startSketchOnFunction in std::sketch

Start a new 2-dimensional sketch on a specific plane or face.

startSketchOn(
  @planeOrSolid: Solid | Plane,
  face?: TaggedFace,
  normalToFace?: TaggedFace,
  alignAxis?: Axis2d,
  normalOffset?: number(Length),
): Plane | Face

Sketch on Face Behavior

There are some important behaviors to understand when sketching on a face:

The resulting sketch will include the face and thus Solid that was sketched on. So say you were to export the resulting Sketch / Solid from a sketch on a face, you would get both the artifact of the sketch on the face and the parent face / Solid itself.

This is important to understand because if you were to then sketch on the resulting Solid, it would again include the face and parent Solid that was sketched on. This could go on indefinitely.

The point is if you want to export the result of a sketch on a face, you only need to export the final Solid that was created from the sketch on the face, since it will include all the parent faces and Solids.

See sketch on face for more details.

Arguments

Name	Type	Description	Required
`planeOrSolid`	`Solid` or `Plane`	Profile whose start is being used.	Yes
`face`	`TaggedFace`	Identify a face of a solid if a solid is specified as the input argument (`planeOrSolid`). Incompatible with `normalToFace`.	No
`normalToFace`	`TaggedFace`	Identify a face of a solid if a solid is specified as the input argument. Starts a sketch on the plane orthogonal to this specified face. Incompatible with `face`, requires `alignAxis`.	No
`alignAxis`	`Axis2d`	If sketching normal to face, this axis will be the new local x axis of the sketch plane. The selected face's normal will be the local y axis. Incompatible with `face`, requires `normalToFace`.	No
`normalOffset`	`number(Length)`	Offset the sketch plane along its normal by the given amount. Incompatible with `face`, requires `normalToFace`.	No

Returns

Plane or Face

Examples

exampleSketch = startSketchOn(XY)
  |> startProfile(at = [0, 0])
  |> line(end = [10, 0])
  |> line(end = [0, 10])
  |> line(end = [-10, 0])
  |> close()

example = extrude(exampleSketch, length = 5)

exampleSketch002 = startSketchOn(example, face = END)
  |> startProfile(at = [1, 1])
  |> line(end = [8, 0])
  |> line(end = [0, 8])
  |> line(end = [-8, 0])
  |> close()

example002 = extrude(exampleSketch002, length = 5)

exampleSketch003 = startSketchOn(example002, face = END)
  |> startProfile(at = [2, 2])
  |> line(end = [6, 0])
  |> line(end = [0, 6])
  |> line(end = [-6, 0])
  |> close()

example003 = extrude(exampleSketch003, length = 5)

// Sketch on the end of an extruded face by tagging the end face.


exampleSketch = startSketchOn(XY)
  |> startProfile(at = [0, 0])
  |> line(end = [10, 0])
  |> line(end = [0, 10])
  |> line(end = [-10, 0])
  |> close()

example = extrude(exampleSketch, length = 5, tagEnd = $end01)

exampleSketch002 = startSketchOn(example, face = end01)
  |> startProfile(at = [1, 1])
  |> line(end = [8, 0])
  |> line(end = [0, 8])
  |> line(end = [-8, 0])
  |> close()

example002 = extrude(exampleSketch002, length = 5, tagEnd = $end02)

exampleSketch003 = startSketchOn(example002, face = end02)
  |> startProfile(at = [2, 2])
  |> line(end = [6, 0])
  |> line(end = [0, 6])
  |> line(end = [-6, 0])
  |> close()

example003 = extrude(exampleSketch003, length = 5)

exampleSketch = startSketchOn(XY)
  |> startProfile(at = [0, 0])
  |> line(end = [10, 0])
  |> line(end = [0, 10], tag = $sketchingFace)
  |> line(end = [-10, 0])
  |> close()

example = extrude(exampleSketch, length = 10)

exampleSketch002 = startSketchOn(example, face = sketchingFace)
  |> startProfile(at = [1, 1])
  |> line(end = [8, 0])
  |> line(end = [0, 8])
  |> line(end = [-8, 0])
  |> close(tag = $sketchingFace002)

example002 = extrude(exampleSketch002, length = 10)

exampleSketch003 = startSketchOn(example002, face = sketchingFace002)
  |> startProfile(at = [-8, 12])
  |> line(end = [0, 6])
  |> line(end = [6, 0])
  |> line(end = [0, -6])
  |> close()

example003 = extrude(exampleSketch003, length = 5)

exampleSketch = startSketchOn(XY)
  |> startProfile(at = [4, 12])
  |> line(end = [2, 0])
  |> line(end = [0, -6])
  |> line(end = [4, -6])
  |> line(end = [0, -6])
  |> line(end = [-3.75, -4.5])
  |> line(end = [0, -5.5])
  |> line(end = [-2, 0])
  |> close()

example = revolve(exampleSketch, axis = Y, angle = 180deg)

exampleSketch002 = startSketchOn(example, face = END)
  |> startProfile(at = [4.5, -5])
  |> line(end = [0, 5])
  |> line(end = [5, 0])
  |> line(end = [0, -5])
  |> close()

example002 = extrude(exampleSketch002, length = 5)

// Sketch on the end of a revolved face by tagging the end face.


exampleSketch = startSketchOn(XY)
  |> startProfile(at = [4, 12])
  |> line(end = [2, 0])
  |> line(end = [0, -6])
  |> line(end = [4, -6])
  |> line(end = [0, -6])
  |> line(end = [-3.75, -4.5])
  |> line(end = [0, -5.5])
  |> line(end = [-2, 0])
  |> close()

example = revolve(
  exampleSketch,
  axis = Y,
  angle = 180deg,
  tagEnd = $end01,
)

exampleSketch002 = startSketchOn(example, face = end01)
  |> startProfile(at = [4.5, -5])
  |> line(end = [0, 5])
  |> line(end = [5, 0])
  |> line(end = [0, -5])
  |> close()

example002 = extrude(exampleSketch002, length = 5)

a1 = startSketchOn({
       origin = { x = 0, y = 0, z = 0 },
       xAxis = { x = 1, y = 0, z = 0 },
       yAxis = { x = 0, y = 1, z = 0 },
       zAxis = { x = 0, y = 0, z = 1 }
     })
  |> startProfile(at = [0, 0])
  |> line(end = [100.0, 0])
  |> yLine(length = -100.0)
  |> xLine(length = -100.0)
  |> yLine(length = 100.0)
  |> close()
  |> extrude(length = 3.14)

sketch001 = startSketchOn(XY)
  |> startProfile(at = [-5, -5])
  |> xLine(length = 10)
  |> yLine(length = 10, tag = $b)
  |> xLine(length = -10)
  |> close()

cube001 = extrude(sketch001, length = 10)
  |> rotate(roll = 10, pitch = 20, yaw = 30)

sketch002 = startSketchOn(cube001, normalToFace = END, alignAxis = Y)
  |> circle(radius = 2, center = [0, 0])
cube002 = extrude(sketch002, length = 4)

subtract(cube001, tools = cube002)

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