modeling-app/docs/kcl/sweep.md

title, excerpt, layout

title	excerpt	layout
sweep	Extrude a sketch along a path.	manual

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(angle = 90, radius = 5)
  |> line(end = [-3, 0])
  |> tangentialArc(angle = -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)

// 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)

// Sweep two sketches along the same path.


sketch001 = startSketchOn(XY)
rectangleSketch = startProfileAt([-200, 23.86], sketch001)
  |> angledLine(angle = 0, length = 73.47, tag = $rectangleSegmentA001)
  |> angledLine(angle = segAng(rectangleSegmentA001) - 90, length = 50.61)
  |> angledLine(angle = segAng(rectangleSegmentA001), length = -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, angle = -90)
  |> xLine(length = 384.93)

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

// 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, angle = -90)
  |> xLine(length = 384.93)

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