:lang: en
:toc:

[[cha:g-code-overview]]
= G-code Overview

:ini: {basebackend@docbook:'':ini}
:hal: {basebackend@docbook:'':hal}
:ngc: {basebackend@docbook:'':ngc}
// begin a listing of INI/HAL/NGC files like so:
//[source,{ini}]
//[source,{hal}]
//[source,{ngc}]

== Overview

The LinuxCNC G-code language is based on the RS274/NGC language.
The G-code language is based on lines of code.
Each line (also called a 'block') may include commands to do several different things.
Lines of code may be collected in a file to make a program.

A typical line of code consists of an optional line number at the
beginning followed by one or more 'words'. A word consists of a letter
followed by a number (or something that evaluates to a number). A word
may either give a command or provide an argument to a command. For
example, 'G1 X3' is a valid line of code with two words. 'G1' is a
command meaning 'move in a straight line at the programmed feed
rate to the programmed end point', and 'X3' provides an argument
value (the value of X should be 3 at the end of the move).
Most LinuxCNC G-code commands start with either G or M (for General and Miscellaneous).
The words for these commands are called 'G-codes' and 'M-codes'.
Also common are subroutine codes that begin with 'o-' which are called 'o-codes'.

The LinuxCNC language has no indicator for the start of a program. The
Interpreter, however, deals with files. A single program may be in a
single file, or a program may be spread across several files. A file
may demarcated with percents in the following way. The first non-blank
line of a file may contain nothing but a percent sign, '%', possibly
surrounded by white space, and later in the file (normally at the end
of the file) there may be a similar line. Demarcating a file with
percents is optional if the file has an 'M2' or 'M30' in it, but is
required if not. An error will be signaled if a file
has a percent line at the beginning but not at the end. The useful
contents of a file demarcated by percents stop after the second percent
line. Anything after that is ignored.

The LinuxCNC G-code language has two commands ('M2' or 'M30'), either of
which ends a program. A program may end before the end of
a file. Lines of a file that occur after the end of a program are not
to be executed. The interpreter does not even read them.

== Format of a line

A permissible line of input 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 block delete character, which is a slash '/'.
* 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. This makes some
strange-looking input legal. The line 'G0X +0. 12 34Y 7' is
equivalent to 'G0 x+0.1234 Y7', for example.

Blank lines are allowed in the input. They are to be ignored.

Input is case insensitive, except in comments, i.e., any letter
outside a comment may be in upper or lower case without changing the
meaning of a line.

[[sub:block-delete]]
=== '/': Block Delete((('/' Block Delete)))

The optional block delete character the slash '/' when placed first on a line
can be used by some user interfaces to skip lines of code when needed. In Axis
the key combination Alt-m-/ toggles block delete on and off. When block delete
is on any lines starting with the slash '/' are skipped.

In AXIS, it is also possible to enable block delete with the following icon:

.AXIS Block Delete Icon
image:../gui/images/tool_blockdelete.png[]

=== Line Number(((Line Number)))

A line number is the letter N followed by an unsigned integer,
optionally followed by a period and another unsigned integer. For
example, 'N1234' and 'N56.78' are valid line numbers. They may be
repeated or used out of order, although normal practice is to avoid
such usage. Line numbers may also be skipped, and that is normal
practice. A line number is not required to be used, but must be in the
proper place if used.

=== Word(((Words)))

A word is a letter other than N followed by a real value.

Words may begin with any of the letters shown in the following Table.
The table includes N for completeness, even
though, as defined above, line numbers are not words. Several letters
(I, J, K, L, P, R) may have different meanings in different contexts.
Letters which refer to axis names are not valid on a machine which does
not have the corresponding axis.

.Words and their meanings
[width="75%",options="header",cols="^1,<5"]
|===
|Letter | Meaning
|A | A axis of machine
|B | B axis of machine
|C | C axis of machine
|D | Tool radius compensation number
|F | Feed rate
|G | General function (See table  <<cap:modal-groups,G-code Modal Groups>>)
|H | Tool length offset index
|I | X offset for arcs and G87 canned cycles
|J | Y offset for arcs and G87 canned cycles
.2+|K | Z offset for arcs and G87 canned cycles.
<| Spindle-Motion Ratio for G33 synchronized movements.
|L | generic parameter word for G10, M66 and others
|M | Miscellaneous function (See table  <<tbl:mcodes-modal-groups,M-code Modal Groups>>)
|N | Line number
.2+|P | Dwell time in canned cycles and with G4.
<| Key used with G10.
|Q | Feed increment in G73, G83 canned cycles
|R | Arc radius or canned cycle plane
|S | Spindle speed
|T | Tool selection
|U | U axis of machine
|V | V axis of machine
|W | W axis of machine
|X | X axis of machine
|Y | Y axis of machine
|Z | Z axis of machine
|===

==== Parameters(((Parameters)))

Parameters are identified with a "#" symbol in front of them. See <<sec:overview-parameters,Parameters Section>> below. 

==== Subroutine Codes(((Subroutine Codes)))

Also called 'o-codes' these provide program flow control (such as if-else logic and callable subroutines) and are covered fully at the page on <<cha:o-codes,o-Codes>> and also below in <<sub:subroutine-parameters,Subroutine Codes and Parameters>>.

NOTE: o-codes are sometimes also called o-words. 

==== Comments(((Comments)))

Comments can be embedded in a line using parentheses () or for the remainder of a line using a semi-colon. There are also 'active' comments like MSG, DEBUG, etc. See the <<gcode:comments,section on comments>>.

=== End of Line Marker(((End of Line Marker)))

This is any combination of carriage return or line feed. 


[[gcode:numbers]]
=== Numbers(((Numbers)))

The following rules are used for (explicit) numbers. In these rules a
digit is a single character between 0 and 9.

* A number consists of:
** an optional plus or minus sign, followed by
** zero to many digits, followed, possibly, by
** one decimal point, followed by
** zero to many digits - provided that there is at least
   one digit somewhere in the number.
* There are two kinds of numbers:
** Integers, that does not have a decimal point,
** Decimals, that do have a decimal point.
* Numbers may have any number of digits, subject to the limitation on
  line length. Only about seventeen significant figures will be retained,
  however (enough for all known applications).
* A non-zero number with no sign but the first character is assumed to be
  positive.

