G Codes and M Codes: CNC Machine Language Explained, Including G90 G28 vs. G91 G28

G Codes and M Codes are the language that CNC machines understand.

In the previous article, we explained the five core systems of a CNC machine and how they work together. In this article, we are entering the world of CNC programming by learning the two main types of instructions used to control a machine tool.

This article uses the FANUC CNC code format as the main example.

When I First Started Working in a Factory, the Program Made No Sense to Me

I still remember when I first started working in a factory.

My instructor handed me a piece of paper covered with lines like these:

O0001
G94 G40 G49 G80
T01 M06
G90 G00 G54 X0. Y0.
S3000 M03
G43 H01 Z100.
G01 Z-5. F200
...
G00 Z50.
M09
G49
G91 G28 Z0.
M30

He said:

First, learn how to read this.

I stared at the program for a long time. I recognized a few letters, but almost everything else looked confusing.

Later, I discovered that these codes follow clear rules and are not as complicated as they first appear.

A CNC program mainly contains two types of instructions:

1. Instructions that tell the cutting tool how to move
2. Instructions that tell the machine which auxiliary function to activate

The first type is called G code.

The second type is called M code.

What Are G Codes and M Codes?

G Codes Tell the Cutting Tool How to Move

G codes are also known as preparatory function codes.

Their main function is to define how the cutting tool moves, including:

• Rapid positioning
• Linear cutting
• Circular interpolation
• Absolute coordinate movement
• Incremental coordinate movement
• Work coordinate system selection
• Machine reference return

A G code begins with the letter G, followed by two digits.

For example:

G00
G01
G54
G90

Before learning the individual commands, it is important to understand the difference between modal and non-modal G codes.

Modal G Codes

A modal code remains active after it has been programmed.

It continues to affect the following program blocks until another G code from the same group replaces it.

For example, after programming:

G01

the CNC machine will continue using linear interpolation in the following blocks, even when G01 is not written again.

The mode remains active until another motion command, such as G00, G02, or G03, replaces it.

Non-Modal G Codes

A non-modal code is only effective in the program block where it appears.

It is executed once and does not remain active in later blocks.

For example:

G04

is a dwell command. It only affects the current program block.

Essential G Codes and M Codes for CNC Beginners

The following commands are among the most important codes for anyone beginning to learn CNC programming. The explanations below follow the structure and examples provided in the original article.

G00 — Rapid Positioning

G00 moves the cutting tool to a specified position at the machine’s rapid traverse speed.

It is normally used for positioning rather than cutting.

Example:

G00 X100. Y50. Z200.

This command rapidly moves the tool toward:

• X = 100 mm
• Y = 50 mm
• Z = 200 mm

Important Safety Warning

G00 does not necessarily move along one controlled straight-line path.

Multiple axes may move simultaneously at their maximum rapid speeds. Depending on the machine control and axis distances, the actual toolpath may be diagonal or dog-leg shaped.

For this reason, never use G00 carelessly when the cutting tool is close to the workpiece, fixture, clamps, or machine table.

When approaching the workpiece, use a controlled feed movement such as G01.

G01 — Linear Cutting

G01 moves the cutting tool along a straight line at a specified feed rate.

It is one of the most commonly used cutting commands in CNC machining.

Example:

G01 X50. Y50. F300.

This command moves the tool in a straight line toward:

• X = 50 mm
• Y = 50 mm

The feed rate is:

F300

The unit of the F value depends on the active feed mode.

Under G94

The feed rate is measured per minute:

mm/min

Under G95

The feed rate is measured per spindle revolution:

mm/rev

CNC milling machines commonly use G94.

G02 and G03 — Circular Interpolation

G02 and G03 are used to machine circular or arc-shaped toolpaths.

G02

Clockwise circular interpolation.

G03

Counterclockwise circular interpolation.

The direction is normally judged while looking from the positive direction of the selected axis toward the negative direction.

For an arc in the XY plane, this normally means looking from the positive Z-axis toward the workpiece.

Example using an R value:

G02 X50. Y0. R25. F200.

