diff --git a/PythonicGcodeMachine/Gcode/Fanuc/__init__.py b/PythonicGcodeMachine/Gcode/Fanuc/__init__.py
new file mode 100644
index 0000000000000000000000000000000000000000..37fdd45a0d6bed35fad763c9e5dbb87020fe76cb
--- /dev/null
+++ b/PythonicGcodeMachine/Gcode/Fanuc/__init__.py
@@ -0,0 +1,384 @@
+####################################################################################################
+#
+# PythonicGcodeMachine - @licence_header_description@
+# Copyright (C) 2018 Fabrice Salvaire
+#
+# This program is free software: you can redistribute it and/or modify
+# it under the terms of the GNU General Public License as published by
+# the Free Software Foundation, either version 3 of the License, or
+# (at your option) any later version.
+#
+# This program is distributed in the hope that it will be useful,
+# but WITHOUT ANY WARRANTY; without even the implied warranty of
+# MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE.  See the
+# GNU General Public License for more details.
+#
+# You should have received a copy of the GNU General Public License
+# along with this program.  If not, see <http://www.gnu.org/licenses/>.
+#
+####################################################################################################
+
+"""Module to implement the G-code language.
+
+History
+-------
+
+The G-code language, also called RS-274, is a programming language for numerical control.  It was
+developed by the EIA in the early 1960s, and finally standardised by ISO in February 1980 as RS274D
+/ ISO 6983.
+
+The G-code language has several flavours and historical versions. A list of reference documents
+follows :
+
+* The NIST RS274NGC Interpreter - Version 3, T. Kramer, F. Proctor, E. Messina, National Institute
+  of Standards and Technology, NISTIR 6556, August 17, 2000
+* The documentation of the `Linux CNC <http://linuxcnc.org>`_ project, formerly Enhanced Machine
+  Controller developed at NIST,
+* EIA Standard RS-274-D Interchangeable Variable Block Data Format for Positioning, Contouring, and
+  Contouring/Positioning Numerically Controlled Machines, 2001 Eye Street, NW, Washington,
+  D.C. 20006: Electronic Industries Association, February 1979
+
+Overview
+--------
+
+The RS274/NGC language is based on lines of code. Each line (also called a “block”) may include
+commands to a machining center to do several different things.
+
+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,
+:code:`G1 X3` is a valid line of code with two words. :code:`G1` is a command meaning “move in a
+straight line at the programmed feed rate,” and :code:`X3` provides an argument value (the value of
+X should be 3 at the end of the move). Most RS274/NGC commands start with either G or M (for
+miscellaneous). The words for these commands are called “G codes” and “M codes.”
+
+Language View of a Machining Center
+-----------------------------------
+
+Parameters
+~~~~~~~~~~
+
+In the RS274/NGC language view, a machining center maintains an array of 5400 numerical
+parameters. Many of them have specific uses. The parameter array should persist over time, even if
+the machining center is powered down.
+
+Coordinate Systems
+~~~~~~~~~~~~~~~~~~
+
+In the RS274/NGC language view, a machining center has an absolute coordinate system and nine
+program coordinate systems.
+
+You can set the offsets of the nine program coordinate systems using G10 L2 Pn (n is the number of
+the coordinate system) with values for the axes in terms of the absolute coordinate system.
+
+You can select one of the nine systems by using G54, G55, G56, G57, G58, G59, G59.1, G59.2, or
+G59.3. It is not possible to select the absolute coordinate system directly. You can offset the
+current coordinate system using G92 or G92.3. This offset will then apply to all nine program
+coordinate systems. This offset may be cancelled with G92.1 or G92.2.
+
+You can make straight moves in the absolute machine coordinate system by using G53 with either G0 or
+G1.
+
+Data for coordinate systems is stored in parameters.
+
+During initialization, the coordinate system is selected that is specified by parameter 5220. A
+value of 1 means the first coordinate system (the one G54 activates), a value of 2 means the second
+coordinate system (the one G55 activates), and so on. It is an error for the value of parameter 5220
+to be anything but a whole number between one and nine.
+
+Format of a Line
+----------------
+
+A permissible line of input RS274/NGC 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 :code:`/` .
+#. an optional line number.
+#. any number of words, parameter settings, and comments.
+#. an end of line marker (carriage return or line feed or both).
+
+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 :code:`g0x +0. 12 34y
+7` is equivalent to :code:`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.
+
+Line Number
+~~~~~~~~~~~
+
+A line number is the letter :code:`N` followed by an integer (with no sign) between 0 and 99999
+written with no more than five digits (000009 is not OK, for example). Line numbers 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
+~~~~
+
+A word is a letter other than :code:`N` followed by a real value.
+
+Words may begin with any of the letters shown in the following table. The table includes :code:`N`
+for completeness, even though, as defined above, line numbers are not words. Several letters
+(:code:`I`, :code:`J, K`, :code:`L`, :code:`P`, :code:`R`) may have different meanings in different
+contexts.
+
+Table. Linux CNC Words and their meanings Letter
+
+====== =====================================================
+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 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
+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 Modal Groups)
+N       Line number
+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
+====== =====================================================
+
+A real value is some collection of characters that can be processed to come up with a number. A real
+value may be an explicit number (such as 341 or -0.8807), a parameter value, an expression, or a
+unary operation value.
+
+Number
+~~~~~
+
+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 (1) an optional plus or minus sign, followed by (2) zero to many digits,
+  followed, possibly, by (3) one decimal point, followed by (4) zero to many digits — provided that
+  there is at least one digit somewhere in the number.
+* There are two kinds of numbers: integers and decimals. An integer does not have a decimal point in
+  it; a decimal does.
+* Numbers may have any number of digits, subject to the limitation on line length.
+* A non-zero number with no sign as 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.
+
+Parameter Value
+~~~~~~~~~~~~~~~
+
+A parameter value is the pound character :code:`#` followed by a real value. The real value must
+evaluate to an integer between 1 and 5399. The integer is a parameter number, and the value of the
+parameter value is whatever number is stored in the numbered parameter.
+
+The :code:`#` character takes precedence over other operations, so that, for example, :code:`#1+2`
+means the number found by adding 2 to the value of parameter 1, not the value found in parameter
+3. Of course, :code:`#[1+2]` does mean the value found in parameter 3. The :code:`#` character may
+be repeated; for example :code:`##2` means the value of the parameter whose index is the (integer)
+value of parameter 2.
+
+Expressions and Binary Operations
+~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+An expression is a set of characters starting with a left bracket :code:`[` and ending with a
+balancing right bracket :code:`]`. In between the brackets are numbers, parameter values,
+mathematical operations, and other expressions. An expression may be 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 :code:`[ 1 + acos[0] - [#3 ** [4.0/2]]]`.
+
+Binary operations appear only inside expressions. Nine binary operations are defined. There are four
+basic mathematical operations: addition :code:`+`, subtraction :code:`-`, multiplication :code:`*`,
+and division :code:`/`. There are three logical operations: non-exclusive or :code:`OR`, exclusive
+or :code:`XOR`, and logical and :code:`AND`. The eighth operation is the modulus operation
+:code:`MOD`. The ninth operation is the “power” operation :code:`**` of raising the number on the
+left of the operation to the power on the right.  The binary operations are divided into three
+groups. The first group is: power. The second group is: multiplication, division, and modulus. The
+third group is: addition, subtraction, logical non- exclusive or, logical exclusive or, and logical
+and. If operations are strung together (for example in the expression :code:`[2.0 / 3 * 1.5 - 5.5 /
+11.0]`), operations in the first group are to be performed before operations in the second group and
+operations in the second group before operations in the third 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: :code:`[((2.0 / 3) * 1.5) - (5.5 /
+11.0)]`, which simplifies to :code:`[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.
+
+Unary Operation Value
+~~~~~~~~~~~~~~~~~~~~~
+
+A unary operation value is either :code:`ATAN` followed by one expression divided by another
+expression (for example :code:`ATAN[2]/[1+3]`) or any other unary operation name followed by an
+expression (for example :code:`SIN[90]`). The unary operations are: :code:`ABS` (absolute value),
+:code:`ACOS` (arc cosine), :code:`ASIN` (arc sine), :code:`ATAN` (arc tangent), :code:`COS`
+(cosine), :code:`EXP` (e raised to the given power), :code:`FIX` (round down), :code:`FUP` (round
+up), :code:`LN` (natural logarithm), :code:`ROUND` (round to the nearest whole number), :code:`SIN`
+(sine), :code:`SQRT` (square root), and :code:`TAN` (tangent). Arguments to unary operations which
+take angle measures (:code:`COS`, :code:`SIN`, and :code:`TAN`) are in degrees. Values returned by
+unary operations which return angle measures (:code:`ACOS`, :code:`ASIN`, and :code:`ATAN`) are also
+in degrees.
+
+The :code:`FIX` operation rounds towards the left (less positive or more negative) on a number line,
+so that :code:`FIX[2.8] = 2` and :code:`FIX[-2.8] = -3`, for example. The :code:`FUP` operation
+rounds towards the right (more positive or less negative) on a number line; :code:`FUP[2.8] = 3` and
+:code:`FUP[-2.8] = -2`, for example.
+
+Parameter Setting
+~~~~~~~~~~~~~~~~~
+
+A parameter setting is the following four items one after the other: (1) a pound character
+:code:`#`, (2) a real value which evaluates to an integer between 1 and 5399, (3) an equal sign
+:code:`=`, and (4) a real value. For example :code:`#3 = 15` is a parameter setting meaning “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 :code:`#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.
+
+Comments and Messages
+~~~~~~~~~~~~~~~~~~~~~
+
+Printable characters and white space inside parentheses is a comment. A left parenthesis always
+starts a comment. The comment ends at the first right parenthesis found thereafter. Once a left
+parenthesis is placed on a line, a matching right parenthesis must appear before the end of the
+line.  Comments may not be nested; it is an error if a left parenthesis is found after the start of
+a comment and before the end of the comment. Here is an example of a line containing a comment:
+:code:`G80 M5 (stop motion)`. Comments do not cause a machining center to do anything.
+
+.. A comment contains a 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. Comments not containing messages need
+  not be displayed there.
+
+Item Repeats
+~~~~~~~~~~~~
+
+A line may have any number of :code:`G` words, but two :code:`G` words from the same modal group may
+not appear on the same line.
+
+A line may have zero to four :code:`M` words. Two :code:`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, :code:`#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 :code:`#3=15 #3=6` has been interpreted, the
+value of parameter 3 will be 6. If the order is reversed to :code:`#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
+:code:`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 :code:`#4=-7.0 g1 #3=15 g40 (foo)`) for the five items.
+
+Commands and Machine Modes
+~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+In RS274/NGC, many commands cause a machining center 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 :code:`G` codes for motion are also modal. If a :code:`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
+cancelling motion.
+
+“Non-modal” codes have effect only on the lines on which they occur. For example, :code:`G4` (dwell)
+is non-modal.
+
+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 Table 4.
+
+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 :code:`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 :code:`G10`, :code:`G28`, :code:`G30`, and :code:`G92`.
+
+G and Input Codes
+-----------------
+
+See ...
+
+..
+  G codes of the RS274/NGC language are shown in Table 5 and described following that.
+
+  In the command prototypes, three dots (...) stand for a real value. As described earlier, a real
+  value may be (1) an explicit number, 4, for example, (2) an expression, :code:`[2+2]`, for example,
+  (3) a parameter value, #88, for example, or (4) a unary function value, :code:`acos[0]`, for
+  example.  In most cases, if axis words (any or all of X..., Y..., Z..., A..., B..., C...) are given,
+  they specify a destination point. Axis numbers are in the currently active coordinate system, unless
+  explicitly described as being in the absolute coordinate system. Where axis words are optional, any
+  omitted axes will have their current value. Any items in the command prototypes not explicitly
+  described as optional are required. It is an error if a required item is omitted.
+
+  In the prototypes, the values following letters are often given as explicit numbers. Unless stated
+  otherwise, the explicit numbers can be real values. For example, :code:`G10 L2` could equally well
+  be written :code:`G[2*5] L[1+1]`. If the value of parameter 100 were 2, :code:`G10 L#100` would also
+  mean the same. Using real values which are not explicit numbers as just shown in the examples is
+  rarely useful.
