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?: tag,
  tagEnd?: tag,
): 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)	Tolerance for the loft operation.	No
tagStart	tag	A named tag for the face at the start of the loft, i.e. the original sketch.	No
tagEnd	tag	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,
)