kcl →

translate

Move a solid or a sketch.

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

Translate is really useful for sketches if you want to move a sketch and then rotate it using the rotate function to create a loft.

translate(
  objects: SolidOrSketchOrImportedGeometry,
  x?: number,
  y?: number,
  z?: number,
  global?: bool,
): SolidOrSketchOrImportedGeometry

Arguments

Name	Type	Description	Required
`objects`	`SolidOrSketchOrImportedGeometry`	The solid, sketch, or set of solids or sketches to move.	Yes
`x`	`number`	The amount to move the solid or sketch along the x axis. Defaults to 0 if not provided.	No
`y`	`number`	The amount to move the solid or sketch along the y axis. Defaults to 0 if not provided.	No
`z`	`number`	The amount to move the solid or sketch along the z axis. Defaults to 0 if not provided.	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, sketch, or an imported geometry.

Examples

// Move a pipe.

// 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)
  |> translate(x = 1.0, y = 1.0, z = 2.5)

Rendered example of translate 0

// Move an imported model.


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

// Circle so you actually see the move.
startSketchOn(XY)
  |> circle(center = [-10, -10], radius = 10)
  |> extrude(length = 10)

cube
  |> translate(x = 10.0, y = 10.0, z = 2.5)

Rendered example of translate 1

// 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)

// Move the sweeps.
translate(
  parts,
  x = 1.0,
  y = 1.0,
  z = 2.5,
)

Rendered example of translate 2

// Move a sketch.


fn square(length) {
  l = length / 2
  p0 = [-l, -l]
  p1 = [-l, l]
  p2 = [l, l]
  p3 = [l, -l]

  return startSketchOn(XY)
    |> startProfileAt(p0, %)
    |> line(endAbsolute = p1)
    |> line(endAbsolute = p2)
    |> line(endAbsolute = p3)
    |> close()
}

square(10)
  |> translate(x = 5, y = 5)
  |> extrude(length = 10)

Rendered example of translate 3

// 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(z = 20)
  |> rotate(axis = [0, 0, 1.0], angle = 45)

loft([profile001, profile002])

Rendered example of translate 4