1. G & M Codes Computer Integrated Manufacturing
© 2013 Project Lead The Way, Inc.

2. What Are G & M Codes? Operate CNC machines
Computer Integrated Manufacturing™
Product Development
What Are G & M Codes?
Operate CNC machines
Began in the form of punch tape
Developed into computer chips in the 1970s
CNC means Computer Numerical Control, where electronic systems are used to perform machine movements.
Project Lead The Way, Inc.
Copyright 2008

3. G & M Today Translates human language to machine language
G & M Codes
Computer Integrated Manufacturing™
Product Development
G & M Today
Translates human language to machine language
Typed into computer or generated by a program
The CNC is moved by a program and is usually written in G & M Codes. Just like any computer-driven mechanism, a CNC communicates using its own language. In order to communicate with the CNC, we must convert our language (turn this, move here) into one that the CNC will comprehend.
Project Lead The Way, Inc.
Copyright 2008

4. Sample Program Block N1 M06 T1 ; Change to tool #1 Comment
G & M Codes
Computer Integrated Manufacturing™
Product Development
Sample Program Block
N1 M06 T1 ; Change to tool #1
Comment
Comment separator
Two types of instructions exist:
Those which define the tool path (such as X and Y axis coordinates).
Those which specify machine operations (such as turning the spindle on or off).
X, Y, and Z are used to define the X, Y, and Z coordinates for the destination when cutting in a straight-line.
I, J, and K are used to communicate to the tool the X, Y and Z coordinates of the center point of an arc (for circular interpolation). In absolute programming, I words represent the X coordinate, J words represent the Y coordinate, and K words represent the Z coordinate.
In incremental programming, the I, J, and K words specify the distance from the start point to the center point of the arc.
F is measured in inches per minute.
S is measured in revolutions per minute (RPM).
Comments must be made on the same line of programming as the semicolon.
Tool Number
Miscellaneous code: Tool change
Block Sequence #
Project Lead The Way, Inc.
Copyright 2008

5. Sample Program Block N02 M03 S1500 Spindle Speed: 1500 rpm
G & M Codes
Computer Integrated Manufacturing™
Product Development
Sample Program Block
N02 M03 S1500
Spindle Speed: 1500 rpm
Two types of instructions exist:
Those which define the tool path (such as X and Y axis coordinates).
Those which specify machine operations (such as turning the spindle on or off).
X, Y, and Z are used to define the X, Y, and Z coordinates for the destination when cutting in a straight-line.
I, J, and K are used to communicate to the tool the X, Y and Z coordinates of the center point of an arc (for circular interpolation). In absolute programming, I words represent the X coordinate, J words represent the Y coordinate, and K words represent the Z coordinate.
In incremental programming, the I, J, and K words specify the distance from the start point to the center point of the arc.
F is measured in inches per minute.
S is measured in revolutions per minute (RPM).
Comments must be made on the same line of programming as the semicolon.
Miscellaneous code: Turn spindle on
Line Number
Project Lead The Way, Inc.
Copyright 2008

6. Sample Program Block N03 G90 G01 X.5 Y.5 Z0 F1 Feed Rate (in./min)
G & M Codes
Computer Integrated Manufacturing™
Product Development
Sample Program Block
N03 G90 G01 X.5 Y.5 Z0 F1
Feed Rate (in./min)
Z Coordinate
Y Coordinate
X Coordinate
Two types of instructions exist:
Those which define the tool path (such as X and Y axis coordinates).
Those which specify machine operations (such as turning the spindle on or off).
X, Y, and Z are used to define the X, Y, and Z coordinates for the destination when cutting in a straight-line.
I, J, and K are used to communicate to the tool the X, Y and Z coordinates of the center point of an arc (for circular interpolation). In absolute programming, I words represent the X coordinate, J words represent the Y coordinate, and K words represent the Z coordinate.
In incremental programming, the I, J, and K words specify the distance from the start point to the center point of the arc.
F is measured in inches per minute.
S is measured in revolutions per minute (RPM).
Comments must be made on the same line of programming as the semicolon.
Prep Code – SL Interpol
Prep Code – Absolute
Line Number
Project Lead The Way, Inc.
Copyright 2008

