Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 594)

Compounding Turning Routines
Chapter 24
24-30
The G75 block is programmed with this format:
G75 P__ Q__ I__ K__ U__ W__ D__ F__ S__ T__;
Where : Is :
P__ The sequence number of the first block in the set of contour blocks that defines the
finished workpiece shape.
Q__ The sequence number of the last block in the set of contour blocks that defines the
finished workpiece shape.
U W Finish allowance. These parameters determine the finishing allowance that is left on
the part when the routine is completed. This finish allowance is typically removed
later in the program when a G72 finishing routine block is executed. The actual value
of the finish allowance is equal to the average of the U and W parameters ((U+W)/2).
It is not necessary to enter both of these parameters in the calling block. If only one
is entered, the control uses half of the entered parameter value as the finish amount.
The finish allowance is optional and does not need to be programmed. See
Figure 24.25 to determine the sign of U and W. U and W are always programmed as
incremental values.
Important: This manual makes the assumption that W and U are assigned in
AMP as the incremental axis names that correspond to the Z and X axes
respectively.
Important: The value assigned to U is affected by radius/diameter mode
(G08/G09). W is not affected by radius diameter mode. If programming in diameter
mode the value of the finish allowance is really ((U/2)+W)/2.
I K These parameters determine the incremental distance between the first and last pass
of the routine. This distance is equal to the average of the I and K parameters
((I+K)/2). The location of the last pass is determined by the contour blocks and the
finish amount ((U+W)/2), if any is programmed. I and K must be programmed. They
are neither positive nor negative.
Important: This total incremental distance should be less than one tool radius if
cutter compensation is on when this cycle is executed.
Important: This manual makes the assumption that K and I are assigned in
AMP as the integrand axis names that correspond to the Z and X axes respectively.
Important: The values assigned to I and K are always an incremental, radius
value regardless of the current mode (radius/diameter or absolute/incremental).
D__ Number of passes. The integer value entered with this parameter determines how
many passes are made to reach the final pass. The depth of each pass is
determined by dividing (I+K)/2 by D-1. The value entered with D must be an integer.
F__
Active feedrate during the routine only (see chapter 17)
S__ Spindle speed during the routine only (see chapter 16)
T__ Tool number and tool offset to be used during the routine only (see chapter 19)
Important: Any F-, S-, or T-words that are in the set of contour blocks are
ignored when the routine is executed. If these words are to be changed
from their current value, it is necessary to program an F-, S-, or T-word in
the G75 block. If programmed in the G75 block these words replace any
previously active modal F-, S-, or T-words for the remainder of G75
routine operation only. When the G75 routine is completed the previously
active modal F-, S-, and T-words are reactivated.