Smithy CNC Mills - Manual (Page 89)

SmithyCNC Programmer’s Reference Manual: Tool File & Compensation 9-7
* To stop cutter radius compensation, program G40.
* If G40, G41, or G42 is programmed in the same block as tool motion, cutter
compensation will be turned on or off before the motion is made. To make the
motion come first, the motion must be programmed in a separate, previous
block.
D Number
The current interpreter requires a D number on each line that has the G41 or
G42 word. The value specified with D must be a non-negative integer. It repre-
sents the slot number of the tool whose radius (half the diameter given in the
tool table) will be used, or it may be zero (which is not a slot number). If it is
zero, the value of the radius will also be zero. Any slot in the tool table may be
selected this way. The D number does not have to be the same as the slot num-
ber of the tool in the spindle.
Tool Table
Cutter radius compensation uses data from the machining center's tool table.
For each slot in the tool carrousel, the tool table contains the diameter of
thetool in that slot (or the difference between the actual diameter of the tool in
the slot and its nominal value). The tool table is indexed by slot number. How
to put data into the table when using the stand-alone interpreter is discussed in
the tool table page.
Two Kinds of Contour
The interpreter handles compensation for two types of contour:
* The contour given in the NC code is the edge of material that is not to be
machined away. We will call this type a "material edge contour".
* The contour given in the NC code is the tool path that would be followed by a
tool of exactly the correct radius. We will call this type a "tool path contour".
The interpreter does not have any setting that determines which type of contour
is used, but the description of the contour will differ (for the same part geome-
try) between the two types and the values for diameters in the tool table will be
different for the two types.