Siemens SINUMERIK 802D sl Programming Manual page 77

04.07
The cutter radius compensation function is called up by the execution of G41 or
G42 and canceled by G40. Direction of offset is determined by the designated G
code (G41, G42) and the offset amount is selected by the D code which is speci-
fied with the G code designated to call up the tool radius offset mode. When the
power is turned ON, the G40 mode is set.
Fig. 3-18
S If a negative value is set in the tool offset data memory specified by the D code,
the offset direction is reversed. The D code must be specified with G41 or G42
in the same block or in a preceding block. If D00 is specified, it specifies the
tool radius of "0".
S The tool radius offset plane is selected by the designation of G17, G18, or G19.
The G code used to select the plane must be specified with G41 or G42 in the
same block or in a block preceding the G41 or G42 block.
Table 3-14
G17
G18
G19
S It is not allowed to change the selected plane in the offset mode. If a plane
selection G code is specified in the offset mode, an alarm occurs.
Start-up of cutter compensation
Since the offset start-up is executed with the offset taken into account, the G code
in 01-group must be either G00 or G01. If a G code other than G00 or G01 is spe-
cified, an alarm occurs. If the offset starts in the G00 mode, the axes move to the
offset point at their individual rapid traverse rates. Therefore, be aware of possible
interference of a cutting tool with the workpiece.
There are two types of start-up such as start-up at inside corner and start-up at
outside corner.
© Siemens AG 2007 All rights reserved
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) - - 04.07 Edition
G41 (offset to the left)
Tool
Programmed path
Cutter radius compensation
Plane selection G codes
G code
XY plane selection
ZX plane selection
YZ plane selection
Movement Control Commands
3.5 Tool offset functions
D
D
G42 (offset to the right)
Function
02
02
02
Group
3-77