A CPU cooler is a device designed to dissipate heat generated by the CPU of a computer. They consist of a brazed heat sink made from aluminum or copper alloys, and one or two axial fans to move airflow across the heat sink.

// CPU Cooler
// A CPU cooler is a device designed to dissipate heat generated by the CPU of a computer. They consist of a brazed heat sink made from aluminum or copper alloys, and one or two axial fans to move airflow across the heat sink.
// Categories: Computer Hardware

// Set units
@settings(defaultLengthUnit = mm)

// Import all parts and parameters into assembly file
import * from "parameters.kcl"
import "fan-housing.kcl" as fanHousing
import "motor.kcl" as motor
import "fan.kcl" as fan
import "heat-sink.kcl" as heatSink
import "mounting-wire.kcl" as mountingWire
import "removable-sticker.kcl" as removableSticker

// Produce the model for each imported part
heatSink

fn translatePart(part) {
  part
    |> translate(x = heatSinkDepth / 2, z = 40 + fanSize / 2)
    |> patternLinear3d(instances = 2, distance = heatSinkDepth + fanHeight, axis = [-1, 0, 0])
  return {  }
}
translatePart(part = fanHousing)
translatePart(part = motor)
translatePart(part = fan)

mountingWire
  |> patternCircular3d(
       instances = 2,
       axis = [0, 1, 0],
       center = [0, 0, 40 + fanSize / 2],
       arcDegrees = 360deg,
       rotateDuplicates = true,
     )
  |> patternCircular3d(
       instances = 2,
       axis = [0, 0, 1],
       center = [0, 0, 0],
       arcDegrees = 360deg,
       rotateDuplicates = true,
     )
removableSticker


// Fan Housing
// The plastic housing that contains the fan and the motor

// Set units
@settings(defaultLengthUnit = mm)

// Import parameters
import * from "parameters.kcl"

// Model the housing which holds the motor, the fan, and the mounting provisions
// Bottom mounting face
bottomFaceSketch = startSketchOn(YZ)
  |> startProfile(at = [-fanSize / 2, -fanSize / 2])
  |> angledLine(angle = 0, length = fanSize, tag = $rectangleSegmentA001)
  |> angledLine(angle = segAng(rectangleSegmentA001) + 90deg, length = fanSize, tag = $rectangleSegmentB001)
  |> angledLine(angle = segAng(rectangleSegmentA001), length = -segLen(rectangleSegmentA001), tag = $rectangleSegmentC001)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)], tag = $rectangleSegmentD001)
  |> close()
  |> subtract2d(tool = circle(center = [0, 0], radius = 4))
  |> subtract2d(tool = circle(
       center = [
         mountingHoleSpacing / 2,
         mountingHoleSpacing / 2
       ],
       radius = mountingHoleSize / 2,
     ))
  |> subtract2d(tool = circle(
       center = [
         -mountingHoleSpacing / 2,
         mountingHoleSpacing / 2
       ],
       radius = mountingHoleSize / 2,
     ))
  |> subtract2d(tool = circle(
       center = [
         mountingHoleSpacing / 2,
         -mountingHoleSpacing / 2
       ],
       radius = mountingHoleSize / 2,
     ))
  |> subtract2d(tool = circle(
       center = [
         -mountingHoleSpacing / 2,
         -mountingHoleSpacing / 2
       ],
       radius = mountingHoleSize / 2,
     ))
  |> extrude(length = 4)

// Add large openings to the bottom face to allow airflow through the fan
airflowPattern = startSketchOn(bottomFaceSketch, face = END)
  |> startProfile(at = [fanSize * 7 / 25, -fanSize * 9 / 25])
  |> angledLine(angle = 140deg, length = fanSize * 12 / 25, tag = $seg01)
  |> tangentialArc(radius = fanSize * 1 / 50, angle = 90deg)
  |> angledLine(angle = -130deg, length = fanSize * 8 / 25)
  |> tangentialArc(radius = fanSize * 1 / 50, angle = 90deg)
  |> angledLine(angle = segAng(seg01) + 180deg, length = fanSize * 2 / 25)
  |> tangentialArc(radius = fanSize * 8 / 25, angle = 40deg)
  |> xLine(length = fanSize * 3 / 25)
  |> tangentialArc(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()
  |> patternCircular2d(
       instances = 4,
       center = [0, 0],
       arcDegrees = 360,
       rotateDuplicates = true,
     )
  |> extrude(length = -4)

