Milling Cycles - Siemens SINUMERIK 808D User Manual

Se quence
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
N20 T10
N30 M06
S800 M3
M08 F140
G0 X0 Y0 Z20
MCALL CYCLE82 (2, 0, 2, -5, 5, 0)
N40 CYCLE802 (111111111, 111111111, 20, 20, 40,
25, 30, 40)
N50 MCALL
N60 M30
12.6

Milling cycles

12.6.1 Requirements
C a ll 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.
The center point coordinates for the milling pattern or the pocket to be machined are programmed in a rectangular
coordinate system.
The G functions active prior to the cycle call and the current programmable frame remain active beyond the cycle.
186
; Absolute dimension data X/Y plane
; Selects the tool
; Tool change
; Spindle speed clockwise rotation of the spindle
; Feedrate Coolant on
; Approach starting position
; Modal call of the drilling
; call cycle positions
; Deselect modal call
; End of the program
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017