G75 CNC Grooving Cycle Explained

On CNC lathes, workpieces sometimes need a retaining ring groove, seal groove, or various other grooves cut into them. These are done by having the cutting tool enter the workpiece to a set depth and remove material.

If you try to cut a wide groove in a single pass;

The tool can be put under excessive strain.
Chips can jam.
The tool can break.
Surface quality can suffer.

To prevent these problems, CNC lathes use the G75 Grooving Cycle.

Thanks to this cycle, the cutting tool;

Plunges a set amount,
Retracts to break the chip,
Advances again,
And automatically repeats this process until the groove reaches the desired dimensions.

Why Is G75 Used?

The G75 cycle;

Breaks the chip.
Prevents the tool from being overloaded.
Improves groove surface quality.
Extends tool life.
Makes program writing easier.

How Does the G75 Code Work?

Let’s say we’re cutting a groove.

The tool;

Plunges in.
↓
Retracts a certain amount.
↓
Advances again.
↓
Breaks the chip.
↓
Continues until the groove is complete.

If the groove width is larger than the tool width;
The tool moves sideways along the groove to machine the entire groove.

An Everyday Analogy

Imagine trying to cut down a thick tree in a single blow. That’s quite difficult and dangerous. But if we swing the axe a few times and pull it back in between;

We tire out less. The wood doesn’t jam the blade. The work becomes safer.
The G75 cycle works on the exact same logic when cutting a groove. The tool retracts at set intervals to break the chip, resulting in safe, efficient machining.

Advantages of the G75 Code

Advantage	Explanation
Chip breaks	Jamming is prevented
Longer tool life	Less excessive load
Better groove quality	Smoother surface
Safer machining	Less tool breakage
Easy to program	It’s a ready-made cycle

Points to Watch When Using G75

The correct grooving tool must be selected. Tool width should match the groove being made.
Cutting speed must be appropriate. Too high a speed can break the tool.
Coolant should be used. This is especially important for deep grooves.
Chip evacuation must be ensured. One of G75’s most important advantages is that it breaks the chip.

Grooving Use Case

The G75 cycle is used for quickly machining narrow grooves on the outer diameter, such as O-ring grooves or retaining ring grooves.

Chip Breaking

The cycle retracts at set intervals, making it easy to break and evacuate long chips.

Groove Width

If the groove width is larger than the cutting tool’s width, the cycle completes the groove using multiple passes.

G75 Command Structure

Basic syntax on Fanuc CNC lathes is as follows:

G75 R...

G75 X... Z... P... Q... R... F...

What the Parameters Mean

Code	Function
G75	Grooving cycle
R	Retraction amount
X	Final diameter of the groove
Z	Final position of the groove
P	Amount of each plunge
Q	Sideways feed amount along the groove
F	Cutting feed rate

Worked Example

On the part shown;

Stock diameter: Ø40 mm
Groove diameter: Ø28 mm
Groove length: 40 mm
Tool width: 3 mm

is to be machined.

Sample program:

O7500
N010 G28 U0 W0
N020 G50 S2000
N030 G54
N040 T0606
N050 G96 S140 M04 M08
N060 G00 X44 Z-33
N070 G75 R1
N080 G75 X28 Z-40 P2000 Q2500 R0 F0.4
N090 G28 U0 W0 M05 M09
N100 M30

Cycle Explanation
G75 R…
G75 X… Z… P… Q… R… F…
R: Retraction after each pass
X: The final X coordinate of the groove
Z: The final Z coordinate of the groove
P: Plunge amount per pass, in microns
Q: Sideways shift outside the groove in the -Z direction, in microns R: Sideways shift inside the groove in the +Z direction (0)
F: Cutting feed rate
Stock Properties
Shaft
Diameter: 40.000
Length: 80.000

Program Explanation

N10 G28 U0 W0         Moves to the machine reference point.
N20 G50 S2000         Sets the maximum spindle speed limit to 2000 RPM.
N30 G54               Selects the workpiece zero point.
N40 T0606             Selects grooving tool number 6.

N50 G96 S140 M04 M08

G96: Constant surface speed
S140: Cutting speed
M04: Spindle rotation counterclockwise
M08: Coolant on

N60 G00 X44 Z-33  / The tool moves to its starting point.
N70 G75 R1        / The tool retracts 1 mm at the end of each plunge.

N80 G75 X28 Z-40 P2000 Q2500 R0 F0.4

X28: The groove’s final diameter.
Z-40: The groove’s final position.
P2000: 2 mm plunge per pass.
Q2500: 2.5 mm feed along the groove.
R0: No extra stock left.
F0.4: Cutting feed rate.

N090 G28 U0 W0 M05 M09    / The tool returns to reference. Coolant and spindle shut off.
N100 M30                  / Program ends

Summary

The G75 Grooving Cycle is a ready-made cycle on CNC lathes that automatically performs groove-cutting operations. The tool advances and retracts a set amount to break the chip and machine the groove safely. The G75 cycle is controlled with the X, Z, P, Q, R, and F parameters and is an important CNC command that, especially on wide or deep grooves, extends tool life, improves surface quality, and simplifies programming.

Questions About This Topic

1. What is the basic purpose of the G75 cycle?
Answer: To break the chip by machining the groove in steps and to keep the tool operating safely.

2. What does the P parameter mean in the G75 command?
Answer: It represents the radial amount the tool advances on each plunge.

3. What is the function of the Q parameter?
Answer: It specifies the axial feed amount along the groove.

4. What is the most important difference between G75 and G01?
Answer: G75 operates in steps, automatically breaking the chip, while G01 feeds continuously.

5. Why is the G75 cycle preferred?
Answer: It’s preferred to prevent chip jamming, extend tool life, improve surface quality, and perform safe groove-cutting operations.

Frequently Asked Questions

If the tool plunges into a deep, wide groove in a single pass, the chip jams and the load on the tool suddenly spikes. G75 repeats plunging and retracting to break the chip into small pieces, putting far less strain on the tool.

Yes, that’s the main purpose. If the tool kept advancing in the same direction continuously, chips would build up and jam inside the groove; the short retractions let that chip break off and clear the groove.