Surface Linear G111 - HEIDENHAIN CNC PILOT 640 User Manual

4

Surface linear G111

G111 moves the tool on a linear path at the feed rate to the Final
point.
Parameters:
Z: Final point
C: End angle
CY: Final point as linear value (reference: unrolled Reference
diameter)
X: Final point (diameter value)
Parameters for contour description (G80):
AN: Angle to positive Z axis
BR: Chamf./round. – defines the transition to the next contour
element
When entering a Chamf./round., program the theoretical end
point.
No entry: Tangential transition
BR = 0: No tangential transition
BR > 0: Rounding radius
BR < 0: Width of chamfer
Q: Intersect. pt. or Final point if the line segment intersects a
circular arc (default: 0)
0: Near point of intersection
1: Far point of intersection
Programming:
Z, C, CY: Absolute, incremental, or modal
Program either Z–C or Z–CY
Using the parameters AN, BR and Q is only allowed if
the contour description is concluded by G80 and used
for a cycle.
400
DIN/ISO programming | Lateral surface machining
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017