// Create the middle segment of the fan housing body
housingMiddleLength = fanSize / 3
housingMiddleRadius = fanSize / 3 - 1
bodyMiddle = startSketchOn(bottomFaceSketch, face = END)
  |> startProfile(at = [
       housingMiddleLength / 2,
       -housingMiddleLength / 2 - housingMiddleRadius
     ])
  |> tangentialArc(radius = housingMiddleRadius, angle = 90deg)
  |> yLine(length = housingMiddleLength)
  |> tangentialArc(radius = housingMiddleRadius, angle = 90deg)
  |> xLine(length = -housingMiddleLength)
  |> tangentialArc(radius = housingMiddleRadius, angle = 90deg)
  |> yLine(length = -housingMiddleLength)
  |> tangentialArc(radius = housingMiddleRadius, angle = 90deg)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> extrude(length = fanHeight - 4 - 4)

// Cut a hole in the body to accommodate the fan
bodyFanHole = startSketchOn(bodyMiddle, face = END)
  |> circle(center = [0, 0], radius = fanSize * 23 / 50)
  |> extrude(length = -(fanHeight - 4 - 4))

// Top mounting face. Cut a hole in the face to accommodate the fan
topFaceSketch = startSketchOn(bodyMiddle, face = END)
topHoles = startProfile(topFaceSketch, at = [-fanSize / 2, -fanSize / 2])
  |> angledLine(angle = 0, length = fanSize, tag = $rectangleSegmentA002)
  |> angledLine(angle = segAng(rectangleSegmentA002) + 90, length = fanSize, tag = $rectangleSegmentB002)
  |> angledLine(angle = segAng(rectangleSegmentA002), length = -segLen(rectangleSegmentA002), tag = $rectangleSegmentC002)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)], tag = $rectangleSegmentD002)
  |> close()
  |> subtract2d(tool = circle(center = [0, 0], radius = fanSize * 23 / 50))
  |> subtract2d(tool = circle(
       center = [
         mountingHoleSpacing / 2,
         mountingHoleSpacing / 2
       ],
       radius = mountingHoleSize / 2,
     ))
  |> subtract2d(tool = circle(
       center = [
         -mountingHoleSpacing / 2,
         mountingHoleSpacing / 2
       ],
       radius = mountingHoleSize / 2,
     ))
  |> subtract2d(tool = circle(
       center = [
         mountingHoleSpacing / 2,
         -mountingHoleSpacing / 2
       ],
       radius = mountingHoleSize / 2,
     ))
  |> subtract2d(tool = circle(
       center = [
         -mountingHoleSpacing / 2,
         -mountingHoleSpacing / 2
       ],
       radius = mountingHoleSize / 2,
     ))
  |> extrude(length = 4)

// Create a housing for the electric motor to sit
motorHousing = startSketchOn(bottomFaceSketch, face = END)
  |> circle(center = [0, 0], radius = 11.2)
  |> extrude(length = 16)

startSketchOn(motorHousing, face = END)
  |> circle(center = [0, 0], radius = 10)
  |> extrude(length = -16)
  |> appearance(color = "#a55e2c")
  |> fillet(
       radius = abs(fanSize - mountingHoleSpacing) / 2,
       tags = [
         getNextAdjacentEdge(rectangleSegmentA001),
         getNextAdjacentEdge(rectangleSegmentB001),
         getNextAdjacentEdge(rectangleSegmentC001),
         getNextAdjacentEdge(rectangleSegmentD001),
         getNextAdjacentEdge(rectangleSegmentA002),
         getNextAdjacentEdge(rectangleSegmentB002),
         getNextAdjacentEdge(rectangleSegmentC002),
         getNextAdjacentEdge(rectangleSegmentD002)
       ],
     )


// Fan
// Spinning axial fan that moves airflow

// Set units
@settings(defaultLengthUnit = mm)

// Import parameters
import * from "parameters.kcl"

