CAD for making

Turning sketches into solids

Extrude, revolve, sweep, loft — and the boolean question every feature quietly asks you.

Four ways to give a sketch a third dimension

You will build ninety percent of everything you print with the first one. The other three matter because knowing they exist stops you from faking them badly.

  • Extrude — push a flat profile along a straight line. Plates, walls, bosses, ribs, holes, slots. This is the default verb of CAD.
  • Revolve — spin a profile around an axis. Anything round: knobs, spacers, bottle adapters, vase forms. Sketch the silhouette of one half and let the axis do the rest.
  • Sweep — drag a profile along a path you drew. Cable channels, handles, tubing, a gasket groove that follows a curved edge.
  • Loft — blend between two or more different profiles on different planes. Transitions: a round duct that becomes a rectangle, an ergonomic grip.

The question every feature asks and beginners ignore

Each of those features has a small set of buttons deciding what happens to the result. This is the boolean operation, and getting it wrong is the most common reason a new user ends up with two overlapping solids that will not slice properly.

  • New — make a separate part. Correct when you are modelling the lid and the box in one Part Studio.
  • Add — fuse into the existing part. Bosses, ribs, mounting ears.
  • Remove — subtract. This is how holes, pockets and slots are made. You sketch the hole and remove it; you do not draw a part with a hole in it.
  • Intersect — keep only the overlap. Rare, but the neatest way to trim a part to a curved face.

Depth options worth knowing on day one

  • Blind — a number you type. Fine, and what you will use most.
  • Symmetric — grows equally both ways from the sketch plane. Use it whenever the sketch sits on a plane through the middle of the part, so the part stays centred as it resizes.
  • Up to face / up to part — the depth is whatever reaches that face. Now the feature tracks the thing it is supposed to reach instead of a number you would have to remember to update.
  • Through all — for removes. A hole that says “through all” is still a hole after you make the plate thicker. A hole that says 4 mm becomes a dimple.

Fillets and chamfers go last

A fillet rounds an edge; a chamfer cuts it at an angle. Both are applied as features to edges of an existing solid, and both belong at the bottom of your feature list.

Two reasons. Cosmetic rounding creates faces that later features would have to reference, and those references are fragile. And when a model misbehaves, suppressing a block of fillets at the end is a one-click way to find out whether they are the cause.

For printing there is a third reason, and it is the one you will care about: a chamfer on a bottom edge prints cleanly while a fillet on a bottom edge is an overhang that starts at 90°. Lesson six goes into this properly.

Hands on

Turn the plate into a wall bracket

Done when: One part, built from an add, a remove, and a chamfer, with the hole set to through-all so it survives a thickness change.

  1. Open your plate. Sketch on its top face a 20 mm square near one end and extrude it 15 mm with Add — an upstand. Notice you did not draw the plate again.
  2. Sketch a 5 mm circle on the top face of the plate, use dimensions from two edges to place it, and extrude it with Remove set to through all.
  3. Change the plate’s extrude depth from 10 mm to 6 mm. The hole is still a hole. Set the removal to a blind 10 mm instead and repeat — now it is a blind pocket. Undo back to through all.
  4. Apply a chamfer of 0.6 mm to the four edges where the plate meets the build plate. Your first prints will be noticeably easier to release, and the elephant-foot bulge stops mattering.
  5. Add a fillet of 3 mm where the upstand meets the plate. That inside corner is where the bracket would snap; the fillet is structural, not decorative.
  6. Drag the fillet feature above the chamfer in the feature list and back again. Watch the rebuild. Order is not cosmetic — it is the program.

Check your recall

Answer from memory — no scrolling back.

  1. 1. How do you put a hole through a part in parametric CAD?
  2. 2. A hole must stay open no matter how thick the plate becomes. Which depth setting?
  3. 3. Why do fillets and chamfers belong late in the tree?
  4. 4. Which feature suits a knob turned from a round silhouette?

Read this next — primary source

Onshape Help — Extrude

Onshape documentation

Read the options list for one feature properly and the rest of the toolbar stops being intimidating, because every feature asks you the same four questions in the same order: what profile, how far, which direction, and what to do with the result.

Stuck, curious, or think this lesson is wrong? Ask your teaching agent. That’s the point of the workspace — the lessons are the scaffold, the conversation is where the learning gets unstuck.