Siemens SINUMERIK 840D sl Programming Manual page 365

Calibration with workpiece probe CYCLE973, measurement of workpiece with CYCLE974
%_N_PART_1_MEAS_MPF
N10 T8 D1 DIAMON
N20 SUPA G0 X300 Z150
N30 _MVAR=13 _MA=1 _MD=1 _CALNUM=1 _TZL=0
_TSA=1 _PRNUM=1 _VMS=0 _NMSP=1 _FA=1
N40 CYCLE973
N50 _MA=2
N60 CYCLE973
N70 G54 G0 Z40
N80 X220
N100 _TUL=0 _TLL=-0.01 _TZL=0.002
_EVNUM=0 _TDIF=0.2 _TSA=0.3 _PRNUM=1
_MVAR=0 _SETVAL=200 _MA=2 _TNUM=1 _KNUM=1
N110 CYCLE974
N120 G0 Z70
N130 X175
N140 _MA=1 _SETVAL=50 _TUL=0.01 _TNUM=2
_KNUM=1
N150 CYCLE974
N160 G0 Z180
N170 _MA=2 _SETVAL=150 _TUL=0.005
_TLL=-0.003 _TNUM=3 _KNUM=1
N180 CYCLE974
N190 G0 Z150
N200 X50
N210 _MA=1 _SETVAL=100 _TUL=0.01
_TLL=-0.01 _TNUM=4 _KNUM=1
N220 CYCLE974
N230 G0 SUPA Z250
N240 SUPA X280
N300 M2
Measuring cycles
Programming Manual, Release 04/2006, 6FC5398-4BP10-0BA0
Measuring Cycles for Turning Machines
6.7 Complex example for tool measurement
;Select tool = probe
;Approach starting position in X and Z,
from
;which it is possible to approach the
reference groove
;for calibration without collision
;Parameters for calibration in ref.
groove
;Calibrate probe in the minus Z direction
;Another measuring axis
;Calibrate probe in the minus X direction
;Select work offset, traverse to
measuring
;point in the Z axis
;Position probe facing P 1
;Define parameters for measurement
;Measure P1
;Position probe facing P2
;Define parameters for measurement in
;another axis
;Measure P2
;Position probe opposite P3
;Change parameters for measurement
;Measure P3
;Position probe opposite P4
;Change parameters for measurement
;Measure P4
;Retraction in Z
;Retraction in X
;End of program
6-89