/// This module contains functions for modifying solids, e.g., by adding a fillet or chamfer, or
/// removing part of a solid.

@no_std
@settings(defaultLengthUnit = mm, kclVersion = 1.0)

import Face from "std::types"

/// Blend a transitional edge along a tagged path, smoothing the sharp edge.
///
/// Fillet is similar in function and use to a chamfer, except
/// a chamfer will cut a sharp transition along an edge while fillet
/// will smoothly blend the transition.
///
/// ```
/// width = 20
/// length = 10
/// thickness = 1
/// filletRadius = 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)
///   |> fillet(
///     radius = filletRadius,
///     tags = [
///       getNextAdjacentEdge(edge1),
///       getNextAdjacentEdge(edge2),
///       getNextAdjacentEdge(edge3),
///       getNextAdjacentEdge(edge4)
///     ],
///   )
/// ```
///
/// ```
/// width = 20
/// length = 10
/// thickness = 1
/// filletRadius = 1
///
/// 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)
///   |> fillet(
///     radius = filletRadius,
///     tolerance = 0.000001,
///     tags = [
///       getNextAdjacentEdge(edge1),
///       getNextAdjacentEdge(edge2),
///       getNextAdjacentEdge(edge3),
///       getNextAdjacentEdge(edge4)
///     ],
///   )
/// ```
@(impl = std_rust)
export fn fillet(
  /// The solid whose edges should be filletted
  @solid: Solid,
  /// The radius of the fillet
  radius: number(Length),
  /// The paths you want to fillet
  tags: [Edge; 1+],
  /// The tolerance for this fillet
  tolerance?: number(Length),
  /// Create a new tag which refers to this fillet
  tag?: tag,
): Solid {}

/// Cut a straight transitional edge along a tagged path.
///
/// 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.
///
/// ```
/// // 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)
/// ```
@(impl = std_rust)
export fn chamfer(
  /// The solid whose edges should be chamfered
  @solid: Solid,
  /// The length of the chamfer
  length: number(Length),
  /// The paths you want to chamfer
  tags: [Edge; 1+],
  /// Create a new tag which refers to this chamfer
  tag?: tag,
): Solid {}

