Introduction

RS-274D is the recommended standard for numerically controlled machines developed by the Electronic Industry Association in the early 1960's. The RS-274D revision was approved in February, 1980. These standards provide a basis for the writing of numeric control programs.
There are a number of historical sidelights to this standard, many having to do with the original use of punched paper tape as the only data interchange medium. The 64-character EIA-244 paper tape standard is now (thankfully) obsolete, and ASCII character bit patterns are now the standard representation. This old tape standard had specific characters used for 'searching' for specific lines (program blocks) on the tape, 'rewinding' the tape, etc. Ocasionally this obsolete language is still used when referring to some cnc control tasks.
The full NIST Enhanced Machine Controller is nc programmed using a variant of the RS274D language to control motion and I/O. This variant is called RS276NGC because it was developed for the Next Generation Controller, a project of the National Center for Manufacturing Science. The version of RS274 used by EMC adheres closely to the publications of the NCMS wherever those publications produce an unambiguous set. In some cases reference to other implementations of RS274 had to be made by NIST.
(back to contents)

---

Blocks
The basic unit of the nc program is the 'block', which is seen in printed form as a 'line' of text. Each block can contain one or more 'words', which consist of a letter, describing a setting to be made, or a function to be performed, followed by a numeric field, supplying a value to that function. A permissible block of input is currently restricted to a maximum of 256 characters.
The following order is required for the construction of a block.

1. an optional block delete character, which is a slash / .
2. an optional line number.
3. any number of segments, where a segment is a word or a comment.
4. an end of line character.

The interpreter allows words starting with any letter except N (which denotes a line number and must be first) to occur in any order. Execution of the block will be the same regardless of the order.An example of a program block would be

/N0001 G0 X123.05

This block is constructed using three words, N0001, G0, and X123.05. The meanings of each of these words is described in detail below. In essence, the n word numbers the line, the g0 word tells the machine to get to its destination as quickly as it can, and the final position of the x axis is to be 123.05. Since it is constructed with a preceeding slash, this block could be deleted during a run if optional block delete were activated.There are some general considerations when writing nc code for the EMC:

• The interpreter allows spaces and tabs anywhere within a block of code. The result of the interpretation of a block will be the same as it would if any white spaces were not there. This makes some strange-looking input legal. The line "g0x +0. 12 34y 7" is equivalent to "g0 x+0.1234 y7", for example.
• Blank lines are allowed in the input by the interpreter. They are ignored.
• The interpreter also assumes input is case insensitive. Any letter may be in upper or lower case without changing the meaning of a line.

Whenever you write nc programs, you would do well to be considerate of others who may have to read that code, even though the interpreter itself does not care about white space and case. Unless your are really up against the 256 digit block size limit, white space between words and the absense of it within words makes a block much easier to understand.There are a number of limitations about the number or types of words that can be strung together into a block. The interpreter uses the following rules:

• A line may have zero to four G words.
• Two G words from the same modal group may not appear on the same line.
• A line may have zero to four M words.
• Two 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.

Don't worry to much about modal codes or the order of execution of the words within a block of nc program just yet. These will become clear as you work your way through the definitions of the permissible words listed in the next unit.For now it is enough to remember that a program block is more than the words that are written in it. Various words can be combined to specify multi-axis moves, or perform special functions. While a block of code has a specific order of execution, it must be considered to be a single command. All of the words within a block combine to produce a single set of actions which may be very different from the actions assigned to the same words were they placed in separate blocks. A simple example using axis words should illustrate this point.

n1 x6 - moves from the current x location to x6
n2 y3 - moves from current y location to y3 at x6
n3 z2 - moves from current z location to z2 at x6 and y3n10 x6 y3 z2 - moves on a single line from current x, y, z to x6 y3 z2

The final position of the first three blocks (n1-n3) and the (n10) block are the same. The first set of blocks might be executed in sequence to move the tool around an obstacle while the path of the tool for the combined block (n10) might run it into the part or the fixture.To make the specification of an allowable line of code precise, NIST defined it in a production language (Wirth Syntax Notation). These definitions appear as Table *** at the end of this chapter. In order that the definition in the appendix not be unwieldy, many constraints imposed by the interpreter are omitted from that appendix. The list of error messages elsewhere in the Handbook indicates all of the additional constraints.

