CNC Lathe | G76 Cycle | Multiple Repetitive Pass Threading (Quick Guide)

In this article, we describe how to use G76 for multiple repetitive threading cycle in CNC lathe machines with all details and examples.

0
528

G76 Cycle Introduction

In CNC lathes ( Turning machine ), G76 cycle is used for threading. In this cycle the thread cutting tool continues automatically by repeating the cycle until it reaches the depth of P (thread height) by removing the sawdust in the cycle.

This is quick guide for G76 Cycle. You will be able to write CNC Program after read this post but if you want more information or all details, please have a look:
“CNC Lathe | G76 Cycle | Multiple Repetitive Threading”

G76 Cycle Format

G76 Paabbcc Q R ;
G76 X Z R P Q F ;

Parameters

First block:
Paa: Number of finish passes (1-99)
Pbb: Chamfering amount (01-99)
Pcc: Angle of tool tip / angle of thread. (0°, 60°, 55°, 30°, 29°)
Q: Minimum depth of cut, subsequent passes depth (Δd√n – Δd√n-1). Number of cutting passes can be controlled by varying this value.
R: Finish allowance

 

Second Block:
X: Minor diameter of the thread in case of external thread – Major diameter in case of internal.
Z: Length of thread – endpoint.
R: Difference of thread radius (for taper threads only)
P: Height of thread / depth of thread
Q: Depth of cut in 1st pass / 1st cut.
F: Lead or pitch of thread

G76 Cycle Examples

G76 CNC Program Example – 1

M20 x 2.5
Pitch = 2.5

External Threading – M20

O000076 ;
T0000 ;
G00 X0. Z-100. ;
T0808 M07 ;
G97 S1000 M04 ;
G00 X22. Z5. ;
G76 P020060 Q200 R100 ;
G76 X16.8 Z-40. P1600 Q500 F2.5 ;
S0 T0000 ;
G00 X0. Z-100. M09 ;
M05 ;
M30 ;

Internal Threading – M20

O0079 ;
T0000 G00 X0 Z-100. ;
T0707 M07 ;
G97 S1000 M04 ;
G00 X15. Z5. ;
G76 P020060 Q200 R100 ;
G76 X20. Z-40. P1600 Q500 F2.5 ;
S0 T0000 X0. Z-100. M09 ;
M05 ;
M30 ;

G76 CNC Program Example – 2

Multiple Start Threading

Four start thread cutting on φ30mm (RH) lead 8mm
Pitch = Lead / No. start
Pitch = 8 / 4 = 2mm

O0763 ;
T0000 ;
G0 X0. Z-100. ;
T0505 M07 ;
G97 S1000 M04 ;
( For 1. Start )
G0 X32. Z10. ;
G76 P020060 Q150 R50 ;
G76 X27.44 Z-60. P11280 Q400 F8.0 ;
( For 2. Start )
G0 X32.Z8. ;
G76 P020060 Q150 R50 ;
G76 X27.44 Z-60. P1280 Q400 F8.0 ;
( For 3. Start )
G0 X32.Z6. ;
G76 P02.0060 Q150 R50 ;
G76 X27.44 Z-60. P1280 Q400 F8.0 ;
( For 3. Start )
G0 X32. Z4. ;
G76 P020060 Q150 R50 ;
G76 X27.44 Z-60. P1280 Q400 F8.0 ;
S0 T0000 M09 ;
G0 X0.2-100. M05 ;
M30 ;


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 articleG71 Cycle Examples for CNC Lathe
Next articleCNC Lathe | G33 and G34 Thread Cutting (Quick Guide)