Corner Behavior: G450, G451; Tool Radius Compensation Off: G40 - Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual

N70 G1 Z-30 F0.15
N80 X60 Z10
N90 M30
8.11.5

Corner behavior: G450, G451

Functionality
Using the functions G450 and G451, you can set the behavior for non-continuous transition from one contour element to
another contour element (corner behavior) when G41/G42 is active.
Internal and external corners are detected automatically by the control system. For internal corners, the intersection of the
equidistant paths is always approached.
Programming
G450
G451
See the following illustration for corner behavior at an external corner:
See the following illustration for corner behavior at an internal corner:
Transition circle G450
The tool center point travels around the workpiece external corner in an arc with the tool radius. In view of the data, for
example, as far as the feedrate value is concerned, the transition 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.
8.11.6

Tool radius compensation OFF: G40

Functionality
The compensation mode (G41/G42) is deselected with G40. G40 is also the switch-on position 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 guaranteed!
Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015
; Starting contour
;Transition circle
;Point of intersection
103