Siemens Sinumerik 840D sl Programming Manual page 58

Motion commands
3.4 Tool offset functions
● A negative offset value of the tool radius is equivalent to a change of compensation side
● The selection of the plane in which the tool radius is active is done with G17, G18 or G19.
Table 3- 11
G function
G17
G18
G19
● The selected plane should not be changed if the tool offset is selected, otherwise there is
Activation/deactivation of tool radius compensation
A drive command must be programmed with G0 or G1 if an NC block contains G40, G41 or
G42. At least one axis of the selected working plane must be specified in this drive
command.
Note
Compensation mode
Compensation mode may only be interrupted by a certain number of consecutive blocks or
M functions which do not contain drive commands or positional data in the compensation
plane: Standard 3.
Note
Machine manufacturer
The number of successive interruptions blocks or M functions can be set via the machine
data 20250 CUTCOM_MAXNUM_DUMMY_BLOCKS (refer to machine manufacturer).
Note
A block with path zero is also taken as interruption!
58
(G41, G42). The D function must either be programmed in the same block as G41 or G42
or in a previous block. D00 means tool radius = "0".
The G function used to select the plane is to be programmed in the same block as G41 or
G42 or in the block before G41 or G42.
G functions for selecting the plane
an error message.
Function
Selection of plane X-Y
Selection of plane Z-X
Selection of plane Y-Z
Programming Manual, 06/09, 6FC5398-7BP10-1BA0
G group
02
02
02
ISO Milling