0 votes
326 views
in cnc programming by (9.4k points)

In this article, we describe how to use G92 cycle for threading (straight and taper threading) in CNC lathe machines with all details and examples.

G92 Cycle Introduction

In CNC turning machines, the G92 cycle is generally used for threading. It can be used for straight threading or taper thread cutting operations, as well as one of the most frequently used CNC Turning cycles. As with other thread and screw cycles, the feedrate cannot be controlled to get the thread out correctly during thread cutting. Therefore, adjusting with the percentage of feedrate during threading does not affect the system, it does not allow you to go controlled or slow/fast.

Some programmers may be used to registering a current tool position with G92 command for milling applications. On CNC lathes, a command for the same purpose is G50, not G92. G92 used for threading has nothing to do with now virtually obsolete position register setting command. This applies for older control systems only – modern controls use advanced geometry offsets.

G92 Cycle Format

G92 X.. Z.. R.. F..

Parameters

X = Current threading pass diameter
Z = Thread end position
R = Taper angle ( If starting point in the X+ direction = R should be negative, If starting point in the X- direction = R should be positive ) ( Optional – Not use for straight threading )
F = Threading feedrate in in/rev ( Depends to control system should be also mm/min )

G92 Cycle Examples

G92 CNC Program Example – 1 – Straight Threading

CNC Lathe G92 Straight Threading Program Example – 1

G30 U0 W0;
G50 S1000 T0100;
G97 S1000 M03;
G00 X60.0 Z5.0 T0101 M08;
G92 X49.5 Z–30.0 F1.5;
X49.2;
X48.9;
X48.7;


G30 U0 W0;
M30;

G92 CNC Program Example – 2 – Straight Threading

CNC Lathe G92 Straight Threading Program Example – 2

Before start to process;
Part diameter = 32mm
Part Length = 65mm
O0019;
N315 G54;
N320 T0101; ( Turning Tool )
N325 G99 F0.25;
N330 G50 S1800;
N335 G96 S100 M03;
N35 G00 X35 Z0;
N40 G01 X–1.6;
N45 G00 X35 Z3;
N50 G42 G00 X34 Z2;
N55 G90 X30. Z–53. F0.2;
N60 G00 X35 Z2;
N65 G00 X22;
N70 G01 Z1;
N75 G01 X30 Z–3;
N80 G01 Z–53;
N85 G00 X35 Z3;
N90 G40;
N95 G28 U0 W0;
N100 T0404; ( Grooving Tool )
N105 G00 X32 Z–43;
N110 G75 R1.;
N115 G75 X24. Z–47. P1000 Q2000 F0.2;
N120 G00 X200 Z200;
N125 T0606; ( Threading Tool )
N130 G00 X32 Z3;
N135 G92 X29.5 Z–42. F2;
N140 X29.1;
N145 X28.8;
N150 X28.5;
N155 X28.2;
N160 X27.9;
N165 X27.7;
N170 X27.7;
N175 G28 U0 W0;
N180 M05 M09;
N185 M30;

G92 CNC Program Example – 3 – Taper Threading

NC Lathe G92 Taper Threading Program Example

G30 U0 W0 :
G50 S1000 T0100 :
G97 S1000 M03 :
G00 X70.0 Z5.0 T0101 M08 :
G92 X49.4 Z–32.0 R–6.166 F1.5 :
X49.0 :
X48.7 :
X48.5 :


G30 U0 W0 :
M30;


Need to more?

In this article, we described How to use G92 cycle for threading (straight and taper threading) in CNC lathe machines with all details and examples. For more details;

For your comments, suggestions and questions, you can write to us from the “Comments Section” below without registration and please consider to share this post!

Your answer

Your name to display (optional):
Privacy: Your email address will only be used for sending these notifications.
Anti-spam verification:
To avoid this verification in future, please log in or register.
...