Instructions

the time to become more proficient with the skills you have learned up to now. Although
these remaining commands are easier to learn than the ones you have been using, I’d
suggest you take a look at my last two programs at the end of this section and read my
closing comments before going on. Though you now know enough to make parts without
them, the following g-commands, when used appropriately, can eliminate many lines of
code from your programs and allow you to enjoy the full power of EMC.
The G80 command
The g80 command is used to cancel a canned cycle. It’s used in a similar fashion as the
g40 and g49 commands.
The g81 command
The g81 command is intended for drilling, and because x, y movements usually take
place with the drill located well above the part to avoid accidental collisions with
fixtures, the most efficient method is to lower the drill in rapid (g00) to the starting point.
However, the computer needs to know the drill starting point to accomplish this. This
second z-axis position is given by entering an r-command defining an absolute position in
the same line of code that contains the g-command that requires it. (Note that the r-
command is also used as a method of entering the radius when programming movements
that produce circular shapes; however, the EMC can tell the difference based on when it
is used.) If the depth of the hole exceeds 1.5 times the diameter of the drill you should use
the g83 command. Also note that we are using the absolute mode.
Example:
%
g90 g40 g20 g00 g80 z2
x0 y0
g81 x2 y1 z-0.50 r0.010 f3
g00 g80 x0 y0
%
(Consider the top of your part to be the 0 position.)
%
An explanation, line by line:
g90 g40 g20 g00 g80 z2 – It’s a good idea to get the z-axis up out of the way before
moving the x- or the y-axis. For example, consider what happens if you start the program
from a different position than you intended and the drill hits the fixture on the move to its
home position.
x0 y0
g81 x2 y1 z-0.50 r0.010 f3 – This line of code contains all the information to put the g81
canned cycle into effect, and you’ll be able to repeat it each time a new x, y position is
given.
g00 g80 x0 y0 – When you have completed drilling all your holes, a g80 is entered to
cancel the canned g-cycle command.
For drilling more than 1 hole, add the needed x, y positions for each hole; for
example:
%
68