Cut Tap Tid-Bits

To All:
Just saw this article in Cutting Tool Engineering. Thought it was
pretty good. Most of it is the basic stuff most everyone already
knows, but there might be a couple of points (pun intended), that might
be new.
The video with a side-by-side comparison between a HSS & carbide tap
is cool.
Some excerpts from the article are below.
formatting link

Understanding Tap Geometry
Tapping problems can be simplified and reduced by understanding tool
geometry and what taps are best suited for a given application.
For example, lowering the chip load can eliminate premature wear on a
tap. Defined as the load induced on any one cutting edge, chip load is
typically controlled by altering the feed rate. As mentioned earlier,
this is not possible when tapping but the chip load can be altered
through tap selection.
One approach might be to use taps with more flutes. With every flute
added to the tap, a cutting face is added. With more cutting faces, the
load on each tooth is reduced. For example, a 4-flute tap would have
half the chip load per tooth of a 2-flute tap. This jives with standard
metalcutting advice, which is to always use a maximum number of flutes.
However, for tapping this advice would probably be wrong.
?More flutes means there is less space for chips as they are cut,? said
David Miskinis, senior application specialist, holemaking for
Kennametal Inc., Latrobe, Pa. ?More flutes on the same circumference
means smaller flutes, both in width and depth. With smaller space comes
the risk of packing chips, which can lead to broken taps.?
So, while adding flutes may not be an option, choosing a different
chamfer length might be.
?Basically, a longer chamfer length means longer tool life,? said Dr.
Peter Haenle, president of Guhring Inc., Brookfield, Wis. ?The load
during the cutting process is distributed over a longer cutting edge
with a lower chip load.?
There are three common lengths of tap chamfers: taper at 7-10 threads,
plug at three to five threads and bottoming with one to two threads. To
provide more options, tap manufacturers have added a few more forms,
including a form consisting of a two- to three-thread length, sometimes
called semibottoming.
Adding length to the chamfer distributes the chip load over a longer
cutting face. Effectively, more teeth are cutting the thread, similar
to a single-point threading tool taking multiple passes.
?Chamfer lengths have a huge impact on tap life because they affect
chip load,? Miskinis explained. ?When comparing chamfer lengths of four
threads or fewer, the tool life will double for every half thread added
to the length.?
Clearly, increasing chamfer length in taps is desirable. Shorter
chamfer lengths, such as in bottoming taps, wear faster and should be
avoided, if possible. Unfortunately, there may not always be a choice.
?Taps with smaller chamfer lengths are usually used to keep the
difference between hole depth and thread length to a minimum,? Haenle
said. ?Very often, the design of the part forces the use of taps with
short chamfer lengths.?
Another way to tap more effectively is to manage chip thickness. For
example, it is possible to thin the chip too much when tapping. Stringy
chips can result from using taper chamfers and the tap may create a
bird?s nest of chips, preventing lubricant from reaching the tool and
chips from properly evacuating. As in other types of machining
operations, increasing chip load can help break the chips.
Tap breakage is another issue that creates anxiety among machinists.
The saying goes that it?s not the fall that kills you, it?s the sudden
stop. But in tapping, it?s not the sudden reversal that causes taps to
break, it?s the chips clogging the tool flutes. In some cases, this
means chips are packed so tightly so that newly formed chips simply
have no place to go, and the tap breaks from the stress.
Tackling Flute Clogging
Even if chips don?t pack so tightly that the tap breaks, flute clogging
keeps lubricant away from the tool/workpiece interface and the friction
of the chips on the tap creates excessive heat. Chip flow is a critical
part of successful tapping. Which direction the chips should move is a
factor of the type of hole to be tapped: through or blind. A
spiral-flute tap lifts chips out of a blind-hole. The helical angle
directs chips out of the hole.
The spiral flute can be referred to as slow, with 15° to 30° helical
angles, or fast, with 40° to 60° angles. Faster spirals have a
freer-cutting geometry, while slower spirals have a stronger cutting
edge. Typically, fast spirals are for softer workpiece materials or
materials that produce stringy chips, while slow spirals are for
short-chipping, harder materials.
A spiral-point, or gun, tap pushes the chips ahead of the tap when
tapping a through-hole. The spiral point itself is actually a
left-handed spiral, ground only at the point of the tap, which creates
a downward flow of chips. Otherwise, a spiral-point tap looks like a
straight-flute hand tap.
Because the flutes of spiral point taps are not actually needed for
chip evacuation and are instead applied to allow lubricant in, they can
