CNC G Code List: Functions and Common Uses

Example of sequence number, G code, X-axis address and value, and feed rate

G codes are commands in CNC programs that specify motion modes and machining functions. Depending on the code and controller, they can control rapid positioning, linear or circular interpolation, canned cycles, coordinate modes, and tool compensation.

Even when CAM software generates the program, engineers and operators still need to inspect the output for unexpected motion or post-processor errors before machining begins.

For an overview of how G codes and M codes work together in CNC programming, see the G and M codes guide.

CNC G Code List and Their Functions

This CNC G code list brings commonly used commands and selected machine-specific codes into one numerical reference table. When a code has different meanings on milling and turning machines, the table lists those uses separately and identifies the relevant controller or machine type.

The descriptions cover common programming conventions rather than a universal code standard. Modal group assignments, address formats, cycle parameters, and execution behavior can vary by controller. Check the programming manual for the target machine before using a code in a production program.

How Do Modal and Non-Modal G Codes Work?

Modal G codes are the most important concept to understand when reading or writing CNC programs. A modal G code stays active after the block where it's programmed. It continues to apply to every subsequent block until a code from the same modal group replaces or cancels it. The CNC controller does not need the code repeated in every block because the mode remains active until it is replaced or cancelled.

Take G01 as an example. Once you program G01 in a block, every subsequent motion block executes as a linear feed move, even if G01 isn't written again. The mode is active until G00, G02, G03, or another Group 1 code appears. This allows consecutive cutting blocks to omit the motion code when the same mode remains active. The controller continues to apply the previously established G01 mode until another code in the same modal group replaces it.

Non-modal G codes apply to the block in which they are programmed rather than remaining active across subsequent blocks. G04 (dwell), for example, pauses execution for the specified time and does not carry the dwell into the next block. G28 and G53 also operate as single-block commands on many common controls, although their exact behavior must be checked against the target controller's documentation.

A program should not rely on the controller's previous modal state. If a program assumes G90 is active but the controller is still in G91, programmed positions may be interpreted incrementally rather than from the active coordinate origin. The resulting motion can differ substantially from the intended toolpath. Explicitly establish the required modes at the start of the program, following the machine builder's programming conventions.

This is why experienced programmers include a safety initialization block at the beginning of every program:

N010 G21 G17 G40 G49 G80 G90 G94

On many milling controls, this block establishes the metric unit system, XY plane, cancelled cutter and tool length compensation, cancelled canned cycle, absolute positioning, and feed-per-minute mode. Adapt the initialization block to the target controller and machine, and explicitly set any additional modes required by the operation.

Modal groups also matter for post-processor configuration. The group assignment for a specific G code determines which other codes it cancels. Modal group assignments determine which active modes are replaced when a new G code is programmed. Do not assume that a code belongs to the same group across different controller families; check the programming manual when configuring a post-processor or troubleshooting unexpected modal behavior.

Example of G Codes in a CNC Program

The following FANUC-style example illustrates a rectangular contour-milling pass on a vertical machining center. It demonstrates coordinate modes, tool length compensation, cutter radius compensation, and a reference return. It does not clear the interior of a pocket. The code is illustrative; verify the syntax, offsets, toolpath, and safe clearances for the target machine and controller before running it.

