Sinumerik 840D G-codes: reference by group

Sinumerik 840D and 840D sl G commands sorted by G group: motion, planes, offsets, frames, feed types, continuous-path mode and the keyword commands that share the groups.

On a Sinumerik control, G commands are organized in numbered G groups. Only one command per group can be written in a block. A command stays active until another command of the same group replaces it (modal), or it acts only in its own block (non-modal). Many groups contain keywords instead of G numbers, for example TRANS, BRISK or CUT2D.

This page lists the groups that matter for everyday milling and turning. Groups for punching, nibbling, grinding, spline transitions and OEM extensions are left out. The “Default” column shows the command that is active after power-on, reset or program end in the delivery state. The machine builder can change these defaults, so the actual state on a machine may differ.

Machining cycles such as CYCLE81 are described on the page Cycles.

Differences to Fanuc-style G-codes

Several numbers have a different meaning than on Fanuc controls. G70/G71 select inch/metric (Fanuc: G20/G21). G74 is a reference point approach and G75 a fixed-point approach, they are no cycles. G500 deselects the work offset. G53 is non-modal and switches off the programmable and settable frames for one block. Leading zeros are optional, G0 and G00 are the same command.

Essential G-codes

Command	Description
G0	Rapid traverse
G1	Straight line at feedrate
G2	Arc, clockwise
G3	Arc, counterclockwise
G4	Dwell
G17	Working plane X/Y, tool axis Z
G18	Working plane Z/X, tool axis Y
G40	Cutter radius compensation off
G41	Cutter radius compensation, tool left of the contour
G42	Cutter radius compensation, tool right of the contour
G54	Work offset 1
G500	Work offset deselected
G64	Continuous-path mode
G71	Metric input
G90	Absolute dimensions
G91	Incremental dimensions
G94	Feed in mm/min
G95	Feed in mm/rev
G96	Constant cutting speed
G97	Constant spindle speed

Full reference

Type: m = modal, s = non-modal (block by block).

Command	Description	Type	Default
G0	Rapid traverse	m
G1	Linear interpolation at feedrate	m	Yes
G2	Circular interpolation clockwise	m
G3	Circular interpolation counterclockwise	m
CIP	Arc defined by an intermediate point and end point	m
CT	Arc that continues tangentially from the previous element	m
ASPLINE	Akima spline	m
BSPLINE	B-spline	m
CSPLINE	Cubic spline	m
POLY	Polynomial interpolation	m
G33	Thread cutting, constant lead	m
G34	Thread cutting, lead increasing linearly	m
G35	Thread cutting, lead decreasing linearly	m
G331	Rigid tapping, cutting move	m
G332	Rigid tapping, return move	m
INVCW	Involute, clockwise	m
INVCCW	Involute, counterclockwise	m
G335	Convex thread, clockwise	m
G336	Convex thread, counterclockwise	m

Command	Description	Type
G4	Dwell time	s
G63	Tapping with compensating chuck, no synchronization	s
G74	Approach reference point	s
G75	Approach fixed point	s
G147	Soft approach on a straight line	s
G247	Soft approach on a quarter circle	s
G347	Soft approach on a semicircle	s
G148	Soft departure on a straight line	s
G248	Soft departure on a quarter circle	s
G348	Soft departure on a semicircle	s
REPOSL, REPOSQ, REPOSH	Return to the contour after an interruption (straight, quarter circle, semicircle)	s
REPOSA, REPOSQA, REPOSHA	As above, moving all axes	s
G5, G7	Oblique plunge grinding and its compensating move	s

Group 3: Programmable frames, limits and pole

Command	Description	Type
TRANS	Programmable zero offset, replaces previous programmable frame	s
ATRANS	Programmable zero offset, added to the current frame	s
ROT	Programmable rotation, replaces previous programmable frame	s
AROT	Programmable rotation, added to the current frame	s
ROTS	Rotation defined by solid angles	s
AROTS	Additive rotation by solid angles	s
SCALE	Scale factor, replaces previous programmable frame	s
ASCALE	Scale factor, added to the current frame	s
MIRROR	Mirroring, replaces previous programmable frame	s
AMIRROR	Mirroring, added to the current frame	s
G25	Lower working area limit, or minimum spindle speed	s
G26	Upper working area limit, or maximum spindle speed	s
G58	Programmable offset, absolute part replaced axis by axis	s
G59	Programmable offset, additive part replaced axis by axis	s
G110	Pole referenced to the last programmed position	s
G111	Pole referenced to the origin of the workpiece coordinate system	s
G112	Pole referenced to the last valid pole	s

