Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 518)

Tool Control Functions
Chapter 20
20-34
Example 20.7
Programming Tool Changes Using Tool Life Management
The following example assumes that the system installer has configured in
AMP, both, the boundary for tool life management at 100, and an M06 to
perform a tool change. It also is assumed that the tool changer is located at
the secondary machine home point called by a G30, this is not necessarily
true for different machine applications.
Program Block Description
G49G30X10Z10F100; Return to secondary home position.
T101; Next tool change will be a tool from group 1.
M06; Change to a group 1 tool.
G43; Activate tool length offset using the offset number for the tool
as assigned in the tool management table.
G29; Return from secondary home position
G42; Activate cutter compensation right using the offset number for
the tool as assigned in the tool management table.
T102; Next tool change will be a tool from group 2.
G01X13Y1F200; Cutting with a group 1 tool.
G30; Return to secondary machine home.
M06T101; Replaces the group 1 tool with a group 2 tool. Note the
T--word is optional in this block.
G29; Return from secondary home position. New tool length offset
values and new tool radius offset values take effect.
G01X2Y2F100; Cutting with a group 2 tool.
G41D2; Changes the current tool radius number that was activated with
this tool and replaces it with the new D2 offset values. Note
that the tool management table does not get changed. Also
changes to cutter compensation left.
M30;
END OF CHAPTER