From TechnoDocs
Revision as of 14:21, 1 October 2010 by Jbeck (Talk | contribs)

Jump to: navigation, search

The following G and M codes are supported by the Control Interface.

Setup Commands

Code Command Format Purpose
F Feed Speed
F<speed>
Sets the feed rate, or rate of movement of the axes.
G4 Dwell Time
G4 P<milliseconds>
Inserts a delay in milliseconds.
G90 Absolute Coordinates
G90
Sets coordinates to absolute, so that the motion commands are relative to the origin.
G91 Incremental Coordinates
G90
Sets coordinates to incremental so that all motion commands are relative to the previous position.
G92 Set Absolute Origin
G92 X<#> Y<#> Z<#>
Sets the origin that is referenced when in absolute mode.
M0 Program Stop/Pause
M0
Stops the g-code file from being further processed until the operator presses Continue or Start.
M30 End of Data
M30
Marks the end of the file. The rest of the file will not be processed.
M3 or M4 Spindle On
M3
or
M4
Starts the spindle.
M5 Spindle Off
M5
Turns the spindle off.
M6 Tool Change
M6 T<#>
Requests the machine change to the specified tool number. It will turn off the spindle and coolant and other required operations when it changes the tool.
M7 or M8 Coolant On
M7
or
M8
Turns the coolant flow on.
M9 Coolant Off
M9
Turns the coolant flow off.
M90 Output Off
M90 OUT<#>
Turns the output to the Off or 0 state.
M91 Output On
M91 OUT<#>
Turns the output to the On or 1 state.

Routing Commands

Code Command Format Purpose
G0 Rapid Move
G0 X<#> Y<#> Z<#> A<#>
Moves one or more of the axes at the rapid speed, to the specified location. Note that not all axes are required to be specified.
G1 Straight Line
G1 X<#> Y<#> Z<#> A<#>
Moves the specified axes in straight (linear) motion. It will use the requested feedrate, either from the F command or whatever the cut speed has been specified to be. This is a cutting move.
G2 Clockwise Arc
G2 X<#> Y<#> I<#> J<#>
or
G2 X<#> Z<#> I<#> K<#>
or
G2 Y<#> Z<#> J<#> K<#>
Moves two axes (XY, XZ or YZ) along the path of an arc in a clockwise direction. The XY specification is the end position, and the IJ specification is the center of the arc.
G3 Couterclockwise Arc
G3 X<#> Y<#> I<#> J<#>
or
G3 X<#> Z<#> I<#> K<#>
or
G3 Y<#> Z<#> J<#> K<#>
Moves two axes (XY, XZ or YZ) along the path of an arc in a counterclockwise direction. The XY specification is the end position, and the IJ specification is the center of the arc.

Drill Cycle Commands

Code Command Format Purpose
G80 Drilling Cycle Off
G80
Turns a drill cycle off.
G81 Standard Drilling Cycle Without Dwell
G81 X<#> Y<#> Z<#> R<#> P<#> F<#>
Provides a feed-in, rapid-out sequence used for standard drilling without a dwell time.
G82 Standard Drilling Cycle With Dwell
G82 X<#> Y<#> Z<#> R<#> P<#> F<#>
Provides a feed-in, rapid-out sequence used for standard drilling with a specified dwell time.
G83 Peck Drilling Cycle
G83 X<#> Y<#> Z<#> R<#> Q<#> V<#> P<#> F<#>
Provides a series of feed=in peck drilling motions with full retract used for drilling holes.
G87 Chip Break Drilling Cycle
G87 X<#> Y<#> Z<#> R<#> Q<#> V<#> W<#> P<#> F<#>
Provides a series of feed-in rapid-out motions that is similar to peck drilling, but the retract is a specified distance instead of a full retract.

Drill Cycle Command Format

G8n X<#> Y<#> Z<#> R<#> Q<#> V<#> W<#> P<#> F<#>
X the x coordinate of the hole
Y the y coordinate of the hole
Z the z coordinate of the hole
R the reference height for start of drill plunge
Q the initial z peck increment
V the subsequent z peck increment
W the peck clearance, z retract between pecks
P the dwell time (in seconds)
F the drilling feedrate, plunge speed
n an integer in the range of zero to nine