propellant-line-brackets

// Propellant Line Bracket
// A propellant line bracket is a mechanical support structure used to secure and stabilize propellant lines in an aerospace vehicle — such as a rocket, spacecraft, or launch platform. These brackets ensure that the fluid lines remain safely in place throughout the vehicle's lifecycle: during assembly, launch, flight, and possibly reentry or landing. These typically come with p-clamps or other types of clamping to secure the tubes.

// Define units
@settings(defaultLengthUnit = in)

// Define parameters
bracketWidth = 2
bracketLength = 4
bracketFlangeHeight = 1.5
bendRadius = 0.25
bracketThickness = 0.25
holeDiameter = 0.5
holeXy = [
  [-1, bracketLength - .5],
  [-1.5, bracketLength / 2],
  [-1, 0.5]
]

// Sketch the bracket body
bracketSketch = startSketchOn(YZ)
profile001 = startProfile(bracketSketch, at = [0, 0])
  |> xLine(length = bracketWidth, tag = $seg03)
  |> yLine(length = bracketThickness, tag = $seg06)
  |> xLine(length = -bracketWidth + bracketThickness, tag = $seg01)
  |> yLine(endAbsolute = bracketFlangeHeight, tag = $seg02)
  |> xLine(endAbsolute = 0, tag = $seg05)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)], tag = $seg04)
  |> close()

// Extrude the bracket sketch to make the body. Add fillets to all corners.
bracketExtrude = extrude(
       profile001,
       length = bracketLength,
       tagStart = $capStart001,
       tagEnd = $capEnd001,
     )
  |> fillet(radius = .125, tags = [getCommonEdge(faces = [seg01, seg02])])
  |> fillet(radius = .25, tags = [getCommonEdge(faces = [seg03, seg04])])
  |> fillet(
       radius = .125,
       tags = [
         getCommonEdge(faces = [seg06, capEnd001]),
         getCommonEdge(faces = [seg06, capStart001]),
         getCommonEdge(faces = [seg05, capStart001]),
         getCommonEdge(faces = [seg05, capEnd001])
       ],
     )

// Create mounting holes on the bottom face of the bracket.
sketch002 = startSketchOn(bracketExtrude, face = seg01)
profile002 = circle(sketch002, center = [holeXy[0][0], holeXy[0][1]], radius = holeDiameter / 2)
profile003 = circle(sketch002, center = [holeXy[1][0], holeXy[1][1]], radius = holeDiameter / 2)
profile004 = circle(sketch002, center = [holeXy[2][0], holeXy[2][1]], radius = holeDiameter / 2)
bottomHoles = extrude([profile002, profile003, profile004], length = -.25)

// Create the mounting holes on the side face of the bracket.
sketch003 = startSketchOn(bracketExtrude, face = seg02)
profile005 = circle(sketch003, center = [-.5, 1], radius = holeDiameter / 2)
profile006 = circle(sketch003, center = [-bracketLength + .5, 1], radius = holeDiameter / 2)
extrude001 = extrude([profile006, profile005], length = -.25)
  |> appearance(%, color = "#a18e30")

  // P-Clamp
  // is a metal bracket shaped like the letter “P” that is used to secure pipes, tubing, hoses, or cables to a structure. It’s widely used in aerospace, automotive, and industrial applications to keep lines in place and isolate them from vibration and abrasion.

// Define parameters
tubeDiameter = 1.5
width = 1
thickness = .125

// Sketch the profile of the P-clamp
pClampSketch = startSketchOn(-XZ)
profile007 = startProfile(pClampSketch, at = [0, 0])
  |> xLine(length = -2, tag = $seg003)
  |> tangentialArc(radius = tubeDiameter / 2 + thickness, angle = -300deg)
  |> xLine(endAbsolute = 0, tag = $seg004)
  |> yLine(length = -thickness, tag = $seg005)
  |> xLine(endAbsolute = -1.5)
  |> arc(
       interiorAbsolute = [
         -2 - (cos(90deg) * tubeDiameter),
         sin(90deg) * tubeDiameter + thickness
       ],
       endAbsolute = [-2, thickness],
     )
  |> xLine(endAbsolute = 0)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)], tag = $seg006)
  |> close()

pClampBody = extrude(
       profile007,
       length = width,
       tagEnd = $capEnd002,
       tagStart = $capStart002,
     )
  |> chamfer(
       length = .125,
       tags = [
         getCommonEdge(faces = [seg005, capEnd002]),
         getCommonEdge(faces = [seg005, capStart002]),
         getCommonEdge(faces = [seg006, capStart002]),
         getCommonEdge(faces = [seg006, capEnd002])
       ],
     )

// Punch a hole through the top mounting surface
sketch004 = startSketchOn(pClampBody, face = seg004)
profile008 = circle(sketch004, center = [width / 2, width / 2], radius = holeDiameter / 2)
topHole = extrude(profile008, length = -.125)

// Punch a hole through the bottom mounting surface
sketch005 = startSketchOn(pClampBody, face = seg003)
profile009 = circle(sketch005, center = [-width / 2, width / 2], radius = holeDiameter / 2)
bottomHole = extrude(profile009, length = -.125)
  |> appearance(%, color = "#4191c3")
  |> rotate(yaw = 90)

// Move the p clamp so that the mounting hole on the bracket and the p clamp align.
translate(
  bottomHole,
  x = bracketLength / 2 + width / 2,
  y = bracketWidth / 2,
  z = bracketThickness,
  global = true,
)