+
+  If L... is written in a prototype the “...” will often be referred to as the “L number”. Similarly the
+  “...” in H... may be called the “H number”, and so on for any other letter.
+
+Order of Execution
+------------------
+
+The order of execution of items on a line is critical to safe and effective machine operation. Items
+are executed in a particular order if they occur on the same line.
+
+"""
diff --git a/PythonicGcodeMachine/Gcode/Fanuc/data/fanuc-gcodes-lathe.yaml b/PythonicGcodeMachine/Gcode/Fanuc/data/fanuc-gcodes-lathe.yaml
new file mode 100644
index 0000000000000000000000000000000000000000..71c4370169cda210f6766c9bb6f3d783d3d36077
--- /dev/null
+++ b/PythonicGcodeMachine/Gcode/Fanuc/data/fanuc-gcodes-lathe.yaml
@@ -0,0 +1,106 @@
+F:
+  meaning: set feed rate
+G00:
+  meaning: Rapid traverse
+G01:
+  meaning: Linear interpolation
+G02:
+  meaning: Circular interpolation CW
+G03:
+  meaning: Circular interpolation CCW
+G04:
+  meaning: Dwell
+G09:
+  meaning: Exact stop
+G10:
+  meaning: Programmable data input
+G20:
+  meaning: Input in inch
+G21:
+  meaning: Input in mm
+G22:
+  meaning: Stored stroke check function ON
+G23:
+  meaning: Stored stroke check function OFF
+G27:
+  meaning: Reference position return check
+G28:
+  meaning: Return to reference position
+G32:
+  meaning: Thread cutting
+G40:
+  meaning: Tool nose radius compensation cancel
+G41:
+  meaning: Tool nose radius compensation left
+G42:
+  meaning: Tool nose radius compensation right
+G70:
+  meaning: Finish machining cycle
+G71:
+  meaning: Turning cycle
+G72:
+  meaning: Facing cycle
+G73:
+  meaning: Pattern repeating cycle
+G74:
+  meaning: Peck drilling cycle
+G75:
+  meaning: Grooving cycle
+G76:
+  meaning: Threading cycle
+G92:
+  meaning: Coordinate system setting or max. spindle speed setting
+G94:
+  meaning: Feed per minute
+G95:
+  meaning: Feed per revolution
+G96:
+  meaning: Constant surface speed control
+G97:
+  meaning: Constant surface speed control cancel
+M00:
+  meaning: Program stop
+M01:
+  meaning: Optional program stop
+M02:
+  meaning: End of program
+M03:
+  meaning: Spindle start forward CW
+M04:
+  meaning: Spindle start reverse CCW
+M05:
+  meaning: Spindle stop
+M08:
+  meaning: Coolant ON
+M09:
+  meaning: Coolant OFF
+M29:
+  meaning: Rigid tap mode
+M30:
+  meaning: End of program reset
+M40:
+  meaning: Spindle gear at middle
+M41:
+  meaning: Low gear select
+M42:
+  meaning: High gear select
+M68:
+  meaning: Hydraulic chuck close
+M69:
+  meaning: Hydraulic chuck open
+M78:
+  meaning: Tailstock advancing
+M79:
+  meaning: Tailstock reversing
+M94:
+  meaning: Cancel mirror image
+M95:
+  meaning: Mirror image of X axis
+M98:
+  meaning: Subprogram call
+M99:
+  meaning: End of subprogram
+S:
+  meaning: set spindle speed
+T:
+  meaning: select tool
diff --git a/PythonicGcodeMachine/Gcode/Fanuc/data/fanuc-gcodes-mill.yaml b/PythonicGcodeMachine/Gcode/Fanuc/data/fanuc-gcodes-mill.yaml
new file mode 100644
index 0000000000000000000000000000000000000000..e4c1198a25c4d51f49af2e2e91603a8642ffa646
--- /dev/null
+++ b/PythonicGcodeMachine/Gcode/Fanuc/data/fanuc-gcodes-mill.yaml
@@ -0,0 +1,134 @@
+F:
+  meaning:  set feed rate
+G00:
+  meaning: Rapid traverse
+G01:
+  meaning: Linear interpolation
+G02:
+  meaning: Circular interpolation CW
+G03:
+  meaning: Circular interpolation CCW
+G04:
+  meaning: Dwell
+G17:
+  meaning: X Y plane selection
+G18:
+  meaning: Z X plane selection
+G19:
+  meaning: Y Z plane selection
+G28:
+  meaning: Return to reference position
+G30:
+  meaning: 2nd, 3rd and 4th reference position return
+G40:
+  meaning: Cutter compensation cancel
+G41:
+  meaning: Cutter compensation left
+G42:
+  meaning: Cutter compensation right
+G43:
+  meaning: Tool length compensation + direction
+G44:
+  meaning: Tool length compensation - direction
+G49:
+  meaning: Tool length compensation cancel
+G53:
+  meaning: Machine coordinate system selection
+G54:
+  meaning: Workpiece coordinate system 1 selection
+G55:
+  meaning: Workpiece coordinate system 2 selection
+G56:
+  meaning: Workpiece coordinate system 3 selection
+G57:
+  meaning: Workpiece coordinate system 4 selection
+G58:
+  meaning: Workpiece coordinate system 5 selection
+G59:
+  meaning: Workpiece coordinate system 6 selection
+G68:
+  meaning: Coordinate rotation
+G69:
+  meaning: Coordinate rotation cancel
+G73:
+  meaning: Peck drilling cycle
+G74:
+  meaning: Left-spiral cutting circle
+G76:
+  meaning: Fine boring cycle
+G80:
+  meaning: Canned cycle cancel
+G81:
+  meaning: Drilling cycle, spot boring cycle
+G82:
+  meaning: Drilling cycle or counter boring cycle
+G83:
+  meaning: Peck drilling cycle
+G84:
+  meaning: Tapping cycle
+G85:
+  meaning: Boring cycle
+G86:
+  meaning: Boring cycle
+G87:
+  meaning: Back boring cycle
+G88:
+  meaning: Boring cycle
+G89:
+  meaning: Boring cycle
+G90:
+  meaning: Absolute command
+G91:
+  meaning: Increment command
+G92:
+  meaning: Setting for work coordinate system or clamp at maximum spindle speed
+G98:
+  meaning: Return to initial point in canned cycle
+G99:
+  meaning: Return to R point in canned cycle
+M00:
+  meaning: Program stop
+M01:
+  meaning: Optional program stop
+M02:
+  meaning: End of program
+M03:
+  meaning: Spindle start forward CW
+M04:
+  meaning: Spindle start reverse CCW
+M05:
+  meaning: Spindle stop
+M06:
+  meaning: Tool change
+M07:
+  meaning: Coolant ON – Mist coolant/Coolant thru spindle
+M08:
+  meaning: Coolant ON – Flood coolant
+M09:
+  meaning: Coolant OFF
+M19:
+  meaning: Spindle orientation
+M28:
+  meaning: Return to origin
+M29:
+  meaning: Rigid tap mode
+M30:
+  meaning: End of program (Reset)
+M41:
+  meaning: Low gear select
+M42:
+  meaning: High gear select
+M94:
+  meaning: Cancel mirror image
+M95:
+  meaning: Mirror image of X axis
+M96:
+  meaning: Mirror image of Y axis
+M98:
+  meaning: Subprogram call
+M99:
+  meaning: End of subprogram
+S:
+  meaning: set spindle speed
+T:
+  meaning: select tool
diff --git a/PythonicGcodeMachine/Gcode/Heidenhain/__init__.py b/PythonicGcodeMachine/Gcode/Heidenhain/__init__.py
new file mode 100644
index 0000000000000000000000000000000000000000..37fdd45a0d6bed35fad763c9e5dbb87020fe76cb
--- /dev/null
+++ b/PythonicGcodeMachine/Gcode/Heidenhain/__init__.py
@@ -0,0 +1,384 @@
+####################################################################################################
+#
+# PythonicGcodeMachine - @licence_header_description@
+# Copyright (C) 2018 Fabrice Salvaire
+#
+# This program is free software: you can redistribute it and/or modify
+# it under the terms of the GNU General Public License as published by
+# the Free Software Foundation, either version 3 of the License, or
+# (at your option) any later version.
+#
+# This program is distributed in the hope that it will be useful,
+# but WITHOUT ANY WARRANTY; without even the implied warranty of
+# MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE.  See the
+# GNU General Public License for more details.
+#
+# You should have received a copy of the GNU General Public License
+# along with this program.  If not, see <http://www.gnu.org/licenses/>.
+#
+####################################################################################################
+
+"""Module to implement the G-code language.
+
+History
+-------
+
+The G-code language, also called RS-274, is a programming language for numerical control.  It was
+developed by the EIA in the early 1960s, and finally standardised by ISO in February 1980 as RS274D
+/ ISO 6983.
+
+The G-code language has several flavours and historical versions. A list of reference documents
+follows :
+
+* The NIST RS274NGC Interpreter - Version 3, T. Kramer, F. Proctor, E. Messina, National Institute
+  of Standards and Technology, NISTIR 6556, August 17, 2000
+* The documentation of the `Linux CNC <http://linuxcnc.org>`_ project, formerly Enhanced Machine
+  Controller developed at NIST,
+* EIA Standard RS-274-D Interchangeable Variable Block Data Format for Positioning, Contouring, and
+  Contouring/Positioning Numerically Controlled Machines, 2001 Eye Street, NW, Washington,
+  D.C. 20006: Electronic Industries Association, February 1979
+
+Overview
+--------
+
+The RS274/NGC language is based on lines of code. Each line (also called a “block”) may include
+commands to a machining center to do several different things.
+
+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,
+:code:`G1 X3` is a valid line of code with two words. :code:`G1` is a command meaning “move in a
+straight line at the programmed feed rate,” and :code:`X3` provides an argument value (the value of
+X should be 3 at the end of the move). Most RS274/NGC commands start with either G or M (for
+miscellaneous). The words for these commands are called “G codes” and “M codes.”
+
+Language View of a Machining Center
+-----------------------------------
+
+Parameters
+~~~~~~~~~~
+
+In the RS274/NGC language view, a machining center maintains an array of 5400 numerical
+parameters. Many of them have specific uses. The parameter array should persist over time, even if
+the machining center is powered down.
+
+Coordinate Systems
+~~~~~~~~~~~~~~~~~~
+
+In the RS274/NGC language view, a machining center has an absolute coordinate system and nine
+program coordinate systems.
+
+You can set the offsets of the nine program coordinate systems using G10 L2 Pn (n is the number of
+the coordinate system) with values for the axes in terms of the absolute coordinate system.
+
+You can select one of the nine systems by using G54, G55, G56, G57, G58, G59, G59.1, G59.2, or
+G59.3. It is not possible to select the absolute coordinate system directly. You can offset the
+current coordinate system using G92 or G92.3. This offset will then apply to all nine program
+coordinate systems. This offset may be cancelled with G92.1 or G92.2.
+
+You can make straight moves in the absolute machine coordinate system by using G53 with either G0 or
+G1.
+
+Data for coordinate systems is stored in parameters.
+
+During initialization, the coordinate system is selected that is specified by parameter 5220. A
+value of 1 means the first coordinate system (the one G54 activates), a value of 2 means the second
+coordinate system (the one G55 activates), and so on. It is an error for the value of parameter 5220
+to be anything but a whole number between one and nine.
+
+Format of a Line
+----------------
+
+A permissible line of input RS274/NGC 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 :code:`/` .
+#. an optional line number.
+#. any number of words, parameter settings, and comments.
+#. an end of line marker (carriage return or line feed or both).
+
+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 :code:`g0x +0. 12 34y
+7` is equivalent to :code:`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.
+
+Line Number
+~~~~~~~~~~~
+
+A line number is the letter :code:`N` followed by an integer (with no sign) between 0 and 99999
+written with no more than five digits (000009 is not OK, for example). Line numbers 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
+~~~~
+
+A word is a letter other than :code:`N` followed by a real value.
