Siemens SINUMERIK 808D ADVANCED - Milling Cycles; Requirements

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014
161
Function
This cycle allows you to freely program positions, i.e., rectangular or polar. Individual positions are approached in the order
in which you program them.
Sequence
The drilling tool in the program traverses all programmed positions in the order in which you program them. Machining of the
positions always starts at the reference point. If the position pattern consists of only one position, the tool is retracted to the
retraction plane after machining.
Explanation of the parameters
X0, Y0...X4, Y4
All positions will be programmed absolutely.
Programming example:
Drilling in G17 at the Positions
X20 Y20
X40 Y25
X30 Y40
N10 G90 G17
; Absolute dimension data X/Y plane
N20 T10
; Selects the tool
N30 M06
; Tool change
S800 M3
; Spindle speed clockwise rotation of the spindle
M08 F140
; Feedrate Coolant on
G0 X0 Y0 Z20
; Approach starting position
MCALL CYCLE82 (2, 0, 2, -5, 5, 0)
; Modal call of the drilling
N40 CYCLE802 (111111111, 111111111, 20, 20, 40,
25, 30, 40)
; call cycle positions
N50 MCALL
; Deselect modal call
N60 M30
; End of the program
9.6
Milling cycles
9.6.1
Requirements
Call and return conditions
Milling cycles are programmed independently of the particular axis name.
Before you call the milling cycles, a tool compensation must be activated.
The appropriate values for feedrate, spindle speed and direction of rotation of spindle must be programmed in the part
program if the appropriate parameters are not provided in the milling cycle.