Group 6: Plane selection

Command	Description	Type	Default
G17	Plane of 1st and 2nd geometry axis (X/Y), infeed in Z	m	Yes
G18	Plane of 3rd and 1st geometry axis (Z/X), infeed in Y	m
G19	Plane of 2nd and 3rd geometry axis (Y/Z), infeed in X	m

Group 7: Cutter radius compensation

Command	Description	Type	Default
G40	Compensation off	m	Yes
G41	Tool runs on the left of the contour	m
G42	Tool runs on the right of the contour	m

Group 8: Settable work offsets

Command	Description	Type	Default
G500	Settable work offset off	m	Yes
G54	Work offset 1	m
G55	Work offset 2	m
G56	Work offset 3	m
G57	Work offset 4	m
G505 to G599	Work offsets 5 to 99	m

How many of the offsets G505 to G599 exist depends on the machine configuration.

Group 9: Suppressing frames and offsets

Command	Description	Type
G53	Programmable and settable frames off for one block	s
G153	As G53, also the basic frames off	s
SUPA	As G153, also handwheel offsets, external offset, PRESET and overlaid motion off	s
SUPD	Active tool offsets off for one block	s

Group 10: Exact stop and continuous-path mode

Command	Description	Type	Default
G60	Exact stop at each block end	m	Yes
G64	Continuous-path mode	m
G641	Continuous-path mode, corners rounded within a programmed distance (ADIS, ADISPOS)	m
G642	Continuous-path mode, rounding within axis tolerances	m
G643	As G642, rounding computed inside the block	m
G644	Continuous-path mode, rounding with highest possible dynamics	m
G645	As G642, also smoothing tangential block transitions	m

Group 11 and 12: Exact stop details

Command	Description	Type	Default
G9	Exact stop in this block only	s
G601	Next block starts when the fine exact stop window is reached	m	Yes
G602	Next block starts when the coarse exact stop window is reached	m
G603	Next block starts when interpolation of the current block ends	m

Group 13: Inch and metric

Command	Description	Type	Default
G70	Lengths in inch	m
G71	Lengths in mm	m	Yes
G700	Lengths and feedrates in inch and inch/min	m
G710	Lengths and feedrates in mm and mm/min	m

Group 14: Absolute and incremental

Command	Description	Type	Default
G90	Absolute dimensions	m	Yes
G91	Incremental dimensions	m

Single values can be switched for one coordinate: X=AC(20) is absolute, X=IC(5) is incremental, regardless of G90/G91.

Group 15: Feed type and spindle speed mode

Command	Description	Type	Default
G93	Inverse time feed	m
G94	Feed per minute (mm/min, inch/min)	m	Yes
G95	Feed per revolution (mm/rev, inch/rev)	m
G96	Feed per revolution with constant cutting speed	m
G97	Feed per revolution, constant cutting speed off	m
G931	Feed given as travel time, constant path velocity off	m
G961	Feed per minute with constant cutting speed	m
G971	Feed per minute, constant cutting speed off	m
G942	Feed per minute, freezes cutting speed or spindle speed	m
G952	Feed per revolution, freezes cutting speed or spindle speed	m
G962	Feed per minute or per revolution with constant cutting speed	m
G972	Feed per minute or per revolution with constant spindle speed	m
G973	Feed per revolution, constant spindle speed without speed limit (ISO mode)	m

Group 16: Feed at curved contours

Command	Description	Type	Default
CFC	Programmed feed applies at the contour, for inside and outside arcs	m	Yes
CFTCP	Programmed feed applies at the tool center point	m
CFIN	Feed reduced on inside arcs only, outside arcs at center point feed	m

Group 17 and 18: Radius compensation at start, end and corners

Command	Description	Type	Default
NORM	Tool stands perpendicular to the contour at start and end point	m	Yes
KONT	Tool travels around the contour point at start and end	m
KONTT	Approach and departure with constant tangent	m
KONTC	Approach and departure with constant curvature	m
G450	Outside corners with a transition arc	m	Yes
G451	Outside corners at the intersection of the offset paths	m

Group 21: Acceleration profile

Command	Description	Type	Default
BRISK	Acceleration step without jerk limitation	m	Yes
SOFT	Jerk-limited acceleration	m
DRIVE	Acceleration reduced as speed rises	m