7. G & M Codes
CIM
Product Development
More Terminology
Address Character – A letter used in G & M code programming to designate a class of functions
Parameter – Attribute of a feature, such as a dimension, that can be modified
N00 G90 G01 X.5 Y.5 Z0 F1
Before we can look at an example, we need to learn the basic terminology associated with G & M codes.
Project Lead The Way, Inc.
Copyright 2010

8. G & M Codes
Computer Integrated Manufacturing™
Product Development
Terminology
Word – The programming expression formed when a letter (address) is combined with a number
Block – A single line of code in an NC part program
N00 G90 G01 X.5 Y.5 Z0 F1
Before we can look at an example, we need to learn the basic terminology associated with G & M codes.
Project Lead The Way, Inc.
Copyright 2008

9. G Codes – Preparatory G90 Absolute Coordinates
G & M Codes
Computer Integrated Manufacturing™
Product Development
G Codes – Preparatory
G90 Absolute Coordinates
G91 Relative Coordinates
G00 Rapid Traverse (non-cutting move)
G01 Straight Line Interpolation (cutting move)
G02 Circular Interpolation (clockwise)
G03 Circular Interpolation (c-clockwise)
G04 Dwell (wait) – Pause measured in seconds on all
axes between motions (i.e., G04F2.3 is a pause for 2.3 s)
G05 Pause – Wait for user intervention
G codes are preparatory functions that involve actual tool movements that control the machine. These include rapid moves, linear feed moves, radial feed moves, etc. Most G codes are modal, meaning that they remain active until canceled by another G-code.
The format of the G04 command can be found in a different format where P is used instead of F (i.e., G04P2.3 is a pause for 2.3 s).
Project Lead The Way, Inc.
Copyright 2008

10. G Codes – Arcs
Method 1: Arc with I & J ( I & J are center point coordinates )
X1Y2
I1J1
Absolute coordinates
Example
N0 G90 ; Absolute coord
N5 G01 X1 Y2 ; start
N10 G02 X2 Y1 I1 J1
X2Y1
X1Y-1
X1Y2
I0 J-1
Relative coordinates
Example
N0 G91; Relative coord
N05 G01 X1 Y2 ; start
N10 G02 X1 Y-1 I0 J-1

11. G Codes – Arcs Method 2: Arc with R (R is arc radius)
Absolute coordinates
Example
N0 G90 ; Absolute coord
N5 G01 X1 Y2 ; start
N10 G02 X2 Y1 R1
X2Y1
X1Y2 R1
X1Y-1
X1Y2 R1
Relative coordinates
Example
N0 G91; Relative coord
N05 G01 X1 Y2 ; start
N10 G02 X1 Y-1 R1

12. Other Common G Codes G20 Inch programming units
G21 Millimeter programming units
G80 Canned cycle cancel
G81 Drilling cycle
G82 Drilling cycle with dwell

13. M Codes – Miscellaneous
G & M Codes
Computer Integrated Manufacturing™
Product Development
M Codes – Miscellaneous
M00 Pause
M01 Optional stop
M02 End of program
M03 Spindle on
M05 Spindle off
M06 Tool change
M08 / M09 Accessory # 1 on / off
M10 / M11 Accessory # 2 on / off
M30 Program end and reset
M47 Rewind (used for handshaking operations)
M codes are miscellaneous functions that include actions necessary for machining but are not actual tool movements. They are auxiliary functions, such as spindle on or off, tool changes, coolant on or off, and program stops.
Project Lead The Way, Inc.
Copyright 2008

14. Code Suggestions Same code not required to be repeated every block
G & M Codes
Computer Integrated Manufacturing™
Product Development
Code Suggestions
Same code not required to be repeated every block
Machine will use same code until changed
Called modal
Tab remarks away from code to facilitate troubleshooting program
Specify absolute or relative coordinates and inch or metric modes at beginning of program
Always use a tool change command to move tool to safe position away from material; change tool if necessary
Indicate spindle speed each time turned on
Project Lead The Way, Inc.
Copyright 2008

