Contour Definitions In The Machining Section; Cycle End / Simple Contour G80 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Contour definitions in the machining section
4.18 Contour definitions in the machining
section

Cycle end / Simple contour G80

By programming G80 (with parameters), a turning contour
consisting of more than one element can be defined in one NC
block. G80 (without parameters) ends a contour definition directly
after a cycle.
Parameters:
XS: Start point of contour in X (diameter value)
ZS: Start point of contour in Z
XE: Final point of contour in X (diameter value)
ZE: Final point of contour in Z
AC: Angle of first element (range: 0° <= AC < 90°)
WC: Angle of second element (range: 0° <= WC < 90°)
BS: -Chamfer/+radius at start
WS: Angle for chamfer
BE: -Chamfer/+radius at end
WE: Angle for chamfer at contour end
RC: Radius
IC: Chamfer width
KC: Chamfer width
JC: Execution
0: Simple contour
1: Expanded contour
EC: Type of contour
0: Rising contour
1: Plunging contour
HC: 1: Transverse – contour direction for finishing
0: Longitudinal
1: Transverse
IC and KC are used in the control to show the chamfer/rounding
cycles.
Example: G80
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G810 P3
N4 G80 XS60 ZS-2 XE90 ZE-50 BS3 BE-2 RC5
N5 ...
N6 G0 X85 Z2
N7 G810 P5
N8 G0 X0 Z0
N9 G1 X20
N10 G1 Z-40
N11 G80
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
339