modeling-app/docs/kcl-std/functions/std-sketch-loft.md

title, subtitle, excerpt, layout

title	subtitle	excerpt	layout
loft	Function in std::sketch	Create a 3D surface or solid by interpolating between two or more sketches.	manual

Create a 3D surface or solid by interpolating between two or more sketches.

loft(
  @sketches: [Sketch; 2+],
  vDegree?: number(_),
  bezApproximateRational?: bool,
  baseCurveIndex?: number(_),
  tolerance?: number(Length),
  tagStart?: TagDecl,
  tagEnd?: TagDecl,
): Solid

The sketches need to be closed and on different planes that are parallel.

Arguments

Name	Type	Description	Required
sketches	[Sketch; 2+]	Which sketches to loft. Must include at least 2 sketches.	Yes
vDegree	number(_)	Degree of the interpolation. Must be greater than zero. For example, use 2 for quadratic, or 3 for cubic interpolation in the V direction.	No
bezApproximateRational	bool	Attempt to approximate rational curves (such as arcs) using a bezier. This will remove banding around interpolations between arcs and non-arcs. It may produce errors in other scenarios. Over time, this field won't be necessary.	No
baseCurveIndex	number(_)	This can be set to override the automatically determined topological base curve, which is usually the first section encountered.	No
tolerance	number(Length)	Defines the smallest distance below which two entities are considered coincident, intersecting, coplanar, or similar. For most use cases, it should not be changed from its default value of 10^-7 millimeters.	No
tagStart	TagDecl	A named tag for the face at the start of the loft, i.e. the original sketch.	No
tagEnd	TagDecl	A named tag for the face at the end of the loft.	No

Returns

Solid - A solid is a collection of extruded surfaces.

Examples

// Loft a square and a triangle.
squareSketch = startSketchOn(XY)
  |> startProfile(at = [-100, 200])
  |> line(end = [200, 0])
  |> line(end = [0, -200])
  |> line(end = [-200, 0])
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()

triangleSketch = startSketchOn(offsetPlane(XY, offset = 75))
  |> startProfile(at = [0, 125])
  |> line(end = [-15, -30])
  |> line(end = [30, 0])
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()

loft([triangleSketch, squareSketch])

// Loft a square, a circle, and another circle.
squareSketch = startSketchOn(XY)
  |> startProfile(at = [-100, 200])
  |> line(end = [200, 0])
  |> line(end = [0, -200])
  |> line(end = [-200, 0])
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()

circleSketch0 = startSketchOn(offsetPlane(XY, offset = 75))
  |> circle(center = [0, 100], radius = 50)

circleSketch1 = startSketchOn(offsetPlane(XY, offset = 150))
  |> circle(center = [0, 100], radius = 20)

loft([
  squareSketch,
  circleSketch0,
  circleSketch1
])

// Loft a square, a circle, and another circle with options.
squareSketch = startSketchOn(XY)
  |> startProfile(at = [-100, 200])
  |> line(end = [200, 0])
  |> line(end = [0, -200])
  |> line(end = [-200, 0])
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()

circleSketch0 = startSketchOn(offsetPlane(XY, offset = 75))
  |> circle(center = [0, 100], radius = 50)

circleSketch1 = startSketchOn(offsetPlane(XY, offset = 150))
  |> circle(center = [0, 100], radius = 20)

loft(
  [
    squareSketch,
    circleSketch0,
    circleSketch1
  ],
  baseCurveIndex = 0,
  bezApproximateRational = false,
  tolerance = 0.000001,
  vDegree = 2,
)