// Pipe
// Piping for the pipe flange assembly

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import pipeInnerDiameter, pipeOuterDiameter, pipeLength from "parameters.kcl"

// Create a function to make the pipe. Export
export fn pipe() {
  // Create the pipe base
  pipeBase = startSketchOn(XZ)
    |> circle(center = [0, 0], radius = pipeOuterDiameter / 2)
    |> extrude(length = pipeLength)

  // Extrude a hole through the length of the pipe
  pipe = startSketchOn(pipeBase, face = END)
    |> circle(center = [0, 0], radius = pipeInnerDiameter / 2)
    |> extrude(length = -pipeLength)
    |> appearance(color = "#a24ed0")
  return pipe
}


1120t74-pipe

// Flange
// Flange used for mating two pipes together in the pipe flange assembly.

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import pipeDiameter, mountingHoleDiameter, mountingHolePlacementDiameter, flangeDiameter, flangeTotalThickness, flangeBackHeight, flangeFrontHeight, flangeBaseThickness, flangeBackDiameter, flangeFrontDiameter from "parameters.kcl"

// Create a function to create the flange. We must create a function since we are using multiple flanges.
export fn flange() {
  // Sketch the mounting hole pattern
  mountingHoles = startSketchOn(XY)
    |> circle(center = [0, mountingHolePlacementDiameter / 2], radius = mountingHoleDiameter / 2)
    |> patternCircular2d(
         instances = 4,
         center = [0, 0],
         arcDegrees = 360,
         rotateDuplicates = false,
       )

  // Create the flange base
  flangeBase = startSketchOn(XY)
    |> circle(center = [0, 0], radius = flangeDiameter / 2)
    |> subtract2d(tool = mountingHoles)
    |> extrude(length = flangeBaseThickness)

  // Create both the raised portions on the front and back of the flange base
  flangeBack = startSketchOn(flangeBase, face = START)
    |> circle(center = [0, 0], radius = flangeBackDiameter / 2)
    |> extrude(length = flangeBackHeight)
  flangeFront = startSketchOn(flangeBase, face = END)
    |> circle(center = [0, 0], radius = flangeFrontDiameter / 2)
    |> extrude(length = flangeFrontHeight)

  // Create the circular cut in the center for the pipe
  pipeCut = startSketchOn(flangeFront, face = END)
    |> circle(center = [0, 0], radius = pipeDiameter / 2)
    |> extrude(length = -flangeTotalThickness)
    |> appearance(color = "#bab0b0")

  return pipeCut
}


68095k348-flange

// Socket Head Cap Screw
// screw for mating the flanges together in the pipe flange assembly

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import boltDiameter, boltLength, boltHeadLength, boltHeadDiameter, boltHexDrive, boltHexFlatLength, boltThreadLength from "parameters.kcl"

// Create a function to make a the bolt
export fn bolt() {
  // Create the head of the cap screw
  boltHead = startSketchOn(XZ)
    |> circle(center = [0, 0], radius = boltHeadDiameter / 2, tag = $topEdge)
    |> extrude(length = -boltHeadLength)
    |> fillet(radius = 0.020, tags = [topEdge, getOppositeEdge(topEdge)])

  // Define the sketch of the hex pattern on the screw head and extrude into the head
  hexPatternSketch = startSketchOn(boltHead, face = START)
    |> startProfile(at = [
         boltHexDrive / 2,
         boltHexFlatLength / 2
       ])
    |> angledLine(angle = 270, length = boltHexFlatLength)
    |> angledLine(angle = 210, length = boltHexFlatLength)
    |> angledLine(angle = 150, length = boltHexFlatLength)
    |> angledLine(angle = 90, length = boltHexFlatLength)
    |> angledLine(angle = 30, length = boltHexFlatLength)
    |> close()
    |> extrude(length = -boltHeadLength * 0.75)

  // create the body of the bolt
  boltBody = startSketchOn(boltHead, face = END)
    |> circle(center = [0, 0], radius = boltDiameter / 2, tag = $filletEdge)
    |> extrude(length = boltLength)
    |> appearance(color = "#4dd043", metalness = 90, roughness = 90)

  return boltBody
}


91251a404-bolt

// Gasket
// Gasket for the pipe flange assembly. A gasket is a mechanical seal that fills the space between two or more mating surfaces, preventing leaks of liquids or gases under compression

