Siemens SINUMERIK User Manual

Programming and Operating Manual (Turning)
122 01/2017
Cancellation of compensation by M2
If the offset mode is canceled with M2 (program end) without writing the command G40, the last block with coordinates ends
in the normal offset vector setting.
No
compensating movement is executed. The program ends with this tool position.
Critical machining cases
When programming, pay special attention to cases where the contour path for inner corners is smaller than the tool radius;
and smaller than the diameter for two successive inner corners.
Such cases should be avoided.
Also check over multiple blocks that the contour contains no "bottlenecks".
When carrying out a test/dry run, use the largest tool radius you are offered.
Acute contour angles
If very sharp outside corners occur in the contour with active G451 intersection, the control system automatically switches to
transition circle. This avoids long idle motions.
11.11.8
Example of tool radius compensation (turning)
See the following example of tool radius compensation, cutting edge radius shown magnified:
Programming example
N1
; Contour cut
N2 T1
; Tool 1 with offset D1
N10 DIAMOF F0.15 S1000 M3
; Radius dimension, technological values
N15 G54 G0 G90 X100 Z15
N20 X0 Z6
N30 G1 G42 G451 X0 Z0
; Start compensation mode
N40 G91 X20 CHF=(5* 1.1223 )
; Insert chamfer, 30 degrees
N50 Z-25
N60 X10 Z-30
N70 Z-8
N80 G3 X20 Z-20 CR=20
N90 G1 Z-20
N95 X5
N100 Z-25
N110 G40 G0 G90 X100
; Terminate compensation mode
N120 M2

Siemens SINUMERIK Specifications

General

Brand	Siemens
Model	SINUMERIK
Category	Control Unit
Language	English