HEIDENHAIN 548431-05, User Manual, Page: 215 / 722

Teach-in | Turning cycles
5
HEIDENHAIN | MANUALplus 620 | User's Manual | 12/2017
215
Cutting, longitudinal plunge
Select
Roughing cycles lon/trans
Select Plunge longit.
The cycle roughs the area described by the Start point contour ,
End point contour and Plunging angle .
The tool plunges with the maximum possible angle,
leaving material remaining
The steeper the tool plunges into the material, the
greater the feed rate decrease (max. 50 %)
Cycle parameters:
X , Z : Start point
X1
,
Z1
:
Start point contour
X2 , Z2 : End point contour
P : Feed depth – Maximum infeed depth
H
:
Contour smoothing
0: With each cut
1: With the last cut
2: No smoothing
A : Plunging angle (range: 0° <= A < 90°; default: 0°)
W
:
Final angle
(range: 0° <=
W
< 90°; default: 0°)
G47 : Safety clearance
Further information: "Safety clearance G47", Page 180
T : Tool number – turret pocket number
G14
:
Tool change point
Further information: "Tool change point G14", Page 180
ID : ID no.
S : Cutting speed or Constant speed
F
:
Feed per revolution
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
WP : No. of spindle – Displays which workpiece spindle is used
to execute the cycle (machine-dependent)
Main drive
Opposing spindle for rear-face machining
BW : Angle in the B axis (machine-dependent)
CW
:
Reverse the tool
(machine-dependent)
HC : Shoe brake (machine-dependent)
DF : Miscellaneous function (machine-dependent)