Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 487)

Tool Control Functions
Chapter 20
20-3
M06 Required - This method defines that a tool is only activated in an
M06 block. A T--word that is programmed by itself becomes the next tool
activated at an M06 block. Programming an M06 by itself activates the
next tool. If a T--word is programmed in an M06 block that T--word is
used as the active tool and any other unactivated T--word is discarded.
Activate Tool in T--word - For this method no M06 needs to be
programmed to change tools. A tool change occurs immediately when the
T--word is executed.
When the correct M06 block or T--word block that will execute a tool
change is programmed the control outputs a tool selection signal to a tool
changer. The tool changer should perform a sequence of operations to
deliver the proper tool in response to the tool selection signal. For
example, to select a cutting tool that is assigned tool number “03”, write
“T03” in the part program.
Since tool changers vary in style, size and function,the system installer is
responsible for specific implementations through PAL. Refer to the PAL
programmers manual and the manual supplied by the system installer for
more details.
Important: When changing cutting tools it is usually necessary to change
the tool offset at the same time. This is done with an H-- or a D--word. For
details see section 10.5.3.
Important: When the MISCELLANEOUS FUNCTION LOCK feature is
activated, the control displays M--, B--, S--, and T--words in the part
program with the exception of M00, M01, M02, M30, M98, and M99.
This feature is activated through the Front Panel screen (as described in
chapter 7) or through some optional switch installed by the system
installer.
To cut a workpiece using the bottom face of the cutting tool, it is more
convenient to write the part program assuming that the gauge line of the
tool holder equals the bottom face of the tool.
The term “gauge point” defines the precise point on the chuck or tool
holder from which all programmed tool paths originate. Offsets refer to
the distance from this gauge point to the edge of the tool that contacts the
part being cut.
But when a cutting tool is set in the spindle, its bottom face is not at the
gauge line. To cut the workpiece to the proper dimensions, offset the tool
path by an amount that equals the difference between the gauge line and
the bottom face of the cutting tool.
20.2
Tool Length Offset Function
(G43, G44, G49)