Swiveling - Cycle800 (Sw 6.2 And Higher) - Siemens SINUMERIK 840D Programming Manual

3
Milling Cycles
3.16 Swiveling – CYCLE800 (SW 6.2 and higher)
The current machining plane (G17, G18, G19) is taken into
account by the swivel cycle.
Swiveling onto a machining or auxiliary surface
always involves three steps:
• Offset of reference point prior to rotation (corresponds
to TRANS or ATRANS)
• Rotation (corresponds to AROT or AROTS)
• Offset of zero point after rotation (corresponds to ATRANS)
The offsets or rotations are not machine-specific, but refer
to the coordinate system X, Y, Z of the workpiece. No
programmable frames are used in the swivel cycle. The frames
programmed by the user are taken into account in additive
swiveling. Swiveling to a new swivel plane clears the
programmable frames (TRANS). After a program reset or if
there is a power failure, the last swivel plane remains active,
with the option to set via machine data. Any type of machining
operation can be performed on the swivel plane,
e.g. through calling standard or measuring cycles.
Note about calling the 5-axis transformation
If a program activating the 5-axis transformation (TRAORI) is to
be executed on the swiveled machining plane, the system
frames for the swivel head/swivel table must be deactivated
before TRAORI is called (see example).
Example (machine with swivel table)
G54
T="MILL_10mm"
M6
CYCLE800(1,"",0,57,0,40,0,-45,0,0,0,0,0,-1)
CYCLE71(50,24,2,0,0,0,80,60,0,4,10,5,0,2000,31,5)
TCARR=0
PAROTOF
TOROTOF
TRAORI
G54
EXTCALL "WALZ"
M2
3-228
;(machine kinematic type "T" and "M" only)
;Calculation of new zero offset
;5-axis machining program with direction vectors
;(A3, B3, C3)
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
12.97
;Swivel cycle
;Face mill
;swivel data record
deselection
© Siemens AG, 2002. All rights reserved
3