Notice that initial (before the decimal point and the first non-zero
digit) and trailing (after the decimal point and the last non-zero
digit) zeros are allowed but not required. A number written with
initial or trailing zeros will have the same value when it is read as
if the extra zeros were not there.

Numbers used for specific purposes in RS274/NGC are often restricted
to some finite set of values or some to some range of values. In many
uses, decimal numbers must be close to integers; this includes the
values of indices (for parameters and carousel slot numbers, for
example), M-codes, and G-codes multiplied by ten. A decimal number
which is intended to represent an integer is considered close enough if
it is within 0.0001 of an integer value.

[[sec:overview-parameters]]
== Parameters(((Parameters)))

The RS274/NGC language supports 'parameters' - what in other
programming languages would be called 'variables'. There are several
types of parameter of different purpose and appearance, each described
in the following sections. The only value type supported by parameters
is floating-point; there are no string, boolean or integer types in
G-code like in other programming languages. However, logic expressions
can be formulated with <<gcode:binary-operators,boolean operators>>
( 'AND', 'OR', 'XOR', and the comparison operators
'EQ','NE','GT','GE','LT','LE'), and the 'MOD', 'ROUND', 'FUP' and
'FIX' <<gcode:functions,operators>> support integer arithmetic.

Parameters differ in syntax, scope, behavior when not yet
initialized, mode, persistence and intended use.

Syntax:: There are three kinds of syntactic appearance:
* 'numbered' - #4711
* 'named local' - #<localvalue>
* 'named global' - #<_globalvalue>

Scope:: The scope of a parameter is either global, or local within a
subroutine. Subroutine parameters and local named variables have local
scope. Global named parameters and numbered parameters starting from
number 31 are global in scope. RS274/NGC uses 'lexical scoping' -
in a subroutine only the local variables defined therein, and any
global variables are visible. The local variables of a
calling procedure are not visible in a called procedure.

Behavior of uninitialized parameters::
* Uninitialized global parameters, and unused subroutine parameters
  return the value zero when used in an expression.
* Uninitialized named parameters signal an error when used in an expression.

Mode:: Most parameters are read/write and may be assigned to
within an assignment statement. However, for many predefined
parameters this does not make sense, so they are are read-only - they
may appear in expressions, but not on the left-hand side of an
assignment statement.

Persistence:: When LinuxCNC is shut down, volatile parameters lose their
values. All parameters except numbered parameters in the current
persistent range footnoteref:[persistent_range,The range of persistent
parameters may change as development progresses. This range is
currently 5161- 5390. It is defined in the '_required_parameters array'
in file the src/emc/rs274ngc/interp_array.cc .]  are volatile.
Persistent parameters are saved in the .var file and
restored to their previous values when LinuxCNC is started again. Volatile
numbered parameters are reset to zero.

Intended Use::
* user parameters - numbered parameters in the range 31..5000, and named
  global and local parameters except predefined parameters. These are
  available for general-purpose storage of floating-point values, like
  intermediate results, flags etc, throughout program execution. They
  are read/write (can be assigned a value).
* <<sub:subroutine-parameters,subroutine parameters>> - these are used to
  hold the actual parameters passed to a subroutine.
* <<sub:numbered-parameters,numbered parameters>> - most of these are used
  to access offsets of coordinate systems.
* <<sub:system-parameters,system parameters>> - used to determine the current
  running version. They are read-only.

[[sub:numbered-parameters]]
=== Numbered Parameters(((Numbered Parameters)))

A numbered parameter is the pound character '#' followed by an
integer between 1 and (currently) 5602 footnote:[The RS274/NGC interpreter
maintains an array of numbered parameters. Its size is defined by the
symbol 'RS274NGC_MAX_PARAMETERS' in the file
src/emc/rs274ngc/interp_internal.hh). This number of numerical
parameters may also increase as development adds support for new
parameters.]. The parameter is referred
to by this integer, and its value is whatever number is stored in the
parameter.

A value is stored in a parameter with the = operator; for example:

----
#3 = 15 (set parameter 3 to 15)
----

A parameter setting does not take
effect until after all parameter values on the same line have been
found. For example, if parameter 3 has been previously set to 15 and
the line '#3=6 G1 X#3' is interpreted, a straight move to a point
where X equals 15 will
occur and the value of parameter 3 will be 6.

The '\#'  character takes precedence over other operations, so that, for
example, '\#1+2' means the number found by adding 2 to the value of
parameter 1, not
the value found in parameter 3. Of course, '\#[1+2]' does mean the
value found in parameter 3. The '\#' character may be repeated; for
example '##2'  means the value of the parameter whose index is the
(integer) value of parameter 2.

