Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 414)

Spindles
Chapter 17
17-16
Where: Is:
R the radius at which the feed axis (typically the X axis) is positioned at the start of
cylindrical interpolation. Can be used to alter the feed axis depth if programmed in a
G16.1 block during cylindrical interpolation.
C the angular coordinate (if in G90 absolute mode) or the angular distance (if in G91
incremental mode) to which the virtual C 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.
F the feedrate to be used by the feed axis to position to radius R, and used by the Z axis
when commanded to move while G16.1 is active.
It also controls the virtual C axis speed as though it were a rotary axis. See chapter 18.
These parameters and their application are described in detail in the
paragraphs that follow:
The valued entered for the R parameter should place the tool at the radius
of the desired cutting depth into the part.
Important: R must be programmed in the initial G16.1 block. If R is not
programmed in the initial G16.1 block, the error message “CYLINDER
RADIUS IS ZERO” appears. At power turn-on, program-end (M02, M30,
or M99) or control reset, the virtual C axis feature is turned off and the R
value is set to zero. It must then be re-entered in the next G16.1 block.
The radius specified by the R parameter is modal and does not need to be
included in subsequent cylindrical interpolation blocks. Programming a
G16.1 block with a different R value modifies the feed depth to the new
radius. Feed depths cannot be changed using the X parameter when G16.1
is active. Programming an X generates the error message “FEED AXIS
MOTION NOT ALLOWED.”
Figure 17.3 illustrates the tool position if the AMP parameter Feed Axis
Park Location is selected as “Farthest from Machine Zero.” If “Nearest
to Machine Zero” were selected, then the tool would be positioned for
cutting into the part from the negative side of the X axis. Refer to the
information provided by your system installer.
A C or Z axis position may be programmed with the R parameter in the
initial G16.1 block. However, once G16.1 mode is established, only the Z
parameter can be programmed in the same block as the R parameter.
When it is, the Z axis motion executes first followed by feed axis motion to
radius R.
If a C axis position is programmed, the C axis rotates to the specified
angle. If the C and Z axes are programmed together in the same block,
then a vector motion results around the circumference of the part.