This cycle (CYCLE96) is for machining thread undercuts in accordance with DIN 76 on parts with a metric ISO thread.
|CYCLE96 (DIATH, SPL, FORM, _VARI)|
|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”|
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.