Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 376)

Axis Motion
Chapter 14
14-18
Important: When the control executes a G28 or G30 block, it temporarily
removes any tool offsets and cutter compensation during the axis move to
the intermediate point. The offsets and/or cutter compensation are
automatically re-activated during the first block containing axis motion
following the G28 or G30, unless that block is a G29 block. If a G29
follows, the offsets and/or cutter compensation remain deactivated on the
way to the intermediate point and are re-activated when the axis moves
from the intermediate point back to the point indicated in the G29 block.
The G04 command delays the execution of the next data block. Dwell
length is specified in either of two types.
Seconds
Number of spindle revolutions
The type used is normally dependant on the feedrate mode (G94 or G95)
active at the time. The type can also be permanently fixed to “seconds”
regardless of G94 or G95 mode, by setting the proper AMP parameter.
Dwell is not possible in the G93 inverse time feed mode.
In the G94 mode (feed per minute) G04 suspends execution of the
commands in the next block for a programmed length of time in seconds.
G94G04 P__; X__; U__;
Specify the required dwell time by either a P-, X-, or U-word in units of
seconds. It does not matter which of these three words you use, as long as
only one appears in the same block. The allowable dwell time is 0.001 -
99999.999 seconds.
When you program a dwell in seconds you system installer has the option
of writing PAL to allow a portion of the dwell to be skipped. If this feature
is used, when the appropriate signal is sent to PAL (from a switch or other
device) the control automatically skips any portion of the dwell that has
not been executed and proceeds to the next block in the program. The axes
positions when the skip signal is sent to PAL is recorded and stored as
system parameters #5071 - #5076. See specifics on the G31 skip cycles for
details.
14.3
Dwell (G04)
14.3.1
Dwell - Seconds