GRBL

For GRBL 1.1 controllers and the senders that drive them, such as Universal G-code Sender, CNCjs or gSender.

What the file looks like

The file starts with comments naming the project, the machine and the tools, then:

G21 G90 G17 G94
G54

Millimetres are G21; a profile that outputs inches writes G20 instead. The spindle starts with S{rpm} M3 followed by a dwell (G4 P seconds) for the spin-up time in your profile, unless spindle control is set to none. Cutting moves are straight lines only — G0 for rapids and G1 for cuts, never arcs — and every line is 80 characters or fewer.

The file ends with:

G0 Z{safe}
M5
M30

Tool changes

• One file per tool works: run the files in order and change the tool between them.
• M6 and pause writes T{n} M6 then M0. GRBL itself ignores M6 and T; the M0 pauses the job, and many senders offer their own tool-change routine at that point.
• M6 with G43 is not available: GRBL has no tool table. The profile refuses it.

Before the first run

GRBL reads one line at a time into a small buffer, which is why ReliefCAM keeps every line short. If your sender adds line numbers or checksums, leave line numbers off in the profile.

Set X and Y zero at the front-left corner of the piece and Z zero on the top of the stock, and run the first file with the tool well above the work and a hand on the feed hold.