HEIDENHAIN TNC 410 - Manual (Page 153)

8 Programming: Cycles 140
POCKET MILLING (Cycle 4)
1 The tool penetrates the workpiece at the starting position (pocket
center) and advances to the first plunging depth.
2 The cutter begins milling in the positive axis direction of the
longer side (on square pockets, always starting in the positive Y
direction) and then roughs out the pocket from the inside out.
3 This process (1 to 3) is repeated until the depth is reached.
4 At the end of the cycle, the TNC retracts the tool to the starting
position.
Before programming, note the following:
Program a positioning block for the starting point (pocket
center) in the working plane with RADIUS
COMPENSATION R0.
Program a positioning block for the starting point in the
tool axis (set-up clearance above the workpiece surface).
The algebraic sign for the depth parameter determines
the working direction.
This cycle requires a center-cut end mill (ISO 1641), or
pilot drilling at the pocket center.
The length and the width must each be greater than 2
times the rounding radius.
ú Setup clearance (incremental value): Distance
between tool tip (at starting position) and workpiece
surface
ú Milling depth (incremental value): Distance between
workpiece surface and bottom of pocket
ú Plunging depth (incremental value):
Infeed per cut. The tool will advance to the depth in
one movement if:
■ the plunging depth equals the depth
■ the plunging depth is greater than the depth
ú Feed rate for plunging: Traversing speed of the tool
during penetration
ú 1st side length : Pocket length, parallel to the main
axis of the working plane
ú 2nd side length : Pocket width
ú Feed rate F: Traversing speed of the tool in the
working plane
8.4 Cy
cles f
or Milling P
o
c
k
ets,
St
uds and Slots
X
Z
Example NC blocks:
27 CYCL DEF 4.0 POCKET MILLING
28 CYCL DEF 4.1 SET UP 2
29 CYCL DEF 4.2 DEPTH -20
30 CYCL DEF 4.3 PLNGNG 5 F100
31 CYCL DEF 4.4 X80
32 CYCL DEF 4.5 Y60
33 CYCL DEF 4.6 F275 DR+ RADIUS 5