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(end = [200, 0])
|> line(end = [0, -200])
|> line(end = [-200, 0])
|> line(endAbsolute = [profileStartX(%), profileStartY(%)])
|> close()
triangleSketch = startSketchOn(offsetPlane('XY', offset = 75))
|> startProfileAt([0, 125], %)
|> line(end = [-15, -30])
|> line(end = [30, 0])
|> line(endAbsolute = [profileStartX(%), profileStartY(%)])
|> close()
loft([squareSketch, triangleSketch])
// Loft a square, a circle, and another circle.
squareSketch = startSketchOn('XY')
|> startProfileAt([-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')
|> startProfileAt([-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,
)