G84 Tapping Cycle on a CNC Lathe Explained

Threaded connections are often used to join machine parts. To install a bolt, a thread of the appropriate size must be cut inside the part. This process is called internal thread cutting or tapping.

On CNC lathes, this process can be done manually, or it can be performed with one of the built-in cycles, the G84 Tapping Cycle.

Thanks to the G84 cycle, the machine automatically advances the tap into the hole, reverses it back at the desired depth, and safely returns it to the starting point.

How Is Tapping Done on a CNC Lathe?

First, a hole is drilled at the appropriate diameter. For example, if an M10x1.5 thread is going to be cut,
The pilot hole diameter should be approximately: Ø8.5 mm.

Then;
↓
The tap approaches the hole.
↓
It advances in sync with the spindle.
↓
It stops at the desired depth.
↓
It reverses direction.
↓
The tap returns to the starting point.

Points to Watch During Tapping

The pilot hole must be drilled correctly. A hole that’s too small can cause the tap to break.
The correct thread pitch must be selected. The F value must match the thread pitch.
Coolant should be used. It extends tool life.
The tap should be of good quality. Worn taps produce poor threads.

What Is the G84 Code For? Why Is It Used?

G84 is a tapping cycle used on CNC lathes.

Thanks to this cycle;

The tap enters the hole,
It forms the thread,
It reaches the specified depth,
It reverses direction,
It withdraws the tap.

These operations are performed automatically.

The G84 cycle;

Simplifies program writing.
Automatically synchronizes the thread pitch.
Reduces the risk of error.
Saves time in mass production.
Improves internal thread quality.

The Difference Between G84 and G76

G84	G76
Uses a tap	Uses a threading tool
Completed in a single pass	Requires multiple passes
Suited to small threads	Suited to large threads
Forms a ready-made thread	Forms a thread by removing chips

Tapping Speed

In the G84 cycle, spindle rotation and axis feed operate in sync; the feed rate equals the thread pitch.

Reverse Rotation

When the tap reaches the bottom of the hole, the spindle automatically reverses direction and the tap exits along the same path.

Rigid Tapping

Modern CNC machines improve synchronization precision with “rigid tapping,” reducing the risk of tap breakage.

G84 Command Structure

General usage:

G84 Z... R... F...

Meaning of the Parameters

Code	Function
G84	Tapping cycle
Z	Final thread depth
R	Starting plane
F	Thread pitch

Why Is the F Parameter So Important?

In tapping, the feed rate must always be equal to the thread pitch. For example:

Thread	F Value
M6x1	F1
M8x1.25	F1.25
M10x1.5	F1.5
M12x1.75	F1.75
M16x2	F2

If the wrong feed is selected; ❌ The tap can break. ❌ The thread can be ruined.

G84 Example Program

An M10x1.5 internal thread will be cut. The pilot hole has been drilled. Thread length: 20 mm
Program:

O8400
N010 G28 U0 W0
N020 G54
N030 T0505
N040 G97 S250 M03 M08
N050 G00 X0 Z2
N060 G84 Z-20 R2 F1.5
N070 G28 U0 W0 M05 M09
N080 M30

Explanation of the Program

N10 G28 U0 W0  Explanation:Goes to the reference point.
N20 G54        Explanation:The workpiece zero is selected.
N30 T0505      Explanation:The tap tool is selected.

N40 G97 S250 M03 M08

Explanation:
G97: Constant surface speed off (constant RPM).
S250: 250 rpm.
M03: Clockwise rotation.
M08: Coolant on.

N50 G00 X0 Z2   Explanation: The tool moves to the starting point.

N60 G84 Z-20 R2 F1.5

Explanation:
Z-20: Taps down to a depth of 20 mm.
R2: Starting plane.
F1.5: Thread pitch.

The machine automatically;

Moves forward,
Cuts the thread,
Reverses direction,
Withdraws.

N070 G28 U0 W0 M05 M09

Explanation:
The tool returns to the reference point.
The spindle and coolant turn off.

N080 M30     Explanation: The program ends.

Questions About the G84 Code

Question: What is the main purpose of the G84 cycle?
Answer: To automatically perform internal thread cutting using a tap.

Question: What does the F parameter represent in the G84 command?
Answer: It represents the pitch of the thread to be cut.

Question: Why is a pilot hole drilled before tapping?
Answer: To allow the tap to work smoothly and prevent it from breaking.

Question: What’s the most important difference between G84 and G76?
Answer: G84 uses a tap tool, while G76 cuts a thread by removing chips with a threading tool.

Question: Why is the G84 cycle preferred?
Answer: It’s preferred because it simplifies programming, improves thread quality, and saves time in mass production.

Topic Summary

The G84 Tapping Cycle is a built-in cycle used on CNC lathes to cut internal threads. In this cycle, the tap moves into the hole in sync with the spindle, reverses back at the desired depth, and the operation is safely completed. The G84 cycle is controlled with the Z (thread length), R (starting plane), and F (thread pitch) parameters. It’s especially preferred for fast, reliable, and high-quality internal thread cutting in mass production.