Siemens CNC | CYCLE85 | Boring 1

CYCLE85 Introduction

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.

Supported CNC Series

Siemens CNC 802D, 810D, 840D, 840D sl, 840Di, 840Di sl series controllers.

CYCLE85 Format



RTP = Retraction plane (absolute)
RFP = Reference plane (absolute)
SDIS = Safety clearance (enter without sign)
DP = Final drilling depth (absolute)
DPR = Final drilling depth relative to the reference plane (enter without sign)
DTB = Dwell time at thread depth (chip breaking)
FFR = Feedrate
RFF = Retraction feedrate

Repeat the Cycle

To repeat the cycle in more than one position, MCALL must be written at the beginning of the cycle. The MCALL command is active until the next call. If it is written after positioning the command, MCALL will be canceled.

MCALL Example

X30. Y20.;
MCALL CYCLExx …….. ;
X10. Y10. ;
X-140. Y35. ;

CYCLE85 Examples

CYCLE85 CNC Program Example – 1

CYCLE85 is called at position Z70 X50 in the ZX plane. The boring axis is the Y axis. The value for the final drilling depth in the cycle call is programmed as a relative value; no dwell time is programmed. The workpiece upper edge is at Y102.

Siemens CNC Cycle85 Program Example

DEF REAL FFR, RFF, RFP=102, DPR=25,SDIS=2 ; Definition of the parameters and value assignments
N10 G0 FFR=300 RFF=1.5*FFR S500 M4 ; Specification of technology values
N20 G18 T1 D1 Z70 X50 Y105 ; Approach drilling position
N21 M6 ;
N30 CYCLE85 (RFP+3, RFP, SDIS, , DPR, , FFR, RFF) ; Cycle call, no dwell time; programmed
N40 M30 ; Program end