All you need to do is pick a point
on the router table where you want
Machine Zero to be located. As
mentioned, this point is stationed in
the lower left-hand corner of your
table some distance away from your
workpiece. It’s perfectly acceptable to
choose a different location on the
router table, but it will be more
confusing to the beginner at this point
in the learning curve.
Next, using the keyboard arrow
and page up/page down keys, slowly
“jog” the X and Y axes so the center
of your cutting tool is directly over the
location you’ve chosen for Machine
Zero. Now, jog the Z axis upwards to a
point you’d like to call Machine Zero
for the Z axis.
Once the center of the cutting tool and the X, Y, and Z
axes have reached their Machine Zero destinations, watch
the main screen in Mach 3 and you’ll see some numbers on
the Digital Read-Out (DRO) display. Verify that the Machine
Coordinates button is turned on (lit red).
At this point, you “zero-out” (clear) the X, Y, and Z
coordinates by hitting the “Ref All Home” button on the
DRO display so it reads 0, 0, and 0. In turn, Mach 3 will
recognize and remember the X, Y, and Z locations you’ve
chosen on the router table as Machine Zero. Now, when
you run the gear pattern program (G-code) and it calls out
a “G28” command (go to the Home position), all three axes
will automatically move to your new Machine Zero
coordinates (X = 0, Y = 0, Z = 0).
You can also enter the G-code command G28 into the
Manual Data Input (MDI) screen in Mach 3 and it will
automatically send all three axes to the Machine Zero
position on your table.
I’m a Little “Offset”
You can set up a Work Offset in Mach 3 by clamping
down a piece of wood at a random location on your CNC
router table. Then, using the Machine Zero position as a
starting point, jog the center of the cutting tool to the
lower left-hand corner of the workpiece.
Starting at the top of the Z axis (Machine Zero),
SLOWLY move the Z axis downward so that the center of
the cutting tool barely touches the top surface (corner) of
Again, looking at the DRO display on the main screen
in your software, mark down on a piece of paper the X, Y,
and Z coordinates for future reference.
At this point, you zero-out (clear) the X, Y, and Z
coordinate buttons (not the Ref All Home button) next to
each DRO so it reads X = 0, Y = 0, Z = 0. This tells the CNC
program where the first Work Offset (i.e., “G54”) is located
on the table in reference to Machine Zero.
Now when the G-code program (gear pattern) is run,
Mach 3 will look up the first Work Offset location (G54)
and — starting at Machine Zero — move the cutting tool to
the first Work Offset coordinates (Program Zero location).
This is where Mach 3 will run the G-code program and
begin cutting out the gear pattern.
Remember, as long as your CAD software specifies Part
Zero on the drawing and your CAM software or G-code
SERVO 02.2018 49