Siemens CNC | CYCLE88 | Boring 4

CYCLE88 Introduction

The tool drills at the programmed spindle speed and feedrate to the entered final drilling depth. During CYCLE88 (boring pass 4), a dwell time, a spindle stop without orientation M5 and a programmed stop M0 are generated when the final drilling depth is reached. Pressing the NC START key traverses the outward movement at rapid traverse until the retraction plane is reached.

Supported CNC Series

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

CYCLE88 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 final drilling depth
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. ;

CYCLE88 Examples

CYCLE88 CNC Program Examples – 1

CYCLE88 is called at position X80 Y90 in the XY plane. The drilling axis is the Z axis. The safety clearance is programmed at 3 mm. The final drilling depth is specified relative to the reference plane. M4 is active in the cycle.

Siemens CNC Cycle88 Program Example

DEF REAL RFP, RTP, DPR, DTB, SDIS ; Definition of parameters
N10 RFP=102 RTP=105 DPR=72 DTB=3 SDIS=3 ; Value assignments
N20 G17 G90 T1 D1 F100 S450 ; Specification of technology values
N21 M6 ;
N30 G0 X80 Y90 Z105 ; Approach drilling position
N40 CYCLE88 (RTP, RFP, SDIS, , DPR, DTB, 4) ; Cycle call with programmed ;direction of spindle rotation M4
N50 M30 ; Program end