Easy CNC Documentation

Modular CNC software for Arduino controller

Status: Beta

Brought to you by: giurlanda

G-Code

Labels: GCode (1)

Authors:

[ < Back ]

G-Code

G-code (also RS-274), which has many variants, is the common name for the most widely used numerical control (NC) programming language. It is used mainly in computer-aided manufacturing to control automated machine tools.
G-code is a language in which people tell computerized machine tools how to make something. The "how" is defined by instructions on where to move, how fast to move, and what path to move. The most common situation is that, within a machine tool, a cutting tool is moved according to these instructions through a toolpath and cuts away material to leave only the finished workpiece. More details in Wikipedia's G-Code article.

This page describes the G-Code words supported by Easy CNC firmware (eCNC fw) and how they work. The fw follows the RS274/NGC G-Code standard.

Instruction

A typical piece of G-Code as sent to the eCNC fw machine might look like this:

G17 G20 G90 G94 G54
G0 Z0.25
X-0.5 Y0.
Z0.1
G01 Z0. F5.
G02 X0. Y0.5 I0.5 J0. F2.5
X0.5 Y0. I0. J-0.5
X0. Y-0.5 I-0.5 J0.
X-0.5 Y0. I0. J0.5
G01 Z0.1 F5.
G00 X0. Y0. Z0.25`

Fields

A permissible line of input G-Code consists of the following, in order, with the
restriction that there is a maximum (currently 256) to the number of characters allowed on a line.

an optional line number;
any number of words, parameter settings, and comments;
an end of line marker (carriage return or line feed or both).

Any input not explicitly allowed is illegal and will cause the Interpreter to signal an error.
Spaces and tabs are allowed anywhere on a line of code and do not change the meaning of the
line, except inside comments. A field can be interpreted as a command, parameter, or for any other special purpose. It consists of one letter directly followed by a number. The letter gives information about the meaning of the field (see the list below in this section). Numbers can be integers (128) or fractional numbers (12.42), depending on context. In this description, the numbers in the fields are represented by nnn as a placeholder.

Letter	Meaning
Gnnn	Standard G-Code commands
Mnnn	Proprietary G-Code commands, they can change from a machine to another depending on the controll software used
Tnnn	Select tool nnn
Snnn	Command parameter, such as time in seconds
Pnnn	Command parameter
Xnnn	X coordinate, usually to move to. This can be an Integer or Fractional number.
Ynnn	Y coordinate, usually to move to. This can be an Integer or Fractional number.
Znnn	Z coordinate, usually to move to. This can be an Integer or Fractional number.
Innn	Parameter - X-offset in arc move
Jnnn	Parameter - Y-offset in arc move
Rnnn	Parameter - radius of an arc move
Lnnn	Parameter - Fixed cycle loop count
Fnnn	Feedrate in mm per minute. (Speed of print head movement)
Nnnn	Line number.

Comments

Gcode comments begin at a semicolon, and end at the end of the line:

N3 T0*57 ; This is a comment
N4 G92 E0*67
; So is this
N5 G28*22

Special fields

G-Commands

G0 & G1: Move

G0: rapid linear move
G1: linear move

Usage
G0 Xnnn Ynnn Znnn
G1 Xnnn Ynnn Znnn Fnnn

Parameters:
Not all parameters need to be used, but at least one has to be used.
Xnnn The position to move to on the X axis
Ynnn The position to move to on the Y axis
Znnn The position to move to on the Z axis
Fnnn The feedrate per minute of the move between the starting point and ending point (if supplied)

Example

1. G0 X12
2. G1 X10 Y5.1 F150
3. G1 X5 Y3.45

First line moves the tool in the position X 12 (the system keeps the Y and Z current values) at the max motion speed of the machine. Second line moves the tool in the position X:10 Y:5.1 with a feedrate of 150 mm/min. Third line moves the tool in X:5 Y:3.45 with the same feedrate of the previous command.

G2 & G3: Arc Move with center format

Usage
G2 Xnnn Ynnn Innn Jnnn Fnnn (Clockwise Arc)
G3 Xnnn Ynnn Innn Jnnn Fnnn (Counter-Clockwise Arc)

Parameters:
Xnnn The position to move to on the X axis
Ynnn The position to move to on the Y axis
Innn The point in X space from the current X position to maintain a constant distance from
Jnnn The point in Y space from the current Y position to maintain a constant distance from
Fnnn The feedrate per minute of the move between the starting point and ending point (if supplied)

