Rigid Tapping - HEIDENHAIN TNC 426 PB/M Technical Manual

Table of Contents

6.12.10 Rigid Tapping

December 2001

Define the rigid tapping process in the NC program with Cycle 17.

While Cycle 17 is running, the TNC switches automatically to velocity

feedforward mode.

Define the dynamic response of the spindle and the machine tool axes in

machine parameters. (See "The Control Loop" on page 6 – 109); (See

"Spindle" on page 6 – 180).

With Cycle 17 the spindle can also be feedback-controlled. This results in a

better speed curve:

Set MP7160 bit 2 = 1 to drive the spindle under position feedback control

with Cycle 17.

With small thread depths and excessive spindle speeds it is possible that the

programmed spindle speed may not be attained. The immediate transition

from the acceleration phase to the braking phase can diminish the quality of

Set MP7160 bit 1 = 1 in order to limit the spindle speed so that the spindle

runs for about 1/3 of the tapping time at a constant speed.

During tapping, the position of the tool axis tracks the actual position of the

Please note that the use of IPC and acceleration feedforward control for the

tool axis makes the tool axis sensitive to fluctuations in spindle speed caused,

for example, by gear transmission. If this happens, the tool axis starts to run

In MP7160, set bit 3 = 1 to switch off IPC and acceleration feedforward

control for Cycle 17.

Before tapping, the axes (e.g. Z and S) are synchronized through an oriented

spindle stop, i.e., every Z position is assigned to a certain spindle angle. The

NC orients the spindle. The NC sets M4017. The position control loop must be

closed (M4012). (See "Oriented Spindle Stop" on page 6 – 201)

Synchronization makes it possible to cut the same thread more than once. The

assigned spindle angle depends on the thread pitch entered in the cycle. You

can deselect this function to save machining time:

Set MP7160 bit 0 = 1

In this case you cannot cut the thread more than once.