Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 653)

Milling Fixed Cycles
Chapter 26
26-21
In the G82 drilling cycle, the control moves the axes in the following
manner:
1. The tool rapids to initial point level point above the hole location.
2. The drilling tool then rapids to the R point level, slows to the
programmed cutting feedrate and begins the drill operation.
3. The cutting tool drills at the programmed feedrate to the
pre-programmed depth of the hole (defined by the Z--word in the
boring cycle block).
4. If a value was programmed for the P parameter, the drilling tool will
dwell after it reaches the bottom of the hole.
5. After the drilling tool reaches the hole bottom and the dwell is
completed, the drilling tool is retracted at a rapid feedrate to the
initial point level as determined by G98.
When the single block function is active, the control stops axis motion
after steps 1, 2 and 5.
The format for the G83 cycle is as follows:
G83X__Y__Z__R__Q__F__L__;
Where : Is :
X,Y specifies location of the hole.
Z defines the hole bottom.
R defines the R point level.
Q ..defines the infeed amount for each step into the hole.
F defines the cutting feedrate.
L defines the number of times the milling fixed cycle is repeated.
(See section 26.3 for a detailed description of these parameters.)
Important: The programmer or operator must start spindle rotation.
(G83): Deep Hole Drilling
Cycle