M-Code/G-Code List

M Code/G Code List

Below you will find a list of common codes many builders use. Please remember, all machines may be configured differently and the list below may not match your machine perfectly. If fact, virtually all M-Codes above M79 will vary from builder to builder. Please make sure to contact your machine tool builder to be sure.

Typical G Command for a Machining Center

• (G – Codes are written by Fanuc)
• G00 Moves the tool in rapid travel (not necessarily a straight line)
• G01 Moves the tool using a set feedrate
• G02 Moves the tool along a clockwise arc path
• G03 Moves the tool along a counter-clockwise path
• G04 Sets a dwell time in seconds or revolutions of the spindle
• G10 Data setting
• G11 Data setting mode cancel
• G17 Establishes axis movement in the X and Y axis planes
• G18 Establishes axis movement in the X and Z axis planes
• G19 Establishes axis movement in the Y and Z axis planes
• G20 Values are in Inches
• G21 Values are in millimeters
• G28 Return to reference position
• G30 Second reference position
• G33 Thread cutting
• G40 Cancel cutter compensation
• G41 Cutter compensation left
• G42 Cutter compensation right
• G43 Tool length compensation positive
• G44 Tool length compensation negative
• G49 Tool length compensation cancel
• G53 Machine Coordinate move
• G54 Use workshift offset #1
• G55 Use workshift offset #2
• G56 Use workshift offset #3
• G57 Use workshift offset #4
• G58 Use workshift offset #5
• G59 Use workshift offset #6
• G60 Single direction positioning
• G65 Macro call
• G66 Macro modal call
• G67 Macro modal call cancel
• G73 Peck drilling cycle
• G76 Fine boring cycle
• G80 Canned cycle cancel
• G81 Drilling cycle or spot boring cycle
• G82 Drilling cycle or counter boring cycle
• G83 Peck drilling cycle
• G84 Tapping cycle
• G85 Boring cycle
• G86 Boring cycle
• G87 Back boring cycle
• G88 Boring cycle
• G89 Boring cycle
• G90 Absolute measurements
• G91 Incremental measurements
• G94 Feed per minute
• G95 Feed per revolution of the spindle
• G96 Constant surface speed control
• G97 Constant surface speed control cancel
• G98 Return to initial point in canned cycle
• G99 Return to R point is canned cycle

Typical M Commands for a Machining Center

• M00 Program stop
• M01 Optional stop
• M02 End of program
• M03 Spindle on Clockwise
• M04 Spindle on Counter-clockwise
• M05 Spindle stop
• M06 Tool change
• M08 Coolant on
• M09 Coolant off
• M10 Clamp
• M11 Unclamp
• M30 End of program and rewind to beginning of program
• M98 Call subprogram
• M99 End subprogram

Typical MDI Commands

M06 T12; Performs a tool change to tool number 12
S1000 M03; Turns spindle on clockwise to 1000 rpm
G01 X10.5 F10.0: Moves the X axis to position 10.5 at a feedrate of 10.0

G00 X……. Y…….. Z…….. ;
G00 Move in rapid travel
X….. X axis address
Y….. Y axis address
Z….. Z axis address

G01 X……. Y…….. Z…….. F……. ;
G01 Move in a straight line
X….. X axis address
Y….. Y axis address
Z….. Z axis address
F….. Feedrate

G02 X……. Y…….. Z…….. I……. J…….. K…….. F……. ;
G02 Move along a clockwise circular path
X….. X axis address
Y….. Y axis address
Z….. Z axis address
I ….. I axis address
J….. J axis address
K….. K axis address
F….. Feedrate

G03 X……. Y…….. Z…….. I……. J…….. K…….. F……. ;
G03 Move along a counter-clockwise circular path
X….. X axis address
Y….. Y axis address
Z….. Z axis address
I ….. I axis address
J….. J axis addressK….. K axis address
F….. Feedrate

G04 X….… ;
G04 Pause machine operation
X….… ( Specify a time/spindle speed with decimal point)

G04 P….… ; ( Specify a time without decimal point)
G04 Pause machine operation
P….… ( Specify a time/spindle speed without decimal point)

G28 G90 X10.0 Y3.0 ;
G28 Return to reference point
G90 Absolute positioning
X10.0 X axis location
Y3.0 Y axis location

This command sequence can be used to move the tool from point A to an
ABSOLUTE Coordinate first, then move the tool to the Reference Point Zero.
G28 G91 X-4.0 Y-3.0 ;
G28 Return to reference point
G91 Incremental positioning
X-4.0 X axis location
Y-3.0 Y axis location

This command sequence can be used to make an incremental move from point A
then move the tool to the Reference Point Zero
G28 G91 X0.0 Y0.0 ;
This line will take the tool back to the reference position direct from the current
location.
G41 D…. X …… ;
G41 Cutter Comp Left
D….. Assigns Radius Offset number
X…. X axis movement

G42 D….… X …… ;
G42 Cutter Comp Right
D….. Assigns Radius Offset number
X…. X axis movement

G40 X….. ;
G40 Cancel Cutter Comp
X….. Cancels comp on way to Here

G43 H…. Z …… ;
G43 Add offset amount
H….. Offset number
Z…. Z axis movement

G44 H… Z …… ;
G44 Subtract offset amount
H….. Offset number
Z…. Z axis movement

G49 H….. Z…… ;
G49 Cancel Offset
H13 Assigns Offset Number 13
Z0.0 Z axis movement to Zero

G65 P……. L…….. ;
G65 Macro call (Modal)
P….. Macro program Number
L….. Number of repetitions

G66 P……. ;
G66 Macro call (Non-Modal)
P….. Macro program Number

G73 X……. Y…….. Z…….. R……. Q…….. F…….. K……. ;
G73 High speed peck drilling cycle
X….. X axis address
Y….. Y axis address
Z….. Z address location of bottom of hole
R ….. Retract plane
Q….. Distance for each peck stroke
F….. Feedrate
K….. Number of repeats

G74 X……. Y…….. Z…….. R……. P…….. F…….. K……. ;
G74 Left handed tapping cycle
X….. X axis address
Y….. Y axis address
Z….. Z address location of bottom of hole
R …. Retract plane
F….. Feedrate
K….. Number of repeats

G76 X……. Y…….. Z…….. R……. Q…….. P…….. F…….. K……. ;
G76 Fine boring cycle
X….. X axis address
Y….. Y axis address
Z….. Z address location of bottom of hole
R ….. Retract plane
Q….. Distance for each peck stroke
P….. Dwell time at bottom of bore
F….. Feedrate
K….. Number of repeats

G81 X……. Y…….. Z…….. R……. F…….. K……. ;
G81 Spot drilling cycle
X….. X axis address
Y….. Y axis address
Z….. Z address location of bottom of hole
R ….. Retract plane
F….. Feedrate
K….. Number of repeats

G82 X……. Y…….. Z…….. R……. P…….. F…….. K……. ;
G82 Drilling cycle counter boring cycle
X….. X axis address
Y….. Y axis address
Z….. Z address location of bottom of hole
R ….. Retract plane
P….. Dwell time at bottom of bore
F….. Feedrate
K….. Number of repeats

G83 X……. Y…….. Z…….. R……. Q…….. F…….. K……. ;
G83 Peck drilling cycle
X….. X axis address
Y….. Y axis address
Z….. Z address location of bottom of hole
R ….. Retract plane
Q….. Distance for each peck stroke
F….. Feedrate
K….. Number of repeats