Supported G and M Codes

This command summary serves as a guide for both new and experienced EIA-274D (G Codes) users. The following table lists the supported G and M codes for VisualCNC controller interface. Parameters within brackets ([ ]) are optional, the fields represented by "d.d" may be any decimal number and fields represented by "d" may be any positive integer number.

G00 [Xd.d] [Yd.d] [Zd.d]	High speed move (slew or rapid), modal
G01 [Xd.d] [Yd.d] [Zd.d] [Fd.d]	Linear move (feed or machine), modal
G02 [Xd.d] [Yd.d] [Zd.d] [Id.d] [Jd.d] [Kd.d] [Fd.d]	CW 2D circular move, modal
G03 [Xd.d] [Yd.d] [Zd.d] [Id.d] [Jd.d] [Kd.d] [Fd.d]	CCW 2D circular move, modal
G04 Pd.d	Dwell (seconds)
G17	Specify XY plane for helical & circular
G18	Specify XZ plane for helical & circular
G19	Specify YZ plane for helical & circular
G30	Cancel Mirror Image
G31	X Mirror
G32	Y Mirror
G37	Find home
G40	Cancel cutter compensation
G41	Cutter compensation left
G42	Cutter compensation right
G43 Hd	Sets tool length offset
G49	Cancel tool length offset
G54	Work Coordinate (Home or Fixture Offset) #1
G55	Work Coordinate (Home or Fixture Offset) #2
G56	Work Coordinate (Home or Fixture Offset) #3
G57	Work Coordinate (Home or Fixture Offset) #4
G58	Work Coordinate (Home or Fixture Offset) #5
G59	Work Coordinate (Home or Fixture Offset) #6
G62	Clear soft home
G70	Enter Inch Mode
G71	Enter Metric Mode
G80	Cancel Drilling Cycle
G81 Rd.d Zd.d [Fd.d]	Drill Cycle
G82 Rd.d Zd.d Pd [Fd.d]	Counter Bore Cycle
G83 Rd.d Zd.d Qd.d [Fd.d]	Peck drill
G85 Rd.d Zd.d [Fd.d]	Boring Cycle
G89 Rd.d Zd.d Pd [Fd.d]	Boring with pause
G90	Absolute coordinate mode
G91	Incremental coordinate mode
G92 [Xd.d] [Yd.d] [Zd.d]	Set soft home
Sd	Set spindle speed (rpm)
M00	Program pause
M01	Optional pause
M02 or M30	Program end
M03	Spindle on
M05	Spindle off
M06	Tool Change (example: T02 M06)
M08	Mist Coolant Device On
M09	Mist Coolant Device Off

The following table lists the letters used to denote various arguments.

( ) � Comments or Tool change operator message ex: (Text to be displayed)
Q - Peck drill delta (used in G83)
F - Feed rate (used in G00, G01, G02, G03, G81, G82, G83, G85, G89) Units per Minute
P - Dwell (used in G04)
I - Circular interpolation value in X dimension (used in G02, G03)
J - Circular interpolation value in Y dimension (used in G02, G03)
K - Circular interpolation value in Z dimension (used in G02, G03)
M - Miscellaneous function (control function)
N - Sequence number
R - Beginning Z motion dimension (used in G81, G82, G83, G85, G89)
S - Spindle rpm
T - Tool change (used in G00)
X - X motion dimension
Y - Y motion dimension
Z - Z motion dimension

Sample File 1 (Standard)

The following is a 10" square. Rapid level .5 inches above material, feed down 45 ipm, cut feed 150 ipm, rapid down to .1 above material, depth .25 inches. Surface or Z=0 is set at the surface of the material to be cut. This is for a single head system with no tool change.

G90	Absolute Coordinate Mode
G00 S18000 M03	Spindle Speed Set to 18,000 RPM's
G00 X0. Y0.	Position X=0.0 and Y=0.0
G00 Z0.1	Position the Z axis 0.1 inches above Z=0.0 or above the Material.
G01 Z-0.25 F45 M08	Position the Z axis 0.25 inches below Z=0.0 or into the Material at the feed rate of 45 inches/minute). The Auxiliary output for the selected tool is turned on. (This output can be wired to operate a tool misting or cooling unit.)
G01 X10. F150	Position the X=10.0 inches at the feed rate of 150 inches/minute
G01 Y10.	Position the Y=10.0 inches (feed rate will continue at last set speed)
G01 X0.	Position the X=0.0 inches
G01 Y0.	Position the Y=0.0 inches
G00 Z0.5 M09	Position the Z axis 0.5 inches above Z=0.0 or above the Material. The Auxiliary output for the selected tool is turned off. (This output can be wired to operate a tool misting or cooling unit.)
G00 X0. Y0.	Position X=0.0 and Y=0.0
M02	End of Program Spindle is turned off.

Sample File 2 (Automatic Tool Change)

The following is a 10" square. Rapid level .5 inches above material, feed down 45 ipm, cut feed 150 ipm, rapid down to .1 above material, depth .25 inches. Surface or Z=0 is set at the surface of the material to be cut. Additionally it calls a second tool to perform another cut of the same size elsewhere on the raw material. This is for a single head system with auto tool change.