Numbers
Since every nc word is composed of a letter and a value. Before we begin a serious discussion of the meaning of nc programming words we need to consider the meaning of value within the interpreter. 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. In this chapter all examples will use explicit numbers. Expressions and unary operations are treated in the computation chapter. The use of parameter values or variables are a described in detail in the Using Variables chapter.
EMC uses the following rules regarding numbers. In these rules a digit is a single character between 0 and 9.
A number consists of :

• an optional plus or minus sign, followed by
• zero to many digits, followed, possibly, by
• one decimal point, followed by
• 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.Some additional rules about the meaning of numbers are that:

• 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.
• Initial and trailing zeros are allowed but not required.
• A number with initial or trailing zeros will have the same value as if the extra zeros were not there.

Numbers used for specific purposes in RS274/NGC are often restricted to some finite set of values or to some range of values. In many uses, decimal numbers must be close to integers; this includes the values of indexes (for parameters and changer slot numbers, for example). In the interpreter, a decimal number which is supposed be close to an integer is considered close enough if it is within 0.0001 of an integer.
Words
An nc program word is an acceptable letter followed by a real_value. Table 2 shows the current list of words that the EMC interpreter recognizes. The meanings of many of these words are listed in detail below. Some are included in and in the chapter on tool radius compensation and the chapter on canned cycles.

Table 2  Words acceptable to the EMC interpreter

D F  G  H  IJ K L

tool radius compensation number  feedrate  general function (see below) tool length offset  X-axis offset for arcs  X offset in G87 canned cycle Y-axis offset for arcs  and Y offset in G87 canned cycle  K Z-axis offset for arcs  and Z offset in G87 canned cycle  L number of repetitions in canned cycles  and key used with G10

M N  PQ R S T  X  Y  Z

miscellaneous function (see below)  line number  dwell time with G4 and canned cycles  key used with G10  Q feed increment in G83 canned cycle  R arc radius  canned cycle plane  S spindle speed  T tool selection  X-axis of machine  Y-axis of machine  Z-axis of machine

Line Number Words
A line number is the letter N followed by an integer (with no sign) between 0 and 99999. Line numbers are not checked except for to many digits. It is not necessary to number lines because they are not used by the interpreter. But they can be convenient when looking over a program. N word line numbers are reported in error messages when errors are caused by program problems.
Line numbers can be confusing because they are not the number that is displayed as being executed. Nor are they the number used to restart an nc program at a line other than the start. That number is the number of the current block in the program file with 0 being the first block.

---

Axis Words
We have already seen examples of axis words. An X word would be X10.001, which by itself indicates the X axis should move to a position of 10.001 user units, which would normally be inches or mm. Table one lists the common names for axis. Not all of these names can be used by all of the EMC interpreters. X, Y, and Z words will be accepted by the current (Jan, 2000) interpreter. NIST will soon release an expanded interpreter that will allow for three rotary axis A, B, C, as well.

Table 3  Definition of Common Axes

X - Primary Linear Axis            Y - Primary Linear Axis            Z - Primary Linear Axis

U - Secondary axis parallel to X   V - Secondary axis parallel to Y    W- Secondary axis parallel to Z

A - Angular axis around X axisB - Angular axis around Y axis  C - Angular axis around Z axis

---

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 Jwords, 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

 
 Canned Cycles/Drill Subroutines (G80-G89)
Look here for a complete reference.
 

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

(back to contents)

---

 
 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.

CNC Programming g,m codes

G-codes are also called preparatory codes, and are any word in a CNC program that begins with the letter "G". Generally it is a code telling the machine tool what type of action to perform, such as:

• rapid move
• controlled feed move in a straight line or arc
• series of controlled feed moves that would result in a hole being bored, a workpiece cut (routed) to a specific dimension, or a decorative profile shape added to the edge of a workpiece.
• set tool information such as offset.

