Siemens SINUMERIK 840D Programming Manual page 260

3 3
Milling Cycles 12.97
11.02
3.17 High Speed Settings – CYCLE832 (SW 6.3 and higher)
Function
The CYCLE832 cycle groups the important G codes and
the machine or setting data required for HSC machining.
In CYCLE832, a distinction is made between three
technological executions:
• "Finishing",
• "Rough-finishing" and
• "Roughing".
In CAD programs, the three machining types are in the HSC
range in direct relation to the accuracy and speed of the path
contour (see help display). The operator / programmer uses
the tolerance value to give relevant weighting.
Different tolerances and settings (customizing technology) can
be assigned to the three machining types.
In the input screen form, the relevant G codes are preset
(customizing technology) to ensure a smoothing path contour
or that the CAM program is executed at optimum speed.
The cycle is located in the main menu before the CAM
program (see typical CYCLE832 call).
Different interpretations of the tolerance values are taken into
account. For example, for G641, the tolerance value is
transferred as ADIS= and for G642, the axis-specific
MD 33100 COMPRESS_POS_TOL[AX] is updated.
When activating the "Customize technology" input field, you
can enable or disable:
• compression (COMPCAD, COMPCURV, COMPOF,
B-SPLINE),
• continuous-path mode (G64, G641, G642) or
• velocity control (FFWON, FFWOF, SOFT, BRISK).
If 5-axis transformation (TRAORI) is set up, this can be
enabled/disabled in the transformation input field.
Take note of the machine manufacturer's
comments!
© Siemens AG, 2002. All rights reserved
3-260
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition