cincinnati CL-707, CL-800 Programming Manual
PROGRAMMING MANUAL
AN OPERATION SUPPLEMENT MANUAL FOR THE
CINCINNATI CL-707, CL-7A, AND CL-800
LASER SYSTEM WITH PC-BASED CONTROL
EM-423 (R-02/11) COPYRIGHT 2011
CINCINNATI INCORPORATED
PROGRAMMING CONTENTS
SECTION 1 STANDARD G-CODES
1.00 G00 RAPID TRAVERSE MOVE...........................................................1-1
1.01 G01 LINEAR MOVE.............................................................................1-1
FEEDRATE.......................................................................................... 1-2
1.02 G02 CLOCKWISE ARC .......................................................................1-2
1.03 G03 COUNTERCLOCKWISE ARC......................................................1-2
RECOMMENDED ARC FEEDRATE...................................................1-3
1.04 G04 DWELL......................................................................................... 1-3
1.09 G09 EXACT STOP (ONE BLOCK) ......................................................1-4
1.20 G20 INCH MODE.................................................................................1-4
1.21 G21 METRIC MODE............................................................................1-4
1.31 G31 POSITION CAPTURE MOVE....................................................... 1-4
1.40 G40 CANCEL KERF COMPENSATION.............................................. 1-4
1.41 G41 LEFT SIDE COMPENSATION..................................................... 1-4
1.42 G42 RIGHT SIDE COMPENSATION...................................................1-4
1.50 G50 CANCEL SCALING...................................................................... 1-5
1.51 G51 WORK COORDINATE SYSTEM SCALING.................................1-5
1.52 G52 LOCAL WORK COORDINATE SYSTEM ................................ 1-6
1.53 G53 RAPID MOVE TO MACHINE COORDINATES............................1-6
1.54 G54 THROUGH G59............................................................................1-6
1.61 G61 EXACT STOP MODE...................................................................1-7
1.64 G64 CANCEL EXACT STOP MODE ...................................................1-7
1.65 G65 SUB-PROGRAM CALL ................................................................1-7
1.68 G68 WORK COORDINATE SYSTEM ROTATION ........................1-7
1.69 G69 CANCEL ROTATION ...................................................................1-7
1.90 G90 ABSOLUTE MODE.......................................................................1-8
1.91 G91 INCREMENTAL MODE................................................................1-8
1.92 G92 WORK COORDINATE SYSTEM SETTING.................................1-8
SECTION 2 CUSTOM G-CODES
2.84 G84 PIERCE AND START CUT ..........................................................2-1
2.85 G85 START CUT WITHOUT PIERCE ................................................. 2-1
PIERCE OPTIONS (G84 T_)...............................................................2-1
AIRBLAST ...........................................................................................2-1
2.89 G89 PROCESS PARAMETERS..........................................................2-2
2.102 G102 ADDITIONAL PARAMETER SETTINGS ................................... 2-3
2.103 G103 RAMPED PIERCE SETTINGS................................................... 2-4
2.120 G120 DISABLE NON-STOP CUTTING ...............................................2-4
2.121 G121 ENABLE NON-STOP CUTTING ................................................2-4
SMART RAPIDS..................................................................................2-5
2.123 G123 PROGRAMMABLE BLEND........................................................ 2-6
2.124 G124 DEFAULT BLEND...................................................................... 2-6
2.125 G125 AUTO BLEND.............................................................................2-6
SECTION 3 M-CODES
3.00 M00 PROGRAM STOP........................................................................3-1
3.01 M01 OPTIONAL STOP ........................................................................3-1
3.02 M02 END OF PROGRAM.................................................................... 3-1
3.30 M30 END OF PROGRAM WITH REWIND ..........................................3-1
3.35 M35 BEAM OFF...................................................................................3-1
3.36 M36 SERVO HOLD FOR NONCONTACT Z-AXIS.............................. 3-1
3.37 M37 BEAM OFF, GAS OFF AND SHUTTER CLOSE .........................3-1
3.38 M38 TIMED NONCONTACT SERVO HOLD ....................................... 3-2
3.41 M41 COMMAND Z-AXIS DOWN TO CUT POSITION.........................3-2
3.42 M42 RETRACT Z-AXIS........................................................................3-2
3.43 M43 LOWER PALLET SPECIAL FUNCTION......................................3-2
3.44 M44 CANCEL LOWER PALLET SPECIAL FUNCTION ......................3-3
3.45 M45 APPLY OPTIONAL STANDOFF FOR CUTTING ........................ 3-3
3.47 M47 RAISE Z-AXIS, OPTIONALLY BY DISTANCE ............................3-3
EM-423 (R-02/11) iii
3.48 M48 FEEDRATE OVERRIDE DISABLE...............................................3-3
3.49 M49 FEEDRATE OVERRIDE ENABLE................................................3-3
3.50 M50 SWITCH PALLETS.......................................................................3-3
3.51 M51 AUXILIARY TIMED OUTPUT.......................................................3-4
3.67 M67 APPLY OPTIONAL ASSIST GAS PRESSURE .......................3-4
3.98 M98 SUB-PROGRAM CALL WITH NO ARGUMENTS........................3-4
3.99 M99 END SUB-PROGRAM AND RETURN .........................................3-4
3.130 M130 Z-AXIS ANTI-DIVE DISABLE .....................................................3-4
3.131 M131 Z-AXIS ANTI-DIVE ENABLE ......................................................3-4
3.135 M135 DISCHARGE CURRENT OFF....................................................3-5
SECTION 4 CINCINNATI MACROS
