shepherds-hook-bolt

// Shepherd’s Hook Bolt // A bent bolt with a curved hook, typically used for hanging or anchoring loads. The threaded end allows secure attachment to surfaces or materials, while the curved hook resists pull-out under tension.  // Set units in millimeters (mm) @settings(defaultLengthUnit = mm, kclVersion = 1.0)  // Define bolt geometry parameters boltDiameter = 5 hookRadius = 12 shankLength = 5 threadedEndLength = 30 nutDistance = 20 hookStartAngle = 290deg hookEndAngle = 150deg  approximatePitch = boltDiameter * 0.15 threadDepth = 0.6134 * approximatePitch innerRadius = boltDiameter / 2 - threadDepth boltNumberOfRevolutions = threadedEndLength / approximatePitch  // Helper values for computing geometry transitions between straight shaft and hook arc hypotenuse = hookRadius / cos(hookStartAngle - 270deg) side = sqrt(pow(hypotenuse, exp = 2) - pow(hookRadius, exp = 2)) shankOffset = hypotenuse + side  // Converts polar coordinates to cartesian points for drawing arcs fn polarToCartesian(radius, angle) {  x = radius * cos(angle)  y = radius * sin(angle)  return [x, y] }  // Create the hook and shank profile path // Includes straight segment and two connected arcs forming the hook hookProfilePlane = startSketchOn(XZ) hookProfileShape = startProfile(hookProfilePlane, at = [0, -shankOffset - shankLength])  |> line(endAbsolute = [0, -shankOffset])  |> tangentialArc(endAbsolute = polarToCartesian(radius = hookRadius, angle = hookStartAngle))  |> tangentialArc(endAbsolute = polarToCartesian(radius = hookRadius, angle = hookEndAngle), tag = $hook)  // Create the circular cross-section used for sweeping along the hook path hookSectionPlane = offsetPlane(XY, offset = -shankOffset - shankLength) hookSectionShape = circle(hookSectionPlane, center = [0, 0], radius = boltDiameter / 2)  // Sweep the section along the hook profile to form the main body of the hook bolt hookBody = sweep(hookSectionShape, path = hookProfileShape, sectional = true)  // Add a cylindrical tip at the hook end tipPlane = startSketchOn(hookBody, face = END) tipShape = circle(  tipPlane,  center = [hookRadius, 0],  radius = boltDiameter / 2,  tag = $seg01, ) tipBody = extrude(  tipShape,  length = hookRadius * 0.5,  tagStart = $startTag,  tagEnd = $capEnd001,  )  |> fillet(  radius = boltDiameter / 4,  tags = [  getCommonEdge(faces = [seg01, capEnd001])  ],  )   // Create the threaded end of the bolt  // Construct the triangular profile for thread cutting boltThreadSectionPlane = startSketchOn(XZ) boltThreadSectionShapeForRevolve = startProfile(  boltThreadSectionPlane,  at = [  innerRadius,  -shankOffset - shankLength - threadedEndLength  ],  )  |> line(end = [threadDepth, approximatePitch / 2])  |> line(end = [-threadDepth, approximatePitch / 2])  |> patternLinear2d(axis = [0, 1], instances = boltNumberOfRevolutions, distance = approximatePitch)  |> xLine(length = -innerRadius * 0.9)  |> yLine(length = -threadedEndLength)  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])  |> close()  // Create a revolved solid representing the thread geometry by repeating and revolving the profile around the shaft boltThreadRevolve = revolve(boltThreadSectionShapeForRevolve, angle = 360deg, axis = Y)