kcl →
shell
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(solid_set: SolidSet, thickness: number, faces: [FaceTag]) -> SolidSet
Arguments
Name | Type | Description | Required |
---|---|---|---|
solid_set | 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)