CNCCookbook  Software and Information for Machinists

GW Editor User Guide

GWE Home

Getting Started

Setup

Commands

Keyboard

Revisions

CNC Simulator

Wizards

Tool Data

Tips

Post List

Customizing Posts

 

GW Conversational CNC

 

Mill G-Codes

Lathe G-Codes

 

Sample G-Code Files

 

GWE Tips

 

GWE Change Log

GWE Install

 

Troubleshooting

 

User's Club

Bookmark and Share

G-Code and M-Code Reference for Milling

These are the common g-codes and m-codes for milling that G-Wizard Editor supports for Mills. Code categories are the groupings for the g-code Wizard (type Ctrl+G for the Wizard). Function tells what the g-code does, Notes gives a little more information such as the parameters, and Tutorial is a link (if any) to a tutorial from our Online G-Code Tutorial that uses G-Wizard Editor to teach how to program the g-code.

 
Code
Category
Function

Notes

Tutorials
 
  G00
Motion
Move in a straight line at rapids speed. XYZ of endpoint

G00 and MDI.

Linear Motion: G00 and G01

 
  G01
Motion
Move in a straight line at last speed commanded by a (F)eedrate XYZ of endpoint

G01 and MDI.

Linear Motion: G00 and G01

 
  G02
Motion
Clockwise circular arc at (F)eedrate

XYZ of endpoint

IJK relative to center

R for radius

G02 / G03 Tutorial and Examples  
  G03
Motion
Counter-clockwise circular arc at (F)eedrate

XYZ of endpoint

IJK relative to center

R for radius

G02 / G03 Tutorial and Examples  
  G04
Motion
Dwell: Stop for a specified time.

P for milliseconds

X for seconds

Precise Timing and Speed: Dwell, Exact Stop, Backlash Compensation  
  G09
Motion
Exact stop check   Precise Timing and Speed: Dwell, Exact Stop, Backlash Compensation  
  G10
Compensation
Programmable parameter input      
  G15
Coordinate
Turn Polar Coordinates OFF, return to Cartesian Coordinates   G15/G16 Polar Coordinates  
  G16
Coordinate
Turn Polar Coordinates ON   G15/G16 Polar Coordinates  
  G17
Coordinate
Select X-Y plane   CNC G-Code Coordinates  
  G18
Coordinate
Select X-Z plane   CNC G-Code Coordinates  
  G19
Coordinate
Select Y-Z plane   CNC G-Code Coordinates  
  G20
Coordinate
Program coordinates are inches   G20 and G21: Unit Conversion  
  G21
Coordinate
Program coordinates are mm   G20 and G21: Unit Conversion  
  G27
Motion
Reference point return check   G28: Return to Reference Point  
  G28
Motion
Return to home position   G28: Return to Reference Point  
  G29
Motion
Return from the reference position   G28: Return to Reference Point  
  G30
Motion
Return to the 2nd, 3rd, and 4th reference point   G28: Return to Reference Point  
  G32
Canned
Constant lead threading (like G01 synchronized with spindle)      
  G40
Compensation
Tool cutter compensation off (radius comp.)      
  G41
Compensation
Tool cutter compensation left (radius comp.)      
  G42
Compensation
Tool cutter compensation right (radius comp.)      
  G43
Compensation
Apply tool length compensation (plus)      
  G44
Compensation
Apply tool length compensation (minus)      
  G49
Compensation
Tool length compensation cancel      
  G50
Compensation
Reset all scale factors to 1.0      
  G51
Compensation
Turn on scale factors      
  G52
Coordinate
Local workshift for all coordinate systems: add XYZ offsets      
  G53
Coordinate
Machine coordinate system (cancel work offsets)      
  G54
Coordinate
Work coordinate system (1st Workpiece)      
  G55
Coordinate
Work coordinate system (2nd Workpiece)      
  G56
Coordinate
Work coordinate system (3rd Workpiece)      
  G57
Coordinate
Work coordinate system (4th Workpiece)      
  G58
Coordinate
Work coordinate system (5th Workpiece)      
  G59
Coordinate
Work coordinate system (6th Workpiece)      
  G61
Other
Exact stop check mode   Precise Timing and Speed: Dwell, Exact Stop, Backlash Compensation  
  G62
Other
Automatic corner override      
  G63
Other
Tapping mode      
  G64
Other
Best speed path      
  G65
Other
Custom macro simple call   Subprograms and Macros  
  G68
Coordinate
Coordinate System Rotation   G68 and G69 Tutorial and Examples  
  G69
Coordinate
Cancel Coordinate System Rotation   G68 and G69 Tutorial and Examples  
  G73
Canned
High speed drilling cycle (small retract)      
  G74
Canned
Left hand tapping cycle      
  G76
Canned
Fine boring cyle      
  G80
Canned
Cancel canned cycle      
  G81
Canned
Simple drilling cycle      
  G82
Canned
Drilling cycle with dwell (counterboring)      
  G83
Canned
Peck drilling cycle (full retract)      
  G84
Canned
Tapping cycle      
  G85
Canned
Boring canned cycle, no dwell, feed out      
  G86
Canned
Boring canned cycle, spindle stop, rapid out      
  G87
Canned
Back boring canned cycle      
  G88
Canned
Boring canned cycle, spindle stop, manual out      
  G89
Canned
Boring canned cycle, dwell, feed out      
  G90
Coordinate
Absolute programming of XYZ (type B and C systems)      
  G90.1
Coordinate
Absolute programming IJK (type B and C systems)      
  G91
Coordinate
Incremental programming of XYZ (type B and C systems)      
  G91.1
Coordinate
Incremental programming IJK (type B and C systems)      
  G92
Coordinate
Offset coordinate system and save parameters      
  G92 (alternate)
Motion
Clamp of maximum spindle speed S    
  G92.1
Coordinate
Cancel offset and zero parameters      
  G92.2
Coordinate
Cancel offset and retain parameters      
  G92.3
Coordinate
Offset coordinate system with saved parameters      
  G94
Motion
Units per minute feed mode. Units in inches or mm.      
  G95
Motion
Units per revolution feed mode. Units in inches or mm.      
  G96
Motion
Constant surface speed   G96: Constant Surface Speed  
  G97
Motion
Cancel constant surface speed   G96: Constant Surface Speed  
  G98
Canned
Return to initial Z plane after canned cycle      
  G99
Canned
Return to initial R plane after canned cycle      
   
