DDCSV

For DDCSV standalone controllers.

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 — G00 for rapids and G01 for cuts, never arcs — and every line is 80 characters or fewer.

The file ends with:

G00 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 is not available on DDCSV, and the profile refuses it. Neither DDCSV manual says what the controller does with T, M6 or M0, so the file might not stop for the change, and the next tool's passes would run with the old bit in the spindle.
• M6 with G43 is not available on DDCSV, and the profile refuses it.

Before the first run

DDCSV firmware is particular about format, so the file is written its way: two-digit G00 and G01, every axis on every line, and comments after a semicolon rather than in brackets.

Let the file set the speeds. Out of the box a DDCSV controller ignores the feed rates and spindle speed in the file: it runs every cutting move at its own default feed (parameter #76, 1500 mm/min) and the spindle at its own default speed (#221, 12000 rpm). Set parameter #15 to 0 and parameter #220 to 0 so it uses the file's feeds and spindle speed. Check this before the first run: a plunge at the default feed can break a small bit.

At the end of the file the M30 line makes the controller raise Z to its own safe height (parameter #82) and move X and Y home. If your clamps stand taller than that height, raise #82 first.

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.