* '31-5000' - G-code user parameters. These parameters are global in the G
  code file, and available for general use. Volatile.
* '5061-5069' - Coordinates of a <<gcode:g38,G38>> probe result (X, Y,
  Z, A, B, C, U, V & W).  Coordinates are in the coordinate system in
  which the G38 took place.  Volatile.
* '5070' - <<gcode:g38,G38>> probe result: 1 if success, 0 if probe
  failed to close.  Used with G38.3 and G38.5. Volatile.
* '5161-5169' - "G28" Home for X, Y, Z, A, B, C, U, V & W. Persistent.
* '5181-5189' - "G30" Home for X, Y, Z, A, B, C, U, V & W. Persistent.
* '5210' - 1 if "G52" or "G92" offset is currently applied, 0
  otherwise.  Persistent by default; volatile if
  'DISABLE_G92_PERSISTENCE = 1' in the '[RS274NGC]' section of the
  INI file.
* '5211-5219' - Shared "G52" and "G92" offset for X, Y, Z, A, B, C, U,
  V & W.  Volatile by default; persistent if
  'DISABLE_G92_PERSISTENCE = 1' in the '[RS274NGC]' section of the
  INI file.
* '5220' - Coordinate System number 1 - 9 for G54 - G59.3. Persistent.
* '5221-5230' - Coordinate System 1, G54 for X, Y, Z, A, B, C, U, V, W & R.
  R denotes the XY rotation angle around the Z axis. Persistent.
* '5241-5250' - Coordinate System 2, G55 for X, Y, Z, A, B, C, U, V, W & R.
  Persistent.
* '5261-5270' - Coordinate System 3, G56 for X, Y, Z, A, B, C, U, V, W & R.
  Persistent.
* '5281-5290' - Coordinate System 4, G57 for X, Y, Z, A, B, C, U, V, W & R.
  Persistent.
* '5301-5310' - Coordinate System 5, G58 for X, Y, Z, A, B, C, U, V, W & R.
  Persistent.
* '5321-5330' - Coordinate System 6, G59 for X, Y, Z, A, B, C, U, V, W & R.
  Persistent.
* '5341-5350' - Coordinate System 7, G59.1 for X, Y, Z, A, B, C, U, V, W & R.
  Persistent.
* '5361-5370' - Coordinate System 8, G59.2 for X, Y, Z, A, B, C, U, V, W & R.
  Persistent.
* '5381-5390' - Coordinate System 9, G59.3 for X, Y, Z, A, B, C, U, V, W & R.
  Persistent.
* '5399' - Result of M66 - Check or wait for input. Volatile.
* '5400' - Tool Number. Volatile.
* '5401-5409' - Tool Offsets for X, Y, Z, A, B, C, U, V & W. Set by G43. Volatile.
* '5410' - Tool Diameter. Volatile.
* '5411' - Tool Front Angle. Volatile.
* '5412' - Tool Back Angle. Volatile.
* '5413' - Tool Orientation. Volatile.
* '5420-5428' - Current relative position in the active coordinate system
  including all offsets and in the current program units for
  X, Y, Z, A, B, C, U, V & W, volatile.
* '5599' - Flag for controlling the output of (DEBUG,) statements.
  1=output, 0=no output; default=1. Volatile.
* '5600' - Toolchanger fault indicator. Used with the iocontrol-v2 component.
  1: toolchanger faulted, 0: normal. Volatile.
* '5601' - Toolchanger fault code. Used with the iocontrol-v2 component.
  Reflects the value of the 'toolchanger-reason' HAL pin if a fault occurred.
  Volatile.

.Numbered Parameters Persistence
The values of parameters in the persistent range are retained over
time, even if the machining center is powered down. LinuxCNC uses a
parameter file to ensure persistence. It is managed by the
Interpreter. The Interpreter reads the file when it starts up, and
writes the file when it exits.

The format of a parameter file is shown in Table
<<gcode:format-parameter-file,Parameter File Format>>.

The Interpreter expects the file to have two columns. It skips any
lines which do not contain exactly two numeric values. The first
column is expected to contain an integer value (the parameter's
number). The second column contains a floating point number (this
parameter's last value). The value is represented as a
double-precision floating point number inside the Interpreter, but a
decimal point is not required in the file.

Parameters in the user-defined range (31-5000) may be added to this
file. Such parameters will be read by the Interpreter and written to
the file as it exits.

Missing Parameters in the persistent range will be initialized to zero
and written with their current values on the next save operation.

The parameter numbers must be arranged in ascending order. An
'Parameter file out of order' error  will be signaled if they are  not in
ascending order.

The original file is saved as a backup file when the new file
is written.

[[gcode:format-parameter-file]]
.Parameter File Format
[width="90%",options="header"]
|===
|Parameter Number | Parameter Value
|5161 | 0.0
|5162 | 0.0
|===

[[sub:subroutine-parameters]]
=== Subroutine Parameters(((Subroutine Parameters)))

* '1-30' Subroutine local parameters of call arguments. These parameters are
  local to the subroutine. Volatile. See also the chapter on
  <<cha:o-codes,O-Codes>>.

[[gcode:named-parameters]]
=== Named Parameters(((Named Parameters)))

Named parameters work like numbered parameters but are easier to read.
All parameter names are converted to lower case and have spaces and
tabs removed, so '#<param>' and '#<P a R am >' refer to the same
parameter. Named parameters must be enclosed with '< >' marks.

'#<named parameter>'  is a local named parameter. By default, a
named parameter is local to the scope in which it is assigned. You can't
access a local parameter outside of its subroutine. This means that two
subroutines can use the same parameter names without fear of one subroutine
overwriting the values in another.

'#<_global named parameter>'  is a global named parameter. They
are accessible from within called subroutines and may set values within
subroutines that are accessible to the caller. As far as scope is concerned,
they act just like regular numeric parameters. They are not stored in files.

Examples:

.Declaration of named global variable
----
#<_endmill_dia> = 0.049
----

.Reference to previously declared global variable
----
#<_endmill_rad> = [#<_endmill_dia>/2.0]
----

.Mixed literal and named parameters
----
o100 call [0.0] [0.0] [#<_inside_cutout>-#<_endmill_dia>] [#<_Zcut>] [#<_feedrate>]
----

Named parameters spring into existence when they are assigned a value
for the first time. Local named parameters vanish when their scope is
left: when a subroutine returns, all its local parameters are deleted
and cannot be referred to anymore.

It is an error to use a non-existent named parameter within an
expression, or at the right-hand side of an assignment. Printing the
value of a non-existent named parameter with a DEBUG statement - like
'(DEBUG, #<no_such_parameter>)' will display the string '######'.

Global parameters, as well as local parameters assigned to at the
global level, retain their value once assigned even when the program
ends, and have these  values when the program is run again.

The <<gcode:functions,'EXISTS' function>> tests whether a given named parameter exists.

[[gcode:predefined-named-parameters]]
=== Predefined Named Parameters(((Predefined Named Parameters)))

The following global read only named parameters are available to
access internal state of the interpreter and machine state. They can
be used in arbitrary expressions, for instance to control flow of the
program with if-then-else statements. Note that new
<<remap:adding-predefined-named-parameters,predefined named parameters>>
can be added easily without changes to the source code.

