MASSO Mill post
Updated v2.4.7At a glance
- Mill G-code in MASSO's dialect — the mill counterpart of the MASSO Router post
- Never writes G43/G49 — MASSO applies tool length from its own tool table on a tool change
- T# M6 tool changes with optional M1 stop and next-tool preload for an automatic changer
- Optional canned G81/G83/G73 drill cycles closed with G80
- N sequence numbers on every block or only at tool changes
- Warns in the header when a setup's work offset falls outside G54–G59
The bundled MASSO Mill post writes G-code for MASSO controllers — the milling counterpart of
the MASSO Router post, built on the same shared mill base as the
GRBL, FluidNC and LinuxCNC posts. Select it on your machine and
everything else about posting works the way it already does: work offsets per
setup, tool changes, spindle and coolant, safe retracts, G2/G3 arcs.
Output defaults to .nc.
Tool length stays with the controller
MASSO measures tool length itself and applies it from its own tool table when it sees a tool
change, so the post writes no G43/G49 — nothing competes with what the control already
knows. There's no switch to turn them on, because G43 and G49 aren't codes MASSO accepts: they
are absent from its supported list, and a program containing them would fail at the control rather
than machine differently.
Tool changes
A tool change retracts to the configured safe position, stops spindle and coolant, optionally emits
M1, then writes T# M6 with the tool's description as a comment. With Preload tool on it
follows with a bare T# naming the next tool in the program, so an automatic changer can stage it
during the current cut. The first tool never gets a needless M1, and the header can list every
tool in the job with diameter and RPM. Spindle and coolant codes are emitted only when something
changes, so consecutive operations sharing a tool don't cycle the spindle between them — unless you
turn Keep spindle between operations off.
Canned drill cycles
With Canned drill cycles on, drill operations fold into MASSO's native
cycles chosen by the operation's peck mode: Single Plunge becomes G81, Full Retract pecking
becomes G83 with a Q peck depth, and Partial Retract becomes the chip-break cycle G73 — each
opened with G98 and closed with G80. Leave it off (the default) and drills post as expanded
G0/G1 peck moves that run identically. If a cycle can't express what the operation asks for,
the post quietly falls back to the expanded moves rather than writing something approximate.
Work offsets
MASSO reads G54–G59. A setup whose work offset falls past that range would post as G54.1 P1,
which MASSO rejects when it loads the file — so the post writes a plain-language warning at the top
of the program naming the offending offsets. Renumber those setups' work offsets and the warning
goes away.
Formatting options
Safe retract is configurable: G28 machine home (the default), G53 machine Z0, or a plain rapid
to clearance height — the last adds a header comment, since nothing guarantees that path is clear.
The header also carries G40 G80 to cancel cutter compensation and any modal cycle left over from
a previous program. Other options: N sequence numbers on every block or only at tool changes,
with start value and increment; (...) or # comments; I/J or R arcs; coordinate decimals;
and machine-info and tool-list header comments.