Instructions
Change n10 to (g91 g81 x0 y0 z-.3 r-.1) (No "L" on this line. Now it will drill one hole at
x0,y0).
Now insert n12 (x.25 y0 r0 L4) (Now it will move to x.25, x.5, x.75, & x1.0 and drill to
z-.40 at each place.)
Note: Because the next move on line n15 is in incremental, the tool will move to
Absolute position x1.0, y.250, then line n20 will drill (4) more holes and end at x0, y.25.
The g92 and g92.2 commands
Can you imagine how hard cnc programming would be if you had to write programs in
relation to the work’s position on the machine? It’s always easier to write code from a
convenient point in relation to the part rather than its actual position on the machine. This
is usually more of a problem on full-size machining centers that have built in homing
cycles than on a Sherline with its convenient “Zero All Axes” command. Many times
you may want to produce duplications of the same part in a single run. Without the g92
command each part would require separate programming.
The g92 is a handy command to eliminate these problems. It simply resets the axis
included in the same line of code to the number included with the axis designation which
is usually zero.
For example:
g92 x0 y0 resets your present position to x0 y0.
The next problem is canceling this command and getting back to the standard g90
coordinate system after that particular section of code has been run. The rules to do this
are a little more specific: You must be in exactly the same position when you cancel this
command with a g92.2 as you were when you entered it; therefore, this is what a full
block of code would look like that might be inserted into some program starting at the
g92 command:
g92 x0 y0
g00 x0.500
z-0.500
g01 z-0.750 f3
x1.500
y1.000
x0.500
y0
z0
x0 y0
g92.2
This leaves you exactly back where you started and back under the g90 command. To
eliminate confusion it’s also important to note that the EMC position display also resets
to whatever is called for when the g92 command is given.
The g98 and g99 commands
These commands are needed when you are under the g91 command (incremental) to
control the retracted z-axis position when drilling a series of holes using the L
command. It’s also another method of bringing confusion into your life.
74