Regardless of manufacturer, control, software, or off-line (CAM) programming system, nearly all CNC machines use preparatory (G) and miscellaneous function (M) codes, and a combination of defining parameters, to execute the operations required to produce parts. Most G codes direct the motion of the machine in some manner, while M codes control anciallary functions such as spindle on / off, coolant on / off, tool changes, etc. It is not essential for the engineering student to memorize these commands, as you would expect of the machinist or CNC programmer, but listing the more commonly used codes here, will allow an engineer, utilizing a CAM software package off-line, to understand the relationship to the executed machine codes.

Common (Mill & Lathe) G-Codes

Feed Move Group

*G00 Rapid linear move. [X,Y,Z] Moves the machine at the fastest rate possible to the X,Y,Z location specified

*G01 Linear feed move [X,Y,Z,F] Moves the machine a the specified feed rate (F) to the X,Y,Z location specified

*G02 Circular feed move; CW [X,Y,Z,F,R (or I,J,K)] Moves the machine, in a clockwise circular path to the X,Y,Z, location specified with radius R, or with a center point defined relative to the start point in the X,Y,& Z axis by I, J,& K respectively.

*G03 Circular feed move; CCW [X,Y,Z,F,R (or I,J,K)] Same as G02, but opposite direction of movement.

_________________________________

G04 Dwell (P) Causes the machine to pause for a period determined by parameter P. If P<value> has a decimal point, the dwell is x.x seconds; otherwise dwell is in milliseconds.

G28 Return to machine home. Causes the machine to return to it’s X0,Y0,Z0 position at a rapid rate.

_________________________________

Coordinate System Group

*G53 Machine coordinate system (MCS). Cancels G-54 thru G59

*G54-G59 Work coordinate offsets. Allows the user to establish one or more alternative coordinate systems to correspond to individual work coordinate systems (WCS)

_________________________________

Units Group

*G70 Inch Programming (This facility uses inch programming unless otherwise stated)

*G71 Metric Programming

_________________________________

Common Canned Cycles (See Canned Cycles Page)

G80 Cancel all canned cycles

G81 Basic drill cycle

G83 Peck drilling cycle

G84 R.H. tapping cycle

G85 Basic boring cycle

G86 Boring cycle, spindle stop at bottom, rapid out

_________________________________

Absolute / Incremental Mode

*G90 Absolute Programming Mode All X,Y,Z coordinates determined from a single from a single origin.

*G91 Incremental Programming Mode Next X,Y,Z, coordinates are determined from current location

_________________________________

Feedrate Mode Selection

*G94 Feedrate input in inches (or millimeters) per minute. Primarily used on mills

*G95 Feedrate input in inches (or millimeters) per revolution. Primarily used on lathes

Common (Mill & Lathe) M-Codes

M00 Machine stop stops the machine, requiring the operator to restart the program to continue.

M01 Optional stop stops the machine as above only when the optional stop button has been pressed prior to this command in the program

M02 Program end tells the machine control that the program is complete

M03 Spindle start clockwise (S) at the RPM specified by the S word accompanying the code

M04 Spindle start counter clockwise as above

M05 Spindle stop

M06 Tool change (T) commands to machine to exchange the tool currently in use for the one called by the T word

M07 / M08 Coolant on If the machine is equipped with only one coolant system, it is generally commanded by the M08

M09 Coolant off

M19 Spindle orientation

M30 Program stop and rewind to program start

_______________________________________

Lathe Only G-codes

G33 Thread cutting, constant lead [ ]

G34 Thread cutting, increasing lead [ ]

G35 Thread cutting, decreasing lead [ ]

G50 Maximum Spindle RPM for constant surface speed operation

______________________________________

Lathe specific canned cycles (See Canned Cycles Page)

G73 OD or ID roughing cycle [ ]

G74 Rough facing cycle [ ]

______________________________________

Mill Only G-codes