Siemens SINUMERIK 808D Programming And Operating Manual

Cycles
2.4 Drilling cycles
Turning Part 2: Programming (Siemens instructions)
132 Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
For example, to machine a center hole (in Z) in the G18 plane, you program:
G18
AXN=1
Programming example: Tapping without encoder
Tapping is carried out without encoder at position X0; the drilling axis is the Z axis. The
parameters SDR and SDAC for the direction of rotation must be assigned; parameter ENC is
assigned the value 1, the value for the depth is the absolute value. Lead parameter PIT can
be omitted. A compensating chuck is used in machining.
N10 G90 G0 G54 D1 T6 S500 M3 ; Specification of technology
values
N20 G17 X0 Z60 ; Approach drilling position
N30 G1 F200 ; Setting the path feedrate
N40 CYCLE840(3, 0, , -15, 0, 1, 4, 3, 1, , ,3) ; Cycle call; dwell time 1 s;
direction of rotation for
retraction M4; direction of
rotation after cycle M3; no
safety clearance
The MPIT and PIT parameters have
been omitted.
N50 M2 ; End of program
Programming example: Tapping with encoder
This program is used for tapping with encoder at position X0. The drilling axis is the Z axis.
The lead parameter must be defined, automatic reversal of the direction of rotation is
programmed. A compensating chuck is used in machining.
N10 G90 G0 G54 D1 T6 S500 M3 ; Specification of technology
values
N20 G17 X0 Z60 ; Approach drilling position
N30 G1 F200 ; Setting the path feedrate
N40 CYCLE840(3, 0, , -15, 0, 0, , ,0, 3.5, ,3) ; Cycle call without safety
clearance
N50 M2 ; End of program

Siemens SINUMERIK 808D Specifications

General

Brand	Siemens
Model	SINUMERIK 808D
Category	Control Unit
Language	English