Siemens CNC Turning | CYCLE98 | Thread Chaining

In this article, we describe how to use CYCLE98 for thread chaining in Siemens CNC controlled turning (lathe) machines with all details and examples.

0
189

CYCLE98 Introduction

With CYCLE98, you can produce several concatenated cylindrical or tapered threads with a constant pitch in longitudinal or face machining, all of which can have different thread pitches.

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.

Neither feedrate nor spindle override have any effect in thread travel blocks. The spindle override must not be changed during thread machining.

You may be interested also:
“Siemens CNC Turning | CYCLE97 | Thread Cutting”

CYCLE98 Format

CYCLE98 (PO1, DM1, PO2, DM2, PO3, DM3, PO4, DM4, APP, ROP, TDEP, FAL, IANG, NSP, NRC, NID, PP1, PP2, PP3, VARI, NUMT, _VRT)

Parameters

PO1 = Thread starting point in the longitudinal axis
DM1 = Thread diameter at the starting point
PO2 = First intermediate point in the longitudinal axis
DM2 = Diameter at the first intermediate point
PO3 = Second intermediate point
DM3 = Diameter at the second intermediate point
PO4 = Thread end point in the longitudinal axis
DM4 = 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)
PP1 = Thread pitch 1 as a value (enter without sign)
PP2 = Thread pitch 2 as a value (enter without sign)
PP3 = Thread pitch 3 as a value (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)

CYCLE98 Examples

CYCLE98 CNC Program Example – 1

With this program, you can produce a chain of threads, starting with a cylindrical thread. The infeed is performed vertically to the thread; neither finishing allowance, nor starting point offset are programmed. Five roughing cuts and one non cut are performed. The machining type is defined as longitudinal, external, with constant cross-section of cut.

Siemens CNC Turning CYCLE98 Program Example

N10 G18 G95 T5 D1 S1000 M4 ; Specification of technology values
N20 G0 X40 Z10 ; Approach starting position
N30 CYCLE98 (0, 30, -30, 30, -60, 36, -80, 50, 10, 10, 0.92, , , , 5, 1, 1.5, 2, 2, 3, 1) ; Cycle call
N40 G0 X55 ; Traverse axis by axis
N50 Z10 ;
N60 X40 ;
N70 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 | CYCLE97 | Thread Cutting
Next articleCNC Lathe | G32 Code | Constant Lead Threading