kcl-samples → a-parametric-bearing-pillow-block →
a-parametric-bearing-pillow-block
KCL
// A Parametric Bearing Pillow Block
// A bearing pillow block, also known as a plummer block or pillow block bearing, is a pedestal used to provide support for a rotating shaft with the help of compatible bearings and various accessories. Housing a bearing, the pillow block provides a secure and stable foundation that allows the shaft to rotate smoothly within its machinery setup. These components are essential in a wide range of mechanical systems and machinery, playing a key role in reducing friction and supporting radial and axial loads.
// Define constants such as length, width, height, counter-bore depth and diameter, bearing diameter, hole location padding, and more
length = 6
width = 4
height = 1
cbDepth = .25
cbDia = .7
holeDia = .375
padding = 1.5
bearingDia = 3
// (Needs to be updated). Sketch the block and extrude up to where the counterbore diameter starts.
block = startSketchOn('XY')
|> startProfileAt([-width / 2, -length / 2], %)
|> lineTo([width / 2, -length / 2], %)
|> lineTo([width / 2, length / 2], %)
|> lineTo([-width / 2, length / 2], %)
|> close(%)
|> hole(circle({
center = [
-(width / 2 - (padding / 2)),
-(length / 2 - (padding / 2))
],
radius = holeDia / 2
}, %), %)
|> hole(circle({
center = [
-(width / 2 - (padding / 2)),
length / 2 - (padding / 2)
],
radius = holeDia / 2
}, %), %)
|> hole(circle({
center = [
width / 2 - (padding / 2),
length / 2 - (padding / 2)
],
radius = holeDia / 2
}, %), %)
|> hole(circle({
center = [
width / 2 - (padding / 2),
-(length / 2 - (padding / 2))
],
radius = holeDia / 2
}, %), %)
|> hole(circle({
center = [0, 0],
radius = bearingDia / 2
}, %), %)
|> extrude(height - cbDepth, %)
// Create a second sketch that creates the counterbore diameters and extrude the rest of the way to get the total height. Note: You cannot use startSketchOn(block, 'end'). The extrude lives outside the bounds, and the engine will not execute. This is a known issue.
secondHalf = startSketchOn({
plane = {
origin = { x = 0, y = 0, z = height - cbDepth },
xAxis = { x = 1, y = 0, z = 0 },
yAxis = { x = 0, y = 1, z = 0 },
zAxis = { x = 0, y = 0, z = 1 }
}
})
|> startProfileAt([-width / 2, -length / 2], %)
|> lineTo([width / 2, -length / 2], %)
|> lineTo([width / 2, length / 2], %)
|> lineTo([-width / 2, length / 2], %)
|> close(%)
|> hole(circle({
center = [
-(width / 2 - (padding / 2)),
-(length / 2 - (padding / 2))
],
radius = cbDia / 2
}, %), %)
|> hole(circle({
center = [
-(width / 2 - (padding / 2)),
length / 2 - (padding / 2)
],
radius = cbDia / 2
}, %), %)
|> hole(circle({
center = [
width / 2 - (padding / 2),
length / 2 - (padding / 2)
],
radius = cbDia / 2
}, %), %)
|> hole(circle({
center = [
width / 2 - (padding / 2),
-(length / 2 - (padding / 2))
],
radius = cbDia / 2
}, %), %)
|> hole(circle({
center = [0, 0],
radius = bearingDia / 2
}, %), %)
|> extrude(cbDepth, %)