A to Z Letter address used on CNC Machining

A to Z Letter address used on CNC Machining

Letter Address	Description	Refers to
A	Angular Value about the X-axis. Measured in degrees	Axis nomenclature
B	Angular Value about the Y-axis. Measured in degrees	Axis nomenclature
C	Angular Value about the Z-axis. Measured in degrees	Axis nomenclature
D	the tool diameter or radius used for cutter compensation	Cutter compensation Parameter
E	second feed function	accuracy required when cutting a corner
F	Feed word (code)	Feed words
G	Preparatory word (code)	G-code Words
H	Unassigned/specifying for tool height compensation
I	Interpolation parameter or thread lead parallel to the X-axis	Circular interpolation and threading
J	Interpolation parameter or thread lead parallel to the Y-axis	Circular interpolation and threading
K	Interpolation parameter or thread lead parallel to the Z-axis	Circular interpolation and threading
L	Unassigned
M	Miscellaneous or auxilliary function	Machine Control Codes
N	Sequence number	Program Line numbers
O	Sequence number for secondary head only	Indicates Program Number
P	P address character is used for a dwell time	Delay of time
Q	character is used in canned cycles	Depth specification
R	used in canned cycles or circular interpolation	Axis nomenclature
S	Spindle-speed function	Spindle speed
T	Tool Change function	Tool function
U	Secondary-motion dimension parallel to X	Axis nomenclature
V	Secondary-motion dimension parallel to Y	Axis nomenclature
W	Secondary-motion dimension parallel to Z	Axis nomenclature
X	Dimension of Tool movement in X direction	Axis nomenclature
Y	Dimension of Tool movement in Y direction	Axis nomenclature
Z	Dimension of Tool movement in Z direction	Axis nomenclature

ALPHABETICAL ADDRESS CODES

The following is a list of the Address Codes used in programming the Mill.

A -  FOURTH AXIS ROTARY MOTION:

The A address character is used to specify motion for the optional fourth, A- axis, which is angular value about X-axis. It specifies an angle in degrees for the rotary axis. It is always followed by a signed number and up to three fractional decimal positions. If no decimal point is entered, the last digit is assumed to be 1/1000 degrees.

B -  FIFTH AXIS ROTARY MOTION:

The B address character is used to specify motion for the optional fifth, B, axis, which is angular value about Y-axis. It specifies an angle in degrees or the rotary axis. It is always followed by a signed number and up to three fractional decimal positions. If no decimal point is entered, the last digit is assumed to be 1/1000 degrees.

C -  AUXILIARY EXTERNAL ROTARY AXIS:

The C address character is used to specify motion for the optional external sixth, C, axis, which is angular value about Z-axis It, specifies an angle in degrees for the rotary axis. It is always followed by a signed number and up to three fractional decimal positions. If no decimal point is entered, the last digit is assumed to be 1/1000 degrees.

D - TOOL DIAMETER OFFSET SELECTION:

The D address character is used to select the tool diameter or radius used for cutter compensation. The number following must be between 0 and 200 (100 programs on an older machine). The Dnn selects that number offset register that is in the offset display which contains the tool diameter/radius offset amount when using cutter compensation (G41 G42). D00 will cancel cutter compensation so that the tool size is zero and it will cancel any previously defined Dnn.

E -  ENGRAVING FEED RATE / CONTOURING ACCURACY:

The E address character is used, with G187, to select the accuracy required when cutting a corner during high speed machining operations. The range of values possible is 0.0001 to 0.25 for the E code.

F - FEED RATE:

The F address character is used to select the feed rate. It is either in inches per minute with four fractional positions or mm per minute with three fractional positions.

G - PREPARATORY FUNCTIONS (G codes):

The G address character is used to specify the type of operation to occur by the tool in the block containing the G code. The G is followed by a two or three digit number between 0 and 187. Each G code defined in this control is part of a group of G codes.

H - TOOL LENGTH OFFSET SELECTION:

The H address character is used to select the tool length offset entry from the offsets memory. The H is followed by a two digit number between 0 and 200 (100 programs on an older machine). H0 will clear any tool length offset. You must select either G43 or G44 to activate a tool length (H) offsets. The G49 command is the default condition and this command will clear any tool length offsets.

I - CIRCULAR INTERPOLATION / CANNED CYCLE DATA:

The “I” address character is used to specify Interpolation parameter or thread lead parallel to the X-axis. It is defined in inches with four fractional positions or mm with three fractional positions.

