HEIDENHAIN MANUALplus 4110 - Manual (Page 362)

362 6 DIN Programming
6.20 F
a
ce Mac
h
ining
Circular arc, face G102/G103
Geometry command: G102/G103 defines a circular arc in a contour
on the face.
Machining command: The tool moves on a circular arc at feed rate to
the end point.
The direction of rotation is shown in the graphic support window.
Parameters
 X end point (diameter value)
 C end angle —for angle direction, see graphic support window
 XK end point (Cartesian coordinates)
 YK end point (Cartesian coordinates)
 R radius
 I center point (Cartesian coordinates)
 K center point (Cartesian coordinates)
 Q point of intersection (default: Q=0): If entered data permit two
possible solutions for the end point, "Q" defines the end point.
 B chamfer/rounding arc: Transition to the next contour element
When entering a chamfer/rounding, program the theoretical end
point of the contour element.
„ B no input: Tangential transition
„ B=0: No tangential transition
„ B>0: Radius of rounding
„ B<0: Width of chamfer
 Z end point
Example: G102, G103
%100.nc
[G100, G101, G102, G103, G793]
N1 T70 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N5 G793 Z2 ZE-5 P2 U0.5 R0 I0.5 F0.15 H0 Q0
N6 G100 XK20 YK5
N7 G101 XK50 B5
N8 G103 XK5 YK50 R50 Q1 B5
N9 G101 XK5 YK20 B5
N10 G102 XK20 YK5 R20 B5
N11 G80
N12 M15
END
„ Define the end point either in polar or Cartesian
coordinates.
„ End point in the coordinate origin: Program XK=0,
YK=0.
„ Program either center or radius.
„ If you do not program the center, MANUALplus
automatically calculates the possible solutions for the
center and chooses that point as the center which
results in the shortest arc.
„ Permitted as geometry command only for G102/G103:
Parameters Q, B
„ Permitted as machining command only for G102/G103:
Parameter Z