-
Notifications
You must be signed in to change notification settings - Fork 295
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
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 |
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 |
Getting Started Pages
- Home
- What is g2core?
- Who uses g2core?
- Jerk-Controlled Motion
- Getting Started with g2core
- Connecting to g2core
- Configuring g2core
- Flashing g2core
- Troubleshooting
Reference Pages
- Gcodes
- Mcodes
- Text Mode
- JSON Communications
- GPIO Digital IO
- Alarms & Exceptions
- Power Management
- Coordinate Systems
- Status Reports
- Status Codes
- G2 Communications
- Tool Offsets and Selection
- Probing
- Feedhold, Resume, Job Kill
- Marlin Compatibility
- 9 Axis UVW Operation
- gQuintic Specs
Discussion Topics
- Roadmap
- GPIO for 1.X Releases
- Toolheads
- Raster Streaming Prototol
- g2core REST Interface
- Gcode Parsing
- G2 3DP Dialect
- Consensus Gcode
- Digital DRO
- Overview of Motion Processing
Developer Pages
- Development & Contribution
- Branching and Release - DRAFT
- Getting Started with g2core Development
- Project Structure & Motate
- Compiling G2
- OSX w/Xcode
- OSX/Linux Command Line
- Windows10 w/AtmelStudio7
- Debugging G2 on OSX
- Board and Machine Profiles
- Arduino Due Pinout
- Arduino DUE External Interfaces
- Diagnostics
- Debugging w/Motate Pins
- Development Troubleshooting
- g2core Communications
- Git Procedures
- Windows 10 / VMware 8 Issues
- Dual Endpoint USB Internals
- G2core License
- VSCode Setup
- Compatibility Axioms
- Wiki History