Circular Arc On Front/Rear Face G102/G103 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Front and rear face machining

Circular arc on front/rear face G102/G103

G102 and G103 move the tool in a circular arc at the feed rate to
the Final point. The direction of rotation is shown in the graphic
support window.
Parameters:
X: Final point (diameter value)
C: End angle
XK: Final point (Cartesian)
YK: Final point (Cartesian)
R: Radius
I: Center (Cartesian)
J: Center (Cartesian)
K: Center for H = 2 or 3 (Z direction)
Z: Final point
H: Rot. plane – working plane (default: 0)
H = 0 or 1: Machining in XY plane (front face)
H = 2: Machining in YZ plane
H = 3: Machining in XZ plane
Parameters for contour description (G80):
AN: Angle to positive XK 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.
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
397