Example

1. G2 X90.6 Y13.8 I5 J10
2. G3 X90.6 Y13.8 I5 J10

First line moves in a Clockwise arc from the current point to point (X=90.6,Y=13.8), with a center point at (X=current_X+5, Y=current_Y+10).
Second line moves in a Counter-Clockwise arc from the current point to point (X=90.6,Y=13.8), with a center point at (X=current_X+5, Y=current_Y+10)

G2 & G3: Arc Move with radius format

Usage
G2 Xnnn Ynnn Rnnn Fnnn (Clockwise Arc)
G3 Xnnn Ynnn Rnnn Fnnn (Counter-Clockwise Arc)

Parameters
Xnnn The position to move to on the X axis
Ynnn The position to move to on the Y axis
Rnnn The radius of the arc.
Fnnn The feedrate per minute of the move between the starting point and ending point (if supplied)

Example

1. G2 X90.6 Y13.8 R5
2. G3 X90.6 Y13.8 R10

First line moves in a Clockwise arc from the current point to point (X=90.6,Y=13.8), with a radius of 5mm
Second line moves in a Counter-Clockwise arc from the current point to point (X=90.6,Y=13.8), with a radius of 10mm

G4: Pause

Usage
G4 Pnnn

Parameters
Pnnn Number of milliseconds to be paused

Example

1. G4 P5

First line pauses the machine for five seconds.

G20: Set Units to Inches

G20 sets units in inches from now on.

G21: Set Units to Millimeters

G21 sets units in millimeters from now on. It is the default setting.

G90: Absolute positioning

G90 sets absolute coordinates system for the tool positioning.

G91: Relative positioning

G91 sets relative coordinates system for the tool positioning.

G92: Set Position

Usage
G92 Xnnn Ynnn Znnn

Parameters
Xnnn The position of X axis
Ynnn The position of Y axis
Rnnn Z postion of Z axis
Lnnn Times that has to repeat the operation

Example

1. G92 X10 Y10 Z10
2. G92 X10 Y10
3. G92

First line sets the current position to X=10, Y=10 and Z=10.
Second line sets the current position to X=10, Y=10 and Z=0.
Third line sets all axes to X=Y=Z=0

G98 & G99 Cycle retraction mode

G98 sets the retraction position after a drilling sycle at the Z position specified by R.
G99 sets the retraction position after a drilling sycle at the Z position kept before the cycple beginning. But if the Z position is lower than R, the retraction will be at R.

G81: Simple drilling cycle

Usage
G81 Xnnn Ynnn Znnn Rnnn Lnnn

Parameters
Xnnn The position to move to on the X axis
Ynnn The position to move to on the Y axis
Rnnn Z postion after retraction
Lnnn Times that has to repeat the operation

Example

1. G90 G81 G98 X400 Y500 Z150 R280
2. G91 G81 G98 X400 Y500 Z-60 R180 L3

First line stes absolute coodinates, than makes the below operations
1. rapid movement to position (X=400, Y=500)
2. rapid movement to Z position Z=280
3. move down Z to position Z=150 with the current feedrate
4. rapid tool retraction at Z=280.

Second line sets relative coordinate system (G91) and the retraction mode to R (98), let suppose that the current position is (X=100, Y=200, Z=300), so the cycle makes the below operations:
1. rapid movement to the position (X=100, Y=200, Z=300+180)
2. rapid movement to the position (X=100+400, Y=200+500, Z=480)
3. move down up to the position (X=500, Y=700, Z=480-60)
4. rapid tool retraction at the position (X=500, Y=700, Z=480)
5. repeat from point 2 with current position (X=500, Y=700, Z=480), the cycle is repeated for three times.

M-Commands

M0: Stop or Unconditional stop

M0 stops the router and the tool

M3: Tool On or Spindle On, Clockwise

M3 has different behaviours depending on the tools:
LASER: it turns on the laser,
MILLING MACHINE: it turns on the milling machine and set the CW spindle if it is supported,
* SERVO PLOTTER: it moves down the pen

M4: Tool On or Spindle On, Counter-Clockwise

M4 has different behaviours depending on the tools:
LASER: it turns on the laser,
MILLING MACHINE: it turns on the milling machine and set the CCW spindle if it is supported,
* SERVO PLOTTER: it moves down the pen

M5: Tool off or Spindle Off

M5 has different behaviours depending on the tools:
LASER: it turns off the laser,
MILLING MACHINE: it turns off the milling machine,
* SERVO PLOTTER: it moves up the pen

[ < Back ]

Easy CNC by Francesco Giurlanda is licensed under a Creative Commons Attribution-ShareAlike 4.0 International License.
Permissions beyond the scope of this license may be available at http://sourceforge.net/projects/easycnc/support?source=navbar.