HEIDENHAIN 548431-05, User Manual, Page: 305 / 722

Teach-in | Recessing cycles
5
HEIDENHAIN | MANUALplus 620 | User's Manual | 12/2017
305
Undercut. Form K
Select Recessing cycle
Select
Undercut K
This cycle performs only one linear cut at an angle of 45°. The
resulting contour geometry therefore depends on the tool that is
used.
Cycle parameters:
X , Z : Start point
X1
,
Z1
:
Contour corner
I : Undercut depth
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)
Type of machining for technology database access:
Finishing
Cycle run:
1 Pre-position at an angle of 45° to
Safety clearance above the
Contour corner X1
,
Z1
at rapid traverse
2 Plunge by Undercut depth I
3 Return the tool to the Start point on the same path
4 Move to the Tool change point
according to the setting in
G14