kcl-std → functions → 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; 1+],
  length: number(Length),
  symmetric?: bool,
  bidirectionalLength?: number(Length),
  tagStart?: TagDecl,
  tagEnd?: TagDecl,
  twistAngle?: number(Angle),
  twistAngleStep?: number(Angle),
  twistCenter?: Point2d,
): [Solid; 1+]

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; 1+]`	Which sketch or sketches should be extruded.	Yes
`length`	`number(Length)`	How far to extrude the given sketches.	Yes
`symmetric`	`bool`	If true, the extrusion will happen symmetrically around the sketch. Otherwise, the extrusion will happen on only one side of the sketch.	No
`bidirectionalLength`	`number(Length)`	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`	`TagDecl`	A named tag for the face at the start of the extrusion, i.e. the original sketch.	No
`tagEnd`	`TagDecl`	A named tag for the face at the end of the extrusion, i.e. the new face created by extruding the original sketch.	No
`twistAngle`	`number(Angle)`	If given, the sketch will be twisted around this angle while being extruded.	No
`twistAngleStep`	`number(Angle)`	The size of each intermediate angle as the sketch twists around. Must be between 4 and 90 degrees. Only used if `twistAngle` is given, defaults to 15 degrees.	No
`twistCenter`	`Point2d`	The center around which the sketch will be twisted. Relative to the sketch's center. Only used if `twistAngle` is given, defaults to [0, 0] i.e. sketch's center.	No

Returns

[Solid; 1+]

Examples

example = startSketchOn(XZ)
  |> startProfile(at = [0, 0])
  |> line(end = [10, 0])
  |> arc(angleStart = 120deg, 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 = 120deg, angleEnd = -60deg, 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 = 120deg, angleEnd = -60deg, 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 = 120deg, angleEnd = -60deg, 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

example = startSketchOn(XZ)
  |> polygon(radius = 10, numSides = 3, center = [0, 0])
  |> extrude(length = 10, twistAngle = 120deg)

Rendered example of extrude 4

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