linuxcnc/nc_files/OFFSETS.md

Offsets Quick Reference

Coordinate Stack

What you see = machine position + work offset (G54...) + G52/G92 + tool length offset (G43)

G53 bypasses everything and moves in machine coords.

Work Offsets (G54–G59.3)

9 available coordinate systems. G54 is default. Persist across power cycles (stored in linuxcnc.var).

Touching off work zero

In GMOCCAPY: Jog to desired zero, click the axis letter (X/Y/Z) in the DRO, enter 0. Done. Internally: G10 L20 P0 <axis> 0

Pendant: Macro 5/6/7 = zero X/Y/Z. Macro 1/2 = halve X/Y (center-finding: zero one edge, jog to other edge, halve).

In G-code:

G10 L20 P1 X0 Y0 Z0    ; set G54 origin to current position
G10 L20 P0 X0           ; set current system's X to 0

Switching systems

G55    ; all coords now relative to work offset 2

In GMOCCAPY: Offset page > click row > "Set Active".

Editing numerically

In GMOCCAPY: Offset page > double-click a cell > type value. This uses G10 L2 (absolute set), not touch-off.

Temporary offsets

G52 X1 Y1    ; shift on top of active G5x (good for pattern repeats)
G52 X0 Y0    ; cancel

Avoid G92 — it persists across program runs and causes confusion. Use G92.1 to clear if needed.

Tool Length

Setting up a tool (first time)

1. In GMOCCAPY Tool page: set diameter (D column) and any known Z offset. Click "Apply Changes".
2. Or in G-code: G10 L1 P1 Z-2.5 R0.125 (R = radius, stored as D = diameter = 2R)

Loading a tool

T1 M6    ; select + change (pops up dialog, operator confirms)
G43      ; activate its Z offset — REQUIRED or Z is wrong

Touching off tool length

Jog tool tip down to top of workpiece, then in MDI:

G10 L10 P1 Z0    ; "tip is at Z=0, calculate and store the offset"
G43               ; activate it

Or: GMOCCAPY DRO > click Z letter > enter 0 (but this sets the work offset, not the tool offset — different thing).

Canceling

G49    ; cancel tool length offset

Standard practice: G49 before each tool change, G43 after.

Cutter Radius Compensation (G41/G42)

Offsets the toolpath left or right of the programmed line by the tool's radius. Program the actual part edge; the machine handles the rest.

G41      ; offset LEFT of path (climb milling outside profiles)
G42      ; offset RIGHT
G40      ; cancel

The D word in G41/G42 is a tool number (not a diameter): G41 D1 looks up tool 1's diameter from the table. Omit D to use the current tool.

Rules:

• Lead-in move after G41/G42 must be >= tool radius
• Lead-out move with G40 must be >= tool radius
• Must be in G17 (XY plane)

G41                  ; comp on
G1 X0 Y0 F10        ; lead-in (this IS the first compensated move)
G1 X2 Y0            ; cut along part edge — tool rides 1 radius to the left
G1 X2 Y2
G40                  ; comp off (next linear move is lead-out)
G0 X-1 Y-1

Dynamic variant: G41.1 D0.250 — D is a literal diameter value, not a tool number.

Our macros handle radius compensation internally via #<_td>. Don't use G41/G42 with macro calls.

Tool Table Columns (mill)

Column	Meaning
T	Tool number
P	Pocket (we use P = T)
Z	Length offset
D	Diameter (not radius)

DRO Modes (click axis value to cycle)

Mode	Color	Shows
Relative	Black	Work coords (what G-code sees)
Absolute	Blue	Machine coords (G53)
DTG	Yellow	Distance to go

Green digits = homed. Red = unhomed.

Named Parameters

Parameter	Value
#<_current_tool> / #5400	Tool in spindle
#5410	Current tool diameter
#<_td>	Our macros' tool diameter (user-set, not built-in)