Siemens SINUMERIK 840D sl Function Manual page 71

Figure 2-14
G450 (transition circle)
With the active G command G450, on outside corners, the center point of the tool travels a
circular path along the tool radius. The circular path starts with the normal position
(perpendicular to the path tangent) at the end point of the previous path section (program block)
and ends in normal position at the start point of the new path section (program block).
Where outside corners are very flat, the response with G450 (transition circle) and G451
(intersection) becomes increasingly similar (see "Very flat outside corners").
If pointed outside corners are desired, the tool must be retracted from the contour (see Section
"DISC").
DISC
The G450 transition circle does not produce sharp outside contour corners because the path of
the tool center point through the transition circle is controlled so that the cutting edge stops at
the outside corner (programmed position). When sharp outside corners are to be machined
with G450, the DISC statement can be used to program an overshoot. Thus, the transition circle
becomes a conic and the tool cutting edge retracts from the outside corner.
The range of values of the DISC statement is 0 to 100, in increments of 1.
Value
DISC = 0
DISC = 100
The programmable maximum value for DISC can be set via the machine data:
MD20220 $MC_CUTCOM_MAX_DISC (max. value for DISC).
Values greater than 50 are generally not advisable with DISC.
Tools
Function Manual, 06/2019, A5E47435126B AA
Example of a 90 degree outside corner with G450 and G451
Meaning
Overshoot disabled, transition circle active
Overshoot large enough to theoretically produce a response similar to intersec‐
tion (G451).
W1: Tool offset
2.5 2D tool radius compensation
71