Siemens SINUMERIK 840D sl Programming Manual page 190

Measuring Cycles for Milling and Machining Centers
5.4 CYCLE977 workpiece: Measure hole/shaft/groove/web/rectangle parallel to axes
The probe is already calibrated. Arrays for
workpiece probe 1: _WP[0, ...]
The following is entered under T9, D1 in
the tool offset memory:
Tool type (DP1):
Length 1 - geometry (DP3):
Radius - geometry (DP6):
Length 1 (L1) must refer to the center of
the probe ball (_CBIT[14]=0), as for
calibration.
Careful when positioning! Radius R in
length (L1) is ignored.
%_N_WEB_MEASURE_MPF
N10 G54 G17 G90 T9 D1
N20 M6
N30 G0 X220 Y130
N40 Z101
N60 _TSA=1.2 _PRNUM=1 _VMS=0 _NMSP=1
_FA=4
N61 _MVAR=104 _SETVAL=132 _MA=1 _ID=-
40 _KNUM=0
N70 CYCLE977
N80 G0 Z160
N100 M2
Explanation of example
The measuring results of web width, web center in X, and associated differences are entered
in result array _OVR[ ]. If the difference in the position of the web center is >1.2 mm
(_TSA=1.2) an alarm is output. Only cancellation with NC RESET is then possible.
The setpoint of the web center is the position of the probe in the workpiece coordinate
system at the beginning of the cycle in the X axis.
5-56
710
L1 = 50.000
R = 3.000
;ZO, select tool as probe ...
;Insert probe,
;activate tool offset
;Position probe in X/Y plane at setpoint web
center
;position in X and measurement position Y
;Position Z axis above web
;Set parameter for measuring cycle call
;with ZO and without tool compensation,
;note negative prefix for _ID!
;Probe lowered in Z axis!
;Measuring variant with ZO calculation has
been
;selected (MVAR=X1xxx) because web center
;is to be monitored (with _TSA),
;but KNUM=0: without running
;the ZO calculation and ZO compensation
;Call measuring cycle
;Traverse up Z axis
;End of program
Programming Manual, Release 04/2006, 6FC5398-4BP10-0BA0
Measuring cycles