Siemens SINUMERIK 840D Programming Manual page 135

03.96
3
Further notes
A tool offset must be activated before the cycle is
called. Otherwise the cycle is aborted and alarm
61000 "No tool offset active" is output.
A new workpiece coordinate system that influences the
actual value display is used in the cycle. The zero point
of this coordinate system lies on the pocket center
point.
The original coordinate system becomes active again
after the end of the cycle.
Programming example
Pocket
With this program you can machine a pocket that is
60 mm long, 40 mm wide, 17.5 mm deep (difference
between the reference plane and the base of the
pocket) and which has a corner radius of 8 mm in
the XY plane. The angle to the X axis is 0 degrees.
The final machining allowance of the pocket edges is
0.75 mm, the safety clearance in the Z axis, which is
added to the reference plane, is 0.5 mm. The center
point of the pocket lies at X60 and Y40, the
maximum depth infeed is 4 mm.
Only roughing is to be performed.
DEF REAL LENG, WID, DPR, CRAD
DEF INT VARI
N10 LENG=60 WID=40 DPR=17.5 CRAD=8
N20 VARI=1
N30 G90 T20 D2 S600 M4
N40 G17 G0 X60 Y40 Z5
N50 POCKET1 (5, 0, 0.5, , DPR, ->
-> LENG, WID, CRAD, 60, 40, 0, ->
-> 120, 300, 4, 2, 0.75, VARI)
N60 M30
-> Must be programmed in a single block
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
3.7 Milling rectangular pockets - POCKET1
Definition of variables
Value assignments
Specification of technology values
Approach starting position
Cycle call
Parameters MIDF, FFP2 and SSF are
omitted
End of program
Milling Cycles
Y
A
B
60
3
Y
A - B
X Z
17,5
3-135