For many years, engineers sought improved twist-drill performance.
In the quest, they developed solid-carbide drills, carbide tips,
superabrasive inserts, powder-metal steel, new HSS alloys, and, most
recently, titanium nitride (TiN) coatings. However, these new materials
do not work alone. To yield longer tool life and better performance,
they must be coupled with proper geometry and good tool design. Here
are some cases where more expensive special tools proved to be cheaper
in the long run because they cut overall production cost or did a better
job. Often, we didn’t even need the exotic new tool materials.
For example, Figure 1 shows an application where a standard drill
wandered off course. To drill a 0.1122″-dia through-hole into an
injector nozzle, our customer first tried a jobber-length drill working
through a bushing. He found he couldn’t get the bushing close
enough to the workpiece surface to handle the oblique entry and exit.
Because of the angled entry, holes were often off-center, and heavy
lateral forces acted on the drill, causing excessive land wear and
premature drill failure.
The solution was simple. Our trouble-shooting engineers wanted to
keep a good length of the plain portion of the drill shank engaged in
the bushing before the tool point made contact with the work. Therefore,
they reduced the flute length by 50 percent, leaving the overall drill
length the same as before. This design greatly increased drill
rigidity, and, coupled with a special 140-degree drill point, solved the
problem. Yes, the special drill cost twice as much as a standard, but
tool performance quadrupled, and overall productivity increased eight
Another customer had a simple job, but wanted longer tool life. He
was drilling sheet packs, each consisting of 10 sheet-metal plates
31.5″ X 59″ X 0.118″. The 0.394″ (10 mm) jobber drills originally used could not cope. Frequent breakages occurred on
the corners of the cutting edges.
To solve this problem, our engineers modified standard jobbers by
grinding a double-angle point, using 118 degrees and 90 degrees. This
design, similar to that used for cast iron, doubled tool life. The point
was also specially web thinned to reduce thrust load and pressure on the
sheets that formerly had tended to bend. A further benefit, the
double-angle design aided breakthrough, avoiding grabbing and leaving a
clean, burr-free finish to the underside of the hole.
The difficulty in machining GRP is well known to many tool
engineers. In the application shown in Figure 2, a simple 1/4″-dia
hole was needed, but conditions were severe. The graphite material was
embedded in a sandwich. The top layer consisted of stainless steel, the
bottom, aluminum. The first choice would normally be a heavy-duty
drill, but this won’t deliver the exact concentricity and burrless
performance demanded by the user.
Beginning with a tungsten carbide base, we designed a special step
drill with no margins at the pilot diameter. The step served for
predrilling and as a guide pilot. The guide allowed the larger diameter
to finish the hole through the sandwich with minimum torsional
To reduce burr formation, we reduced the standard 32-degree helix
angle to 22 degrees. Tool life proved to be 200 holes between regrinds.
The tools served in pneumatic drilling guns, suggesting that carbide is
not as fragile as some might think. It will handle severe jobs as long
as it can be kept from vibrating and facing intermittent cutting.
In another case, the task was to drill 0.2953″-dia
through-holes 0.6693″ long in 100 Cr 6 having a hardness of 99.5
RB, Figure 3. The drill ran horizontally at 835 rpm with a feed of
0.0039 ipr. Coolant was soluble oil. Unfortunately, even a drill
bushing could not keep the hole concentric. And there were burrs at the
The user tried solving the problem by dividing the operation into
two steps. First he predrilled a pilot hole, and then finished with a
core drill. But this was too expensive. Our solution used a HSS
subland drill with special diameters of 0.2953″ and 0.2362″,
and a step length of 0.2362″. The smaller diameter handled
predrilling and centering, and also served as a pilot guide.
To aid centering, we gave the tool a split point to form C with
coinciding center lines. Thus, the pilot stabilized the countersink
diameter (0.2953″), which worked as a core drill in this case.
Good chatter-free cutting was achieved with improved hole finish.
Here’s a problem we could blame on the workpiece, but of
course we had to solve it just the same. After a bending operation, the
piece shown in Figure 4 required realignment of prepunched holes. The
manufacturer tried to use a core drill to correct the average
0.0197″ error. It would have worked except for flexing of the
relatively flimsy workpiece.