+
+Words may begin with any of the letters shown in the following table. The table includes :code:`N`
+for completeness, even though, as defined above, line numbers are not words. Several letters
+(:code:`I`, :code:`J, K`, :code:`L`, :code:`P`, :code:`R`) may have different meanings in different
+contexts.
+
+Table. Linux CNC Words and their meanings Letter
+
+====== =====================================================
+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 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
+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 Modal Groups)
+N       Line number
+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
+====== =====================================================
+
+A real value is some collection of characters that can be processed to come up with a number. A real
+value may be an explicit number (such as 341 or -0.8807), a parameter value, an expression, or a
+unary operation value.
+
+Number
+~~~~~
+
+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 (1) an optional plus or minus sign, followed by (2) zero to many digits,
+  followed, possibly, by (3) one decimal point, followed by (4) zero to many digits — provided that
+  there is at least one digit somewhere in the number.
+* There are two kinds of numbers: integers and decimals. An integer does not have a decimal point in
+  it; a decimal does.
+* Numbers may have any number of digits, subject to the limitation on line length.
+* A non-zero number with no sign as 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.
+
+Parameter Value
+~~~~~~~~~~~~~~~
+
+A parameter value is the pound character :code:`#` followed by a real value. The real value must
+evaluate to an integer between 1 and 5399. The integer is a parameter number, and the value of the
+parameter value is whatever number is stored in the numbered parameter.
+
+The :code:`#` character takes precedence over other operations, so that, for example, :code:`#1+2`
+means the number found by adding 2 to the value of parameter 1, not the value found in parameter
+3. Of course, :code:`#[1+2]` does mean the value found in parameter 3. The :code:`#` character may
+be repeated; for example :code:`##2` means the value of the parameter whose index is the (integer)
+value of parameter 2.
+
+Expressions and Binary Operations
+~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+An expression is a set of characters starting with a left bracket :code:`[` and ending with a
+balancing right bracket :code:`]`. In between the brackets are numbers, parameter values,
+mathematical operations, and other expressions. An expression may be 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 :code:`[ 1 + acos[0] - [#3 ** [4.0/2]]]`.
+
+Binary operations appear only inside expressions. Nine binary operations are defined. There are four
+basic mathematical operations: addition :code:`+`, subtraction :code:`-`, multiplication :code:`*`,
+and division :code:`/`. There are three logical operations: non-exclusive or :code:`OR`, exclusive
+or :code:`XOR`, and logical and :code:`AND`. The eighth operation is the modulus operation
+:code:`MOD`. The ninth operation is the “power” operation :code:`**` of raising the number on the
+left of the operation to the power on the right.  The binary operations are divided into three
+groups. The first group is: power. The second group is: multiplication, division, and modulus. The
+third group is: addition, subtraction, logical non- exclusive or, logical exclusive or, and logical
+and. If operations are strung together (for example in the expression :code:`[2.0 / 3 * 1.5 - 5.5 /
+11.0]`), operations in the first group are to be performed before operations in the second group and
+operations in the second group before operations in the third 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: :code:`[((2.0 / 3) * 1.5) - (5.5 /
+11.0)]`, which simplifies to :code:`[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.
+
+Unary Operation Value
+~~~~~~~~~~~~~~~~~~~~~
+
+A unary operation value is either :code:`ATAN` followed by one expression divided by another
+expression (for example :code:`ATAN[2]/[1+3]`) or any other unary operation name followed by an
+expression (for example :code:`SIN[90]`). The unary operations are: :code:`ABS` (absolute value),
+:code:`ACOS` (arc cosine), :code:`ASIN` (arc sine), :code:`ATAN` (arc tangent), :code:`COS`
+(cosine), :code:`EXP` (e raised to the given power), :code:`FIX` (round down), :code:`FUP` (round
+up), :code:`LN` (natural logarithm), :code:`ROUND` (round to the nearest whole number), :code:`SIN`
+(sine), :code:`SQRT` (square root), and :code:`TAN` (tangent). Arguments to unary operations which
+take angle measures (:code:`COS`, :code:`SIN`, and :code:`TAN`) are in degrees. Values returned by
+unary operations which return angle measures (:code:`ACOS`, :code:`ASIN`, and :code:`ATAN`) are also
+in degrees.
+
+The :code:`FIX` operation rounds towards the left (less positive or more negative) on a number line,
+so that :code:`FIX[2.8] = 2` and :code:`FIX[-2.8] = -3`, for example. The :code:`FUP` operation
+rounds towards the right (more positive or less negative) on a number line; :code:`FUP[2.8] = 3` and
+:code:`FUP[-2.8] = -2`, for example.
+
+Parameter Setting
+~~~~~~~~~~~~~~~~~
+
+A parameter setting is the following four items one after the other: (1) a pound character
+:code:`#`, (2) a real value which evaluates to an integer between 1 and 5399, (3) an equal sign
+:code:`=`, and (4) a real value. For example :code:`#3 = 15` is a parameter setting meaning “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 :code:`#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.
+
+Comments and Messages
+~~~~~~~~~~~~~~~~~~~~~
+
+Printable characters and white space inside parentheses is a comment. A left parenthesis always
+starts a comment. The comment ends at the first right parenthesis found thereafter. Once a left
+parenthesis is placed on a line, a matching right parenthesis must appear before the end of the
+line.  Comments may not be nested; it is an error if a left parenthesis is found after the start of
+a comment and before the end of the comment. Here is an example of a line containing a comment:
+:code:`G80 M5 (stop motion)`. Comments do not cause a machining center to do anything.
+
+.. A comment contains a 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. Comments not containing messages need
+  not be displayed there.
+
+Item Repeats
+~~~~~~~~~~~~
+
+A line may have any number of :code:`G` words, but two :code:`G` words from the same modal group may
+not appear on the same line.
+
+A line may have zero to four :code:`M` words. Two :code:`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, :code:`#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 :code:`#3=15 #3=6` has been interpreted, the
+value of parameter 3 will be 6. If the order is reversed to :code:`#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
+:code:`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 :code:`#4=-7.0 g1 #3=15 g40 (foo)`) for the five items.
+
+Commands and Machine Modes
+~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+In RS274/NGC, many commands cause a machining center 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 :code:`G` codes for motion are also modal. If a :code:`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
+cancelling motion.
+
+“Non-modal” codes have effect only on the lines on which they occur. For example, :code:`G4` (dwell)
+is non-modal.
+
+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 Table 4.
+
+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 :code:`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 :code:`G10`, :code:`G28`, :code:`G30`, and :code:`G92`.
+
+G and Input Codes
+-----------------
+
+See ...
+
+..
+  G codes of the RS274/NGC language are shown in Table 5 and described following that.
+
+  In the command prototypes, three dots (...) stand for a real value. As described earlier, a real
+  value may be (1) an explicit number, 4, for example, (2) an expression, :code:`[2+2]`, for example,
+  (3) a parameter value, #88, for example, or (4) a unary function value, :code:`acos[0]`, for
+  example.  In most cases, if axis words (any or all of X..., Y..., Z..., A..., B..., C...) are given,
+  they specify a destination point. Axis numbers are in the currently active coordinate system, unless
+  explicitly described as being in the absolute coordinate system. Where axis words are optional, any
+  omitted axes will have their current value. Any items in the command prototypes not explicitly
+  described as optional are required. It is an error if a required item is omitted.
+
+  In the prototypes, the values following letters are often given as explicit numbers. Unless stated
+  otherwise, the explicit numbers can be real values. For example, :code:`G10 L2` could equally well
+  be written :code:`G[2*5] L[1+1]`. If the value of parameter 100 were 2, :code:`G10 L#100` would also
+  mean the same. Using real values which are not explicit numbers as just shown in the examples is
+  rarely useful.
+
+  If L... is written in a prototype the “...” will often be referred to as the “L number”. Similarly the
+  “...” in H... may be called the “H number”, and so on for any other letter.
+
+Order of Execution
+------------------
+
+The order of execution of items on a line is critical to safe and effective machine operation. Items
+are executed in a particular order if they occur on the same line.
+
+"""
diff --git a/PythonicGcodeMachine/Gcode/Heidenhain/data/heidenhain-TNC-426-mcodes.yaml b/PythonicGcodeMachine/Gcode/Heidenhain/data/heidenhain-TNC-426-mcodes.yaml
new file mode 100644
index 0000000000000000000000000000000000000000..ea4160dae65546fdf758f8752e45747a25b2a5f5
--- /dev/null
+++ b/PythonicGcodeMachine/Gcode/Heidenhain/data/heidenhain-TNC-426-mcodes.yaml
@@ -0,0 +1,38 @@
+M0:
+  meaning: Program stop
+M1:
+  meaning: Optional stop (program stop only with opt. stop)
+M2:
+  meaning: Program end
+M3:
+  meaning: Spindle ON clockwise
+M4:
+  meaning: Spindle ON counterclockwise
+M5:
+  meaning: Spindle Stop
+M6:
+  meaning: Tool change
+M8:
+  meaning: Coolant ON
+M9:
+  meaning: Coolant OFF
+M10:
+  meaning: Dividing head, clamping ON
+M11:
+  meaning: Dividing head, clamping OFF
+M17:
+  meaning: End of subprogram
+M25:
+  meaning: Open clamp/ machine vice
+M26:
+  meaning: Close clamp/ machine vice
+M27:
+  meaning: Swivel dividing head
+M30:
+  meaning: Main program end
+M71:
+  meaning: Puff blowing device ON
+M72:
+  meaning: Puff blowing device OFF
+M99:
+  meaning: Cycle call
diff --git a/PythonicGcodeMachine/Gcode/Heidenhain/data/heidenhain-gcodes.yaml b/PythonicGcodeMachine/Gcode/Heidenhain/data/heidenhain-gcodes.yaml
new file mode 100644
index 0000000000000000000000000000000000000000..456523fdd8bb89fd202a3be6a7e2de2cfe100871
--- /dev/null
+++ b/PythonicGcodeMachine/Gcode/Heidenhain/data/heidenhain-gcodes.yaml
@@ -0,0 +1,473 @@
+F:
+  meaning: set feed rate
+# Tool movements
+G00:
+  meaning: Straight-line interpolation, Cartesian coordinates, rapid traverse
+G01:
+  meaning: Straight-line interpolation, Cartesian coordinates
+G02:
+  meaning: Circular interpolation, Cartesian coordinates, clockwise
+G03:
+  meaning: Circular interpolation, Cartesian coordinates, counterclockwise
+G05:
+  meaning: Circular interpolation, Cartesian coordinates, without indication of direction
+G06:
+  meaning: Circular interpolation, Cartesian coordinates, tangential contour approach
+G07:
+  meaning: Paraxial positioning block
+G10:
+  meaning: Straight-line interpolation, polar coordinates, rapid traverse
+G11:
+  meaning: Straight-line interpolation, polar coordinates
+G12:
+  meaning: Circular interpolation, polar coordinates, clockwise
+G13:
+  meaning: Circular interpolation, polar coordinates, counterclockwise
+G15:
+  meaning: Circular interpolation, polar coordinates, without indication of direction
+G16:
+  meaning: Circular interpolation, polar coordinates, tangential contour approach
