Thread Milling - Cycle90 - Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual

Programming example: Circular pocket
With this program, you can machine a circular pocket in the YZ plane. The center point is determined by Y50 Z50. The
infeed axis for the depth infeed is the X axis. Neither finishing dimension nor safety clearance is specified. The pocket is
machined with down-cut milling. Infeed is performed along a helical path.
A milling cutter with 10 mm radius is used. See the following programming example for circular pocket:
N10 G17 G90 G0 S650 M3 T1 D1
N20 X50 Y50
N30 POCKET4(3, 0, 0, -20, 25, 50, 60, 6, 0, 0, 200, 100, 1,
21, 0, 0, 0, 2, 3)
N40 M02
9.6.11

Thread milling - CYCLE90

Programming
CYCLE90 (RTP, RFP, SDIS, DP, DPR, DIATH, KDIAM, PIT, FFR, CDIR, TYPTH, CPA, CPO)
Parameters
Parameter Data type
RTP REAL
RFP REAL
SDIS REAL
DP REAL
DPR REAL
DIATH REAL
KDIAM REAL
PST REAL
FFR REAL
CDIR INT
TYPTH INT
CPA REAL
CPO REAL
206
Description
Retraction plane (absolute)
Reference plane (absolute)
Safety clearance (enter without sign)
Final drilling depth (absolute)
Final drilling depth relative to the reference plane (enter without sign)
Nominal diameter, outer diameter of the thread
Core diameter, internal diameter of the thread
Thread pitch; value range: 0.001 ... 2000.000 mm
Feedrate for thread milling (enter without sign)
Direction of rotation for thread milling
Values: 2 (for thread milling with G2), 3 (for thread milling with G3)
Thread type
Values: 0=internal thread, 1=external thread
Center point of circle, abscissa (absolute)
Center point of circle, ordinate (absolute)
; Specification of technology values
; Approach starting position
; Cycle call
Parameters FAL and FALD are omitted
; End of program
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014