PROGRAMMING
96-8000
143
June 1999
G Preparatory functions (G codes)
The G address character is used to specify the type of operation to occur in a block. The G is followed by a
two or three digit number between 00 and 150. Each G code is part of a numbered group. The Group 0 codes
are non-modal; that is, they specify a function applicable to this block only and do not effect other blocks. The
other groups are modal and the specification of one code in the group cancels the previous code applicable
from that group. A modal G code applies to all subsequent blocks so those blocks do not need to re-specify
the same G code. Multiple G codes can be placed in a block in order to specify all of the setup conditions for
an operation, provided no two are from the same numbered group. See Section 3 for a detailed list 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 100. H0 will cause no offset to be used and Hn will use the tool
length entry n from the Offsets display. Note that G49 is the default condition and will clear the tool length
offsets; so you must select either G43 or G44 to activate tool length offsets. The TOOL OFSET MESUR button
will enter a value into the offsets to correspond to the use of G43.
I Canned cycle and circular optional data
The I address character is used to specify data used for some canned cycles and circular motions. It is either
in inches with four fractional positions or mm with three fractional positions. It is followed by a signed number in
inches between -15400.0000 and 15400.0000 or between -39300.000 and 39300.000mm for metric.
J Canned cycle and circular optional data
The J address character is used to specify data used for some canned cycles and circular motions. It is
formatted just like the I data. It is followed by a signed number in inches between -15400.0000 and 15400.0000
or between -39300.000 and 39300.000mm for metric.
K Canned cycle and circular optional data
The K address character is used to specify data used for some canned cycles and circular motions. It is
formatted just like the I data. It is followed by a signed number in inches between -15400.0000 and 15400.0000
or between -39300.000 and 39300.000mm for metric.
L Loop count for repeated cycles
The L address character is used to specify a repetition count for some canned cycles and auxiliary functions. It
is followed by an unsigned number between 0 and 32767.
M M Code miscellaneous functions
The M address character is used to specify an M code for a block. These codes are used to control miscella-
neous machine functions. Note that only one M code is allowed per block of the CNC program and all M codes
are performed at the end of the block. See the "M Codes" section for a detailed list of M codes.
N Number of block
The N address character is entirely optional. It can be used to identify or number each block of a program. It is
followed by a number between 0 and 99999. The M97 function must reference an N line number.
O Program number/name
The O address character is used to identify a program. It is followed by a number between 0 and 9999. A
program saved in memory always has a Onnnnn identification in the first block; it cannot be deleted. Altering
the O in the first block causes the program to be renamed. An Onnnnn can be placed in other blocks of a
program but will have no effect and can be confusing to the reader. A colon (:) may be used in the place of O in
a program, but is always displayed as îš“Oîš”.
To Next Page
Loading...
Need help?
General