+# Chamfer/Rounding/Approach contour/Depart contour
+G24:
+  meaning: Chamfer with length R
+G25:
+  meaning: Corner rounding with radius R
+G26:
+  meaning: Tangential contour approach with radius R
+G27:
+  meaning: Tangential contour approach with radius R
+# Tool definition
+G99:
+  meaning: With tool number T, length L, radius R
+# Tool radius compensation
+G40:
+  meaning: No tool radius compensation
+G41:
+  meaning: Tool radius compensation, left of the contour
+G42:
+  meaning: Tool radius compensation, right of the contour
+G43:
+  meaning: Paraxial compensation for G07, lengthening
+G44:
+  meaning: Paraxial compensation for G07, shortening
+# Blank form definition for graphics
+G30:
+  meaning: (G17/G18/G19) min. point
+G31:
+  meaning: (G90/G91) max. point
+# Cycles for drilling, tapping and thread milling
+G83:
+  meaning: Pecking
+G84:
+  meaning: Tapping with a floating tap holder
+G85:
+  meaning: Rigid tapping
+G86:
+  meaning: Thread cutting
+G200:
+  meaning: Drilling
+G201:
+  meaning: Reaming
+G202:
+  meaning: Boring
+G203:
+  meaning: Universal drilling
+G204:
+  meaning: Back boring
+G205:
+  meaning: Universal pecking
+G206:
+  meaning: Tapping with a floating tap holder
+G207:
+  meaning: Rigid tapping
+G208:
+  meaning: Bore milling
+G209:
+  meaning: Tapping with chip breaking
+Cycles for creating point patterns
+# G220:
+  meaning: Circular pattern
+G221:
+  meaning: Linear pattern
+SL Cycles, group 1
+# G37:
+  meaning: Contour geometry, list of subcontour program numbers
+G56:
+  meaning: Pilot drilling
+G57:
+  meaning: Rough-out
+G58:
+  meaning: Contour milling in clockwise direction (finishing)
+G59:
+  meaning: Contour milling, counterclockwise (finishing)
+# SL cycles, group 2
+G37:
+  meaning: Contour geometry, list of subcontour program numbers
+G120:
+  meaning: Contour data (applies to G121 to G124)
+G121:
+  meaning: Pilot drilling
+G122:
+  meaning: Rough-out
+G123:
+  meaning: Floor finishing
+G124:
+  meaning: Side finishing
+G125:
+  meaning: Contour train (machining open contour)
+G127:
+  meaning: Cylinder surface
+G128:
+  meaning: Cylindrical surface slot
+# Coordinate transformation
+G53:
+  meaning: Datum shift in datum table
+G54:
+  meaning: Datum shift in program
+G28:
+  meaning: Mirror image
+G73:
+  meaning: Rotation of the coordinate system
+G72:
+  meaning: Scaling factor (reduce or enlarge contour)
+G80:
+  meaning: Tilting the working plane
+G247:
+  meaning: Datum setting
+# Cycles for multipass milling
+G60:
+  meaning: Run 3-D data
+G230:
+  meaning: Multipass milling of plane surfaces
+G231:
+  meaning: Multipass milling of tilted surfaces
+G232:
+  meaning: Face milling
+# Special cycles
+G04:
+  meaning: Dwell time with F seconds
+G36:
+  meaning: Spindle orientation
+G39:
+  meaning: Program call
+G62:
+  meaning: Tolerance deviation for fast contour milling
+G440:
+  meaning: Measure axis shift
+G441:
+  meaning: Fast probing
+# Define machining plane
+G17:
+  meaning: Working plane X/Y, tool axis Z
+G18:
+  meaning: Working plane Z/X, tool axis Y
+G19:
+  meaning: Working plane Y/Z, tool axis X
+G20:
+  meaning: Tool axis IV
+# Dimensions
+G90:
+  meaning: Absolute dimensions
+G91:
+  meaning: Incremental dimensions
+# Unit of measure
+G70:
+  meaning: Inches (set at start of program)
+G71:
+  meaning: Millimeters (set at start of program)
+# Other G functions
+G29:
+  meaning: Transfer the last nominal position value as a pole (circle center)
+G38:
+  meaning: STOP program run
+G51:
+  meaning: Next tool number (with central tool file)
+G79:
+  meaning: Cycle call
+G98:
+  meaning: Set label number
+# Cycles for drilling, tapping and thread milling
+G240:
+  meaning: Centering
+G200:
+  meaning: Drilling
+G201:
+  meaning: Reaming
+G202:
+  meaning: Boring
+G203:
+  meaning: Universal drilling
+G204:
+  meaning: Back boring
+G205:
+  meaning: Universal pecking
+G206:
+  meaning: Tapping with a floating tap holder
+G207:
+  meaning: Rigid tapping
+G208:
+  meaning: Bore milling
+G209:
+  meaning: Tapping with chip breaking
+G241:
+  meaning: Single-lip deep-hole drilling
+# Cycles for drilling, tapping and thread milling
+G262:
+  meaning: Thread milling
+G263:
+  meaning: Thread milling/countersinking
+G264:
+  meaning: Thread drilling/milling
+G265:
+  meaning: Helical thread drilling/milling
+G267:
+  meaning: External thread milling
+# Cycles for milling pockets, studs and slots
+G74:
+  meaning: Slot milling
+G75:
+  meaning: Rectangular pocket milling in clockwise direction
+G76:
+  meaning: Rectangular pocket milling in counterclockwise direction
+G77:
+  meaning: Circular pocket milling in clockwise direction
+G78:
+  meaning: Circular pocket milling in counterclockwise direction
+G210:
+  meaning: Slot milling with reciprocating plunge
+G211:
+  meaning: Round slot with reciprocating plunge
+G212:
+  meaning: Rectangular pocket finishing
+G213:
+  meaning: Rectangular stud finishing
+G214:
+  meaning: Circular pocket finishing
+G215:
+  meaning: Circular stud finishing
+# Cycles for milling pockets, studs and slots
+G251:
+  meaning: Rectangular pocket, complete
+G252:
+  meaning: Circular pocket, complete
+G253:
+  meaning: Slot, complete
+G254:
+  meaning: Circular slot, complete
+G256:
+  meaning: Rectangular stud
+G257:
+  meaning: Circular stud
+# Cycles for creating point patterns
+G220:
+  meaning: Circular point pattern
+G221:
+  meaning: Point patterns on lines
+# Cycles for multipass milling
+G230:
+  meaning: Multipass milling of smooth surfaces
+G231:
+  meaning: Multipass milling of tilted surfaces
+G232:
+  meaning: Face milling
+# Touch probe cycles for measuring workpiece misalignment
+G400:
+  meaning: Basic rotation using two points
+G401:
+  meaning: Basic rotation from two holes
+G402:
+  meaning: Basic rotation from two studs
+G403:
+  meaning: Compensate a basic rotation via a rotary axis
+G404:
+  meaning: Set basic rotation
+G405:
+  meaning: Compensating misalignment with the C axis
+# Touch probe cycles for datum setting
+G408:
+  meaning: Slot center reference point
+G409:
+  meaning: Reference point at center of hole
+G410:
+  meaning: Datum from inside of rectangle
+G411:
+  meaning: Datum from outside of rectangle
+G412:
+  meaning: Datum from inside of circle
+G413:
+  meaning: Datum from outside of circle
+G414:
+  meaning: Datum in outside corner
+G415:
+  meaning: Datum in inside corner
+G416:
+  meaning: Datum circle center
+G417:
+  meaning: Datum in touch probe axis
+G418:
+  meaning: Datum in center of 4 holes
+G419:
+  meaning: Reference point in selectable axis
+# Touch probe cycles for workpiece measurement
+G55:
+  meaning: Measure any coordinate
+G420:
+  meaning: Measure any angle
+G421:
+  meaning: Measure hole
+G422:
+  meaning: Measure cylindrical stud
+G423:
+  meaning: Measure rectangular pocket
+G424:
+  meaning: Measure rectangular stud
+G425:
+  meaning: Measure slot
+G426:
+  meaning: Measure ridge
+G427:
+  meaning: Measure any coordinate
+G430:
+  meaning: Measure circle center
+G431:
+  meaning: Measure any plane
+# Touch probe cycles for tool measurement
+G480:
+  meaning: Calibrating the TT
+G481:
+  meaning: Measure tool length
+G482:
+  meaning: Measure tool radius
+G483:
+  meaning: Measure tool length and tool radius
+#
+M0:
+  meaning: Stop program run (Spindle STOP, Coolant OFF)
+M1:
+  meaning: Optional program STOP (Spindle STOP, Coolant OFF)
+M2:
+  meaning: Stop program run (Spindle STOP,Coolant OFF,Go to block 1,Clear the status display(depending on machine parameter))
+M3:
+  meaning: Spindle ON clockwise
+M4:
+  meaning: Spindle ON counterclockwise
+M5:
+  meaning: Spindle STOP
+M6:
+  meaning: Tool change (STOP program run (depending on machine parameter),Spindle STOP)
+M8:
+  meaning: Coolant ON
+M9:
+  meaning: Coolant OFF
+M13:
+  meaning: Spindle ON clockwise (Coolant ON)
+M14:
+  meaning: Spindle ON counterclockwise (Coolant ON)
+M30:
+  meaning: Same as M2
+M89:
+  meaning: Vacant miscellaneous function or Cycle call, modally effective (depending on machine parameter)
+M91:
+  meaning: Within the positioning block: Coordinates are referenced to machine datum
+M92:
+  meaning: Within the positioning block: Coordinates are referenced to position defined by machine tool builder, such as tool change position
+M94:
+  meaning: Reduce the rotary axis display to a value below 360°
+M97:
+  meaning: Machine small contour steps
+M98:
+  meaning: Machine open contours completely
+M99:
+  meaning: Blockwise cycle call (Cycle call, NON-MODAL)
+M101:
+  meaning: Automatic tool change with replacement tool if maximum tool life has expired
+M102:
+  meaning: Reset M101
+M103:
+  meaning: Reduce feed rate during plunging to factor F (percentage)
+M104:
+  meaning: Reactivate the datum as last defined
+M105:
+  meaning: Machining with second kv factor
+M106:
+  meaning: Machining with first kv factor
+M107:
+  meaning: Suppress error message for replacement tools with oversize
+M108:
+  meaning: Reset M107
+M109:
+  meaning: Constant contouring speed at tool cutting edge (increase and decrease feed rate)
+M110:
+  meaning: Constant contouring speed at tool cutting edge (feed rate decrease only)
+M111:
+  meaning: Reset M109/M110
+M112:
+  meaning: Enter contour transition between two contour elements
+M113:
+  meaning: Reset M112
+M114:
+  meaning: Automatic compensation of machine geometry when working with tilted axes
+M115:
+  meaning: Reset M114
+M116:
+  meaning: Feed rate for rotary axes in mm/min
+M117:
+  meaning: Reset M116
+M118:
+  meaning: Superimpose handwheel positioning during program run
+M120:
+  meaning: Pre-calculate radius-compensated contour (LOOK AHEAD)
+M124:
+  meaning: Contour filter
+M126:
+  meaning: Shortest-path traverse of rotary axes
+M127:
+  meaning: Reset M126
+M128:
+  meaning: Retain the position of the tool tip when positioning the tilted axes (TCPM)
+M129:
+  meaning: Reset M128
+M130:
+  meaning: Moving to position in an untilted coordinate system with a tilted working plane
+M134:
+  meaning: Exact stop at nontangential contour transitions when positioning with rotary axes
+M135:
+  meaning: Reset M134
+M136:
+  meaning: Feed rate F in millimeters per spindle revolution
+M137:
+  meaning: Reset M136
+M138:
+  meaning: Selection of tilted axes
+M140:
+  meaning: Retraction from the contour in the tool-axis direction
+M141:
+  meaning: Suppress touch probe monitoring
+M142:
+  meaning: Delete modal program information
+M143:
+  meaning: Delete basic rotation
+M144:
+  meaning: Compensating the machine’s kinematics configuration for ACTUAL/NOMINAL positions at end of block
+M145:
+  meaning: Reset M144
+M148:
+  meaning: Retract the tool automatically from the contour at NC stop
+M149:
+  meaning: Reset M148
+M150:
+  meaning: Suppress limit switch message
+M200:
+  meaning: Laser cutting: Output programmed voltage directly
+M201:
+  meaning: Laser cutting: Output voltage as a function of distance
+M202:
+  meaning: Laser cutting: Output voltage as a function of speed
+M203:
+  meaning: Laser cutting: Output voltage as a function of time (ramp)
+M204:
+  meaning: Laser cutting: Output voltage as a function of time (pulse)
+S:
+  meaning: set spindle speed
+T:
+  meaning: select tool
diff --git a/PythonicGcodeMachine/Gcode/LinuxCnc/__init__.py b/PythonicGcodeMachine/Gcode/LinuxCnc/__init__.py
new file mode 100644
index 0000000000000000000000000000000000000000..37fdd45a0d6bed35fad763c9e5dbb87020fe76cb
--- /dev/null
+++ b/PythonicGcodeMachine/Gcode/LinuxCnc/__init__.py
@@ -0,0 +1,384 @@
+####################################################################################################
+#
+# PythonicGcodeMachine - @licence_header_description@
+# Copyright (C) 2018 Fabrice Salvaire
+#
+# This program is free software: you can redistribute it and/or modify
+# it under the terms of the GNU General Public License as published by
+# the Free Software Foundation, either version 3 of the License, or
+# (at your option) any later version.
