Manufacturing > CL Output > Supported CL Data Commands
Supported CL Data Commands
$$—any line or portion of a line preceded by "$$" is a comment or command for the use of Creo NC.
Command
Description
Attributes
CALSUB/a
where:
a=subroutine name.
CIRCLE/ x, y, z {, i, j, k} , r
output for circular interpolated tool movement
COOLNT / type, pressure
where:
type = ON, OFF, FLOOD, MIST, TAP, or THRU.
pressure = LOW, MEDIUM, or HIGH (if the value for the COOLANT_PRESSURE parameter is NONE, it will not be output).
CUTCOM / LEFT {,n}
where:
LEFT, RIGHT = the direction of cutter compensation offset.
n = the number of the register of the machine controller that holds the tool compensation data. If CUTCOM_REGISTER is 0, it is not output.
CUTCOM / RIGHT {,n}
CUTCOM / OFF
CYCLE / type
output for Holemaking cycles
DEFSUB / a
start of a subroutine definition
where:
a = subroutine name (by default, the number of the corresponding NC sequence).
DELAY / t
where:
t = delay in seconds
DMIS / a
enables or disables the processing of DMIS statements
where:
a = ON or OFF
ENDSUB
end of a subroutine definition
FEDRAT/f,units
where:
f = feedrate value in the specified units.
units = units for feedrate. Can be FPM, IPM, FPR, IPR, MMPM, MMPR.
FEDRAT / INVERS, AUTO
specifies the inverse time feed rate, or the rate of rotation, for machines with rotary axes (if you set INVERSE_FEED to YES)
FEDRAT / INVERS, OFF
output at the end of an NC sequence with inverse time feed rate.
FINI
last statement in the program.
FLUSH / ON, a
where:
a = flush register (if specified)
FROM / x, y, z {, i, j, k}
where:
x, y, z—coordinates of the tool control point.i, j, k—the tool axis vector.
GENRTR / genrtr register
GOTO / x, y, z {, i, j, k}
where:
x, y, z—coordinates of the tool control point.i, j, k—the tool axis vector.
HEAD / n, OPTION, #
output for multiple turrets
HEAD / BOTH
output before a pair of synchronized NC sequences.
HEAD / OFF
output after a pair of synchronized NC sequences.
LINTOL / r
where:
r—the value of the manufacturing parameter LINTOL. Used by post-processor for interpolation. Will be output only if the LINTOL parameter value is other than dash (-).
LOADTL / n, LENGTH, l, OSETNO, o
where:
n = TOOL_POSITION (defined using the tool table). If the tool is not included in the tool table, its TOOL_ID (as set in the parameters file) will be used.
LENGTH, l = gauge length value for a tool. Will be output only if GAUGE_Z_LENGTH is other than dash (-).
OSETNO, o = tool offset change specified in the tool table (if any).
* 
When a sequence uses MULTI TIP type of tools, OSETNO -3 is output for cancelling the tool offset.
MACHIN / name, m
where:
name = the NC sequence parameter MACH_NAME
m = the NC sequence parameter MACH_ID
MODE/INCR and MODE/ABSOL
output inside subroutine definitions to make the post transform the subroutine data into incremental data.
MODE/MILL and MODE/TURN
output for the Mill/Turn centers.
MULTAX / ON
puts the post-processor in the multi-axis output mode (to process the i,j,k vector). When in multi-axis output mode, Creo NC outputs the i,j,k vector even when the tool is in 0, 0, 1 orientation.
OP / THREAD, TURN, DEPTH, totdepth, TPI, thread_feed, MULTRD, t, CUTS, c, FINCUT, n, CUTANG, a
ISO output for Thread Turning.
where:
DEPTH, totdepth = the depth of cut for the thread.
TPI (or MMPR, or IPR), thread_feed = thread pitch (parameters THREAD_FEED_UNITS, THREAD_FEED).
MULTRD, t = number of threading starts in multiple start threading.
CUTS, c = the number of times the tool is positioned to a multiple cut (parameter NUMBER_CUTS).
FINCUT, n = the number of passes made at the final thread depth (NUMBER_FIN_PASSES).
CUTANG, a = angle at which the tool begins the cut (INFEED_ANGLE).
OP / THREAD, NOMORE
designates the end of ISO thread output
PARTNO
part name
PIVOTZ / z2, z1, z2, z1, z1
output for 4-Axis Wire EDM only.
z2 = the highest mid-point of the surfaces traversed
PPRINT
output model information. In order to issue this command, you have to set up the PPRINT table.
PROBE / ON, OFF, RANGE, CALIB
probe statements.
RAPID
next motion statement will be a rapid traverse feed.
ROTATE / AAXIS|BAXIS| CAXIS, INCR, a, CLW|CCLW
rotational transition between the Machine and NC Sequence coordinate systems if CL_DATA_MODE is TRANS_ROTABL
where:
AAXIS, BAXIS, CAXIS—rotate about X, Y, or Z axis respectively.
a = rotation angle value.
CLW = clockwise motion.
CCLW = counter-clockwise motion.
