g2dialect Consensus Gcode

This page provides reference information used by the g2dialect.

OK, There is no "standard" Gcode, despite multiple attempts to establish one. These pages collect common Gcode and Mcode uses derived from the following sources:

• NIST
• LinuxCNC
• Haas
• Fanuc
• Tormach
• CNC Cookbook

It also lists Reprap, Machinekit, TinyG and other usage that is incompatible with the common usage, and provides some notes and some recommendations for alternatives.

See also: Consensus Mcodes

Consensus Gcode Usage

This table lists rough consensus usage from the above sources.

Gcode	Command	Usage / Notes
G0	Coordinated Straight Motion at Rapid Rate	Rapid Traverse
G1	Coordinated Straight Motion at Feed Rate	Feed rate is honored, as are abs/inv-time feed rate modes
G2	Clockwise Circular/Helical Interpolation at Feed Rate	Controlled Arc Move
G3	Counterclockwise Circular/Helical Interpolation at Feed Rate	Controlled Arc Move
G4	Dwell	P is in seconds, not milliseconds or other units
G5.x	Reserved for curve and spline interpolation
G5	Cubic Spline	(LinuxCNC)
G5.1	Quadratic B-Spline	(LinuxCNC)
G5.2	NURBS, add control point	(LinuxCNC)
G5.3	NURBS, execute	(LinuxCNC)
G6	Not used
G7	Diameter Mode	Lathe usage
G8	Radius Mode	Lathe usage
G9	Exact Stop (non-modal)	Fanuc, Haas
G10	Programmable Data Input	See G10 Lxx commands below
G10 L1	Set Tool Table Entry
G10 L10	Set Tool Table, Calculated, Workpiece
G10 L11	Set Tool Table, Calculated, Fixture
G10 L2	Coordinate System Origin Setting
G10_L20	Coordinate Origin Setting Calculated
G11	Not Used
G12	CW circular pocket	(Haas, Tormach)
G13	CCW circular pocket	(Haas, Tormach)
G15	Polar coordinates	(Tormach, CNC Cookbook)
G16	Polar coordinates	(Tormach, CNC Cookbook)
G17	Select XY Plane
G17.1	Select UV Plane
G18	Select XZ Plane
G18.1	Select UW Plane
G19	Select YZ Plane
G19.1	Select VW Plane
G20	Set Units to Inches (Imperial)	Units selection governs movement, displays, and settings
G21	Set Units to Millimeters (Metric)	Units selection governs movement, displays, and settings
G22	Not used
G23	Not used
G24	Not used
G25	Not used
G26	Not used
G27	Reference Position Check	(Fanuc)
G28	Go To Predefined Position Through Point (G28)	Move to G28.1 stored position via optional intermediate point
G28.1	Set Predefined Position	Store current position for G28. All axes are stored.
G29	Go to G29 Reference Point	(Haas)
G30	Go To Predefined Position Through Point (G30)	Move to G30.1 stored position via optional intermediate point
G30.1	Set Predefined Position	Store current position for G30. All axes are stored.
G31	Straight Probe Until Skip	(Haas, Tormach)
G32	Thread Cutting	(Fanuc)
G33	Spindle Synchronized Motion
G33.1	Rigid Tapping
G34	Not used
G35	Automatic Tool Diameter Measurement	(Haas)
G36	Automatic Work Offset Measurement	(Haas)
G37	Automatic Tool Length Measurement	(Haas)
G38.2	Straight Probe To Workpiece	Report if failure
G38.3	Straight Probe To Workpiece
G38.4	Straight Probe Away From Workpiece	Report if failure
