HEIDENHAIN SW 54843x-02 DIN Programming - Manual (Page 409)

HEIDENHAIN MANUALplus 620, CNC PILOT 640 409
4.35 G codes fr
om pr
evious contr
o
ls Simple turning cycles
Simple longitudinal roughing G81
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.
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 infeed distance is <= I.
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
. . .
Parameters
X
Starting point of contour in X (diameter value)
Z Contour end point
I Maximum infeed in X
K Offset in Z direction (default: 0)
Q G code for infeed (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 Type of departure (default: 0)
 0: With each cut (machine contour outline after each pass)
 2: No smoothing (retracts at 45°; no contour smoothing)
 Programming X, Z: Absolute, incremental or modal
 The tool radius compensation is not active.
 Safety clearance after each pass: 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.