kcl library reference → std → sketch → extrude

extrudeFunction in std::sketch

Extend a 2-dimensional sketch through a third dimension in order to create new 3-dimensional volume, or if extruded into an existing volume, cut into an existing solid.

extrude(
  @sketches: [Sketch],
  length: number,
  symmetric?: bool,
  bidirectionalLength?: number,
  tagStart?: TagDeclarator,
  tagEnd?: TagDeclarator,
): [Solid]

You can provide more than one sketch to extrude, and they will all be extruded in the same direction.

Arguments

Name	Type	Description	Required
`sketches`	`[Sketch]`	Which sketch or sketches should be extruded	Yes
`length`	`number`	How far to extrude the given sketches	Yes
`symmetric`	`bool`	If true, the extrusion will happen symmetrically around the sketch. Otherwise, the	No
`bidirectionalLength`	`number`	If specified, will also extrude in the opposite direction to 'distance' to the specified distance. If 'symmetric' is true, this value is ignored.	No
`tagStart`	`TagDeclarator`	A named tag for the face at the start of the extrusion, i.e. the original sketch	No
`tagEnd`	`TagDeclarator`	A named tag for the face at the end of the extrusion, i.e. the new face created by extruding the original sketch	No

Returns

[Solid]

Examples

example = startSketchOn(XZ)
  |> startProfile(at = [0, 0])
  |> line(end = [10, 0])
  |> arc(angleStart = 120, angleEnd = 0, radius = 5)
  |> line(end = [5, 0])
  |> line(end = [0, 10])
  |> bezierCurve(control1 = [-10, 0], control2 = [2, 10], end = [-5, 10])
  |> line(end = [-5, -2])
  |> close()
  |> extrude(length = 10)

Rendered example of extrude 0

exampleSketch = startSketchOn(XZ)
  |> startProfile(at = [-10, 0])
  |> arc(angleStart = 120, angleEnd = -60, radius = 5)
  |> line(end = [10, 0])
  |> line(end = [5, 0])
  |> bezierCurve(control1 = [-3, 0], control2 = [2, 10], end = [-5, 10])
  |> line(end = [-4, 10])
  |> line(end = [-5, -2])
  |> close()

example = extrude(exampleSketch, length = 10)

Rendered example of extrude 1

exampleSketch = startSketchOn(XZ)
  |> startProfile(at = [-10, 0])
  |> arc(angleStart = 120, angleEnd = -60, radius = 5)
  |> line(end = [10, 0])
  |> line(end = [5, 0])
  |> bezierCurve(control1 = [-3, 0], control2 = [2, 10], end = [-5, 10])
  |> line(end = [-4, 10])
  |> line(end = [-5, -2])
  |> close()

example = extrude(exampleSketch, length = 20, symmetric = true)

Rendered example of extrude 2

exampleSketch = startSketchOn(XZ)
  |> startProfile(at = [-10, 0])
  |> arc(angleStart = 120, angleEnd = -60, radius = 5)
  |> line(end = [10, 0])
  |> line(end = [5, 0])
  |> bezierCurve(control1 = [-3, 0], control2 = [2, 10], end = [-5, 10])
  |> line(end = [-4, 10])
  |> line(end = [-5, -2])
  |> close()

example = extrude(exampleSketch, length = 10, bidirectionalLength = 50)

Rendered example of extrude 3