G90	Absolute Coordinate Mode
G00 S18000 M03	Spindle Speed Set to 18,000 RPM's
G00 T1 M06 (E-MILL .250 2FLUTE)	Tool 1 call. Following moves will use tool one."E-MILL .250 2FLUTE" will displayed on the keypad.
G00 X0. Y0.	Position X=0.0 and Y=0.0
G00 Z0.1	Position the Z axis 0.1 inches above Z=0.0 or above the Material.
G01 Z-0.25 F45 M08	Position the Z axis 0.25 inches below Z=0.0 or into the Material at the feed rate of 45 inches/minute). The Auxiliary output for the selected tool is turned on. (This output can be wired to operate a tool misting or cooling unit.)
G01 X10. F150	Position the X=10.0 inches at the feed rate of 150 inches/minute
G01 Y10.	Position the Y=10.0 inches (feed rate will continue at last set speed)
G01 X0.	Position the X=0.0 inches
G01 Y0.	Position the Y=0.0 inches
G00 Z0.5 M09	Position the Z axis 0.5 inches above Z=0.0 or above the Material. The Auxiliary output for the selected tool is turned off. (This output can be wired to operate a tool misting or cooling unit.)
G00 T2 M06 (E-MILL .125 3FLUTE)	Tool 2 call. Following moves will use tool one."E-MILL .125 3FLUTE" will displayed on the keypad.
G00 X12. Y0.	Position X=12.0 and Y=0.0
G00 Z0.1	Position the Z axis 0.1 inches above Z=0.0 or above the Material.
G01 Z-0.25 F45 M08	Position the Z axis 0.25 inches below Z=0.0 or into the Material at the feed rate of 45 inches/minute). The Auxiliary output for the selected tool is turned on. (This output can be wired to operate a tool misting or cooling unit.)
G01 X22. F150	Position the X=22.0 inches at the feed rate of 150 inches/minute
G01 Y10.	Position the Y=10.0 inches (feed rate will continue at last set speed)
G01 X12.	Position the X=12.0 inches
G01 Y0.	Position the Y=0.0 inches
G00 Z0.5 M09	Position the Z axis 0.5 inches above Z=0.0 or above the Material. The Auxiliary output for the selected tool is turned off. (This output can be wired to operate a tool misting or cooling unit.)
G00 T0 M06	Optional command to put current away tool
G00 X0. Y0.	Position X=0.0 and Y=0.0
M02	End of Program Spindle is turned off.

Cutter Compensation G40\G41\G42

Note that all G41\G42 contours MUST start with a lead in and end with a lead out.

G90 G70	Absolute coordinate system, Inch Mode
S18000	Set spindle speed to 18000 RPM
G00 T1 M06 (.250 End Mill)	Select Tool #1 and display �.250 End Mill�
G00 Z-0.5	Rapid move to safe rapid level
G00 X0. Y-0.25	Rapid move
Z.1	Compensation entry move
G41 D01	Turn on left tool compensation for table entry #1
Y0
G01 Z-.250 F30 M08	Feed Z to -.25 at 30ipm and turn on tool mist
Y10 F200	Feed to Y=10 at 200 ipm
X10	Feed move
Y0	Feed move
X0	Feed move
G40	Turn tool compensation off
G0 Z.5 M09	Rapid Z=.5 and turn mist off
X -.2	Exit tool compensation move
M02	End of file

G81 / G83 Drilling, Peck Drilling

G90 G70	absolute coordinate system, inch mode
S12000	set spindle speed to 12000 RPM
G00 X0Y0	Rapid move
G00 Z.1 M08	rapid Z move (note Z positive is UP), turn misting unit on
G81 Z-.2 F50	Drill cycle next coordinates to Z=-.2 at 50 ipm
X1Y1	Drill
X2	Drill
X3	Drill
G80	Drill cycle off
G00 Z1.	Rapid Move
X0Y2	Rapid Move
G83 R.1 Z-.5 Q.1 F30	Peck drill cycle next coordinates to Z=-.5 at .1 lift, .1 peck, 30 ipm
X1	Peck drill
X2	Peck Drill
X3	Peck Drill
M09	Mist Unit Off
G80	Cancel Drill Cycle
G00 Z-0.5	Rapid Z move
G00 X0. Y0.	rapid XY move
M02	End of Job

MISCELLANEOUS

It is not uncommon that some software packages do NOT support all g-codes. For example the codes involved with cutter compensation. Be sure to check the documentation of your software.
Line numbers are optional, they have no effect on program execution.
Decimal points for whole numbers are optional, they are only necessary for fractional numbers
Drilling with an electric/pneumatic feed drill is accomplished by calling Tool 31�40 (T31 M06) with standard G00 rapid moves immediately after the tool call to position the drill. At the end of the rapid move the drill will be fed into the material. The next rapid will produce the same results. To stop drilling call another tool (T01 M06)
Peck drilling and standard drilling cycles (G80,81,83) are not supported on electric/pneumatic feed drills.
Depending on features purchased with any particular machine, all or a portion of the G&M codes are supported.

HOME TABLE GCODES TOOLS LINKS