Siemens CNC | CYCLE82 | Drilling and Counterboring


CYCLE82 Introduction

The tool drills at the programmed spindle speed and feedrate to the specified final drilling
depth. A dwell time can be allowed to elapse when the final drilling depth has been reached.

Supported CNC Series

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

CYCLE82 Format

CYCLE82 (RTP, RFP, SDIS, DP, DPR, DTB)

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)
DTB = Dwell time at final drilling depth

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;

CYCLE82 Examples

CYCLE82 CNC Program Example – 1

The program machines a single hole of a depth of 27 mm at position X24 Y15 in the XY
plane with cycle CYCLE82.

The dwell time programmed is 2 s, the safety clearance in the drilling axis Z is 4 mm.

Siemens CNC CYCLE82 Program Example

N10 G0 G90 F200 S300 M3 ; Specification of technology values
N20 D1 T3 Z110 ; Approach retraction plane
N21 M6 ;
N30 X24 Y15 ; Approach drilling position
N40 CYCLE82 (110, 102, 4, 75, , 2) ; Cycle call with absolute end drilling depth, ;and safety clearance
N50 M30 ; Program end