modeling-app/docs/kcl/rotate.md

title, excerpt, layout

title	excerpt	layout
rotate	Rotate a solid or a sketch.	manual

Rotate a solid or a sketch.

This is really useful for assembling parts together. You can create a part and then rotate it to the correct orientation.

For sketches, you can use this to rotate a sketch and then loft it with another sketch.

Using Roll, Pitch, and Yaw

When rotating a part in 3D space, "roll," "pitch," and "yaw" refer to the three rotational axes used to describe its orientation: roll is rotation around the longitudinal axis (front-to-back), pitch is rotation around the lateral axis (wing-to-wing), and yaw is rotation around the vertical axis (up-down); essentially, it's like tilting the part on its side (roll), tipping the nose up or down (pitch), and turning it left or right (yaw).

So, in the context of a 3D model:

• Roll: Imagine spinning a pencil on its tip - that's a roll movement.

• Pitch: Think of a seesaw motion, where the object tilts up or down along its side axis.

• Yaw: Like turning your head left or right, this is a rotation around the vertical axis

Using an Axis and Angle

When rotating a part around an axis, you specify the axis of rotation and the angle of rotation.

rotate(
  objects: SolidOrSketchOrImportedGeometry,
  roll?: number,
  pitch?: number,
  yaw?: number,
  axis?: [number],
  angle?: number,
  global?: bool,
): SolidOrSketchOrImportedGeometry

Arguments

Name	Type	Description	Required
objects	SolidOrSketchOrImportedGeometry	The solid, sketch, or set of solids or sketches to rotate.	Yes
roll	number	The roll angle in degrees. Must be between -360 and 360. Default is 0 if not given.	No
pitch	number	The pitch angle in degrees. Must be between -360 and 360. Default is 0 if not given.	No
yaw	number	The yaw angle in degrees. Must be between -360 and 360. Default is 0 if not given.	No
axis	[number]	The axis to rotate around. Must be used with angle.	No
angle	number	The angle to rotate in degrees. Must be used with axis. Must be between -360 and 360.	No
global	bool	If true, the transform is applied in global space. The origin of the model will move. By default, the transform is applied in local sketch axis, therefore the origin will not move.	No

Returns

SolidOrSketchOrImportedGeometry - Data for a solid or an imported geometry.

Examples

// Rotate a pipe with roll, pitch, and yaw.

// Create a path for the sweep.
sweepPath = startSketchOn(XZ)
  |> startProfileAt([0.05, 0.05], %)
  |> line(end = [0, 7])
  |> tangentialArc(angle = 90, radius = 5)
  |> line(end = [-3, 0])
  |> tangentialArc(angle = -90, radius = 5)
  |> line(end = [0, 7])

// Create a hole for the pipe.
pipeHole = startSketchOn(XY)
  |> circle(center = [0, 0], radius = 1.5)

sweepSketch = startSketchOn(XY)
  |> circle(center = [0, 0], radius = 2)
  |> hole(pipeHole, %)
  |> sweep(path = sweepPath)
  |> rotate(roll = 10, pitch = 10, yaw = 90)

// Rotate a pipe with just roll.

// Create a path for the sweep.
sweepPath = startSketchOn(XZ)
  |> startProfileAt([0.05, 0.05], %)
  |> line(end = [0, 7])
  |> tangentialArc(angle = 90, radius = 5)
  |> line(end = [-3, 0])
  |> tangentialArc(angle = -90, radius = 5)
  |> line(end = [0, 7])

// Create a hole for the pipe.
pipeHole = startSketchOn(XY)
  |> circle(center = [0, 0], radius = 1.5)

sweepSketch = startSketchOn(XY)
  |> circle(center = [0, 0], radius = 2)
  |> hole(pipeHole, %)
  |> sweep(path = sweepPath)
  |> rotate(roll = 10)

// Rotate a pipe about an axis with an angle.

// Create a path for the sweep.
sweepPath = startSketchOn(XZ)
  |> startProfileAt([0.05, 0.05], %)
  |> line(end = [0, 7])
  |> tangentialArc(angle = 90, radius = 5)
  |> line(end = [-3, 0])
  |> tangentialArc(angle = -90, radius = 5)
  |> line(end = [0, 7])

// Create a hole for the pipe.
pipeHole = startSketchOn(XY)
  |> circle(center = [0, 0], radius = 1.5)

sweepSketch = startSketchOn(XY)
  |> circle(center = [0, 0], radius = 2)
  |> hole(pipeHole, %)
  |> sweep(path = sweepPath)
  |> rotate(axis = [0, 0, 1.0], angle = 90)

// Rotate an imported model.


import "tests/inputs/cube.sldprt" as cube

cube
  |> rotate(axis = [0, 0, 1.0], angle = 9)

// Sweep two sketches along the same path.


sketch001 = startSketchOn(XY)
rectangleSketch = startProfileAt([-200, 23.86], sketch001)
  |> angledLine(angle = 0, length = 73.47, tag = $rectangleSegmentA001)
  |> angledLine(angle = segAng(rectangleSegmentA001) - 90, length = 50.61)
  |> angledLine(angle = segAng(rectangleSegmentA001), length = -segLen(rectangleSegmentA001))
  |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
  |> close()

circleSketch = circle(sketch001, center = [200, -30.29], radius = 32.63)

sketch002 = startSketchOn(YZ)
sweepPath = startProfileAt([0, 0], sketch002)
  |> yLine(length = 231.81)
  |> tangentialArc(radius = 80, angle = -90)
  |> xLine(length = 384.93)

parts = sweep([rectangleSketch, circleSketch], path = sweepPath)

// Rotate the sweeps.
rotate(parts, axis = [0, 0, 1.0], angle = 90)

// Translate and rotate a sketch to create a loft.
sketch001 = startSketchOn(XY)

fn square() {
  return startProfileAt([-10, 10], sketch001)
    |> xLine(length = 20)
    |> yLine(length = -20)
    |> xLine(length = -20)
    |> line(endAbsolute = [profileStartX(%), profileStartY(%)])
    |> close()
}

profile001 = square()

profile002 = square()
  |> translate(x = 0, y = 0, z = 20)
  |> rotate(axis = [0, 0, 1.0], angle = 45)

loft([profile001, profile002])