G54 to G59: Work Coordinate Systems (and G53)

The machine knows its own position from machine zero, the point it finds when it homes. Your part could be anywhere on the table. A work offset stores the distance from machine zero to the part zero you picked, such as the top-left corner of the stock. With a work offset active, X0 Y0 Z0 in the program means that corner.

The six standard work offsets

Code	Work coordinate system
G54	1 (the default on most controls)
G55	2
G56	3
G57	4
G58	5
G59	6

All six are modal: once selected, an offset stays active until another one is called. Programs normally state the offset in the safety line at the start, for example G21 G17 G90 G54.

Running several parts with one program

A common use is one vise per offset. You set G54 on the first part and G55 on the second, and the program runs the same toolpath twice:

G54
(toolpath for part 1)
G55
(the same toolpath for part 2)

Because the code is identical apart from the offset, you only have to prove out one toolpath.

Extended work offsets

Six isn't always enough for fixtures with many parts:

• Fanuc: G54.1 P1 to G54.1 P48 (more with an option).
• Haas: G154 P1 to G154 P99. The first 20 can also be called as G110 to G129.
• LinuxCNC: G59.1, G59.2 and G59.3, for nine in total.
• GRBL: the six standard offsets only.

Setting offsets in the program with G10

Offsets are usually set at the machine by touching off. They can also be set from the program:

• G10 L2 P1 X-250 Y-180 Z-90 sets offset 1 (G54) to those machine coordinates. Fanuc, Haas, LinuxCNC and GRBL all support it.
• G10 L20 P1 X0 Y0 Z0 (LinuxCNC and GRBL) sets offset 1 so that the current position becomes X0 Y0 Z0.

G53: machine coordinates

G53 ignores the active work offset for one line only and moves in machine coordinates. It's non-modal, so the next line is back in the work offset.

G53 G0 Z0

This raises the spindle to machine Z zero, normally the top of travel, whatever work offset is active. Haas programs use it before tool changes and at the end of a program. Use it with G0 or G1 in absolute mode (G90).

G53 is different from G28: G53 moves straight to the machine position you give, with no intermediate point.

How CutViewer shows G54 to G59 and G53

CutViewer tracks which work offset is active and shows it in the status bar, but it doesn't know your offset values. Everything is drawn in program coordinates, so toolpaths for G54 and G55 appear on top of each other rather than side by side.

CutViewer also doesn't know your machine coordinates, so it doesn't draw G53 moves: the next move is drawn from the last position it knows. A line such as G53 G0 Z0 at the end of a program won't show as a move into the part.