* '#<_vmajor>' - Major package version. If current version was 2.5.2 would return 2.5.
* '#<_vminor>' - Minor package version. If current version was 2.6.2 it would return 0.2.
* '#<_line>' - Sequence number. If running a G-code file, this returns the current line number.
* '#<_motion_mode>' - Return the interpreter's current motion mode:

[width="20%",options="header"]
|===
|Motion mode | return value
|      G1    | 10
|      G2    | 20
|      G3    | 30
|      G33   | 330
|      G38.2 | 382
|      G38.3 | 383
|      G38.4 | 384
|      G38.5 | 385
|      G5.2  | 52
|      G73   | 730
|      G76   | 760
|      G80   | 800
|      G81   | 810
|      G82   | 820
|      G83   | 830
|      G84   | 840
|      G85   | 850
|      G86   | 860
|      G87   | 870
|      G88   | 880
|      G89   | 890
|===

* '#<_plane>' - returns the value designating the current plane:

[width="20%",options="header"]
|===
| Plane | return value
| G17   | 170
| G18   | 180
| G19   | 190
| G17.1 | 171
| G18.1 | 181
| G19.1 | 191
|===

* '#<_ccomp>' - Status of cutter compensation. Return values:

[width="20%",options="header"]
|===
| Mode  | return value
| G40   | 400
| G41   | 410
| G41.1 | 411
| G41   | 410
| G42   | 420
| G42.1 | 421
|===

* '#<_metric>' - Return 1 if G21 is on, else 0.
* '#<_imperial>' - Return 1 if G20 is on, else 0.
* '#<_absolute>' - Return 1 if G90 is on, else 0.
* '#<_incremental>' - Return 1 if G91 is on, else 0.
* '#<_inverse_time>' - Return 1 if inverse feed mode (G93) is on, else 0.
* '#<_units_per_minute>' - Return 1 if Units/minute feed mode (G94) is on, else 0.
* '#<_units_per_rev>' - Return 1 if Units/revolution mode (G95) is on, else 0.
* '#<_coord_system>' - Return a float of the current coordinate system name (G54..G59.3).
  For example if your in G55 coordinate system the return value is
  550.000000 and if your in G59.1 the return value is 591.000000.

[width="20%",options="header"]
|===
| Mode  | return value
| G54   | 540
| G55   | 550
| G56   | 560
| G57   | 570
| G58   | 580
| G59   | 590
| G59.1 | 591
| G59.2 | 592
| G59.3 | 593
|===

* '#<_tool_offset>' - Return 1 if tool offset (G43) is on, else 0.
* '#<_retract_r_plane>' - Return 1 if G98 is set, else 0.
* '#<_retract_old_z>' - Return 1 if G99 is on, else 0.

[[sub:system-parameters]]
=== System Parameters(((System Parameters)))

* '#<_spindle_rpm_mode>' - Return 1 if spindle rpm mode (G97) is on, else 0.
* '#<_spindle_css_mode>' - Return 1 if constant surface speed mode (G96) is on, else 0.
* '#<_ijk_absolute_mode>' - Return 1 if Absolute Arc distance mode (G90.1) is on, else 0.
* '#<_lathe_diameter_mode>' - Return 1 if this is a lathe configuration and diameter (G7) mode is on, else 0.
* '#<_lathe_radius_mode>' - Return 1 if this is a lathe configuration and radius (G8) mode is on, else 0.
* '#<_spindle_on>' - Return 1 if spindle currently running (M3 or M4) else 0.
* '#<_spindle_cw>' - Return 1 if spindle direction is clockwise (M3) else 0.
* '#<_mist>' - Return 1 if mist (M7) is on.
* '#<_flood>' - Return 1 if flood (M8) is on.
* '#<_speed_override>' - Return 1 if feed override (M48 or M50 P1) is on, else 0.
* '#<_feed_override>' - Return 1 if feed override (M48 or M51 P1) is on, else 0.
* '#<_adaptive_feed>' - Return 1 if adaptive feed (M52 or M52 P1) is on, else 0.
* '#<_feed_hold>' - Return 1 if feed hold switch is enabled (M53 P1), else 0.
* '#<_feed>' - Return the current value of F, not the actual feed rate.
* '#<_rpm>' - Return the current value of S, not the actual spindle speed.
* '#<_x>' - Return current relative X coordinate including all offsets. Same as #5420.
  In a lathe configuration, it always returns radius.
* '#<_y>' - Return current relative Y coordinate including all offsets. Same as #5421.
* '#<_z>' - Return current relative Z coordinate including all offsets. Same as #5422.
* '#<_a>' - Return current relative A coordinate including all offsets. Same as #5423.
* '#<_b>' - Return current relative B coordinate including all offsets. Same as #5424.
* '#<_c>' - Return current relative C coordinate including all offsets. Same as #5425.
* '#<_u>' - Return current relative U coordinate including all offsets. Same as #5426.
* '#<_v>' - Return current relative V coordinate including all offsets. Same as #5427.
* '#<_w>' - Return current relative W coordinate including all offsets. Same as #5428.
* '#<_abs_x>' - Return current absolute X coordinate (G53) including no offsets.
* '#<_abs_y>' - Return current absolute Y coordinate (G53) including no offsets.
* '#<_abs_z>' - Return current absolute Z coordinate (G53) including no offsets.
* '#<_abs_a>' - Return current absolute A coordinate (G53) including no offsets.
* '#<_abs_b>' - Return current absolute B coordinate (G53) including no offsets.
* '#<_abs_c>' - Return current absolute C coordinate (G53) including no offsets.
* '#<_current_tool>' - Return number of the current tool in spindle. Same as #5400.
* '#<_current_pocket>' - Return the tooldata index for the current tool.
* '#<_selected_tool>' - Return number of the selected tool post a T code. Default -1.
* '#<_selected_pocket>' - Return the tooldata index of the selected pocket post a T code.
  Default -1 (no pocket selected).
* '#<_value>' - Return value from the last O-word 'return' or 'endsub'. Default
  value 0 if no expression after 'return' or 'endsub'. Initialized
  to 0 on program start.
* '#<_value_returned>' - 1.0 if the last O-word 'return' or 'endsub' returned a value, 0
  otherwise. Cleared by the next O-word call.
* '#<_task>' - 1.0 if the executing interpreter instance is part of milltask, 0.0
  otherwise. Sometimes it is necessary to treat this case specially
  to retain proper preview, for instance when testing the success of
  a probe (G38.n) by inspecting #5070, which will always fail in the
  preview interpreter (e.g. Axis).
* '#<_call_level>' - current nesting level of O-word procedures. For debugging.
* '#<_remap_level>' - current level of the remap stack. Each remap in a block adds one
  to the remap level. For debugging.