4.65 GRID MACROS...................................................................................4-1
PART SUB GRID MACRO G65 P9800...............................................4-1
PART GRID MACRO: G65 P9900......................................................4-2
CUTTING MACROS.......................................................................................4-3
4.73 G73 HOLE MACRO ................................................................4-4
4.76 G76 SLOT MACRO.................................................................4-4
4.79 G79 LINE MACRO..................................................................4-4
4.83 G83 OUTSIDE CIRCLE MACRO............................................4-5
4.86 G86 OUTSIDE RECTANGLE MACRO...................................4-5
4.88 G88 BOLT CIRCLE MACRO...................................................4-5
4.104 G104 SHAPE MACRO...........................................................4-6
4.105 G105 LEAD-IN MACRO.........................................................4-8
SECTION 5 PROGRAM STRUCTURE
5.1 PROGRAM NAME.................................................................................5-1
5.2 PROGRAM BODY.................................................................................5-1
5.3 BEAM ON AND OFF COMMANDS.......................................................5-1
5.4 PROGRAM COMMENTS ......................................................................5-1
5.5 PROGRAM LINE NUMBERS ................................................................5-2
5.6 BLOCK DELETE....................................................................................5-2
5.7 END OF PROGRAM..............................................................................5-2
M02 ......................................................................................................5-2
M99 (P_)...............................................................................................5-2
M30 ......................................................................................................5-2
5.8 SUB-PROGRAMS AND MACROS........................................................5-2
SECTION 6 PROGRAM VARIABLES
6.1 LOCAL AND COMMON VARIABLES....................................................6-1
LOCAL VARIABLES: #1 - #99 ............................................................6-1
COMMON VARIABLES: #100 - #999 .................................................6-1
6.2 SYSTEM VARIABLES...........................................................................6-1
OFFSET DATA SYSTEM VARIABLES................................................6-1
CNC DATA SYSTEM VARIABLES......................................................6-2
MODAL DATA SYSTEM VARIABLES.................................................6-3
COORDINATE SYSTEM VARIABLES.................................................6-3
SECTION 7 AUXILIARY FUNCTIONS
7.1 MATH FUNCTIONS...............................................................................7-1
BRACES [ ]..........................................................................................7-1
7.2 LOGIC FUNCTIONS..............................................................................7-2
CONDITIONAL EXPRESSIONS..........................................................7-2
PROGRAM CONTROL COMMANDS..................................................7-2
7.3 AUXILIARY COMMANDS......................................................................7-3
DPRNT COMMAND (OPTION)...........................................................7-3
AUTOMATIC CORNER ROUNDING...................................................7-3
7.4 PROGRAMMING FOR MATERIAL HANDLING OPTION.....................7-4
7.5 WORKPIECE EDGE DETECTION........................................................7-5
CALIBRATION .....................................................................................7-5
OPERATION........................................................................................7-6
SPECIFICATIONS ...............................................................................7-7
7.6 OPTICAL PROBE................................................................................7-11
7.7 LASER OPTICAL PROBE...................................................................7-11
SECTION 8 FILE TRANSFER & NETWORKING
8.1 FILE TRANSFER ..................................................................................8-1
NETWORK: .........................................................................................8-1
FLOPPY DISK: .................................................................................... 8-1
RS-232 INTERFACE: .......................................................................... 8-1
8.2 NETWORKING......................................................................................8-1
NETWORKING OPTIONS...................................................................8-2
SECTION 9 INDEX
INDEX ............................................................................................................9-1
EM-423 (R-02/11) v
SECTION 1 STANDARD G-CODES
the block in G90 mode, and incremental distances when
commanded in G91 mode. The command must specify
CODE DESCRIPTION SEC.
G00 Rapid move to Work Coordinates 1.00
G01 Linear move to Work Coordinates 1.01
G02 Clockwise arc to Work Coordinates 1.02
G03 Counterclockwise arc to Work
Coordinates
G04 Dwell 1.04
G09 Exact Stop (one block) 1.09
G20 Inch Mode 1.20
G21 Metric Mode 1.21
G31 Position Capture Move 1.31
G40 Cancel Kerf Compensation 1.40
G41 Kerf Compensation Left 1.41
G42 Kerf Compensation Right 1.42
G50 Cancel Scaling 1.50
G51 Work Coordinate System Scaling 1.51
G52 Temporary Local Work Coordinate
System
G53 Rapid move to Machine Coordinates 1.53
G54
G59
G61 Modal Exact Stop 1.61
G64 Cancel Exact Stop Mode 1.64
G65 Sub-program call 1.65
G68 Work Coordinate System Rotation 1.68
G69 Cancel Rotation 1.69
G90 Absolute mode 1.90
G91 Incremental mode 1.91
G92 Set Work Coordinate Origin 1.92
Work Coordinate Offset selection 1.54
to
1.03
1.52
at least one axis.
