Mach3 and Mach4

For Mach3 and Mach4. Both read the same file.

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 M3 S{rpm} 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; Mach runs its own M6 macro first.
• M6 with G43 writes T{n} M6 and G43 H{h}, where h is the tool's length offset number, from Mach's tool table.

Before the first run

Mach's dwell is in seconds by default, which is what the file assumes. If you have changed Mach to milliseconds, change it back or the spin-up dwell will be a thousand times too short.

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.