15. Code Suggestions Move tool to start position in two lines
First line moves in X-Y plane, then moves in Z axis
Prevents ramping or inadvertently cutting a part
Raise tool out of the stock at end of program
Always move table to safe unload position and turn spindle off at end of program
Use M02 command to end program

16. Sample Part – Absolute Absolute Coordinates Origin G & M Codes
Computer Integrated Manufacturing™
Product Development
Sample Part – Absolute
Absolute
Coordinates
Origin
In this example, you will notice that each line represents a quarter inch.
Project Lead The Way, Inc.
Copyright 2008

17. Sample Program Absolute
G & M Codes
Computer Integrated Manufacturing™
Product Development
Sample Program Absolute
N1 G90 G20 ; ABSOLUTE COORD & INCH MODE
N2 M06 T1 ; TOOL CHANGE – LOAD TOOL 1
N3 M03 S3000 ; TURN SPINDLE ON CW TO 3000 RPM
N4 G00 X.5 Y.5 ; RAPID TO POINT A
N5 G00 Z.1 ; RAPID TO .1 ABOVE PART
N6 G01 Z F9 ; PLUNGE 1/16 AT 9 IN./MIN
N7 G01 X.5 Y1.5 F18 ; STRAIGHT LINE INTERP TO B
N8 G01 X.875 Y1 ; STRAIGNT LINE INTERP TO C
N9 G01 X1.25 Y1.5 ; STRAIGHT LINE INTERP TO D
N10 G01 X1.25 Y.5 ; STRAIGHT LINE INTERP TO E
Characters following a semicolon are ignored by the machine. This space is used to add comments to the code. Comments are important in any programming to document the purpose of a line for the original programmer or for another person working with the program.
Project Lead The Way, Inc.
Copyright 2008

18. Sample Program Absolute
G & M Codes
Computer Integrated Manufacturing™
Product Development
Sample Program Absolute
N11 G01 Z.1 ; RETRACT CUTTING TOOL
N12 G00 X1.75 Y1.5 ; RAPID TO POINT F
N13 G01 Z F9 ; PLUNGE AT 9 IN./MIN
N14 G01 X1.75 Y.5 F18 ; STRAIGHT LINE INTERP TO H
N15 G03 X1.75 Y1.5 I1.75 J1 ; CCW CIRCLE INTERP
N16 G01 Z.1 ; RETRACT CUTTING TOOL
N17 M05 ; TURN OFF SPINDLE
N18 G00 Z2 ; RAPID Z TO SAFE POSITION
N19 G00 X4 Y3 ; MOVE TABLE TO UNLOAD POSITION
N20 M02 ; END OF PROGRAM
Project Lead The Way, Inc.
Copyright 2008

19. Sample Part – Incremental
G & M Codes
Computer Integrated Manufacturing™
Product Development
Sample Part – Incremental
Incremental
Coordinates
Origin
In this example, you will notice that each line represents a quarter inch.
Project Lead The Way, Inc.
Copyright 2008

20. Sample Program Incremental / Relative
G & M Codes
Computer Integrated Manufacturing™
Product Development
Sample Program Incremental / Relative
N1 G90 G20   ; ABSOLUTE COORD & INCH MODE
N2 M06 T1   ; TOOL CHANGE – LOAD TOOL 1
N3 M03 S3000 ; TURN SPINDLE ON CW TO 3000 RPM
N4 G00 X.5 Y.5  ; RAPID TO POINT A
N5 G00 Z.1  ; RAPID TO .1 ABOVE POINT A
N6 G91  ; INCREMENTAL COORD & INCH MODE
N7 G01 Z F9 ; PLUNGE 1/16 AT 9 IN./MIN
N8 G01 X0 Y1 F16 ; STRAIGHT LINE INTERP TO B
N9 G01 X.375 Y-.5 ; STRAIGHT LINE INTERP TO C
N10 G01 X.375 Y.5 ; STRAIGHT LINE INTERP TO D
N11 G01 X0 Y-1 ; STRAIGHT LINE INTERP TO E
Characters following a semicolon are ignored by the machine. This space is used to add comments to the code. Comments are important in any programming to document the purpose of a line for the original programmer or for another person working with the program.
Project Lead The Way, Inc.
Copyright 2008

