| X## = X position | Y## = Y position | Z## = Z position |
| I## = X arc center | J## = Y arc center | K## = Z arc center |
| U## = linear opposite X sometimes used as incremental (lathe) |
V## = linear opposite Y sometimes used as incremental (lathe) |
W## = linear opposite Z sometimes used as incremental (lathe) |
| A## = rotary around X | B## = rotary around Y | C## = rotary around Z |
| F## = feedrate | R## = drill retract | Q## = drill peck |
| ## = | ## = | ## = |
| R+## = arc radius(+) if < 180° | R-## = arc radius(-) if > 180° |
| D## = cutter dia/rad offset | H## = tool length offset |
| P## = dwell time in 10000th sec |
G-Codes
| G00 = Rapid
linear move example: G00 X## Y## Z## (X,Y,Z = position) |
| G01 = Feed linear move example: G01 F## X## Y## Z## (F=feedrate to move at) |
| G02 = Circular move CW example: G02 X## Y## I## J## (XY=end point, IJ=center point) |
| G02 = Circular move CW example: G02 X## Y## R±## (R=size of radius arc to swing. R+ if radius < 180°, R- if radius is > 180°) |
| G03 = Circular move CCW example: G03 X## Y## I## J## (XY=end point, IJ=center point) |
| G03 = Circular move CCW example: G03 X## Y## R±## (R=size of arc radius to swing. R+ if radius < 180°, R- if radius is > 180°) |
| G04 = Dwell time example: G04 P## (P=time to dwell. P20000 is 2 seconds) |
| G10 = Zero offset shift example: G10 X## Y## Z##(X=shift dist. Y=shift dist. Z=shift dist.) |
| G11 = Zero offset shift cancel example: G11 |
| G17 = Contour plane is XY (Z = spindle) example: G17 |
| G18 = Contour plane is ZX (Y = spindle) example: G18 |
| G19 = Contour plane is YZ (X = spindle) example: G19 |
| G20 = Inch mode (G70 on older controls) example: G20 |
| G21 = MM mode (G71 on older controls) example: G21 |
| G28 = Return to reference point example: G0 G91 G28 X## Y## Z## (Go to machine XYZ home,passing thru XYZ incremental zero) |
| G29 = Return from reference point example: G0 G90 G29 X## Y## Z## (Go to this XYZ position, returning from home) |
| G30 = Return to 2nd, 3rd (ect..) reference point example: Similar to G28 |
| G40 = Cutter (dia.or rad.) compensation off example: G40 X## Y## |
| G41 = Cutter compensation to the left of the
programmed path example: G40 X## Y## |
| G42 = Cutter compensation to the right of the
programmed path example: G40 X## Y## |
| G43 = Tool length compensation with spindle approach
from +
side example: G43 H## Z## |
| G44 = Tool length compensation with spindle approach
from -
side example: G44 H## Z## |
| G49 = Tool length compensation cancel example: G49 |
| G45 = Increase end position by tool offset value example: G45 X## D## (Go to X position, plus offset value in D##) |
| G46 = Decrease end position by tool offset value example: G46 X## D## (Go to X position, less offset value in D##) |
| G47 = Increase end position by twice the offset
value example: G47 X## D## (Go to X position, plus 2x the offset value) |
| G48 = Decrease end position by twice the offset
value example: G48 X## D## (Go to X position, less 2x the offset value) |
| G53 = Coordinate system referenced from machine home
example: G53 X## Y## Z## (Go to this XYZ position referenced from machine home) |
| G54 = Work coordinate shift,offset #1 example: G54 X## Y## Z## (Go to this XYZ position referenced from WCS #1) |
| G55 - G59 = Work coordinate shift,offset G55-G59 example: G5# X## Y## Z## (Go to this XYZ position referenced from WCS G55-G59) |
| G09 = Exact stop positioning move example: G09 F## X## Y## Z## (active for single block only) |
| G61 = Exact stop cutting mode example: G61 X## Y## Z## (Decelerated at point XYZ, before next move) |
| G64 = Exact stop mode off example: G64 X## Y## Z## (Tool is not decelerated at point XYZ) |
| G63 = Feed overide lock out example: G63 X## Y## Z## |