There are other codes; the type codes can be thought of like registers in a computer.

[edit]Letter addresses

Some letter addresses are used only in milling or only in turning; most are used in both. Bold below are the letters seen most frequently throughout a program.

Sources: Smid^[1]; Green et al.^[2]

Variable	Description	Corollary info
A	Absolute or incremental position of A axis (rotational axis around X axis)
B	Absolute or incremental position of B axis (rotational axis around Y axis)
C	Absolute or incremental position of C axis (rotational axis around Z axis)
D	Defines diameter or radial offset used for cutter compensation. D is used for depth of cut on lathes.
E	Precision feedrate for threading on lathes
F	Defines feed rate
G	Address for preparatory commands	G commands often tell the control what kind of motion is wanted (e.g., rapid positioning, linear feed, circular feed, fixed cycle) or what offset value to use.
H	Defines tool length offset; Incremental axis corresponding to C axis (e.g., on a turn-mill)
I	Defines arc size in X axis for G02or G03 arc commands. Also used as a parameter within some fixed cycles.
J	Defines arc size in Y axis forG02 or G03 arc commands. Also used as a parameter within some fixed cycles.
K	Defines arc size in Z axis for G02or G03 arc commands. Also used as a parameter within some fixed cycles, equal to Laddress.
L	Fixed cycle loop count; Specification of what register to edit using G10	Fixed cycle loop count: Defines number of repetitions ("loops") of a fixed cycle at each position. Assumed to be 1 unless programmed with another integer. Sometimes the K address is used instead of L. With incremental positioning (G91), a series of equally spaced holes can be programmed as a loop rather than as individual positions. G10 use: Specification of what register to edit (work offsets, tool radius offsets, tool length offsets, etc.).
M	Miscellaneous function	Action code, auxiliary command; descriptions vary. Many M-codes call for machine functions, which is why people often say that the "M" stands for "machine", although it was not intended to.
N	Line (block) number in program; System parameter number to be changed using G10	Line (block) numbers: Optional, so often omitted. Necessary for certain tasks, such as M99 P address (to tell the control which block of the program to return to if not the default one) or GoTo statements (if the control supports those). N numbering need not increment by 1 (for example, it can increment by 10, 20, or 1000) and can be used on every block or only in certain spots throughout a program. System parameter number: G10 allows changing of system parameters under program control.
O	Program name	For example, O4501.
P	Serves as parameter address for various G and M codes	With G04, defines dwell time value. Also serves as a parameter in some canned cycles, representing dwell times or other variables. Also used in the calling and termination of subprograms. (With M98, it specifies which subprogram to call; with M99, it specifies which block number of the main program to return to.)
Q	Peck increment in canned cycles	For example, G73, G83 (peck drilling cycles)
R	Defines size of arc radius or defines retract height in canned cycles
S	Defines speed, either spindle speed or surface speed depending on mode	Data type = integer. In G97 mode (which is usually the default), an integer after S is interpreted as a number of rev/min (rpm). In G96 mode (CSS), an integer after S is interpreted as surface speed—sfm (G20) or m/min (G21). See also Speeds and feeds. On multifunction (turn-mill or mill-turn) machines, which spindle gets the input (main spindle or subspindles) is determined by other M codes.
T	Tool selection	To understand how the T address works and how it interacts (or not) with M06, one must study the various methods, such as lathe turret programming, ATC fixed tool selection, ATC random memory tool selection, the concept of "next tool waiting", and empty tools. Programming on any particular machine tool requires knowing which method that machine uses.
U	Incremental axis corresponding to X axis (typically only lathe group A controls) Also defines dwell time on some machines (instead of "P" or "X").	In these controls, X and U obviate G90 and G91, respectively. On these lathes, G90 is instead a fixed cycle address for roughing.
V	Incremental axis corresponding to Y axis	Until the 2000s, the V address was very rarely used, because most lathes that used U and W didn't have a Y-axis, so they didn't use V. (Green et al 1996[2] did not even list V in their table of addresses.) That is still often the case, although the proliferation of live lathe tooling and turn-mill machining has made V address usage less rare than it used to be (Smid 2008[1] shows an example). See also G18.
W	Incremental axis corresponding to Z axis (typically only lathe group A controls)	In these controls, Z and W obviate G90 and G91, respectively. On these lathes, G90 is instead a fixed cycle address for roughing.
X	Absolute or incremental position of X axis. Also defines dwell time on some machines (instead of "P" or "U").
Y	Absolute or incremental position of Y axis
Z	Absolute or incremental position of Z axis	The main spindle's axis of rotation often determines which axis of a machine tool is labeled as Z.

