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(
@solids: [Solid; 1+],
thickness: number(Length),
faces: [TaggedFace; 1+],
): [Solid]
Arguments
| Name | Type | Description | Required |
|---|---|---|---|
solids | [Solid; 1+] | Which solid (or solids) to shell out | Yes |
thickness | number(Length) | The thickness of the shell | Yes |
faces | [TaggedFace; 1+] | The faces you want removed | Yes |
Returns
Examples
// Remove the end face for the extrusion.
firstSketch = startSketchOn(XY)
|> startProfile(at = [-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)
|> startProfile(at = [-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)
|> startProfile(at = [-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)
|> startProfile(at = [-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)
|> startProfile(at = [-size, -size])
|> line(end = [2 * size, 0])
|> line(end = [0, 2 * size])
|> tangentialArc(endAbsolute = [-size, size])
|> close()
|> extrude(length = 65)
thing1 = startSketchOn(case, face = END)
|> circle(center = [-size / 2, -size / 2], radius = 25)
|> extrude(length = 50)
thing2 = startSketchOn(case, face = 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)
|> startProfile(at = [-size, -size])
|> line(end = [2 * size, 0])
|> line(end = [0, 2 * size])
|> tangentialArc(endAbsolute = [-size, size])
|> close()
|> extrude(length = 65)
thing1 = startSketchOn(case, face = END)
|> circle(center = [-size / 2, -size / 2], radius = 25)
|> extrude(length = 50)
thing2 = startSketchOn(case, face = 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)
|> startProfile(at = [-size, -size])
|> line(end = [2 * size, 0])
|> line(end = [0, 2 * size])
|> tangentialArc(endAbsolute = [-size, size])
|> close()
|> extrude(length = 65)
thing1 = startSketchOn(case, face = END)
|> circle(center = [-size / 2, -size / 2], radius = 25)
|> extrude(length = 50)
thing2 = startSketchOn(case, face = 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)
