Siemens SINUMERIK 840D sl Programming Manual page 148

Measuring Cycles for Milling and Machining Centers
5.2 CYCLE971 tool: Measuring milling tools, drills
%_N_CALIBRATE_MTT_X_MPF
N05 G0 G17 G94 G54
N10 T7 D1
N15 M6
N30 G0 Z100
N35 X70 Y90
N40 _TZL=0.005 _TSA=5 _VMS=0 _NMSP=1
_PRNUM=1 _FA=6
N41 _MVAR=10 _MA=1
N50 CYCLE971
N55 Z100
N60 M2
Explanation of example 2
The calibration tool moves with its point from the starting position at
N35 (X70, Y90, Z100) in Y to the center of the probe Y31 ((_TPW[0,2] + (_TPW[0,3]) /
2 = (42+20) / 2=31)); then in the measuring axis X (_MA=1, G17) to position X61 (_TPW[0,0]
+ _FA + R = 50 + 6 + 5 = 61). Here it is lowered to position
Z76 (_TPW[0,4] - _TPW[0,9] = 80 - 4 = 76). Then measuring (calibration) is performed in the
minus X direction. At the end, the calibration tool is again at position X61.
The new trigger values in minus X are stored in the data of tool probe 1 (_PRNUM=1)
_TP[0,0] if they deviate by more than 0.005 mm (_TZL=0.005) from the old values.
Deviations of up to 5 mm (_TSA=5) are permissible.
In block N55 the calibration tool is moved up to position Z100 and the program ends with
block N60.
5-14
;Define machining plane, zero offset and
;feed type
;Select calibration tool
;Change calibration tool and
;activate compensation
;Position infeed axis over tool
;
;Position in plane on tool
;
;Parameters for calibration in the X axis
;The array of
;tool probe 1 is effective: _TPW[0,i]
;Calibration in minus X direction
;Traverse up in infeed axis in rapid
traverse
;End of program
Programming Manual, Release 04/2006, 6FC5398-4BP10-0BA0
Measuring cycles