// Model the center of the fan
fanCenter = startSketchOn(YZ)
  |> circle(center = [0, 0], radius = fanHeight / 2, tag = $centerBend)
  |> extrude(length = fanHeight)
  |> fillet(radius = 1.5, tags = [getOppositeEdge(centerBend)])

// Create a function for a lofted fan blade cross section that rotates about the center hub of the fan
fn fanBlade(offsetHeight, startAngle) {
  fanBlade = startSketchOn(offsetPlane(YZ, offset = offsetHeight))
    |> startProfile(at = [
         15 * cos(startAngle),
         15 * sin(startAngle)
       ])
    |> arc(angleStart = startAngle, angleEnd = startAngle + 14deg, radius = 15)
    |> arc(
         endAbsolute = [
           fanSize * 22 / 50 * cos(startAngle - 20deg),
           fanSize * 22 / 50 * sin(startAngle - 20deg)
         ],
         interiorAbsolute = [
           fanSize * 11 / 50 * cos(startAngle + 3deg),
           fanSize * 11 / 50 * sin(startAngle + 3deg)
         ],
       )
    |> arc(
         endAbsolute = [
           fanSize * 22 / 50 * cos(startAngle - 24deg),
           fanSize * 22 / 50 * sin(startAngle - 24deg)
         ],
         interiorAbsolute = [
           fanSize * 22 / 50 * cos(startAngle - 22deg),
           fanSize * 22 / 50 * sin(startAngle - 22deg)
         ],
       )
    |> arc(
         endAbsolute = [profileStartX(%), profileStartY(%)],
         interiorAbsolute = [
           fanSize * 11 / 50 * cos(startAngle - 5deg),
           fanSize * 11 / 50 * sin(startAngle - 5deg)
         ],
       )
    |> close()
  return fanBlade
}

// Loft the fan blade cross sections into a single blade, then pattern them about the fan center
crossSections = [
  fanBlade(offsetHeight = 4.5, startAngle = 50deg),
  fanBlade(offsetHeight = (fanHeight - 2 - 4) / 2, startAngle = 30deg),
  fanBlade(offsetHeight = fanHeight - 2, startAngle = 0)
]
bladeLoft = loft(crossSections)
  |> patternCircular3d(
       instances = 9,
       axis = [1, 0, 0],
       center = [0, 0, 0],
       arcDegrees = 360deg,
       rotateDuplicates = true,
     )

[fanCenter, bladeLoft]
  |> appearance(color = "#110803")


// Heat Sink
// Conductive metal device made from brazed tubes and fins

// Set units
@settings(defaultLengthUnit = mm)

// Import parameters
import * from "parameters.kcl"

// Draw the sweep path for the outermost tubes
endTubePath = startSketchOn(offsetPlane(YZ, offset = -20))
  |> startProfile(at = [fanSize / 4, fanSize + 38])
  |> yLine(endAbsolute = bendRadius + 10, tag = $seg01)
  |> tangentialArc(radius = bendRadius, angle = -90deg)
  |> xLine(endAbsolute = 0, tag = $seg02)
  |> xLine(length = -segLen(seg02))
  |> tangentialArc(radius = bendRadius, angle = -90deg)
  |> yLine(length = segLen(seg01))

// Sweep and translate the outermost tube on each end
endTube = startSketchOn(offsetPlane(XY, offset = fanSize + 38))
  |> circle(center = [-20, fanSize / 4], radius = 3)
  |> subtract2d(tool = circle(center = [-20, fanSize / 4], radius = 2.5))
  |> sweep(path = endTubePath)
  |> patternCircular3d(
       instances = 2,
       axis = [0, 0, 1],
       center = [0, 0, 0],
       arcDegrees = 360,
       rotateDuplicates = false,
     )

// Draw the sweep path for the 4 interior tubes
centerTubePath = startSketchOn(offsetPlane(YZ, offset = -4))
  |> startProfile(at = [fanSize / 2.67, fanSize + 38])
  |> yLine(endAbsolute = bendRadius + 15 + 10)
  |> tangentialArc(radius = bendRadius, angle = -45deg)
  |> angledLine(angle = -135deg, lengthY = 15)
  |> tangentialArc(radius = bendRadius, angle = -45deg)
  |> xLine(endAbsolute = 0, tag = $seg03)
  |> xLine(length = -segLen(seg03))
  |> tangentialArc(radius = bendRadius, angle = -155deg)
  |> tangentialArc(radius = bendRadius, angle = 65deg)
  |> yLine(endAbsolute = fanSize + 38)

