HEIDENHAIN CNC PILOT 640 - Circular Arc on Lateral Surface G112;G113

DIN/ISO programming | Lateral surface machining
4
402
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
Circular arc on lateral surface G112/G113
G112 and G113 move the tool in a circular arc 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)
R: Radius
K: Center (in Z)
J: Center as linear value (referenced to unrolled G120 reference
diameter)
W: Center – Angle (angular direction: see help graphic)
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
Using the parameters AN, BR and Q is only allowed if
the contour description is concluded by G80 and used
for a cycle.
Programming:
Z, C, CY: Absolute, incremental, or modal
K, W, J: Absolute or incremental
Program either Z–C or Z–CY and K–J
Program either center or radius
For radius: Only arcs <= 180° are possible