chamferFunction in std::solid

Cut a straight transitional edge along a tagged path.

chamfer(
  @solid: Solid,
  length: number(Length),
  tags: [Edge; 1+],
  secondLength?: number(Length),
  angle?: number(Angle),
  tag?: TagDecl,
): Solid

Chamfer is similar in function and use to a fillet, except a fillet will blend the transition along an edge, rather than cut a sharp, straight transitional edge.

Arguments

Name	Type	Description	Required
`solid`	`Solid`	The solid whose edges should be chamfered	Yes
`length`	`number(Length)`	Chamfering cuts away two faces to create a third face. This is the length to chamfer away from each face. The larger this length to chamfer away, the larger the new face will be.	Yes
`tags`	[`Edge`; 1+]	The paths you want to chamfer	Yes
`secondLength`	`number(Length)`	Chamfering cuts away two faces to create a third face. If this argument isn't given, the lengths chamfered away from both the first and second face are both given by `length`. If this argument is given, it determines how much is cut away from the second face. Incompatible with `angle`.	No
`angle`	`number(Angle)`	Chamfering cuts away two faces to create a third face. This argument determines the angle between the two cut edges. Requires `length`, incompatible with `secondLength`. The valid range is 0deg < angle < 90deg.	No
`tag`	`TagDecl`	Create a new tag which refers to this chamfer	No

Returns

Solid - A solid is a collection of extruded surfaces.

Examples

// Chamfer a mounting plate.
width = 20
length = 10
thickness = 1
chamferLength = 2

mountingPlateSketch = startSketchOn(XY)
  |> startProfile(at = [-width / 2, -length / 2])
  |> line(endAbsolute = [width / 2, -length / 2], tag = $edge1)
  |> line(endAbsolute = [width / 2, length / 2], tag = $edge2)
  |> line(endAbsolute = [-width / 2, length / 2], tag = $edge3)
  |> close(tag = $edge4)

mountingPlate = extrude(mountingPlateSketch, length = thickness)
  |> chamfer(
       length = chamferLength,
       tags = [
         getNextAdjacentEdge(edge1),
         getNextAdjacentEdge(edge2),
         getNextAdjacentEdge(edge3),
         getNextAdjacentEdge(edge4)
       ],
     )

// Sketch on the face of a chamfer.
fn cube(pos, scale) {
  sg = startSketchOn(XY)
    |> startProfile(at = pos)
    |> line(end = [0, scale])
    |> line(end = [scale, 0])
    |> line(end = [0, -scale])

  return sg
}

part001 = cube(pos = [0, 0], scale = 20)
  |> close(tag = $line1)
  |> extrude(length = 20)
  // We tag the chamfer to reference it later.
  |> chamfer(length = 10, tags = [getOppositeEdge(line1)], tag = $chamfer1)

sketch001 = startSketchOn(part001, face = chamfer1)
  |> startProfile(at = [10, 10])
  |> line(end = [2, 0])
  |> line(end = [0, 2])
  |> line(end = [-2, 0])
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()
  |> extrude(length = 10)

// Specify a custom chamfer angle.
fn cube(pos, scale) {
  sg = startSketchOn(XY)
    |> startProfile(at = pos)
    |> line(end = [0, scale])
    |> line(end = [scale, 0])
    |> line(end = [0, -scale])

  return sg
}

part001 = cube(pos = [0, 0], scale = 20)
  |> close(tag = $line1)
  |> extrude(length = 20)
  |> chamfer(length = 10, angle = 30deg, tags = [getOppositeEdge(line1)])

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