Siemens SINUMERIK 840D Programming Manual page 263

3
12.97
11.02
With G641, the tolerance value corresponds to the
ADIS value.
On initial entry, the following values are set for the
tolerance:
• Finishing: 0.01 (linear axes) 0.08 deg (rotary axes)
• Rough-finishing: 0.05 (linear axes) 0.4 deg (rotary
axes)
• Roughing: 0.1 (linear axes) 0.8 deg (rotary axes)
• Deselection: 0.1 (linear axes) 0.1 deg (rotary axes)
The mm/inch system of units is taken into account.
If the tolerance value is also to be effective for rotary
axes, 5-axis transformation must be set up by the
machine manufacturer.
Transformation (_TOLM)
The transformation input field is only displayed when the
NC option is set (machining package 5 axes set).
• No
CAM programs with resolved rotary axis positions
are supported.
• TRAORI
• TRAORI(2)
Selection of the transformation number or of the
manufacturer cycle to call 5-axis transformation.
The parameter is in relation to the following GUD7
variables _TOLT2.
The name of a manufacturer cycle can be stored,
resulting in calling the manufacturer cycle of
transformation. If _TOLT2 is empty ("" default),
selection transformation 1,2... calls the 5-axis
transformation with TRAORI(1), TRAORI(2).
Customization, customizing the technology
(see subsection 3.17.3)
• Yes
• No
The subsequent input parameters can only be
changed if customization is set to "Yes".
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
3.17 High Speed Settings – CYCLE832 (SW 6.3 and higher)
3
Milling Cycles
3-263