HEIDENHAIN MANUALplus 4110 - Manual (Page 320)

320 6 DIN Programming
6.12 Simple T
u
rn
ing Cy
cles
Roughing transverse G82
G82 machines the contour area defined by the current tool position
and "Z, X" in transverse direction.
Parameters
 X end point of contour section (diameter value)
 Z starting point of contour section
 I offset: Infeed in Z (default: 0)
 K maximum infeed in X: The proportioning of cuts is calculated so that
an "abrasive cut" is avoided and the calculated infeed distance is <=
K.
„ K>0: With machining contour outline
„ K<0: Without machining contour outline
 Q G function infeed: Infeed is executed through G function
„ Q=0: Infeed with G0 (rapid traverse)
„ Q=1: Infeed with G1 (feed rate)
 V type of retraction (default: 0)
„ V=0: Return to cycle starting point in Z and last retraction diameter
in X
„ V=1: Return to starting point of cycle
Note on the execution of the cycle:
„ If you wish to machine an oblique cut, you can define the angle with
I and K.
„ MANUALplus automatically determines the cutting and infeed
directions from the current tool position relative to the starting point
/ end point of the contour area.
Example: G82
%82.nc
[G82]
N1 T3 G95 F0.25 G96 S200 M3
N2 G0 X120 Z2
N3 G82 X20 Z-15 I4 K4 V0
N4 G0 X120 Z-15
N5 G82 X50 Z-26 I2 K-4 V1
N6 G0 X120 Z-26
N7 G82 X80 Z-45 K4 Q1
END
„ Cutter radius compensation: is not carried out.
„ Oversizes: Oversizes programmed with G57 are taken
into account. The oversizes remain in effect after
execution of the cycle.
„ Safety clearance after a pass is 1 mm.