Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 419)

Spindles
Chapter 17
17-21
End Face Milling Block Format
The block used to activate virtual C axis end face milling has this format:
G16.2 X__ Y__ Z__ R__ F__
Where : Is :
X The coordinate (if in G90 absolute mode) or the linear distance (if in G91
incremental mode) to which the X axis is to move. Be aware that this value is
affected by diameter (G08) or radius (G07) programming mode.
Y The coordinate (if in G90 absolute mode) or the linear distance (if in G91
incremental mode) to which the simulated Y axis is to move.
Z The coordinate (if in G90 absolute mode) or the linear distance (if in G91
incremental mode) to which the Z axis is to move. This axis determines depth of
cut in End Face Milling.
R The radius of the arc to be cut in the face of the part. This parameter can be
used only if G02 or G03 circular interpolation has been activated, and must be
programmed with the correct X and Y coordinates. See chapter 14.
F The feedrate to be used by the X, Y, and Z axes when commanded to move while
G16.2 is active.
These parameters and their application are described in detail in the
paragraphs that follow:
Any axis motions except for C axis motions can be programmed in the
G16.2 block. The control generates C axis motion in response to
programmed requests for simulated Y axis motion. This allows the
programmer to enter his contour moves as though he were working with an
XY plane, with cutting depth controlled by the Z axis.
If G02 or G03 circular interpolation is made active while in G16.2 end face
milling mode, circular cuts can be made in the face of the part (for
example, the corners could be rounded in the contour illustrated in
Figure 17.5). This is accomplished by programming the X and Y axis
endpoints along with the desired circle radius R as described in chapter 14.
The R parameter used here defines the radius of the circular path to be cut.
Important: When programming circular interpolation in G16.2 mode,
only radius programming (using R) may be used. Integrand programming
(using I, J) is not allowed and generates the error message “CIRCLE
PROGRAMMING ERROR.”
Important: When programming circular interpolation in incremental
mode (G91), the programmed X move length along with the programmed
Y move length, must position the X and Y axes at a legal endpoint for the
circular radius defined by the R value in the G02/G03 block. In absolute
mode (G90) the coordinate programmed for the X axis along with the
coordinate programmed for the Y axis, must position the X and Y axes at
a legal endpoint for the circular radius defined by the R value in the
G02/G03 block.