HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 231)

HEIDENHAIN CNC PILOT 4290 231
4.21 Simple T
u
rn
ing Cy
cles
4.21 Simple Turning Cycles
End of cycle G80
G80 concludes a fixed cycle.
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 CNC PILOT 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 Target point contour (diameter)
Z Target point contour
I Maximum infeed in X direction
„ I<0: With machining contour outline
„ I>0: Without machining contour outline
K Offset in Z direction (default: 0)
Q G function for infeed (default: 0)
„ 0: Infeed with G0 (rapid traverse)
„ 1: Infeed with G1 (feed rate)
„ 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.