This command moves the tool clockwise to:

• X = 50 mm
• Y = 0 mm
• Radius = 25 mm
• Feed rate = 200 mm/min

Example using center offsets:

G03 X0. Y50. I0. J25. F200.

This command moves the tool counterclockwise using I and J to define the arc-center offset.

Easy Way to Remember

G02 = Clockwise
G03 = Counterclockwise

The direction should be viewed from the positive Z direction toward the negative Z direction when working in the XY plane.

G90 and G91 — Absolute and Incremental Coordinates

G90 and G91 are two commands that CNC beginners often confuse.

G90 — Absolute Coordinate Programming

Under G90, all programmed coordinates refer to the origin of the currently active coordinate system.

For example:

G90 G00 X50.

This means:

Move to the absolute coordinate position X = 50 mm.

It does not mean moving another 50 mm from the current position.

A simple comparison is entering a specific destination into a navigation system.

G91 — Incremental Coordinate Programming

Under G91, every coordinate value represents a movement distance relative to the current tool position.

For example:

G91 G00 X50.

This means:

Move another 50 mm in the positive X direction from the current position.

It does not mean moving to the absolute coordinate X = 50 mm.

A simple comparison is saying:

Move forward another 500 metres, and then turn right.

G90 and G91 Comparison

Command	Coordinate Type	Meaning of X50
G90	Absolute coordinates	Move to X = 50 mm
G91	Incremental coordinates	Move another 50 mm from the current position

G28 — Return to the Machine Reference Point

G28 commands the machine axis to return to its preset reference point.

The basic format is:

G28 X_ Y_ Z_

The X, Y, and Z values define an intermediate point.

Under G90, the intermediate point is interpreted as an absolute coordinate.

Under G91, the intermediate point is interpreted as an incremental movement.

This intermediate-point concept is the key to understanding why G91 G28 Z0. is commonly used instead of G90 G28 Z0..

What Is the Intermediate Point?

When the machine executes a G28 command, the axis does not simply move directly to the machine reference point in one step.

The movement normally contains two stages:

1. Move to the programmed intermediate point
2. Move from the intermediate point to the machine reference point

The programmed coordinate mode determines where that intermediate point is located.

How Does G90 G28 Z0. Move?

Assume the cutting tool is currently located at:

Z50.

Now consider the following command:

G90 G28 Z0.

Under G90, the value Z0. is an absolute coordinate in the currently active coordinate system.

Therefore, the movement happens in two stages:

1. The Z-axis first moves from its current position to the absolute position Z0.
2. It then moves from Z0. to the machine reference point

Before executing a G28 return command, tool-length compensation is often cancelled.

In this situation, moving first to the work coordinate position Z0. may cause the tool to move downward toward the workpiece.

If the workpiece zero is located on the top surface of the part, the cutting tool may move directly into the workpiece.

That is why using:

G90 G28 Z0.

without fully understanding the intermediate position can create a serious collision risk.

The original article emphasizes that the tool may first move toward the workpiece coordinate zero before returning to the machine reference position.

How Does G91 G28 Z0. Move?

Now consider:

G91 G28 Z0.

Under G91, Z0. represents an incremental movement of zero.

In other words, the current tool position is used as the intermediate point.

The movement happens as follows:

1. The Z-axis moves by an incremental distance of zero
2. The current position becomes the intermediate point
3. The Z-axis then returns to the preset machine reference point

Because the programmed intermediate movement is zero, the tool does not first move to the work-coordinate position Z0..

Instead, it begins returning from its current position toward the machine Z-axis reference point.

This is why CNC programs commonly use:

G91 G28 Z0.

The meaning is:

Use the current Z position as the intermediate point, and then return the Z-axis to the machine reference point.

This movement logic is the main reason the original article recommends G91 G28 Z0. rather than G90 G28 Z0. for this situation.

G90 G28 and G91 G28 Comparison

Command	Intermediate Point	Main Risk or Effect
G90 G28 Z0.	Absolute Z0 in the active coordinate system	The tool may first move toward the workpiece zero
G91 G28 Z0.	Zero incremental movement from the current position	The current position becomes the intermediate point before reference return

Common FANUC Programming Format

G91 G28 Z0.