[edit]List of G-codes commonly found on Fanuc and similarly designed controls

Sources: Smid^[1]; Green et al.^[2]

Code	Description	Milling ( M )	Turning ( T )	Corollary info
G00	Rapid positioning	M	T	On 2- or 3-axis moves, G00 (unlike G01) traditionally does not necessarily move in a single straight line between start point and end point. It moves each axis at its max speed until its vector is achieved. Shorter vector usually finishes first (given similar axis speeds). This matters because it may yield a dog-leg or hockey-stick motion, which the programmer needs to consider depending on what obstacles are nearby, to avoid a crash. Some machines offer interpolated rapids as a feature for ease of programming (safe to assume a straight line).
G01	Linear interpolation	M	T	The most common workhorse code for feeding during a cut. The program specs the start and end points, and the control automatically calculates (interpolates) the intermediate points to pass through that will yield a straight line (hence "linear"). The control then calculates the angular velocities at which to turn the axis leadscrews. The computer performs thousands of calculations per second. Actual machining takes place with given feed on linear path.
G02	Circular interpolation, clockwise	M	T	Cannot start G41 or G42 in G02 or G03 modes. Must already be compensated in earlier G01 block.
G03	Circular interpolation, counterclockwise	M	T	Cannot start G41 or G42 in G02 or G03 modes. Must already be compensated in earlier G01 block.
G04	Dwell	M	T	Takes an address for dwell period (may be X, U, or P). The dwell period is specified in milliseconds.
G05P10000	High-precision contour control (HPCC)	M		Uses a deep look-ahead buffer and simulation processing to provide better axis movement acceleration and deceleration during contour milling
G05.1 Q1.	Ai Nano contour control	M		Uses a deep look-ahead buffer and simulation processing to provide better axis movement acceleration and deceleration during contour milling
G07	Imaginary axis designation	M
G09	Exact stop check	M	T
G10	Programmable data input	M	T
G11	Data write cancel	M	T
G12	Full-circle interpolation, clockwise	M		Fixed cycle for ease of programming 360° circular interpolation with blend-radius lead-in and lead-out. Not standard on Fanuc controls.
G13	Full-circle interpolation, counterclockwise	M		Fixed cycle for ease of programming 360° circular interpolation with blend-radius lead-in and lead-out. Not standard on Fanuc controls.
G17	XY plane selection	M
G18	ZX plane selection	M	T	On most CNC lathes (built 1960s to 2000s), ZX is the only available plane, so no G17 to G19 codes are used. This is now changing as the era begins in which live tooling, multitask/multifunction, and mill-turn/turn-mill gradually become the "new normal". But the simpler, traditional form factor will probably not disappear—just move over to make room for the newer configurations. See also V address.
G19	YZ plane selection	M
G20	Programming ininches	M	T	Somewhat uncommon except in USA and (to lesser extent) Canada and UK. However, in the global marketplace, competence with both G20 and G21 always stands some chance of being necessary at any time. The usual minimum increment in G20 is one ten-thousandth of an inch (0.0001"), which is a larger distance than the usual minimum increment in G21 (one thousandth of a millimeter, .001 mm, that is, one micrometre). This physical difference sometimes favors G21 programming.
G21	Programming inmillimeters (mm)	M	T	Prevalent worldwide. However, in the global marketplace, competence with both G20 and G21 always stands some chance of being necessary at any time.
G28	Return to home position (machine zero, aka machine reference point)	M	T	Takes X Y Z addresses which define the intermediate point that the tool tip will pass through on its way home to machine zero. They are in terms of part zero (aka program zero), NOT machine zero.
