Programming Basics

The Ready Motion Controller uses the G CODE language. G-code is relatively easy to read. It consists of commands (which start with G, and some with M) followed by parameters. G0 moves as fast as the machine can go and is called “traverse”, G1 moves at the speed given by the F parameter and is called “feed rate”, G2 and G3 draw arcs, clockwise and counterclockwise. The expectation is that when the laser or spindle occurs during G1, G2 and G3, but not G0, which is why there’s no speed (“feed rate”) control for G0. Of the parameters, X, Y, A, B, C, D, E and Z are the coordinates to move to (usually absolute, but there’s a relative mode too), and, for arcs, I, J and K are the coordinates of the center. If a coordinate does not change during a move, it can be omitted (which is why you see almost no Z parameters). With some commands (G0 to G3 included), you don’t need to repeat the command on a new line if it’s the same as before: you can supply just the new set of parameters (coordinates, and maybe feed rate), which is why most of your lines are just X, Y, I, J and F. Linear moves would be just X and Y (and/or Z if moving vertically too, and/or F if speed has to change). Coordinates in various forms (“0”, “0.” and “0.0000” are all ok), But has line length limits of 70 characters.

G-CODE Overview

G-code Meaning Notes
F Defines feed rate.  Example: G1 X10 F100
G Address for preparatory commands G commands often tell the control what kind of motion is wanted
I Defines arc center in X axis for G02 or G03 arc commands. Also used as a parameter within some fixed cycles.
J Defines arc center in Y axis for G02 or G03 arc commands. Also used as a parameter within some fixed cycles.
K Defines arc center in Z axis for G02 or G03 arc commands. Also used as a parameter within some fixed cycles, equal to L address.
M Miscellaneous function Many M-codes call for machine functions
P Serves as parameter address for various G and M codes With G04, defines dwell time value
S Defines speed, either spindle speed laser frequency  Example: M3 S300
X Absolute or incremental position of X axis.  Example: G00 X1 F400
Y Absolute or incremental position of Y axis  Example: G00 Y1 F400
Z Absolute or incremental position of Z axis  Example: G00 Z1 F400
A Absolute or incremental position of A axis  Example: G00 A1 F400
B Absolute or incremental position of B axis  Example: G00 B1 F400
C Absolute or incremental position of C axis  Example: G00 C1 F400
D Absolute or incremental position of D axis  Example: G00 D1 F400
E Absolute or incremental position of E axis  Example: G00 E1 F400

Motion (G)

G-code Meaning Notes
G0/G00 Rapid positioning Switch to rapid linear motion mode (seek). Used to get the tool somewhere quickly without cutting — moves the machine as quickly as possible along each axis — an axis which needs less movement will finish before the others, so one cannot count on the movement being a straight line.
G1/G01 Linear interpolation Switch to linear motion at the current feed rate. Used to cut a straight line — the interpreter will determine the acceleration needed along each axis to ensure direct movement from the original to the destination point at no more than the current Feed rate (F see below).
G2/G02 Circular interpolation, clockwise Switch to clockwise arc mode. The interpreter will cut an arc or circle from the current position to the destination using the specified radius (R) or center (IJK location) at the current Feed rate (F see below) in the plane selected by G17/18/19 (see below).
G3/G03 Circular interpolation, counterclockwise Switch to anti-clockwise arc mode. Corollary to G02 above.
G4/G04 Dwell (pause) This should probably be calculated to be only one or two spindle rotations for best efficiency. Dwell time is expressed using a parameter (may be X, U, or P) which determines the time unit (seconds, milliseconds, &c.) P, for seconds, is supported and used by Ready Motion’s UI typically X and U express the duration in milliseconds.
G10 Set Work Coordinate Origin (and resultant Offsets) Coordinate system origin setting. This setting is persistent and expects the user to follow good practices and not manually move the machine, instead only using jogging commands via the interface or a pendant which works through the control system, or to have and use homing switches. Examples:

  • G10 P1 L20 — (which is the equivalent of G92 X0 Y0 Z0) for work co-ordinate system G54 (#P1)[7](#P2–#P6 are G55–G59 respectively) L2 sets the WCS offsets with regard to the machine zero. The current machine position does not matter when you use G10 L2.[8]
  • G10 Px L2 (by automatically setting the specified axes from the machine position data) to (re)set the persistent work coordinate offsets.[9] L20 sets the WCS offsets such that the current position becomes what you say in the axis words (X, Y, Z). The offsets depend on the current machine position.[10]

See Re: Move after Homing to a position for a discussion of this.

