modeling-app/docs/kcl/revolve.md

title, excerpt, layout

title	excerpt	layout
revolve	Rotate a sketch around some provided axis, creating a solid from its extent.	manual

Rotate a sketch around some provided axis, creating a solid from its extent.

This, like extrude, is able to create a 3-dimensional solid from a 2-dimensional sketch. However, unlike extrude, this creates a solid by using the extent of the sketch as its revolved around an axis rather than using the extent of the sketch linearly translated through a third dimension.

Revolve occurs around a local sketch axis rather than a global axis.

You can provide more than one sketch to revolve, and they will all be revolved around the same axis.

revolve(
  sketches: [Sketch],
  axis: Axis2dOrEdgeReference,
  angle?: number,
  tolerance?: number,
): [Solid]

Arguments

Name	Type	Description	Required
sketches	[Sketch]	The sketch or set of sketches that should be revolved	Yes
axis	Axis2dOrEdgeReference	Axis of revolution.	Yes
angle	number	Angle to revolve (in degrees). Default is 360.	No
tolerance	number	Tolerance for the revolve operation.	No

Returns

[Solid]

Examples

part001 = startSketchOn('XY')
  |> startProfileAt([4, 12], %)
  |> line(end = [2, 0])
  |> line(end = [0, -6])
  |> line(end = [4, -6])
  |> line(end = [0, -6])
  |> line(end = [-3.75, -4.5])
  |> line(end = [0, -5.5])
  |> line(end = [-2, 0])
  |> close()
  |> revolve(axis = 'y') // default angle is 360

// A donut shape.
sketch001 = startSketchOn('XY')
  |> circle(center = [15, 0], radius = 5)
  |> revolve(angle = 360, axis = 'y')

part001 = startSketchOn('XY')
  |> startProfileAt([4, 12], %)
  |> line(end = [2, 0])
  |> line(end = [0, -6])
  |> line(end = [4, -6])
  |> line(end = [0, -6])
  |> line(end = [-3.75, -4.5])
  |> line(end = [0, -5.5])
  |> line(end = [-2, 0])
  |> close()
  |> revolve(axis = 'y', angle = 180)

part001 = startSketchOn('XY')
  |> startProfileAt([4, 12], %)
  |> line(end = [2, 0])
  |> line(end = [0, -6])
  |> line(end = [4, -6])
  |> line(end = [0, -6])
  |> line(end = [-3.75, -4.5])
  |> line(end = [0, -5.5])
  |> line(end = [-2, 0])
  |> close()
  |> revolve(axis = 'y', angle = 180)

part002 = startSketchOn(part001, 'end')
  |> startProfileAt([4.5, -5], %)
  |> line(end = [0, 5])
  |> line(end = [5, 0])
  |> line(end = [0, -5])
  |> close()
  |> extrude(length = 5)

box = startSketchOn('XY')
  |> startProfileAt([0, 0], %)
  |> line(end = [0, 20])
  |> line(end = [20, 0])
  |> line(end = [0, -20])
  |> close()
  |> extrude(length = 20)

sketch001 = startSketchOn(box, "END")
  |> circle(center = [10, 10], radius = 4)
  |> revolve(angle = -90, axis = 'y')

box = startSketchOn('XY')
  |> startProfileAt([0, 0], %)
  |> line(end = [0, 20])
  |> line(end = [20, 0])
  |> line(end = [0, -20], tag = $revolveAxis)
  |> close()
  |> extrude(length = 20)

sketch001 = startSketchOn(box, "END")
  |> circle(center = [10, 10], radius = 4)
  |> revolve(angle = 90, axis = getOppositeEdge(revolveAxis))

box = startSketchOn('XY')
  |> startProfileAt([0, 0], %)
  |> line(end = [0, 20])
  |> line(end = [20, 0])
  |> line(end = [0, -20], tag = $revolveAxis)
  |> close()
  |> extrude(length = 20)

sketch001 = startSketchOn(box, "END")
  |> circle(center = [10, 10], radius = 4)
  |> revolve(angle = 90, axis = getOppositeEdge(revolveAxis), tolerance = 0.0001)

sketch001 = startSketchOn('XY')
  |> startProfileAt([10, 0], %)
  |> line(end = [5, -5])
  |> line(end = [5, 5])
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()

part001 = revolve(
  sketch001,
  axis = {
    custom = {
      axis = [0.0, 1.0],
      origin = [0.0, 0.0]
    }
  },
)

// Revolve two sketches around the same axis.


sketch001 = startSketchOn('XY')
profile001 = startProfileAt([4, 8], sketch001)
  |> xLine(length = 3)
  |> yLine(length = -3)
  |> xLine(length = -3)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()

profile002 = startProfileAt([-5, 8], sketch001)
  |> xLine(length = 3)
  |> yLine(length = -3)
  |> xLine(length = -3)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()

revolve([profile001, profile002], axis = "X")

// Revolve around a path that has not been extruded.


profile001 = startSketchOn('XY')
  |> startProfileAt([0, 0], %)
  |> line(end = [0, 20], tag = $revolveAxis)
  |> line(end = [20, 0])
  |> line(end = [0, -20])
  |> close(%)

sketch001 = startSketchOn('XY')
  |> circle(center = [-10, 10], radius = 4)
  |> revolve(angle = 90, axis = revolveAxis)

// Revolve around a path that has not been extruded or closed.


profile001 = startSketchOn('XY')
  |> startProfileAt([0, 0], %)
  |> line(end = [0, 20], tag = $revolveAxis)
  |> line(end = [20, 0])

sketch001 = startSketchOn('XY')
  |> circle(center = [-10, 10], radius = 4)
  |> revolve(angle = 90, axis = revolveAxis)