This model generates a hexagonal nut with: a hex exterior defined by across-flats dimension, circular chamfers applied to both end faces, and central through-hole

// Hex Nut with Chamfered Ends
// This model generates a hexagonal nut with: a hex exterior defined by across-flats dimension, circular chamfers applied to both end faces, and central through-hole
// Categories: Mechanical Components

@settings(defaultLengthUnit = mm, kclVersion = 2.0)

// Parameters
// Nut
nutAcrossCorners = 20 // Across-corners distance of the hex
nutThickness = 10 // Overall thickness of the nut
hexCircumscribedRadius = nutAcrossCorners / 2 // Radius to the hex vertices


// Chamfer
chamferCircleRadius = hexCircumscribedRadius * 1.1
chamferLength = 2.5 // Chamfer setback distance


// Hole
holeRadius = 4 // Through-hole radius


// Base profiles
// Hex exterior with center hole
hexProfile = sketch(on = XY) {
  line1 = line(start = [var 10mm, var 0mm], end = [var 5mm, var 8.66mm])
  line2 = line(start = [var 5mm, var 8.66mm], end = [var -5mm, var 8.66mm])
  line3 = line(start = [var -5mm, var 8.66mm], end = [var -10mm, var 0mm])
  line4 = line(start = [var -10mm, var 0mm], end = [var -5mm, var -8.66mm])
  line5 = line(start = [var -5mm, var -8.66mm], end = [var 5mm, var -8.66mm])
  line6 = line(start = [var 5mm, var -8.66mm], end = [var 10mm, var 0mm])

  circle1 = circle(start = [var 3.25mm, var 2.33mm], center = [var 0mm, var 0mm])
  circle2 = circle(start = [var 10mm, var 0mm], center = [var 0mm, var 0mm], construction = true)
  line7 = line(start = [var 0mm, var 0mm], end = [var 10mm, var 0mm], construction = true)

  coincident([line1.end, line2.start])
  coincident([line2.end, line3.start])
  coincident([line3.end, line4.start])
  coincident([line4.end, line5.start])
  coincident([line5.end, line6.start])

  coincident([circle2.center, ORIGIN])
  coincident([circle2.center, circle1.center])
  coincident([line7.start, circle2.center])

  coincident([circle2.start, line6.end])
  coincident([line1.start, circle2.start])
  coincident([line7.end, circle2.start])

  coincident([line2.start, circle2])
  coincident([line3.start, circle2])
  coincident([line4.start, circle2])
  coincident([line5.start, circle2])
  coincident([line6.start, circle2])

  horizontal(line7)
  horizontalDistance([line7.start, line7.end]) == nutAcrossCorners / 2
  equalLength([
    line1,
    line2,
    line3,
    line4,
    line5,
    line6
  ])
  radius(circle1) == holeRadius
}

region001 = region(segments = [hexProfile.line1, hexProfile.line2])

// Main nut body from the hex profile
nutSolid = extrude(region001, length = nutThickness)

// Auxiliary circle used to build the chamfer source solid
chamferCircleSketch = sketch(on = XY) {
  circle1 = circle(start = [var 9.57mm, var 2.89mm], center = [var 0mm, var 0mm])
  coincident([circle1.center, ORIGIN])
  radius(circle1) == nutAcrossCorners / 2 * 1.01 // Slight oversize keeps the boolean overlap stable
}

region002 = region(segments = [chamferCircleSketch.circle1])

// Auxiliary solid whose end edges are chamfered before intersecting the nut body
chamferSourceSolid = extrude(
  region002,
  length = nutThickness,
  tagStart = $chamferStartFace,
  tagEnd = $chamferEndFace,
)

// Apply chamfers to the auxiliary solid's circular end edges
chamferedCircularSolid = chamfer(
  chamferSourceSolid,
  tags = [
    getCommonEdge(faces = [region002.tags.circle1, chamferEndFace]),
    getCommonEdge(faces = [
      region002.tags.circle1,
      chamferStartFace
    ])
  ],
  length = chamferLength,
)

// Keep only the shared volume to imprint the chamfers into the hex body
nutWithChamfer = intersect([nutSolid, chamferedCircularSolid])

// Final appearance
appearance(nutWithChamfer, color = "#0040ff")

hide(hexProfile)
hide(chamferCircleSketch)


Hex Nut with Chamfered Ends

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