Programming Example - Siemens SINUMERIK 840D sl Programming Manual

6.4.2.2

Programming example

Calibrate workpiece probe in reference groove
The workpiece probe 1 with cutting edge position SL=7 is to be calibrated in reference
groove 1 in both axes and in both directions in X. The probe is inserted as tool T8, D1.
Probe lengths L1 and L2 always refer to the probe ball center and must be entered in the
tool offset memory before the measuring cycle is called, T8, D1:
Tool type (DP1):
Cutting edge position (DP2):
Length 1 - geometry (DP3):
Length 2 - geometry (DP4):
Radius - geometry (DP6):
The data for reference groove 1 have already been entered:
_KB[0,0] = 60.123, _KB[0,1] = 50.054,
_KB[0,2] = 15.021
%_N_CALIBRATE_IN_GROOVE_MPF
N10 T8 D1
N20 G0 SUPA G90 DIAMOF Z125 X95
N30 _TZL=0 _TSA=1 _VMS=0 _NMSP=1 _FA=3 _PRNUM=1
N31 _MVAR=13 _MA=1 _MD=1 _CALNUM=1
N40 CYCLE973
N50 _MVAR=02013 _MA=2
N60 CYCLE973
N70 G0 SUPA Z125
N80 SUPA X95
N100 M2
Explanation of example
The cycle automatically approaches reference groove 1 from the starting position and
performs calibration in both axes and in the X axis in a double cycle call. The new trigger
values are stored in the data of the workpiece probe 1 _WP[0,1], _WP[0,3], _WP[0,4].
At the end, result array _OVR[ ] contains the values of the 2nd cycle call.
Measuring cycles
Programming Manual, Release 04/2006, 6FC5398-4BP10-0BA0
Measuring Cycles for Turning Machines
6.4 CYCLE973 Calibrating workpiece probes
580
7
L1 = 40.123
L2 =
100.456
3.000
;Tool offset of the probe
;Position in front of cycle call
;(start position),
;position without ZO
;Set parameters for calibration,
;minus Z-direction
; Cycle call
;In X axis, both directions
; Cycle call
;Retraction in Z
;Retraction in X
;End of program
6-61