+#
+# This program is distributed in the hope that it will be useful,
+# but WITHOUT ANY WARRANTY; without even the implied warranty of
+# MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE.  See the
+# GNU General Public License for more details.
+#
+# You should have received a copy of the GNU General Public License
+# along with this program.  If not, see <http://www.gnu.org/licenses/>.
+#
+####################################################################################################
+
+"""Module to implement the G-code language.
+
+History
+-------
+
+The G-code language, also called RS-274, is a programming language for numerical control.  It was
+developed by the EIA in the early 1960s, and finally standardised by ISO in February 1980 as RS274D
+/ ISO 6983.
+
+The G-code language has several flavours and historical versions. A list of reference documents
+follows :
+
+* The NIST RS274NGC Interpreter - Version 3, T. Kramer, F. Proctor, E. Messina, National Institute
+  of Standards and Technology, NISTIR 6556, August 17, 2000
+* The documentation of the `Linux CNC <http://linuxcnc.org>`_ project, formerly Enhanced Machine
+  Controller developed at NIST,
+* EIA Standard RS-274-D Interchangeable Variable Block Data Format for Positioning, Contouring, and
+  Contouring/Positioning Numerically Controlled Machines, 2001 Eye Street, NW, Washington,
+  D.C. 20006: Electronic Industries Association, February 1979
+
+Overview
+--------
+
+The RS274/NGC language is based on lines of code. Each line (also called a “block”) may include
+commands to a machining center to do several different things.
+
+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,
+:code:`G1 X3` is a valid line of code with two words. :code:`G1` is a command meaning “move in a
+straight line at the programmed feed rate,” and :code:`X3` provides an argument value (the value of
+X should be 3 at the end of the move). Most RS274/NGC commands start with either G or M (for
+miscellaneous). The words for these commands are called “G codes” and “M codes.”
+
+Language View of a Machining Center
+-----------------------------------
+
+Parameters
+~~~~~~~~~~
+
+In the RS274/NGC language view, a machining center maintains an array of 5400 numerical
+parameters. Many of them have specific uses. The parameter array should persist over time, even if
+the machining center is powered down.
+
+Coordinate Systems
+~~~~~~~~~~~~~~~~~~
+
+In the RS274/NGC language view, a machining center has an absolute coordinate system and nine
+program coordinate systems.
+
+You can set the offsets of the nine program coordinate systems using G10 L2 Pn (n is the number of
+the coordinate system) with values for the axes in terms of the absolute coordinate system.
+
+You can select one of the nine systems by using G54, G55, G56, G57, G58, G59, G59.1, G59.2, or
+G59.3. It is not possible to select the absolute coordinate system directly. You can offset the
+current coordinate system using G92 or G92.3. This offset will then apply to all nine program
+coordinate systems. This offset may be cancelled with G92.1 or G92.2.
+
+You can make straight moves in the absolute machine coordinate system by using G53 with either G0 or
+G1.
+
+Data for coordinate systems is stored in parameters.
+
+During initialization, the coordinate system is selected that is specified by parameter 5220. A
+value of 1 means the first coordinate system (the one G54 activates), a value of 2 means the second
+coordinate system (the one G55 activates), and so on. It is an error for the value of parameter 5220
+to be anything but a whole number between one and nine.
+
+Format of a Line
+----------------
+
+A permissible line of input RS274/NGC 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 :code:`/` .
+#. an optional line number.
+#. any number of words, parameter settings, and comments.
+#. an end of line marker (carriage return or line feed or both).
+
+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 :code:`g0x +0. 12 34y
+7` is equivalent to :code:`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.
+
+Line Number
+~~~~~~~~~~~
+
+A line number is the letter :code:`N` followed by an integer (with no sign) between 0 and 99999
+written with no more than five digits (000009 is not OK, for example). Line numbers 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
+~~~~
+
+A word is a letter other than :code:`N` followed by a real value.
+
+Words may begin with any of the letters shown in the following table. The table includes :code:`N`
+for completeness, even though, as defined above, line numbers are not words. Several letters
+(:code:`I`, :code:`J, K`, :code:`L`, :code:`P`, :code:`R`) may have different meanings in different
+contexts.
+
+Table. Linux CNC Words and their meanings Letter
+
+====== =====================================================
+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 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
+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 Modal Groups)
+N       Line number
+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
+====== =====================================================
+
+A real value is some collection of characters that can be processed to come up with a number. A real
+value may be an explicit number (such as 341 or -0.8807), a parameter value, an expression, or a
+unary operation value.
+
+Number
+~~~~~
+
+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 (1) an optional plus or minus sign, followed by (2) zero to many digits,
+  followed, possibly, by (3) one decimal point, followed by (4) zero to many digits — provided that
+  there is at least one digit somewhere in the number.
+* There are two kinds of numbers: integers and decimals. An integer does not have a decimal point in
+  it; a decimal does.
+* Numbers may have any number of digits, subject to the limitation on line length.
+* A non-zero number with no sign as 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.
+
+Parameter Value
+~~~~~~~~~~~~~~~
+
+A parameter value is the pound character :code:`#` followed by a real value. The real value must
+evaluate to an integer between 1 and 5399. The integer is a parameter number, and the value of the
+parameter value is whatever number is stored in the numbered parameter.
+
+The :code:`#` character takes precedence over other operations, so that, for example, :code:`#1+2`
+means the number found by adding 2 to the value of parameter 1, not the value found in parameter
+3. Of course, :code:`#[1+2]` does mean the value found in parameter 3. The :code:`#` character may
+be repeated; for example :code:`##2` means the value of the parameter whose index is the (integer)
+value of parameter 2.
+
+Expressions and Binary Operations
+~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+An expression is a set of characters starting with a left bracket :code:`[` and ending with a
+balancing right bracket :code:`]`. In between the brackets are numbers, parameter values,
+mathematical operations, and other expressions. An expression may be 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 :code:`[ 1 + acos[0] - [#3 ** [4.0/2]]]`.
+
+Binary operations appear only inside expressions. Nine binary operations are defined. There are four
+basic mathematical operations: addition :code:`+`, subtraction :code:`-`, multiplication :code:`*`,
+and division :code:`/`. There are three logical operations: non-exclusive or :code:`OR`, exclusive
+or :code:`XOR`, and logical and :code:`AND`. The eighth operation is the modulus operation
+:code:`MOD`. The ninth operation is the “power” operation :code:`**` of raising the number on the
+left of the operation to the power on the right.  The binary operations are divided into three
+groups. The first group is: power. The second group is: multiplication, division, and modulus. The
+third group is: addition, subtraction, logical non- exclusive or, logical exclusive or, and logical
+and. If operations are strung together (for example in the expression :code:`[2.0 / 3 * 1.5 - 5.5 /
+11.0]`), operations in the first group are to be performed before operations in the second group and
+operations in the second group before operations in the third 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: :code:`[((2.0 / 3) * 1.5) - (5.5 /
+11.0)]`, which simplifies to :code:`[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.
+
+Unary Operation Value
+~~~~~~~~~~~~~~~~~~~~~
+
+A unary operation value is either :code:`ATAN` followed by one expression divided by another
+expression (for example :code:`ATAN[2]/[1+3]`) or any other unary operation name followed by an
+expression (for example :code:`SIN[90]`). The unary operations are: :code:`ABS` (absolute value),
+:code:`ACOS` (arc cosine), :code:`ASIN` (arc sine), :code:`ATAN` (arc tangent), :code:`COS`
+(cosine), :code:`EXP` (e raised to the given power), :code:`FIX` (round down), :code:`FUP` (round
+up), :code:`LN` (natural logarithm), :code:`ROUND` (round to the nearest whole number), :code:`SIN`
+(sine), :code:`SQRT` (square root), and :code:`TAN` (tangent). Arguments to unary operations which
+take angle measures (:code:`COS`, :code:`SIN`, and :code:`TAN`) are in degrees. Values returned by
+unary operations which return angle measures (:code:`ACOS`, :code:`ASIN`, and :code:`ATAN`) are also
+in degrees.
+
+The :code:`FIX` operation rounds towards the left (less positive or more negative) on a number line,
+so that :code:`FIX[2.8] = 2` and :code:`FIX[-2.8] = -3`, for example. The :code:`FUP` operation
+rounds towards the right (more positive or less negative) on a number line; :code:`FUP[2.8] = 3` and
+:code:`FUP[-2.8] = -2`, for example.
+
+Parameter Setting
+~~~~~~~~~~~~~~~~~
+
+A parameter setting is the following four items one after the other: (1) a pound character
+:code:`#`, (2) a real value which evaluates to an integer between 1 and 5399, (3) an equal sign
+:code:`=`, and (4) a real value. For example :code:`#3 = 15` is a parameter setting meaning “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 :code:`#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.
+
+Comments and Messages
+~~~~~~~~~~~~~~~~~~~~~
+
+Printable characters and white space inside parentheses is a comment. A left parenthesis always
+starts a comment. The comment ends at the first right parenthesis found thereafter. Once a left
+parenthesis is placed on a line, a matching right parenthesis must appear before the end of the
+line.  Comments may not be nested; it is an error if a left parenthesis is found after the start of
+a comment and before the end of the comment. Here is an example of a line containing a comment:
+:code:`G80 M5 (stop motion)`. Comments do not cause a machining center to do anything.
+
+.. A comment contains a 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. Comments not containing messages need
+  not be displayed there.
+
+Item Repeats
+~~~~~~~~~~~~
+
+A line may have any number of :code:`G` words, but two :code:`G` words from the same modal group may
+not appear on the same line.
+
+A line may have zero to four :code:`M` words. Two :code:`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, :code:`#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 :code:`#3=15 #3=6` has been interpreted, the
+value of parameter 3 will be 6. If the order is reversed to :code:`#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
+:code:`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 :code:`#4=-7.0 g1 #3=15 g40 (foo)`) for the five items.
+
+Commands and Machine Modes
+~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+In RS274/NGC, many commands cause a machining center 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 :code:`G` codes for motion are also modal. If a :code:`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
+cancelling motion.
+
+“Non-modal” codes have effect only on the lines on which they occur. For example, :code:`G4` (dwell)
+is non-modal.
+
+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 Table 4.
+
+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 :code:`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 :code:`G10`, :code:`G28`, :code:`G30`, and :code:`G92`.
+
+G and Input Codes
+-----------------
+
+See ...
+
+..
+  G codes of the RS274/NGC language are shown in Table 5 and described following that.
+
+  In the command prototypes, three dots (...) stand for a real value. As described earlier, a real
+  value may be (1) an explicit number, 4, for example, (2) an expression, :code:`[2+2]`, for example,
+  (3) a parameter value, #88, for example, or (4) a unary function value, :code:`acos[0]`, for
+  example.  In most cases, if axis words (any or all of X..., Y..., Z..., A..., B..., C...) are given,
+  they specify a destination point. Axis numbers are in the currently active coordinate system, unless
+  explicitly described as being in the absolute coordinate system. Where axis words are optional, any
+  omitted axes will have their current value. Any items in the command prototypes not explicitly
+  described as optional are required. It is an error if a required item is omitted.
+
+  In the prototypes, the values following letters are often given as explicit numbers. Unless stated
+  otherwise, the explicit numbers can be real values. For example, :code:`G10 L2` could equally well
+  be written :code:`G[2*5] L[1+1]`. If the value of parameter 100 were 2, :code:`G10 L#100` would also
+  mean the same. Using real values which are not explicit numbers as just shown in the examples is
+  rarely useful.
+
+  If L... is written in a prototype the “...” will often be referred to as the “L number”. Similarly the
+  “...” in H... may be called the “H number”, and so on for any other letter.
+
+Order of Execution
+------------------
+
+The order of execution of items on a line is critical to safe and effective machine operation. Items
+are executed in a particular order if they occur on the same line.
