What is G Code and M Code: Differences, Uses & Examples

G and M codes for CNC machining are instruction types used in CNC programs. G codes define tool motion and machining modes, while M codes typically control auxiliary functions such as spindle operation, coolant, and program stops. Their exact behavior depends on the CNC controller and machine configuration. This guide explains how the two code types differ, how they work together in a program, and where to find common code references.

What Are G Codes and M Codes in CNC Programming?

CNC milling machine cutting an aluminum workpiece

Basic G code and M code are widely used in CNC part programs. ISO 6983-1:2009 defines a program data format and address-word framework for certain numerically controlled machines. It does not make every G or M code number, modal group, or machine function universal. The meaning and availability of individual codes can vary by controller, machine type, enabled options, and machine-builder configuration. The letter identifies an address category, while the following number specifies a command within that controller's programming system. The letter prefix "G" and "M" tells you what kind of instruction it is. The number tells you which specific function within that category.

What G Codes Control

G codes define motion commands and many of the operating modes that determine how a CNC program is interpreted. Depending on the code and controller, they can select absolute or incremental positioning, set the interpolation plane, activate cutter compensation, or call a canned cycle. Motion commands such as G00, G01, G02, and G03 determine how the tool moves between programmed positions.

To understand how these commands relate to the cutter's actual route through the material, read our guide to CNC toolpaths.

Some of the motion types G codes define:

• G00 commands rapid positioning to a programmed location. It is commonly used to approach a cutting position or retract after machining, but it does not guarantee a collision-free path. The programmed move must account for the workpiece, fixtures, tool geometry, and machine-specific rapid-motion behavior.
• G01 tells the machine to move the tool in a straight line at a specified feed rate, while cutting. It's used when the tool needs to remove material along a straight path.
• G02 tells the machine to move in a circular arc clockwise.
• G03 tells the machine to move in a circular arc counterclockwise.
• G codes like G81 through G89 activate canned cycles. Canned cycles are pre-programmed sequences of movements that the machine performs using a single code. G81 is a basic drilling canned cycle on many milling controllers. A typical block specifies the hole coordinates, the R-plane position, the final Z depth, and the drilling feed rate. The controller handles the approach, feed, and retract motions according to its cycle definition and the active positioning modes. The programmer must verify the retract level and clearance above the workpiece before running the cycle.

For a more complete list of G codes, please check JLCCNC's G code list.

What M Codes Control

M codes generally control auxiliary machine functions rather than defining the tool's geometric path. Depending on the machine, they may start or stop the spindle, switch coolant, initiate a tool change, pause the program, or trigger machine-specific operations.

The spindle is controlled by M codes. M03 commands clockwise spindle rotation, M04 commands counterclockwise rotation, and M05 stops the spindle. Confirm the control's direction convention and the spindle setup before running the program. Coolant is controlled by M codes, M08 turns flood coolant on, M09 turns it off. M codes can initiate tool changes, pause or end a program, and control machine-specific auxiliary functions. On turning centers and machines with multiple spindles or turrets, additional M codes may select or synchronize machine units, depending on the machine-builder implementation.

For a more complete list of M codes, please check JLCCNC's M code list.

Precision CNC Machining Service

Upload your CAD files to get an instant CNC machining quote and DFM feedback from JLCCNC engineers.

Get Instant Quote

How Do G Codes and M Codes Work Together in a CNC Program?

Annotated CNC program block showing the sequence number

A CNC program file has a sequence of lines of code. Each line can have G codes and M codes alongside others. The controller reads each line in sequence and executes the combined instructions.

How a CNC Program Block Is Structured

A CNC program block may contain a sequence number (N), one or more G codes, axis coordinates, a feed-rate word (F), a spindle-speed word (S), a tool number (T), and an M code. The required words depend on the operation and the controller. Many blocks contain only the addresses needed for that step, with modal settings carried forward from earlier blocks.