The G00 command moves the axes at the rapid traverse
rate of the machine. G01, G02 and G03 move the axes at
the contouring feedrate (optionally specified in the block
with “F”). When the block does not command a feedrate,
the program uses the last defined contouring feedrate.
When the control applies the rapid traverse rate for a
G00 move, it does not change the contouring feedrate
used by the G01, G02, and G03 blocks.
1.00 G00 RAPID TRAVERSE MOVE
The G00 command moves the cutting nozzle to a work
coordinate location (or incremental distance) using the
rapid traverse rate.
G00 X__ Y__
Example: (G91) G00 X10 Y6
When the command requires both axes to move, the axis
These four G-codes move the cutting nozzle to
commanded Work coordinates:
G00 Rapid Traverse move
G01 Linear move
G02 Clockwise Arc
G03 Counterclockwise Arc
These four G-codes form a modal group; the last G-code
moving the longer distance uses the rapid traverse rate of
the machine. The other axis moves at a lower velocity
proportional to the distance required, so both reach their
endpoints at the same time, approximating linear
interpolation.
If the command syntax is incorrect, a Message window
displays RAPID MOVE SYNTAX ERROR.
commanded in the group is active for all blocks until the
program commands another G-code in the group. The
default code when a program starts is G00. The leading
zero can be omitted; G0, G1, G2 and G3 are the same as
G00, G01, G02 and G03.
Each of these G-codes specifies the end of the move
with X and Y in the Work coordinate system. X and Y
1.01 G01 LINEAR MOVE
This command moves the cutting head to the work
coordinates (or incremental distance) defined by X and
Y, at a contouring feedrate optionally specified by F.
G01 X__ Y__ (F_)
are absolute coordinates when the program commands
EM-423 (R-02/11) 1-1
Example: (G91) G01 X6 Y4 F250
When the command requires both axes to change
position, the machine moves each axis at a velocity
required to produce a combined feedrate equal to the
contouring feedrate. The move follows the linear path
between start and end points.
If the command syntax is incorrect, a Message window
displays LINEAR MOVE SYNTAX ERROR.
FEEDRATE
The program can specify contouring feedrate from a
parameter library. For example, the program can
command F#148 after a block calling G89 Pfilename.lib.
The user can also configure the control to assign feedrate
to a different variable than #148 (see “Common
Variables”, SECTION 6).
1.02 G02 CLOCKWISE ARC
1.03 G03 COUNTERCLOCKWISE
ARC
A program uses G02 or G03 to command a circular
contouring move ending at the work coordinates (or
incremental distances) specified by X and Y. The
command defines the shape of the arc either by
specifying incremental distances (with I and J) from the
starting position to the center, or by specifying the radius
(with R). The control software interprets “I” and “J” as
distances in the X and Y directions (respectively) from
the starting position to the center. When the command
specifies radius “R”, the control moves the nozzle along
a circular path with that radius.
The machine maintains the modal contouring feedrate
(F) along the circular path.
Example: (G91) G02 X5 Y4 I7 J-3
When the block uses “R” instead of “I and J”, there are
two possible arcs for a given direction (cw or ccw) and
end coordinates. To specify which arc to contour, the
block commands “R” with a positive or negative sign.
To specify an arc that is less than 180 degrees, the block
commands a positive “R” value. To specify an arc
greater than 180 degrees, the G02 or G03 block
commands “R” with a negative value.
Example:
When G02 or G03 specifies the same coordinates for the
start and end of the arc, the machine contours a complete
circle. For complete circles, the block must specify the
center with I and J. Programming software must specify
both coordinates accurately. If the ending coordinates for
a circular move are not exactly the same as the starting
coordinates, the path may be a very small arc instead of
a complete circle. To avoid this problem, programs can
omit X and Y from a G02 or G03 block to command a
complete circle; the control will automatically apply the
same starting and ending coordinates.
1-2 EM-423 (R-02/11)
Example: (G91) G03 I3 J0
CL-707 Arc Feedrate Programming
(Original Drive Design)
Model K T0 Tmax
If the syntax is incorrect, the software will display the
CIRCULAR INTERPOLATION SYNTAX ERROR
message.
RECOMMENDED ARC FEEDRATE
Recommended maximum G02 or G03 feedrate depends
on machine design, arc radius, and allowable roundness
error. Use this equation to calculate the maximum
feedrate for each arc:
F = arc feedrate (IPM or mm/min.)
K = constant (1 / min.) See tables.
R = arc radius (inches or mm)
T = roundness tolerance (inches or mm)
T
= minimum radial error (inches or mm)
0
Roundness tolerance “T” is the radial distance between
two concentric circles that enclose the contoured shape.
To use this formula, the specified roundness tolerance
must be greater than “T
” and not more than “Tmax”.
0
4x8 18,000
5x10 18,000
6x12 18,000
.0002 in.
(.005 mm)
.0002 in.
(.005 mm)
.0002 in.
(.005 mm)
.006 in.
