giannissc
commented
1 year ago 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 blockG-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
spindle->speedcommon.py->groups.pyaddress.pywithXYZandIJKclasses moveprint_xyz()andprint_ijk()GCodeEnum->GCodeAddressGCodeEnum.to_gcode()->GCodeEnum.__repr__()andGCodeEnum._str_()precisionparameter and choose precision based on selected Unit addressclass FeedRate(GCodeEnum)and createprint_feed()