/// Remove volume from a 3-dimensional shape such that a wall of the
/// provided thickness remains, taking volume starting at the provided
/// face, leaving it open in that direction.
///
/// ```
/// // Remove the end face for the extrusion.
/// firstSketch = startSketchOn(XY)
///     |> startProfile(at = [-12, 12])
///     |> line(end = [24, 0])
///     |> line(end = [0, -24])
///     |> line(end = [-24, 0])
///     |> close()
///     |> extrude(length = 6)
///
/// // Remove the end face for the extrusion.
/// shell(
///     firstSketch,
///     faces = [END],
///     thickness = 0.25,
/// )
/// ```
///
/// ```
/// // Remove the start face for the extrusion.
/// firstSketch = startSketchOn(-XZ)
///     |> startProfile(at = [-12, 12])
///     |> line(end = [24, 0])
///     |> line(end = [0, -24])
///     |> line(end = [-24, 0])
///     |> close()
///     |> extrude(length = 6)
///
/// // Remove the start face for the extrusion.
/// shell(
///     firstSketch,
///     faces = [START],
///     thickness = 0.25,
/// )
/// ```
///
/// ```
/// // Remove a tagged face and the end face for the extrusion.
/// firstSketch = startSketchOn(XY)
///     |> startProfile(at = [-12, 12])
///     |> line(end = [24, 0])
///     |> line(end = [0, -24])
///     |> line(end = [-24, 0], tag = $myTag)
///     |> close()
///     |> extrude(length = 6)
///
/// // Remove a tagged face for the extrusion.
/// shell(
///     firstSketch,
///     faces = [myTag],
///     thickness = 0.25,
/// )
/// ```
///
/// ```
/// // Remove multiple faces at once.
/// firstSketch = startSketchOn(XY)
///     |> startProfile(at = [-12, 12])
///     |> line(end = [24, 0])
///     |> line(end = [0, -24])
///     |> line(end = [-24, 0], tag = $myTag)
///     |> close()
///     |> extrude(length = 6)
///
/// // Remove a tagged face and the end face for the extrusion.
/// shell(
///     firstSketch,
///     faces = [myTag, END],
///     thickness = 0.25,
/// )
/// ```
///
/// ```
/// // Shell a sketch on face.
/// size = 100
/// case = startSketchOn(-XZ)
///     |> startProfile(at = [-size, -size])
///     |> line(end = [2 * size, 0])
///     |> line(end = [0, 2 * size])
///     |> tangentialArc(endAbsolute = [-size, size])
///     |> close()
///     |> extrude(length = 65)
///
/// thing1 = startSketchOn(case, face = END)
///     |> circle( center = [-size / 2, -size / 2], radius = 25 )
///     |> extrude(length = 50)
///
/// thing2 = startSketchOn(case, face = END)
///     |> circle( center = [size / 2, -size / 2], radius = 25 )
///     |> extrude(length = 50)
///
/// // We put "case" in the shell function to shell the entire object.
/// shell(case, faces = [START], thickness = 5)
/// ```
///
/// ```
/// // Shell a sketch on face object on the end face.
/// size = 100
/// case = startSketchOn(XY)
///     |> startProfile(at = [-size, -size])
///     |> line(end = [2 * size, 0])
///     |> line(end = [0, 2 * size])
///     |> tangentialArc(endAbsolute = [-size, size])
///     |> close()
///     |> extrude(length = 65)
///
/// thing1 = startSketchOn(case, face = END)
///     |> circle( center = [-size / 2, -size / 2], radius = 25 )
///     |> extrude(length = 50)
///
/// thing2 = startSketchOn(case, face = END)
///     |> circle( center = [size / 2, -size / 2], radius = 25 )
///     |> extrude(length = 50)
///
/// // We put "thing1" in the shell function to shell the end face of the object.
/// shell(thing1, faces = [END], thickness = 5)
/// ```
///
/// ```
/// // Shell sketched on face objects on the end face, include all sketches to shell
/// // the entire object.
///
/// size = 100
/// case = startSketchOn(XY)
///     |> startProfile(at = [-size, -size])
///     |> line(end = [2 * size, 0])
///     |> line(end = [0, 2 * size])
///     |> tangentialArc(endAbsolute = [-size, size])
///     |> close()
///     |> extrude(length = 65)
///
/// thing1 = startSketchOn(case, face = END)
///     |> circle( center = [-size / 2, -size / 2], radius = 25 )
///     |> extrude(length = 50)
///
/// thing2 = startSketchOn(case, face = END)
///     |> circle( center = [size / 2, -size / 2], radius = 25)
///     |> extrude(length = 50)
///
/// // We put "thing1" and "thing2" in the shell function to shell the end face of the object.
/// shell([thing1, thing2], faces = [END], thickness = 5)
/// ```
@(impl = std_rust)
export fn shell(
  /// Which solid (or solids) to shell out
  @solids: [Solid; 1+],
  /// The thickness of the shell
  thickness: number(Length),
  /// The faces you want removed
  faces: [tag; 1+],
): [Solid] {}


/// Make the inside of a 3D object hollow.
///
/// Remove volume from a 3-dimensional shape such that a wall of the
/// provided thickness remains around the exterior of the shape.
///
/// ```
/// // Hollow a basic sketch.
/// firstSketch = startSketchOn(XY)
///     |> startProfile(at = [-12, 12])
///     |> line(end = [24, 0])
///     |> line(end = [0, -24])
///     |> line(end = [-24, 0])
///     |> close()
///     |> extrude(length = 6)
///     |> hollow (thickness = 0.25)
/// ```
///
/// ```
/// // Hollow a basic sketch.
/// firstSketch = startSketchOn(-XZ)
///     |> startProfile(at = [-12, 12])
///     |> line(end = [24, 0])
///     |> line(end = [0, -24])
///     |> line(end = [-24, 0])
///     |> close()
///     |> extrude(length = 6)
///     |> hollow (thickness = 0.5)
/// ```
///
/// ```
/// // Hollow a sketch on face object.
/// size = 100
/// case = startSketchOn(-XZ)
///     |> startProfile(at = [-size, -size])
///     |> line(end = [2 * size, 0])
///     |> line(end = [0, 2 * size])
///     |> tangentialArc(endAbsolute = [-size, size])
///     |> close()
///     |> extrude(length = 65)
///
/// thing1 = startSketchOn(case, face = END)
///     |> circle( center = [-size / 2, -size / 2], radius = 25 )
///     |> extrude(length = 50)
///
/// thing2 = startSketchOn(case, face = END)
///     |> circle( center = [size / 2, -size / 2], radius = 25 )
///     |> extrude(length = 50)
///
/// hollow(case, thickness = 0.5)
/// ```
@(impl = std_rust)
export fn hollow(
  /// Which solid to hollow out
  @solid: Solid,
  /// The thickness of the remaining shell
  thickness: number(Length),
): Solid {}