A typical block might look like this

N050 G01 X75.000 Y30.000 F350

This block commands a linear move to X75.000, Y30.000 at a programmed feed rate of 350 in the currently active feed mode. The actual distance units and feed interpretation depend on the active modal settings, including the unit-selection and feed-mode commands established earlier in the program.

Multiple G codes can appear in one block when they belong to compatible modal groups. A modal group contains mutually exclusive G codes, so only one code from that group can be active at a time. G codes from the same group cannot both appear in the same block because they would conflict. One M code per block is the standard practice on most controllers, even where the syntax technically permits more.

Reading a CNC Milling Program Line by Line

The following example illustrates a basic three-axis milling sequence. It is intended to show how G codes and M codes work together in a program, not to serve as a production-ready program. Actual code behavior and safe motion depend on the CNC control and machine setup.

Several lines illustrate how a CNC program executes:

• N010 G21 G17 G40 G49 G80 — Initial mode setup. Selects metric units and the XY plane, then cancels cutter radius compensation, tool length compensation, and canned cycles. It does not reset every modal state.
• N020 G28 G91 Z0 — Reference return. Uses a common G28 return pattern. The actual motion depends on the control and machine configuration, so the return path and clearance must be verified.
• N040 T01 M06 and N050 G90 G54 — Tool and work coordinate system selection. The program calls tool 1, commands a tool change, selects absolute positioning, and activates work coordinate system G54. A tool length offset must also be applied with the appropriate G43 H command before machining at a programmed Z position that depends on tool length.
• N060 S4500 M03 — Spindle start. Commands 4,500 RPM and clockwise spindle rotation.
• N070 to N090 — Positioning and feed motion. The tool moves to the programmed XY position, moves to Z5.0, and then feeds to Z−8.0. The Z positions are relative to the active work coordinate system; confirm that the path clears the stock and fixtures.
• N100 X120.0 F350 — Modal motion. G01 remains active from the previous block, so the tool continues with a linear feed move to X120.0. The feed values use the active feed mode; this example does not explicitly set G94.
• N110 to N140 — Retract and program end. The program commands a Z retract, stops the spindle, switches coolant off, and ends with M30. The retract height and end-of-program behavior must be checked against the machine setup and control.

Modal and Non-Modal Codes in Program Execution

Modal G-codes are settings that stay active until you change them.

For example, in CNC machining:

• G01 means the machine moves in a straight line at a controlled feed rate.
• Once you write G01, the machine keeps using that movement mode for the next moves, even if you don't write G01 again.
• G00 tells the machine to switch to rapid movement, so it moves quickly instead of following the G01 feed movement.

Example

G01 X10
X20
X30
G00 X50

Here's what happens:

Because G01 is modal, it does not need to be repeated in every subsequent block while that motion mode remains active. This reduces repetition, but the programmer must still track which motion mode is in effect.

However, you must remember which mode is currently active. If you assume the machine is moving slowly with G01 when G00 is actually active, you could cause an error or even damage the tool or workpiece.

While, non-modal codes are active for a single block only.

Example

G04 (dwell, pause for a specified time)

It executes once in the block where it appears and has no effect on subsequent blocks.

Understanding modal behavior is essential for debugging CNC programs. A machining error that appears in the middle of a program often traces back to a modal state set several blocks earlier rather than to the block where the error manifested.

How Are G Codes and M Codes Generated and Verified?

CNC programming workflow

Most production CNC programs are not written from scratch in G code. They're generated by CAM software from 3D geometry and then verified before running on the machine.

CAD/CAM and Post-Processor Workflow

In a typical CAD/CAM workflow, the programmer imports the part geometry, defines machining operations, and generates toolpaths using selected tools and cutting parameters. The post-processor then converts the CAM output into NC program syntax suited to the target machine and controller. A post-processor configured for one machine may not be suitable for another, even when both use the same controller family, because axis configuration, machine options, tool-change logic, and auxiliary M codes can differ.

