Instructions

with some fonts and are located close together on any keyboard. You are not writing a

letter when you program, and it has to be accurate.

Circle program

Note: In these instructions, the code you should retype into your program will always

shown in bold face red type.

The entire program:

(g02 circle program)

g01 g20 g40 g49 g90 x0 y0 z0 f2

g02 x0 y0 i-.5 j0

g01 g90 x0 y0 z0 f2

1) % –Always start a new program with a % sign. This informs our robot that a

program is coming in. Each time you press [Enter], the program will start a new

line, so [ENTER] it is, and we’re off and running.

2) (g02 circle program) –Words in parentheses are not part of program and are used

to help the operators quickly understand the program. You can enter notes into a

program at any point to remind yourself or another operator in the future why the

upcoming code was entered.

3) Note: The g20, g40, g49 commands are not totally necessary for this program to

run. They are added to protect your program from being polluted by commands that

may have been active in previous programs and never canceled out. About the only

one of this group that could eliminate a potential problem is the g20 which could

keep your inch program from running in metric if a g21 was left active. I really

didn’t want to get into this subject this early in the instructions; however, if you

were using a computer that other people use it could be a problem so I believed I

should mention it and I’ll only do so in this first programming example.

4) g01 g20 g40 g49 g90 x0 y0 z0 f2 –What we just ordered our robot to do is go to the

home position if it’s not already there.

A) g01–Enters a mode where the feed (speed) is controlled by “f” which can be

entered. Also note that the slow feed of f2 was entered so you could fully

appreciate just what the machine slides do to generate a circle. The feed could

be set for a faster rate for the backplot test and slowed down for the machine

test if desired.)

B) g20–Orders the machine to use the inch measurement system. Metric machine

owners will use a g21 in place of the g20.

C) g40–-Cancels any unwanted tool diameter compensation that may have been

left active from previous run programs.