HEIDENHAIN TNC 310 (286 140) - Manual (Page 109)

97 HEIDENHAIN TNC 310
PECKING (Cycle 1)
1 The tool drills from the current position to the first plunging
depth at the programmed feed rate F.
2 When it reaches the first plunging depth, the tool retracts in rapid
traverse FMAX to the starting position and advances again to the
first plunging depth minus the advanced stop distance t.
3 The advanced stop distance is automatically calculated by the
control:
■ At a total hole depth of up to 30 mm: t = 0.6 mm
■ At a total hole depth exceeding 30 mm: t = hole depth / 50
Maximum advanced stop distance: 7 mm
4 The tool then advances with another infeed at the programmed
feed rate F.
5 The TNC repeats this process (1 to 4) until the programmed total
hole depth is reached.
6 After a dwell time at the hole bottom, the tool is returned to the
starting position in rapid traverse FMAX for chip breaking.
Before programming, note the following:
Program a positioning block for the starting point (hole
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 cycle parameter TOTAL HOLE
DEPTH determines the working direction.
ú Setup clearance (incremental value): Distance
between tool tip (at starting position) and
workpiece surface
ú Total hole depth (incremental value):
Distance between workpiece surface and bottom
of hole (tip of drill taper)
ú Plunging depth (incremental value):
Infeed per cut. The TNC will go to depth in one
movement if:
■ the plunging depth is the same as the total hole
depth
■ the plunging depth is greater than the total hole
depth
The total hole depth does not have to be a multiple
of the plunging depth.
ú Dwell time in seconds: Amount of time the tool
remains at the total hole depth for chip breaking
ú Feed rate F: Traversing speed of the tool during
drilling in mm/min
8.2 Dr
illing Cy
cles
X
Z