SET / HOLDER , adaptor_number, SETOOL, xoffset, yoffset, zoffset, ATANGL, at, SETANG, st
output when using a tool attachment
where:
adaptor_number = value of the attachment model parameter ADAPTOR_NUMBER
xoffset, yoffset and zoffset define the position of the tool attach point with respect to the spindle control point
at = ZF rotation of the tool axis in degrees with respect to the SPINDLE_CONTROL_POINT coordinate system.
st = XY rotation of the tool axis in degrees with respect to the SPINDLE_CONTROL_POINT coordinate system.
SET / OFSETL, n and SET / OFSETL, OFF
where:
n = FIXT_OFFSET_REG
output only if the FIXT_OFFSET_REG parameter value is other than dash (-).
SPINDL / RPM, s, CLW|CCLW, MAXRPM, m, RANGE, r
SPINDL / SFM or SMM, v, CLW| CCLW, MAXRPM, m, RANGE, r
SPINDL / ON
SPINDL / OFF
SPINDL / PARLEL, XAXIS|ZAXIS (Mill/Turn milling only)
SPINDL / ORIENT
TRANS / X, Y, Z
CSYS / X1, Y1, Z1, V1,
X2, Y2, Z2, V2,
m = MAX_SPINDLE_RPM. If MAX_SPINDLE_RPM is set to dash (-), "MAXRPM, m" will not be output.
r = range value
(SPINDLE_RANGE). Can be LOW, MEDIUM, HIGH. If SPINDLE_RANGE is NUMBER, then r is equal to the RANGE_NUMBER parameter value. If SPINDLE_RANGE is NO_RANGE, "RANGE, r" will not be output.
PARLEL indicates which axis the milling spindle is parallel to.
ORIENT indicates the ORIENT_ANGLE set for the tool. For example, while boring, this indicates the orientation of a boring bar before retract.
STAN / a, [ LEAD | LAG, b ], [ NOW | NEXT ]
Output STAN, NOW, NEXT statement for 2-Axis Contouring Wire EDM when the Taper Angle option on the INT CUT menu is specified.
Output STAN, LEAD LAG, NEXT statement for 4-Axis Contouring Wire EDM when the CL_OUTPUT_MODE parameter is set to TAPER.
STAN /a specifies an angle perpendicular to the direction of motion. For example, if the bottom wire guide moves along the X-axis direction, then a is the angle of rotation for the wire around the X-axis.
LEAD b specifies an angle in the direction of motion. For example, if the bottom wire guide moves along the X-axis direction, then b is the angle of rotation for the wire around the Y-axis. A positive value for b indicates that the upper wire guide is ahead of the bottom wire guide by b degree.
LAG b specifies an angle in the direction of motion. For example, if the bottom wire guide moves along the X-axis direction, then b is the angle of rotation for the wire around the Y-axis. A positive value for b indicates that the upper wire guide is behind the bottom wire guide by b degree.
NOW—Update the tool axis position at the current point.
NEXT (default for 2-Axis Wire EDM)—Update the tool axis position at the next GOTO point. For example, both the bottom wire guide and upper wire guide move simultaneously to achieve a and b angles at the end of the next GOTO point.
THREAD/AUTO, x1, y1, z1, TO, x2, y2, z2, TPI, thread_feed, AT, percent, DEEP, depth, LAST, n, TYPE, 0, totdepth, angle, IPM, ipm, FEDTO, d, x, TIMES, t, OFSETL, n, o
AI Macro output for Thread Turning,
where:
TPI(or MMPR, or IPR), thread_feed = thread pitch (parameters THREAD_FEED_UNITS, THREAD_FEED).
AT, percent = the percentage of remaining metal to be removed with each pass (PERCENT_DEPTH).
DEEP, depth = determines the final programmed thread depth (STOCK_ALLOW).
LAST, n = the number of passes made at the final thread depth (NUMBER_FIN_PASSES).
TYPE, 0, totdepth, angle = provides thread depth and infeed angle.
IPM, ipm = feedrate used during each threading cycle.
FEDTO, d = the clearance distance from the workpiece.
x = IN (internal thread), OUT (external thread—default), FACE (facing thread).
TIMES, t = the number of threading starts.
OFSETL
n = the number of times the tool is positioned to a multiple cut
.o = offset distance between each of the cuts.
TRANS / x, y, z
linear translation between the Machine and NC Sequence coordinate systems if CL_DATA_MODE is TRANS_ROTABL.
Will be commented out if the FIX_OFFSET_REGISTER parameter value is set to default dash (-).
TURRET / n, XAXIS, x, ZAXIS, z, OSETNO, o
output for turning NC sequences, and for Mill and Holemaking NC sequences performed on lathes and Mill/Turn centers, instead of LOADTL."XAXIS, x" and "ZAXIS, z" will only be output if GAUGE_X_LENGTH and GAUGE_Z_LENGTH for the tool are other than dash (-).
* 
When a sequence uses MULTI TIP type of tools, OSETNO -3 is output for cancelling the tool offset.
UNITS / u
length units used for the NC sequence (INCHES, MM, etc.)
VERIFY / CORNER, PNT, RCTNGL, ROUND, XYZ
probe statements.
Was this helpful?