HEIDENHAIN TNC 320 (340 551-01) - Manual (Page 226)

226 8 Programming: Cycles
8.3 Cy
cles f
o
r Milling P
o
c
k
ets, St
uds and Slots
POCKET MILLING (Cycle 4)
Cycles 1, 2, 3, 4, 5, 17, 18 are in a group of cycles called special cycles.
Here in the second soft-key row, select the OLD CYCLS soft key.
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.
Example: NC blocks
11 L Z+100 R0 FMAX
12 CYCL DEF 4.0 POCKET MILLING
13 CYCL DEF 2.1 SETUP 2
14 CYCL DEF 4.2 DEPTH -10
15 CYCL DEF 4.3 PECKG 4 F80
16 CYCL DEF 4.4 X80
17 CYCL DEF 4.5 Y40
18 CYCL DEF 4.6 F100 DR+ RADIUS 10
19 L X+60 Y+35 FMAX M3
20 L Z+2 FMAX M99
X
Z
1 1
1 2
1 3
1 4
1 5
Before programming, note the following:
This cycle requires a center-cut end mill (ISO 1641), or pilot
drilling at the pocket center.
Pre-position over the pocket center 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 cycle parameter DEPTH
determines the working direction. If you program
DEPTH = 0, the cycle will not be executed.
The following prerequisite applies for the 2nd side length:
2nd side length greater than [(2 x rounding radius) +
stepover factor k].
Use the machine parameter suppressDepthErr to define
whether, if a positive depth is entered, the TNC should
output an error message (on) or not (off).
Danger of collision!