G38.5	Straight Probe Away From Workpiece
G39	Not used
G40	Cancel Cutter Compensation	Turn Compensation Off
G41	Start Cutter Radius Compensation Left
G41.1	Dynamic Cutter Compensation
G42	Start Cutter Radius Compensation Right
G42.1	Dynamic Cutter Compensation
G43	Tool Length Offset	Use Tool Length Offset from Tool Table.
G43	Tool Length Compensation, Positive	(Fanuc, Haas)
G43.1	Dynamic Tool Length Offset
G43.2	Apply additional Tool Length Offset
G44	Tool Length Compensation, Negative (Fanuc, Haas)
G49	Cancel Tool Length Compensation
G50	Reset Scale Factors to 1.0	(Haas, Tormach)
G51	Set Axis Data Input Scale Factors	(Haas, Tormach)
G52	Local Work Shift	(Fanuc, Haas)
G53	Motion In Machine Coordinate System	Non-Modal
G54	Select Coordinate System 1	Use Preset Work Coordinate System 1
G55	Select Coordinate System 2	Use Preset Work Coordinate System 2
G56	Select Coordinate System 3	Use Preset Work Coordinate System 3
G57	Select Coordinate System 4	Use Preset Work Coordinate System 4
G58	Select Coordinate System 5	Use Preset Work Coordinate System 5
G59	Select Coordinate System 6	Use Preset Work Coordinate System 6
G59.1	Select Coordinate System 7	Use Preset Work Coordinate System 7
G59.2	Select Coordinate System 8	Use Preset Work Coordinate System 8
G59.3	Select Coordinate System 9	Use Preset Work Coordinate System 9
G60	Unidirectional Positioning	(Haas)
G61	Exact Path Mode
G61.1	Exact Stop Mode
G62	Automatic Corner Override	(CNC Cookbook)
G63	Tapping Mode	(CNC Cookbook)
G64	Continuous Mode	Path Blending Mode
G65	Macro Subroutine Call	(Haas)
G68	Coordinate System Rotation
G69	Cancel Coordinate System Rotation
G70	Bolt Hole Circle	(Haas)
G71	Bolt Hole Arc	(Haas)
G72	Bolt Holes Along and Angle	(Haas)
G73	Drilling Cycle with Chip Breaking
G74	Reverse Tap Canned Cycle	(Haas)
G76	Multi-pass Threading Cycle	(Lathe)
G77	Back Bore Canned Cycle	(Haas)
G80	Cancel Motion Mode	including Canned Cycle
G81	Drilling Cycle
G82	Drilling Cycle with Dwell
G83	Drilling Cycle with Peck
G84	Tapping Canned Cycle	(Haas)
G85	Boring Cycle, No Dwell, Feed Out
G86	Boring Cycle, Stop, Rapid Out
G87	Bore/Manual Retract Canned Cycle	(Haas)
G88	Bore/Dwell Canned Cycle	(Haas)
G89	Boring Cycle, Dwell, Feed Out
G90	Absolute Distance Mode
G09.1	Absolute Arc Distance Mode
G91	Incremental Distance Mode	Set to Relative Positioning
G91.1	Incremental Arc Distance Mode
G91.x	Reset Coordinate System Offsets
G92	Set Coordinate System Offsets
G92.1	Cancel Coordinate System Offsets
G92.2	Cancel Offset Coordinate Systems, Do Not Reset Parameters
G92.3	Apply Parameters to Offset Coordinate Systems	Restore Axis Offsets
G93	Inverse Time Feed Rate Mode	Inverse Time Mode
G94	Units Per Minute Feed Rate Mode	Feed Rate Mode
G95	Units Per Revolution Feed Rate Mode
G96	Constant Surface Speed
G97	RPM Mode	Cancel Constant Surface Speed
G98	Initial Level Return In Canned Cycles	Canned Cycle Z Retract Mode
G99	R-point Level Return In Canned Cycles
G100+	Haas Gcodes continue from G100 to G188

