Siemens SINUMERIK 802D sl Programming Manual page 36

Commands Calling Axis Movements
2.2 Reference point return
Supplements to the automatic reference point return commands
Tool radius offset and canned cycle
G28 must not be specified in the tool radius offset mode (G41, G42) or in a canned
cycle.
Warning
!
Issuing G28 will cancel tool radius offset (G40) followed by axes movement to-
wards the reference point. For that reason, make sure to disable tool radius offset
before issuing G28.
Tool position offset
If G28 is specified in the tool position offset mode, positioning at the intermediate
positioning point is made with the offset data valid. However, for the positioning at
the reference point, the offset data are invalid and positioning is made at the abso-
lute reference point.
Tool length offset
It is possible to cancel the tool length offset mode by G28 by changing the setting
for a parameter. Although cancellation of the tool length offset mode is possible by
G28, the tool length offset mode should be canceled before the designation of G28.
Machine lock intervention
The lamp for indicating the completion of return does not go on when the machine
lock is turned on, even when the tool has automatically returned to the reference
position. In this case, it is not checked whether the tool has returned to the refer-
ence position even when a G27 command is specified.
2-36
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) -- 04.07 Edition
© Siemens AG 2007 All rights reserved
04.07