       
 
M-Codes
 
Code
Category
Function

Notes

Tutorials
 
  M00
M-Code
Program Stop (non-optional)      
  M01
M-Code
Optional Stop: Operator Selected to Enable      
  M02
M-Code
End of Program      
  M03
M-Code
Spindle ON (CW Rotation)   M03 and MDI.  
  M04
M-Code
Spindle ON (CCW Rotation)      
  M05
M-Code
Spindle Stop   M05 and MDI.  
  M06
M-Code
Tool Change      
  M07
M-Code
Mist Coolant ON   M07 and MDI.  
  M08
M-Code
Flood Coolant ON   M08 and MDI.  
  M09
M-Code
Coolant OFF   M09 and MDI.  
   
       
  M30
M-Code
End of Program, Rewind and Reset Modes      
   
       
  M97
M-Code
Haas-Style Subprogram Call   Subprograms and Macros  
  M98
M-Code
Subprogram Call   Subprograms and Macros  
  M99
M-Code
Return from Subprogram   Subprograms and Macros  

 

 

Home      

 

Software

  GW Calculator

  GW Editor

  Gearotic

  Conversational

Blog

  Software

  Techniques

  Beginner

  Cool

  Projects

 

 

Cookbooks

     Feeds and Speeds

     G-Code Tutorial

     CNC Machining & Manufacturing

     CNC Beginner Articles

     CNC Dictionary

CNC Projects

Machines

     CNC Mill Retrofit

     Plasma Table

     Welding

     

Resources

     Machinist's Search

     Videos

     Online Groups

     Individuals

     Reference Data

     Books

     Suppliers

     Tool Brands

Workshop

     Hall of Fame

 

About

     Support

     Customers

     Partners

     Our History

     Cheapskate Page

     Privacy Policy

 
All material © 2010-2012, CNCCookbook, Inc.