// Draw the profile and sweep the 4 interior tubes
centerTube = startSketchOn(offsetPlane(XY, offset = fanSize + 38))
  |> circle(center = [-4, fanSize / 2.67], radius = 3)
  |> subtract2d(tool = circle(center = [-4, fanSize / 2.67], radius = 2.5))
  |> sweep(path = centerTubePath)
  |> patternCircular3d(
       instances = 2,
       axis = [0, 0, 1],
       center = [-4 * 2, 0, 0],
       arcDegrees = 360,
       rotateDuplicates = true,
     )
  |> patternLinear3d(instances = 2, distance = 4 * 4, axis = [1, 0, 0])

// Draw a heat fin with built-in clips to secure the mounting wire. Pattern the fin upwards by the height of the fan
heatFins = startSketchOn(offsetPlane(XY, offset = 45))
  |> startProfile(at = [0, -fanSize / 2])
  |> xLine(length = 9)
  |> angledLine(angle = -60deg, length = 2.5, tag = $seg04)
  |> xLine(length = 0.75)
  |> arc(interiorAbsolute = [lastSegX(%) + 1, lastSegY(%) + 1.2], endAbsolute = [lastSegX(%) + 2, lastSegY(%)])
  |> xLine(length = 0.75)
  |> angledLine(angle = 60deg, length = segLen(seg04))
  |> xLine(endAbsolute = heatSinkDepth / 2 - 3)
  |> tangentialArc(angle = 90deg, radius = 3)
  |> yLine(endAbsolute = 0)
  |> mirror2d(axis = X)
  |> mirror2d(axis = Y)
  |> close()
  |> extrude(length = 1)
  |> patternLinear3d(instances = 31, distance = (fanSize - 10) / 30, axis = [0, 0, 1])

// Create the mounting base for the CPU cooler. The base should consist of two pieces that secure around each of the tubes at the bottom
coolerBase = startSketchOn(-XZ)
baseLower = startProfile(coolerBase, at = [0, 10])
  |> xLine(length = -0.9)
  |> arc(angleStart = 0, angleEnd = -180deg, radius = 3.1)
  |> xLine(length = -1.8)
  |> arc(angleStart = 0, angleEnd = -180deg, radius = 3)
  |> xLine(length = -1.8)
  |> arc(angleStart = 0, angleEnd = -180deg, radius = 3)
  |> xLine(length = -1.8)
  |> xLine(length = -2)
  |> yLine(length = -10)
  |> xLine(endAbsolute = 0)
  |> mirror2d(axis = Y)
  |> extrude(length = 2 * segLen(seg02), symmetric = true)

baseUpper = startProfile(coolerBase, at = [0, 10])
  |> xLine(length = -0.9)
  |> arc(angleStart = 0, angleEnd = 180deg, radius = 3.1)
  |> xLine(length = -1.8)
  |> arc(angleStart = 0, angleEnd = 180deg, radius = 3)
  |> xLine(length = -1.8)
  |> arc(angleStart = 0, angleEnd = 180deg, radius = 3)
  |> xLine(length = -1.8)
  |> xLine(length = -1)
  |> yLine(length = 4)
  |> tangentialArc(angle = -90deg, radius = 2)
  |> xLine(endAbsolute = 0)
  |> mirror2d(axis = Y)
  |> extrude(length = 2 * segLen(seg02) * 3 / 4, symmetric = true)