+
+"""
diff --git a/PythonicGcodeMachine/Gcode/LinuxCnc/data/linuxcnc-gcodes.yaml b/PythonicGcodeMachine/Gcode/LinuxCnc/data/linuxcnc-gcodes.yaml
new file mode 100644
index 0000000000000000000000000000000000000000..349ccb73ccab407db9ba41209e2023223d89f80c
--- /dev/null
+++ b/PythonicGcodeMachine/Gcode/LinuxCnc/data/linuxcnc-gcodes.yaml
@@ -0,0 +1,287 @@
+# cf. http://linuxcnc.org/docs/2.7/html/gcode.html
+F:
+  meaning: Set feed rate
+# Motion (X Y Z A B C U V W apply to all motions)
+G0:
+  meaning: Rapid Move
+G1:
+  meaning: Linear Move
+G23:
+  meaning: Arc Move
+  parameters: I J K or R, P
+G3:
+  meaning: Arc Move
+  parameters: I J K or R, P
+G4:
+  meaning: Dwell
+  parameters: P
+G5:
+  meaning: Cubic Spline
+  parameters: I J P Q
+G5.1:
+  meaning: Quadratic Spline
+  parameters: I J
+G5.2:
+  meaning: NURBS
+  parameters: P L
+G38.2:
+  meaning: Straight Probe
+G38.3:
+  meaning: Straight Probe
+G38.4:
+  meaning: Straight Probe
+G38.5:
+  meaning: Straight Probe
+G33:
+  meaning: Spindle Synchronized Motion
+  parameters: K
+G33.1:
+  meaning: Rigid Tapping
+  parameters: K
+G80:
+  meaning: Cancel Canned Cycle
+# Canned cycles (X Y Z or U V W apply to canned cycles, depending on active plane)
+G81:
+  meaning: Drilling Cycle
+  parameters: R L (P)
+G82:
+  meaning: Drilling Cycle, Dwell
+  parameters: R L (P)
+G83:
+  meaning: Drilling Cycle, Peck
+  parameters: R L Q
+G73:
+  meaning: Drilling Cycle, Chip Breaking
+  parameters: R L Q
+G85:
+  meaning: Boring Cycle, Feed Out
+  parameters: R L (P)
+G89:
+  meaning: Boring Cycle, Dwell, Feed Out
+  parameters: R L (P)
+G76:
+  meaning: Threading Cycle
+  parameters: P Z I J R K Q H L E
+# Distance Mode
+G90:
+  meaning: Distance Mode
+G91:
+  meaning: Distance Mode
+G90.1:
+  meaning: Arc Distance Mode
+G91.1:
+  meaning: Arc Distance Mode
+G7:
+  meaning: Lathe Diameter Mode
+G8:
+  meaning: Lathe Radius Mode
+# Feed Rate Mode
+G93:
+  meaning: Feed Rate Mode
+G94:
+  meaning: Feed Rate Mode
+G95:
+  meaning: Feed Rate Mode
+# Spindle Control
+M3:
+  meaning: Spindle Control
+  parameters: S
+M4:
+  meaning: Spindle Control
+  parameters: S
+M5:
+  meaning: Spindle Control
+  parameters: S
+M19:
+  meaning: Orient Spindle
+G96:
+  meaning: Spindle Control Mode
+  parameters: S D
+G97:
+  meaning: Spindle Control Mode
+  parameters: S D
+# Coolant
+M7:
+  meaning: Coolant Control
+M8:
+  meaning: Coolant Control
+M9:
+  meaning: Coolant Control
+# Tool Length Offset
+G43:
+  meaning: Tool Length Offset
+  parameters: H
+G43.1:
+  meaning: Dynamic Tool Length Offset
+G43.2:
+  meaning: Apply additional Tool Length Offset
+  parameters: H
+G49:
+  meaning: Cancel Tool Length Compensation
+# Stopping
+M0:
+  meaning: Program Pause
+M1:
+  meaning: Program Pause
+M2:
+  meaning: Program End
+M30:
+  meaning: Program End
+M60:
+  meaning: Pallet Change Pause
+# Units
+G20:
+  meaning: Units (inch, mm)
+G21:
+  meaning: Units (inch, mm)
+# Plane Selection: (affects G2, G3, G81…G89, G40…G42)
+G17:
+  meaning: Plane Select
+G17.1:
+  meaning: Plane Select
+G18:
+  meaning: Plane Select
+G18.1:
+  meaning: Plane Select
+G19:
+  meaning: Plane Select
+G19.1:
+  meaning: Plane Select
+# Cutter Radius Compensation
+G40:
+  meaning: Compensation Off
+G41:
+  meaning: Cutter Compensation
+  parameters: D
+G42:
+  meaning: Cutter Compensation
+  parameters: D
+G41.1:
+  meaning: Dynamic Cutter Compensation
+  parameters: D L
+G42.1:
+  meaning: Dynamic Cutter Compensation
+  parameters: D L
+# Path Control Mode
+G61.1:
+  meaning: Exact Path Mode
+G61.1:
+  meaning: Exact Path Mode
+G64:
+  meaning: Path Blending
+  parameters: P Q
+# Return Mode in Canned Cycles
+G98:
+  meaning: Canned Cycle Return Level
+G99:
+  meaning: Canned Cycle Return Level
+# Other Modal Codes
+F:
+  meaning: Set Feed Rate
+S:
+  meaning: Set Spindle Speed
+T:
+  meaning: Select Tool)
+M48, M49:
+  meaning: Speed and Feed Override Control
+M50:
+  meaning: Feed Override Control
+  parameters: P0 (off) or P1 (on)
+M51:
+  meaning: Spindle Speed Override Control
+  parameters: P0 (off) or P1 (on)
+M52:
+  meaning: Adaptive Feed Control
+  parameters: P0 (off) or P1 (on)
+M53:
+  meaning: Feed Stop Control
+  parameters: P0 (off) or P1 (on)
+G54-G59.3:
+  meaning: Select Coordinate System
+# Flow-control Codes
+## o sub:
+##   meaning: Subroutines, sub/endsub call
+## o while:
+##   meaning: Looping, while/endwhile do/while
+## o if:
+##   meaning: Conditional, if/else/endif
+## o repeat:
+##   meaning: Repeat a loop of code
+## '[]':
+##   meaning: Indirection
+## o call:
+##   meaning: Call named file
+M70:
+  meaning: Save modal state
+M71:
+  meaning: Invalidate stored state
+M72:
+  meaning: Restore modal state
+M73:
+  meaning: Save and Auto-restore modal state
+# Input/Output Codes
+M62:
+  meaning: Digital Output Control
+M63:
+  meaning: Digital Output Control
+M64:
+  meaning: Digital Output Control
+M65:
+  meaning: Digital Output Control
+  parameters: P
+M66:
+  meaning: Wait on Input
+  parameters: P E L Q
+M67:
+  meaning: Analog Output,Synchronized
+  parameters: T
+M68:
+  meaning: Analog Output, Immediate
+  parameters: T
+# Non-modal Codes
+M6:
+  meaning: Tool Change
+  parameters: T
+M61:
+  meaning: Set Current Too
+  l # Q
+G10 L1:
+  meaning: Set Tool Table
+  parameters: P Q R
+G10 L10:
+  meaning: Set Tool Table
+  parameters: P
+G10 L11:
+  meaning: Set Tool Table
+  parameters: P
+G10 L2:
+  meaning: Set Coordinate System
+  parameters: P R
+G10 L20:
+  meaning: Set Coordinate System
+  parameters: P
+G28:
+  meaning: Go/Set Predefined Position
+G28.1:
+  meaning: Go/Set Predefined Position
+G30:
+  meaning: Go/Set Predefined Position
+G30.1:
+  meaning: Go/Set Predefined Position
+G53:
+  meaning: Move in Machine Coordinates
+G92:
+  meaning: Coordinate System Offset
+G92.1:
+  meaning: Reset G92 Offsets
+G92.2:
+  meaning: Reset G92 Offsets
+G92.3:
+  meaning: Restore G92 Offsets
+M101 - M199: # Don't expand !
+  meaning: User Defined Commands
+  parameters: P Q
+S:
+  meaning: Set spindle speed
+T:
+  meaning: Select tool
diff --git a/PythonicGcodeMachine/Gcode/MachineKit/__init__.py b/PythonicGcodeMachine/Gcode/MachineKit/__init__.py
new file mode 100644
index 0000000000000000000000000000000000000000..37fdd45a0d6bed35fad763c9e5dbb87020fe76cb
--- /dev/null
+++ b/PythonicGcodeMachine/Gcode/MachineKit/__init__.py
@@ -0,0 +1,384 @@
+####################################################################################################
+#
+# PythonicGcodeMachine - @licence_header_description@
+# Copyright (C) 2018 Fabrice Salvaire
+#
+# This program is free software: you can redistribute it and/or modify
+# it under the terms of the GNU General Public License as published by
+# the Free Software Foundation, either version 3 of the License, or
+# (at your option) any later version.
+#
+# This program is distributed in the hope that it will be useful,
+# but WITHOUT ANY WARRANTY; without even the implied warranty of
+# MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE.  See the
+# GNU General Public License for more details.
+#
+# You should have received a copy of the GNU General Public License
+# along with this program.  If not, see <http://www.gnu.org/licenses/>.
+#
+####################################################################################################
+
+"""Module to implement the G-code language.
+
+History
+-------
+
+The G-code language, also called RS-274, is a programming language for numerical control.  It was
+developed by the EIA in the early 1960s, and finally standardised by ISO in February 1980 as RS274D
+/ ISO 6983.
+
+The G-code language has several flavours and historical versions. A list of reference documents
+follows :
+
+* The NIST RS274NGC Interpreter - Version 3, T. Kramer, F. Proctor, E. Messina, National Institute
+  of Standards and Technology, NISTIR 6556, August 17, 2000
+* The documentation of the `Linux CNC <http://linuxcnc.org>`_ project, formerly Enhanced Machine
+  Controller developed at NIST,
+* EIA Standard RS-274-D Interchangeable Variable Block Data Format for Positioning, Contouring, and
+  Contouring/Positioning Numerically Controlled Machines, 2001 Eye Street, NW, Washington,
+  D.C. 20006: Electronic Industries Association, February 1979
+
+Overview
+--------
+
+The RS274/NGC language is based on lines of code. Each line (also called a “block”) may include
+commands to a machining center to do several different things.
+
+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,
+:code:`G1 X3` is a valid line of code with two words. :code:`G1` is a command meaning “move in a
+straight line at the programmed feed rate,” and :code:`X3` provides an argument value (the value of
+X should be 3 at the end of the move). Most RS274/NGC commands start with either G or M (for
+miscellaneous). The words for these commands are called “G codes” and “M codes.”
+
+Language View of a Machining Center
+-----------------------------------
+
+Parameters
+~~~~~~~~~~
+
+In the RS274/NGC language view, a machining center maintains an array of 5400 numerical
+parameters. Many of them have specific uses. The parameter array should persist over time, even if
+the machining center is powered down.
+
+Coordinate Systems
+~~~~~~~~~~~~~~~~~~
+
+In the RS274/NGC language view, a machining center has an absolute coordinate system and nine
+program coordinate systems.
+
+You can set the offsets of the nine program coordinate systems using G10 L2 Pn (n is the number of
+the coordinate system) with values for the axes in terms of the absolute coordinate system.
+
+You can select one of the nine systems by using G54, G55, G56, G57, G58, G59, G59.1, G59.2, or
+G59.3. It is not possible to select the absolute coordinate system directly. You can offset the
+current coordinate system using G92 or G92.3. This offset will then apply to all nine program
+coordinate systems. This offset may be cancelled with G92.1 or G92.2.
+
+You can make straight moves in the absolute machine coordinate system by using G53 with either G0 or
+G1.
+
+Data for coordinate systems is stored in parameters.
+
+During initialization, the coordinate system is selected that is specified by parameter 5220. A
+value of 1 means the first coordinate system (the one G54 activates), a value of 2 means the second
+coordinate system (the one G55 activates), and so on. It is an error for the value of parameter 5220
+to be anything but a whole number between one and nine.
