HEIDENHAIN CNC Pilot 4290 - Manual (Page 146)

4 DIN PLUS 134
■ Programming X, Z: absolute,
incremental or modal
■ Cutter radius compensation: Not
active
■ Safety clearance After every step: 1 mm.
4.7 T
u
rning Cy
cles
Simple longitudinal roughing G81
G81 machines (roughs) the contour area described 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 proportioning of cuts is calculated so that an ”abrasive cut” is
avoided and the calculated infeed distance <= maximum infeed I.
Oversizes:
■ G57 oversizes
■ are calculated with algebraic sign (oversizes are therefore
impossible for inside contour machining)
■ stay in effect after cycle end
■ G58 oversizes: are not taken into account
Cycle run
1 Calculate the cut segmentation (infeeds).
2 Approach workpiece for first pass from starting point on paraxial path.
3 Move at feed rate to target point Z.
4 Depending on the algebraic sign of I:
■ I<0: Machine contour outline.
■ I>0: Retract by 1 mm at 45°.
5 Return at rapid traverse and approach for next pass.
6 Repeat 3 to 5 until target point X has been reached.
7 Move to:
■ X – last position at which the tool retracts.
■ Z – starting point of cycle.
Parameters
X/Z: Contour target point (X diameter)
I: Maximum infeed distance 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 Infeed – default: 0
■ 0: Infeed with G0 (rapid traverse).
■ 1: Infeed with G1 (feed rate).
4.7.2 Simple Turning Cycles
End of cycle G80
Concludes the fixed cycles.