[[gcode:ini-hal-params]]
== HAL pins and INI values(((HAL pins and INI values)))

If enabled in the <<sub:ini:sec:rs274ngc, INI file>> G-code has access
to the values of INI file entries and HAL pins.

* '#<_ini[section]name>' Returns the value of the corresponding item in
  the INI file.

For example, if the INI file looks like so:

[source,{ini}]
---------------------------------------------------------------------
[SETUP]
XPOS = 3.145
YPOS = 2.718
---------------------------------------------------------------------

you may refer to the named parameters `#<_ini[setup]xpos>` and
`#<_ini[setup]ypos>` within G-code.

`EXISTS` can be used to test for presence of a given INI file
variable:

[source,{ngc}]
---------------------------------------------------------------------
o100 if [EXISTS[#<_ini[setup]xpos>]]
  (debug, [setup]xpos exists: #<_ini[setup]xpos>)
o100 else
  (debug, [setup]xpos does not exist)
o100 endif
---------------------------------------------------------------------

The value is read from the INI file once, and cached in the
interpreter. These parameters are read-only - assigning a value will
cause a runtime error. In the G-code the names are not case sensitive - they are
converted to uppercase before consulting the INI file. Hence INI entries that
contain lowercase characters can not be accessed from G-code.

* '#<_hal[HAL item]>'
  Allows G-code programs to read the values of HAL pins Variable access is
  read-only, the only way to _set_ HAL pins from G-code remains M62-M65,
  M67, M68 and custom M100-M199 codes.
  Note that the value read will not update in real-time, typically the
  value that was on the pin when the G-code program was started will be
  returned. It is possible to work round this by forcing a state synch.
  One way to do this is with a dummy M66 command: M66E0L0

Example:

[source,{ngc}]
---------------------------------------------------------------------
(debug, #<_hal[motion-controller.time]>)
---------------------------------------------------------------------

Access of HAL items is read-only. Currently, only all-lowercase HAL
names can be accessed this way.

`EXISTS` can be used to test for the presence of a given HAL item:

[source,{ngc}]
---------------------------------------------------------------------
o100 if [EXISTS[#<_hal[motion-controller.time]>]]
  (debug, [motion-controller.time] exists: #<_hal[motion-controller.time]>)
o100 else
  (debug, [motion-controller.time] does not exist)
o100 endif
---------------------------------------------------------------------

This feature was motivated by the desire for stronger coupling between
user interface components like `GladeVCP` and `PyVCP` to act as
parameter source for driving NGC file behavior. The alternative -
going through the M6x pins and wiring them - has a limited,
non-mnemonic namespace and is unnecessarily cumbersome just as a
UI/Interpreter communications mechanism.

[[gcode:expressions]]
== Expressions(((Expressions)))

An expression is a set of characters starting with a left bracket '['
and ending with a balancing right bracket ']' . In between the brackets
are numbers, parameter values, mathematical
operations, and other expressions. An expression is evaluated to
produce a number. The expressions on a line are evaluated when the line
is read, before anything on the line is executed. An example of an
expression is '[1 + acos[0] - [#3 ** [4.0/2]]]'.

[[gcode:binary-operators]]
== Binary Operators(((Binary Operators)))

Binary operators only appear inside expressions. There are four basic
mathematical operations: addition ('+'), subtraction ('-'),
multiplication ('\*'), and division ('/'). There are three logical
operations: non-exclusive or ('OR'), exclusive or ('XOR'), and logical
and ('AND'). The eighth operation is the modulus operation ('MOD'). The
ninth operation is the 'power' operation ('**') of raising the number
on the left of the operation to the power on
the right. The relational operators are equality ('EQ'), inequality
('NE'), strictly greater than ('GT'), greater than or equal to ('GE'),
strictly less than ('LT'), and less than or equal to ('LE').

The binary operations are divided into several groups according to their
precedence. If operations in different precedence groups are strung together
(for example in the expression '[2.0 / 3 * 1.5 - 5.5 / 11.0]'), operations
in a higher group are to be performed before operations
in a lower group. If an expression contains more than one operation
from the same group (such as the first '/' and '*'  in the example),
the operation on the left is performed first. Thus,
the example is equivalent to: '[ [ [2.0 / 3] * 1.5] - [5.5 / 11.0] ]' ,
which is equivalent to to '[1.0 - 0.5]' , which is '0.5'.

The logical operations and modulus are to be performed on any real
numbers, not just on integers. The number zero is equivalent to logical
false, and any non-zero number is equivalent to logical true.

[[gcode:operators-precedence]]
.Operators Precedence(((Operators Precedence)))
[width="60%",options="header",cols="2*^"]
|===
|Operators         | Precedence
|**                | 'highest'
|* / MOD           |
|+ -               |
|EQ NE GT GE LT LE |
|AND OR XOR        | 'lowest'
|===

== Equality and floating-point values

Testing for equality or inequality of two
double-precision floating-point values is inherently problematic.
The interpreter solves this problem by considering values equal if
their absolute difference is less than 1e-6 (this value is defined as
'TOLERANCE_EQUAL' in src/emc/rs274ngc/interp_internal.hh).

[[gcode:functions]]
== Functions(((Functions)))(((Unary operations)))

The available functions are shown in following table. Arguments to unary
operations which take angle measures ('COS', 'SIN', and 'TAN' ) are in
degrees. Values returned by unary operations which return angle measures
('ACOS', 'ASIN', and 'ATAN') are also in degrees.

.G-code Functions
[width="75%",options="header",cols="^,<"]
|===
|Function Name    | Function result
|ATAN[arg]/[arg]  | Four quadrant inverse tangent
|ABS[arg]         | Absolute value
|ACOS[arg]        | Inverse cosine
|ASIN[arg]        | Inverse sine
|COS[arg]         | Cosine
|EXP[arg]         | e raised to the given power
|FIX[arg]         | Round down to integer
|FUP[arg]         | Round up to integer
|ROUND[arg]       | Round to nearest integer
|LN[arg]          | Base-e logarithm
|SIN[arg]         | Sine
|SQRT[arg]        | Square Root
|TAN[arg]         | Tangent
|EXISTS[arg]      | Check named Parameter
|===

The 'FIX' function rounds towards the left (less positive or more negative)
on a number line, so that 'FIX[2.8] =2' and 'FIX[-2.8] = -3'.

