Skip to main content

Running the CNC

Our CNC is a Shapeoko 3 XL — a computer-controlled router. You design a toolpath on a computer, the machine drives a spinning bit through material to match it. It is the loudest, dustiest, and least forgiving machine in the shop, and the one with the longest queue, so preparation matters more here than anywhere else.

You must be certified before running it without an adult standing with you. See Machine Certification.

Carbide 3D — who make the machine and the software — publish a complete free course, Running a Shapeoko. Work through it rather than treating this page as a substitute; this page covers our machine, our sequence, and our shop rules.

Before you touch the machine​

  • PPE. Safety glasses always. Hearing protection while it's cutting — for you and for anyone standing nearby. An N95 for MDF and heavy dust. Details on the PPE page.
  • No gloves. The router spins, and a glove can catch on a spinning tool and pull your hand in.
  • Tie back anything loose — hair, sleeves, drawstrings, lanyards.
  • Have your design finished and exported. DXF, correct units, closed contours. See Exporting Your Design. Machine time is not CAD time.

Software: two programs, two jobs​

ProgramWhat it does
Carbide CreateTurns your 2D outlines into toolpaths and exports the file the machine runs
Carbide MotionDrives the machine — jogging, zeroing, starting the job

Both are free from Carbide 3D (Carbide Create, Carbide Motion) and installed on the shop computer. Carbide 3D's Carbide Create course is the walkthrough; we won't duplicate it.

Making toolpaths in Carbide Create​

  1. Set the stock size and thickness to the actual piece of material you're going to clamp down — measured, not nominal.
  2. Import your DXF and check one known dimension against your CAD model. If it's off, the units are wrong. Fix it now.
  3. Set the zero corner to match where you'll zero on the real machine — typically the bottom left. Getting these two out of sync is the most common way a job cuts into a clamp.
  4. Pick your bit from the tool library — the one you're going to use. It doesn't have to be in the machine yet, but the toolpath has to match what ends up in the collet.
  5. Create the toolpaths — contour for outlines, pocket for recesses, and choose whether the cut runs inside, outside, or on the line. Cutting on the line makes every part half a bit-width too small; this trips up nearly everyone once.
  6. Add tabs to any part that gets cut all the way through.
  7. Simulate. The simulation runs very fast by default — slow it down so you can actually see the order of cuts. Look for cuts going where you didn't intend, features that vanished because they're smaller than the bit, and plunges deeper than your stock.
  8. Save the file with a version number in the name.

At the machine​

  1. Unplug the router first. Everything in the next few steps happens with your hands near the bit, so take the spindle's power out of the picture before you start.

  2. Secure the stock. Clamps or screws into the wasteboard, with the border you left in your design — or double-stick tape where that suits the part better. Wiggle it: if you can move it by hand, the router can move it at speed.

  3. Install the bit and tighten the collet properly, router still unplugged. A bit that slips mid-cut plunges deeper as it goes.

  4. Initialize the machine in Carbide Motion and let it home itself. Keep hands clear; it moves on its own.

  5. Check the router height as soon as you start jogging, before you zero. Z can only travel so far in each direction, and a job that runs past either end loses its position:

    • Topping out. Our machine stops counting position once the Z axis reaches the top of its travel — so if a retract sends it that high, the next plunge goes deeper than the toolpath intends.
    • Bottoming out. The Z carriage is only supported while every one of its wheels is still on a plate. Below that point it jumps, skews the cut, and knocks on the way back up.

    Jog the bit down to the bottom of the cut — the wasteboard surface, for a through-cut — and confirm every wheel is still on its plate. Then jog up to the height the job retracts to above your stock and confirm Z isn't at the top of its travel.

    Most jobs fit without changing anything. The two that usually don't are a very thick part, which pushes the job toward the top, and cutting into the wasteboard on purpose — making a fence, say — which pushes it toward the bottom. Where the router sits in its holder decides which limit you're near:

    • Coming off the bottom? Lower the router in its holder. The tip then sits lower for any given carriage position, so the carriage doesn't have to descend as far to reach the same cut depth.
    • Hitting the top? Raise it, for the same reason in reverse.

    Each move trades one limit for the other, so the job has to fit in the window between them. If it won't, get June rather than splitting the difference and hoping.

  6. Set zero — X, Y, and Z — to the same corner you chose in Carbide Create. This comes after the router height check because moving the router moves the bit tip, so a Z zero set beforehand would be wrong. Carbide 3D's Movements and Zeroing lesson covers this in detail. Double-check Z: a Z zero that's off by the thickness of your material is how a bit gets driven into the wasteboard.

  7. Confirm the job fits your stock. Compare the job's dimensions against the piece you just clamped down, in both X and Y. This catches more mistakes than watching the machine move through the air does.

  8. Plug the router back in, turn on dust collection, then start the job. The software will take you through the steps of setting the bit and speed. Turn on the router before hitting "ok" on the speed setting step. Our dust collection is a shop vac with a cyclone attachment.

  9. Stay with the machine the entire time. Hand on the stop, eyes on the cut. Never walk away from a running job — not for a minute, not to grab something.

Stop the machine if​

  • The sound changes — a new pitch, chattering, or a stall.
  • You hear knocking as Z retracts — it's bottoming out.
  • You see smoke or smell burning.
  • The stock shifts, or a clamp moves.
  • The bit is cutting somewhere you didn't expect.
  • You're not sure. Stopping a job costs a few minutes; the alternatives cost more.

Get an adult before restarting after any of these.

After the job​

  1. Let the spindle stop completely, then unplug the router before reaching in. Unplug the router itself, not the CNC.
  2. Retrieve your parts, then cut or snap the tabs and clean up the edges.
  3. Vacuum the machine and the floor around it. The next person is queued behind you and shouldn't inherit your chips.
  4. Return the bit to its case and log anything odd — a dull bit, a loose clamp, a strange noise — to June (jpeters@universityprep.org) so the next team doesn't rediscover it the hard way.

Planning around the queue​

There is one CNC and a whole class. Two habits keep this from becoming your bottleneck:

  • Get your CAD and toolpaths finished before your machine slot, not during it.
  • Cut a cardboard test template first on the Silhouette. It costs minutes instead of an hour and catches the mistakes that would otherwise cost you a second slot.