| Code |
Supported |
Meaning |
| A,B,C |
Yes* |
Auxiliary Axis, *A supported |
| D |
Yes |
Offset CRC |
| E |
No |
IPR Feedrate |
| F |
Yes |
IPM/IPR Feedrate |
| G0/G00 |
Yes |
Non-Linear Rapid moves |
| G1/G01 |
Yes |
Linear Interpolation |
| G2/G02 |
Yes |
CW Interpolation |
| G3/G03 |
Yes |
CCW Interpolation |
| G4/G04 |
Yes |
Dwell |
| G17 |
Yes |
X,Y Plane of Interpolation |
| G18 |
Yes |
X,Z Plane of Interpolation |
| G19 |
Yes |
Y,Z Plane of Interpolation |
| G28 |
Yes |
Return to Machine zero |
| G40 |
Yes |
CRC cancel |
| G41 |
Yes |
CRC left |
| G42 |
Yes |
CRC right |
| G43 |
No |
Tool length comp. + |
| G44 |
No |
Tool length comp. - |
| G49 |
No |
Tool Length comp. Cancel |
| G50 |
Yes |
Set Program Zero |
| G54-G59 |
No |
Set Local Coordinate Systems |
| G70 |
No |
Rough turning canned cycle |
| G71 |
No |
Finishing turning canned cycle |
| G73 |
No |
Drill CHPBRKR |
| G80 |
Yes |
Canned Cycle cancel |
| G81 |
Yes |
Spot Drilling Cycle |
| G82 |
No |
Drill/Counterbore |
| G83 |
Yes |
Peck Drilling Cycle |
| G85 |
No |
Bore |
| G90 |
Yes |
Absolute Programming |
| G91 |
Yes |
Incremental Programming |
| G92 |
Yes |
Set Program Zero |
| G94 |
No |
IPM Programming |
| G95 |
No |
IPR Programming |
| G97 |
No |
Direct Spindle Speed Programming |
| G98 |
Yes |
Return to initial level |
| G99 |
Yes |
Return to R level |
| H |
No |
Tool length offset call |
| I,J,K |
Yes |
Arc center location |
| MO/MOO |
Yes |
Program stop |
| M1/M01 |
Yes |
Optional stop |
| M2/M02 |
Yes |
Program stop |
| M3/M03 |
No |
Spindle normal rotation |
| M4/M04 |
No |
Spindle reverse rotation |
| M5/M05 |
No |
Spindle off |
| M6/M06 |
No |
Tool change |
| M8/M08 |
No |
Coolant on |
| M9/M09 |
No |
Coolant off |
| M30 |
Yes |
Program reset/tape rewind |
| M98 |
Yes |
Sub-Program call |
| M99 |
Yes |
Return to previous program |
| N |
Yes |
Sequence Numbers |
| O |
Yes |
Program Numbers |
| P |
Yes |
Dwell time |
| Q |
No |
Peck Depth |
| R |
Yes |
Rapid level |
| R |
Yes |
Arc center radius |
| S |
No |
Spindle speed |
| T |
No |
Tool number |
| U,V,W |
No |
Incremental Move in X, Y, Z |
| X,Y,Z |
Yes |
Absolute Move in X, Y, Z |
Supported G&M code examples
Example
G0 X-1.780 Y-1.025 Z0.1
Description
Moves the tool to location (-1.78,-1.025,0.1) at the move speed specified
in Setup|CNC defaults. The Z axis will be moved first. |
Example
G1 X0.939
X0.948 Y0.333
Description
Moves the tool along the X axis to location (0.939) at the feed speed
specified in Setup|CNC defaults. Then moves the tool to location
(0.948, 0.333). |
Example
G1 X0.948 Y0.333 F2.5
Description
Moves the tool to location (0.948,0.333) at speed 2.5. Any subsequent
G1 commands or coordinates will continue to use speed of 2.5 until you
set it to some other value or you cancel the F command. To cancel
the F command, use F0. This will reset the feed speed to the value
in the Setup|CNC Defaults form. If you specify a speed higher than
the MaxSpeed value specified in the Setup|Motor Parameters form, the MaxSpeed
value will be used instead. |
Example
G2 X-1.535 Y0.469 I0.500 J0.000
Description
Move in a clockwise arc from the current position to location (-1.535,
0.469) using a center point located 0.5 units in the X direction from the
current position. |
Example
G3 X-1.535 Y0.469 I-0.500 J0.000
Description
Move in a counter-clockwise arc from the current position to location
(-1.535, 0.469) using a center point located 0.5 units in the negative
X direction from the current position. |
Example
G4 P2000
Description
Pause the tool for 2 seconds (2000 milliseconds) before continuing. |
Example
G27
Description
Rapid return home. Move directly to location (0, 0, 0) at the
move speed specified in Setup|GNC Defaults. |
Example
G28 X0.5 Y-.2 Z.1
Description
Rapid return home via point. Move directly to location (0.5,
-0.2, 0.1) at the default move speed, then move directly home to location
(0, 0, 0). |
Example
G50 X0.5 Y-.2 Z.1
Description
Redefine the tools current location to be (0.5, -0.2, 0.1). |
Example
G81
D .125
M1
X-0.470 Y0.597 Z-0.030 L0.01
G80
Description
Start Drill cycle with G81. D parameter specifies drill bit radius
(not diameter) of 0.125. Pause program with M1 command giving you
time to load a drill bit. Manually adjust the tool depth so that
the tip of the new drill bit is at the same depth as the one removed.
When you are ready, click the Continue button. The tool moves up
to Zsafe defined in Setup|GNC Defaults form. Then it moves to location
(-0.47, 0.597) at the default move speed. Then it moves down to 0.01
at the default move speed. Then it moves down to the Z depth of –0.030
at the default feed speed. If you leave out the L coordinate, it
will travel at the feed speed from Zsafe to the Z depth. Subseqent
X,Y coordinates will drill new holes at the new coordinates. The
tool will lift up before moving to the next hole. Finally, drill
cycle is cancelled with G80. |
Example
G83
D .125
M1
X-0.470 Y0.597 Z-1 L0.01 Q.3
G80
Description
Start Peck Drill cycle with G83. D parameter specifies drill
bit radius (not diameter) of 0.125. Pause program with M1 command
giving you time to load a drill bit. Manually adjust the tool depth
so that the tip of the new drill bit is at the same depth as the one removed.
When you are ready, click the Continue button.
1) The tool moves up to Zsafe defined in Setup|GNC Defaults form.
2) Moves to location (-0.47, 0.597) at the default move speed.
3) Moves down to 0.01 at the move speed. If L parameter not defined,
it will use Zsafe.
4) Moves down another 0.3 units at the default feed speed If
Q parameter not defined, it will use 2 times the drill bit diameter.
5) Moves back up to 0.01 at move speed.
6) Moves down to within one radius of previous depth at move speed
7) Moves down another 0.3 units at feed speed
8) Repeats steps 5-7 until Z depth of –1.0 has been reached
9) Moves up to 0.01 at move speed
10) Subseqent X,Y coordinates will peck drill new holes at the new
coordinates. The tool will lift up to Zsafe before moving to the
next hole.
11) Finally, drill cycle is cancelled with G80. |
Example
G98
Description
Move Z axis to depth set in L code at the default move speed defined
in Setup|GNC defaults form. |
Example
G99
Description
Move Z axis to depth set in R code at the default move speed defined
in Setup|GNC defaults form. |
Example
M0
Description
Stop program |
Example
M30
Description
Reset program back to the top and start running again from there |
Here's a good site for more CNC
Programming information.
|