Comment:

The Z-axis makes a zero incremental move and then returns to the machine Z reference point.

G54 to G59 — Work Coordinate System Selection

G54 is one of the most commonly used work-coordinate-system commands.

After setting the workpiece origin during edge finding, probing, or tool setting, the coordinate values are entered into the G54 work offset.

When the program contains:

G54

the machine interprets it as:

Use the workpiece origin stored in G54.

Additional work coordinate systems include:

G55
G56
G57
G58
G59

These represent the second through sixth standard work coordinate systems.

They are useful for:

• Machining multiple parts
• Using multiple fixtures
• Programming different workpiece positions
• Running several work offsets in one setup

M Codes Tell the Machine Which Function to Activate

M codes are also known as miscellaneous function codes or auxiliary function codes.

Unlike most G codes, M codes normally do not define the cutting tool’s position.

Instead, they control supporting machine functions such as:

• Starting and stopping the spindle
• Changing tools
• Turning coolant on and off
• Pausing the program
• Ending the program
• Calling a subprogram

The original article lists the following commonly used M codes.

Common CNC M Codes

M Code	Function	Example or Explanation
M03	Spindle forward rotation	Used with an S value, such as S3000 M03
M04	Spindle reverse rotation	Used for special tools or some tapping operations
M05	Spindle stop	The spindle should normally stop before a tool change
M06	Automatic tool change	Used with a T command, such as T02 M06
M08	Coolant on	Turns on coolant during cutting
M09	Coolant off	Turns off coolant before tool changing or program completion
M00	Program stop	Waits for the operator to press CYCLE START
M01	Optional stop	Stops only when the OPTIONAL STOP switch is enabled
M30	Program end and reset	Normally used at the end of a complete program
M98	Subprogram call	Calls a specified subprogram, sometimes with a repeat count

Why Every CNC Program Needs a Safety Initialization Block

There is one rule that CNC operators usually remember after witnessing even one serious machine collision:

Every CNC program should begin with a safety initialization block.

A common FANUC-format safety line is:

G90 G94 G40 G49 G80

This line clears potentially dangerous modal conditions left active by a previous program.

G90 — Select Absolute Coordinate Mode

G90

This prevents the new program from accidentally running under G91 incremental mode left active by the previous program.

Without G90, a coordinate intended as an absolute position might be interpreted as an additional movement distance.

G94 — Select Feed per Minute

G94

This selects feed per minute, normally expressed in:

mm/min

It prevents the program from accidentally using G95 feed per revolution left active by another operation.

G40 — Cancel Cutter Radius Compensation

G40

This cancels active cutter radius compensation.

It prevents a previous G41 or G42 compensation value from changing the programmed toolpath unexpectedly.

G49 — Cancel Tool-Length Compensation

G49

This cancels active tool-length compensation.

It prevents a previous H offset from continuing to affect the Z-axis position in the new program.

G80 — Cancel Canned Cycles

G80

This cancels active drilling, boring, tapping, or other canned cycles.

It prevents a drilling cycle left active by the previous program from being repeated unexpectedly in the new program.

The source article highlights these commands as essential for clearing retained modal conditions before the machining program begins.

Easy Safety Rule to Remember

G40 G49 G80 clear the previous compensation and cycles.
G90 G94 establish the correct coordinate and feed modes.

In simple words:

Clear the old settings first, and then establish the new program mode.

---

Why This Safety Block Matters

Imagine that the previous program ended while G43 tool-length compensation was still active.

The next program begins directly with G54, without first cancelling the remaining compensation.

When the Z-axis moves down, the control may still apply the previous tool-length offset. As a result, the tool may move tens of millimetres farther than expected and collide with the workpiece.

A short initialization block can prevent an expensive tool, workpiece, fixture, spindle, or machine accident.

Complete FANUC Program Example

Now let us combine the G Codes and M Codes into a simple program.

O0001
G94 G40 G49 G80
T01 M06
G90 G00 G54 X0. Y0.
S3000 M03
G43 H01 Z100.
G01 Z-5. F200
...
G00 Z50.
M09
G49
G91 G28 Z0.
M30

The program shown in the source uses tool change, work-offset selection, spindle control, tool-length compensation, cutting feed, coolant shutoff, compensation cancellation, and Z-axis reference return.

