involuteCircularFunction in std::sketch

Extend the current sketch with a new involute circular curve.

involuteCircular(
  @sketch: Sketch,
  angle: number(Angle),
  startRadius?: number(Length),
  endRadius?: number(Length),
  startDiameter?: number(Length),
  endDiameter?: number(Length),
  reverse?: bool,
  tag?: TagDecl,
): Sketch

Arguments

Name	Type	Description	Required
`sketch`	`Sketch`	Which sketch should this path be added to?	Yes
`angle`	`number(Angle)`	The angle to rotate the involute by. A value of zero will produce a curve with a tangent along the x-axis at the start point of the curve.	Yes
`startRadius`	`number(Length)`	The involute is described between two circles, startRadius is the radius of the inner circle. Either `startRadius` or `startDiameter` must be given (but not both).	No
`endRadius`	`number(Length)`	The involute is described between two circles, endRadius is the radius of the outer circle. Either `endRadius` or `endDiameter` must be given (but not both).	No
`startDiameter`	`number(Length)`	The involute is described between two circles, startDiameter describes the inner circle. Either `startRadius` or `startDiameter` must be given (but not both).	No
`endDiameter`	`number(Length)`	The involute is described between two circles, endDiameter describes the outer circle. Either `endRadius` or `endDiameter` must be given (but not both).	No
`reverse`	`bool`	If reverse is true, the segment will start from the end of the involute, otherwise it will start from that start.	No
`tag`	`TagDecl`	Create a new tag which refers to this line.	No

Returns

Sketch - A sketch is a collection of paths.

Examples

a = 10
b = 14
startSketchOn(XZ)
  |> startProfile(at = [0, 0])
  |> involuteCircular(startRadius = a, endRadius = b, angle = 60deg)
  |> involuteCircular(
       startRadius = a,
       endRadius = b,
       angle = 60deg,
       reverse = true,
     )

// Example: a gear that uses an involute circular profile for the teeth.
@settings(defaultLengthUnit = mm)

/// // Define gear parameters
nTeeth = 21
module = 1.5
pressureAngle = 14deg
gearHeight = 6
pitchDiameter = module * nTeeth
addendum = module
deddendum = 1.25 * module
baseDiameter = pitchDiameter * cos(pressureAngle)
tipDiameter = pitchDiameter + 2 * module

// Using the gear parameters, sketch an involute tooth spanning from the base diameter to the tip diameter
gearSketch = startSketchOn(XY)
  |> startProfile(at = polar(angle = 0, length = baseDiameter / 2))
  |> involuteCircular(
       startDiameter = baseDiameter,
       endDiameter = tipDiameter,
       angle = 0,
       tag = $seg01,
     )
  |> line(endAbsolute = polar(angle = 160deg / nTeeth, length = tipDiameter / 2))
  |> involuteCircular(
       startDiameter = baseDiameter,
       endDiameter = tipDiameter,
       angle = -atan(segEndY(seg01) / segEndX(seg01)) - (180deg / nTeeth),
       reverse = true,
     )
  // Position the end line of the sketch at the start of the next tooth
  |> line(endAbsolute = polar(angle = 360deg / nTeeth, length = baseDiameter / 2))
  // Pattern the sketch about the center by the specified number of teeth, then close the sketch
  |> patternCircular2d(
       instances = nTeeth,
       center = [0, 0],
       arcDegrees = 360deg,
       rotateDuplicates = true,
     )
  |> close()
  // Extrude the gear to the specified height
  |> extrude(length = gearHeight)

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