+
+Format of a Line
+----------------
+
+A permissible line of input RS274/NGC 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 :code:`/` .
+#. an optional line number.
+#. any number of words, parameter settings, and comments.
+#. an end of line marker (carriage return or line feed or both).
+
+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 :code:`g0x +0. 12 34y
+7` is equivalent to :code:`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.
+
+Line Number
+~~~~~~~~~~~
+
+A line number is the letter :code:`N` followed by an integer (with no sign) between 0 and 99999
+written with no more than five digits (000009 is not OK, for example). Line numbers 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
+~~~~
+
+A word is a letter other than :code:`N` followed by a real value.
+
+Words may begin with any of the letters shown in the following table. The table includes :code:`N`
+for completeness, even though, as defined above, line numbers are not words. Several letters
+(:code:`I`, :code:`J, K`, :code:`L`, :code:`P`, :code:`R`) may have different meanings in different
+contexts.
+
+Table. Linux CNC Words and their meanings Letter
+
+====== =====================================================
+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 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
+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 Modal Groups)
+N       Line number
+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
+====== =====================================================
+
+A real value is some collection of characters that can be processed to come up with a number. A real
+value may be an explicit number (such as 341 or -0.8807), a parameter value, an expression, or a
+unary operation value.
+
+Number
+~~~~~
+
+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 (1) an optional plus or minus sign, followed by (2) zero to many digits,
+  followed, possibly, by (3) one decimal point, followed by (4) zero to many digits — provided that
+  there is at least one digit somewhere in the number.
+* There are two kinds of numbers: integers and decimals. An integer does not have a decimal point in
+  it; a decimal does.
+* Numbers may have any number of digits, subject to the limitation on line length.
+* A non-zero number with no sign as 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.
+
+Parameter Value
+~~~~~~~~~~~~~~~
+
+A parameter value is the pound character :code:`#` followed by a real value. The real value must
+evaluate to an integer between 1 and 5399. The integer is a parameter number, and the value of the
+parameter value is whatever number is stored in the numbered parameter.
+
+The :code:`#` character takes precedence over other operations, so that, for example, :code:`#1+2`
+means the number found by adding 2 to the value of parameter 1, not the value found in parameter
+3. Of course, :code:`#[1+2]` does mean the value found in parameter 3. The :code:`#` character may
+be repeated; for example :code:`##2` means the value of the parameter whose index is the (integer)
+value of parameter 2.
+
+Expressions and Binary Operations
+~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+An expression is a set of characters starting with a left bracket :code:`[` and ending with a
+balancing right bracket :code:`]`. In between the brackets are numbers, parameter values,
+mathematical operations, and other expressions. An expression may be 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 :code:`[ 1 + acos[0] - [#3 ** [4.0/2]]]`.
+
+Binary operations appear only inside expressions. Nine binary operations are defined. There are four
+basic mathematical operations: addition :code:`+`, subtraction :code:`-`, multiplication :code:`*`,
+and division :code:`/`. There are three logical operations: non-exclusive or :code:`OR`, exclusive
+or :code:`XOR`, and logical and :code:`AND`. The eighth operation is the modulus operation
+:code:`MOD`. The ninth operation is the “power” operation :code:`**` of raising the number on the
+left of the operation to the power on the right.  The binary operations are divided into three
+groups. The first group is: power. The second group is: multiplication, division, and modulus. The
+third group is: addition, subtraction, logical non- exclusive or, logical exclusive or, and logical
+and. If operations are strung together (for example in the expression :code:`[2.0 / 3 * 1.5 - 5.5 /
+11.0]`), operations in the first group are to be performed before operations in the second group and
+operations in the second group before operations in the third 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: :code:`[((2.0 / 3) * 1.5) - (5.5 /
+11.0)]`, which simplifies to :code:`[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.
+
+Unary Operation Value
+~~~~~~~~~~~~~~~~~~~~~
+
+A unary operation value is either :code:`ATAN` followed by one expression divided by another
+expression (for example :code:`ATAN[2]/[1+3]`) or any other unary operation name followed by an
+expression (for example :code:`SIN[90]`). The unary operations are: :code:`ABS` (absolute value),
+:code:`ACOS` (arc cosine), :code:`ASIN` (arc sine), :code:`ATAN` (arc tangent), :code:`COS`
+(cosine), :code:`EXP` (e raised to the given power), :code:`FIX` (round down), :code:`FUP` (round
+up), :code:`LN` (natural logarithm), :code:`ROUND` (round to the nearest whole number), :code:`SIN`
+(sine), :code:`SQRT` (square root), and :code:`TAN` (tangent). Arguments to unary operations which
+take angle measures (:code:`COS`, :code:`SIN`, and :code:`TAN`) are in degrees. Values returned by
+unary operations which return angle measures (:code:`ACOS`, :code:`ASIN`, and :code:`ATAN`) are also
+in degrees.
+
+The :code:`FIX` operation rounds towards the left (less positive or more negative) on a number line,
+so that :code:`FIX[2.8] = 2` and :code:`FIX[-2.8] = -3`, for example. The :code:`FUP` operation
+rounds towards the right (more positive or less negative) on a number line; :code:`FUP[2.8] = 3` and
+:code:`FUP[-2.8] = -2`, for example.
+
+Parameter Setting
+~~~~~~~~~~~~~~~~~
+
+A parameter setting is the following four items one after the other: (1) a pound character
+:code:`#`, (2) a real value which evaluates to an integer between 1 and 5399, (3) an equal sign
+:code:`=`, and (4) a real value. For example :code:`#3 = 15` is a parameter setting meaning “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 :code:`#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.
+
+Comments and Messages
+~~~~~~~~~~~~~~~~~~~~~
+
+Printable characters and white space inside parentheses is a comment. A left parenthesis always
+starts a comment. The comment ends at the first right parenthesis found thereafter. Once a left
+parenthesis is placed on a line, a matching right parenthesis must appear before the end of the
+line.  Comments may not be nested; it is an error if a left parenthesis is found after the start of
+a comment and before the end of the comment. Here is an example of a line containing a comment:
+:code:`G80 M5 (stop motion)`. Comments do not cause a machining center to do anything.
+
+.. A comment contains a 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. Comments not containing messages need
+  not be displayed there.
+
+Item Repeats
+~~~~~~~~~~~~
+
+A line may have any number of :code:`G` words, but two :code:`G` words from the same modal group may
+not appear on the same line.
+
+A line may have zero to four :code:`M` words. Two :code:`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, :code:`#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 :code:`#3=15 #3=6` has been interpreted, the
+value of parameter 3 will be 6. If the order is reversed to :code:`#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
+:code:`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 :code:`#4=-7.0 g1 #3=15 g40 (foo)`) for the five items.
+
+Commands and Machine Modes
+~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+In RS274/NGC, many commands cause a machining center 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 :code:`G` codes for motion are also modal. If a :code:`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
+cancelling motion.
+
+“Non-modal” codes have effect only on the lines on which they occur. For example, :code:`G4` (dwell)
+is non-modal.
+
+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 Table 4.
+
+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 :code:`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 :code:`G10`, :code:`G28`, :code:`G30`, and :code:`G92`.
+
+G and Input Codes
+-----------------
+
+See ...
+
+..
+  G codes of the RS274/NGC language are shown in Table 5 and described following that.
+
+  In the command prototypes, three dots (...) stand for a real value. As described earlier, a real
+  value may be (1) an explicit number, 4, for example, (2) an expression, :code:`[2+2]`, for example,
+  (3) a parameter value, #88, for example, or (4) a unary function value, :code:`acos[0]`, for
+  example.  In most cases, if axis words (any or all of X..., Y..., Z..., A..., B..., C...) are given,
+  they specify a destination point. Axis numbers are in the currently active coordinate system, unless
+  explicitly described as being in the absolute coordinate system. Where axis words are optional, any
+  omitted axes will have their current value. Any items in the command prototypes not explicitly
+  described as optional are required. It is an error if a required item is omitted.
+
+  In the prototypes, the values following letters are often given as explicit numbers. Unless stated
+  otherwise, the explicit numbers can be real values. For example, :code:`G10 L2` could equally well
+  be written :code:`G[2*5] L[1+1]`. If the value of parameter 100 were 2, :code:`G10 L#100` would also
+  mean the same. Using real values which are not explicit numbers as just shown in the examples is
+  rarely useful.
+
+  If L... is written in a prototype the “...” will often be referred to as the “L number”. Similarly the
+  “...” in H... may be called the “H number”, and so on for any other letter.
+
+Order of Execution
+------------------
+
+The order of execution of items on a line is critical to safe and effective machine operation. Items
+are executed in a particular order if they occur on the same line.
+
+"""
diff --git a/PythonicGcodeMachine/Gcode/Lexer.py b/PythonicGcodeMachine/Gcode/Rs274/Lexer.py
similarity index 100%
rename from PythonicGcodeMachine/Gcode/Lexer.py
rename to PythonicGcodeMachine/Gcode/Rs274/Lexer.py
diff --git a/PythonicGcodeMachine/Gcode/Parser.py b/PythonicGcodeMachine/Gcode/Rs274/Parser.py
similarity index 100%
rename from PythonicGcodeMachine/Gcode/Parser.py
rename to PythonicGcodeMachine/Gcode/Rs274/Parser.py
diff --git a/PythonicGcodeMachine/Gcode/Rs274/__init__.py b/PythonicGcodeMachine/Gcode/Rs274/__init__.py
new file mode 100644
index 0000000000000000000000000000000000000000..37fdd45a0d6bed35fad763c9e5dbb87020fe76cb
--- /dev/null
+++ b/PythonicGcodeMachine/Gcode/Rs274/__init__.py
@@ -0,0 +1,384 @@
+####################################################################################################
+#
+# PythonicGcodeMachine - @licence_header_description@
+# Copyright (C) 2018 Fabrice Salvaire
+#
+# This program is free software: you can redistribute it and/or modify
+# it under the terms of the GNU General Public License as published by
+# the Free Software Foundation, either version 3 of the License, or
+# (at your option) any later version.
+#
+# This program is distributed in the hope that it will be useful,
+# but WITHOUT ANY WARRANTY; without even the implied warranty of
+# MERCHANTABILITY or FITNESS FOR A PARTICULAR PURPOSE.  See the
+# GNU General Public License for more details.
+#
+# You should have received a copy of the GNU General Public License
+# along with this program.  If not, see <http://www.gnu.org/licenses/>.
+#
+####################################################################################################
+
+"""Module to implement the G-code language.
+
+History
+-------
+
+The G-code language, also called RS-274, is a programming language for numerical control.  It was
+developed by the EIA in the early 1960s, and finally standardised by ISO in February 1980 as RS274D
+/ ISO 6983.
+
+The G-code language has several flavours and historical versions. A list of reference documents
+follows :
+
+* The NIST RS274NGC Interpreter - Version 3, T. Kramer, F. Proctor, E. Messina, National Institute
+  of Standards and Technology, NISTIR 6556, August 17, 2000
+* The documentation of the `Linux CNC <http://linuxcnc.org>`_ project, formerly Enhanced Machine
+  Controller developed at NIST,
+* EIA Standard RS-274-D Interchangeable Variable Block Data Format for Positioning, Contouring, and
+  Contouring/Positioning Numerically Controlled Machines, 2001 Eye Street, NW, Washington,
+  D.C. 20006: Electronic Industries Association, February 1979
+
+Overview
+--------
+
+The RS274/NGC language is based on lines of code. Each line (also called a “block”) may include
+commands to a machining center to do several different things.
+
+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,
+:code:`G1 X3` is a valid line of code with two words. :code:`G1` is a command meaning “move in a
+straight line at the programmed feed rate,” and :code:`X3` provides an argument value (the value of
+X should be 3 at the end of the move). Most RS274/NGC commands start with either G or M (for
+miscellaneous). The words for these commands are called “G codes” and “M codes.”
+
+Language View of a Machining Center
+-----------------------------------
+
+Parameters
+~~~~~~~~~~
+
+In the RS274/NGC language view, a machining center maintains an array of 5400 numerical
+parameters. Many of them have specific uses. The parameter array should persist over time, even if
+the machining center is powered down.
