Rigid Tapping (Cycle 17) - HEIDENHAIN TNC 426 B User Manual

RIGID TAPPING (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).
Setup clearance
between tool tip (at starting position) and workpiece
surface
Total hole depth
between workpiece surface (beginning of thread) and
end of thread
PITCH :
Pitch of the thread. The algebraic sign differentiates
between right-hand and left-hand threads:
+ = right-hand thread
– = left-hand thread
164
www.EngineeringBooksPdf.com
(incremental value): Distance
(incremental value): Distance
Z
Example NC blocks:
18 Y L DEF 17.0 RIGID TAPPING GS
19 Y L DEF 17.1 SET UP
20 Y L DEF 17.2 DEPTH -20
21 Y L DEF 17.3 PIT H +1
Retracting after a program interruption
If you interrupt program run during tapping with the
machine stop button, the TNC will display the soft
key MANUAL OPERATION. If you press the MANU-
AL OPERATION key, you can retract the tool under
program control. Simply press the positive axis
direction button of the active tool axis.
X
2
8 Programming: Cycles