Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 607)

Thread Cutting
Chapter 25
25-7
Where : Is :
X This parameter is the end point of the thread cutting move in the X axis. This parameter may be an incremental or absolute and radius or
diameter value. If not present there must be a Z parameter. If an X parameter is present, it indicates either a face, tapered, or lead-in
thread. When used in a G33 block without a Z parameter, a facing thread is made parallel to the X-axis at the Z axis position prior to the
G33 block. X values maybe entered as a radius or a diameter value. X may also be programmed as an incremental or absolute value.
The initial minor diameter of any straight or tapered thread is determined by the position of the X axis prior to the G33 block.
Z This parameter is the end point of the thread cutting move in the Z axis. This parameter may be an incremental or absolute value. If not
present there must be an X parameter. When a Z parameter is used in a G33 block without an X parameter the threading pass is made
parallel to the Z-axis at whatever X position the tool tip was at prior to the G33 block.
E F This parameter may be entered by using either an E- or F-word. It represents the thread lead along the axis with the largest programmed
distance to travel to make the thread cut. It is mandatory when cutting any threads.
If the E-word is programmed, its value (sign ignored) is equal to the number of threads per inch or inches per thread (determined in AMP)
regardless of whether inch or metric mode is active at the time.
If the F-word is programmed, its value (sign ignored) is the thread lead in inches per revolution or millimeters per revolution, depending on
the mode in which the control is operating.
Q This optional parameter provides a relative value for the start offset angle of the thread. Its primary use is in cutting multistart threads.
For example, if a threading pass were made with a value of zero here, and then followed by another pass with a value of 180 then the
second cut would be started 180 degrees from the first resulting in a two start thread. If two more passes are then made, one with a
parameter value of 90 and one with a value of 270, the result would be a four-start thread.
Figure 25.4
G33 Block Parameters
Z
Inc.
Z
Abs.
Z
X Abs.
X Inc.
X
Q
1/E, E or F
Important: Do not re-program the G33 command in consecutive threading
blocks. Doing so will cause the control to pause axis motion (possibly
damaging the thread) while the axis re--synchronizes with the spindle.
Consecutive threading blocks in the following example are blocks N3 and
N4, and blocks N8 and N9.