G10 Programmable data input, offsets / Programmable data input

Fanuc G-code · Mill, Lathe

On mills: Programmable data input, offsets

Writes values into the offset pages from the program. L2 sets work offsets G54 to G59, L20 sets G54.1 extra offsets, and L10 to L13 set tool length and radius offsets.

Verify on your machine. This entry could not be fully checked against the maker manual. Check your machine manual before you run it.

Format

G10 L2 P X Y Z or G10 L20 P X Y Z or G10 L P R

Addresses

Address	What it does
`L2`	Work offset, P0 external shift, P1 to P6 for G54 to G59
`L20`	Extra work offset, P1 to P48 for G54.1 P1 to P48
`L10`	Tool length geometry for H, offset memory C
`L11`	Tool length wear for H, offset memory C
`L12`	Cutter radius geometry for D, offset memory C
`L13`	Cutter radius wear for D, offset memory C
`P`	Offset or work offset number
`R`	Tool offset value
`X Y Z`	Work offset values for each axis

How it works

One shot, group 00.

Example program

G90 G10 L2 P1 X-15.2345 Y-8.5000 Z0. (SET G54)
G90 G10 L2 P2 X-10.2345 Y-8.5000 Z0. (SET G55)
G90 G10 L20 P1 X-5. Y-8.5 Z0. (SET G54.1 P1)
G90 G10 L10 P5 R-6.2500 (SET H5 LENGTH GEOMETRY)
…

The full 7-line example is in the app. Example is in inch. Check offsets and clearances first.

Watch out for

In G90 the value replaces what is there. In G91 it is added to the existing value. Check the mode before running.
With offset memory A or B the L numbers differ. Memory B uses L10 for geometry and L11 for wear only.
On a lathe G10 uses different addresses, so do not copy mill G10 lines to a lathe.

On lathes: Programmable data input

Writes offsets from the program. On a lathe it sets work offsets with L2 and tool offsets with P. X and Z replace the value, U and W add to it.

Format

G10 L2 P X Z or G10 P X(U) Z(W) R Q

Addresses

Address	What it does
`L2 P`	Work offset. P0 is the external shift, P1 to P6 are G54 to G59
`P`	Tool offset number. P1 and up is wear. 10000 plus the number is geometry
`X Z`	Value to set
`U W`	Value to add to the existing offset
`R`	Tool nose radius
`Q`	Imaginary tool tip direction

How it works

Non-modal.

Example program

G10 L2 P1 X0 Z-12.5 (SET G54 Z SHIFT)
G10 P1 U-.002 (TAKE .002 OFF DIAMETER ON WEAR 1)
G10 P10002 R.0313 Q3 (TOOL 2 GEOMETRY, NOSE RADIUS, TIP 3)

Example is in inch. Check offsets and clearances first.

Watch out for

X sets and U adds. Using X when you meant U overwrites the offset.
Wear and geometry offset numbering can differ by parameter. Prove it with a dry run on one offset.
Many shops lock G10 out with a parameter for safety.

Related codes

G11 · G54 · G54.1 · G43 · G41 · G42

G10 on other controls

The same number can mean something different on another control.

Control	Meaning
Haas NGC	Programmable offset setting
Mazak (EIA)	Program data setting, offsets
Okuma OSP	Cancel coordinate shift and rotation
Mitsubishi M70 M80	Program data input for offsets
Brother Speedio	Programmable data input
Heidenhain TNC (ISO)	Rapid straight line, polar
Fagor 8055 8065	Mirror image cancel
Mach3 Mach4	Set offsets from the program
Centroid CNC12 Acorn	Set parameter or offset from program
Hurco WinMax (NC)	Data setting, offsets by program
Fadal	Programmable data input

Every G-code for Fanuc in your pocket. The app has the full example programs, search by number or shop word, a line decoder and calculators for tapping, threading and drilling.

Open G10 in the app All Fanuc G-codes

App Store Google Play