(.152 mm)
.006 in.
(.152 mm)
.005 in.
(.127 mm)
Arc feedrate programming parameters in the following
table apply to CL-707 laser systems with Serial
Numbers: 51226, 51242, 51296, 51466, 51509, 51553,
51572, 51631 and higher:
CL-707 Arc Feedrate Programming
(“Fast Pack” Drive Design)
Model K T0 Tmax
4x8 26,500
5x10 26,500
6x12 26,500
8x20 18,000
.0002 in.
(.005 mm)
.0002 in.
(.005 mm)
.0002 in.
(.005 mm)
.001 in.
(.025 mm)
.004 in.
(.102 mm)
.003 in.
(.076 mm)
.003 in.
(.076 mm)
.005 in.
(.127 mm)
CL-7A Arc Feedrate Programming
The maximum acceleration also determines the
maximum feedrate for contouring an arc. The following
tables include that requirement by specifying a
maximum roundness “Tmax” for each value of K. If the
roundness tolerance does not exceed Tmax, then the
calculated feedrate will not command the machine to
exceed the maximum acceleration.
EM-423 (R-02/11) 1-3
Model K T0 Tmax
4x8 6,000
5x10 6,000
6x12 6,000
.001 in.
(.025 mm)
.001 in.
(.025 mm)
.001 in.
(.025 mm)
.005 in.
(.127 mm)
.005 in.
(.127 mm)
.005 in.
(.127 mm)
To determine the feedrate for contouring an arc, compare
the calculated maximum feedrate to a minimum arc
feedrate (typically 30 IPM) and select the higher value.
Then compare the selected value to the material feedrate,
and use the lower value.
1.04 G04 DWELL
The G04 (or G4) command causes the CNC program to
dwell for the time specified by the P argument (in
milliseconds).
Example (to dwell for one second):
G04 P1000
1.31 G31 POSITION CAPTURE
MOVE
This dwell time does not include the block processing
time of the CNC command.
If the software finds a syntax error, a message window
will display “DWELL SYNTAX ERROR”.
1.09 G09 EXACT STOP (ONE
BLOCK)
The program commands G09 (or G9) in the same block
as a G00, G01, G02 or G03 command. When the block
commands G09, the control does not proceed to the next
block until the axes reach zero feedrate. If the block does
not command G09, the control proceeds to the next
block when each axis position is within a specified
distance of the commanded position. The specified
distance is a system parameter.
Example: (G01 X_ Y_ ) G09
If the software finds a syntax error, a message window
will display “PROGRAMMING SYNTAX ERROR”.
1.20 G20 INCH MODE
1.21 G21 METRIC MODE
The G20 command puts the CNC in the inch units mode.
In G20 mode, the control interprets program coordinates
and feedrates in inch system units. (Positions are in
inches and feedrates are in inches per minute).
The G21 command puts the CNC in the metric units
mode. In G21 mode, the control interprets program
coordinates and feedrates in metric system units.
(Positions are in millimeters and feedrates are in
millimeters per minute).
When a program commands G31, the X and Y-axes
move to the specified coordinates in the Work
coordinate system. The G31 command uses the modal
contouring feedrate (F). While the axes are moving, the
control system monitors the Position Capture input. If
the control system receives the Position Capture input, it
records the X and Y-axis Machine coordinates at that
time and stores the values in system variables #5061 and
#5062.
G31 X_ Y_ (F_)
If the control detects more than one Position Capture
input during the move, it only saves the coordinates of
the first occurrence. If the control does not receive the
Position Capture input, it stores the coordinates at the
end of the move. The control always completes the move
to the coordinates specified in the G31 block (unless an
overtravel alarm stops motion).
Position Capture system variables:
#5061 = X axis Machine Coordinate
#5062 = Y axis Machine Coordinate
CINCINNATI macro programs use G31 to find
coordinates associated with optional measurement
functions (Workpiece Edge Detection or Optical Probe).
The machine control does not accept the G31 command
unless the machine configuration includes one of those
options.
1.40 G40 CANCEL KERF
COMPENSATION
1.41 G41 LEFT SIDE
COMPENSATION
The default mode is G20 when the CNC LASER
application starts. After the control runs a program, the
default mode is the same as the last program. To make
sure the control interprets a program correctly, the
program should begin by commanding G20 or G21 to
specify units.
G20 and G21 do not change the units mode of
CINCINNATI control windows. The windows display
values in inch or metric units as selected by the VIEW,
UNITS menu item.
1-4 EM-423 (R-02/11)
1.42 G42 RIGHT SIDE
COMPENSATION
G40 cancels G41 or G42. The cutting nozzle moves
from the compensated position to the commanded
coordinates during the G40 move.
Example: G40
The CNC automatically commands the closest possible
position for the nozzle to contour the programmed shape
with the specified kerf size. If necessary, the control
inserts small moves so compensated paths intersect and
do not over-cut the shape.
Examples:
The control automatically cancels kerf compensation at
the end of any G00 or G53 move if the program
commands G00, G53, M02 or M30 in the next block.
If a program commands G40 in a block by itself, and
then commands a move without G41 or G42, the control
cancels compensation during that move.
