Linear Interpolation; Linear Interpolation With Rapid Traverse: G0 - Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual

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).
● Guiding grooves:
TRACYL does not create the same groove for guiding grooves as it would be with a tool with the diameter producing the
width of the groove. It is basically not possible to create the same groove side geometry with a smaller cylindrical tool as
it is with a larger one. TRACYL minimizes the error. To avoid problems of accuracy, the tool radius should only be slightly
smaller than half the groove width.
Note
OFFN and TRC
With TRAFO_TYPE_n = 512, the value is effective under OFFN as an allowance for TRC. With TRAFO_TYPE_n = 513, half
the groove width is programmed in OFFN. The contour is retracted with OFFN-TRC.
8.3

Linear interpolation

8.3.1

Linear interpolation with rapid traverse: G0

Functionality
The rapid traverse movement G0 is used for fast positioning of the tool, however, not for direct workpiece machining.
All axes can be traversed simultaneously - on a straight path.
For each axis, the maximum speed (rapid traverse) is defined in machine data. If only one axis traverses, it uses its rapid
traverse. If two axes are traversed simultaneously, the path velocity (resulting velocity) is selected to achieve the maximum
possible path velocity in consideration of both axes.
Any programmed feedrates (F word) are not relevant for G0.
G0 remains active until canceled by another instruction from this G group (G0, G1, G2, G3, ...).
Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015
69