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 postprocessor 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).


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 postprocessor in the multiaxis output mode (to process the i,j,k vector). When in multiaxis 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 4Axis Wire EDM only.

z2 = the highest midpoint 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 / AAXISBAXIS CAXIS, INCR, a, CLWCCLW

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 = counterclockwise 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, CLWCCLW, MAXRPM, m, RANGE, r
SPINDL / SFM or SMM, v, CLW CCLW, MAXRPM, m, RANGE, r
SPINDL / ON
SPINDL / OFF
SPINDL / PARLEL, XAXISZAXIS (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 for tool axis in Wire EDM, if CL_OUTPUT_MODE is set to TAPER\

NOW—Update the tool axis position at the current point (available for 2 Axis Wire EDM only).
NEXT (default)—Update the tool axis position at 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 ().


UNITS / u

length units used for the NC sequence (INCHES, MM, etc.)


VERIFY / CORNER, PNT, RCTNGL, ROUND, XYZ

probe statements.
