Programming instructions

4-30
Motion Blocks NC Programming 17VRS
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Rigid Tapping 'G63' / 'G64'
Threads can be tapped without a compensating chuck using the function
G63. With thread tapping without compensating chuck the spindle align-
ment is controlled and not, as would be the case in normal tapping, the
spindle rpm. The spindle motion and the infeed motion of the axis which
is programmed together with G63 are interpreted linearly. A positionable
main spindle is needed for tapping without compensating chuck. The
spindle must be driven directly (slip), and the position encoder should be
located directly on the spindle.
The CNC supplies two preparatory functions for tapping without compen-
sating chuck. These functions are only active for the duration of the NC-
block containing them.
•
G63 - Spindle stops at end of motion
The functions G63 and G64 differ only with respect to the end of motion.
G63 <end point [X,Y,Z]> <feed per spindle revolution [F]>
G64 <end point [X,Y,Z]> <feed per spindle revolution [F]>
Two cases are possible when the feed/spindle link is established:
•
The spindle is stopped (n=0)
•
The spindle is already rotating (n=S)
If the spindle is stopped when the feed/spindle link is established, the link
can be activated at the start of the common acceleration phase so that
the spindle and the feed axis are already interpolating upon acceleration.
Which acceleration is selected will depend on which axis is the weakest
(main spindle or feed axis).
If the spindle is already rotating when the feed/spindle link is established,
the feed axis is accelerated to the required speed at its maximum accel-
eration, and then the link is activated, so that the main spindle and the
feed axis do not interpolate until the constant-speed range is reached.
•
Clockwise or counter-clockwise thread tapping is achieved by stating
the direction of spindle rotation: M03 or M04.
•
If a different spindle is to be selected for thread tapping using G63/64,
the spindle must be activated by means of the SPF <spindle number>
command prior to the G63 NC-block. The first spindle (S/S1) is always
active in the power-on state.
•
Tapping should be performed using the preparatory function G06 po-
sitioning with minimized lag. If G06 is not active with tapping without
compensating chuck or if analog axis cards are installed, the same
gain factor must be set for the spindle and for the infeed axis for
G63/G64.
•
The functions G08 contouring mode (acceleration) and G61 exact stop
before NC-block transition are meaningless for tapping.
•
A main spindle which is stopped at the end of motion (G63) can be
reactivated using the spindle control commands M03/M04 and by pro-
gramming the rpm value (S value).
•
If the tap is turned out of the thread using G64, the spindle stops
briefly at the end point of the NC-block in order to change from posi-
tion-controlled to rpm-controlled mode.
•
Except for time-based dwell G04 and the auxiliary functions, no NC
commands can be programmed between the G63 command tap to
depth <X, Y or Z> and the G63/G64 command withdraw tap.
•
With digital drives, if the spindle is activated prior to the NC-block
containing G63 tapping, the spindle will stop briefly in the G63 NC-
block in order to switch from rpm-controlled mode to position-con-
trolled mode.
Syntax