Siemens SINUMERIK 840D sl Programming Manual page 235

Workpiece probe 1, used as tool T9, D1, is
to be used.
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_ANGLEMEAS_MPF
N10 G54 G17 G90 T9 D1
N20 M6
N30 G0 C0
N40 X-20 Y-40
N50 Z40
N60 _PRNUM=1 _VMS=0 _NMSP=1 _EVNUM=0
N61 _MVAR=105 _SETVAL=-18 _MA=102
_ID=40 _RA=4 _KNUM=1 _STA1=0 _TSA=5
_FA=8
N70 CYCLE998
N80 G0 Z160
N90 G54 C0
N100 M2
Explanation of example
Measurement is performed in the Y direction, offset is in X direction, intermediate position at
an angle. The cycle determines the measuring direction from the actual position in the Y
direction and _SETVAL.
Automatic correction is performed in G54, offset in the C axis (4th channel axis) with the
calculated angle (_STA1=0).
In block N90, the corrected ZO G54 is activated and the C axis is moved from position zero
to position zero; the ZO difference is eliminated. The workpiece is then paraxial.
The results are entered in result array _OVR[ ].
Measuring cycles
Programming Manual, Release 04/2006, 6FC5398-4BP10-0BA0
Measuring Cycles for Milling and Machining Centers
5.7 CYCLE998 workpiece: Angle measurement and ZO determination
710
L1 = 50.000
R = 3.000
;Select T No. probe
;Insert probe as tool,
;activate offset
;Position rotary table at 0°
;Position probe in X/Y plane opposite
;measuring point
;Z axis at measurement height
;Set parameters for measuring cycle call
;Measuring cycle for angle measurement
;Traverse up Z axis
;Repeat call of ZO G54
;The changes thereby take effect!
;Position rotary table at 0°
;(edge is now setup).
;End of program
5-101