0 votes
in cnc programming by (9.4k points)

In this article, we describe how to use Siemens CYCLE84 code on CNC machines with all details and examples.

The tool drills at the programmed spindle speed and feedrate to the entered final thread
CYCLE84 can be used to make tapped holes without compensating chuck.
The cycle is also capable of performing tapping operations in several stages (deep-hole


CYCLE84 can be used if the spindle to be used for the boring operation is technically able
to be operated in the position-controlled spindle operation.



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)
SDAC = Direction of rotation after end of cycle (Values: 3, 4 or 5)
MPIT = Pitch as a thread size (signed) ( Range of values: 3: (for M3) to 48: (for M48), the sign determines the direction of rotation in the thread )
PIT = Pitch as a value (signed) ( Range of values: 0.001 … 2000.000 mm), the sign determines the direction of rotation in the thread: if _PTAB=0 or 1: in mm (as previously); if _PTAB=2: in thread grooves per inch; if _PTAB=3: in inches/rotation )
POSS = Spindle position for oriented spindle stop in the cycle (in degrees)
SST = Speed for tapping
SST1 = Speed for retraction
_AXN = Tool axis ( Values: 1: 1st geometrical axis; 2: 2ndgeometrical axis; otherwise 3rd geometrical axis )
_PTAB = Evaluation of thread pitch PIT; ( Values: 0: corresponds to programmed measuring system inch/metric; 1: pitch in mm; 2: pitch in thread grooves per inch; 3: pitch in inches/rotation)
_TECHNO = Technological settings; Values :
UNITS DIGIT: Exact stop behavior
0: as programmed before cycle call
1: (G601)
2: (G602)
3: (G603)
TENS DIGIT: Feed-forward control
0: as programmed before cycle call
1: with feed-forward control (FFWON)
2: without feed-forward control (FFWOF)
HUNDREDS DIGIT: Acceleration
0: as programmed before cycle call
1: axis acceleration with jerk limitation (SOFT)
2: abrupt axis acceleration (BRISK)
3: reduced axis acceleration (DRIVE)
_TECHNO integer
0: reactivate spindle operation (for MCALL)
1: remain in position-controlled operation (for MCALL)
_VARI = Machining type; ( Values: 0: tapping in one pass; 1: deep-hole tapping with chip breakage; 2: deep-hole tapping with chip removal)
_DAM = Incremental drilling depth; (Range of values: 0 <= max. value)
_VRT = Variable retraction value for chip breakage; ( Range of values: 0 <= max. value )
Note: 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. ;


A thread is tapped without compensating chuck at position X30 Y35 in the XY plane; the
tapping axis is the Z axis. No dwell time is programmed; the depth is programmed as a

relative value. The parameters for the direction of rotation and for the pitch must be assigned values. A metric thread M5 is tapped.

Siemens CNC CYCLE84 Program Example

N10 G0 G90 T4 D1 ;Specification of technology values
N20 G17 X30 Y35 Z40 ;Approach drilling position
N30 CYCLE84 (40, 36, 2, , 30, , 3, 5, 90, 200, 500)
;Cycle call, parameter PIT has been
;omitted, no indication of absolute
;depth, no dwell time,
;Spindle stop at 90 degrees,
;rotational speed during tapping is 200,
;Speed for retraction is 500
N40 M30 ;Program end

Note :

For tapping with compensating chuck, a separate cycle CYCLE840 is provided.

Your answer

Your name to display (optional):
Privacy: Your email address will only be used for sending these notifications.
Anti-spam verification:
To avoid this verification in future, please log in or register.