Programming Example - Siemens SINUMERIK 840D sl Programming Manual

6.5.2.2

Programming example

ZO calculation at a workpiece
The intention is to determine the zero offset in the Z axis on a clamped workpiece with
workpiece probe 1, inserted as tool T8, D1. The position determined should retain the value
60 mm in the new workpiece with G54. Measurement is also performed with G54.
The probe is already calibrated and the tool data are entered in T8, D1:
Tool type (DP1):
Cutting edge position (DP2):
Length 1 - geometry (DP3):
Length 2 - geometry (DP4):
Radius - geometry (DP6):
Zero offset, with settable ZO G54: NVz
%_N_ZO_DETERMINING_1_MPF
N10 G54 G90 G18 DIAMON T8 D1
N20 G0 X36 Z100
N30 _MVAR=100 _SETVAL=60 _MA=1 _TSA=1 _KNUM=1
_EVNUM=0 _PRNUM=1 _VMS=0 _NMSP=1 _FA=1
N40 CYCLE974
N50 G0 Z100
N60 X114
N100 M2
Note
If parameter _VMS has value 0, the default value of the measuring cycle is used for the
variable measuring velocity:
if _FA=1: 150 mm/min
if _FA>1: 300 mm/min
(see section "Description of the most important defining parameters")
Measuring cycles
Programming Manual, 03/2009 Edition, 6FC5398-4BP10-2BA0
Measuring Cycles for Turning Machines
6.5 CYCLE974 workpiece: 1-point measurement
580
7
L1 = 40.123
L2 =
100.456
3.000
;Call ZO, tool = probe
;Starting position before cycle call
;Parameters for cycle call
;Measurement in the Z-direction
;Retraction in Z
;Retraction in X
;End of program
337