Filter
Top Products
Section Section 44 System ProgrammingSystem Programming
5555
M06 T3 Pauses program, displays dialog informing
operator to change to tool number 3
Note: For compatibility reasons, the T command can be used on any line prior to
the M06 command; it does not need to be on the same line as M06.
Once the M06 command has set the current tool, the G43 command applies the
proper offset to account for the current tool’s length as follows:
G43 Hn
where n is the tool number for the current tool.
The G43 command tells LC to shift all subsequent Z axis moves away from the
workpiece (in the positive Z direction) by an offset amount. The offset amount is
equal to the difference in lengths between the current tool when the G43
command is executed and the previous tool. LC uses the Length Offset values in
the Tooling Setup dialog box to calculate the difference in lengths between two
tools.
Example:
G43 H3 Shifts all subsequent Z axis moves away
from the workpiece (in the positive Z
direction) by the difference in lengths
between tool number 3 and the previous tool
The G44 command is identical to the G43 command, except that it shifts all Z
axis moves in the direction opposite from G43. Unless you are an experienced
CNC programmer and know how to use G44 correctly, G43 is the preferred
command.
The G49 command cancels tool length compensation. It removes any offset that
LC has applied since the G-Code program began running.
When using tool length compensation there are several important things to keep in
mind:
• You must predefine all tools and tool lengths in the Tooling Setup
dialog box.
• It’s good practice to include an M06 tool change and a G43
compensation command for the first tool used, near the beginning of
the G-Code program.
• LC automatically cancels tool offset when it finishes processing a G-
Code file, or during any operation that ends the current run of the G-
Code file (such as resetting the program, opening a new program, and
so on.) TO AVOID CRASHING THE MACHINE TOOL, IT IS
VERY IMPORTANT THAT YOU REMOVE THE CURRENT
TOOL FROM THE SPINDLE WHENEVER LC CANCELS TOOL
OFFSET.