G17 Select the XY plane (for arcs)
G18 Select the XZ plane (for arcs)
G19 Select the YZ plane (for arcs)
G20 After this, units will be in inches Best practice: do this at the start of a program and nowhere else. The usual minimum increment in G20 is one ten-thousandth of an inch (0.0001″).
G21 After this, units will be in mm Best practice: do this at the start of a program and nowhere else. The usual minimum increment in G21 (one thousandth of a millimeter, .001 mm, that is, one micrometre).
G28 Go to Pre-Defined Position Takes an argument of an X Y Z coordinate for the intermediate point that the tool tip will pass through on its way home to machine zero. v0.7 “Incorrectly performed the homing cycle”[11]Usually used to park the machine.[12]

http://www.cnccookbook.com/CCCNCGCodeG28ReturntoReference.htm

G30 Go to Pre-Defined Position (Return to secondary home position) Takes a P address specifying which machine zero point is desired, if the machine has several secondary points (P1 to P4). Takes X Y Z addresses which define the intermediate point that the tool tip will pass through on its way home to machine zero. v0.7 “Incorrectly performed the homing cycle”[13]Usually used to park the machine.[14] c.f., G28 above.
G30.1 Set Pre-Defined Position Stores the current absolute position.
G38.1 Probe cycle Using a Touch Plate
G38.2 Straight Probe Probe toward workpiece, stop on contact, signal error if failure
G38.3 Probe Probe toward workpiece, stop on contact
G38.4 Probe Probe away from workpiece, stop on loss of contact, signal error if failure
G38.5 Probe Probe away from workpiece, stop on loss of contact
G43.1 Dynamic tool length offset Change subsequent motions by offsetting the Z and/or X offsets stored in the tool table. Does not cause any motion, but will be applied the next time a compensated axis is moved, that axis’s endpoint will be the compensated location. See G38.1 above for a link which discusses using this.[15]
G49 Cancel tool offset. Cancels tool offset set by G43 or G44
G53 Absolute mode override Move in Machine Coordinates. Preface to a movement command on the same line which causes the machine to disregard any coordinate system which is in effect. G53 G0 X0 Y0 Z0 will return to the machine home / origin. Useful to move the tool relative to the machine, e.g., for tool changes.
G54–G59 Work Coordinate Systems Fixture offset 1–6.
G61 Exact path control mode This is the default path mode Ready Motion run in.
G80 Motion mode cancel Canned cycle
G90 Switch to absolute distance mode Coordinates are now relative to the origin of the currently active coordinate system, as opposed to the current position. G0 X-10 Y5 will move to the position 10 units to the left and 5 above the origin X0,Y0. cf. G91 below.
G91 Switch to incremental distance mode Coordinates are now relative to the current position, with no consideration for machine origin. G0 X-10 Y5 will move to the position 10 units to the left and 5 above the current position. cf. G90 above.
G92 Coordinate offset. Change the current coordinates without moving e.g. “G92 x0 y0 z0” makes the current position a temporary home position. The intent is to allow one to re-use code (say for a part when doing multiples) which has a given origin. The temporary origin can then be cleared and the actual machine origin, set via G10 restored by the command below.[21]
G92.1 Clear (temporary) Coordinate System Offsets Previously set by G92 (see above).
G93 Set inverse time feed rate mode An F word is interpreted to mean that the move should be completed in (one divided by the F number) minutes. For example, if F is 2, the move should be completed in half a minute
G94 Set units per minute feed rate mode An F Word is interpreted to mean the controlled point should move at a certain number of units (or degrees) per minute

Feed Rate (F)

F-code Meaning Notes
F Defines feed rate Unit used is that set by G20 or G21 (see above). The Feed setting in the G-Code determines the maximum rate at which the motor can rotate when moving a given distance so as to get up to (but not exceed) the Feed rate and the maximum acceleration limit which is set in Ready Motion’s UI. It can be on a separate line or on the same line as a G1/G2/G3 command.