G30	Return to secondary home position (machine zero, aka machine reference point)	M	T	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. They are in terms of part zero (aka program zero), NOT machine zero.
G31	Skip function (used for probes and tool length measurement systems)	M
G32	Single-point threading, longhand style (if not using a cycle, e.g., G76)		T	Similar to G01 linear interpolation, except with automatic spindle synchronization for single-point threading.
G33	Constant-pitchthreading	M
G33	Single-point threading, longhand style (if not using a cycle, e.g., G76)		T	Some lathe controls assign this mode to G33 rather than G32.
G34	Variable-pitch threading	M
G40	Tool radius compensation off	M	T	Cancels G41 or G42.
G41	Tool radius compensation left	M	T	Milling: Given righthand-helix cutter and M03 spindle direction, G41 corresponds to climb milling (down milling). Takes an address (Dor H) that calls an offset register value for radius. Turning: Often needs no D or H address on lathes, because whatever tool is active automatically calls its geometry offsets with it. (Each turret station is bound to its geometry offset register.)
G42	Tool radius compensation right	M	T	Similar corollary info as for G41. Given righthand-helix cutter and M03 spindle direction, G42 corresponds to conventional milling (up milling).
G43	Tool height offset compensation negative	M		Takes an address, usually H, to call the tool length offset register value. The value is negative because it will be added to the gauge line position. G43 is the commonly used version (vs G44).
G44	Tool height offset compensation positive	M		Takes an address, usually H, to call the tool length offset register value. The value is positive because it will be subtracted from the gauge line position. G44 is the seldom-used version (vs G43).
G45	Axis offset single increase	M
G46	Axis offset single decrease	M
G47	Axis offset double increase	M
G48	Axis offset double decrease	M
G49	Tool length offset compensation cancel	M		Cancels G43 or G44.
G50	Define the maximum spindle speed		T	Takes an S address integer which is interpreted as rpm. Without this feature, G96 mode (CSS) would rev the spindle to "wide open throttle" when closely approaching the axis of rotation.
G50	Scaling function cancel	M
G50	Position register (programming of vector from part zero to tool tip)		T	Position register is one of the original methods to relate the part (program) coordinate system to the tool position, which indirectly relates it to the machine coordinate system, the only position the control really "knows". Not commonly programmed anymore because G54 to G59 (WCSs) are a better, newer method. Called via G50 for turning, G92 for milling. Those G addresses also have alternate meanings (which see). Position register can still be useful for datum shift programming.
G52	Local coordinate system (LCS)	M		Temporarily shifts program zero to a new location. This simplifies programming in some cases.
G53	Machine coordinate system	M	T	Takes absolute coordinates (X,Y,Z,A,B,C) with reference to machine zero rather than program zero. Can be helpful for tool changes. Nonmodal and absolute only. Subsequent blocks are interpreted as "back to G54" even if it is not explicitly programmed.
G54 to G59	Work coordinate systems (WCSs)	M	T	Have largely replaced position register (G50 and G92). Each tuple of axis offsets relates program zero directly to machine zero. Standard is 6 tuples (G54 to G59), with optional extensibility to 48 more via G54.1 P1 to P48.
G54.1 P1 to P48	Extended work coordinate systems	M	T	Up to 48 more WCSs besides the 6 provided as standard by G54 to G59. Note floating-point extension of G-code data type (formerly all integers). Other examples have also evolved (e.g., G84.2). Modern controls have the hardware to handle it.
