HEIDENHAIN TNC 310 (286 140) - Manual (Page 122)

8 Programming: Cycles 110
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.
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:
n the plunging depth equals the depth
n 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
8.3 Cy
cle f
or Milling P
o
c
k
ets,
St
uds and Slots
X
Z