HEIDENHAIN TNC 410 - Manual (Page 147)

8 Programming: Cycles 134
RIGID TAPPING GS
(Cycle 17)
Machine and control must be specially prepared by the
machine tool builder to enable rigid tapping.
The TNC cuts the thread without a floating tap holder in one or
more passes.
Rigid tapping offers the following advantages over tapping with a
floating tap holder
■ Higher machining speeds possible
■ Repeated tapping of the same thread is possible; repetitions are
enabled via spindle orientation to the 0° position during cycle call
(depending on machine parameter 7160).
■ Increased traverse range of the spindle axis due to absence of a
floating tap holder.
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 parameter total hole depth
determines the working direction.
The TNC calculates the feed rate from the spindle speed.
If the spindle speed override is used during tapping, the
feed rate is automatically adjusted.
The feed-rate override knob is disabled.
At the end of the cycle the spindle comes to a stop.
Before the next operation, restart the spindle with M3
(or M4).
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 (beginning of thread) and
end of thread
ú PITCH :
Pitch of the thread. The algebraic sign differentiates
between right-hand and left-hand threads:
+ = right-hand thread
– = left-hand thread
8.3 Dr
illing Cy
cles
X
Z
Example NC blocks:
18 CYCL DEF 17.0 RIGID TAPPING GS
19 CYCL DEF 17.1 SET UP 2
20 CYCL DEF 17.2 DEPTH -20
21 CYCL DEF 17.3 PITCH +1