Group 22: Type of tool radius compensation

Command	Description	Type	Default
CUT2D	2½D compensation in the working plane	m	Yes
CUT2DF	2½D compensation in the plane of the current frame (inclined plane)	m
CUT3DC	3D compensation, peripheral milling	m
CUT3DF	3D compensation, face milling with changing orientation	m
CUT3DFS	3D compensation, face milling with fixed orientation from G17 to G19	m
CUT3DFF	3D compensation, face milling with fixed orientation from G17 to G19 including frame rotation	m
CUT3DCC	3D peripheral milling with limiting surface, path on the machined surface	m
CUT3DCCD	3D peripheral milling with limiting surface, path of the tool center point	m

Group 23: Collision check at inside contours

Command	Description	Type	Default
CDOF	Collision check off	m	Yes
CDON	Collision check on, bottlenecks are detected	m
CDOF2	Collision check off for 3D peripheral milling	m

Group 28 and 29: Working area limit and diameter programming

Command	Description	Type	Default
WALIMON	Working area limit active	m	Yes
WALIMOF	Working area limit off	m
DIAMOF	Radius programming	m	Yes
DIAMON	Diameter programming, absolute and incremental values	m
DIAM90	Diameter programming for G90, radius for G91	m
DIAMCYCOF	Diameter programming off during cycle execution	m

Group 30 and 39: Block compression and contour accuracy

Command	Description	Type	Default
COMPOF	Block compression off	m	Yes
COMPON	Compressor for short linear blocks	m
COMPCURV	Compressor with constant curvature	m
COMPCAD	Compressor optimized for surface quality from CAD/CAM data	m
COMPSURF	Compressor for free-form surfaces	m
CPRECOF	Programmable contour accuracy off	m	Yes
CPRECON	Programmable contour accuracy on (value in CTOL)	m

Group 47: Language mode

Command	Description	Type	Default
G290	Sinumerik mode	m	Yes
G291	ISO dialect mode (Fanuc-style programs)	m

Group 49 and 55: Point-to-point and rapid traverse

Command	Description	Type	Default
CP	Path motion, the tool point follows the path	m	Yes
PTP	Point-to-point, axes move synchronized in machine coordinates	m
PTPG0	PTP for G0 only, path motion otherwise	m
RTLION	G0 interpolates linearly	m	Yes
RTLIOF	G0 moves each axis independently	m

Group 52 and 53: Frame alignment for inclined machining

Command	Description	Type	Default
PAROTOF	Rotation aligned to the workpiece off	m	Yes
PAROT	Workpiece coordinate system rotated to match the workpiece	m
TOROTOF	Rotation aligned to the tool off	m	Yes
TOROT, TOROTZ	Frame rotated so Z points along the tool	m
TOROTY, TOROTX	Frame rotated so Y or X points along the tool	m
TOFRAME, TOFRAMEZ	As TOROT, frame set on the current tool orientation	m
TOFRAMEY, TOFRAMEX	As TOROTY/TOROTX with TOFRAME behavior	m

Group 57 and 59: Corner deceleration and dynamics

Command	Description	Type	Default
FENDNORM	Corner deceleration off	m	Yes
G62	Slow down at inside corners with radius compensation active	m
G621	Slow down at every corner	m
DYNNORM	Standard dynamic settings	m	Yes
DYNPOS	Dynamic settings for positioning and tapping	m
DYNROUGH	Dynamic settings for roughing	m
DYNSEMIFIN	Dynamic settings for semi-finishing	m
DYNFINISH	Dynamic settings for finishing	m
DYNPREC	Dynamic settings for precision finishing	m

Sinumerik 840D G-codes: reference by group

Essential G-codes

Full reference

Group 1: Modal motion commands

Group 2: Non-modal motion and dwell

Group 3: Programmable frames, limits and pole

Group 6: Plane selection

Group 7: Cutter radius compensation

Group 8: Settable work offsets

Group 9: Suppressing frames and offsets

Group 10: Exact stop and continuous-path mode

Group 11 and 12: Exact stop details

Group 13: Inch and metric

Group 14: Absolute and incremental

Group 15: Feed type and spindle speed mode

Group 16: Feed at curved contours

Group 17 and 18: Radius compensation at start, end and corners

Group 21: Acceleration profile

Group 22: Type of tool radius compensation

Group 23: Collision check at inside contours

Group 28 and 29: Working area limit and diameter programming

Group 30 and 39: Block compression and contour accuracy

Group 47: Language mode

Group 49 and 55: Point-to-point and rapid traverse

Group 52 and 53: Frame alignment for inclined machining

Group 57 and 59: Corner deceleration and dynamics