Siemens CNC | CYCLE86 | Boring 2

CYCLE86 Introduction

The tool drills at the programmed spindle speed and feedrate velocity up to the entered
drilling depth. With CYCLE86 (Boring 2), oriented spindle stop is activated with the SPOS command once the drilling depth has been reached. Then, the programmed retraction positions are approached in rapid traverse and, from there, the retraction plane.

Note: Cycle CYCLE86 can be used if the spindle to be used for the boring operation is technically able to go into position-controlled spindle operation.

Supported CNC Series

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

CYCLE86 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)
SDIR = Direction of rotation; Values: 3: (for M3); 4: (for M4)
RPA = Retraction path along the abscissa of the active plane (incremental, enter with sign)
RPO = Retraction path along the ordinate of the active plane (incremental, enter with sign)
RPAP = Retraction path along the boring axis (incremental, enter with sign)
POSS = Spindle position for oriented spindle stop in the cycle (in degrees)

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. ;

CYCLE86 Examples

CYCLE86 CNC Program Example – 1

CYCLE86 is called at position X70 Y50 in the XY plane. The drilling axis is the Z axis. The final drilling depth is programmed as an absolute value; no safety clearance is specified. The dwell time at the final drilling depth is 2 sec. The top edge of the workpiece is positioned at Z110. In the cycle, the spindle is to rotate with M3 and to stop at 45 degrees.

Siemens CNC Cycle86 Program Example

DEF REAL DP, DTB, POSS ; Definition of parameters
N10 DP=77 DTB=2 POSS=45 ; Value assignments
N20 G0 G17 G90 F200 S300 ; Specification of technology values
N30 D1 T3 Z112 ; Approach retraction plane
N40 X70 Y50 ; Approach drilling position
N50 CYCLE86 (112, 110, , DP, , DTB, 3, –1, –1, +1, POSS) ; Cycle call with absolute drilling depth
N60 M30 ; Program end