Align types with gcode spec

[giannissc]

• Missing module-level documentation (see comments below)
• spindle -> speed
• common.py -> groups.py
• Create address.py with XYZ and IJK classes move print_xyz() and print_ijk()
• GCodeEnum -> GCodeAddress
• GCodeEnum.to_gcode() -> GCodeEnum.__repr__() and GCodeEnum._str_()
• Remove precision parameter and choose precision based on selected Unit address
• Introduce class FeedRate(GCodeEnum) and create print_feed()

[giannissc]

G-code Letter and Word Address Syntax (common.py)

G-code (also RS-274) is the most widely-used computer numerical control (CNC) programming language.
It is used mainly in computer-aided manufacturing to control automated machine tools, as well as from a 3D-printing slicer app.
Here we concentrate on a subset of G-code relevant for 3-axis CNC machining. Explanations of commands that are out of scope will be included for completeness and it will be indicated that they are out of scope.

A G-code command (word address) is formed by single letter (letter address) followed by 2 digits. Multiple G-code commands on the same line are called command blocks

 G 01 XYZ
⌊ ⌋  letter address
⌊   ⌋  word  address
⌊       ⌋  command block

G-code word addresses are used to configure the machine state and control the motors. The two primary letter addresses are M-codes and G-codes. M-codes are known as machine codes (or more accurately miscellaneous codes) and G-codes are called preparatory codes. M-codes allow for state changes of the machine components and the running program. G-codes control the motion of the motors and the internal configuration of the machine. In addition to the G and M address there are other letter addresses that are used in conjunction with them

Below is a comprehensive list of the available letter addresses:

• A <inch/mm> - 4th Axis: G0, G1, G2, G3 (out of scope)
• B <inch/mm> - 5th Axis: G0, G1, G2, G3 (out of scope)
• C <inch/mm> - 6th Axis: G0, G1, G2, G3 (out of scope)
• D <0-200> - Radius Offset: G41, G42
• E <0.0001-0.25>- Engraving Feed Rate: G187 (out of scope)
• G <0-187> - Preparatory Function:
• F <inch/mm> - Feed Rate: G1, G2, G3, G73, G74, G76, G81, G82, G83, G84, G85, G86, G87, G88, G89
• H <0-200> - Tool Length Offset: G43, G44
• I <inch/mm> - Arc Center in X Axis: G2, G3
• J <inch/mm> - Arc Center in Y Axis: G2, G3
• K <inch/mm> - Arc Center in Z Axis: G2, G3
• L <0-32767> - Canned Cycle Loop Count: G81, G82, G83, G84, G85, G86, G88, G89
• M <> - Miscllanesous Functions
• N <0-99999> - Number of Block
• O <0-99999> - Program Number
• P <0.001-1000.0> - Dwell Time: G4, G73, G76, G85, G86, G88, G89
• Q <0.001-100.0> - Canned Cycle Optional Data: G73, G76, G83, G87,
• R <inch/mm> - Circular Interpolation/Canned Cycle Data:, G73, G74, G76, G81, G82, G83, G84, G85, G86, G87, G88, G89
• S <1-99999> - Spindle Speed: M3, M4
• T <1-20>- Tool Selection: M6
• X <inch/mm> - X Axis: G0, G1, G2, G3
• Y <inch/mm> - Y Axis: G0, G1, G2, G3
• Z <inch/mm> - Y Axis: G0, G1, G2, G3

inch: 4 fractional positions
mm: 3 fractional positions

G-code commands can be categorized as modal or non-modal. Modal commands remain in effect until they are replaced or cancelled by another command. Non-modal commands execute in their block scope. M-code and G-code are further organized into modal groups

G-code Modal Groups:

• Group 0 - Non-modal codes: G4, G10 G28, G30, G52, G53, G92, G92.1, G92.2, G92.3
• Group 1 - Motion: G0, G1, G2, G3, G33, G38.n, G73, G74, G76, G80, G81, G82, G83, G84, G85, G86, G87, G88, G89
• Group 2 - Plane: G17, G18, G19, G17.1, G18.1, G19.1
• Group 3 - Distance Mode: G90, G91
• Group 4 - Arc Distance Mode: G90.1, G91.1
• Group 5 - Feed Rate Mode: G93, G94, G95
• Group 6 - Units: G20, G21
• Group 7 - Cutter Diameter Compensation: G40, G41, G42, G41.1, G42.1
• Group 8 - Tool Length Offset: G43, G43.1, G49
• Group 10 - Canned Cycle Return Mode: G98, G99
• Group 12 - Coordinate System: G54, G55, G56, G57, G58, G59, G59.1, G59.2, G59.3
• Group 13 - Planner Control Mode: G61, G61.1, G64
• Group 14 - Spindle Speed Mode: G96, G97

M-code Modal Groups:

• Group 4 - Stopping: M0, M1, M2, M30, M60
• Group 7 - Spindle: M3, M4, M5
• Group 8 - Coolant: M7, M8, M9

[giannissc]

G-code Block Syntax (command.py)

Letter Address Order:
N G X Y Z R P Q I J K F M S T

Word Address Groups:

• XYZ - End Position: G0, G1, G2, G3
• IJK - Center Position: G3, G3
• F - Feed Rate: G1, G2, G3

G-code Command Formats:

• G00 X<inch/mm> Y<inch/mm> Z<inch/mm>
• G01 X<inch/mm> Y<inch/mm> Z<inch/mm> F<inch/mm>

G02 X<inch/mm> Y<inch/mm> Z<inch/mm>            I<inch/mm> J<inch/mm> K<inch/mm> F<inch/mm> (preferred)
                                     R<inch/mm>                                  F<inch/mm>

• `G03 X<inch/mm> Y<inch/mm> Z<inch/mm> I<inch/mm> J<inch/mm> K<inch/mm> F<inch/mm> (preferred)
• `G03 X<inch/mm> Y<inch/mm> Z<inch/mm> R<inch/mm> F<inch/mm>
• `G04 P<0.001-1000.0>
• Fixed Cycle
  • `G73
  • `G74
  • `G76
  • `G80
• Canned Cycle

G98 G81 X<inch/mm> Y<inch/mm> Z<inch/mm> R<inch/mm>                 F<inch/mm>
G99 G82                                             P<0.001-1000.0>
    G83
    G84
    G85
    G86
    G87
    G88
    G89

[giannissc]

G-code Program Structure (fluent.py)

• Header/Prelude
  • Safety Block
  • Start Sequence
• Main
  • Tool Change
  • Operation
• Footer/Postlude
  • Stop Sequence
  • Home Position
  • Safety Block
  • Program End