Siemens CNC Turning | CYCLE94 | Undercut Cycle


CYCLE94 Introduction

With CYCLE94, you can machine undercuts of form E and F in accordance with DIN509 with the usual load on a finished part diameter of >3 mm.

Another cycle, CYCLE96, exists for producing thread undercuts (see Section “Thread Undercut – CYCLE96).

CYCLE94 Format

CYCLE94 (SPD, SPL, FORM, _VARI)

Parameters

SPD = Starting point in the facing axis (enter without sign)
SPL = Starting point of the contour in the longitudinal axis (enter without sign)
FORM = Definition of the form; Values: E (for form E), F (for form F)
_VARI = Specification of undercut position; Values: 0 (corresponding to the tool point direction of the tool), 1 to 4 (define position)

Examples

CYCLE94 CNC Program Example – 1 – Undercut

You can machine an undercut of form E with this program.

Siemens CNC Turning CYCLE94 Program Example

N10 T25 D3 S300 M3 G18 G95 F0.3 ; Specification of technology values
N20 G0 G90 Z100 X50 ; Selection of starting position
N30 CYCLE94(20, 60, “E”) ; Cycle call
N40 G90 G0 Z100 X50 ; Approach next position
N50 M02 ; End of program