O3001                              ; Program number
N010 G21 G17 G40 G49 G80 G90 G94
                                   ; Metric units, XY plane, cancel compensation
                                   ; and canned cycles, absolute mode, feed per minute
N020 G28 G91 Z0                    ; Return Z to the machine reference position
N030 G90 G54                       ; Restore absolute mode and select work offset G54
N040 T01 M06                       ; Tool change: tool 1
N050 S5000 M03                     ; Set spindle speed to 5000 RPM and start clockwise
N060 G00 G43 H01 Z50.0             ; Apply tool length offset H01 and move to Z50
N070 G00 X10.0 Y10.0               ; Rapid to the programmed XY position
N080 G00 Z2.0                      ; Rapid to the approach plane
N090 G01 Z-5.0 F200                ; Feed to the programmed depth
N100 G01 G41 D01 X15.0 F200        ; Activate cutter compensation on the lead-in move
N110 G01 Y40.0 F400                ; Mill the first side
N120 X65.0                         ; Mill the second side
N130 Y10.0                         ; Mill the third side
N140 X15.0                         ; Mill the fourth side
N150 G40 X10.0 Y10.0               ; Cancel cutter compensation during lead-out
N160 G00 Z50.0                     ; Retract to the programmed clearance position
N170 G49                           ; Cancel tool length compensation
N180 G28 G91 Z0                    ; Return Z to the machine reference position
N190 G90                           ; Restore absolute positioning
N200 M30                           ; End program and rewind

How to read the program

Coordinate and motion modes: G21 selects metric input, G54 selects the work coordinate system, G90 selects absolute positioning, and G94 selects feed per minute. G28 commands a return to the machine reference position. In this example, G91 Z0 specifies a zero incremental Z move before the reference-return sequence.

Tool length compensation: G43 H01 applies the configured tool length offset during the move to the programmed Z position. Z50.0 is expressed in the active work coordinate system, with the controller applying the active compensation according to its rules.

Cutter radius compensation: G41 activates left cutter compensation using the configured D01 offset. G40 cancels compensation during the exit move. The lead-in and lead-out distances must be checked against the cutter diameter, compensation value, contour geometry, and controller requirements.

Feed and spindle commands: S5000 M03 sets the spindle speed to 5000 RPM and starts clockwise rotation. F200 and F400 specify feed rates in the active G94 mode, normally interpreted as mm/min under G21.

This example shows a single contour pass, not a complete pocketing strategy. The cutter compensation moves are illustrative. Their suitability depends on the actual cutter diameter, D01 offset, contour geometry, and controller requirements. Validate the toolpath and clearance positions through simulation and at the machine before running the program.

Precision CNC Machining Service

Preparing a part for CNC machining? Upload your CAD file to JLCCNC for a project-specific engineering review, with quotes starting from $1 and lead times as short as 3 days.

Get Instant Quote

How to Verify G Code Compatibility Before Running a CNC Program

1. Check the machine builder's programming manual. The manual lists every G code the machine implements, which modal group it belongs to, its parameters, prerequisites, and any machine-specific behavior. Machine builders and controller manufacturers may provide programming manuals for their products. Use the documentation for the exact machine and control series rather than relying on a generic G code reference.
2. Check the controller documentation separately from the machine manual. The machine builder and the controller manufacturer are sometimes different. A machine may use a Fanuc 0i-MF controller with machine-builder additions layered on top. The Fanuc programming manual covers the controller-level G codes. The machine builder's manual covers machine-specific additions and any modifications to standard behavior.
3. Verify the CAM post-processor matches the machine and controller. The post-processor translates CAM toolpaths into G code for a specific machine and controller. A generic post-processor may produce code that is syntactically plausible but incompatible with the target machine, such as an unsupported cycle format or a missing required address. The post-processor should be specific to the machine model and controller version. Run a test program from the post-processor and compare the output against the machine manual's cycle syntax before committing to production use.
4. Simulate the program before running. CAM simulation shows the toolpath geometrically but doesn't interpret the G code the way the controller does. NC verification software such as VERICUT, simulates the program as the specific controller will read it, including modal state behavior, work offset application, cutter comp logic, and canned cycle execution. This step catches post-processor errors and code-level problems that visual CAM simulation misses.
5. Dry run at the machine. Before the first production run, run the program at the machine with the spindle off, rapid override at 10-20%, and feed override ready to zero. Watch each move and verify that the programmed positions, approach distances, and cycle depths match the intended setup. Investigate any unexpected motion before machining the workpiece. Any motion that looks wrong, a Z approach that comes closer to the part than expected, an arc that goes the wrong direction, should be investigated before material is loaded.

FAQs About CNC G Codes