A program commands kerf compensation with G41 or
G42. When a G01, G02 or G03 block commands G41 or
G42, the control begins that move with the nozzle offset
to one side of the programmed path. If a block
commands G41 or G42 without commanding a move,
the control ends the previous move with the cutting
nozzle offset to one side of the path.
Example: G41 and G42
1.50 G50 CANCEL SCALING
1.51 G51 WORK COORDINATE
SYSTEM SCALING
The CNC automatically offsets the cutting nozzle by half
the kerf width specified by last G89 command. (See
Section 2.89.)
G40, G41 and G42 form a modal group; the last G-code
commanded in the group is active for all blocks until the
program commands another code in the group. When
each program starts, the default code is G40.
EM-423 (R-02/11) 1-5
G51 X__ Y__ P__
G51 X__ Y__ I__ J__
The control interprets the work coordinate system at a
different scale or as a mirror image when the program
commands G51. The program can restore the normal
scale by commanding G50. When each program starts,
the default mode is G50. The Absolute Position window
and system variables indicate the actual position.
The G51 block defines the center of scaling with X and
Y, and the scale factor with “P”, “I” or “J”. To
command 1.0 scale (where the contoured shape is the
same as the programmed shape), the G51 block uses
P1000 (or I1000 or J1000). The G51 block can use I and
J to command separate scale factors for the X and Y axes
(respectively). To contour a mirror image of the
programmed shape, the block commands I or J with a
negative value. The control does not scale the kerf
compensation offset distance when the program
commands scaling.
Example 1:
G91
G51 X0 Y0 P500
G01 X6
Y4
X-6
Y-4
G50
specified by X and Y in the G52 block. After the G52
block, the program makes contouring moves using the
new coordinate system. To restore the original work
coordinate system, the program commands “G52 X0
Y0”.
G52 X__ Y__
The G52 block does not move the cutting nozzle. The
Absolute Position window changes to indicate the nozzle
position in the temporary coordinate system.
Example 2:
G91
G51 X0 Y0 I-1000
G01 X6
Y4
X-6
Y-4
G50
To demonstrate how a program could use G52, consider
a program that uses a sub-program to contour the same
shape several times, and both the main program and subprogram use G90 (absolute) mode. The main program
would command a work coordinate system with G92 and
the sub-program would command a local coordinate
system with G52, then cancel it with G52 X0 Y0.
1.53 G53 RAPID MOVE TO MACHINE
COORDINATES
G53 X_ Y_
The G53 command moves the cutting nozzle at the rapid
traverse rate to a position specified by X and Y in the
machine coordinate system. G53 is only active in one
block and only in G90 absolute mode. No motion occurs
if the program commands G53 in G91 (incremental)
mode. The control does not change the machine
coordinate system when the program commands kerf
compensation, rotation, scaling, or mirror image, or if
the program changes the work coordinate system.
1.52 G52 LOCAL WORK
COORDINATE SYSTEM
The G52 command temporarily defines a new work
coordinate system while remembering the original. The
zero position of the new (or “local”) coordinate system
is at the coordinates in the original coordinate system
1-6 EM-423 (R-02/11)
1.54 G54 THROUGH G59
WORK COORDINATE SYSTEM SELECTION
A program can use G54 through G59 to command one of
six different pre-defined work coordinate systems. The
user can set the distance from Machine X0 Y0 to the
Work X0 Y0 position of each coordinate system with the
“Position, Work Offset” window, or the program can
assign the distance with system variables #2501 through
#2506 (X) and #2601 through #2606 (Y).
G54 (OFFSET 1)
G55 (OFFSET 2)
G56 (OFFSET 3)
G57 (OFFSET 4)
G58 (OFFSET 5)
G59 (OFFSET 6)
program is in a separate file then the G65 block must
command “P” followed by the sub-program filename
including its extension (if any) and its path if different
from the calling program.
If the G65 command includes arguments, the command
must have a space between the last character of the
program name and the first argument. This is required
because program names can contain both numerals and
alphabetic characters.
A work coordinate system defined with G54 through
G59 does not need G92 to define its X0 Y0 position.
G54 through G59 override G92 by commanding a work
coordinate system with its X0 Y0 position preset on the
machine.
The G54 through G59 block does not move the cutting
nozzle. The absolute position window changes to
indicate the nozzle position in the new work coordinate
system.
If the block contains a syntax error, the control will
display the message “WORK COORDINATE SYNTAX
ERROR”.
1.61 G61 EXACT STOP MODE
1.64 G64 CANCEL EXACT STOP
MODE
G61 commands the CNC to use exact stop mode. In this
mode, the axes decelerate to a stop at the end of every
G00, G01, G02 or G03 block. The CNC remains in G61
mode until the program commands G64 or the program
ends.
The G64 command cancels exact stop mode. The default
mode when each program starts is G64. In G64 mode,
the control proceeds to the next block when each axis
position is within a specified distance of the commanded
position. The specified distance is a system parameter.
1.65 G65 SUB-PROGRAM CALL
(WITH OPTIONAL ARGUMENTS)
The G65 block specifies the sub-program name after
“P”, and may use other arguments to set local variables
in the subprogram.
