Basics of Drill Selection - Haas University
13 Video Views·Aug 8, 2025
Hey there, welcome to the first episode of our new series Haas U, where we tap into the talents
and experience of the folks here at Haas to bring you easy to understand topics that'll help you get
your machining done better. I've come here to our tool crib to grab a handful of twist drills so we
can talk about their differences and how to select the right one. Hey Richard, cool, thanks a lot.
Take it easy. Let's head out to the photo area and check out how these drills work.
When it comes to twist drills, selecting the right one can be overwhelming.
From cheap no-name drills to high-end special helix solid carbide through tool drills,
the choices can seem endless. In this video, we're focusing on getting value from your drilling
operations with the basic knowledge you need to select the right drill and some tips for getting
the most out of each of your drills. So let's get started. Three basic things separate one drill
from another. Material, coating, and geometry. Let's start with the material your drill is made
from. High-speed steel is the most basic, least expensive general purpose drill material. It's
very forgiving in drill press and hand drilling operations, and they can be resharpened to extend
their life. Next is high-speed steel with cobalt added, which holds up better than generic high-speed
steel. Cobalt gives high-speed steel more heat and wear resistance, and these drills can still
be easily resharpened, similar to high-speed steel. Carbide is the most expensive but longest
lasting drill material. There are different grades, with the most expensive drills usually
giving the best heat and chip resistance. Carbide also allows for coolant through holes to be added
to the drill. These through tool drills are primarily for deeper holes and tough to drill
materials, where the high-pressure coolant flowing to the tool flushes chips out much better, keeps
the cutting zone cooler, and provides extra lubrication to prevent wear. While all these
drills will cut a hole in most materials, the carbide drills will outlive cobalt by a factor
of 10 or 20 times in a rigid CNC machine. In other words, if a cobalt drill will cut 100 holes,
the carbide drill will cut 1,000 or 2,000 holes before needing to be resharpened. Here in the
factory, with a properly dialed-in drilling op, we have examples where we're getting 5,000 plus holes
in cast iron from just one drill. All that said, a carbide drill can easily cost 10 times more than
a cobalt drill, so the investment is a lot higher. Despite the high price, the cost per hole when
using carbide will usually be the lowest, since it can produce so many more holes. Also, because
carbide is typically capable of running three to five times faster, the decreased cycle time to
produce those holes goes right to your bottom line. Now, let's talk about selecting the proper
coating for the material you're drilling. This decision can really influence performance. I've
lined up a few examples here on the table, so we can get a good look at the differences.
Bright finish is the cheapest option, and fares well in certain applications. For example, low
steel and aluminum can both be drilled with a bright finish tool, usually without problems.
Black oxide provides an advantage over bright finish, in that it has a bit more lubricity,
often more resistance to oxidation, and an additional heat treatment that can offer
upwards of 50% longer life, while still keeping your tooling costs low. Titanium nitride,
abbreviated TIN, is the most common coating, and is a great entry-level coating for applications
where lots of heat won't be transferred to the tool from cutting harder or tougher materials.
You can tell titanium nitride by its bright gold color. Titanium carbonitride coating,
abbreviated TICN, is a step up from TIN, and provides a higher service temperature.
Slightly harder and better wearing than TIN, it's typically bluish or purple in color. Finally,
titanium aluminum nitride, abbreviated TIALN, has a much higher service temperature rating than TIN
or TICN. This great colored coating is excellent for your high temperature materials, and still a
good choice for steels and stainless steels. But, because of the aluminum content, it isn't a good
choice for drilling aluminum. Beyond these common coatings, many manufacturers have proprietary ones
of their own that tout features like high lubricity and extremely high service temperature range.
Here at Haas, we use TIN coated drills mostly when we're working mild steel,
where the increased hardness and heat resistance equals long life. We move up to TICN coatings
for drills used on cast iron, where it shows good toughness and resistance to chipping.
And, when we're cutting high strength, harder steels, we'll step up to the high end TIALN coatings
to handle the heat and high stresses, where the coating helps reflect the heat back into the chips,
away from the tool and the workpiece. Generally, unless you're cutting difficult materials,
a good quality cobalt drill with a TIN or TICN coating is a relatively inexpensive way to get
higher productivity. Also, do some shopping around. Pricing varies a lot, and you can find drills with
high-end coatings at decent prices. So, we've talked about materials and coatings. The third
key ingredient to choosing the right drill is geometry, which plays an equally important role
in drill performance. Probably the most obvious aspect of drill geometry is the drill's length.
Drills come in two common lengths. Screw machine length, commonly referred to as stub length, and
jobber length. When it comes to drilling on a CNC, stub length drills are the most common choice
because they are more rigid. There are, of course, all kinds of custom lengths available for special
applications. As with any cutting tool, you want to use the shortest drill length possible, because
the shorter the bit, the more rigid it is. Just make sure you have enough flute length to get the
chips out of the hole. Turns out this is geometry question number two. How much flute length do you
need for the hole you're drilling? Ideally, you want two times the drill diameter in flute length above
the hole when the drill is at the deepest point in the hole. This allows for chip evacuation.
