Instructions

This allows you to measure the tool length directly with calipers by measuring the overall
length of the holder with the tool mounted. Also remember that the home stopping
position for the z-axis shouldn’t be zero. It should be a positive number that allows you to
change the tool if necessary. The x0, y0 and z0 position should be chosen carefully and
be related to the part that is being programmed, not to a convenient place to change tools.
Write a couple of lines of code with and without the tool length compensation to test
what you have just learned. Run it using the backplot to fully understand it before going
on, and, above all, always remember to cancel the tool length compensation after using it.
Time to get serious
Let’s think about just what g40, g41 and g42 does. To begin with g41 (g42 is the opposite
of g41) will locate the spindle to the left of the programmed edge that you want to
machine according to the d (tool dia.) amount entered into the tool data table. G40 simply
cancels the g41 or g42 commands.
Computers can keep you from ruining your part
These commands allow you to put the actual dimensions of the part you want directly
into the program and then it will take the diameter that you entered into a [Tools] file and
automatically correct the path of the cutter so that the edge of the cutter is always located
on the edge on the part. Your computer will be making thousands of calculations a
second to do this, and old Millie will just bust her hump for you to make this happen if
you follow their rules. If you don’t, they’ll start sending you those nasty little messages
again, but look at it as a blessing. They’ll keep you from wrecking your part.
Another thing to keep in mind is that one of the great benefits of the tool offset
commands is being able to use end mills with slightly different diameters without having
to calculate all new tangent points. Before CNC, when NC was the only system available,
there was a surplus of used end mills on the market that had not been re-sharpened
because it was cheaper to scrap out dull end mills without re-sharpening them than to
write long complex programs to account for their smaller diameter.
Don’t ask for impossible
The first thing you have to learn about using the g41 or g42 cutter comp commands is
that you can’t ask your machine to do the impossible. What is impossible is cutting an
inside “V” with an end-mill.
If you firmly imbed this into your mind, you’ll save the many hours of wasted time that I
spent learning. Of course I knew that this is impossible, but I kept asking my computer to
do it when I was entering the cutter offset mode. As soon as a g41 or g42 is entered into
the program you can’t ask your machine to cut “V” shapes without an arc being
programmed that is at least the radius of the cutter you are using. What confused me was
the cutter diameter that was retrieved with the d-command had an effect on whether you
would or would not have an error. I believe I truly understand it now and had to rewrite
several pages of garbage I wrote with confusing rules.
42