The post-processor must match the target machine and controller. It determines how CAM operations are translated into controller-specific motion commands, cycles, and auxiliary functions. However, a valid post-processed program can still contain incorrect toolpaths, offsets, or machining parameters, so the output must be verified before production use.

Internal toolpath simulation and final NC program verification serve different purposes. Toolpath simulation checks the programmed cutting path generated in CAM, while NC program verification evaluates the post-processed code against a model of the target machine and its operating conditions. The reliability of either check depends on how accurately the simulation or verification setup represents the actual controller, machine configuration, tools, fixtures, and stock. A successful simulation does not by itself establish that the final NC program is safe to run on the machine.

See how a CNC post-processor converts CAM toolpaths into machine-ready G-code in detail.

Verifying and Proving Out Generated CNC Programs

CAM systems can simulate toolpaths generated within the CAM environment. This can reveal issues such as unintended cutting paths, incorrect tool selection, or rapid moves into the stock. However, CAM simulation does not necessarily reproduce how the target controller interprets the final post-processed NC program.

Dedicated NC verification software can analyze post-processed programs using supported controller models and machine configurations. Depending on the software and its configuration, verification may account for modal states, coordinate transformations, canned cycles, and machine motion. Its ability to detect post-processor errors depends on the functions supported and the accuracy of the controller model and machine setup.

Before running a new or modified program in production, follow the machine manufacturer's program proving and verification procedures. Where supported, use graphics or machine simulation first. Then perform a controlled dry run or other prescribed proving procedure, ensuring adequate clearance between the tool, workpiece, fixtures, and other machine components. Use single-block execution and appropriate feed and rapid overrides as required by the machine manual. Reduced override settings provide additional time to observe motion but do not eliminate collision risk.

Precision CNC Machining Service

Upload your CAD file to get a fast quote starting from $1, with lead times as short as 3 days.

Get Instant Quote

Common G Codes and M Codes Used in CNC Machining

Common Milling G Codes — Typical Fanuc/Haas-Style Definitions

Common M Codes for Spindle, Coolant, and Program Control

These represent the most widely implemented codes. Specific code numbers and their exact behavior depend on the controller. Verify against the machine's programming manual.

Do G Codes and M Codes Work the Same on Every CNC Machine?

The short answer is no, and this is one of the most consistent sources of confusion for programmers moving between machines.

Differences Between CNC Milling and Turning

Milling and turning programs use largely the same G code structure for motion but differ significantly in axis naming, coordinate systems, and some cycle behaviors. On a turning center, the X axis controls the diameter dimension (often specified as diameter value, not radius), and Z controls length along the spindle axis. A G01 move to X50.0 on a lathe means moving to a diameter of 50mm, very different from the same code on a mill where X50.0 is a linear position.

Threading on a turning center uses G32 (single-pass thread cutting) or G76 (multi-pass thread cycle), codes that have no equivalent in milling. Facing and turning cycles specific to lathes (G70, G71, G72 on Fanuc) don't exist in milling contexts. Live tooling on turning centers introduces milling-type motion codes (G12.1 polar coordinate interpolation, for example) alongside turning codes, making turning center programming its own dialect.

Controller and Machine-Builder Variations

The ISO 6983 standard defines the framework but leaves significant room for manufacturer implementation. Fanuc controls dominate production CNC globally, and Fanuc syntax has become something of a de facto standard, but Fanuc 0i, 10/11, 16/18, 30/31/32 series all have syntax differences between them. Haas controls are Fanuc-compatible for most basic codes but use different M codes for machine-specific functions. Siemens 840D uses its own syntax for cycles and some G codes. Mitsubishi, Mazak MAZATROL, and Okuma OSP each have their own implementation.

M codes especially are machine-specific. M08 for flood coolant is common but not universal. The M code for through-spindle coolant, high-pressure coolant, air blast, or chip conveyor varies between machine builders and sometimes between models from the same builder. Never assume an M code from one machine works on another without verifying against the specific machine's documentation.

Basic G Code and M Code Mistakes That Affect Machining

FAQs About G Codes and M Codes