be shallow. Thus, they permit a larger core and a stronger tap. This
also means that spiral-point taps can benefit from additional flutes
without the problem of chip packing.
Selecting a Tap
Because tapping is a relatively complex operation, and because there
are so many taps to choose from, selecting a tap can seem a daunting
task. The main reason there are so many taps is because there are so
many work materials. Tap manufacturers tailor tap design to the work
material primarily through rake and relief.
The cutting face is that portion of the tap flute located between the
major and minor diameter of the thread that cuts, or shears, the
workpiece. The rake is the angle of the cutting face compared to a line
from the center of the tap to the cutting face at the major diameter.
Courtesy of OSG
A rake is positive if the crest of the cutting edge is angularly ahead
of the remaining part of the face. While not as strong as negative
rakes, positive rake angles have excellent shearing capabilities.
A negative rake has the crest of the cutting face behind the rest of
the cutting face. While this is a stronger geometry than a positive
rake, it also requires more torque and creates more heat in the cut.
The shape of the cutting face is also a factor in tap performance.
Cutting faces can also be straight or curved. The straight surfaces are
normally referred to as rakes or straight rakes and the curved surfaces
as hooks.
?Applying a rake, or straight face, will improve strength while a hook,
or curved shape, will result in greater shearing ability,? said Andrew
Strauchen, engineering and marketing manager, OSG Tap & Die Inc.,
Glendale Heights, Ill. ?For performance taps, cutting [rake] angles are
determined by the intended work material; higher angles are used for
softer materials and low angles for harder materials.?
Tap relief is defined as the removal of metal from behind the cutting
edge. A higher relief indicates more clearance between the tool and the
workpiece. There are three main types of relief: concentric, eccentric
and con-eccentric.
Concentric relief indicates that the lands of the tap, the part of the
tap that remains after the flutes are cut, are concentric with the
threads. This actually provides no relief and thus the surface of the
tap rubs on the surface of the threads being cut.
Hand taps are made with concentric relief. Because they are used by
hand, cutting speeds are low and friction and heat do not limit tool
life. Because the lands are concentric, the threads on the tap help
guide the tool into the threads on the workpiece as they are cut.
Eccentric relief means that the lands are cut to an arc that is not on
center with the bulk of the tool. This type of relief provides the best
clearance between the tap and the thread being cut. Because the tool
doesn?t rub against the material, friction can be minimized.
Con-eccentric relief is a combination of the other two styles. A small
part of the land remains concentric at the leading edge while the rest
of the relief is eccentric. This style provides a balance between
reduced friction, as provided by eccentric relief, and tool guidance,
as provided by concentric relief.
Concentric relief and, to a lesser degree, con-eccentric relief taps
rub the workpiece material as the tool enters and exits the hole,
causing friction, which in turn produces heat. Heat diminishes tool
life. As a result, premium taps are most often made with eccentric
relief. ?The higher the relief, the lower the friction of the tool,?
Haenle said. ?Therefore, a higher relief results in less wear and
longer tool life. However, a lower relief guides the tool better in the
axial direction because it has less tendency to cut in the radial
Premium taps are not for all machines. A high-end tap will not guide
itself when creating the thread. Therefore, taps with eccentric relief
require the machine?s feeding mechanism to be highly accurate.
?In newer CNC machines, you can use taps with higher relief angles,?
Haenle said. ?On the other hand, when using older equipment or drilling
machines with less rigidity and with standard tapping chucks, a smaller
relief angle helps to guide the tap better.?
Reply to
Loading thread data ...
One could arger, tho, that the first couple of flutes do the vast majority of the cutting, consistent with a recent ditty here (or on rcm) that only a few threads are involved with bolt/nut strength.
I have seen cut taps where the thread cutting part is mebbe 3/8-1/2 long, and everything in back of this clearance. At first kind of eye-brow raising, but it made sense.
Which suggest that cut taps could be made a lot more inexpensively, with no loss in performance, and, ito chip-induced breakage, proly increased performance. I may try experimenting with this, just grinding off most of the threads beyond the first 1/2".
Reply to
Proctologically Violated©®
If the tap is being driven by a machine using rigid tapping, the 'extra' threads have little purpose. Hand tapping they likely center the tap and add to keeping the pitch correct. Maybe you have something there.
Reply to
Blind holes, use a spiral tap and report back.
Reply to

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.