G70	Fixed cycle, multiple repetitive cycle, for finishing (including contours)		T
G71	Fixed cycle, multiple repetitive cycle, for roughing (Z-axis emphasis)		T
G72	Fixed cycle, multiple repetitive cycle, for roughing (X-axis emphasis)		T
G73	Fixed cycle, multiple repetitive cycle, for roughing, with pattern repetition		T
G73	Peck drilling cycle for milling - high-speed (NO full retraction from pecks)	M		Retracts only as far as a clearance increment (system parameter). For when chipbreaking is the main concern, but chip clogging of flutes is not.
G74	Peck drilling cycle for turning		T
G74	Tapping cycle for milling, lefthand thread, M04 spindle direction	M
G75	Peck grooving cycle for turning		T
G76	Fine boring cycle for milling	M
G76	Threading cycle for turning, multiple repetitive cycle		T
G80	Cancel canned cycle	M	T	Milling: Cancels all cycles such as G73, G83, G88, etc. Z-axis returns either to Z-initial level or R-level, as programmed (G98 or G99, respectively). Turning: Usually not needed on lathes, because a new group-1 G address (G00 to G03) cancels whatever cycle was active.
G81	Simple drilling cycle	M		No dwell built in
G82	Drilling cycle with dwell	M		Dwells at hole bottom (Z-depth) for the number of milliseconds specified by the P address. Good for when hole bottom finish matters.
G83	Peck drilling cycle (full retraction from pecks)	M		Returns to R-level after each peck. Good for clearing flutes of chips.
G84	Tapping cycle,righthand thread,M03 spindle direction	M
G84.2	Tapping cycle, righthand thread,M03 spindle direction, rigid toolholder	M
G90	Absolute programming	M	T (B)	Positioning defined with reference to part zero. Milling: Always as above. Turning: Sometimes as above (Fanuc group type B and similarly designed), but on most lathes (Fanuc group type A and similarly designed), G90/G91 are not used for absolute/incremental modes. Instead, U and W are the incremental addresses and X and Z are the absolute addresses. On these lathes, G90 is instead a fixed cycle address for roughing.
G90	Fixed cycle, simple cycle, for roughing (Z-axis emphasis)		T (A)	When not serving for absolute programming (above)
G91	Incremental programming	M	T (B)	Positioning defined with reference to previous position. Milling: Always as above. Turning: Sometimes as above (Fanuc group type B and similarly designed), but on most lathes (Fanuc group type A and similarly designed), G90/G91 are not used for absolute/incremental modes. Instead, U and W are the incremental addresses and X and Z are the absolute addresses. On these lathes, G90 is a fixed cycle address for roughing.
G92	Position register (programming of vector from part zero to tool tip)	M	T (B)	Same corollary info as at G50 position register. Milling: Always as above. Turning: Sometimes as above (Fanuc group type B and similarly designed), but on most lathes (Fanuc group type A and similarly designed), position register is G50.
G92	Threading cycle, simple cycle		T (A)
G94	Feedrate per minute	M	T (B)	On group type A lathes, feedrate per minute is G98.
G94	Fixed cycle, simple cycle, for roughing (X-axis emphasis)		T (A)	When not serving for feedrate per minute (above)
G95	Feedrate per revolution	M	T (B)	On group type A lathes, feedrate per revolution is G99.
G96	Constant surface speed (CSS)		T	Varies spindle speed automatically to achieve a constant surface speed. See speeds and feeds. Takes an S address integer, which is interpreted as sfm in G20 mode or as m/min in G21 mode.
G97	Constant spindle speed	M	T	Takes an S address integer, which is interpreted as rev/min (rpm). The default speed mode per system parameter if no mode is programmed.
G98	Return to initial Z level in canned cycle	M
G98	Feedrate per minute (group type A)		T (A)	Feedrate per minute is G94 on group type B.
G99	Return to R level in canned cycle	M
G99	Feedrate per revolution (group type A)		T (A)	Feedrate per revolution is G95 on group type B.