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import gasketOutsideDiameter, gasketInnerDiameter, gasketThickness from "parameters.kcl"

// Create the base of the gasket
gasketBase = startSketchOn(XY)
  |> circle(center = [0, 0], radius = gasketOutsideDiameter / 2)
  |> extrude(length = gasketThickness)

// Extrude a circular hole through the gasket base
startSketchOn(gasketBase, face = END)
  |> circle(center = [0, 0], radius = gasketInnerDiameter / 2)
  |> extrude(length = -gasketThickness)
  |> appearance(color = "#d0cb3e")


9472k188-gasket

// Hex Nut
// Hex nut for the screws in the pipe flange assembly.

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import hexNutDiameter, hexNutFlatToFlat, hexNutThickness, hexNutFlatLength from "parameters.kcl"

// Create a function to make the hex nut. Must be a function since multiple hex nuts are used
export fn hexNut() {
  // Create the base of the hex nut
  hexNutBase = startSketchOn(XY)
    |> startProfile(at = [
         hexNutFlatToFlat / 2,
         hexNutFlatLength / 2
       ])
    |> angledLine(angle = 270, length = hexNutFlatLength)
    |> angledLine(angle = 210, length = hexNutFlatLength)
    |> angledLine(angle = 150, length = hexNutFlatLength)
    |> angledLine(angle = 90, length = hexNutFlatLength)
    |> angledLine(angle = 30, length = hexNutFlatLength)
    |> close()
    |> extrude(length = hexNutThickness)

  // Create the hole in the center of the hex nut
  hexNut = startSketchOn(hexNutBase, face = END)
    |> circle(center = [0, 0], radius = hexNutDiameter / 2)
    |> extrude(length = -hexNutThickness)
    |> appearance(color = "#4edfd5")

  return hexNut
}


95479a127-hex-nut

// 98017A257 Washer
// Washer for the screws in the pipe flange assembly.

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Import parameters
import washerInnerDia, washerOuterDia, washerThickness from "parameters.kcl"

// Create a function to make the washer. Must be a function since multiple washers are used.
export fn washer() {
  // Create the base of the washer
  washerBase = startSketchOn(XY)
    |> circle(center = [0, 0], radius = washerOuterDia / 2)
    |> extrude(length = washerThickness)

  // Extrude a hole through the washer
  washer = startSketchOn(washerBase, face = END)
    |> circle(center = [0, 0], radius = washerInnerDia / 2)
    |> extrude(length = -washerThickness)
    |> appearance(color = "#ee4f4f")

  return washer
}


98017a257-washer

// Parameters

// Set units
@settings(defaultLengthUnit = in, kclVersion = 1.0)

// Flange (68095K348)
export pipeDiameter = 2.440
export mountingHoleDiameter = 0.750
export mountingHolePlacementDiameter = 4.750

export flangeDiameter = 6.0
export flangeTotalThickness = 1.0
export flangeBackHeight = 0.060
export flangeFrontHeight = 0.250
export flangeBaseThickness = flangeTotalThickness - flangeBackHeight - flangeFrontHeight

export flangeBackDiameter = 3.620
export flangeFrontDiameter = 3.060

// Washer (98017A257)
export washerInnerDia = 0.640
export washerOuterDia = 1.188
export washerThickness = 0.032

// Bolt (91251A404)
export boltDiameter = 0.625
export boltLength = 2.500
export boltHeadLength = boltDiameter
export boltHeadDiameter = 0.938
export boltHexDrive = 1 / 2
export boltHexFlatLength = boltHexDrive / (2 * cos(30deg))
export boltThreadLength = 1.750

// Hex nut (95479A127)
export hexNutDiameter = 5 / 8
export hexNutFlatToFlat = 15 / 16
export hexNutThickness = 35 / 64
export hexNutFlatLength = hexNutFlatToFlat / (2 * cos(30deg))

// Gasket (9472K188)
export gasketOutsideDiameter = 4.125
export gasketInnerDiameter = 2.375
export gasketThickness = 0.031

// Pipe (1120T74)
export pipeInnerDiameter = 2.0
export pipeOuterDiameter = 2.375
export pipeLength = 6


parameters

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Zoo Developer Tools

pipe-flange-assembly

pipe-flange-assembly

KCL

Parts