Cylindrical Interpolation (G07.1) - Siemens Sinumerik 840D sl Programming Manual

Supplementary conditions
Both the starting point and the end point must be outside the area of the base circle of the
involute (circle with radius R around the center point specified by I, J, K). If this condition is
not satisfied, an alarm is generated and the program execution is aborted.
Note
For more information about machine data and supplementary conditions that are relevant to
involute interpolation, please see References: /FB1/, A2 Chapter "Settings for involute
interpolation".
2.1.7

Cylindrical interpolation (G07.1)

Randomly running grooves can be cut on cylindrical workpieces with Function G07.1
(cylindrical interpolation). The path of the grooves is programmed with reference to the
unwinded, plane surface of the cylinder.
The G functions specified below can be used to switch the operation of cylindrical
interpolation on or off.
Table 2- 3
G function
G07.1
Format
G07.1 A (B, C) r
G07.1 A (B, C) 0
A, B, C: Address of the rotary axis
r: Radius of the cylinder
No other commands should be present in the block containing G07.1.
The G07.1 command is modal. Once G07.1 is specified, the cylindrical interpolation remains
active till G07.1 A (B, C) is deselected. The cylindrical interpolation is deactivated in closed
position or after NC RESET.
Note
G07.1 is based on the Siemens option TRACYL. Appropriate machine data is to be set for
this.
The corresponding data on this is available in the manual "Extended Functions", Section M1,
TRACYL.
ISO Milling
Programming Manual, 06/09, 6FC5398-7BP10-1BA0
G functions for activating/deactivating the cylindrical interpolation
Function
Operation with cylindrical interpolation
;Activation of operation with cylindrical interpolation
;Deselection of operation with cylindrical interpolation
Drive commands
2.1 Interpolation commands
G group
16
27