Reaming1 - Cycle85 - Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual

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
N20 G17 X0 Z60
N30 G1 F200
N40 CYCLE840(3, 0, , -15, 0, 0, , ,0, 3.5, ,3)
N50 M2
9.4.8

Reaming1 - CYCLE85

Programming
CYCLE85 (RTP, RFP, SDIS, DP, DPR, DTB, FFR, RFF)
Parameters
Parameter Data type
RTP REAL
RFP REAL
SDIS REAL
DP REAL
DPR REAL
DTB REAL
FFR REAL
RFF REAL
Function
The tool drills at the programmed spindle speed and feedrate velocity to the entered final drilling depth.
The inward and outward movement is performed at the feedrate assigned to FFR and RFF respectively.
This cycle can be used for reaming of bore holes.
Sequence
Position reached prior to cycle start:
The drilling position is the position in the two axes of the selected plane.
See the following illustration for sequence of operations:
Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015
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)
Dwell time at final drilling depth (chip breakage)
Feedrate
Retraction feedrate
; Specification of technology values
; Approach drilling position
; Setting the path feedrate
; Cycle call without safety clearance
; End of program
141