// Create a flexible mounting bracket to secure the heat sink to the motherboard once adhered
mountingBracket = startSketchOn(XZ)
  |> startProfile(at = [-10, 16])
  |> xLine(length = -20)
  |> tangentialArc(angle = 20deg, radius = bendRadius)
  |> angledLine(angle = -160deg, length = 14, tag = $seg09)
  |> tangentialArc(angle = -30deg, radius = bendRadius + sheetThickness)
  |> angledLine(angle = 170deg, length = 21.5, tag = $seg04Q)
  |> angledLine(angle = 170deg - 90, length = sheetThickness, tag = $seg08)
  |> angledLine(angle = segAng(seg04Q) + 180deg, length = segLen(seg04Q), tag = $seg05E)
  |> tangentialArc(angle = 30deg, radius = bendRadius)
  |> angledLine(angle = segAng(seg09) + 180deg, length = segLen(seg09))
  |> tangentialArc(angle = -20deg, radius = bendRadius + sheetThickness)
  |> xLine(endAbsolute = profileStartX(%))
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)], tag = $seg07)
  |> close()
  |> extrude(
       length = 16,
       symmetric = true,
       tagEnd = $capEnd001,
       tagStart = $capStart001,
     )
  |> fillet(
       radius = 2,
       tags = [
         getCommonEdge(faces = [seg07, capEnd001]),
         getCommonEdge(faces = [seg08, capEnd001]),
         getCommonEdge(faces = [seg08, capStart001]),
         getCommonEdge(faces = [seg07, capStart001])
       ],
     )

// Create a clearance hole in the bracket for an M3 screw and countersink the hole
thruHole = startSketchOn(mountingBracket, face = seg05E)
  |> circle(center = [70, 0], radius = 3.4 / 2, tag = $seg06E)
  |> extrude(length = -sheetThickness)
  |> chamfer(
       length = sheetThickness * 0.75,
       tags = [
         getCommonEdge(faces = [seg05E, seg06E])
       ],
     )

  // Duplicate the bracket to the other side of the heat sink base
  |> patternCircular3d(
       instances = 2,
       axis = [0, 0, 1],
       center = [0, 0, 0],
       arcDegrees = 360deg,
       rotateDuplicates = true,
     )


// Motor
// A small electric motor to power the fan

// Set Units
@settings(defaultLengthUnit = mm)

// Import Parameters
import * from "parameters.kcl"

// Model the motor body and stem
startPlane = offsetPlane(YZ, offset = 4)
motorBody = startSketchOn(startPlane)
  |> circle(center = [0, 0], radius = 10, tag = $seg04)
  |> extrude(length = 17)
  |> fillet(radius = 2, tags = [getOppositeEdge(seg04), seg04])
  |> appearance(color = "#021b55")
motorStem = startSketchOn(offsetPlane(YZ, offset = 21))
  |> circle(center = [0, 0], radius = 1)
  |> extrude(length = 3.8)
  |> appearance(color = "#cbcccd")
[motorBody, motorStem]


// Mounting Wire
// The flexible metal wire used to clip the fans onto the heat sink

// Set units
@settings(defaultLengthUnit = mm)

// Import parameters
import * from "parameters.kcl"

// Draw the XZ component of the mounting wire path
upperArm = startSketchOn(offsetPlane(XZ, offset = fanSize / 2 + 2))
  |> startProfile(at = [-12, 40 + fanSize / 2])
  |> yLine(length = 7)
  |> tangentialArc(radius = 2, angle = 90deg)
  |> xLine(length = -9)
  |> tangentialArc(radius = 2, angle = -90deg)
  |> yLine(length = 14)
  |> tangentialArc(radius = 2, angle = 90deg)
  |> xLine(length = -9)
  |> tangentialArc(radius = 2, angle = -80deg)
  |> angledLine(angle = 100deg, endAbsoluteY = 40 + fanSize / 2 + mountingHoleSpacing / 2 - 1.5)
  |> tangentialArc(radius = 2, angle = 80deg, tag = $seg07)

// Draw the XZ component of the mounting wire path
lowerArm = startSketchOn(offsetPlane(XZ, offset = fanSize / 2 + 2))
  |> startProfile(at = [-12, 40 + fanSize / 2])
  |> yLine(length = -7)
  |> tangentialArc(radius = 2, angle = -90deg)
  |> xLine(length = -9)
  |> tangentialArc(radius = 2, angle = 90deg)
  |> yLine(length = -14)
  |> tangentialArc(radius = 2, angle = -90deg)
  |> xLine(length = -9)
  |> tangentialArc(radius = 2, angle = 80deg)
  |> angledLine(angle = -100deg, endAbsoluteY = 40 + fanSize / 2 - (mountingHoleSpacing / 2) + 1.5)
  |> tangentialArc(radius = 2, angle = -80deg, tag = $seg08)

