Programming Example - Siemens SINUMERIK 840D sl Programming Manual

Measuring Cycles for Milling and Machining Centers
5.6 CYCLE979 workpiece: Measure hole/shaft/groove/rib at an angle
5.6.3.2

Programming example

Measuring a hole with CYCLE979
The trueness of a circular segment in plane G17 (semi-circle, contour element "hole") is to
be checked. Machining was performed with milling tool T20, D1.
With a variance of >0.01 mm from the setpoint diameter _SETVAL = 130 mm, the tool radius
of this tool should be automatically offset in the wear. The maximum permissible deviation is
taken as max. 1 mm. To obtain a minimum measuring path of 1 mm to the contour, the
measuring path is specified as _FA = 1+1 =2 mm (max. total measuring path = 4 mm).
The center point of the circular segment (setpoint) is X = 180 mm, Y = 0 mm (_CPA, _CPO).
Measurement is to be performed with three-point measurement at a measuring height of Z =
20 mm at initial angle 15° and following angles 80°.
Traversing between points is carried out with a circular feed of _RF= 900 mm/min.
The offset must take the empirical value in memory _EV[19] into consideration. Mean value
calculation _MV[19] and inclusion in calculation are also to be used.
This tool offset will therefore affect the production of the next workpieces or possible
remachining.
Clamping for workpiece:
Zero offset, with settable ZO G54: NVx, NVy, ...
The probe is already calibrated. Arrays for workpiece probe 1: _WP[0, ...]
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.
5-90
710
L1 = 50.000
R = 3.000
Programming Manual, Release 04/2006, 6FC5398-4BP10-0BA0
Measuring cycles