Machine Options (M)

M-code Meaning Notes
M0 Program Pause and End Stops the machine so you can change the tool
M2 Program Pause and End Reset Program Flow
 Spindle and Laser Control
M16 Turn on Output 0 Spindle and Laser Control
M17 Turn off Output 0 Spindle and Laser Control
M18 / M7 Turn on Output 1 Spindle and Laser Control / Mist Coolant
M19 / M9 Turn off Output 1 Spindle and Laser Control / Mist Off
M20 Turn on Output 2 Spindle and Laser Control
M21 Turn off Output 2 Spindle and Laser Control
M22 / M8 Turn on Output 3 Spindle and Laser Control / Coolant On
M23 / M9 Turn off Output 3 Spindle and Laser Control / Coolant Off
M24 Turn on Output 4 Spindle and Laser Control
M25 Turn off Output 4 Spindle and Laser Control
M26 / M4 Turn on Output 5 Spindle and Laser Control / Spindle On (counterclockwise rotation)
M2 / M3 Turn off Output 5 Spindle and Laser Control / Spindle On (clockwise rotation)
M28 Turn on Output 6 Spindle and Laser Control
M29 Turn off Output 6 Spindle and Laser Control
M30 Turn on Output 7 Spindle and Laser Control
M31 Turn off Output 7 Spindle and Laser Control
Output Block 2
M32 Turn on Output 0 Output Block 2
M33 Turn off Output 0 Output Block 2
M34 Turn on Output 1 Output Block 2
M35 Turn off Output 1 Output Block 2
M36 Turn on Output 2 Output Block 2
M37 Turn off Output 2 Output Block 2
M38 Turn on Output 3 Output Block 2
M39 Turn off Output 3 Output Block 2
M40 Turn on Output 4 Output Block 2
M41 Turn off Output 4 Output Block 2
M42 Turn on Output 5 Output Block 2
M43 Turn off Output 5 Output Block 2
M44 Turn on Output 6 Output Block 2
M45 Turn off Output 6 Output Block 2
M46 Turn on Output 7 Output Block 2
M47 Turn off Output 7 Output Block 2
Output Block 3
M48 Turn on Output 0 Output Block 3
M49 Turn off Output 0 Output Block 3
M50 Turn on Output 1 Output Block 3
M51 Turn off Output 1 Output Block 3
M52 Turn on Output 2 Output Block 3
M53 Turn off Output 2 Output Block 3
M54 Turn on Output 3 Output Block 3
M55 Turn off Output 3 Output Block 3
M56 Turn on Output 4 Output Block 3
M57 Turn off Output 4 Output Block 3
M58 Turn on Output 5 Output Block 3
M59 Turn off Output 5 Output Block 3
M60 Turn on Output 6 Output Block 3
M61 Turn off Output 6 Output Block 3
M62 Turn on Output 7 Output Block 3
M63 Turn off Output 7 Output Block 3
Output Block 5
M64 Turn on Output 0 Output Block 5
M65 Turn off Output 0 Output Block 5
M66 Turn on Output 1 Output Block 5
M67 Turn off Output 1 Output Block 5
M68 Turn on Output 2 Output Block 5
M69 Turn off Output 2 Output Block 5
M70 Turn on Output 3 Output Block 5
M71 Turn off Output 3 Output Block 5
M72 Turn on Output 4 Output Block 5
M73 Turn off Output 4 Output Block 5
M74 Turn on Output 5 Output Block 5
M75 Turn off Output 5 Output Block 5
M76 Turn on Output 6 Output Block 5
M77 Turn off Output 6 Output Block 5
M78 Turn on Output 7 Output Block 5
M79 Turn off Output 7 Output Block 5

