kcl →

sweep

Extrude a sketch along a path.

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 path. This is useful for creating more complex shapes that can't be created with a simple extrusion.

You can provide more than one sketch to sweep, and they will all be swept along the same path.

sweep(
  sketches: [Sketch],
  path: SweepPath,
  sectional?: bool,
  tolerance?: number,
  tagStart?: TagDeclarator,
  tagEnd?: TagDeclarator,
): [Solid]

Arguments

Name	Type	Description	Required
`sketches`	`[Sketch]`	The sketch or set of sketches that should be swept in space	Yes
`path`	`SweepPath`	The path to sweep the sketch along	Yes
`sectional`	`bool`	If true, the sweep will be broken up into sub-sweeps (extrusions, revolves, sweeps) based on the trajectory path components.	No
`tolerance`	`number`	Tolerance for this operation	No
`tagStart`	`TagDeclarator`	A named tag for the face at the start of the sweep, i.e. the original sketch	No
`tagEnd`	`TagDeclarator`	A named tag for the face at the end of the sweep	No

Returns

[Solid]

Examples

// Create a pipe using a sweep.

// Create a path for the sweep.
sweepPath = startSketchOn(XZ)
  |> startProfileAt([0.05, 0.05], %)
  |> line(end = [0, 7])
  |> tangentialArc({ offset = 90, radius = 5 }, %)
  |> line(end = [-3, 0])
  |> tangentialArc({ offset = -90, radius = 5 }, %)
  |> line(end = [0, 7])

// Create a hole for the pipe.
pipeHole = startSketchOn(XY)
  |> circle(center = [0, 0], radius = 1.5)

sweepSketch = startSketchOn(XY)
  |> circle(center = [0, 0], radius = 2)
  |> hole(pipeHole, %)
  |> sweep(path = sweepPath)

Rendered example of sweep 0

// Create a spring by sweeping around a helix path.

// Create a helix around the Z axis.
helixPath = helix(
  angleStart = 0,
  ccw = true,
  revolutions = 4,
  length = 10,
  radius = 5,
  axis = 'Z',
)

// Create a spring by sweeping around the helix path.
springSketch = startSketchOn(YZ)
  |> circle(center = [0, 0], radius = 1)
  |> sweep(path = helixPath)

Rendered example of sweep 1

// Sweep two sketches along the same path.


sketch001 = startSketchOn(XY)
rectangleSketch = startProfileAt([-200, 23.86], sketch001)
  |> angledLine([0, 73.47], %, $rectangleSegmentA001)
  |> angledLine([
       segAng(rectangleSegmentA001) - 90,
       50.61
     ], %)
  |> angledLine([
       segAng(rectangleSegmentA001),
       -segLen(rectangleSegmentA001)
     ], %)
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()

circleSketch = circle(sketch001, center = [200, -30.29], radius = 32.63)

sketch002 = startSketchOn(YZ)
sweepPath = startProfileAt([0, 0], sketch002)
  |> yLine(length = 231.81)
  |> tangentialArc({ radius = 80, offset = -90 }, %)
  |> xLine(length = 384.93)

sweep([rectangleSketch, circleSketch], path = sweepPath)

Rendered example of sweep 2

// Sectionally sweep one sketch along the path


sketch001 = startSketchOn(XY)
circleSketch = circle(sketch001, center = [200, -30.29], radius = 32.63)

sketch002 = startSketchOn(YZ)
sweepPath = startProfileAt([0, 0], sketch002)
  |> yLine(length = 231.81)
  |> tangentialArc({ radius = 80, offset = -90 }, %)
  |> xLine(length = 384.93)

sweep(circleSketch, path = sweepPath, sectional = true)

Rendered example of sweep 3