Siemens CNC | CYCLE81 | Drilling and Centering


CYCLE81 Introduction

The tool drills at the programmed spindle speed and feedrate to the specified final drilling depth.

Supported CNC Series

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

CYCLE81 Format

CYCLE81 (RTP, RFP, SDIS, DP, DPR)

Parameters

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)

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. ;
MCALL;
M30;

CYCLE81 Examples

CYCLE81 CNC Program Example – 1

Use this program to produce 3 drill holes using the CYCLE81 drilling cycle, whereby this is
called using different parameters. The drilling axis is always the Z axis.

Siemens CNC Milling CYCLE81 Program Example

N10 G0 G90 F200 S300 M3 ; Specification of technology values
N20 D1 T3 Z110 ; Approach retraction plane
N21 M6 ;
N30 X40 Y120 ; Approach first drilling position
N40 CYCLE81(110, 100, 2, 35) ; Cycle call with absolute end drilling ;depth, safety clearance and incomplete ;parameter list
N50 Y30 ; Approach next drilling position
N60 CYCLE81(110, 102, , 35) ; Cycle call without safety clearance
N70 G0 G90 F180 S300 M03 ; Specification of technology values
N80 X90 ; Approach next position
N90 CYCLE81(110, 100, 2, , 65) ; Cycle call with relative end drilling;depth, and safety clearance
N100 M30 ; Program end