|
MultiCam CNC Language Summary
The MultiCam CNC controller can interpret 2 languages HPGL and EIA-274D (G 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 the MultiCam CNC controller interface. You will also find many samples.
Uses For This Document:
• Post Processor or driver creation to interface CAM or Graphics software output with the MultiCam Controller. (Note many CAM and Graphics software already have post or driver support. Please check with your distributor or email the support department if you have any questions.)
• Code level trouble shooting and file creation.
M and G Code Table
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] [Fd.d] [Td] [Ctext string] |
High
speed move (slew) |
| G01 [Xd.d]
[Yd.d] [Zd.d] [Fd.d] |
Linear
move (machine) |
| G02 [Xd.d]
[Yd.d] [Zd.d] [Id.d] [Jd.d] [Kd.d] [Fd.d] |
CW
2D circular move |
| G03 [Xd.d]
[Yd.d] [Zd.d] [Id.d] [Jd.d] [Kd.d] [Fd.d] |
CCW
2D circular move |
| G04 Fd.d |
Dwell
(seconds) |
| G17 |
Specify
XY plane for helical |
| G18 |
Specify
ZX plane for helical |
| G19 |
Specify
YZ plane for helical |
| G40 |
CANCEL
Tool Compensation |
| G41 |
LEFT
Tool Compensation |
| G42 |
RIGHT
Tool Compensation |
| G62 |
Clear
soft home |
| G72 [Xd.d]
[Yd.d] [Zd.d] [Id.d] [Jd.d] [Kd.d] [Fd.d] |
CW
3D circular move |
| G73 [Xd.d]
[Yd.d] [Zd.d] [Id.d] [Jd.d] [Kd.d] [Fd.d] |
CCW
3D circular move |
| G74 |
Incremental
mode for G02/03 arcs |
| G75 |
(G90/G91)
mode for G02/03 arcs |
| G83 Rd.d
Zd.d Dd.d [Fd.d] |
Peck
drill (With Router) |
| G90 |
Absolute
coordinate mode |
| G91 |
Incremental
coordinate mode |
| G92 [Xd.d]
[Yd.d] [Zd.d] |
Set
soft home |
| G97 Sd |
Set
spindle speed (rpm) |
| G98 P145 Dd |
Go to pre-recorded
home position, D(1) Home 1, D(2) Home 2, etc. |
| G98 P147
Dd |
Park
X axis , D(0) X-Min, D(1) X-Max |
| G98 P300
Dd |
Boring
Unit Drill Select. |
| |
|
| Plasma Systems only |
The plasma
system ignors feed rates sent in the job file by default. |
| G98 P133 D1 |
Feedrate will
be used from now on. |
| G98 P133 D0 |
Feedrates
will be ignored from now on. |
| |
The following table lists the
letters used to denote various arguments.
C -
Tool change operator message (G00 required)
D -
Peck drill delta (used in G83), Data selection in G98.
F -
Feed rate (used in G00, G01, G02, G03, G72, G73, G83) Units
per Second
F -
Dwell (used in G04)
G -
Preparatory function
I -
Circular interpolation value in X dimension (used in G02, G03,
G72, G73)
J -
Circular interpolation value in Y dimension (used in G02, G03,
G72, G73)
K -
Circular interpolation value in Z dimension (used in G02, G03,
G72, G73)
M -
Miscellaneous function (control function)
N -
Sequence number
R -
Beginning Z motion dimension (used in G83)
S -
Spindle rpm (used in G97)
T -
Tool change (used in G00)
X -
X motion dimension
Y -
Y motion dimension
Z -
Z motion dimension
|
M-Codes:
The table below lists the available
M-Codes and how they should be configured for Job Server.
| |
Job
Server Settings |
|
| Code |
Description |
Device # |
State |
Graphics |
Notes |
Init File Compatibility |
| M00 |
Program
Pause |
N/A |
N/A |
N/A |
0
prg_pause |
|
| M01 |
Optional
Program Pause |
N/A |
N/A |
N/A |
1
prg_pause |
|
| M02 |
End of
Job |
N/A |
N/A |
N/A |
end_plot |
|
| M03 |
Start Spindle
Clockwise |
113 |
Active |
N/A |
Spindle
ON Clockwise |
|
| M04 |
Start Spindle
Counter-Clockwise |
114 |
Active |
N/A |
Spindle
ON Counter-Clockwise |
|
| M05 |
Spindle
Off |
105 |
Active |
N/A |
spindle_off |
|
| M11 |
2D Device
ON |
-1 or 101 |
Active |
ON |
If
you use -1, the current tool number is passed for M11. If you
use 101, then the INIT file handles selecting the current tool
number.
