G-Code (RS-274) Support

Supported G-Code Letters

The G-code letters in the table that follow are supported by the language.

Table: Supported G-Code Letters

More details about the G-code letters follow:

• Each of these letters is supported by the G-code (RS-274) standard.
• These letters are case-insensitive, so that both G1 and g1 mean the same thing.
• Most of the remaining letters are allowed to be used as axis names (e.g., X, Y, and Z). See Axis Naming Conventions for more information.
• Some additional letters (H and L) are part of the G-code (RS-274) standard but are unused in AeroScript. These letters are reserved for future use.

Many concepts in G-code are not whitespace-sensitive. Whitespace between G-code letters and their expressions is optional. For example, each of the following lines of G-code programming have the same meaning.

If you specify two or more G-code commands on one AeroScript program line, the commands are usually executed in the order that follows:

1. Modal G-code words (G17, G71, G90, and so on).
2. F, E, S, and T commands, in that order (F100, T10, and so on).
3. Spindle on or off (M3, M4, M5).
4. Cutter compensation commands (G40, G41, G42, G43, G44, G143, G144, and G149).
5. Motion mode commands (G0, G1, G2, and G3).
6. Motion commands (x10, Y-10, and so on).
7. Control M-codes (M0, M1, M2, M30, M47, and so on).

E Command

The E command is used to specify the feedrate for dependent axes when performing coordinated motion. Coordinated motion includes the following types of motion:

• G1, MoveLinear()
• G2, MoveCw()
• G3, MoveCcw()
• G12 and G13

An E command may be specified on its own program line, or it can be specified on the same program line as G-code motion.

An E command can either be specified with a constant value or with a numeric expression.

The dependent feedrate is used for coordinated moves that contain only dependent axes. If a coordinated move contains only dominant axes, or a mixture of dominant and dependent axes, then the move will use the dominant feedrate (the F command).

F Command

The F command is used to specify the feedrate for dominant axes when performing coordinated motion. Coordinated motion includes the following types of motion:

• G1, MoveLinear()
• G2, MoveCw()
• G3, MoveCcw()
• G12 and G13

An F command may be specified on its own program line, or it can be specified on the same program line as G-code motion.

An F command can either be specified with a constant value or with a numeric expression.

The dominant feedrate is used for coordinated moves that contain only dominant axes or a mixture of dominant and dependent axes. If a coordinated move contains only dependent axes, then the move will use the dependent feedrate (the E command).

G-Codes

G-codes are used to configure and perform various types of motion on the controller.

G-codes must be specified with a numeric integer constant. Preceding zeros are allowed to be used in the numeric value, making both of the following G-codes equivalent:

Refer to the list of Supported G-Codes for more information.

I/J/K Offsets

The I, J, and K offsets are only applicable with the G2, G3, G12, and G13 G-codes.

M-Codes

M-codes are used to perform miscellaneous functionality on the controller.

M-codes must be specified with a numeric integer constant. Preceding zeros are allowed to be used in the integer value. The following two M-codes are equivalent:

• M2
• M02

Refer to the list of Supported M-Codes for more information.

N-Codes

N-codes are used to label a line or a block of G-code. N-codes are optional on G-code lines. If an N-code is specified on a program line that contains G-code concepts, then it must be specified before all other G-codes on the same line.

N-codes must be specified with a positive numeric integer constant. Preceding zeros are allowed to be used in the numeric value.

• N01G1X10
• N02G1X15

P Command

The P command has different meanings depending upon the context in which it is specified. A P command cannot be specified on its own program, and must be specified on the same line as G2, G3, G12, or G13 G-code motion, or with the G4 G-code.

• When specified along with the G4 G-code, the numeric value of the P command is used to specify the amount of time that the G4 command will delay execution of the task.

• When specified with G2, G3, G12, or G13 G-code motion, the numeric value of the P command is used to specify the absolute starting angle for the G2 or G3 arc move.

In both usages, the numeric value specified as part of the P command can be a numeric constant or a numeric expression.

Q Command

The Q command is used to specify the absolute ending angle for a G2, G3, G12, or G13 arc move. A Q command cannot be specified on its own line, and must be specified on the same line as G2, G3, G12, or G13 G-code motion.

The numeric value specified as part of a Q command can be a numeric constant or a numeric expression.

R Command

The R command is used to specify the radius in an arc move (G2, G3, G12, and G13 G-codes). The R command cannot be specified on its own line. When using G-codes, an R command can only be specified on the same line as a G2, G3, G12, or G13 G-code motion.

The numeric value specified as part of an R command can be a numeric constant or a numeric expression.

S Command

The S command is used to define the speed of the spindle that is active on the current task.

T Command

Use the T command together with custom T-codes to make a user-defined tool selection routine in AeroScript.

For more information about how to use custom T-codes, see Custom T-codes.

Supported G-Codes

Supported M-Codes

G-Code Specification Rules

G-Code and Exponential Notation

AeroScript has special rules when parsing G-code programs due to the existence of the E command in the G-code dialect, in addition to support for constant floating-point values that are specified with exponential notation, as well as the G-code dialect being whitespace-insensitive.

A floating-point value specified with exponential notation must be delimited on both its left and right sides in order to prevent conflicts with the E command in G-code programming. The following examples show how exponential notation and the E command are treated in various circumstances.

// E commands
E100E 100
				
// Exponential notation
$myVar = 1e10

// Move with Y = 1, E command = 10
G1 Y1E10

// Move with Y = 1, E command = 10
G1 Y1 E10

// Move with Y = 1E10 (no E command)
G1 Y 1E10

// Move with Y = 1, E command = 10
G1 Y 1 E 10

// Exponential notation can be enforced by using delimiter characters
G1 Y(1E10)G1 Y=1E10

G-Code and Hexadecimal Notation

In addition to the exceptions that were made for the E command and exponential notation, there are also exceptions when specifying hexadecimal literals in a G-code program.

A hexadecimal literal must be delimited on both its left and right sides in order to prevent conflicts with an axis called either X or x that is directly followed by an integer value in G-code. The following examples show how hexadecimal notation and G-code are treated in various circumstances.

// G-code
X10

// Hexadecimal notation
$myVar = 0x10

// Move with Y = 0, X = 10
G1 Y0X10

// Move with Y = 0, X = 10
G1 Y0 X10

// Move with Y = 0x10 (16, no move on X)
G1 Y 0X10

// Move with Y = 0, X = 10
G1 Y 0 X 10

// Hexadecimal notation can be enforced by using delimiter characters
G1 Y(0X10)G1 Y=0X10