Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 392)

Axis Motion
Chapter 14
14-16
Cylindrical Interpolation Block Format
The block used to activate cylindrical interpolation has the following
format:
G16.1 R__ X__ Z__ A__ F__
Where : Is :
R The radius at which the feed axis (typically the Z axis) will be 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.
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.
Z The coordinate (if in G90 absolute mode) or the linear distance (if in G91
incremental mode) to which the Z axis (feed axis) is to move.
A The angular coordinate (if in G90 absolute mode) or the angular distance (if in
G91 incremental mode) to which the A rotary axis is to move.
F The feedrate to be used by the X and Z axes when commanded to move while
G16.1 is active. It also controls the A rotary axis speed as. Refer to chapter 18.
These parameters and their application are described in detail in the
paragraphs that follow:
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” will appear. At power turn-on, program-end (M02,
M30, or M99) or control reset the cylindrical interpolation 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 will modify the feed depth to the new
radius. Feed depths cannot be changed using the Z parameter when G16.1
is active. Programming a Z will generate the error message “FEED AXIS
MOTION NOT ALLOWED”.
Figure 14.9 illustrates the tool position if the AMP parameter Feed Axis
Park Location is selected as “Nearest to Machine Zero”. If “Farthest
from Machine Zero” were selected, then the tool would be positioned for
cutting into the part from the positive side of the Z axis. Refer to the
information provided by your system installer.
An A or X axis position may be programmed with the R parameter in the
initial G16.1 block. However, once G16.1 mode is established, only the X
parameter can be programmed in the same block as the R parameter.
When it is, the X axis motion will be executed first followed by feed axis
motion to radius R.