Siemens CNC Milling | CYCLE90 | Thread Milling

In this article, we describe how to use CYCLE90 for thread milling in Siemens CNC controlled milling (machine centre) machines with all details and examples.

0
433

CYCLE90 Introduction

By using the cycle CYCLE90, you can produce internal or external threads. The path when milling threads is based on a helix interpolation. All three geometry axes of the current plane, which you will define before calling the cycle, are involved in this motion. The programmed feedrate F acts according to the the axis grouping defined in the FGROUP instruction before the call.

You may be interested also:
“Siemens CNC | CYCLE801 | Dot Matrix”

Supported CNC Series

Siemens CNC 802D, 810D, 840D, 840D sl, 840Di, 840Di sl series controllers.

CYCLE90 Format

CYCLE90 (RTP, RFP, SDIS, DP, DPR, DIATH, KDIAM, PIT, FFR, CDIR, TYPTH, CPA, CPO)

Parameters

RTP = Retraction plane (absolute)
RFP = Reference plane (absolute)
SDIS = Safety clearance (enter without sign)
DP = Final drilling depth (absolute)
DPR = Final drilling depth relative to the reference plane (enter without sign)
DIATH = Nominal diameter, outer diameter of the thread
KDIAM = Core diameter, internal diameter of the thread
PIT = Pitch ; Range of values: 0.001 … 2000.000 mm
FFR = Feedrate for thread milling (enter without sign)
CDIR = Direction of rotation for thread milling (Values:2: (for thread milling at G2); 3: (for thread milling at G3)
TYPTH = Thread type ( Values: 0: Internal thread; 1: External thread, diameter programming via DIATH; 2: External thread, diameter programming via KDIAM)
CPA = Center point of circle, abscissa (absolute)
CPO = Center point of circle, ordinate (absolute)

CYCLE90 Examples

CYCLE90 CNC Program Example – 1

By using this program, you can mill an internal thread at point X60 Y50 of the G17 plane.

Siemens CNC Milling CYCLE90 Program Example

DEF REAL RTP=48, RFP=40, SDIS=5, DPR=40, DIATH=60, KDIAM=50 ; Definition of variables with value assignments
DEF REAL PIT=2, FFR=500, CPA=60,CPO=50
DEF INT CDIR=2, TYPTH=0
N10 G90 G0 G17 X0 Y0 Z80 S200 M3 ; Approach start position
N20 T5 D1 ; Specification of technology values
N30 CYCLE90 (RTP, RFP, SDIS, DPR, DIATH, KDIAM, PIT, FFR, CDIR, TYPTH, CPA, CPO) ; Cycle call
N40 G0 G90 Z100 ; Approach position after cycle
N50 M02 ; Program end


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 | CYCLE801 | Dot Matrix
Next articleSiemens CNC Milling | LONGHOLE | Long Holes located on a Circle