Siemens SINUMERIK 808D Programming And Operating Manual page 73

Symbols and figures
Given below is an explanation of the individual fixed cycles. These symbols are used in the following figures:
Note
In all fixed cycles the address character R (distance "initial plane - point R") is treated as radius.
However, Z or X (Distance "point R - bottom of a hole) is always treated as diameter or radius, depending upon the type of
programming.
Deep hole drilling cycle (G83)/Side deep hole drilling cycle (G87)
Whether a deep hole drilling cycle (chip removal) or a high-speed deep hole drilling cycle (chip breaking) is executed,
depends on the setting USER DATA, _ZSFI[20].
If no infeed is specified for the drilling cycle, a normal drilling cycle is executed.
High-speed deep hole drilling cycle (G83, G87) (USER DATA, _ZSFI[20]=0)
In case of the high-speed deep hole drilling cycle, the drill repeats the infeed with the cutting feedrate. This is retracted by a
certain amount till the tool has reached the bottom of a hole.
Format
G83 X(U)... C(H)... Z(W)... R... Q... P... F... M... ;
or
G87 Z(W)... C(H)... X(U)... R... Q... P... F... M... ;
X, C or Z, C: Position of the hole
Z or X: Distance from the point R to the bottom of the hole
R_: Distance from the initial plane to the plane R
Q_: Infeed
P_: Dwell time at the bottom of a hole
F_: Cutting feedrate
K_: Number of repetitions (if required)
M_: M function for locking the C axis (if needed)
Programming and Operating Manual (ISO Turning/Milling)
73
01/2017