holder-rod-angle

// Holder for (shower) rod at a ~45° angle
// This is used to mount a rod to a 45° angled ceiling




@settings(defaultLengthUnit = cm)

depth = 1

length_1 = 4
length = 3
circle_center = length_1 / 2

hole_radius = 2.25 / 2 // correct size


holde_depth = 0.9

radius001 = 0.25

angle = atan(108 / 103)

angled_bracket_sketch = startSketchOn(XY)
  |> startProfile(at = [0, 0])
  |> yLine(length = length_1, tag = $seg01)
  |> angledLine(angle = -90deg + angle, lengthY = length_1, tag = $seg02)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)], tag = $seg03)
  |> close()
angled_bracket = extrude(
       angled_bracket_sketch,
       length = length_1,
       tagStart = $capStart001,
       tagEnd = $capEnd001,
     )
  |> fillet(
       radius = radius001,
       tags = [
         getCommonEdge(faces = [seg03, capStart001]),
         getCommonEdge(faces = [seg03, capEnd001]),
         getCommonEdge(faces = [seg01, capStart001]),
         getCommonEdge(faces = [seg01, capEnd001]),
         getCommonEdge(faces = [seg03, seg01])
       ],
     )

/* holder_sketch = startSketchOn(YZ)
  |> startProfile(at = [
       (length_1 - length) / 2,
       (length_1 - length) / 2
     ])
  |> yLine(length = length, tag = $h_seg02)
  |> xLine(length = length, tag = $h_seg03)
  |> yLine(length = -length, tag = $h_seg04)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)], tag = $h_seg05)
  |> close()
holder = extrude(
       holder_sketch,
       length = -depth,
       tagStart = $h_capStart001,
       tagEnd = $h_capEnd002,
     )
  |> fillet(
       radius = radius001,
       tags = [
         getCommonEdge(faces = [h_seg02, h_capStart001]),
         getCommonEdge(faces = [h_seg03, h_capStart001]),
         getCommonEdge(faces = [h_seg04, h_capStart001]),
         getCommonEdge(faces = [h_seg05, h_capStart001]),
         // outside
         getCommonEdge(faces = [h_seg02, h_seg03]),
         getCommonEdge(faces = [h_seg03, h_seg04]),
         getCommonEdge(faces = [h_seg04, h_seg05]),
         getCommonEdge(faces = [h_seg05, h_seg02])
       ],
     ) */

hole_angled_bracket_sketch = startSketchOn(-YZ, face = seg01)
hole_angled_bracket_profile = circle(hole_angled_bracket_sketch, center = [-circle_center, circle_center], radius = hole_radius)
hole_angled_bracket = extrude(hole_angled_bracket_profile, length = -holde_depth)

// hole_holder_sketch = startSketchOn(-YZ, face = seg01)  |> circle(center = [-circle_center, circle_center], radius = hole_radius)
// hold_holder = extrude(hole_holder_sketch, length = 4)

// subtract is broken right now
subtractedPart1 = subtract([angled_bracket], tools = [hole_angled_bracket])
// subtractedPart2 = subtract([holder], tools = [hold_holder])


long_length = length_1 / cos(angle)

a = cos(angle) * length_1

padding = 0.8

plate_sketch = startSketchOn(subtractedPart1, face = seg02)
plate = startProfile(plate_sketch, at = [0, -padding])
  |> xLine(length = a + padding, tag = $p_seg03)
  |> yLine(length = length_1 + 2 * padding, tag = $seg07)
  |> xLine(length = -(long_length + 2 * padding), tag = $seg06)
  |> yLine(length = -(length_1 + 2 * padding), tag = $seg04)
  |> close(tag = $seg05)

// hole_inset = 0.6
hole_inset = 0.55

hole_x = a + padding

screw_hole = 0.45 / 2

outerEdge = 0.5

plate_thickness = 0.25
screw_champfer = (0.86 - 0.45) / 2

extrude001 = extrude(
       plate,
       length = plate_thickness,
       tagStart = $capStart002,
       tagEnd = $capEnd002,
     )
  |> fillet(radius = outerEdge, tags = [getCommonEdge(faces = [seg04, seg05])])
  |> fillet(radius = outerEdge, tags = [getCommonEdge(faces = [seg06, seg04])])
  |> fillet(radius = outerEdge, tags = [getCommonEdge(faces = [seg07, seg06])])
  |> fillet(
       radius = outerEdge,
       tags = [
         getCommonEdge(faces = [p_seg03, seg07])
       ],
     )
hole_1 = startSketchOn(extrude001, face = START)
  |> circle(
       center = [
         -a + long_length + padding - hole_inset,
         -padding + hole_inset
       ],
       radius = screw_hole,
       tag = $seg12,
     )

hole_2 = startSketchOn(extrude001, face = START)
  |> circle(
       center = [
         -a - padding + hole_inset,
         length_1 + padding - hole_inset
       ],
       radius = screw_hole,
       tag = $seg11,
     )

hole_3 = startSketchOn(extrude001, face = START)
  |> circle(
       center = [
         -a - padding + hole_inset,
         -padding + hole_inset
       ],
       radius = screw_hole,
       tag = $seg10,
     )

hole_4 = startSketchOn(extrude001, face = START)
  |> circle(
       center = [
         -a + long_length + padding - hole_inset,
         length_1 + padding - hole_inset
       ],
       radius = screw_hole,
       tag = $seg08,
     )

  /* hole = startSketchOn(extrude001, face = END)
  |> circle(
       center = [
         1,1
       ],
       radius = screw_hole,
       tag = $seg09,
     ) */

  // mounting_holes = extrude([hole_2, hole_1, hole_3, hole_4], length = -1)

/* mounting_hole = extrude(hole, length = -0.2) |>  chamfer(
       length = 0.1,
       tags = [
         getCommonEdge(faces = [capEnd002, seg09])
       ],
     ) */
mounting_hole1 = extrude(hole_1, length = -plate_thickness)
  |> chamfer(
       length = screw_champfer,
       tags = [
         getCommonEdge(faces = [capStart002, seg12])
       ],
     )

mounting_hole2 = extrude(hole_2, length = -plate_thickness)
  |> chamfer(
       length = screw_champfer,
       tags = [
         getCommonEdge(faces = [capStart002, seg11])
       ],
     )

mounting_hole3 = extrude(hole_3, length = -plate_thickness)
  |> chamfer(
       length = screw_champfer,
       tags = [
         getCommonEdge(faces = [capStart002, seg10])
       ],
     )

mounting_hole4 = extrude(hole_4, length = -plate_thickness)
  |> chamfer(
       length = screw_champfer,
       tags = [
         getCommonEdge(faces = [capStart002, seg08])
       ],
     )