To meet the challenge, we modified our standard No 533 core drill
to a point angle of 195 degrees to improve centering ability and greatly
reduce burr formation. The required accuracy ruled out use of a
conventional pilot diameter. Instead, we built a drilling jig designed
to compensate for thrust load and eliminate flexing of the joint plate.
After some effort to finalize drill-bushing guidance, the setup
increased production rates.
A deep-hole assignment is shown in Figure 5. The 0.1024″-dia
hole had to be drilled 3.622″ deep with maximum axial-alignment
error of only 0.03937″. Depth-to-diameter ratio was 35, and the
material was C 45 round bar.
We first thought of our standard deep-hole drills, which tackle
depths up to 15 times drill diameter, usually without pecking. But
would the design work with a ratio of 35? To find out, we built a
high-speed cobalt drill with a specially optimized profile similar to
the GT 100 type. Its length was 5.512″, with flute length of
3.937″, point angle of 130 degrees, and standard web thinning.
Trial runs were better than expected. Average alignment accuracy
was 0.0177″, with 0.0374″ maximum. We told the customer he
could use a setup with 17 withdrawals, 2820 rpm, peripheral cutting of
75.5 sfm, and 0.000 59 ipr feed. On the job, the tools gave 42 holes
per regrind, some 20 percent more than originally specified.
We dealt with a really intractable material for the workpiece shown
in Figure 6. It was a rotor body made of V4A vanadium steel, requiring
a 0.3937″-dia center hole. The user’s plan required first
drilling with a 3/16″ carbide-tipped tool, then countersinking with
a solid-carbide tool having the required 60-degree form. He used a
cutting speed of 213 sfm for both operations, feeding manually and
flooding with a soluble-oil coolant. If lucky, he got six pieces per
grind. Often, one of the tools broke before he even got six!
The solution was to use a cheaper tool. We decided that cobalt
super-high-speed steel would work better than carbide. We designed a
special centerdrill made of cobalt high-speed steel and told the user to
run it at a much slower surface speed than used for carbide. This loss
was amply made up by the increased feed rate made possible. More
efficient cutting angles eliminated the breakages that plagued the
former setup, and drill life between regrinds increased to 18 or more
parts. Thus, a lower-cost tool allowed a single setup, longer too life,
and less downtime. Carbide isn’t always the answer.
No drill would work in the hard laminated silicon sheets shown in
Figure 7. The user wanted to drill a 0.150″-dia blind hole 1″
deep in the hard sheets–in the direction of the laminations! All
combinations of drills, feeds, speeds, and coolants failed. After a
slight penetration, all cutting surfaces became completely blunt.
We found that the sheets formed hard grainy swarf when drilled
together in the plane of the laminations. The hard swarf immediately
dulled cutting edges. Furthermore, drills would not withstand the great
heat generated in the operation.
Our solution took the form of a drill made of cobalt alloyed
high-speed steel. It works better in sophisticated material and can
take much more heat. A high-pressure air-hose pipe was installed to
blow chip fragments off the hole before they could affect the drill. We
took 20 cuts at 30 sfm and 0.0024 ipr. After 20 holes, only slight wear
marks appeared on the cutting edges, and the lands showed no visible
Benefits of hard coating
As suggested earlier, many given tools, whether specials or
standards, can be improved by coatings that make tool-edge surfaces very
hard without affecting the condition of the base material. For
instance, a TiN coating (what we call an S coating) can dramatically
increase tool life, sometimes by more than 2000 percent.
We have tested coated twist drills on a wide range of workpieces
and find they almost always offer longer life than identical uncoated
tools. This is particularly true when the tool must cut highly abrasive
materials, workpieces prone to cold welding, hard or abrasive nonferrous
alloys, and difficult materials including synthetics.
The coating treatment also improves finish in the hole–so much so
that secondary reaming can often be eliminated.
