Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual page 68

Offset contour normal OFFN (transformation type 513)
To mill grooves with TRACYL, the following is programmed:
● Groove center line in the part program
● Half the groove width programmed using OFFN.
To avoid damage to the groove side OFFN acts only when the tool radius compensation is active. Furthermore, OFFN
should also be >= the tool radius to avoid damage occurring to the opposite side of the groove.
A part program for milling a groove generally comprises the following steps:
1. Selecting a tool
2. Select TRACYL
3. Select suitable coordinate offset (frame)
4. Positioning
5. Program OFFN
6. Select TRC
7. Approach block (position TRC and approach groove side)
8. Groove center line contour
9. Deselect TRC
10. Retraction block (retract TRC and move away from groove side)
11. Positioning
12. Deselect OFFN
13. TRAFOOF
14. Re-select original coordinate shift (frame)
Special features
● TRC selection:
TRC is not programmed in relation to the groove side, but relative to the programmed groove center line. To prevent the
tool traveling to the left of the groove side, G42 is entered (instead of G41). You avoid this if in OFFN, the groove width is
entered with a negative sign.
● OFFN acts differently with TRACYL than it does without TRACYL. As, even without TRACYL, OFFN is included when
TRC is active, OFFN should be reset to zero after TRAFOOF.
● It is possible to change OFFN within a part program. This could be used to shift the groove center line from the center
(see diagram).
68
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014