Siemens SINUMERIK 840D Programming Manual page 193

3
12.97
10.00
3.13 Milling rectangular spigots – CYCLE76 (SW 5.3 and higher)
Further notes
A tool offset must be activated before the cycle is
called. The cycle is otherwise aborted with alarm 61009
"Active tool number=0".
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
Spigots
This program allows you to machine a spigot that is
60mm long, 40mm wide, 15mm deep in the XY plane
and with a corner radius of 15mm. The spigot has an
angle of 10 degrees in relation to the X axis and is
programmed from a corner point P1. When a spigot is
dimensioned with reference to corners, the length and
width must be entered with a sign to define a unique
position for the spigot. The spigot is premachined with
an allowance of 80mm in its length and 50mm in its
width.
N10 G90 G0 G17 X100 Y100 T20 D1 S3000 M3 Specification of technology values
N11 M6
N20 _ZSD[2]=1
N30 CYCLE76 (10, 0, 2, -17.5, , -60, ->
-> -40, 15, 80, 60, 10, 11, , , 900, ->
-> 800, 0, 1, 80, 50)
N40 M30
-> Must be programmed in a single block
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
Y
A
P1
10 °
R15
B
80
Dimensioning of spigot referred to
corners
Cycle call
End of program
3
Milling Cycles
Y
A - B
X Z
17.5
3-193