HEIDENHAIN 548431-05 User Manual page 283

Teach-in | Recessing cycles
Radial recess turning—Expanded
Select Recessing cycle
Select Recess turning
Select Radial recess turning
Select the Expanded soft key
Taking the oversizes into account, the cycle machines the area
described by the Start point X/Start point contour Z1 and the End
point contour.
Further information: "Recess turning", Page 279
Cycle parameters:
X, Z: Start point
X1, Z1: Start point contour
X2, Z2: End point contour
P: Feed depth – Maximum infeed depth
O: Recessing feed (default: active feed rate)
I, K: O-size X and Z
A: Start angle (range: 0° <= A < 90°; default: 0°)
W: Final angle (range: 0° <= W < 90°; default: 0°)
R: Rounding
T: Tool number – turret pocket number
G14: Tool change point
Further information:
ID: ID no.
S: Cutting speed or Constant speed
F: Feed per revolution
B1, B2: -B cham./+B round. (B1 at contour start and B2 at
contour end)
B > 0: Radius of rounding
B < 0: Width of chamfer
B: Offset width (default: 0)
U: Unidir. turning (default: 0)
0: Bidirectional
1: Unidirectional
G47: Safety clearance
Further information:
MT: M after T: M function that is executed after the tool call T
MFS: M at beginning: M function that is executed at the
beginning of the machining step
MFE: M at end: M function that is executed at the end of the
machining step
HEIDENHAIN | MANUALplus 620 | User's Manual | 12/2017
"Tool change point G14", Page 180
"Safety clearance G47", Page 180
5
283