Plane Selection (G17, G18, G19); Parallel Axes (G17, G18, G19) - Siemens SINUMERIK 802D sl Programming Manual

Movement Control Commands
3.1 The coordinate system
3.1.8

Plane selection (G17, G18, G19)

The plane where circular interpolation, tool radius offset, and coordinate system
rotation are executed is selected by specifying the following G code.
Table 3-1
G17
G18
G19
A plane is defined in the following manner (in the case of XY plane):
The horizontal axis in the first quadrant is "+X-axis" and the vertical axis in the
same quadrant "+Y-axis".
Fig. 3-10
S When the power is turned ON, the XY plane (G17) is selected.
S Axis move command of a single axis can be specified independent of the selec-
tion of plane by G17, G18, and G19. For example, the Z-axis can be moved by
specifying "G17 Z ....;".
S Execution of a canned cycle is possible only in the G17 plane (hole machining
axis: Z-axis).
S The plane on which the tool radius offset is executed by the G41 or G42 com-
mand is determined by the designation of G17, G18 or G19; the plane that inc-
ludes the rotary 4th- or 5th-axis cannot be selected as the offset plane.
3.1.9

Parallel axes (G17, G18, G19)

Using the function G17 (G18, G19) <axis name>, an axis parallel to one of the
three basic axes of the coordinate system can be activated.
The three basic axes are, for example, X, Y, and Z.
3-54
Plane selection G codes
G code
XY plane
ZX plane
YZ plane
+Y-axis
0
Plane selection
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) - - 04.07 Edition
Function
02
02
02
+X-axis
© Siemens AG 2007 All rights reserved
04.07
Group