Program Commands

Code Meaning Notes
() Comments (Here is a comment)
$$ Configuration View Machine Configuration
$# Configuration View # Parameter
$G Configuration View Parser State
$I Configuration View Build Info
$N Configuration View Startup Blocks
$x=value Configuration Save Machine Setting
$Nx=line Configuration Save Startup Block
$C Configuration Check Gcode Mode
$X Configuration Kill Alarm Lock
$H Configuration Run Homing Cycle
~ Configuration Cycle Start
! Configuration Feed Hold
? Configuration Current Status
ctrl-x Configuration Reset
$ Configuring For better detail of configuring commands please check out Configuring-Grbl-v0.9
$0 Configuration step pulse, usec
$1 Configuration step idle delay, msec
$2 Configuration step port invert mask:00000000
$3 Configuration dir port invert mask:0000000
$4 Configuration step enable invert, bool
$5 Configuration limit pins invert, bool
$6 Configuration probe pin invert, bool (TESTING STILL)
$10 Configuration status report mask:00000011
$11 Configuration junction deviation, mm
$12 Configuration arc tolerance, mm
$13 Configuration report inches, bool
$20 Configuration soft limits, bool
$21 Configuration hard limits, bool
$22 Configuration homing cycle, bool
$23 Configuration homing dir invert mask:00000000
$24 Configuration homing feed, mm/min
$25 Configuration homing seek, mm/min
$26 Configuration homing debounce, msec
$27 Configuration homing pull-off, mm
$100 Configuration x, step/mm
$101 Configuration y, step/mm
$102 Configuration z, step/mm
$103 Configuration a, step/mm
$104 Configuration b, step/mm
$105 Configuration c, step/mm
$106 Configuration d, step/mm
$107 Configuration e, step/mm
$110 Configuration x max rate, mm/min
$111 Configuration y max rate, mm/min
$112 Configuration z max rate, mm/min
$113 Configuration a max rate, mm/min
$114 Configuration b max rate, mm/min
$115 Configuration c max rate, mm/min
$116 Configuration d max rate, mm/min
$117 Configuration e max rate, mm/min
$120 Configuration x accel, mm/sec^2
$121 Configuration y accel, mm/sec^2
$122 Configuration z accel, mm/sec^2
$123 Configuration a accel, mm/sec^2
$124 Configuration b accel, mm/sec^2
$125 Configuration c accel, mm/sec^2
$126 Configuration d accel, mm/sec^2
$127 Configuration e accel, mm/sec^2
$130 Configuration x max travel, mm
$131 Configuration y max travel, mm
$132 Configuration z max travel, mm
$133 Configuration a max travel, mm
$134 Configuration b max travel, mm
$135 Configuration c max travel, mm
$136 Configuration d max travel, mm
$137 Configuration e max travel, mm

Example Code

(HEADER)
(BACKSTOP 127.876 FROM START )
(READY MOTION)
(This program as developed as an example and not intended for any particular)
(application. Ready Motion does not except any responsibility for how this program is used in applications.)

(STEPPER SETTINGS)
($100=76.7400)
($101=125.984)
$100=386.025
$101=629.921
$102=314.960
$103=125.984
$120=200
$121=200
$122=200
$123=200
(END)

G92 X0 Y0 Z0 A0 B0 C0 D0 E0
(LASER NOT ENABLED)
M5
(MAKE SURE NO POWER)
M25
(MAKE SURE NO FREQ)
S0
(HOUSEKEEPING)
M28

(HEADER END)
G21 (All units in mm)

(Start cutting path id: path3108-0-3)
(Change tool to Default tool)

G00 Z 0.000
G00 X -0.008 Y 133.883
M22 (AIR ON)
M24
M3 S1000
G01 Z 0.000 F 250.000(Penetrate)
G01 X 0.041 Y 134.950 Z 0.000
G03 X -0.019 Y 134.959 Z 0.000 I -0.053 J -0.157 F 300
G03 X -0.074 Y 134.948 Z 0.000 I 0.007 J -0.178
G03 X 0.090 Y 134.931 Z 0.000 I -0.224 J -0.194
G00 Z 0.000
M5
M25 (U CONTROL OFF)
M23 (AIR OFF)

(End cutting path id: path3108-0-3)

(FOOTER)
(LASER NOT ENABLED)
M5
M23 (AIR OFF)
M25 (U CONTROL OFF)
G4 P1
M31 (REDLIGHT OFF)
M29 (HOIUSEKEEPING OFF)
G00 X0 Y0 Z0 A0 B0 C0 D0 E0
M2
(END

Programming Ready Motion

Leave a Reply

Your email address will not be published. Required fields are marked *