Programming instructions

4-24
Motion Blocks NC Programming 17VRS
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Thread Cutting 'G33'
The G33 function thread cutting can be used to cut
•
single or multiple point longitudinal threads,
•
face threads and
•
taper threads with a constant lead.
Lead
Longitudinal Thread
1 Thread
Fig. 4-32: Longitudinal threads
G33 <end point [X,Y,Z]> <lead [I,J,K]> <starting angle [P]>
The thread length is the difference between the starting point and the end
point that is programmed in the G33 NC-block. The thread entry length
and exit length in which the feedrate will be accelerated or reduced must
be taken into account. The coordinate values can be programmed using
absolute (G90) or incremental (G91) positioning data.
The thread lead is entered in addresses I, J and K; however, no more
than one interpolation parameter can be programmed in a single thread
NC-block. The interpolation parameters I, J and K are programmed as
unsigned incremental values. The interpolation parameters I, J and K are
assigned to axes X, Y and Z.
The thread starting angle may be programmed as a value from 0° to 360°
in address P. Programming a thread starting angle allows multiple threads
to be cut without offsetting the starting point. If a starting angle is not pro-
grammed at address P, it is assumed that the starting angle is 0°.
Clockwise or counterclockwise threads are produced by stating the direc-
tion of spindle rotation: M03 or M04. If a different spindle is selected for
thread cutting using G33, the spindle must be activated by means of the
SPF <spindle number> command prior to the G33 NC-block. The spindle
number 1 (S/S1) is always active in the power-on state. The spindle must
be starting at the desired RPM prior to or in the G33 NC-block.
In any event, positioning with minimized lag G06 must always be used for
thread cutting with G33 since this function improves thread quality.
G33 is one of the G-codes which are active only for one NC-block at a
time so that it stops being active after the NC-block is completed. The
thread is cut from the cutting starting point up to the programmed end
point of the NC-block; motion is possible in several axes (taper threads).
•
No more than 500 threads can be cut per thread NC-block. If more
than 500 threads are required, they can be machined using thread NC-
block sequences.
•
The maximum spindle speed in the thread NC-block is 13,500 rpm:
The necessary approach distance increases as the spindle speed and
thread lead increase.
•
The constant surface speed, G96, is ignored with thread cutting via
G33. The spindle speed which was last programmed under G97 is set.
Syntax