Siemens SINUMERIK 840D sl Programming Manual page 170

Measuring Cycles for Milling and Machining Centers
5.5 CYCLE978 workpiece: Measuring a surface parallel to the axis
Workpiece probe 1, used as tool T9, D1, is
to be used.
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_ONE_POINT_MEASURE_MPF
N10 G54 G17 G90 T9 D1
N20 M6
N30 G0 G90 X120 Y150
N40 Z40
N50 _CHBIT[4]=1
N60 _TUL=0.03 _TLL=-0.03 _TNUM=20
_EVNUM=20 _K=3 _TZL=0.01 _TMV=0.02
_TDIF=0.06 _TSA=1 _PRNUM=1 _VMS=0
_NMSP=1 _FA=2
N61 _MVAR=0 _SETVAL=100 _MA=1
_KNUM=2001
N70 CYCLE978
N80 G0 Z160
N100 M2
170
710
L1 = 50.000
R = 3.000
;ZO, select tool as probe ...
;Insert probe,
;activate tool offset
;Position probe in X/Y plane in front of
;measuring surface
;Position probe at measuring height
;with mean value calculation
;Set parameters for measuring cycle call
;Measuring cycle for 1-point measurement in
;X axis
;Traverse up Z axis
;End of program
Programming Manual, 03/2009 Edition, 6FC5398-4BP10-2BA0
Measuring cycles