HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 257)

HEIDENHAIN CNC PILOT 4290 257
4.25 F
ront/Rear
-F
ace Mac
h
ining
Circular arc on front/rear face G102/G103
G102/G103 moves the tool in a circular arc at the feed rate to the “end
point.” The direction of rotation is shown in the graphic support
window.
If you program H=2 or H=3, you can machine linear slots with a
circular base. If
„ H=2: Define the circle center with I and K.
„ H=3: Define the circle center with J and K.
Example: G102, G103
. . .
N1 T7 G197 S1200 G195 F0.2 M104
N2 M14
N3 G110 C0
N4 G0 X100 Z2
N6 G100 XK20 YK5
N7 G101 XK50
N8 G103 XK5 YK50 R50 [circular arc]
N9 G101 XK5 YK20
N10 G102 XK20 YK5 R20
N12 M15
. . .
Parameters
X End point (diameter)
C End angle—for angle direction, see help graphic
XK End point (Cartesian)
YK End point (Cartesian)
R Radius
I Center point (Cartesian)
K Center point (Cartesian)
Z End point (default: current Z position)
H Circular plane (working plane)—(default: 0)
„ H=0, 1: Machining in XY plane (front face)
„ H=2: Machining in YZ plane
„ H=3: Machining in XZ plane
K Center point for H=2, 3 (Z direction)
Programming:
„ X, C, XK, YK, Z: Absolute, incremental or modal
„ I, J, K: Absolute or incremental
„ Program either X–C or XK–YK
„ Program either center or radius
„ For radius: Only arcs <= 180° are possible
„ End point in the coordinate origin: Program XK=0 and
YK=0.