Skip to main content

Designing for the CNC

Everything on this page follows from one fact: the cutting bit is a spinning cylinder. It removes material in a circle, so any shape it cuts inherits the roundness of that circle. Designs that ignore this look fine in Fusion and fail on the machine.

Read this while you're still in CAD. Fixing these problems after the toolpath is made means going back to CAD anyway.

A round bit cannot cut a sharp inside corner​

If you draw a square pocket and cut it with a 1/4 inch (6.35 mm) bit, the inside corners come out with a 3.18 mm radius — half the bit diameter. The bit physically cannot reach into the corner.

This matters most when a square tab has to seat into that pocket: the tab's sharp corners hit the pocket's round corners and the joint won't close.

Three ways to handle it:

  • Design the radius in. Round the inside corners of your pocket to the bit radius or larger, and round the mating part's corners to match. Cleanest result, and the part looks intentional.
  • Add relief cuts — dogbones or T-bones. A small extra circle or slot cut into each corner gives the tab's corner somewhere to go. Standard practice for finger joints and slot-together assemblies. Slightly visible; completely functional.
  • Sand or chisel the corners by hand. Fine for one or two corners, tedious for twenty.

Outside corners are the opposite: a bit cuts those perfectly sharp, no allowance needed.

Minimum feature size​

  • No hole, slot, or gap smaller than the bit diameter. A 3 mm slot cannot be cut with a 6.35 mm bit at all — the software will silently skip it, or cut something wider than you drew.
  • Keep thin walls thicker than the bit. A 2 mm-wide standing rib in plywood will splinter off during the cut even if the geometry is technically valid.
  • Avoid tiny islands. A small piece surrounded by cut material has nothing holding it and becomes a projectile. If your design needs one, keep it attached with tabs.

Tabs: keep your part from moving mid-cut​

When a through-cut finishes, the part is a loose piece inside a spinning cutter. Tabs are small uncut bridges that hold it to the surrounding stock until you cut or snap them free afterward.

  • Put tabs on straight edges, not on corners or on a surface that has to end up perfectly flat.
  • More small tabs beat a few thick ones — easier to clean up, same holding power.
  • Plan where they'll go while you're designing, so they don't land in the middle of a joint face.

Model to the real thickness of the material​

A sheet sold as 1/2 inch plywood is usually not 12.7 mm, and two sheets from the same rack can differ. If you model a 12.7 mm dado and the sheet is 11.6 mm, the shelf rattles.

Measure the actual sheet with calipers, then model that number. Better still, drive the dimension from a Fusion parameter named something like stockThickness, so switching to a different sheet is a one-number edit rather than a remodel.

See Tolerance and Fit for how much clearance to leave once you have the real measurement.

Depth, and why one pass isn't enough​

The machine cuts through thick material in several shallow passes rather than one deep plunge. A pass that's too deep is how bits break and edges burn. The toolpath software handles this for you once you've picked the right bit and material. Carbide 3D's own feeds and speeds guidance is the source to check before you invent your own numbers, and ask June if you're unsure what to run for a given bit and material.

What this means for your design: depth costs time. A pocket 3 mm deep cuts in a fraction of the time of one 12 mm deep. With one CNC shared across the class, shallow-where-possible is a real design consideration, not just an optimization.

Leave room for work holding​

The stock has to be held down, and the bit cannot cut where a clamp is sitting. Leave a border of waste material around your parts — generally an inch or so — and don't nest parts right up to the edge of the sheet.

Clamps and screws into the wasteboard are the usual answer. Double-stick tape also works when it suits the part, and it has the advantage of leaving the whole top surface clear. Which one to use depends on the cut, so talk it through before you commit a layout that only works one way.

Plywood-specific gotchas​

  • Cut direction affects tearout. The top veneer can splinter along the cut edge. It shows most on cross-grain cuts and on the face you'll see.
  • Voids happen. Cheap plywood has internal gaps you can't see until you cut through one. Not your fault; plan a spare if a visible face matters.
  • Sanding changes dimensions. If you plan to sand a joint face, you're removing material after you cut to size. Account for it or sand only the faces that don't have to fit anything.

Watch out for both ends of Z travel​

Our machine has a limited window of Z travel. A retract that runs to the top makes the next plunge cut too deep, and a cut that runs the carriage off its plates at the bottom jumps and skews. It's mostly a setup check rather than a design rule, but a very thick part or a cut deliberately into the wasteboard is where your design will run into it. See Running the CNC for the check to run before you zero.