CNC Milling | G33 Code | Thread Cutting

In this article, we describe how to use G33 code for simple and multiple threading in CNC milling machines with all details and examples.

0
374

G33 Code Introduction

Straight threads with a constant lead can be cut with G33 code. The position coder mounted on the spindle reads the spindle speed in real-time. The read spindle speed is converted to the feedrate per minute to feed the tool.

G33 Code Format

G33 IP_ F_

Parameters

IP_ = End point for related axis ( Ex : Z-15. )
F = Long axis direction lead

Things to Know

In general, threading is repeated along the same tool path in rough cutting through finish cutting for a screw. Since threading starts when the position coder mounted on the spindle outputs a 1-turn signal, threading is started at a fixed point and the tool path on the workpiece is unchanged for repeated threading.,

Note that the spindle speed must remain constant from rough cutting through finish cutting. If not, incorrect thread lead will occur. In general, the lag of the servo system, etc. will produce somewhat incorrect leads at the starting and ending points of a thread cut. To compensate for this, a threading length somewhat longer than required should be specified.

G33 Code Example

Pitch = 2mm.

G33 Z15. F2.0

G33 Multiple Threading

Using the Q address to specify an angle between the one-spindle-rotation signal and the start of threading shifts the threading start angle, making it possible to produce multiple-thread screws with ease.

Multiple thread screws

G33 Code Format for Multiple Threading

G33 IP _ F_ Q_ ;

Parameters

IP : End point
F_ : Lead in longitudinal direction
Q_ : Threading start angle

G33 Double Threaded Screws Example

Program for producing double-threaded screws (with start angles of 0 and 180 degrees)

G00 X40.0 ;
G33 W-38.0 F4.0 Q0 ;
G00 X72.0 ;
W38.0 ;
X40.0 ;
G33 W-38.0 F4.0 Q180000 ;
G00 X72.0 ;
W38.0 ;


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 articleCNC | G28 Code | Automatic Reference Point Return
Next articleCNC Milling | G12.4 and G13.4 Codes | Groove Cutting