Siemens SINUMERIK 828D Function Manual page 1480

W1: Tool offset
18.5 Tool radius compensation 2D (TRC)
G450 (transition circle)
With the G function G450 active, 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 → refer to very flat outside corners.
If pointed outside corners are desired, the tool must be retracted from the contour ( → see "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 instruction 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 instruction is 0 to 100, in increments of 1.
Value Significance
Overshoot disabled, transition circle active
DISC = 0
Overshoot large enough to theoretically produce a response similar to
DISC = 100
intersection (G451).
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.
Figure 18-24 Example: Overshoot with DISC= 25
1480
Function Manual, 09/2011, 6FC5397-0BP40-2BA0
Basic Functions