Article Contents
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 |
| You may be interested also: |
| “Siemens CNC Turning | CYCLE95 | Stock Removal Cycle” |
Examples
CYCLE96 CNC Program Example – 1 – Thread Undercut
This program can be used to program a thread undercut of form A.
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.
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.
Need to More?
Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.