The 'FUP'  operation rounds towards the right (more positive or less
negative) on a number line; 'FUP[2.8] = 3' and 'FUP[-2.8] = -2'.

The 'EXISTS' function checks for the existence of a single named parameter.
It takes only one named parameter and returns 1 if it exists and 0 if it does
not exist. It is an error if you use a numbered parameter or an expression.
Here is an example for the usage of the EXISTS function:

[source,{ngc}]
----
o<test> sub
o10 if [EXISTS[#<_global>]]
    (debug, _global exists and has the value #<_global>)
o10 else
    (debug, _global does not exist)
o10 endif
o<test> endsub

o<test> call
#<_global> = 4711
o<test> call
m2
----

== Repeated Items

A line may have any number of G words, but two G words from the same
modal group may not appear on the same line.
See the <<gcode:modal-groups,Modal Groups>> section for more information.

A line may have zero to four M words. Two M words from the same modal
group may not appear on the same line.

For all other legal letters, a line may have only one word beginning
with that letter.

If a parameter setting of the same parameter is repeated on a line,
'#3=15 #3=6', for example, only the last setting will take effect.
It is silly,
but not illegal, to set the same parameter twice on the same line.

If more than one comment appears on a line, only the last one will be
used; each of the other comments will be read and its format will be
checked, but it will be ignored thereafter. It is expected that putting
more than one comment on a line will be very rare.

== Item order

The three types of item whose order may vary on a line (as given at
the beginning of this section) are word, parameter setting, and
comment. Imagine that these three types of item are divided into three
groups by type.

The first group (the words) may be reordered in any way without
changing the meaning of the line.

If the second group (the parameter settings) is reordered, there will
be no change in the meaning of the line unless the same parameter is
set more than once. In this case, only the last setting of the
parameter will take effect. For example, after the line '#3=15 #3=6'
has been interpreted, the value of parameter 3 will be 6. If the
order is reversed to '#3=6 #3=15' and the line is interpreted, the
value of parameter 3 will be 15.

If the third group (the comments) contains more than one comment and
is reordered, only the last comment will be used.

If each group is kept in order or reordered without changing the
meaning of the line, then the three groups may be interleaved in any
way without changing the meaning of the line. For example, the line
'g40 g1 #3=15 (foo) #4=-7.0' has five items and means exactly the
same thing in any of the 120
possible orders (such as '#4=-7.0 g1 #3=15 g40 (foo)') for the five
items.

== Commands and Machine Modes

Many commands cause the controller to change from one mode to another,
and the mode stays active until some other command changes it
implicitly or explicitly. Such commands are called 'modal'. For
example, if coolant is turned on, it stays on until it is explicitly
turned off. The G-codes for motion are also modal. If a G1 (straight
move) command is given on one line, for example, it will be executed
again on the next line if one or more axis words is available on the
line, unless an explicit command is given on that next line using the
axis words or canceling motion.

'Non-modal' codes have effect only on the lines on which they occur.
For example, G4 (dwell) is non-modal.

[[gcode:polar-coordinates]]
== Polar Coordinates(((Polar Coordinates)))

Polar Coordinates can be used to specify the XY coordinate of a move.
The @n is the distance and ^n is the angle. The advantage of this is
for things like bolt hole circles which can be done very simply by
moving to a point in the center of the circle, setting the offset and
then moving out to the first hole then run the drill cycle.
Polar Coordinates always are from the current XY zero position.
To shift the Polar Coordinates from machine zero use an offset
or select a coordinate system.

In Absolute Mode the distance and angle is from the XY zero position
and the angle starts with 0 on the X Positive axis and increases in a CCW
direction about the Z axis. The code G1 @1^90 is the same as G1 Y1.

In Relative Mode the distance and angle is also from the XY zero
position but it is cumulative.
This can be confusing at first how this works in incremental mode.

For example if you have the following program you might expect it to
be a square pattern:

[source,{ngc}]
----
F100 G1 @.5 ^90
G91 @.5 ^90
@.5 ^90
@.5 ^90
@.5 ^90
G90 G0 X0 Y0 M2
----

You can see from the following figure that the output is not what you
might expect. Because we added 0.5 to the distance each time the
distance from the XY zero position increased with each line.

[[fig:polar-spiral]]
.Polar Spiral
image::images/polar01.png["Polar Spiral",align="center"]

The following code will produce our square pattern:

[source,{ngc}]
----
F100 G1 @.5 ^90
G91 ^90
^90
^90
^90
G90 G0 X0 Y0 M2
----

As you can see by only adding to the angle by 90 degrees each time the
end point distance is the same for each line.

[[fig:polar-square]]
.Polar Square
image::images/polar02.png["Polar Square",align="center"]

It is an error if:

* An incremental move is started at the origin
* A mix of Polar and X or Y words are used

[[gcode:modal-groups]]
== Modal Groups(((Modal Groups)))

Modal commands are arranged in sets called 'modal groups', and only
one member of a modal group may be in force at any given time. In
general, a modal group contains commands for which it is logically
impossible for two members to be in effect at the same time - like
measure in inches vs. measure in millimeters. A machining center may be
in many modes at the same time, with one mode from each modal group
being in effect. The modal groups are shown in the following Table.

