Siemens CNC | CYCLE87 | Boring 3

CYCLE87 Introduction

The tool drills at the programmed spindle speed and feedrate to the entered final drilling
depth. During boring 3, a spindle stop without orientation M5 is generated after reaching the final drilling depth, followed by a programmed stop M0. Pressing the NC START key continues the retraction 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.

CYCLE87 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)
SDIR = Direction of rotation; Values: 3: (for M3); 4: (for M4)

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. ;

CYCLE87 Examples

CYCLE87 CNC Program Example – 1

CYCLE87 is called at position X70 Y50 in the XY plane. The drilling axis is the Z axis. The
final drilling depth is specified as an absolute value. The safety clearance is 2 mm.

Siemens CNC Cycle87 Program Example

DEF REAL DP, SDIS ; Definition of parameters
N10 DP=77 SDIS=2 ; Value assignments
N20 G0 G17 G90 F200 S300 ; Specification of technology values
N30 D1 T3 Z113 ; Approach retraction plane
N40 X70 Y50 ; Approach drilling position
N50 CYCLE87 (113, 110, SDIS, DP, , 3) ; Cycle call with programmed ;direction of spindle rotation M3
N60 M30 ; Program end