Commands Calling Axis Movements; Interpolation Commands; Positioning (G00) - Siemens Sinumerik 802D sl Programming Manual

Commands Calling Axis Movements

2.1

Interpolation commands

2.1.1

Positioning (G00)

The G00 command moves a tool to the position in the workpiece system specified
with an absolute or an incremental command at a rapid traverse rate. In the abso-
lute command, coordinate value of the end point is programmed. In the incremental
command the distance the tool moves is programmed.
For calling the positioning, the following G code can be used.
Table 2-1
G00
Format
G00 X... Z... ;
When "G00 X(U)... Z(W)... (C(H)... Y(V)...);" is designated, positioning is executed.
The program advances to the next block only when the number of lag pulses due
to servo lag are checked after the completion of pulse distribution has reduced to
the permissible value.
In the G00 mode, positioning is made at a rapid traverse rate in the simultaneous
2-axis control mode. The axes not designated in the G00 block do not move. In
positioning operation, the individual axes move independently of each other at a
rapid traverse rate that is set for each axis. The rapid traverse rates set for the indi-
vidual axes differ depending on the machine. For the rapid traverse rates of your
machine, refer to the manuals published by the machine tool builder.
© SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning -- 04.07 Edition
G code for positioning
G code
Positioning
+X
Z
Function
01
W
X
2
Group
U
2
+Z
2-23