modeling-app/docs/kcl/translate.md

title, excerpt, layout

title	excerpt	layout
translate	Move a solid or a sketch.	manual

Move a solid or a sketch.

translate(
  objects: SolidOrSketchOrImportedGeometry,
  translate: [number],
  global?: bool,
): SolidOrSketchOrImportedGeometry

Arguments

Name	Type	Description	Required
objects	SolidOrSketchOrImportedGeometry	The solid, sketch, or set of solids or sketches to move.	Yes
translate	[number]	The amount to move the solid or sketch in all three axes.	Yes
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

// Move a pipe.

// Create a path for the sweep.
sweepPath = startSketchOn(XZ)
  |> startProfileAt([0.05, 0.05], %)
  |> line(end = [0, 7])
  |> tangentialArc({ offset = 90, radius = 5 }, %)
  |> line(end = [-3, 0])
  |> tangentialArc({ offset = -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(translate = [1.0, 1.0, 2.5])

// Move an imported model.


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

cube
  |> translate(translate = [1.0, 1.0, 2.5])

// Sweep two sketches along the same path.


sketch001 = startSketchOn(XY)
rectangleSketch = startProfileAt([-200, 23.86], sketch001)
  |> angledLine([0, 73.47], %, $rectangleSegmentA001)
  |> angledLine([
       segAng(rectangleSegmentA001) - 90,
       50.61
     ], %)
  |> angledLine([
       segAng(rectangleSegmentA001),
       -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, offset = -90 }, %)
  |> xLine(length = 384.93)

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

// Move the sweeps.
translate(parts, translate = [1.0, 1.0, 2.5])

// 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(translate = [5, 5, 0])
  |> extrude(length = 10)

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

loft([profile001, profile002])