G-Code Commands

Motion Commands

G0 - Rapid Positioning

Syntax: G0 X[coordinate] Y[coordinate] Z[coordinate]

Function: Move to the specified position at maximum speed without machining operations.

Description:

• Used for rapid positioning without cutting material
• Movement path may not be linear
• Displayed as red path in 3D visualization
• Automatically turns off laser in laser mode

Examples:

G0 X10 Y20 Z5    ; Rapid move to (10, 20, 5)
G0 Z10           ; Z-axis only rapid move to 10mm

G1 - Linear Interpolation

Syntax: G1 X[coordinate] Y[coordinate] Z[coordinate] F[feed rate] S[laser power/spindle speed]

Function: Move linearly to the target position at specified feed rate, can perform machining operations.

Description:

• Used for precise linear cutting or laser engraving
• Displayed as blue path in 3D visualization
• In laser mode, S parameter controls laser power
• In CNC mode, S parameter controls spindle speed

Examples:

G1 X50 Y30 F1000      ; Move to (50,30) at 1000mm/min
G1 Z-2 F100 S800      ; Move down to Z-2, laser power 800

G2 - Clockwise Arc Interpolation

Syntax: G2 X[end X] Y[end Y] I[center X offset] J[center Y offset] F[feed rate]

Function: Arc interpolation from current position to specified endpoint in clockwise direction.

Description:

• I, J parameters represent center offset relative to start point
• Currently treated as linear in visualization
• Suitable for arc cutting and engraving

Examples:

G2 X20 Y20 I10 J0 F500    ; Clockwise arc to (20,20)

G3 - Counterclockwise Arc Interpolation

Syntax: G3 X[end X] Y[end Y] I[center X offset] J[center Y offset] F[feed rate]

Function: Arc interpolation from current position to specified endpoint in counterclockwise direction.

Description:

• I, J parameters represent center offset relative to start point
• Currently treated as linear in visualization
• Suitable for arc cutting and engraving

Examples:

G3 X0 Y20 I0 J10 F500     ; Counterclockwise arc to (0,20)

Plane Selection Commands

G17 - XY Plane Selection

Syntax: G17

Function: Select XY plane as working plane.

Description:

• Default working plane
• Arc interpolation performed in XY plane
• Z-axis is the vertical axis

G18 - XZ Plane Selection

Syntax: G18

Function: Select XZ plane as working plane.

Description:

• Arc interpolation performed in XZ plane
• Y-axis is the vertical axis

G19 - YZ Plane Selection

Syntax: G19

Function: Select YZ plane as working plane.

Description:

• Arc interpolation performed in YZ plane
• X-axis is the vertical axis

Unit Setting Commands

G20 - Inch Units

Syntax: G20

Function: Set coordinate units to inches.

Description:

• All subsequent coordinate values interpreted in inches
• 1 inch = 25.4 millimeters
• Affects all coordinates and feed rates

G21 - Millimeter Units

Syntax: G21

Function: Set coordinate units to millimeters.

Description:

• Default unit setting
• All subsequent coordinate values interpreted in millimeters
• Recommended unit to use

Homing and Reset Commands

G28 - Return to Machine Home

Syntax: G28 or G28 X Y Z

Function: Return to machine home position.

Description:

• Without parameters, all axes return to origin (0,0,0)
• With parameters, specified axes return to origin
• Current position set to (0,0,0) after execution

Examples:

G28           ; All axes return to origin
G28 Z         ; Z-axis only return to origin

G30 - Return to Preset Position

Syntax: G30

Function: Return to preset reference position.

Description:

• Similar to G28, but returns to preset position
• Specific position determined by machine configuration

G92 - Set Current Position

Syntax: G92 X[coordinate] Y[coordinate] Z[coordinate]

Function: Set current position to specified coordinate values.

Description:

• Does not move machine, only redefines current position
• Used to establish workpiece coordinate system
• Affects all subsequent coordinate calculations

Examples:

G92 X0 Y0 Z0    ; Set current position as origin
G92 X10         ; Set current X position to 10

Pause Commands

G4 - Dwell

Syntax: G4 P[seconds]

Function: Pause program execution for specified time.

Description:

• P parameter specifies pause time (seconds)
• Used for waiting spindle stabilization, cooling, etc.
• Does not change current position

Examples:

G4 P2.5       ; Pause for 2.5 seconds
G4 P1         ; Pause for 1 second

Coordinate Mode Commands

G90 - Absolute Coordinate Mode

Syntax: G90

Function: Set to absolute coordinate mode.

Description:

• Default mode
• All coordinate values relative to workpiece origin
• Recommended coordinate mode

G91 - Relative Coordinate Mode

Syntax: G91

Function: Set to relative coordinate mode.

Description:

• All coordinate values relative to current position
• Used for incremental movements
• Use with caution

Coordinate System Selection Commands

G53 - Machine Coordinate System

Syntax: G53

Function: Temporarily select machine coordinate system.

Description:

• Only effective for current line
• Coordinates relative to machine origin
• Often used with G0/G1

Examples:

G0 G53 Z0     ; Z-axis return to 0 position in machine coordinate system

G54-G59 - Workpiece Coordinate Systems

Syntax: G54 / G55 / G56 / G57 / G58 / G59

Function: Select workpiece coordinate systems 1-6.

