G74 CNC Drilling (Peck) Cycle Explained

When manufacturing on CNC (Computer Numerical Control) machines, certain operations repeat continuously. For example, when drilling a deep hole in a part, the drill needs to keep advancing and retracting. If we had to program these movements one by one, the programs would become extremely long and complex.

Ready-made commands called cycles are used to solve this problem. One of these commands is the G74 Drilling Cycle. On Fanuc-controlled CNC lathes, G74 is used specifically for peck drilling operations.

What Is G74? Why Is It Used?

G74 is an automatic drilling cycle that makes the drill advance a set amount, then retract a short distance to break the chip.

The basic logic behind it:

Advance → Retract → Advance → Retract → Advance…
This motion continues until the target depth is reached.

how the G74 CNC code works and what it does

Why Is G74 Used?

If the drill goes into a deep hole in a single pass;

Chips can jam.
The drill can break.
The cutting tool can overheat.
Hole quality can suffer.

Thanks to the G74 Code;

How Does G74 Work?

For example, let’s say we’re drilling a hole 60 mm deep.

The drill:

Advances 10 mm.
↓
Retracts a certain amount.
↓
Advances 10 mm again.
↓
Retracts again.
↓
Continues until it reaches a depth of 60 mm.

G74 Syntax Format

Basic usage on Fanuc CNC lathes is as follows:

G74 R...
G74 Z... Q... F...

What the Parameters Mean

Code	Meaning
G74	Drilling cycle
R	Retraction amount
Z	Final depth of the hole
Q	Amount of each advance step
F	Feed rate

The Pecking Motion

The G74 cycle applies a short forward-and-back “peck drilling” motion to break the chip on deep holes.

Chip Evacuation

After each peck step, the drill partially retracts, letting the chip be ejected from the hole.

Depth-to-Diameter Ratio

When hole depth exceeds 3-4 times the drill diameter, using a peck cycle significantly reduces the risk of breakage.

Sample G74 Program

Let’s drill a hole 50 mm deep in a part.

N10 T0505
N20 G97 S600 M03
N30 G00 X0 Z2
N40 G74 R1
N50 G74 Z-50 Q10000 F0.15
N60 G00 X100 Z100
N70 M30

Program Explanation

N10 T0505
Selects drill tool number 5.

N20 G97 S600 M03

G97: Constant spindle speed
S600: 600 RPM
M03: Spindle rotation clockwise

N30 G00 X0 Z2

The drill approaches the part.

N40 G74 R1

At the end of each peck step, the drill retracts by 1 mm.

N50 G74 Z-50 Q10000 F0.15

Z-50: 50 mm depth
Q10000: 10 mm advance per step
F0.15: Feed rate

N60

The tool retracts to a safe zone.

N70

The program ends.

Points to Watch When Using G74

The right drill must be selected. Use a tool suited to the hole diameter.
Spindle speed and feed rate must be appropriate. Too high a speed can break the tool.
Coolant should be used. It extends tool life on deep holes.
Chip evacuation is important. G74’s most important purpose is preventing chip buildup.

Differences Between G74 and G01

G01	G74
Continuous feed	Stepped feed
Chip doesn’t break	Chip breaks automatically
Risky for deep holes	Suited to deep holes
The programmer writes out every movement	The machine performs the cycle automatically

Let’s use an everyday analogy;
Imagine you’re digging a long tunnel.
The G01 method: You try to dig without ever stopping.
The G74 method: You dig a bit, clear out the loose dirt, then dig again.

Working by clearing the dirt as you go makes the job safer and more efficient. G74 works on a CNC machine using the exact same logic.

Summary

The G74 Drilling Cycle is a ready-made drilling command used on CNC lathes. It’s especially useful for deep holes, letting the drill periodically retract to break the chip. This extends tool life, produces higher-quality machined parts, and simplifies program writing. The G74 cycle is controlled with the R (retraction), Z (hole depth), Q (peck amount), and F (feed rate) parameters, and it’s one of the efficient hole-machining methods used in modern CNC manufacturing.

Frequently Asked Questions

If the drill goes deep in a single pass, the chip can’t exit through the flute, it builds up, and wraps around the drill. This can cause both overheating and breakage of the drill.

This motion resembles the habit of periodically pulling the drill back to clear chips when drilling a hole by hand. CNC repeats this automatically and consistently to provide the same safety.