Siemens CNC Turning | CYCLE96 | Thread Undercut


CYCLE96 Introduction

This cycle (CYCLE96) is for machining thread undercuts in accordance with DIN 76 on parts with a metric ISO thread.

CYCLE96 Format

CYCLE96 (DIATH, SPL, FORM, _VARI)

Parameters

DIATH = Nominal diameter of the thread
SPL = Starting point on the contour of the longitudinal axis
FORM = Definition of the form ; Values:
A (for form A)
B (for form B)
C (for form C)
D (for form D)
_VARI = Specification of undercut position ; Values:
0: Corresponding to tool point direction
1 to 4: Define position

Examples

CYCLE96 CNC Program Example – 1 – Thread Undercut

This program can be used to program a thread undercut of form A.

Siemens CNC Turning CYCLE96 Program Example

N10 D3 T1 S300 M3 G95 F0.3 ; Specification of technology values
N20 G0 G18 G90 Z100 X50 ; Selection of starting position
N30 CYCLE96 (10, 60, “A”) ; Cycle call
N40 G90 G0 X30 Z100 ; Approach next position
N50 M30 ; End of program

FORM Parameter Explanation

Thread undercuts of the forms A and B are defined for external threads, form A for standard run-outs of threads, and form B for short run-outs of threads. Thread undercuts of the forms C and D are used for internal threads, form C for a standard run-out of the thread, and form D for a short run-out.

Siemens CNC Turning CYCLE96 FORM Parameter Explanation

If the parameter has a value other than A … D, the cycle aborts and creates alarm 61609 “Form defined incorrectly”.

Internally in the cycle, the tool radius compensation is selected automatically.