| G62 = Feed compensation on inner corner example: G62 G02 X## Y## I## J## |
| G81 = Basic drilling cycle - Feed in , rapid out. example: G81 X## Y## Z## R## F## |
| G82 = Counter bore cycle - Feed in, dwell, rapid
out. example: G82 X## Y## Z## R## F## P#### |
| G83 = Peck drilling cycle - Feed in peck amount,
rapid out,
rapid in within .050 of last peck & repeat until depth is reached. example: G83 X## Y## Z## R## F## Q## |
| G84 = Tapping cycle - Feed in, spindle stop,
reverse, feed out. (note: this cycle will vary depending on the machine mfgr.) example: G84 X## Y## Z## R## F## |
| G85, G86, G87, G88, G89 = Boring cycles. Function
& imput
will vary depending on the machine mfgr. Variations include.... Feed in, feed out. Feed in, dwell, feed out. Feed in, dwell, spindle stop, rapid out. Feed in, dwell, spindle stop, move insert from wall, rapid out. Rapid in, dwell, start spindle, feed up, dwell, rapid down, dwell (reverse counter boring, back facing, back boring cycle). |
| G90 = Absolute
coordinate positioning.
Points based from XYZ zero. example: G90 G00 X## Y## Z## |
| G91 = Incremental
coordinate positioning.
Point to point positioning. example: G91 G00 X## Y## Z## |
| G92 = Absolute Zero Pre-Set - An old format used to
set XYZ
Zero. The current position is set to the values shown in the line. example: G92 X10 Y5 Z-3 After running this command the current position is X10 Y5 Z-3. Very strange way to shift zero's. Avoid this code if you can. |
| G94 = Feedrate is read as Inches/Minute. Used mostly
for milling. example: G94 G01 X## Y## Z## F## |
| G95 = Feedrate is read as Inches/revolution. Used
mostly for
turning. example: G95 G01 X## Y## Z## F##.### |
| G96 = Constant surface speed (CSS) control (lathe).
Increases
the RPM as the tool moved closer to the center line of the part
(smaller
diameter). This keeps the amount of material (chip load) moving past
the
tip of the tool constant for and improved tool load, tool wear and
surface
finish. In the example below, the control will do an internal
calculation
to keep the tool moving at 200 surface feed/second. example: G96 S200 |
| G97 = The opposite of constant surface speed control
(G96). example: G97 |
| G98 = Retract the tool to the starting Z height when
drilling.
Used for high retrect clearance moved between drilled holes. Assume Z
is
currently at Z+1.0. Running the line below will rapid to the R
plane,
drill to the Z depth and return to the starting height of Z+1.00 when
the
cycle is finished. example: G98 G81 X## Y## Z-.875 R.100 F## |
| G99 = Retract the tool to the R plane when the
drilling cycle
is finished. Regardless of the starting height, the tool will return to
Z.100 (the Rplane shown below). example: G99 G81 X## Y## Z-.875 R.100 F## |
| G = example: |
| G = example: |
| G = example: |
| G = example: |
| G = example: |
M-Function Codes
| M00 = Program stop |
| M01 = Optional program stop |
| M02 = End of program (no rewind or return to start of program) |
| M03 = Start the spindle in the forward direction (CW) |
| M04 = Start the spindle in the reverse direction (CCW) |
| M05 = Stop the spindle / Spindle off. |
| M06 = Tool change command |
| M07 = Coolant on mist |
| M08 = Coolant on flood |
| M09 = Coolant off |
| M13 = Spindle on forward, coolant on |
| M14 = Spindle on reverse, coolant on |
| M15 = Spindle off, coolant off |
| M19 = Spindle orientation on. Used to locate the tool tip position for boring tools. Sometimes output with a value that represents the angle of the tool tip orientation. |
| M20 = Spindle orientation off |
| M30 = End of program (rewind/return to start of program) |
| M98 = Call sub program |
| M99 = Sub program end |
| Not all of these M Functions work on all machines. |
This Page Written By Mike Mattera