Cylindrical Interpolation (G07.1) - Siemens SINUMERIK 802D sl Programming Manual

04.07
4.7

Cylindrical interpolation (G07.1)

This interpolation feature allows the machining to be accomplished by the combina-
tion of tool movements and rotation of a workpiece in the virtual orthogonal coordi-
nate system. Machining is possible on the circumference of cylindrical workpiece
by using the commands in an orthogonal coordinate system. To use this function,
an additional axis of rotation is necessary in addition to the normal servo axes (X,
Y, and Z axes).
Programming format
The cylindrical interpolation mode is turned ON and OFF by the G codes indicated
below.
Table 4-6
G code
G07.1
Format
G07.1 A (B, C) r ;
Starts the cylindrical interpolation mode (enables cylindrical interpolation).
G07.1 A (B, C) 0 ;
The cylindrical interpolation mode is cancelled.
A, B, C: An address for the rotation axis
r: The radius of the cylinder
Specify the G07.1 command in a block without other commands.
The G07.1 command is modal and once the G07.1 command is specified, the cy-
lindrical interpolation mode remains ON until the G07.1 A (B, C) command is speci-
fied. The NC is in the cylindrical interpolation OFF mode when the power is turned
ON or when the NC is reset.
Note
G07.1 is based on the Siemens option TRACYL. The relevant machine data
S
need to be set accordingly.
For details refer to the manual "Extended Functions", chapter M1, 2.2 "TRA-
S
CYL".
© Siemens AG 2007 All rights reserved
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) -- 04.07 Edition
G codes used for cylindrical interpolation
Cylindrical interpolation mode
Enhanced Level Commands
4.7 Cylindrical interpolation (G07.1)
Function
16
Group
4-139