Note: Revised CNC software (installed July 2001 or
later) does not require a space between the
program number and the first argument if a G65
command specifies P9800 or P9900.
For instructions on calling sub-programs with G65, see
SECTION 5. If the G65 block contains a syntax error,
the control displays the message “G65 SYNTAX
ERROR”.
1.68 G68 WORK COORDINATE
SYSTEM ROTATION
1.69 G69 CANCEL ROTATION
A program can use the G68 command to rotate the work
coordinate system relative to the machine axes. The
command specifies the center of rotation with X and Y
work coordinates (or incremental distances). The
command specifies the amount of rotation with “R” in
degrees, with counterclockwise positive. In G90 mode,
R is the absolute angle of rotation. In G91 mode, R is the
incremental rotation angle that the control adds to any
previous rotation.
G68 X_ Y_ R_
The work coordinate system remains rotated until the
program commands G69 or the program is reset. G69
cancels all coordinate rotation. To cancel only the last
incremental rotation, command G68 in G91 mode with
the opposite amount for “R”.
The G68 or G69 block does not move the cutting nozzle.
The Absolute Position window and System Variables
indicate the nozzle position in the un-rotated work
coordinate system.
G65 P_ (A_ B_ C_ D_ etc. )
The G65 block must include “P” followed by the name
of the sub-program. If the sub-program is in the same
file as the CNC program, then the sub-program name
does not need an extension or path. However, if the sub-
EM-423 (R-02/11) 1-7
Example 1: G68 X0 Y0 R30
X0 Y0 at Machine X0, Y0. The G92 command can
move the work coordinate system to any location.
G92 X_ Y_
X and Y define the new work coordinates corresponding
to the cutting nozzle position when the G92 block is
executed.
The G92 block does not move the cutting nozzle. The
Absolute Position window changes to indicate the nozzle
position in the new work coordinate system.
Example: G92 X0 Y0
Example 2: G68 X5 Y5 R90
1.90 G90 ABSOLUTE MODE
1.91 G91 INCREMENTAL MODE
In G90 absolute mode, the nozzle moves to the
coordinate location specified by the arguments in a G00,
G01, G02, G03 or G53 command. G90 mode is active
until the program commands G91 mode. When each
program starts, the default mode is G90.
The G92 X0 Y0 command moves the work coordinate
system X0 Y0 location to the current position of the
cutting nozzle. Programmers often use this command to
begin a sub-program written in G90 mode.
G92 Example:
In G90 mode, X and Y coordinate values are modal. In
other words, if a block does not specify X or Y, the
control uses the last commanded value for X or Y.
In G91 incremental mode, the cutting nozzle moves a
distance from its starting location specified by X and Y
in a G00, G01, G02 or G03 command. G91 mode is
active until the program commands G90 or the program
ends. The control ignores a G53 command while
operating in G91 mode.
1.92 G92 WORK COORDINATE
SYSTEM SETTING
This command sets the work coordinate system location.
When the machine completes the Axes Home operation,
the control establishes the work coordinate system with
1-8 EM-423 (R-02/11)
EM-423 (R-02/11) 1-9
1-10 EM-423 (R-02/11)
SECTION 2 CUSTOM G-CODES
The CINCINNATI control has built-in functions
programmed with custom G-Codes.
CODE DESCRIPTION SEC.
G84 Pierce and Start Cut 2.84
G85 Start Cut without Pierce 2.85
G89 Process Parameters 2.89
G102 Additional Parameters 2.102
G103 Ramped Pierce Parameters 2.103
G120 Disable Non-Stop Cutting 2.120
G121 Enable Non-Stop Cutting 2.121
G123 Programmable Blend 2.123
G124 Default Blend 2.124
G125 Auto Blend 2.125
2.84 G84 PIERCE AND START CUT
2.85 G85 START CUT WITHOUT
PIERCE
A program uses G84 or G85 to begin user-programmed
cutting sequences. G84 and G85 command the Z-axis to
move the nozzle down to the standoff position (if not
already there), and then command the pierce and/or cut
parameters. When the control finishes the G84 or G85
command, it returns to the program with the laser beam
on, assist gas on, and shutter open, ready to proceed with
contouring commands (G01, G02, G03). G84 and G85
also turn coolant on if the process parameters specify
coolant.
A program uses G85 to begin a cut sequence when the
application does not require the pierce cycle of G84.
G85 duplicates all other functions of G84, including
precut dwell and power burst time (see G102
description). After a program commands processing
parameters with G89, any cut sequence can start with
G84 or G85. Examples of G85 applications are: starting
a cut inside an opening, off the edge of the sheet, or in a
kerf.
AUTO RESTART
Tracing Function Forward or Reverse button to move in
the forward or reverse direction to another program
block. De-select Tracing mode and then press Cycle
Start to resume the cut. If an alarm condition interrupts
a program and the operator presses Cycle Start without
selecting Tracing mode, the cutting nozzle moves to the
start of the interrupted block and resumes cutting.