+
+Coordinate Systems
+~~~~~~~~~~~~~~~~~~
+
+In the RS274/NGC language view, a machining center has an absolute coordinate system and nine
+program coordinate systems.
+
+You can set the offsets of the nine program coordinate systems using G10 L2 Pn (n is the number of
+the coordinate system) with values for the axes in terms of the absolute coordinate system.
+
+You can select one of the nine systems by using G54, G55, G56, G57, G58, G59, G59.1, G59.2, or
+G59.3. It is not possible to select the absolute coordinate system directly. You can offset the
+current coordinate system using G92 or G92.3. This offset will then apply to all nine program
+coordinate systems. This offset may be cancelled with G92.1 or G92.2.
+
+You can make straight moves in the absolute machine coordinate system by using G53 with either G0 or
+G1.
+
+Data for coordinate systems is stored in parameters.
+
+During initialization, the coordinate system is selected that is specified by parameter 5220. A
+value of 1 means the first coordinate system (the one G54 activates), a value of 2 means the second
+coordinate system (the one G55 activates), and so on. It is an error for the value of parameter 5220
+to be anything but a whole number between one and nine.
+
+Format of a Line
+----------------
+
+A permissible line of input RS274/NGC 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 :code:`/` .
+#. an optional line number.
+#. any number of words, parameter settings, and comments.
+#. an end of line marker (carriage return or line feed or both).
+
+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 :code:`g0x +0. 12 34y
+7` is equivalent to :code:`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.
+
+Line Number
+~~~~~~~~~~~
+
+A line number is the letter :code:`N` followed by an integer (with no sign) between 0 and 99999
+written with no more than five digits (000009 is not OK, for example). Line numbers 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
+~~~~
+
+A word is a letter other than :code:`N` followed by a real value.
+
+Words may begin with any of the letters shown in the following table. The table includes :code:`N`
+for completeness, even though, as defined above, line numbers are not words. Several letters
+(:code:`I`, :code:`J, K`, :code:`L`, :code:`P`, :code:`R`) may have different meanings in different
+contexts.
+
+Table. Linux CNC Words and their meanings Letter
+
+====== =====================================================
+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 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
+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 Modal Groups)
+N       Line number
+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
+====== =====================================================
+
+A real value is some collection of characters that can be processed to come up with a number. A real
+value may be an explicit number (such as 341 or -0.8807), a parameter value, an expression, or a
+unary operation value.
+
+Number
+~~~~~
+
+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 (1) an optional plus or minus sign, followed by (2) zero to many digits,
+  followed, possibly, by (3) one decimal point, followed by (4) zero to many digits — provided that
+  there is at least one digit somewhere in the number.
+* There are two kinds of numbers: integers and decimals. An integer does not have a decimal point in
+  it; a decimal does.
+* Numbers may have any number of digits, subject to the limitation on line length.
+* A non-zero number with no sign as 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.
+
+Parameter Value
+~~~~~~~~~~~~~~~
+
+A parameter value is the pound character :code:`#` followed by a real value. The real value must
+evaluate to an integer between 1 and 5399. The integer is a parameter number, and the value of the
+parameter value is whatever number is stored in the numbered parameter.
+
+The :code:`#` character takes precedence over other operations, so that, for example, :code:`#1+2`
+means the number found by adding 2 to the value of parameter 1, not the value found in parameter
+3. Of course, :code:`#[1+2]` does mean the value found in parameter 3. The :code:`#` character may
+be repeated; for example :code:`##2` means the value of the parameter whose index is the (integer)
+value of parameter 2.
+
+Expressions and Binary Operations
+~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+An expression is a set of characters starting with a left bracket :code:`[` and ending with a
+balancing right bracket :code:`]`. In between the brackets are numbers, parameter values,
+mathematical operations, and other expressions. An expression may be 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 :code:`[ 1 + acos[0] - [#3 ** [4.0/2]]]`.
+
+Binary operations appear only inside expressions. Nine binary operations are defined. There are four
+basic mathematical operations: addition :code:`+`, subtraction :code:`-`, multiplication :code:`*`,
+and division :code:`/`. There are three logical operations: non-exclusive or :code:`OR`, exclusive
+or :code:`XOR`, and logical and :code:`AND`. The eighth operation is the modulus operation
+:code:`MOD`. The ninth operation is the “power” operation :code:`**` of raising the number on the
+left of the operation to the power on the right.  The binary operations are divided into three
+groups. The first group is: power. The second group is: multiplication, division, and modulus. The
+third group is: addition, subtraction, logical non- exclusive or, logical exclusive or, and logical
+and. If operations are strung together (for example in the expression :code:`[2.0 / 3 * 1.5 - 5.5 /
+11.0]`), operations in the first group are to be performed before operations in the second group and
+operations in the second group before operations in the third 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: :code:`[((2.0 / 3) * 1.5) - (5.5 /
+11.0)]`, which simplifies to :code:`[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.
+
+Unary Operation Value
+~~~~~~~~~~~~~~~~~~~~~
+
+A unary operation value is either :code:`ATAN` followed by one expression divided by another
+expression (for example :code:`ATAN[2]/[1+3]`) or any other unary operation name followed by an
+expression (for example :code:`SIN[90]`). The unary operations are: :code:`ABS` (absolute value),
+:code:`ACOS` (arc cosine), :code:`ASIN` (arc sine), :code:`ATAN` (arc tangent), :code:`COS`
+(cosine), :code:`EXP` (e raised to the given power), :code:`FIX` (round down), :code:`FUP` (round
+up), :code:`LN` (natural logarithm), :code:`ROUND` (round to the nearest whole number), :code:`SIN`
+(sine), :code:`SQRT` (square root), and :code:`TAN` (tangent). Arguments to unary operations which
+take angle measures (:code:`COS`, :code:`SIN`, and :code:`TAN`) are in degrees. Values returned by
+unary operations which return angle measures (:code:`ACOS`, :code:`ASIN`, and :code:`ATAN`) are also
+in degrees.
+
+The :code:`FIX` operation rounds towards the left (less positive or more negative) on a number line,
+so that :code:`FIX[2.8] = 2` and :code:`FIX[-2.8] = -3`, for example. The :code:`FUP` operation
+rounds towards the right (more positive or less negative) on a number line; :code:`FUP[2.8] = 3` and
+:code:`FUP[-2.8] = -2`, for example.
+
+Parameter Setting
+~~~~~~~~~~~~~~~~~
+
+A parameter setting is the following four items one after the other: (1) a pound character
+:code:`#`, (2) a real value which evaluates to an integer between 1 and 5399, (3) an equal sign
+:code:`=`, and (4) a real value. For example :code:`#3 = 15` is a parameter setting meaning “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 :code:`#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.
+
+Comments and Messages
+~~~~~~~~~~~~~~~~~~~~~
+
+Printable characters and white space inside parentheses is a comment. A left parenthesis always
+starts a comment. The comment ends at the first right parenthesis found thereafter. Once a left
+parenthesis is placed on a line, a matching right parenthesis must appear before the end of the
+line.  Comments may not be nested; it is an error if a left parenthesis is found after the start of
+a comment and before the end of the comment. Here is an example of a line containing a comment:
+:code:`G80 M5 (stop motion)`. Comments do not cause a machining center to do anything.
+
+.. A comment contains a 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. Comments not containing messages need
+  not be displayed there.
+
+Item Repeats
+~~~~~~~~~~~~
+
+A line may have any number of :code:`G` words, but two :code:`G` words from the same modal group may
+not appear on the same line.
+
+A line may have zero to four :code:`M` words. Two :code:`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, :code:`#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 :code:`#3=15 #3=6` has been interpreted, the
+value of parameter 3 will be 6. If the order is reversed to :code:`#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
+:code:`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 :code:`#4=-7.0 g1 #3=15 g40 (foo)`) for the five items.
+
+Commands and Machine Modes
+~~~~~~~~~~~~~~~~~~~~~~~~~~
+
+In RS274/NGC, many commands cause a machining center 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 :code:`G` codes for motion are also modal. If a :code:`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
+cancelling motion.
+
+“Non-modal” codes have effect only on the lines on which they occur. For example, :code:`G4` (dwell)
+is non-modal.
+
+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 Table 4.
+
+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 :code:`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 :code:`G10`, :code:`G28`, :code:`G30`, and :code:`G92`.
+
+G and Input Codes
+-----------------
+
+See ...
+
+..
+  G codes of the RS274/NGC language are shown in Table 5 and described following that.
+
+  In the command prototypes, three dots (...) stand for a real value. As described earlier, a real
+  value may be (1) an explicit number, 4, for example, (2) an expression, :code:`[2+2]`, for example,
+  (3) a parameter value, #88, for example, or (4) a unary function value, :code:`acos[0]`, for
+  example.  In most cases, if axis words (any or all of X..., Y..., Z..., A..., B..., C...) are given,
+  they specify a destination point. Axis numbers are in the currently active coordinate system, unless
+  explicitly described as being in the absolute coordinate system. Where axis words are optional, any
+  omitted axes will have their current value. Any items in the command prototypes not explicitly
+  described as optional are required. It is an error if a required item is omitted.
+
+  In the prototypes, the values following letters are often given as explicit numbers. Unless stated
+  otherwise, the explicit numbers can be real values. For example, :code:`G10 L2` could equally well
+  be written :code:`G[2*5] L[1+1]`. If the value of parameter 100 were 2, :code:`G10 L#100` would also
+  mean the same. Using real values which are not explicit numbers as just shown in the examples is
+  rarely useful.
+
+  If L... is written in a prototype the “...” will often be referred to as the “L number”. Similarly the
+  “...” in H... may be called the “H number”, and so on for any other letter.
+
+Order of Execution
+------------------
+
+The order of execution of items on a line is critical to safe and effective machine operation. Items
+are executed in a particular order if they occur on the same line.
+
+"""
diff --git a/PythonicGcodeMachine/Machine/data/make-yaml.py b/PythonicGcodeMachine/Gcode/Rs274/data/make-yaml.py
similarity index 100%
rename from PythonicGcodeMachine/Machine/data/make-yaml.py
rename to PythonicGcodeMachine/Gcode/Rs274/data/make-yaml.py
diff --git a/PythonicGcodeMachine/Machine/data/rs274-default-parameter-file.yaml b/PythonicGcodeMachine/Gcode/Rs274/data/rs274-default-parameter-file.yaml
similarity index 100%
rename from PythonicGcodeMachine/Machine/data/rs274-default-parameter-file.yaml
rename to PythonicGcodeMachine/Gcode/Rs274/data/rs274-default-parameter-file.yaml
diff --git a/PythonicGcodeMachine/Machine/data/rs274-execution-order.yaml b/PythonicGcodeMachine/Gcode/Rs274/data/rs274-execution-order.yaml
similarity index 100%
rename from PythonicGcodeMachine/Machine/data/rs274-execution-order.yaml
rename to PythonicGcodeMachine/Gcode/Rs274/data/rs274-execution-order.yaml
diff --git a/PythonicGcodeMachine/Machine/data/rs274-gcodes.yaml b/PythonicGcodeMachine/Gcode/Rs274/data/rs274-gcodes.yaml
similarity index 100%
rename from PythonicGcodeMachine/Machine/data/rs274-gcodes.yaml
rename to PythonicGcodeMachine/Gcode/Rs274/data/rs274-gcodes.yaml
diff --git a/PythonicGcodeMachine/Machine/data/rs274-modal-groups.yaml b/PythonicGcodeMachine/Gcode/Rs274/data/rs274-modal-groups.yaml
similarity index 100%
rename from PythonicGcodeMachine/Machine/data/rs274-modal-groups.yaml
rename to PythonicGcodeMachine/Gcode/Rs274/data/rs274-modal-groups.yaml
diff --git a/PythonicGcodeMachine/Machine/data/rs274-word-starting-letter.yaml b/PythonicGcodeMachine/Gcode/Rs274/data/rs274-word-starting-letter.yaml
similarity index 100%
rename from PythonicGcodeMachine/Machine/data/rs274-word-starting-letter.yaml
rename to PythonicGcodeMachine/Gcode/Rs274/data/rs274-word-starting-letter.yaml