hex-nut-with-chamfer

// Hex Nut with Chamfered Ends and Through-Hole
// 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

@settings(defaultLengthUnit = mm)

// ──────────
// PARAMETERS
// ──────────
// Primary nut dimensions
nutAcrossCorners = 20 // Across-corners distance of the hex
nutThickness = 10 // Overall thickness of the nut (extrusion length)
hexCircumscribedRadius = nutAcrossCorners / 2 // Radius to hex vertices for a regular 6-sided polygon


// Chamfer control
chamferCircleRadius = hexCircumscribedRadius * 1.1 // Radius of the auxiliary circular solid used to define chamfer edges
chamferLength = 3.5 // Chamfer setback distance along the end edges


// Hole control
holeRadius = 4 // Radius of the central through-hole


// ───────────────────────
// 2D PROFILES ON XY PLANE
// ───────────────────────


baseSketch = startSketchOn(XY)

// Auxiliary circle used to produce circular end edges for chamfering
chamferCircleSketch = circle(
  baseSketch,
  center = [0, 0],
  radius = chamferCircleRadius,
  tag = $chamferCircleTag,
)

// Hex nut exterior profile (regular hexagon, circumscribed about hexCircumscribedRadius)
hexProfile = polygon(
  baseSketch,
  radius = hexCircumscribedRadius,
  numSides = 6,
  center = [0, 0],
)

// Central hole sketch (axis-aligned with the nut center)
holeSketch = circle(baseSketch, center = [0, 0], radius = holeRadius)

// ─────────
// 3D SOLIDS
// ─────────

// Hex nut main body created from the hex profile
nutSolid = extrude(hexProfile, length = nutThickness)

// Circular auxiliary solid; its start/end faces provide the circular edges for chamfering
chamferSourceSolid = extrude(
  chamferCircleSketch,
  length = nutThickness,
  tagStart = $chamferStartFace,
  tagEnd = $chamferEndFace,
)

// Apply chamfers to both circular end edges of the auxiliary solid
chamferedCircularSolid = chamfer(
  chamferSourceSolid,
  tags = [
    getCommonEdge(faces = [chamferCircleTag, chamferStartFace]),
    // Edge at start face perimeter
    getCommonEdge(faces = [chamferCircleTag, chamferEndFace]),
    // Edge at end face perimeter
  ],
  length = chamferLength,
)

// Through-hole solid created from the center circle (used as subtraction tool)
holeSolid = extrude(holeSketch, length = nutThickness)

// ──────────────────────────────
// BOOLEAN COMPOSITION OF FEATURES
// ──────────────────────────────

// Keep only the overlapping volume of the hex body and the chamfered circular solid
// This imprints the circular chamfers into the hex nut geometry
nutWithChamfer = intersect([nutSolid, chamferedCircularSolid])

// Subtract the central cylindrical hole from the nut
finishedNut = subtract(nutWithChamfer, tools = holeSolid)

// Apply a visual appearance to the finished nut
appearance(finishedNut, color = "#0040ff")