HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 187)

171 HEIDENHAIN TNC 410, TNC 426, TNC 430
POCKET MILLING (Cycles G75, G76)
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 2) 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 G40.
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 following condition must be met for the second line
length:
2nd side length greater than [(2 x rounding-off radius) +
stepover factor k].
Direction of rotation during rough-out
■ In clockwise direction: G75
■ Counterclockwise: G76
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
8.4 Cy
cles f
or Milling P
o
c
k
ets,
St
uds and Slots
X
Z
ú Feed rate F: Traversing speed of the
tool in the working plane
ú Rounding off radius: Radius for the
pocket corners.
If Radius = 0 is entered, the pocket
corners will be rounded with the
radius of the cutter.
Example NC blocks:
N27 G75 P01 2 P02 -20 P03 5 P04 100
P05 X+80 P06 Y+60 P07 275 P08 5*
...
N35 G76 P01 2 P02 -20 P03 5 P04 100
P05 X+80 P06 Y+60 P07 275 P08 5*
Calculations:
Stepover factor k = K x R
where
K is the overlap factor, preset in machine
parameter 7430, and
R: is the cutter radius
Kkap8.pm6 29.06.2006, 08:06 171