Less than this, and chips can pack up inside the flutes and cause poor surface finish, hole size,
and straightness issues. Or worse, they break the drill. But you also don't want a long jobber length
drill with flutes all the way up if you're just drilling shallow holes. This drill won't be as
rigid and will yield less precise hole position. The drill point angle is probably another familiar
aspect of drill geometry for most people. When you're drilling metal on a CNC machine, you're
generally choosing between a 118 degree point and a wider 135 to 140 degree point. The 118 degree
point is most common on general purpose high speed steel drills made for cutting mild steel, aluminum,
and other soft metals. And it's what you'll usually find on regular jobber length drills.
The 135 degree point is more typical for stub length drills aimed at CNC machining and harder,
tougher materials. Here at Haas, almost all the drills we use have 135 degree points when we're
cutting cast iron and harder steels. Next up, we want to consider the helix angle of the drill.
This is important for proper chip clearance. Typically, helix angles in the 30 degree range
are used for general purpose drilling in most materials. Most of the time, these will work just
fine and you won't need to concern yourself with other options. But if your application calls for
some specialization, small helix angles below 30 down to around 10 degrees are usually selected
for harder steels and aluminum alloys where good chip evacuation, fracture resistance,
and edge strength are important. On the other end, large angles up to 40 plus degrees are often used
for drilling difficult to machine materials like stainless steel where low torque requirements and
cutting resistance help cut these tough, gummy metals. Last on our geometry list is the self-
centering point. This is found on many cobalt drills and almost all carbide drills. This
eliminates the need for a starting drill and helps drill in true position. Regular high-speed steel
drills aren't usually self-centering since it's more time consuming and expensive to grind them
with this feature. Because of this, they tend to walk or wobble when they are trying to cut into a
flat surface. More expensive cobalt and carbide drills are ground with this self-centering point,
allowing them to start cutting very easily with very little tool pressure. This virtual
self-centering means there's no need for a spot drilled hole and it's another way these expensive
drills can be more productive than their economical brothers. Not spot drilling every hole saves
lots of cycle time. Okay, we've looked at the basics, materials, coatings, and geometry. Now,
let's get into some specific cutting condition and application related tips. As we mentioned,
drill manufacturers could put holes through the drill so coolant can get delivered right to the
cutting edge down in the hole. This keeps the cutting zone cool, lubricated, and greatly aids
in chip evacuation. Typically, steel drills without through tool coolant can only drill about
two or three times their diameter deep before requiring you to peck drill to remove the chips
and get more coolant down in the cutting zone. Good carbide drills without through tool coolant
can drill up to five times diameter deep in carbon steels and aluminum before needing to peck drill.
The problem with peck drilling is that most tool wear occurs when the drill is entering
the material. Once the drill is in the cut, wear rates become very low. Peck drilling significantly
increases tool wear because you're restarting the cut multiple times per hole, not to mention all
the extra time spent pecking each hole where the TSC drill would do it in just one pass.
So, for tools more than five times depth, and particularly when drilling tough or work
hardening materials, TSC and through tool drills really become a necessity. If you need to drill
very deep holes, let's say eight times diameter or greater, you'll usually need a pilot hole to
start the drill. Typically, this is done by using a stub drill to cut the hole about one and a half
times diameter deep. Then, start the long drill with the spindle at three to five hundred rpm
and slowly feed it into the pilot hole. Once the drill main diameter is in the pilot hole,
you can crank up the rpm to full speed and finish drilling to full depth.
When drilling holes that break through the workpiece, pay special attention to the material
and cutting conditions. Drill manufacturers recommend slowing the feed rate before the drill
point breaks through the material to prevent chipping and reduce heat in the cut. We want to
reduce the heat because as the drill gets to the very bottom, before it breaks through, the material
is very thin and there is no place for the heat to go. So, that last bit of material can work harden,
literally heat treating the material. Breaking through this heat treated layer can shorten the
life of the drill. A fifty percent reduction in feed rate for the final two millimeters or a hundred
thou before the drill point reaches the bottom usually eliminates this issue. So, when does a
drill need to be sharpened? Generally speaking, as long as your holes are in tolerance, if wear and
chipping are less than half a millimeter or 20 thou, it's okay to continue using the drill. After
that, it's typically time to resharpen or regrind. Pay close attention for chipping on the drill
margins. If the wear is even, it's okay to regrind, but if it looks like this, the drill is no longer
useful. Now, oftentimes you'll be buying tools and deciding what you should spend on a specific job.
Is it a short run single lot or is it a large recurring job with thousands of parts? Carbide
might not be the best investment if you've got a short run and you can't spend extra time dialing
in your cutting parameters. High speed steel or cobalt might make more sense in this case.
Keep in mind that you can always start with less expensive drills to get the job launched.
Then, if you end up making lots of those same parts down the road, you can work with your tooling
supplier to find the best tool for the job, whether it's carbide or a high-end cobalt drill.
So, let's do a lightning fast recap. Carbide is much more expensive than the others.
It's also less forgiving if used incorrectly. High speed steel and cobalt are easy to resharpen,
but don't offer anywhere near the tool life of carbide. Typically, carbide can also run
significantly faster. When it comes to coatings, if you're machining difficult materials or need
max tool life for long part runs, then select the high-end coatings. And for geometry, we're just
touching on some of the aspects, but consider the material and your cycle time requirements
when deciding which way to go with each of these elements. If you have questions or comments about
how drills have worked in your specific circumstances, let us know in the comment
section. And don't miss the opportunity to tap into the expertise of your local tooling rep.
They've got the insider knowledge on using their tools best, and will get you on the right track
for your application. Thanks for watching this first episode of Haas U, and we'll see you next time.