// Create the profile of the mounting wire and sweep along the XZ path
wireProfile = startSketchOn(offsetPlane(XY, offset = 40 + fanSize / 2))
sweepUpperArm = circle(wireProfile, center = [-12, -fanSize / 2 - 2], radius = 1)
  |> sweep(path = upperArm)

sweepLowerArm = circle(wireProfile, center = [-12, -fanSize / 2 - 2], radius = 1)
  |> sweep(path = lowerArm)

// Draw the XY components of the mounting wire path
upperHook = startSketchOn(offsetPlane(XY, offset = segEndY(seg07)))
  |> startProfile(at = [segEndX(seg07), -fanSize / 2 - 2])
  |> xLine(endAbsolute = -heatSinkDepth / 2 - fanHeight)
  |> tangentialArc(radius = 2, angle = -90deg)
  |> yLine(endAbsolute = -mountingHoleSpacing / 2 - 2)
  |> tangentialArc(radius = 2, angle = -90deg)
  |> xLine(length = fanHeight / 3)

// Draw the XY components of the mounting wire path
lowerHook = startSketchOn(offsetPlane(XY, offset = segEndY(seg08)))
  |> startProfile(at = [segEndX(seg07), -fanSize / 2 - 2])
  |> xLine(endAbsolute = -heatSinkDepth / 2 - fanHeight)
  |> tangentialArc(radius = 2, angle = -90deg)
  |> yLine(endAbsolute = -mountingHoleSpacing / 2 - 2)
  |> tangentialArc(radius = 2, angle = -90deg)
  |> xLine(length = fanHeight / 3)

// Sweep the wire profile around the hook-shaped segments of the mounting wire
hookProfile = startSketchOn(offsetPlane(YZ, offset = segEndX(seg07)))
sweepUpperHook = circle(hookProfile, center = [-fanSize / 2 - 2, segEndY(seg07)], radius = 1)
  |> sweep(path = upperHook)

sweepLowerHook = circle(hookProfile, center = [-fanSize / 2 - 2, segEndY(seg08)], radius = 1)
  |> sweep(path = lowerHook)

// Union each piece of the wire into a single continuous sweep
[
       sweepLowerArm,
       sweepLowerHook,
       sweepUpperArm,
       sweepUpperHook
     ]
  |> appearance(color = "#0d0d0d")


// Global parameters for the CPU cooler

// Set units
@settings(defaultLengthUnit = mm)

// Define Parameters
export fanSize = 120
export fanHeight = 25
export mountingHoleSpacing = 105
export mountingHoleSize = 4.5
export bendRadius = 15
export sheetThickness = 2.125
export heatSinkDepth = 55


// Removable Sticker
// Protective sticker to be removed before adhering the heat sink to the CPU

// Set units
@settings(defaultLengthUnit = mm)

// Create a simple body to represent the removable warning sticker. Brightly color the sticker so that the user will not forget to remove it before installing the device
removableSticker = startSketchOn(-XY)
  |> startProfile(at = [-12, -12])
  |> angledLine(angle = 0, length = 24, tag = $rectangleSegmentA001)
  |> angledLine(angle = segAng(rectangleSegmentA001) + 90deg, length = 24, tag = $rectangleSegmentB001)
  |> angledLine(angle = segAng(rectangleSegmentA001), length = -segLen(rectangleSegmentA001), tag = $rectangleSegmentC001)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)], tag = $rectangleSegmentD001)
  |> close()
  |> extrude(length = .3)
  |> appearance(color = "#021b55")
  |> chamfer(
       length = 3,
       tags = [
         getNextAdjacentEdge(rectangleSegmentA001),
         getNextAdjacentEdge(rectangleSegmentB001),
         getNextAdjacentEdge(rectangleSegmentC001),
         getNextAdjacentEdge(rectangleSegmentD001)
       ],
     )


cpu-cooler

KCL