[edit]List of M-codes commonly found on Fanuc and similarly designed controls

Sources: Smid^[1]; Green et al.^[2]

Code	Description	Milling ( M )	Turning ( T )	Corollary info
M00	Compulsory stop	M	T	Non-optional—machine will always stop upon reaching M00 in the program execution.
M01	Optional stop	M	T	Machine will only stop at M01 if operator has pushed the optional stop button.
M02	End of program	M	T	No return to program top; may or may not reset register values.
M03	Spindle on (clockwise rotation)	M	T	The speed of the spindle is determined by the address S, in surface feet per minute. The right-hand rule can be used to determine which direction is clockwise and which direction is counter-clockwise. Right-hand-helix screws moving in the tightening direction (and right-hand-helix flutes spinning in the cutting direction) are defined as moving in the M03 direction, and are labeled "clockwise" by convention. The M03 direction is always M03 regardless of local vantage point and local CW/CCW distinction.
M04	Spindle on (counterclockwise rotation)	M	T	See comment above at M03.
M05	Spindle stop	M	T
M06	Automatic tool change (ATC)	M	T (some-times)	Many lathes do not use M06 because the T address itself indexes the turret. Programming on any particular machine tool requires knowing which method that machine uses. To understand how the T address works and how it interacts (or not) with M06, one must study the various methods, such as lathe turret programming, ATC fixed tool selection, ATC random memory tool selection, the concept of "next tool waiting", and empty tools. These concepts are taught in textbooks such as Smid,[1] and online multimedia (videos, simulators, etc); the latter are usually paywalled to pay back the costs of their development. They are used in training classes for operators, both on-site and remotely (e.g., Tooling University).
M07	Coolant on (mist)	M	T
M08	Coolant on (flood)	M	T
M09	Coolant off	M	T
M10	Pallet clamp on	M		For machining centers with pallet changers
M11	Pallet clamp off	M		For machining centers with pallet changers
M13	Spindle on (clockwise rotation) and coolant on (flood)	M		This one M-code does the work of both M03 and M08. It is not unusual for specific machine models to have such combined commands, which make for shorter, more quickly written programs.
M19	Spindle orientation	M	T	Spindle orientation is more often called within cycles (automatically) or during setup (manually), but it is also available under program control via M19. The abbreviation OSS (oriented spindle stop) may be seen in reference to an oriented stop within cycles.
M21	Mirror, X-axis	M
M21	Tailstock forward		T
M22	Mirror, Y-axis	M
M22	Tailstock backward		T
M23	Mirror OFF	M
M23	Thread gradual pullout ON		T
M24	Thread gradual pullout OFF		T
M30	End of program with return to program top	M	T
M41	Gear select - gear 1		T
M42	Gear select - gear 2		T
M43	Gear select - gear 3		T
M44	Gear select - gear 4		T
M48	Feedrate override allowed	M	T
M49	Feedrate override NOT allowed	M	T	This rule is also called (automatically) within tapping cycles or single-point threading cycles, where feed is precisely correlated to speed. Same with spindle speed override and feed hold button.
M52	Unload Last tool from spindle	M	T	Also empty spindle.
M60	Automatic pallet change (APC)	M		For machining centers with pallet changers
M98	Subprogram call	M	T	Takes an address P to specify which subprogram to call, for example, "M98 P8979" calls subprogram O8979.
M99	Subprogram end	M	T	Usually placed at end of subprogram, where it returns execution control to the main program. The default is that control returns to the block following the M98 call in the main program. Return to a different block number can be specified by a P address. M99 can also be used in main program with block skip for endless loop of main program on bar work on lathes (until operator toggles block skip).

[edit]Example program

Tool Path for program

This is a generic program that demonstrates the use of G-Code to turn a 1" diameter X 1" long part. Assume that a bar of material is in the machine and that the bar is slightly oversized in length and diameter and that the bar protrudes by more than 1" from the face of the chuck. (Caution: This is generic, it might not work on any real machine! Pay particular attention to point 5 below.)

