Instructions

g01 x-1.6844

g03 x-1.5638 y.1858 r.15

g02 x-1 y0 r.3125

g01 y-.1

g00 g40 x-.5

x0 y0 z0

EMC Tip—Pausing a cut during a long program

If for some reason you have to stop your machine while it's running a long

program and you are planning to complete the part the next day, the safest way to

accomplish this is to stop the program by using [FEEDHOLD]. Turn the spindle

and servo driver off, but leave the computer on. The next day you can restart your

program by simply turning the drivers and spindle on and clicking on the

[CONTINUE] button. In this case the [FEEDHOLD] button becomes the

“Continue” button when it is used to stop the slide movement. If possible, try to

stop the operation at some point where the cutter is either not cutting or is cutting

in an area where finish doesn’t matter. It's also a good idea to write down the zero

positions of the handwheels and slides just in case you have to use the emergency

stop.

The “o” command

This command allows you to create Sub Programs.

A sub program is a program within a program that is defined by the letter “o”. EMC2 will

not allow you to call up a sub program from another file. These Sub programs (or

Subroutines) are entered at the beginning of the Main Program and are labeled by the

letter “o” followed by a number followed by the word sub. You can’t use a letter or letter

and number to define a sub program. I find it wise to further define the sub program

inside parentheses.

Example: o100 call (mill 2″ hole) A sub program may call up another sub program and

they call this procedure “nesting.” EMC2 will allow you to nest as many as ten sub

programs together.

When the sub program is complete, you enter Example: o100 endsub The words I

highlighted in red must be entered in order for the “o” command to function.

Sub Programs offer a programmer a way to shorten a program by thousands of lines.

They are similar to “canned cycles.” Prior to canned cycles if you wanted to peck drill

deep holes, you had to program all of the Z axis moves one line at a time. This could take

several lines of program for each hole. Canned cycles allowed you to put all of the

drilling information on one line, and then program position moves for all of the holes.

Some general areas were sub programs are used are. 1. On parts that have the same shape

cut in several different places. 2. Machining the same parts on several different fixtures.