Siemens CNC Turning | CYCLE95 | Stock Removal Cycle

CYCLE95 Introduction

With the CYCLE95, you can machine any user-programmed contour from a blank with paraxial stock removal. The contour may contain relief cut elements. It is possible to machine contours using longitudinal and face machining, both externally and internally. The technology can be freely selected (roughing, finishing, complete machining). When roughing the contour, paraxial cuts from the maximum programmed infeed depth are programmed and burrs are also removed parallel to the contour after an intersection point with the contour has been reached. Roughing is performed up to the final machining allowance programmed.

Finishing is performed in the same direction as roughing. The tool radius compensation is selected and deselected by the cycle automatically.

CYCLE95 Format



NPP = Name of contour subroutine
MID = Infeed depth (enter without sign)
FALZ = Finishing allowance in the longitudinal axis (enter without sign)
FALX = Finishing allowance in the transverse axis (enter without sign)
FAL = Finishing allowance according to the contour (enter without sign)
FF1 = Feedrate for roughing without undercut
FF2 = Feedrate for insertion into relief cut elements
FF3 = Feedrate for finishing
VARI = Machining type
Range of values: 1…12, 201…212
0: With rounding at the contour
No residual corners remain, the contour is rounded with overlapping. This means that rounding is performed across multiple intersections.
2: Without rounding at the contour
Contours are always rounded to the previous roughing intersection followed by retraction. Residual corners can remain, depending on the ratio of the tool radius to infeed depth (MID).
DT = Dwell time fore chip breaking when roughing
DAM = Path length after which each roughing step is interrupted for chip breaking
_VRT = Lift-off distance from contour when roughing, incremental (to be entered without sign)

CYCLE95 Examples

CYCLE95 CNC Program Example – 1 – Stock Removal

The contour shown in the illustration to explain the defining parameters is to be machined longitudinally externally by complete machining. Axis-specific finishing allowances are specified. Cutting will not be interrupted when roughing. The maximum infeed is 5 mm. The contour is stored in a separate program.

Siemens CNC Turning CYCLE95 Program Example 1

DEF STRING[8] UPNAME ; Definition of a variable for the contour name
N10 T1 D1 G0 G18 G95 S500 M3 Z125 X81 ; Approach position before cycle call
UPNAME=”CONTOUR_1″ ; Assignment of subroutine name
N20 CYCLE95 (UPNAME, 5, 1.2, 0.6, , 0.2, 0.1, 0.2, 9, , , 0.5) ; Cycle call
N30 G0 G90 X81 ; Reapproach starting position
N40 Z125 ; Traverse axis by axis
N50 M30 ; Program end
%_N_ KONTUR_1_SPF ; Beginning of contour subroutine
N100 G1 Z120 X37 ; Traverse axis by axis
N110 Z117 X40
N120 Z112 ; Rounding with radius 5
N130 G1 Z95 X65 RND=5 ; Traverse axis by axis
N140 Z87
N150 Z77 X29
N160 Z62
N170 Z58 X44
N180 Z52
N190 Z41 X37
N200 Z35
N210 G1 X76
N220 M17 ; End of subroutine

CYCLE95 CNC Program Example – 2 – Stock Removal

The stock removal contour is defined in the calling program. The program is completed after the stock removal cycle.

Siemens CNC Turning CYCLE95 Program Example 2

N110 G18 DIAMOF G90 G96 F0.8
N120 S500 M3
N130 T11 D1
N140 G0 X70
N150 Z60
N160 CYCLE95 (“ANFANG:ENDE”,2.5,0.8, 0.8,0,0.8,0.75,0.6,1) ; Cycle call
N170 M02
N180 G1 X10 Z100 F0.6
N190 Z90
N200 Z=AC(70) ANG=150
N210 Z=AC(50) ANG=135
N220 Z=AC(50) X=AC(50)
N230 M02