PIERCE OPTIONS (G84 T_)
Each process parameter library file has one set of cutting
parameters and three pierce options. The G84 “T”
argument selects the pierce option for each cutting path.
Normal Pierce G84 or G84 T1:
G84 T1 is the same command as G84. The program
commands normal pierce parameters with a G89 library
file, or explicitly with G89, G102 and G103 macro calls.
Rapid Pierce G84 T2:
The program commands G84 T2 to use rapid pierce.
Rapid pierce has separate laser power, gas pressure,
dwell time and standoff parameters. Laser pulse mode is
always 5000 Hz and 100% duty cycle. G84 T2 uses the
same assist gas (#1 or #2) and part coolant status as
normal pierce.
Rapid pierce uses a single power level during the pierce,
so ramped pierce is always OFF. Rapid pierce also has a
cooling time parameter independent from G84 T1 and
airblast time parameters.
G89 loads rapid pierce parameters from a library file.
The NC program cannot set rapid pierce parameters
explicitly with G89, G102 or G103. When the program
commands normal pierce parameters explicitly, the
default T2 parameters are the same as T1.
G84 T3:
G84 T3 operates the same as G85 (no pierce).
Note: All G84 pierce options (T1, T2 or T3) command
pre-cut dwell before returning to the program.
For a description of pre-cut dwell, see G102 in
this section.
When a laser system has the CINCINNATI control, the
CNC program does not require special codes or
commands to activate Auto Restart. When an alarm
condition interrupts a program, the operator can restart
the program at any block. After correcting the condition
that caused the interruption, the operator can select
Tracing mode, press Cycle Start, then hold down the
EM-423 (R-02/11) 2-1
AIRBLAST
The rapid pierce process uses a separate blast of
compressed air to help clear molten material from the
pierce area. Two airblast parameters (“OFF time” and
“ON time”) control the opening of the airblast solenoid
valve.
The OFF time is a delay that starts when the pierce
begins. The air valve is closed during the OFF time.
When the delay ends, the air solenoid valve opens. The
valve then stays open for the ON time. To edit the
airblast times, open the Process Library Window.
The following figures show the function of G84 T1 and
T2 parameters:
2.89 G89 PROCESS PARAMETERS
The program sets processing parameters by commanding
G89. When G89 loads processing parameters with a
library file, the operator can edit the parameters while
the program is running; however, changes will NOT take
effect until the next G84 (or G85). To change
parameters, open the library file, edit the parameter(s)
then save the library file.
The CINCINNATI control will also accept G89, G102
and G103 commands programmed with explicit
parameters.
G89 WITH LIBRARY FILE
G89 Pfilename.lib
The G89 command uses address “P” to specify a library
file. The operator can edit library files in the Process
Parameter window. The default path is:
D:\CNCLSR32\MATERIAL\
The filename must include the “.lib” extension.
If the library file is not in the MATERIAL folder, the
G89 command must include the path. The user can
create other library directories, in either the MATERIAL
folder or elsewhere on the disk.
CINCINNATI INCORPORATED provides a set of
read-only library files in this folder:
“D:\CNCLSR32\MATERIAL\ARCHIVE\”
The MATERIAL directory includes copies of the same
library files, which the user can edit.
Library filenames provided by CINCINNATI
INCORPORATED begin with an abbreviation for
material:
AL . . . Aluminum
MS . . . Mild Steel
SS . . . Stainless Steel
After the material abbreviation, the library filename has
a three-digit number representing the material thickness
in mils.
Example: (For 10 gauge mild steel 0.135”): MS135
The filename may include other characters after the
thickness number, to indicate a resonator type or
processing application.
After the thickness number, the filename may have a
chemical abbreviation for the cutting assist gas:
2-2 EM-423 (R-02/11)
O2 . . . Oxygen
N2 . . . Nitrogen
For applications using coolant, the library filename ends
with the word “wet”.
Examples: (10 gauge mild steel, oxygen cut)
Without coolant: MS135O2.lib
With coolant: MS135O2wet.lib
When pulsed laser output is used, frequency and
duty cycle are specified with a 4-digit code in which
the first two digits specify frequency (Hz/100) and
the last two digits specify duty cycle (%).
For DC (diffusion-cooled) resonator, maximum
frequency is 5000 Hz and minimum duty cycle is the
value necessary for a pulse ON time of 26
microseconds at the commanded frequency.
G89 CALL WITH ARGUMENTS:
G89 T_ A_ I_ M_ S_ C_ D_ Q_ B_ E_ H_ R_ J_
K_ U_ V_
T = Cut power level, watts.
A = Cut gas code. See Note 1.
I = Cut gas pressure. See Note 2.
M = Cut laser mode, see Note 3.
S = Cut pulse code, see Note 4.
C = Cut coolant code. See Note 5.
D = Pierce time, seconds.
Q = Pierce power level, watts.
B = Pierce gas code. See Note 1.
E = Pierce gas pressure. See Note 2.
H = Pierce laser mode, see Note 3.
R = Pierce pulse code, see Note 4.
J = Pierce coolant code. See Note 5.
K = Kerf width, see Note 2.
U = Maximum feedrate for Dynamic Power, see Note 2.
