kcl →

loft

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

The sketches need to closed and on the same plane.

loft(sketches: [Sketch], v_degree: NonZeroU32, bez_approximate_rational: bool, base_curve_index?: integer, tolerance?: number) -> Solid

Arguments

Name	Type	Description	Required
`sketches`	`[Sketch]`	Which sketches to loft. Must include at least 2 sketches.	Yes
`v_degree`	`NonZeroU32`	Degree of the interpolation. Must be greater than zero. For example, use 2 for quadratic, or 3 for cubic interpolation in the V direction. This defaults to 2, if not specified.	Yes
`bez_approximate_rational`	`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.	Yes
`base_curve_index`	`integer`	This can be set to override the automatically determined topological base curve, which is usually the first section encountered.	No
`tolerance`	`number`	Tolerance for the loft operation.	No

Returns

Solid - An solid is a collection of extrude surfaces.

Examples

// Loft a square and a triangle.
squareSketch = startSketchOn('XY')
  |> startProfileAt([-100, 200], %)
  |> line([200, 0], %)
  |> line([0, -200], %)
  |> line([-200, 0], %)
  |> lineTo([profileStartX(%), profileStartY(%)], %)
  |> close(%)

triangleSketch = startSketchOn(offsetPlane('XY', 75))
  |> startProfileAt([0, 125], %)
  |> line([-15, -30], %)
  |> line([30, 0], %)
  |> lineTo([profileStartX(%), profileStartY(%)], %)
  |> close(%)

loft([squareSketch, triangleSketch])

Rendered example of loft 0

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

circleSketch0 = startSketchOn(offsetPlane('XY', 75))
  |> circle({ center = [0, 100], radius = 50 }, %)

circleSketch1 = startSketchOn(offsetPlane('XY', 150))
  |> circle({ center = [0, 100], radius = 20 }, %)

loft([
  squareSketch,
  circleSketch0,
  circleSketch1
])

Rendered example of loft 1

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

circleSketch0 = startSketchOn(offsetPlane('XY', 75))
  |> circle({ center = [0, 100], radius = 50 }, %)

circleSketch1 = startSketchOn(offsetPlane('XY', 150))
  |> circle({ center = [0, 100], radius = 20 }, %)

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

Rendered example of loft 2