Sample

Line	Code	Description
%
O4968		(Sample face and turn program)
N01	M216	(Turn on load monitor)
N02	G20 G90 G54 D200 G40	(Inch units. Absolute mode. Call work offset values. Moving coordinate system to the location specified in the register D200. Cancel any existing tool radius offset.)
N03	G50 S2000	(Set maximum spindle speed rev/min - preparing for G96 CSS coming soon)
N04	M01	(Optional stop)
N05	T0300	(Index turret to tool 3. Clear wear offset (00).)
N06	G96 S854 M42 M03 M08	(Constant surface speed [automatically varies the spindle speed], 854 sfm, select spindle gear, start spindle CW rotation, turn on the coolant flood)
N07	G41 G00 X1.1 Z1.1 T0303	(Call tool radius offset. Call tool wear offset. Rapid feed to a point about 0.100" from the end of the bar [not counting 0.005" or 0.006" that the bar-pull-and-stop sequence is set up to leave as a stock allowance for facing off] and 0.050" from the side)
N08	G01 Z1.0 F.05	(Feed in horizontally until the tool is standing 1" from the datum i.e. program Z-zero)
N09	X-0.002	(Feed down until the tool is slightly past center, thus facing the end of the bar)
N10	G00 Z1.1	(Rapid feed 0.1" away from the end of the bar - clear the part)
N11	X1.0	(Rapid feed up until the tool is standing at the finished OD)
N12	G01 Z0.0 F.05	(Feed in horizontally cutting the bar to 1" diameter all the way to the datum, feeding at 0.050" per revolution)
N13	G00 X1.1 M05 M09	(Clear the part, stop the spindle, turn off the coolant)
N14	G91 G28 X0	(Home X axis - return to machine X-zero passing through no intermediate X point [incremental X0])
N15	G91 G28 Z0	(Home Z axis - return to machine Z-zero passing through no intermediate Z point [incremental Z0])
N16	G90 M215	(Return to absolute mode. Turn off load monitor)
N17	M30	(Program stop, rewind to beginning of program)
%

Several points to note:

1. There is room for some programming style, even in this short program. The grouping of codes in line N06 could have been put on multiple lines. Doing so may have made it easier to follow program execution.
2. Many codes are "modal", meaning that they stay in effect until they are cancelled or replaced by a contradictory code. For example, once variable speed cutting (CSS) had been selected (G96), it stayed in effect until the end of the program. In operation, the spindle speed would increase as the tool neared the center of the work in order to maintain a constant surface speed. Similarly, once rapid feed was selected (G00), all tool movements would be rapid until a feed rate code (G01, G02, G03) was selected.
3. It is common practice to use a load monitor with CNC machinery. The load monitor will stop the machine if the spindle or feed loads exceed a preset value that is set during the set-up operation. The job of the load monitor is to prevent machine damage in the event of tool breakage or a programming mistake. On small or hobby machines, it can warn of a tool that is becoming dull and needs to be replaced or sharpened.
4. It is common practice to bring the tool in rapidly to a "safe" point that is close to the part - in this case 0.1" away - and then start feeding the tool. How close that "safe" distance is, depends on the skill of the programmer and maximum material condition for the raw stock.
5. If the program is wrong, there is a high probability that the machine will crash, or ram the tool into the part under high power. This can be costly, especially in newer machining centers. It is possible to intersperse the program with optional stops (M01 code) which allow the program to be run piecemeal for testing purposes. The optional stops remain in the program but they are skipped during the normal running of the machine. Fortunately, most CAD/CAM software ships with CNC simulators that will display the movement of the tool as the program executes. Many modern CNC machines also allow programmers to execute the program in a simulation mode and observe the operating parameters of the machine at a particular execution point. This enables programmers to discover semantic errors (as opposed to syntax errors) before losing material or tools to an incorrect program. Depending on the size of the part, wax blocks may be used for testing purposes as well.
6. For pedagogical purposes, line numbers have been included in the program above. They are usually not necessary for operation of a machine, so they are seldom used in industry. However, if branching or looping statements are used in the code, then line numbers may well be included as the target of those statements (e.g. GOTO N99).
7. Some machines do not allow multiple M codes in the same line.