Plasma Arc On |
|
| M12 |
3D Device
ON |
-1 or 102 |
Active |
ON |
See
note for M11 |
|
| M21 |
2D
Device OFF |
-1
or 101 |
Inactive |
OFF |
See
note for M11
Plasma Arc Off |
|
| M22 |
3D Device
OFF |
-1 or 102 |
Inactive |
OFF |
See
note for M11 |
|
| M25 |
Start of
Sheet |
-99 |
Active |
OFF |
Pause
and load next sheet |
H4LDR Ver
4.50 and later |
| M30 |
Fire Enabled
Drill |
130 |
Active |
OFF |
|
H4LDR Ver
4.55 and later |
| M31 |
Drill 1
ON (Enable + Offset) |
131 |
Active |
OFF |
|
H4LDR Ver
4.55 and later |
| M32 |
Drill 2
ON (Enable + Offset) |
132 |
Active |
OFF |
|
H4LDR Ver
4.55 and later |
| M38 |
Gang Drill
1 ON |
138 |
Active |
OFF |
|
|
| M41 |
Drill 1
OFF (Disable) |
131 |
Inactive |
OFF |
|
H4LDR Ver
4.55 and later |
| M42 |
Drill 2
OFF (Disable) |
132 |
Inactive |
OFF |
|
H4LDR Ver
4.55 and later |
| M48 |
Gang Drill
1 OFF |
138 |
Inactive |
OFF |
|
|
| M60 |
Put Away
Tool |
104 |
Active |
OFF |
This
is ONLY available on ATC machine. |
H4LDR Ver
4.55 and later |
| M90 |
Program
Start |
N/A |
N/A |
N/A |
start_plot
CYCLE_START |
|
| M92 |
ALL Mode
On |
192 |
Active |
OFF |
(Multi
Head) |
H4LDR Ver
4.58 and later. STD ONLY |
| M93 |
ALL Mode
Off, Return to Auto Mode |
192 |
Inactive |
OFF |
(Multi
Head) |
H4LDR Ver
4.58 and later. STD ONLY |
| M94 |
Auto Mode,
Disable Spindle Offset |
194 |
Active |
N/A |
(Multi
Head)
Make the Spindle Offset between heads 0.0. |
H4LDR Ver
4.71 and later. STD ONLY |
| M95 |
Enable
Marking Mode |
195 |
Active |
OFF |
Plasma
Only |
|
| M96 |
Disable
Marking Mode |
195 |
Inactive |
OFF |
Plasma
Only |
|
| M97 |
Double
Velocity |
197 |
Inactive |
OFF |
Plasma
Only, used for faster lead-outs. |
|
| M98 |
Turn off
Z-Tracking, then plasma arc. |
198 |
Inactive |
OFF |
Plasma
Only. Used to turn off the arc before the end of the contour. |
|
| M99 |
Exit CNC
Interpreter |
N/A |
N/A |
N/A |
|
|
General Post Processor Notes
- Z axis parameters
- Material Surface (Z
= 0.0)
- Tool Lift (-Z) (Z=
-0.75 would raise the cutter .75 inches above the material.)
- Depth (+Z) (Z=1.5
would lower the cutter 1.5 inches into the material.)
- G00 C[tool change text]
- This command will
display the text that follows the "C" on the keypad
display. It can be used to perform tool changes on machines
that do not have automatic tool changers.
- The user will have
that ability to surface the new tool when this command is
called.
- Do not use this command
on systems that do have an automatic tool changer.
- The keypad pad display
has 2 lines, 20 characters each line, 40 characters total..
To provide the user with the best possible visual display
spaces can be used to force some of the characters to the
next line.
- Example: G00
CInsert .25 inch end mill will
prompt the user with the following text: "Insert .25
inch end mill".
- When creating a G-Code file
from your post processor, the file must end with a .cnc or .anc file
extension. This is important so the MultiCams DNC program knows
that the file is a G-Code file.
- File comments: "//" is
use for a comment example: // This line is a comment.
- Multiple G codes or M codes
cannot be put on the same line.
|
|
