Planes

A plane is a 2D surface that exists in 3D space. KCL has its own plane type, which is mostly used for starting a sketch. We've previously sketched on standard planes like XY (remember, there are six -- XY, YZ, XZ, -XY, -YZ and -XZ). But you can easily define your own planes too! We'll look at custom planes in this chapter.

Offset planes

You can use the offsetPlane function to copy any other plane, but moved some direction up or down the third axis. For example, let's draw a small circle on XY, a medium circle on a plane 10 units above it, and a big circle 20 units above it.

r = 10
sketch001 = sketch(on = XY) {
  circle1 = circle(start = [var -0.52mm, var 0.56mm], center = [var 0mm, var 0mm])
  coincident([circle1.center, ORIGIN])
  // Construction geometry line, used for the radius constraint.
  radiusLine = line(start = [var -0.52mm, var 0.56mm], end = [var 0mm, var 0mm], construction = true)
  coincident([radiusLine.start, circle1.start])
  coincident([radiusLine.end, circle1.center])
  // Constrain the circle's radius.
  distance([radiusLine.start, radiusLine.end]) == r
  vertical(radiusLine)
}

// Note the `offsetPlane` call!
sketch002 = sketch(on = offsetPlane(XY, offset = 10)) {
  circle1 = circle(start = [var -0.52mm, var 0.56mm], center = [var 0mm, var 0mm])
  coincident([circle1.center, ORIGIN])
  line1 = line(start = [var -0.52mm, var 0.56mm], end = [var 0mm, var 0mm], construction = true)
  coincident([line1.start, circle1.start])
  coincident([line1.end, circle1.center])
  distance([line1.start, line1.end]) == r * 2
  vertical(line1)
}

// Another `offsetPlane` call, offset even further!
sketch003 = sketch(on = offsetPlane(XY, offset = 20)) {
  circle1 = circle(start = [var -0.52mm, var 0.56mm], center = [var 0mm, var 0mm])
  coincident([circle1.center, ORIGIN])
  line1 = line(start = [var -0.52mm, var 0.56mm], end = [var 0mm, var 0mm], construction = true)
  coincident([line1.start, circle1.start])
  coincident([line1.end, circle1.center])
  distance([line1.start, line1.end]) == r * 3
  vertical(line1)
}

Offset planes are a quick and easy way to create new planes by using some other plane as a template. But what if you want to create a plane that actually points in a different direction, i.e. has different axes? What if you wanted to create a plane that was pointing at an unusual angle from the global X Y and Z axes? Let's try it.

Custom planes

You can define your own plane with your own axes like this:

customPlane = {
  origin = { x = 0, y = 1, z = 0},
  xAxis = { x = 1, y = 0, z = 0 },
  yAxis = { x = 0, y = 0, z = 1 },
}

Note the custom plane has a few properties:

  • An origin, which is a 3D point in space, using the global coordinate system (i.e. it's relative to the overall scene)
  • X and Y axes, which are defined as vectors

The plane's Z axis is the cross product of its X and Y axes. It's uniquely determined, so you don't need to specify it. The Z axis respects the right-hand rule.

Now let's use this custom plane in a sketch. We'll build two identical cylinders, but one is on the standard XY plane, and one is on the custom plane we defined above.

customPlane = {
  origin = { x = 0, y = 6, z = 0 },
  xAxis = { x = 1, y = 0.5, z = 0 },
  yAxis = { x = 0, y = 0.5, z = 1 }
}

// Build a cylinder on a custom plane
sketch001 = sketch(on = customPlane) {
  circle1 = circle(start = [var -0.52mm, var 0.56mm], center = [var 0mm, var 0mm])
  coincident([circle1.center, ORIGIN])
  line1 = line(start = [var -0.52mm, var 0.56mm], end = [var 0mm, var 0mm], construction = true)
  coincident([line1.start, circle1.start])
  coincident([line1.end, circle1.center])
  distance([line1.start, line1.end]) == 1
  vertical(line1)
}
region001 = region(point = [0mm, -0.9975mm], sketch = sketch001)
extrude001 = extrude(region001, length = 2)

// Build the same cylinder, but on the XY plane.
sketch002 = sketch(on = XY) {
  circle1 = circle(start = [var -0.52mm, var 0.56mm], center = [var 0mm, var 0mm])
  coincident([circle1.center, ORIGIN])
  line1 = line(start = [var -0.52mm, var 0.56mm], end = [var 0mm, var 0mm], construction = true)
  coincident([line1.start, circle1.start])
  coincident([line1.end, circle1.center])
  distance([line1.start, line1.end]) == 1
  vertical(line1)
}
region002 = region(point = [0mm, -0.9975mm], sketch = sketch002)
extrude002 = extrude(region002, length = 2)

Great! Custom planes give you a lot of power and flexibility. You can draw sketches in any orientation now. But they can be a bit verbose and complicated to define, so you should use offsetPlane if you've already defined a plane on the same X and Y axis. You can even combine offsetPlane and custom planes, like this:

// Make a custom plane.
customPlane = {
  origin = { x = 0, y = 1, z = 0},
  xAxis = { x = 1, y = 0, z = 0 },
  yAxis = { x = 0, y = 0, z = 1 },
}
// Now offset it 20 up its normal axis.
newPlane = offsetPlane(customPlane, offset = 20)

planeOf

There's one last method to create a plane: via the planeOf function. You can choose some 3D solid in your KCL file, and get the plane that its face lies on using planeOf(mySolid, face = myFace). For example:

// Make a square
sketch001 = sketch(on = XY) {
  line1 = line(start = [var -1.53mm, var -1.41mm], end = [var 1.99mm, var -1.41mm])
  line2 = line(start = [var 1.99mm, var -1.41mm], end = [var 1.99mm, var 1.42mm])
  line3 = line(start = [var 1.99mm, var 1.42mm], end = [var -1.53mm, var 1.42mm])
  line4 = line(start = [var -1.53mm, var 1.42mm], end = [var -1.53mm, var -1.41mm])
  coincident([line1.end, line2.start])
  coincident([line2.end, line3.start])
  coincident([line3.end, line4.start])
  coincident([line4.end, line1.start])
  parallel([line2, line4])
  parallel([line3, line1])
  perpendicular([line1, line2])
  horizontal(line3)
}
region001 = region(point = [0.23mm, -1.4075mm], sketch = sketch001)

// Make an arc to sweep the square along
sketch002 = sketch(on = YZ) {
  line1 = line(start = [var 0mm, var 0mm], end = [var 0mm, var 2.39mm])
  coincident([line1.start, ORIGIN])
  vertical([line1.end, ORIGIN])
  arc1 = arc(start = [var 0mm, var 2.39mm], end = [var -2.32mm, var 5.96mm], center = [var -3.91mm, var 2.39mm])
  coincident([line1.end, arc1.start])
  tangent([line1, arc1])
}

// Sweep the square along the arc
sweep001 = sweep(region001, path = [sketch002.line1, sketch002.arc1])

// Store the plane at the end of the sweep
p = planeOf(sweep001, face = END)

This plane can be used for sketching on, or altered with offsetPlane.

We've covered three different ways to create planes:

  • Offsetting from an existing plane
  • Manually defining a plane with axes and an origin
  • Using the plane of a face.

Combined with the six standard planes, you have a wide range of planes that you can use to sketch on, or build solids with. In the next chapter, we'll look at how to manipulate and change those solids.