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).

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 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.