Through holes are generally much more demanding on a drill than
blind holes. Surprisingly, tests show an even greater increase in
performance in through holes than in blind holes. These results are
attributable to the wellbonded, wear-resistant coating.
The coating also reduces cutting forces. We tested thrust and
torque in a number of applications. For example, in a through-hole
operation on 35 Rc plate steel 1.1811″ thick, using
0.2953″-dia drills, thrust loading of an S-drill was 17 percent
less than that required for an untreated tool. Also, the range of
thrustload variation was reduced by 75 percent with the coated drill.
In the same test, torque load was lessened and was more uniform with the
coated drills. These benefits stem from reduced resistance to chip flow
with treated drills. Also, the coating has a smooth, oily surface that
aids cutting action.
TiN coatings at work
Coating benefits range from significant to spectacular. For
example, in 1045 medium carbon steel with a hardness of 16 to 23 Rc,
Figure 8, performance increased 500 percent. The rocker bearing
required a 0.315″-dia through-hole, 1.338″ deep, bordering on
a tangential 1.575″-dia hole. Cutting speed with a
competitor’s standard cobalt HSS drill was 66 sfm at 0.005 ipr
feed. The setup used a horizontal spindle, hydraulic feed, and
soluble-oil coolant. Tool life was 105 holes, with occasional drill
breakage brought about by unstable performance and drill flexing.
Switching to a GT 100 S-treated drill of the same type increased
performance 500 percent, producing 530 holes before regrind. Even after
regrinding, the drills machined 320 holes, allowing safe programming for
300 holes per tool change.
In cutting a 0.394″-dia hole 0.591″ deep in armor plate
hardened to 38 to 43 Rc, production increased from 12 holes per tool to
50 holes, an increase of 415 percent. Cutting speed was 33 sfm at
0.0051 ipr in a vertical spindle with automatic feed drive. Standard
cutting oil served as coolant.
The yoke plate in Figure 9 is made of free-cutting 12L13
resulphurized carbon steel. Two 0.512″-dia through holes are
drilled to a depth of 0.224″. The original taper-shank tool
machined 2100 parts before regrinding, compared to 20,500 parts for an
S-coated drill of the same type. Even after repointing, the TiN-coated
tool processed 11,300 parts. The improvement amounts to 980 percent for
first use, and 550 percent after regrinding. Spot drilling was not
required. Instead, the vertical spindle fed the drill through a
bushing. Very rich soluble oil served as coolant for the 85-rpm,
Finally, consider this last case. The workpiece was 316 stainless
steel, requiring a 0.236″-dia through-hole to a 1-3/16″
drilling depth. Three tools were tested at 26 sfm, 0.0024 ipr, in a
vertical spindle with mechanical drive. The operation used soluble-oil
coolant and required two drill withdrawals. A premium cobalt HSS tool
lasted for only 30 cuts; an HSS drill with TiN coating survived 110
holes, but a cobalt HSS tool with TiN coating drilled 675 holes.
That’s a performance increase of 2250 percent!
For small holes or large, nonferrous materials, soft workpieces,
cold-extruded materials, superhard tool steels–and almost anything
else–TiN coatings generally provide significant tool-life improvement.
Even if tool life is only doubled, the coating pays for itself in tool
cost alone, not to mention overall productivity gains and reductions in
Nothing is as easy as it first appears, and there are some things
to watch for in applying TiN coatings. For example, the coating
increases surface hardness of the tool from 80 Rc to greater than 2000
Vickers. It’s harder than tungsten carbide. Because hard
materials are sensitive to vibration and chatter, you must make setups
as rigid as possible, with no axial or radial play in the
drilling-machine spindle or backlash in the feed mechanisms.
The drills are resharpened in exactly the same way as standard or
cobalt HSS tooling. Although coated-drill performance is lowered
somewhat by regrinding, it remains superior to that of untreated drills.
Maximum performance of coated drills is achieved by increasing the
cutting speed while maintaining the same feed rate. This results in
better tool life and superior hole surface finish. However, you do have
to watch details carefully. Drill geometry can drastically affect the
life of coated drills, as illustrated in Figure 10.
For more information about special drills, circle E21.