J - CIRCULAR INTERPOLATION / CANNED CYCLE DATA:

The J address character is used to specify Interpolation parameter or thread lead parallel to the Y-axis. It is defined in inches with four fractional positions or mm with three fractional positions.

K - CIRCULAR INTERPOLATION / CANNED CYCLE DATA:

The K address character is used to specify Interpolation parameter or thread lead parallel to the Z-axis. It is defined in inches with four fractional positions or mm with three fractional positions.

L - LOOP COUNTS TO REPEAT A COMMAND LINE:

The L address character is used to specify a repeat count for some canned cycles and auxiliary functions. It is followed by a number between 0 and 32767.

M - M-CODE MISCELLANEOUS FUNCTIONS:

The M address character is used to specify an M code. These codes are used to control miscellaneous machine functions.

N - NUMBER OF BLOCK:

The N address character is used to identify or number each block of a program. It is followed by a number between 0 and 99999.

O - PROGRAM NUMBER:

The O address character is used to identify a program. It is followed by a number between 0 and 99999. You can have up to 500 program numbers (200 programs on an older machine) in your List of Programs.

P - DELAY OF TIME / M98 PROGRAM NUMBER Call:

The P address character is used for either a dwell time in seconds with a G04, or in canned cycles G82, G83, G86, G88, G89 and G73. When used as a dwell time, it is defined as a positive decimal value between 0.001 and 1000.0 in seconds. When ‘P” is used to search for a program number with an M98, or for a program number block in an M97. When P is used in a M97 or M98 the P value is a positive number with no decimal point up to 99999.

Q - CANNED CYCLE OPTIONAL DATA:

The Q address character is used in canned cycles and is always a positive number in inches between 0.001 and 100.0.

R - CIRCULAR INTERPOLATION / CANNED CYCLE DATA:

The R address character is used in canned cycles or circular interpolation. It's either in inches with four fractional positions or mm with three fractional positions. It is followed by number in inches or metric. It's usually used to define the reference plane for canned cycles.

S - SPINDLE SPEED COMMAND:

The S address character is used to specify the spindle speed; The S is followed by an unsigned number between 1 - 99999. The S command sets the desired speed.

T - TOOL SELECTION CODE:

The T address character is used to select the tool for the next tool change. The number following must be a positive number between 1 and (20) the number in Parameter 65.

U - AUXILIARY EXTERNAL LINEAR AXIS:

The U address character is used to specify motion for the optional external linear, U-axis.

It specifies a position of motion in inches. It is always followed by a signed number and up to four fractional decimal positions. If no decimal point is entered, the last digit is assumed to be 1/10000 inches. The smallest magnitude is 0.0001 inches, the most negative value is -8380.0000 inches, and the largest number is 8380.0000 inches.

V - AUXILIARY EXTERNAL LINEAR AXIS:

The V address character is used to specify motion for the optional external linear, V-axis.

It specifies a position of motion in inches. It is always followed by a signed number and up to four fractional decimal positions. If no decimal point is entered, the last digit is assumed to be 1/10000 inches.

W - AUXILIARY EXTERNAL LINEAR AXIS:

The W address character is used to specify motion for the optional external linear, W-axis.

It specifies a position of motion in inches. It is always followed by a signed number and up to four fractional decimal positions. If no decimal point is entered, the last digit is assumed to be 1/10000 inches.

X - LINEAR X-AXIS MOTION:

The X address character is used to specify motion for the X-axis. It specifies a position or distance along the X-axis. It is either in inches with four fractional positions or mm with three fractional positions. It is followed by a signed number in inches or metric. If no decimal point is entered, the last digit is assumed to be 1/10000 inches or 1/1000 mm.

Y - LINEAR Y-AXIS MOTION:

The Y address character is used to specify motion for the Y-axis. It specifies a position or distance along the Y-axis. It is either in inches with four fractional positions or mm with three fractional positions. It is followed by a signed number in inches or metric. If no decimal point is entered, the last digit is assumed to be 1/10000 inches or 1/1000 mm.

Z - LINEAR Z-AXIS MOTION:

The Z address character is used to specify motion for the Z-axis. It specifies a position or distance along the Z-axis. It is either in inches with four fractional positions or mm with three fractional positions. It is followed by a signed number in inches or metric. If no decimal point is entered, the last digit is assumed to be 1/10000 inches or 1/1000 mm.