Line-by-Line Explanation

Program Number

O0001

Defines the CNC program number.

Safety Initialization

G94 G40 G49 G80

This line:

• Selects feed per minute
• Cancels cutter radius compensation
• Cancels tool-length compensation
• Cancels active canned cycles

For additional protection, many programs also include G90 in the safety initialization line:

G90 G94 G40 G49 G80

Tool Change

T01 M06

This selects Tool 1 and performs an automatic tool change.

Select Work Offset and Move to the Start Position

G90 G00 G54 X0. Y0.

This line:

• Selects absolute coordinate programming
• Selects rapid positioning
• Activates the G54 work coordinate system
• Moves rapidly to X0 and Y0

Start the Spindle

S3000 M03

This starts the spindle in the forward direction at:

3000 rpm

Activate Tool-Length Compensation

G43 H01 Z100.

This line:

• Activates positive tool-length compensation
• Uses tool-length offset H01
• Positions the Z-axis at 100 mm

Feed the Tool into the Workpiece

G01 Z-5. F200

This moves the tool in a straight line to:

Z = -5 mm

at a feed rate of:

200 mm/min

Retract to a Safe Plane

G00 Z50.

This rapidly retracts the tool to:

Z = 50 mm

Turn Off Coolant

M09

This turns off the coolant system.

Cancel Tool-Length Compensation

G49

This cancels the active tool-length compensation.

Return the Z-Axis to the Reference Point

G91 G28 Z0.

This uses incremental mode.

The Z-axis first performs a zero incremental move, meaning that its current location becomes the intermediate point. It then returns to the machine Z-axis reference point.

End the Program

M30

This ends and resets the program.

Summary: Understanding G Codes and M Codes

G Codes and M Codes perform two different but complementary functions in a CNC program.

G Codes

G codes mainly control tool movement and coordinate modes.

Important examples include:

• G00 — Rapid positioning
• G01 — Linear cutting
• G02 — Clockwise circular interpolation
• G03 — Counterclockwise circular interpolation
• G90 — Absolute coordinate programming
• G91 — Incremental coordinate programming
• G28 — Return to the machine reference point
• G54 — Select the first work coordinate system

M Codes

M codes mainly control auxiliary machine functions.

Important examples include:

• M03 — Start the spindle
• M05 — Stop the spindle
• M06 — Change the tool
• M08 — Turn coolant on
• M09 — Turn coolant off
• M30 — End and reset the program

Key Points to Remember

• Modal codes remain active until another code from the same group replaces them.
• Non-modal codes only apply to the program block in which they appear.
• G00 should not be used carelessly near the workpiece.
• G90 uses absolute coordinates.
• G91 uses incremental coordinates.
• G28 normally moves through an intermediate point before returning to the machine reference point.
• G90 G28 Z0. may first move the tool toward the absolute work-coordinate position Z0.
• G91 G28 Z0. uses the current position as the intermediate point before returning to the Z reference point.
• Every program should begin with a safety initialization block such as G90 G94 G40 G49 G80.

CNC Machining Support from Cast Mold

At Cast Mold, CNC machining is an important part of our one-stop manufacturing service.

We provide integrated support covering:

• Die-casting mold design
• Mold manufacturing
• Aluminum and zinc alloy die casting
• CNC machining
• Drilling and tapping
• Surface finishing
• Dimensional inspection
• Assembly and shipment

For die-cast components, CNC-machined features are often required for:

• Precision mounting holes
• Threads
• Sealing surfaces
• Bearing positions
• Assembly interfaces
• Flatness-critical areas
• Tight-tolerance dimensions

By combining tooling, die casting, CNC machining, surface treatment, and inspection, we help customers reduce communication time between multiple suppliers and improve dimensional consistency in batch production.

For a project evaluation, please provide:

• 2D drawings
• 3D models
• Material requirements
• Annual quantity
• Surface-finish requirements
• Critical tolerances
• Inspection requirements