Description:

• G54 is default workpiece coordinate system
• Each coordinate system has independent origin offset
• Used for multi-workpiece machining

Feed Rate Mode Commands

G93 - Inverse Time Feed Mode

Syntax: G93

Function: Set inverse time feed mode.

Description:

• F value represents reciprocal of time required to complete the movement
• Less commonly used feed mode

G94 - Units Per Minute Feed Mode

Syntax: G94

Function: Set units per minute feed mode.

Description:

• Default feed mode
• F value represents distance moved per minute
• Units: mm/min or inch/min

Tool Compensation Commands

G40 - Cancel Tool Compensation

Syntax: G40

Function: Cancel tool radius compensation.

Description:

• Default state
• Move precisely along programmed path

G41 - Left Tool Compensation

Syntax: G41

Function: Enable left tool radius compensation.

Description:

• Tool center offset to left of programmed path
• Compensation value set by tool table

G42 - Right Tool Compensation

Syntax: G42

Function: Enable right tool radius compensation.

Description:

• Tool center offset to right of programmed path
• Compensation value set by tool table

G43 - Tool Length Compensation

Syntax: G43

Function: Enable tool length compensation.

Description:

• Compensate for tool length differences in Z-axis direction
• Compensation value set by tool table

G49 - Cancel Tool Length Compensation

Syntax: G49

Function: Cancel tool length compensation.

Description:

• Return to uncompensated state
• Z-axis moves according to programmed values

Canned Cycle Commands

G80 - Cancel Canned Cycle

Syntax: G80

Function: Cancel current canned cycle.

Description:

• End cycle machining
• Return to normal movement mode

G81 - Drilling Cycle

Syntax: G81 X[position] Y[position] Z[depth] R[retract height] F[feed]

Function: Execute simple drilling cycle.

Description:

• Rapid descent to R height
• Drill to Z depth at F speed
• Rapid retract to R height

G82 - Drilling Cycle with Dwell

Syntax: G82 X[position] Y[position] Z[depth] R[retract height] P[dwell time] F[feed]

Function: Execute drilling cycle with dwell.

Description:

• Similar to G81, but dwell P seconds at bottom
• Used for chip breaking or chip evacuation

G83 - Deep Hole Drilling Cycle

Syntax: G83 X[position] Y[position] Z[depth] R[retract height] Q[peck feed] F[feed]

Function: Execute peck drilling cycle.

Description:

• Multiple feed increments for deep holes
• Q parameter specifies feed increment per peck
• Retract for chip evacuation each time

Spindle Control Commands

M3 - Spindle On Clockwise/Laser On

Syntax: M3 S[speed/power]

Function: Start spindle clockwise rotation or turn on laser.

Description:

• CNC mode: S parameter is spindle speed (RPM)
• Laser mode: S parameter is laser power (0-1000)
• Must execute before cutting

Examples:

M3 S12000     ; Spindle 12000 RPM
M3 S800       ; Laser power 800

M4 - Spindle On Counterclockwise

Syntax: M4 S[speed]

Function: Start spindle counterclockwise rotation.

Description:

• Used for special machining requirements
• Such as tapping operations

M5 - Spindle Stop/Laser Off

Syntax: M5

Function: Stop spindle or turn off laser.

Description:

• Safely stop spindle
• Turn off laser output in laser mode
• Must execute at end of machining

Coolant Control Commands

M7 - Mist Coolant On

Syntax: M7

Function: Turn on mist coolant.

Description:

• Used for light cooling
• Reduce dust

M8 - Flood Coolant On

Syntax: M8

Function: Turn on flood coolant.

Description:

• Used for heavy cooling
• Improve machining quality

M9 - Coolant Off

Syntax: M9

Function: Turn off all coolant.

Description:

• Stop coolant supply
• Execute at program end

Program Control Commands

M0 - Program Pause

Syntax: M0

Function: Pause program execution, wait for operator to continue.

Description:

• Requires manual continuation
• Used for workpiece inspection or tool change

M1 - Optional Pause

Syntax: M1

Function: Optional program pause.

Description:

• Only effective when optional pause is enabled
• Used for program debugging

M2 - Program End

Syntax: M2

Function: Program end.

Description:

• Stop spindle and coolant
• Program execution complete

M30 - Program End and Return to Origin

Syntax: M30

Function: Program end and return to origin.

Description:

• Similar to M2, but automatically return to origin
• Recommended program end method

Parameter Description

Coordinate Parameters

• X: X-axis coordinate value
• Y: Y-axis coordinate value
• Z: Z-axis coordinate value
• I: Arc center X-axis offset
• J: Arc center Y-axis offset
• K: Arc center Z-axis offset

Control Parameters

• F: Feed rate (mm/min or inch/min)
• S: Spindle speed (RPM) or Laser power (0-1000)
• P: Dwell time (seconds)
• Q: Peck feed amount (for cycles)
• R: Retract height (for cycles)

Working Range Limits

• X-axis: -500mm to +500mm
• Y-axis: -500mm to +500mm
• Z-axis: -200mm to +200mm
• Spindle Speed: 0-24000 RPM
• Laser Power: 0-1000

Comment Format

• Use semicolon ( ; ) to add comments
• Comment content does not affect program execution
• Recommend adding necessary explanations

Examples:

G0 X0 Y0 Z5    ; Move to start position
M3 S800        ; Turn on laser, power 800
G1 X10 F1000   ; Linear move to X10
M5             ; Turn off laser