V = Minimum percent for Dynamic Power (% at zero
feedrate)
Notes:
1. Assist gas codes (A & B):
11 = Gas Port #1 (usually O2)
12 = Gas Port #2 (usually N2)
2. G89 interprets pressures, kerf width, and dynamic
power feedrate in the active units:
Parameter G20 unit G21 unit
I & E PSI kPa
K inches mm
U IPM mm/min
5. Coolant codes (C & J):
8 = coolant ON
9 = coolant OFF
When CINCINNATI laser systems with Fanuc control
have the Macro Executor option, programs written for
those laser systems can specify process parameters with
G89 X_, where X is followed by a library code number
from 1 to 100. The CINCINNATI control will accept a
program with the “G89 X” command (instead of G89 P),
if the Material folder has a library file with the same
name as the number following “X”. For example, the
CINCINNATI control will accept a program
commanding “G89 X32” if the Material folder has a
library file named “32.lib”.
When a program commands G89, G102 or G103 with
explicit parameters, the CINCINNATI control checks
the parameters for out-of-range values. If the control
finds any, it displays an error message in a pop-up
window indicating which parameter has the error. The
window identifies parameters by the name used in the
Process Parameter Library window, not by the G89,
G102 or G103 argument. For example, “Pierce Gas
Pressure out-of-range” instead of “G89 E out-of-range”.
2.102 G102 ADDITIONAL
PARAMETER SETTINGS
The Parameter Library window includes settings for
dynamic gas pressure, noncontact standoff, optional
pressure, precut dwell and power burst time. In addition
to commanding these parameters in a library file with
G89, the program can also command these parameters
explicitly with G102.
G102 A_ B_ S_ Z_ D_ I_ T_ Q_ R_ U_ V_
3. Laser mode (M & H):
61 = Continuous Wave
62 = Gated Pulse
66 = Dynamic Power
4. Pulse codes (S and R):
EM-423 (R-02/11) 2-3
A = Dynamic gas pressure near field setting
B = Dynamic gas pressure far field setting
S = Pierce standoff
Z = Cut standoff
D = Precut dwell, seconds
I = Optional pressure
T = Power burst time, seconds
Q = Pierce Focus, Near Field
R = Pierce Focus, Far Field
U = Cut Focus, Near Field
V = Cut Focus, Far Field
G102 interprets pressure, standoff and focus settings in
the active units:
Parameters G20 unit G21 unit
A, B & I PSI kPa
S & Z inches mm
Q, R, U & V inches mm
A & B: When a program commands dynamic gas
pressure, the control regulates cutting assist gas
pressure between the Near (A) and Far (B) field
settings based on the machine position of the nozzle.
Near field is where the laser beam length is shortest.
S & Z: The program uses these settings to command
pierce and cut nozzle standoff distance for the
noncontact head.
G103 A_ B_ C_ D_ E_ F_ Q_ R_ S_ T_ U_ V_ W_
A = Ramp 1 duration, seconds
B = Ramp 2 duration, seconds
C = Ramp 3 duration, seconds
D = Ramp 4 duration, seconds
E = Ramp 5 duration, seconds
F = Tip cooling time, seconds
Q = Number of ramp steps (1 to 5)
R = Percent power at start of first ramp
S = Percent power at start of second ramp
T = Percent power at start of third ramp
U = Percent power at start of fourth ramp
V = Percent power at start of fifth ramp
W = Percent power at end of fifth ramp
D: Before returning to the program, G84 and G85
command the cutting parameters and then command
the pre-cut dwell.
I: The assist gas pressure controller uses the optional
pressure setting when a program commands M67.
T: When the laser system starts a contouring move using
dynamic power, the control maintains dynamic power
at 100% for the time specified for Power Burst. After
the Power Burst time, the control regulates dynamic
power according to the actual feedrate.
Q, R, U and V: When CL-707 lasers or CL-7A lasers
with CINCINNATI control have the Auto Focus
Cutting Head option, the G102 command has
additional arguments to specify focus settings. The
settings specify focus position relative to the nozzle
tip. The Auto Focus drive uses the Near field settings
when the cutting head is closest to the laser source,
and changes focus between the Near and Far settings
as X and Y-axis motion changes the optical path
length. Q and R specify the Near and Far field pierce
focus settings. U and V specify the Near and Far
field cut focus settings.
2.103 G103 RAMPED PIERCE
SETTINGS
To set parameters for ramped pierce power, the CNC
program can either command G89 with a library file, or
command G103 with explicit settings.
G103 Ramped Pierce Arguments
2.120 G120 DISABLE NON-STOP
CUTTING
2.121 G121 ENABLE NON-STOP
CUTTING
When a program commands Non-Stop Cutting (G121),
the CNC replaces short G00 moves between cut
sequences with “Smart Rapid” moves. A Smart Rapid
move commands the laser beam off and on without
stopping the axes. (See Smart Rapids description below.)
During a Smart Rapid move, the control maintains assist
gas flow, even when the laser beam is off.
Notes: A program can only command Non-Stop cutting
mode when the process parameters specify no
pierce time and no precut dwell.
2-4 EM-423 (R-02/11)
Loading...