Tool Radius Compensation Off: G40 - Siemens SINUMERIK 802D sl Programming And Operating Manual

Programming
3.6 Tool and tool offset
Transition circle G450
The tool center point travels around the workpiece external corner in an arc with the tool ra-
dius. In view of the data, for example, as far as the feedrate value is concerned, the transi-
tion circle belongs to the next block containing traversing movements.
Point of intersection G451
For a G451 intersection of the equidistant paths, the point (intersection) that results from the
center point paths of the tool (circle or straight line) is approached.
3.6.5

Tool radius compensation OFF: G40

Functionality
The compensation mode (G41/G42) is deselected with G40. G40 is also the switch-on posi-
tion at the beginning of the program.
The tool ends the block before G40 in the normal end position (compensation vector vertical
to the tangent in the end point); independently of the start angle.
If G40 is active, the reference point is the tool tip. The tool tip then travels to the programmed
point upon deselection.
Always select the end point of the G40 block such that collision-free traversing is guaran-
teed!
Programming
G40 X... Z...
Remark: The compensation mode can only be deselected with linear interpolation (G0, G1).
Program both axes. If you only specify one axis, the second axis is automatically completed
with the last programmed value.
S
Figure 3-33 Ending the tool radius compensation with G40, with the example of G42, cutting edge position =3
3-68
; Tool radius compensation OFF
S
Programming and Operating manual, 06/2006, 6FC5398-4CP10-0BA0
Grinding