Siemens SINUMERIK 802D sl Programming Manual page 78

Movement Control Commands
3.5 Tool offset functions
Blocks not including axis move commands in the offset mode
In the tool radius offset mode, the NC generates the tool paths by buffering the
data of two blocks. If a block not including axis move commands is read, the NC
reads one more block to generate the offset tool paths. Designation of such a block
which does not include axis move commands is allowed in the tool radius offset
mode for up to two consecutive blocks.
After the designation of G41, there must not be three or more consecutive blocks
that do not include the movement commands of the axes in the offset plane.
Consecutive three or more blocks not including axis move commands
If three or more blocks not containing axis move commands in the offset plane are
given consecutively, the cutting tool is moved to the position offset normally by the
specified offset amount at the end point of the block immediately preceding such
blocks.
Example of programming
G17 G01 G41 X ...Y... D... F... ;
X... Y... ;
·
·
X... Y... ;
G04 P1000 ;
X... Y... ;
·
·
X... Y... ;
Z... ;
Z... ;
X... Y... ;
·
·
X... Y... ;
G40 X... Y... ;
Fig. 3-19
3-78
Example of programming
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) - - 04.07 Edition
Blocks not including axis movement
commands in the offset plane
(If such blocks continue up to two
blocks, the NC can generate tool
paths without a problem.)
© Siemens AG 2007 All rights reserved
04.07