0 votes
in cnc programming by (9.0k points)

In this article, we describe how to use Siemens CYCLE83 code on CNC machines with all details and examples.

The tool drills at the programmed spindle speed and feedrate to the entered final drilling
Deep hole drilling is performed with a depth infeed of a maximum definable depth executed
several times, increasing gradually until the final drilling depth is reached.

Optionally, the drilling machine can be retracted after each infeed depth either to the
reference plane + safety clearance for chip removal or by the length of the programmed
retraction path for chip breakage.



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)
FDEP = First drilling depth (absolute)
FDPR = First drilling depth relative to the reference plane (enter without sign)
DAM = Degression (enter without sign) ( Values: > 0: degression as a quantity; < 0: degression factor; = 0: no degression )
DTB = Dwell time at drilling depth (chip breakage) ( Values: > 0: in seconds; < 0: in revolutions )
DTS = Dwell time at starting point and for chip removal ( Values: > 0: in seconds; < 0: in revolutions )
FRF = Feedrate factor for first drilling depth (enter without sign); (Value range: 0.001…1)
VARI = Machining type ( Values: 0: chip breakage; 1: chip removal )
_AXN = Tool axis ( Values: 1: 1st geometrical axis; 2: 2ndgeometrical axis; otherwise 3rd geometrical axis )
_MDEP = Minimum drilling depth (only in connection with degression factor)
_VRT = Variable retraction value for chip breakage (VARI=0) ( Values: > 0: if retraction value; = 0: retraction value 1 mm set )
_DTD = Dwell time at final drilling depth ( Values: > 0: in seconds; < 0: in revolutions; = 0: value same as DTB )
_DIS1 = Programmable limit distance for reimmersion in the drill hole (for chip removal VARI=1); ( Values: > 0: programmable value applies; = 0: automatic calculation )
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. ;


This program executes the cycle CYCLE83 at the positions X80 Y120 and X80 Y60 in the
XY plane. The first drill hole is drilled with a dwell time zero and machining type chip
The final drilling depth and the first drilling depth are entered as absolute values. In the
second cycle call, a dwell time of 1 s is programmed. Machining type chip removal is

selected, the final drilling depth is relative to the reference plane. The drilling axis in both
cases is the Z axis.
The drilling stroke is calculated on the basis of a degression factor and must not become
shorter than the minimum drilling depth of 8 mm.

Siemens CNC Cycle83 Program Example

DEF REAL RTP=155, RFP=150, SDIS=1, ;Definition of parameters
DP=5, DPR=145, FDEP=100, FDPR=50,
DAM=20, DTB=1, FRF=1, VARI=0, _VRT=0.8,
_MDEP=8, _DIS1=0.4
N10 G0 G17 G90 F50 S500 M4 ;Specification of technology values
N20 D1 T42 Z155 ;Approach retraction plane
N30 X80 Y120 ;Approach first drilling position
N40 CYCLE83 (RTP, RFP, SDIS, DP, ,->
-> FDEP, , DAM, , , FRF, VARI, , , _VRT) ; ;Call of cycle depth parameters with ;absolute values
N50 X80 Y60 ;Approach next drilling position
N55 DAM=-0.6 FRF=0.5 VARI=1 ;Value assignment
N60 CYCLE83 (RTP, RFP, SDIS, , DPR, , ->
-> , , _DIS1) ;Call of cycle with relative ;specifications of final drilling depth ;and 1st drilling depth, the safety ;clearance is 1 mm and the feedrate ;factor is 0.5
N70 M30 ;Program end

Note :
-> means: it must be programmed in a block.

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.