

// Define and revolve wheel exterior
startSketchOn(XY)
  |> startProfile(at = [
       wheelDiameter / 2,
       -wheelWidth + backSpacing + offset
     ])
  |> yLine(length = wheelWidth * 0.25)
  |> line(end = [-wheelWidth * 0.02, wheelWidth * 0.02])
  |> yLine(length = wheelWidth * 0.25)
  |> line(end = [wheelWidth * 0.02, wheelWidth * 0.02])
  |> yLine(endAbsolute = backSpacing + offset)
  |> line(end = [wheelWidth * 0.05, wheelWidth * .01])
  |> yLine(length = wheelWidth * 0.05)
  |> xLine(length = -wheelWidth * 0.03)
  |> yLine(length = -wheelWidth * 0.02)
  |> line(end = [-wheelWidth * 0.05, -wheelWidth * 0.01])
  |> yLine(length = -backSpacing * 0.7)
  |> line(end = [
       -wheelDiameter * 0.01,
       -wheelWidth * 0.02
     ])
  |> yLine(endAbsolute = offset - 0.2)
  |> line(end = [
       -wheelDiameter * 0.03,
       -wheelWidth * 0.02
     ])
  |> yLine(length = -wheelWidth * 0.02)
  |> line(end = [
       wheelDiameter * 0.03,
       -wheelWidth * 0.1
     ])
  |> yLine(length = -wheelWidth * 0.05)
  |> line(end = [wheelWidth * 0.02, -wheelWidth * 0.02])
  |> yLine(endAbsolute = -wheelWidth + backSpacing + offset - 0.28)
  |> line(end = [wheelWidth * 0.05, -wheelWidth * 0.01])
  |> yLine(length = -wheelWidth * 0.02)
  |> xLine(length = wheelWidth * 0.03)
  |> yLine(length = wheelWidth * 0.05)
  |> close()
  |> revolve(axis = Y)
  |> appearance(color = "#ffffff", metalness = 0, roughness = 0)


car-wheel

// Lug Nut
// lug Nuts are essential components used to create secure connections, whether for electrical purposes, like terminating wires or grounding, or for mechanical purposes, such as providing mounting points or reinforcing structural joints.

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import lugDiameter, lugHeadLength, lugThreadDiameter, lugLength, lugThreadDepth, lugSpacing from "parameters.kcl"

customPlane = {
  origin = { x = lugSpacing / 2, y = -30mm, z = 0 },
  xAxis = { x = 1, y = 0, z = 0 },
  yAxis = { x = 0, y = -1, z = 0 }
}

fn lug(plane, length, diameter) {
  lugSketch = startSketchOn(customPlane)
    |> startProfile(at = [0 + diameter / 2, 0])
    |> angledLine(angle = 70, lengthY = lugHeadLength)
    |> xLine(endAbsolute = lugDiameter / 2)
    |> yLine(endAbsolute = lugLength)
    |> tangentialArc(angle = 90deg, radius = 3mm)
    |> xLine(endAbsolute = 0 + .001, tag = $c1)
    |> yLine(endAbsolute = lugThreadDepth)
    |> xLine(endAbsolute = lugThreadDiameter)
    |> yLine(endAbsolute = 0)
    |> close()
    |> revolve(axis = Y)
    |> appearance(color = "#dbcd70", roughness = 90, metalness = 90)
  return lugSketch
}

lugNut = lug(plane = customPlane, length = lugLength, diameter = lugDiameter)


lug-nut

// Car wheel assembly parameters

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Car wheel
export lugCount = 5
export lugSpacing = 114.3mm
export offset = -35mm
export backSpacing = 6.38
export wheelWidth = 9.5
export wheelDiameter = 19
export spokeCount = 6
export spokeGap = 0.2
export spokeAngle = 0.02
export spokeThickness = 0.95

// Lug Nut
export lugDiameter = 24mm
export lugHeadLength = lugDiameter * .5
export lugThreadDiameter = lugDiameter / 2 * .85
export lugLength = 30mm
export lugThreadDepth = lugLength - 12.7mm

// Car rotor
export rotorDiameter = 12
export rotorInnerDiameter = 6
export rotorSinglePlateThickness = 0.25
export rotorInnerDiameterThickness = 0.5
export lugHolePatternDia = 3
export rotorTotalThickness = 1
export spacerPatternDiameter = 11
export spacerDiameter = 0.25
export spacerLength = rotorTotalThickness - (2 * rotorSinglePlateThickness)
export spacerCount = 16
export yAxisOffset = 0.5
export drillAndSlotCount = 5

// Car tire
export tireInnerDiameter = 19
export tireOuterDiameter = 24
export tireDepth = 11.02
export bendRadius = 1.6
export tireTreadWidth = 0.39
export tireTreadDepth = 0.39
export tireTreadOffset = 3.15

// Brake caliper
export caliperTolerance = 0.050
export caliperPadLength = 1.6
export caliperThickness = 0.39
export caliperOuterEdgeRadius = 0.39
export caliperInnerEdgeRadius = 0.12


parameters

Geometry Engine

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Zoo Developer Tools

car-wheel-assembly

car-wheel-assembly

KCL

Parts