Exceptions to Consensus Gcode Usage

The following table lists incompatibilities (bolded) with consensus Gcode. Incompatibilities may be due to:

• Differences in implementation from a consensus Gcode command
• Differences in parameter usage from a consensus Gcode command
• Additional or incompatible dot extensions
• Additional Gcode commands that are not in the consensus set

The implementation is noted in (Parens). When (Reprap) is noted it means that one or more of the major Reprap implementations do this, as there are variations.

Gcode	Consensus Usage	Non-Consensus Usage / Notes
G0	Coordinated Straight Motion at Rapid Rate	(Reprap) provides feed rate for G0. (Reprap) uses S to set endstop options during movement, (Reprap) defines E axes, which are not part of the Gcode axis set (XYZ ABC UVW). (Reprap) may invoke retraction and recharge on G0.
G1	Coordinated Straight Motion at Feed Rate	(Reprap) uses S to set endstop options during movement, (Reprap) defines E axes, which are not part of the Gcode axis set (XYZ ABC UVW)
G2	Clockwise Circular/Helical Interpolation at Feed Rate	(Reprap) motion features similar to G1. Note: circular/helical motion is rarely used in 3D printing.
G3	Counterclockwise Circular/Helical Interpolation at Feed Rate	(Reprap) motion features similar to G1. Note: circular/helical motion is rarely used in 3D printing.
G4	Dwell	(Reprap) dwell may use S to set dwell time in milliseconds (not seconds). Uses P for seconds. Note: S is a modal word who's usage here is incompatible as it conflicts with Spindle RPM setting
G5.x	Reserved for curve and spline interpolation
G5	Cubic Spline
G5.1	Quadratic B-Spline
G5.2	NURBS, add control point
G5.3	NURBS, execute
G6	Not used
G7	Diameter Mode
G8	Radius Mode
G9	Exact Stop (non-modal)
G10	Programmable Data Input
G10 L1	Set Tool Table Entry
G10 L10	Set Tool Table, Calculated, Workpiece
G10 L11	Set Tool Table, Calculated, Fixture
G10 L2	Coordinate System Origin Setting
G10_L20	Coordinate Origin Setting Calculated
G11	Not Used
G12	CW circular pocket
G13	CCW circular pocket
G15	Polar coordinates
G16	Polar coordinates
G17	Select XY Plane
G17.1	Select UV Plane
G18	Select XZ Plane
G18.1	Select UW Plane
G19	Select YZ Plane
G19.1	Select VW Plane
G20	Set Units to Inches (Imperial)
G21	Set Units to Millimeters (Metric)
G22	Not used	(MachineKit) Firmware Controlled Retract
G23	Not used	(MachineKit) Firmware Controlled Precharge
G24	Not used
G25	Not used
G26	Not used
G27	Reference Position Check
G28	Go To Predefined Position Through Point (G28)
G28.1	Set Predefined Position
G28.2	Not used	(TinyG) Homing Sequence.
G28.3	Not used	(TinyG) Set Absolute Axis to Defined Position
G29	Go to G29 Reference Point	(Marlin, MachineKit) Detailed Z-Probe
G29.1	Not used	(MachineKit) Set Z probe head offset
G29.2	Not used	(MachineKit) Set Z probe head offset calculated from toolhead position
G30	Go To Predefined Position Through Point (G30)	(Marlin, Smoothie, Reprap) Single Z-Probe
G30.1	Set Predefined Position
G31	Straight Probe Until Skip	(Marlin) Dock Z Probe Sled
G31	Straight Probe Until Skip	(Smoothie) Report Current Probe Status
G32	Thread Cutting	(Marlin) Undock Z Probe Sled
G32	Thread Cutting	(Smoothie) Probe Z and Calculate Z Plane
G33	Spindle Synchronized Motion
G33.1	Rigid Tapping
G34	Not used
G35	Automatic Tool Diameter Measurement
G36	Automatic Work Offset Measurement
G37	Automatic Tool Length Measurement
G38.2	Straight Probe To Workpiece, Report if failure
G38.3	Straight Probe To Workpiece
G38.4	Straight Probe Away From Workpiece, Report if failure
G38.5	Straight Probe Away From Workpiece
G39	Not used
G40	Cancel Cutter Compensation
G41	Start Cutter Radius Compensation Left
G41.1	Dynamic Cutter Compensation
G42	Start Cutter Radius Compensation Right
G42.1	Dynamic Cutter Compensation
G43	Tool Length Offset
G43	Tool Length Compensation, Positive
G43.1	Dynamic Tool Length Offset
G43.2	Apply additional Tool Length Offset
G44	Tool Length Compensation, Negative (Fanuc, Haas)
G49	Cancel Tool Length Compensation
G50	Reset Scale Factors to 1.0
G51	Set Axis Data Input Scale Factors
G52	Local Work Shift
G53	Motion In Machine Coordinate System
G54	Select Coordinate System 1
G55	Select Coordinate System 2
G56	Select Coordinate System 3
G57	Select Coordinate System 4
G58	Select Coordinate System 5
G59	Select Coordinate System 6
G59.1	Select Coordinate System 7
G59.2	Select Coordinate System 8
G59.3	Select Coordinate System 9
G60	Unidirectional Positioning
G61	Exact Path Mode
G61.1	Exact Stop Mode
G62	Automatic Corner Override
G63	Tapping Mode
G64	Continuous Mode
G65	Macro Subroutine Call
G68	Coordinate System Rotation
G69	Cancel Coordinate System Rotation
G70	Bolt Hole Circle
G71	Bolt Hole Arc
G72	Bolt Holes Along and Angle
G73	Drilling Cycle with Chip Breaking
G74	Reverse Tap Canned Cycle
G76	Multi-pass Threading Cycle
G77	Back Bore Canned Cycle
G80	Cancel Motion Mode
G81	Drilling Cycle
G82	Drilling Cycle with Dwell
G83	Drilling Cycle with Peck
G84	Tapping Canned Cycle
G85	Boring Cycle, No Dwell, Feed Out
G86	Boring Cycle, Stop, Rapid Out
G87	Bore/Manual Retract Canned Cycle
G88	Bore/Dwell Canned Cycle
G89	Boring Cycle, Dwell, Feed Out
G90	Absolute Distance Mode
G09.1	Absolute Arc Distance Mode
G91	Incremental Distance Mode
G91.1	Incremental Arc Distance Mode
G91.x	Reset Coordinate System Offsets
G92	Set Coordinate System Offsets
G92.1	Cancel Coordinate System Offsets
G92.2	Cancel Offset Coordinate Systems, Do Not Reset Parameters
G92.3	Apply Parameters to Offset Coordinate Systems
G93	Inverse Time Feed Rate Mode
G94	Units Per Minute Feed Rate Mode
G95	Units Per Revolution Feed Rate Mode
G96	Constant Surface Speed
G97	RPM Mode / Cancel Constant Surface Speed
G98	Initial Level Return In Canned Cycles
G99	R-point Level Return In Canned Cycles
G100+	Haas Gcodes continue from G100 to G188