Siemens CNC Turning | CYCLE97 | Thread Cutting

In this article, we describe how to use CYCLE97 for thread cutting in Siemens CNC controlled turning (lathe) machines with all details and examples.

1
433

CYCLE97 Introduction

With this thread cutting cycle (CYCLE97), you can machine cylindrical and tapered outside and inside threads with constant pitch in longitudinal or face machining. The thread can be single or multiple. With multiple threads, the individual thread turns are machined one after the other.

Infeed is automatic. You can select either constant infeed per cut or constant cross-section of cut.

Right-hand or left hand thread is determined by the direction of rotation of the spindle which must be programmed prior to the cycle start.

Siemens CNC |CYCLE97 | Thread Cutting

Neither feedrate nor spindle override have any effect in thread travel blocks. The spindle override must not be changed during thread machining.
Note: To be able to use this cycle, a speed-controlled spindle with position measuring system is required.

You may be interested also:
“Siemens CNC Turning | CYCLE96 | Thread Undercut”

CYCLE97 Format

CYCLE97 (PIT, MPIT, SPL, FPL, DM1, DM2, APP, ROP, TDEP, FAL, IANG, NSP, NRC, NID, VARI, NUMT, _VRT)

Parameters

PIT = Thread pitch as a value (enter without sign)
MPIT = Thread pitch as thread size; Range of values: 3 (for M3) … 60 (for M60)
SPL = Thread starting point in the longitudinal axis
FPL = Thread end point in the longitudinal axis
DM1 = Thread diameter at the starting point
DM2 = Thread diameter at the end point
APP = Run-in path (enter without sign)
ROP = Run-out path (enter without sign)
TDEP = Thread depth (enter without sign)
FAL = Finishing allowance (enter without sign)
IANG = Infeed angle; Range of values:
“+” (for flank infeed at the flank)
“–” (for alternating flank infeed)
NSP = Starting point offset for the first thread turn (enter without sign)
NRC = Number of roughing cuts (enter without sign)
NID = Number of idle passes (enter without sign)
VARI = Definition of the machining type for the thread ; Range of values: 1 … 4
NUMT = Number of thread turns (enter without sign)
_VRT = Variable retraction distance based on initial diameter, incremental (enter without sign)

Examples

CYCLE97 CNC Program Example – 1 – Thread Cutting

With this program, you can cut an M42x2 metric outside thread with flank infeed. Infeed is carried out with constant cutting cross-section. 5 roughing cuts are carried out at a thread depth of 1.23 mm without finishing allowance. At completion of this operation, 2 idle passes will be carried out.

Siemens CNC Turning CYCLE97 Program Example

DEF REAL MPIT=42, SPL=0, FPL=-35, ; Definition of parameters with value assignments
DM1=42, DM2=42, APP=10, ROP=3,
TDEP=1.23, FAL=0, IANG=30, NSP=0
DEF INT NRC=5, NID=2, VARI=3, NUMT=1
N10 G0 G18 G90 Z100 X60 ; Selection of starting position
N20 G95 D1 T1 S1000 M4 ; Specification of technology values
N30 CYCLE97 ( , MPIT, SPL, FPL, DM1, DM2, APP, ROP, TDEP, FAL, IANG, NSP, NRC, NID, VARI, NUMT) ; Cycle call
N40 G90 G0 X100 Z100 ; Approach next position
N50 M30 ; End of program


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.


Previous articleSiemens CNC Turning | CYCLE96 | Thread Undercut
Next articleSiemens CNC Turning | CYCLE98 | Thread Chaining

1 COMMENT

Comments are closed.