Simple Longitudinal Roughing G81 - Simple Turning Cycles - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | G codes from previous controls
Simple longitudinal roughing G81 – simple turning
cycles
G81 roughs the contour area defined by the current tool position
and X, Z. If you wish to machine an oblique cut, you can define the
angle with I and K.
Parameters:
X: Contour Start point (diameter value)
Z: Final point
I: Max. approach
K: Offset (in Z; default: 0)
Q: G-Fct.approach (default: 0)
0: Infeed with G0 (rapid traverse)
1: Infeed with G1 (feed rate)
V: Type of retraction (default: 0)
0: Return to cycle starting point in Z and last retraction
diameter in X
1: Return to cycle starting point
H: Contour smoothing
0: With each cut (machine contour outline after each pass)
2: No smoothing (retracts at 45°; no contour smoothing)
The control uses the position of the target point to distinguish
between external and internal machining. The number of cutting
passes is calculated so that an abrasive cut is avoided and the
calculated Max. approach <= I.
Programming X, Z: Absolute, incremental or modal
Tool radius compensation is inactive.
Safety clearance after each step: 1 mm
A G57 oversize
Is calculated with algebraic sign (oversizes are
therefore impossible for inside contour machining)
Remains effective after cycle end
A G58 oversize is not taken into account.
Example: G81
. . .
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G81 X100 Z-70 I4 K4 Q0
N4 G0 X100 Z2
N5 G81 X80 Z-60 I-4 K2 Q1
N6 G0 X80 Z2
N7 G81 X50 Z-45 I4 Q1
. . .
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
499