Siemens SINUMERIK 840D Programming Manual page 142

3
Milling Cycles
3.5 Slots on a circle – SLOT1
Further notes
A tool offset must be activated before the cycle is
called. Otherwise the cycle is aborted with Alarm 61000
"No tool offset active".
If incorrect values are assigned to the parameters that
determine the arrangement and size of the slots and
thus cause mutual contour violation of the slots, the
cycle is not started. The cycle is aborted after the error
message
61104 "Contour violation of slots/elongated holes".
During the cycle, the workpiece coordinate system is
shifted and rotated. The values in the workpiece
coordinate system displayed on the actual value
display are such that the longitudinal axis of the slot
that has just been machined corresponds to the first
axis of the current machining plane.
When the cycle is completed, the workpiece coordinate
system is again in the same position as it was before
the cycle was called.
Programming example
Slots
This program produces the same arrangement of
four slots on a circle as the program for elongated
hole machining (see Section 3.4).
The slots have the following dimensions:
Length 30mm, width 15mm and depth 23mm. The
safety distance is 1mm, the final machining
allowance is 0.5mm, the milling direction is G2, the
maximum infeed in the depth is 10mm.
The slots must be machined completely with an
oscillating insertion motion.
N10 G19 G90 S600 M3
N15 T10 D1
N17 M6
N20 G0 Y20 Z50 X5
N30 SLOT1 (5, 0, 1, -23, , 4, 30, 15, ->
->40, 45, 20, 45, 90, 100, 320, 10, ->
->2, 0.5, 30, 10, 400, 1200, 0.6, 5)
N40 M30
-> Must be programmed in a single block
3-142
Contour violation
Z
90°
20
40
Specification of technology values
Approach starting position
Cycle call, parameters VARI, MIDF,
FFP2 and SSF omitted
End of program
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
3
12.97
04.00
Z
A A - B
45°
Y
X
B 23
© Siemens AG, 2002. All rights reserved