[[cap:modal-groups]]
.G-code Modal Groups(((Modal Groups: G-codes)))
[width="80%",cols="4,6",options="header"]
|===
|Modal Group Meaning                    | Member Words
|Non-modal codes (Group 0)              | G4, G10 G28, G30, G52, G53, G92, G92.1, G92.2, G92.3,
|Motion (Group 1)                       | G0, G1, G2, G3, G33, G38.n, G73, G76, G80, G81
                                          G82, G83, G84, G85, G86, G87, G88, G89
|Plane selection (Group 2)              | G17, G18, G19, G17.1, G18.1, G19.1
|Distance Mode (Group 3)                | G90, G91
|Arc IJK Distance Mode (Group 4)        | G90.1, G91.1
|Feed Rate Mode (Group 5)               | G93, G94, G95
|Units (Group 6)                        | G20, G21
|Cutter Diameter Compensation (Group 7) | G40, G41, G42, G41.1, G42.1
|Tool Length Offset (Group 8)           | G43, G43.1, G49
|Canned Cycles Return Mode (Group 10)   | G98, G99
|Coordinate System (Group 12)           | G54, G55, G56, G57, G58, G59, G59.1, G59.2, G59.3
|Control Mode (Group 13)                | G61, G61.1, G64
|Spindle Speed Mode (Group 14)          | G96, G97
|Lathe Diameter Mode (Group 15)         | G7, G8
|===

[[tbl:mcodes-modal-groups]]
.M-code Modal Groups(((Modal Groups: M-codes)))
[width="80%",cols="4,6",options="header"]
|===
|Modal Group Meaning         | Member Words
|Stopping (Group 4)          | M0, M1, M2, M30, M60
|I/O Pins (Group 5)          | (M62-M65 digital output), (M66 digital or analog input),
                               (M67, M68 analog output)
|Toolchange (Group 6)        | M6 T__n__
|Spindle (Group 7)           | M3, M4, M5
|Coolant (Group 8)           | (M7 M8 can both be on), M9
|Override Switches (Group 9) | M48, M49
|User Defined (Group 10)     | M100-M199
|===

For several modal groups, when a machining center is ready to accept
commands, one member of the group must be in effect. There are default
settings for these modal groups. When the machining center is turned on
or otherwise re-initialized, the default values are automatically in
effect.

Group 1, the first group on the table, is a group of G-codes for
motion. One of these is always in effect. That one is called the
current motion mode.

It is an error to put a G-code from group 1 and a G-code from group 0
on the same line if both of them use axis words. If an axis word-using
G-code from group 1 is implicitly in effect on a line (by having been
activated on an earlier line), and a group 0 G-code that uses axis
words appears on the line, the activity of the group 1 G-code is
suspended for that line. The axis word-using G-codes from group 0 are
G10, G28, G30, G52 and G92.

It is an error to include any unrelated words on a line with 'O-' flow
control.

[[gcode:comments]]
== Comments(((Comments)))

Comments are purely informative and have no influence on machine behaviour.

Comments can be added to lines of G-code to help clear up the
intention of the programmer. Comments can be embedded in a line using
parentheses () or for the remainder of a line using a semi-colon. The
semi-colon is not treated as the start of a comment when enclosed in
parentheses.

Comments may appear between words, but not between words and their
corresponding parameter. So, 'S100(set speed)F200(feed)' is OK while
'S(speed)100F(feed)' is not.

Here is an example of a commented program:

[source,{ngc}]
----
G0 (Rapid to start) X1 Y1
G0 X1 Y1 (Rapid to start; but don't forget the coolant)
M2 ; End of program.
----

There are several 'active' comments which look like comments but cause
some action, like '(debug,..)' or '(print,..)'. If there are
several comments on a line, only the last comment will be interpreted
according to these rules. Hence, a normal comment following an active
comment will in effect disable the active comment. For example, '(foo)
(debug,#1)' will print the value of parameter '#1', however
'(debug,#1)(foo)' will not.

A comment introduced by a semicolon is by definition the last comment
on that line, and will always be interpreted for active comment syntax.

NOTE: Inline comments on O-words should not be used see the O-code
<<ocode:comments,comments>> section for more information.

[[gcode:messages]]
== Messages(((Messages)))

* '(MSG,)' - displays message if 'MSG' appears after the left parenthesis
  and before any other printing characters. Variants of 'MSG' which include
  white space and lower case characters are allowed. The rest of the
  characters before the right parenthesis are considered to be a message.
  Messages should be displayed on the message display device of the user
  interface if provided.

.Message Example
----
(MSG, This is a message)
----

[[gcode:probe-logging]]
== Probe Logging(((Probe Logging)))

* '(PROBEOPEN filename.txt)' - will open filename.txt and store the 9-number
  coordinate consisting of XYZABCUVW of each successful straight probe in it.
* '(PROBECLOSE)' - will close the open probelog file.

For more information on probing see the <<gcode:g38,G38>> section.

[[gcode:logging]]
== Logging(((Logging)))

* '(LOGOPEN,filename.txt)' - opens the named log file. If the file already
  exists, it is truncated.
* '(LOGAPPEND,filename)' - opens the named log file. If the file already
  exists, the data is appended.
* '(LOGCLOSE)' - closes an open log file.
* '(LOG,)' - everything past the ',' is written to the log file if it is open.
  Supports expansion of parameters as described below.

Examples of logging are in 'nc_files/examples/smartprobe.ngc' and in
'nc_files/ngcgui_lib/rectange_probe.ngc' sample G-code files.

[[gcode:debug]]
== Debug Messages(((Debug Messages)))

* '(DEBUG,)' - displays a message like '(MSG,)' with the addition of special
  handling for comment parameters as described below.

[[gcode:print]]
== Print Messages(((Print Messages)))

* '(PRINT,)' - messages are output to 'stderr' with special handling for
  comment parameters as described below.

[[gcode:comment-parameters]]
== Comment Parameters(((Comment Parameters)))

In the DEBUG, PRINT and LOG comments, the values of parameters in the
message are expanded.

For example: to print a named global variable to stderr (the default
console window).

.Parameters Example
----
(print,endmill dia = #<_endmill_dia>)
(print,value of variable 123 is: #123)
----

Inside the above types of comments, sequences like '\#123' are replaced
by the value of the parameter 123. Sequences like '\#<named parameter>'
are replaced by the value of the named parameter. Named parameters
will have white space removed from them. So, '\#<named parameter>'
will be converted to '#<namedparameter>'.

Parameter numbers can be formatted, e.g.:

----
(DEBUG, value = %d#<some_value>)
----
will print the value rounded to an integer.

* %lf is default if there is no formatting string.
* %d = 0 decimals
* %f = four decimals
* %.xf = x (0-9) number of decimals

The formatting will be performed on all parameters in the same line unless
changed, i.e., multiple formatting is allowed in one line.