21. Sample Program Incremental / Relative
G & M Codes
Computer Integrated Manufacturing™
Product Development
Sample Program Incremental / Relative
N12 G01 Z ; RETRACT CUTTING TOOL
N13 G00 X.5 Y1 ; RAPID TO POINT F
N14 G01 Z F9 ; PLUNGE AT 9 IN./MIN
N15 G01 X0 Y-1 F16 ; STRAIGHT LINE INTERP TO H
N16 G03 X0 Y1 I0 J.5 ; CCW CIRCLE INTERP
N17 G01 Z ; RETRACT CUTTING TOOL
N18 M05 ; TURN OFF SPINDLE
N19 G90 ; CHANGE TO ABSOLUTE COORD
N20 G00 Z2 ; RAPID Z TO SAFE POSITION
N21 G00 X4 Y3 ; MOVE TABLE TO UNLOAD POSITION
N22 M02 ; END OF PROGRAM
Project Lead The Way, Inc.
Copyright 2008

22. Your Turn
What line in the last example uses the arc command? N16 Change the arc command in the last example into the format with R (radius). N16 G03 X0 Y1 R.5 ; CCW CIRCLE INTERP See next slide for change in program.

23. Solution N12 G01 Z.1625 ; RETRACT CUTTING TOOL
G & M Codes
Computer Integrated Manufacturing™
Product Development
Solution
N12 G01 Z ; RETRACT CUTTING TOOL
N13 G00 X.5 Y1 ; RAPID TO POINT F
N14 G01 Z F9 ; PLUNGE AT 9 IN./MIN
N15 G01 X0 Y-1 F16 ; STRAIGHT LINE INTERP TO H
N16 G03 X0 Y1 R.5 ; CCW CIRCLE INTERP
N17 G01 Z ; RETRACT CUTTING TOOL
N18 M05 ; TURN OFF SPINDLE
N19 G90 ; CHANGE TO ABSOLUTE COORD
N20 G00 Z2 ; RAPID Z TO SAFE POSITION
N21 G00 X4 Y3 ; MOVE TABLE TO UNLOAD POSITION
N22 M02 ; END OF PROGRAM
Project Lead The Way, Inc.
Copyright 2008

24. Explain the Code N2 G1 X2.5 Y3 F2 N2G1X2.5Y3F2 Block two
G & M Codes
Computer Integrated Manufacturing™
Product Development
Explain the Code
N2G1X2.5Y3F2
N2 G1 X2.5 Y3 F2
Block two
Linear interpolation
2.5 on the X axis
3 on the Y axis
Explain each word in the code.
Feed rate = 2 IPM
Project Lead The Way, Inc.
Copyright 2008

25. What’s Wrong with These?
G & M Codes
Computer Integrated Manufacturing™
Product Development
What’s Wrong with These?
N1G01G90X2X2;
N1G00G01X2Y2;
N3G01X.5Y2F1;
N4G01X.5Y3.5F1;
Changing N6G00X0.500Y1.500; to N6G0X.5Y1.5;
Changing N2G90Z0.05M00; to N2G9Z.5M;
This example includes two X codes. The use of two G codes, however, is correct, because one G code is from the Interpolation Group and the other is from the Programming Mode Group.
This example uses two G codes from the same group.
This example is not really wrong, it is just unnecessary. You do not have to repeat the feed rate, linear interpolation, and X value code in the line N4 because they remain the same.
There is nothing wrong with this example. It is OK to take out extra zeroes.
There is no such thing as a G9; the Z value has changed from .05 to .5, and the M address character has been left without a parameter.
Project Lead The Way, Inc.
Copyright 2008

26. References
Mattson, M. (2010). CNC programming principles and applications. Oregon City, OR: Delmar.