modeling-app/public/kcl-samples/counterdrilled-weldment/main.kcl

// Counterdrilled Weldment
// A metal weldment consisting of a counterdrilled plate, a centrally mounted housing tube, and four structural support fins.

// Set units
@settings(defaultLengthUnit = in)

// Define parameters
boltSpacingX = 5
boltSpacingY = 3
boltDiameter = 1 / 4
counterdrillDiameter = 7 / 16
counterdrillDepth = 3 / 16
tubeInnerDiameter = 1 + 1 / 4
tubeThickness = 0.115
tubeHeight = 2
stockThickness = .5

// Calculate the dimensions of the block using the specified bolt spacing. The size of the block can be defined by adding a multiple of the counterdrill diameter to the bolt spacing
blockLength = boltSpacingX + boltDiameter * 6
blockWidth = boltSpacingY + boltDiameter * 6

// Draw the base plate
plateSketch = startSketchOn(XY)
  |> startProfile(at = [-blockLength / 2, -blockWidth / 2])
  |> angledLine(angle = 0, length = blockLength, tag = $rectangleSegmentA001)
  |> angledLine(angle = segAng(rectangleSegmentA001) + 90, length = blockWidth, 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 = tubeInnerDiameter / 2))
plateBody = extrude(plateSketch, length = stockThickness)
  |> chamfer(
       length = boltDiameter * 2,
       tags = [
         getNextAdjacentEdge(rectangleSegmentB001),
         getNextAdjacentEdge(rectangleSegmentA001),
         getNextAdjacentEdge(rectangleSegmentC001),
         getNextAdjacentEdge(rectangleSegmentD001)
       ],
     )

// Define hole positions
holePositions = [
  [-boltSpacingX / 2, -boltSpacingY / 2],
  [-boltSpacingX / 2, boltSpacingY / 2],
  [boltSpacingX / 2, -boltSpacingY / 2],
  [boltSpacingX / 2, boltSpacingY / 2]
]

// Function to create a counterdrilled hole
fn counterdrill(@holePosition) {
  cbdrill = startSketchOn(plateBody, face = END)
    |> circle(center = holePosition, radius = counterdrillDiameter / 2)
    |> extrude(length = -counterdrillDepth)
  cbBolt = startSketchOn(cbdrill, face = START)
    |> circle(center = holePosition, radius = boltDiameter / 2, tag = $hole01)
    |> extrude(length = -stockThickness + counterdrillDepth)
    // Use a chamfer to create a 90-degree counterdrill edge
    |> chamfer(length = (counterdrillDiameter - boltDiameter) / 2 * sqrt(2), tags = [hole01])
  return {  }
}

// Place a counterdrilled hole at each bolt hole position
map(holePositions, f = counterdrill)

// Drill a small pin hole in the side of the tube
pinhole = startSketchOn(YZ)
  |> circle(center = [0, 2.2], radius = 0.125)
  |> extrude(length = -10)

// Model the central tube and subtract the pin hole
centralTube = startSketchOn(offsetPlane(XY, offset = stockThickness))
  |> circle(center = [0, 0], radius = tubeInnerDiameter / 2 + tubeThickness)
  |> subtract2d(tool = circle(center = [0, 0], radius = tubeInnerDiameter / 2))
  |> extrude(length = tubeHeight)
  |> subtract(tools = [pinhole])

// Create a function to create a fin which spans from the central tube to the bolt hole
fn fin(@i) {
  diagPlane = {
    origin = [0.0, 0.0, 0.0],
    xAxis = [
      boltSpacingX / 2 * i,
      boltSpacingY / 2,
      0.0
    ],
    yAxis = [0.0, 0.0, 1.0]
  }

  finSketch = startSketchOn(diagPlane)
    |> startProfile(at = [
         tubeInnerDiameter / 2 + tubeThickness,
         stockThickness
       ])
    |> xLine(endAbsolute = sqrt((boltSpacingX / 2) ^ 2 + (boltSpacingY / 2) ^ 2) - counterdrillDiameter)
    |> yLine(length = 0.15)
    |> line(endAbsolute = [
         profileStartX(%) + 0.15,
         stockThickness + tubeHeight * .8
       ])
    |> xLine(length = -0.15)
    |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
    |> close()
    |> extrude(length = tubeThickness, symmetric = true)

  // Use a circular pattern to create an identical fin on the opposite side
  otherFin = patternCircular3d(
    finSketch,
    instances = 2,
    axis = [0, 0, 1],
    center = [0, 0, 0],
    arcDegrees = 360,
    rotateDuplicates = true,
  )
  return {  }
}

// Place a pair of support fins along each diagonal axis of the bolt pattern
fin(1)
fin(-1)