The formatting string does not need to be right beside the parameter.

If the formatting string is created with the wrong pattern it will be
printed as characters.

[[gcode:file-requirements]]
== File Requirements(((File Requirements)))

A G-code file must contain one or more lines of G-code and be terminated
with a <<mcode:m2-m30,Program End>>. Any G-code past the program end
is not evaluated.

If a program end code is not used a pair of percent signs '%' with the first
percent sign on the first line of the file followed by one or more lines of
G-code and a second percent sign. Any code past the second percent sign is not
evaluated.

[WARNING]
Using % to wrap a G-code file will not do the same thing as using a program
end. The machine will be in what ever state the program left it in using %,
the spindle and coolant may still be on and things like G90/91 are left as the
last program set them. If you don't use a proper preamble the next program
could start in a dangerous condition.

[NOTE]
The file must be created with a text editor like Gedit and not a word
processor like Open Office Word Processor.

[[gcode:file-size]]
== File Size(((File Size)))

The interpreter and task are carefully written so that the only limit
on part program size is disk capacity. The TkLinuxCNC and Axis interface
both load the program text to display it to the user, though, so RAM
becomes a limiting factor. In Axis, because the preview plot is drawn
by default, the redraw time also becomes a practical limit on program
size. The preview can be turned off in Axis to speed up loading large
part programs. In Axis sections of the preview can be turned off using
<<axis:preview-control,preview control>> comments.

[[gcode:order-of-execution]]
== G-code Order of Execution(((G-code Order of Execution)))

The order of execution of items on a line is defined not by the
position of each item on the line, but by the following list:

* O-word commands (optionally followed by a comment but no other words allowed
  on the same line)
* Comment (including message)
* Set feed rate mode (G93, G94).
* Set feed rate (F).
* Set spindle speed (S).
* Select tool (T).
* HAL pin I/O (M62-M68).
* Change tool (M6) and Set Tool Number (M61).
* Spindle on or off (M3, M4, M5).
* Save State (M70, M73), Restore State (M72), Invalidate State (M71).
* Coolant on or off (M7, M8, M9).
* Enable or disable overrides (M48, M49,M50,M51,M52,M53).
* User-defined Commands (M100-M199).
* Dwell (G4).
* Set active plane (G17, G18, G19).
* Set length units (G20, G21).
* Cutter radius compensation on or off (G40, G41, G42)
* Cutter length compensation on or off (G43, G49)
* Coordinate system selection (G54, G55, G56, G57, G58, G59, G59.1, G59.2, G59.3).
* Set path control mode (G61, G61.1, G64)
* Set distance mode (G90, G91).
* Set retract mode (G98, G99).
* Go to reference location (G28, G30) or change coordinate system
  data (G10) or set axis offsets (G52, G92, G92.1, G92.2, G94).
* Perform motion (G0 to G3, G33, G38.n, G73, G76, G80 to G89), as modified
  (possibly) by G53.
* Stop (M0, M1, M2, M30, M60).

[[gcode:best-practices]]
== G-code Best Practices(((G-code Best Practices)))

.Use an appropriate decimal precision
Use at least 3 digits after the decimal when milling in millimeters,
and at least 4 digits after the decimal when milling in inches.

In particular, tolerance checks of arcs are done for .001 and .0001
according to the active units.

.Use consistent white space
G-code is most legible when at least one space appears before words.
While it is permitted to insert white space in the middle of numbers,
there is no reason to do so.

.Use Center-format arcs
Center-format arcs (which use 'I- J- K-' instead of 'R-' ) behave more
consistently than R-format arcs, particularly for
included angles near 180 or 360 degrees.

.Use a Preamble set modal groups
When correct execution of your program depends on modal settings, be
sure to set them at the beginning of the part program. Modes can carry
over from previous programs and from the MDI commands.

.Example Preamble for a Mill

[source,{ngc}]
----
G17 G20 G40 G49 G54 G80 G90 G94
----

G17 use XY plane, G20 inch mode, G40 cancel diameter compensation,
G49 cancel length offset, G54 use coordinate system 1, G80 cancel canned
cycles, G90 absolute distance mode, G94 feed/minute mode.

Perhaps the most critical modal setting is the distance units--If you
do not include G20 or G21, then different machines will mill the
program at different scales. Other settings, such as the return mode in
canned cycles may also be important.

.Don't put too many things on one line
Ignore everything in section <<gcode:order-of-execution,Order of Execution>>, and instead
write no line of code that is the slightest bit ambiguous.

.Don't set & use a parameter on the same line
Don't use and set a parameter on the same line, even though the
semantics are well defined. Updating a variable to a new value, such as
'#1=[#1+#2]' is OK.

.Don't use line numbers
Line numbers offer no benefits. When line numbers are reported in
error messages, the numbers refer to the line number in the file, not
the N-word value.

.When several coordinate systems are moved

Consider using the inverse time speed mode.

Because the meaning of an 'F' word in meters per minute varies depending on
the type of axis to be moved and because the amount of removed material does
not depend only on the feed rate, it can be simpler to use G93, inverse
speed of time, to achieve the removal of desired material.

== Linear and Rotary Axis

Because the meaning of an F-word in feed-per-minute mode varies
depending on which axes are commanded to move, and because the amount
of material removed does not depend only on the feed rate, it may be
easier to use G93 inverse time feed mode to achieve the desired
material removal rate.

== Common Error Messages

* 'G-code out of range' - A G-code greater than G99 was used, the scope of G
  codes in LinuxCNC is 0 - 99. Not every number between 0 and 99 is a valid
  G-code.
* 'Unknown G-code used' - A G-code was used that is not part of the LinuxCNC
  G-code language.
* 'i,j,k word with no Gx to use it' - i, j and k words must be used on the same
  line as the G-code.
* 'Cannot use axis values without a G-code that uses them' - Axis values can
  not be used on a line without either a modal G-code in effect or a G-code
  on the same line.
* 'File ended with no percent sign or program end' - Every G-code file must
  end in a M2 or M30 or be wrapped with the percent sign %.

// vim: set syntax=asciidoc:
