Preparatory Words

Some G words alter the state of the machine so that it changes from cutting straight lines to cutting arcs. Other G words cause the interpretation of numbers as millimeters rather than inches. While still others set or remove tool length or diameter offsets. Most of the G words tend to be related to motion or sets of motions. Table 4 lists the currently available g words.
Table 4
G Code List G0 rapid positioning
G1 linear interpolation
G2 circular/helical interpolation (clockwise)
G3 circular/helical interpolation (c-clockwise)
G4 dwell
G10 coordinate system origin setting
G17 xy plane selection
G18 xz plane selection
G19 yz plane selection
G20 inch system selection
G21 millimeter system selection
G40 cancel cutter diameter compensation
G41 start cutter diameter compensation left
G42 start cutter diameter compensation right
G43 tool length offset (plus)
G49 cancel tool length offset
G53 motion in machine coordinate system
G54 use preset work coordinate system 1
G55 use preset work coordinate system 2
G56 use preset work coordinate system 3
G57 use preset work coordinate system 4 G58 use preset work coordinate system 5
G59 use preset work coordinate system 6
G59.1 use preset work coordinate system 7
G59.2 use preset work coordinate system 8
G59.3 use preset work coordinate system 9
G80 cancel motion mode (includes canned)
G81 drilling canned cycle
G82 drilling with dwell canned cycle
G83 chip-breaking drilling canned cycle
G84 right hand tapping canned cycle
G85 boring, no dwell, feed out canned cycle
G86 boring, spindle stop, rapid out canned
G87 back boring canned cycle
G88 boring, spindle stop, manual out canned
G89 boring, dwell, feed out canned cycle
G90 absolute distance mode
G91 incremental distance mode
G92 offset coordinate systems
G92.2 cancel offset coordinate systems
G93 inverse time feed mode
G94 feed per minute mode
G98 initial level return in canned cycles

Tool diameter compensation (g40, g41, g42) and tool length compensation (g43, g49) are covered in a separate page. Canned milling cycles (g80 - g89, g98) are covered in their own page. Coordinate systems and how to use them is also covered in a separate page. (g10, G53 - G59.3, G92, G92.2)

Basic Motion and Feedrate

G0 Rapid Positioning

Using a G0 in your code is equivilant to saying "go rapidly to point xxx yyyy". This code causes motion to occur at the maximum traverse rate.

Example:
N100 G0 X10.00 Y5.00

This line of code causes the spindle to rapid travel from wherever it is currently to coordinates X= 10", Y=5"

When more than one axis is programmed on the same line, they move simultaneously until each axis arrives at the programmed location. Note that the axes will arrive at the same time, since the ones that would arrive before the last axis gets to the end are slowed down. The overall time for the move is exactly the same as if they all went at their max speeds and the last axis to arrive stops the clock.

To set values for rapid travel in EMC, one would look for this line in the appropriate emc.ini file:

[AXIS_#] MAX_VELOCITY = (units/second)

The previous value for the rapid rate, [TRAJ] MAX_VELOCITY, is still used as the upper bound for the tool center point velocity. You can make this much larger than each of the individual axis values to ensure that the axes will move as fast as they can.

One thing to remember when doing rapid positioning, is to make sure that there are no obstacles in the way of the tool or spindle while making a move. G0 code can make spectacular crashes, if Z is not clear of clamps, vises, uncut parts, etc.....Try to raise the tool out of the way to a "safe" level before making a rapid.

I like to put a G0 Z2.0 (Z value depending on clamp height) towards the beginning of my code, before making any X or Y moves.

Example:
N100 G0 Z1.5 ----move spindle above obstacles
N110 G0 X2.0 Y1.5 ----rapid travel to first location

G1 Linear Interpolation

G1 causes the machine to travel in a straight line with the benefit of a programmed feed rate (using "F" and the desired feedrate). This is used for actual machining and contouring.

Example:
N120 Z0.1 F6.0 ----move the tool down to Z=0.1 at a rate of 6 inches/minute
N130 Z-.125 F3.0 ----move tool into the workpiece at 3 inches/minute
N140 X2.5 F8.0 ----move the table, so that the spindle travels to X=2.5 at a rate of 8 inches/minute

G2 Circular/Helical Interpolation (Clockwise)

G2 causes clockwise circular motion to be generated at a specified feed rate (F). The generated motion can be 2-dimensional, or 3-dimensional (helical). On a common 3-axis mill, one would normally encounter lots of arcs generated for the X,Y plane, with Z axis motion happening independently (2 axis moves in G17 plane). But, the machine is capable of making helical motion, just by mixing Z axis moves in with the circular interpolation.

When coding circular moves, you must specify where the machine must go and where the center of the arc is in either of two ways: By specifying the center of the arc with I and J words, or giving the radius as an R word.

I is the incremental distance from the X starting point to the X coordinate of the center of the arc. J is the incremental distance from the Y starting point to the Y coordinate of the center of the arc.

