modeling-app/docs/kcl/shell.md

title, excerpt, layout

title	excerpt	layout
shell	Remove volume from a 3-dimensional shape such that a wall of the	manual

Remove volume from a 3-dimensional shape such that a wall of the

provided thickness remains, taking volume starting at the provided face, leaving it open in that direction.

shell(
  solidSet: SolidSet,
  thickness: number,
  faces: [FaceTag],
) -> SolidSet

Arguments

Name	Type	Description	Required
solidSet	SolidSet	Which solid (or solids) to shell out	Yes
thickness	number	The thickness of the shell	Yes
faces	[FaceTag]	The faces you want removed	Yes

Returns

SolidSet - A solid or a group of solids.

Examples

// Remove the end face for the extrusion.
firstSketch = startSketchOn('XY')
  |> startProfileAt([-12, 12], %)
  |> line(end = [24, 0])
  |> line(end = [0, -24])
  |> line(end = [-24, 0])
  |> close()
  |> extrude(length = 6)

// Remove the end face for the extrusion.
shell(firstSketch, faces = ['end'], thickness = 0.25)

// Remove the start face for the extrusion.
firstSketch = startSketchOn('-XZ')
  |> startProfileAt([-12, 12], %)
  |> line(end = [24, 0])
  |> line(end = [0, -24])
  |> line(end = [-24, 0])
  |> close()
  |> extrude(length = 6)

// Remove the start face for the extrusion.
shell(firstSketch, faces = ['start'], thickness = 0.25)

// Remove a tagged face and the end face for the extrusion.
firstSketch = startSketchOn('XY')
  |> startProfileAt([-12, 12], %)
  |> line(end = [24, 0])
  |> line(end = [0, -24])
  |> line(end = [-24, 0], tag = $myTag)
  |> close()
  |> extrude(length = 6)

// Remove a tagged face for the extrusion.
shell(firstSketch, faces = [myTag], thickness = 0.25)

// Remove multiple faces at once.
firstSketch = startSketchOn('XY')
  |> startProfileAt([-12, 12], %)
  |> line(end = [24, 0])
  |> line(end = [0, -24])
  |> line(end = [-24, 0], tag = $myTag)
  |> close()
  |> extrude(length = 6)

// Remove a tagged face and the end face for the extrusion.
shell(firstSketch, faces = [myTag, 'end'], thickness = 0.25)

// Shell a sketch on face.
size = 100
case = startSketchOn('-XZ')
  |> startProfileAt([-size, -size], %)
  |> line(end = [2 * size, 0])
  |> line(end = [0, 2 * size])
  |> tangentialArcTo([-size, size], %)
  |> close()
  |> extrude(length = 65)

thing1 = startSketchOn(case, 'end')
  |> circle(center = [-size / 2, -size / 2], radius = 25)
  |> extrude(length = 50)

thing2 = startSketchOn(case, 'end')
  |> circle(center = [size / 2, -size / 2], radius = 25)
  |> extrude(length = 50)

// We put "case" in the shell function to shell the entire object.
shell(case, faces = ['start'], thickness = 5)

// Shell a sketch on face object on the end face.
size = 100
case = startSketchOn('XY')
  |> startProfileAt([-size, -size], %)
  |> line(end = [2 * size, 0])
  |> line(end = [0, 2 * size])
  |> tangentialArcTo([-size, size], %)
  |> close()
  |> extrude(length = 65)

thing1 = startSketchOn(case, 'end')
  |> circle(center = [-size / 2, -size / 2], radius = 25)
  |> extrude(length = 50)

thing2 = startSketchOn(case, 'end')
  |> circle(center = [size / 2, -size / 2], radius = 25)
  |> extrude(length = 50)

// We put "thing1" in the shell function to shell the end face of the object.
shell(thing1, faces = ['end'], thickness = 5)

// Shell sketched on face objects on the end face, include all sketches to shell
// the entire object.


size = 100
case = startSketchOn('XY')
  |> startProfileAt([-size, -size], %)
  |> line(end = [2 * size, 0])
  |> line(end = [0, 2 * size])
  |> tangentialArcTo([-size, size], %)
  |> close()
  |> extrude(length = 65)

thing1 = startSketchOn(case, 'end')
  |> circle(center = [-size / 2, -size / 2], radius = 25)
  |> extrude(length = 50)

thing2 = startSketchOn(case, 'end')
  |> circle(center = [size / 2, -size / 2], radius = 25)
  |> extrude(length = 50)

// We put "thing1" and "thing2" in the shell function to shell the end face of the object.
shell([thing1, thing2], faces = ['end'], thickness = 5)