Cycle832 And Cust_832 - Siemens SINUMERIK 828D Manual

Important functions for 3- to 5-axis machining

3.6.2 CYCLE832 and CUST_832

The manufacturer cycle CUST_832 is available for individual adaptation of CYCLE832. This is
individually adapted according to the machine by the machine manufacturer. Special NC
commands for machining are also set in CUST_832. As a consequence, the parameters in the
CYCLE832 dialog can deviate from the descriptions in Section 3.6.1 if the machine manufacturer
has made specific adaptations.
NC commands in connection with Advanced Surface and Top Surface
The following NC code commands are preset in CUST_832.SPF and are activated when the
technology groups are selected in CYCLE832:
DYNNORM, DYNROUGH, DYNSEMIFIN, DYNFINISH (G code group 59).
COMPCAD makes it possible to combine part programs with short linear blocks (G1), with
the associated tolerance, using polynomials.
COMPSURF, compressor ensures a better workpiece surface for inclined line-by-line
finishing programs, poor data quality - or for example, irregular point distribution in NC
programs from the CAD/CAM system.
SOFT (G code group 21) activates the jerk-limited velocity control.
G645 (G code group 10) switches to the continuous-path mode (Look Ahead).
FIFOCTRL (G code group 4) switches to the automatic pre-processing memory control.
FFWON (G code group 24) switches to the parameterized feedforward control (speed or
acceleration feedforward control). Can be optionally activated in CUST_832.
Important NC commands for 5-axis machining
In CUST_832.SPF, the following NC code commands can be preset by the machine
manufacturer.
TRAORI activates the 5-axis transformation set in the transformer machine data and must be
programmed alone in the block.
UPATH (G code group 45) ensures synchronous movements of the rotary and linear axes in
5-axis spline interpolation, as performed with active compressor, for example.
ORIAXES (G code group 51) linearly interpolates the orientation axes in the block up to the
end of block.
ORIWKS (G code group 25) defines the workpiece coordinate system for orientation
programming.
ORISON (G code group 61) activates the orientation smoothing for 5-axis machining with
active 5-axis transformation (TRAORI).
You can see which functions of CYCLE832 are currently active during processing in the
"All G functions" display.See "Executing programs (AUTOMATIC)" on page 64.
In the following sections, you will find the relevant machine functions such as Compressor and
Look Ahead, which are only explained briefly here, because they are automatically called up with
optimal values by CYCLE832 or CUST_832.
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling
3.6
109