Examples:
G1 X0.0 Y1.0 F20.0 ----go to X1.0, Y0.0 at a feed rate of 20 inches/minute
G2 X1.0 Y0.0 I0.0 J-1.0 ----go in an arc from X0.0, Y1.0 to X1.0 Y0.0, with the center of the arc at X0.0, Y0.0
G1 X0.0 Y1.0 F20.0 ----go to X1.0, Y0.0 at a feed rate of 20 inches/minute
G2 X1.0 Y0.0 R1.0 ----go in an arc from X0.0, Y1.0 to X1.0 Y0.0, with a radius of R=1.0

G3 Circular/Helical Interpolation (Counterclockwise)
G3 is the counterclockwise sibling to G2.
G4 Dwell

Plane selection for coordinated motion

G17 xy plane selection
G18 xz plane selection
G19 yz plane selection

Short term change in programming units

G20 inch system selection
G21 millimeter system selection


Fixture Offsets (G54-G59.3)

Fixture offset are used to make a part home that is different from the absolute, machine coordinate system. This
allows the part programmer to set up home positions for multiple parts. A typical operation that uses fixture offsets
would be to mill multiple copies of parts on "islands" in a piece, similar to the figure below:


To use fixture offsets, the values of the desired home positions must be stored in the control, prior to running a program that uses them. Once there are values assigned, a call to G54, for instance, would add 2 to all X values in a program. A call to G58 would add 2 to X values and -2 to Y values in this example.

G53 is used to cancel out fixture offsets. So, calling G53 and then G0 X0 Y0 would send the machine back to the actual coordinates of X=0, Y=0.

G53 motion in machine coordinate system
G54 use preset work coordinate system 1
G55 use preset work coordinate system 2
G56 use preset work coordinate system 3
G57 use preset work coordinate system 4
G58 use preset work coordinate system 5
G59 use preset work coordinate system 6
G59.1 use preset work coordinate system 7
G59.2 use preset work coordinate system 8
G59.3 use preset work coordinate system 9


Distance Modes

G90 absolute distance mode
G91 incremental distance mode

Feedrate and feed modes

G93 inverse time feed mode
G94 feed per minute mode

Miscellaneous words

M words are used to control many of the I/O functions of a machine. M words can start the spindle and turn on mist or flood coolant. M words also signal the end of a program or a stop withing a program. The complete list of M words available to the RS274NGC programmer is included in table 5.
Table 5
M Word List M0 program stop
M1 optional program stop
M2 program end
M3 turn spindle clockwise
M4 turn spindle counterclockwise
M5 stop spindle turning
M6 tool change
M7 mist coolant on M8 flood coolant on
M9 mist and flood coolant off
M26 enable automatic b-axis clamping
M27 disable automatic b-axis clamping
M30 program end, pallet shuttle, and reset
M48 enable speed and feed overrides
M49 disable speed and feed overrides
M60 pallet shuttle and program stop

Modal Codes

Many G codes and M codes cause the machine 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".

Modal codes are like a light switch. Flip it on and the lamp stays lit until someone turns it off. For example, the coolant commands are modal. If coolant is turned on, it stays on until it is explicitly turned off. The G codes for motion are also modal. If a G1 (straight move) command is given on one line, it will be executed again on the next line unless a command is given specifying a different motion (or some other command which implicitly cancels G1 is given).

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

Modal commands are arranged in sets called "modal groups". 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. Measurement in inches vs. measure in millimeters are modal. A machine tool may be in many modes at the same time, with one mode from each group being in effect. The modal groups used in the interpreter are shown in Table 1.

Table 6
G and M Code Modal Groups group 1 = {G0, G1, G2, G3, G80, G81, G82, G83, G84, G85, G86, G87, G88, G89} - motion
group 2 = {G17, G18, G19} - plane selection
group 3 = {G90, G91} - distance mode
group 5 = {G93, G94} - spindle speed mode
group 6 = {G20, G21} - units
group 7 = {G40, G41, G42} - cutter diameter compensation
group 8 = {G43, G49} - tool length offset
group 10 = {G98, G99} - return mode in canned cycles
group12 = {G54, G55, G56, G57, G58, G59, G59.1, G59.2, G59.3} coordinate system selection
group 2 = {M26, M27} - axis clamping
group 4 = {M0, M1, M2, M30, M60} - stopping
group 6 = {M6} - tool change
group 7 = {M3, M4, M5} - spindle turning
group 8 = {M7, M8, M9} - coolant
group 9 = {M48, M49} - feed and speed override bypass

There is some question about the reasons why some codes are included in the modal group that surrounds them. But most of the modal groupings make sence in that only one state can be active at a time.

I'm really really new to CNC.. but if I'm reading this correctly, the G-code will trace the boundaries of the part to be cut, and then by using the cutter diameter, and offset (left or right) the path will cut correctly... is that correct?

Based on that, it'd be possible to program basic shapes using notepad, and a simple coordinate system approach to describing the finished item, preceded by information concerning cutters, and placement of kerf.

How are tapered cutters treated?

Des

Just wanted to say how much I have refered to this post
(and a copy I have on my machine at home) and how helpful
it has been, thanks Brian.

Bryan

This is a great posting. I am getting ready to make the jump and this information will be invaluable.

Rick Kernell

Lots of Info like this on the net....I got this in a search and just Pasted it here for reference