Technical Tips - Threading
A tap must have a chamfer to create a thread. Chamfers are the tapered or incomplete threads at the front of the tap.
The major diameters of the threads are ground to a smaller diameter at the front. This is known as the point diameter and is slightly smaller that the pre-drilled hole size or tap-drill size.
When the tap enters the hole and begins to cut, each tooth in the chamfer gradually enlarges the thread in the part. Only the first full thread behind the chamfer produces the finished size of the thread. The teeth beyond the first full thread guide and support the tap as it completes the threaded depth of the tapped hole.
The most common lengths of standard chamfers are taper, plug, and bottoming. The taper chamfer has 7 to 10 threads tapered; plug has 3 to 5 threads tapered; and bottoming has 1 to 2 threads.
A taper chamfer, often called a starter tap, is used for roughing or heat-treated material. Plug is the most common and preferred chamfer for most tapping applications. Bottoming chamfers are used when there is not enough depth of hole for the taper or plug.
Chamfer lengths are selected based upon the type of hole to be tapped. If the hole goes completely through the part or if the drill depth is considerably deeper than the required thread depth, a taper or plug chamfer is used. A bottoming chamfer should be avoided, and used only when the threads must come close to the bottom of the drilled hole. A bottoming tap creates the greatest amount of torque, requires slower speed (RPM), produces a rougher finish, and reduces tool life substantially.
In addition to taper, plug, and bottoming chamfers, there are semi- and modified-bottoming chamfers found on specialty taps (such as high-performance taps and some cast iron taps used in the automotive industry). Semi-bottoming chamfers are typically 2 to 2-1/2 threads in length; modified-bottoming chamfers range between 2-1/2 and 4 threads in length depending on the tap style. The additional length helps to reduce chip load, add tool life in difficult-to-machine materials, and enable higher tapping speeds.
It is important to use the longest chamfer possible for the tapped hole condition. Sometimes this includes purchasing a special. An increase in chamfer length will result in an increase in tap life!
To determine the longest chamfer for blind holes, subtract the full thread length required plus one pitch from the drill depth. The extra pitch enables clearance at the bottom of the hole for spindle over-spin and chips. Then divide this figure by the number of threads per inch (TPI). The resulting number is the recommended chamfer length. Select a tap with a chamfer length no longer than this figure.
Example:
Size: ¼-20 NC
Full thread length: .250
Drill depth: .473
Pitch: 1/ 20 = .050
.473 - .250 - .050 = .173
(drill depth minus full thread length and one pitch)
.173 ÷ .050 = 3.5
(new drill depth divided by threads per inch (TPI)
3.5 = recommended chamfer length
In this case, select a standard tap with thread chamfer no longer than 3.5.
For a safety margin, a 3-thread chamfer may be preferable.
A 4-flute semi-bottoming tap has 12 working teeth; a bottoming tap has 8. The semi-bottoming tap has 50% more tap teeth to dramatically improve tap life!
By selecting a tap with a longer chamfer length, you will reduce chipload per tooth and tapping torque, enabling increased tapping speeds and tool life. When tapping harder steels and space-age alloys such as nickel, titanium and stainless, a longer chamfer length may determine success or failure.
Specifying the proper chamfer length will ensure greater tool life. For each chamfer tooth added, the tap life will increase exponentially.
The use of carbide tooling has increased dramatically. The benefits include reducing costs by running tools longer and faster, while producing parts with greater precision. Carbide taps can provide the same benefits, which is advantageous for long production runs.
One of the most significant improvements made to carbide has been increased toughness. This has made carbide taps more practical than in the past.
Carbide taps should be run in rigid or synchronous CNC or lead screw machines with precise feed capability. Taps should be held rigidly or in synchronous holders with TG or TGHP collets, or hydraulic or shrink fit adapters.
If the tap has a driving square, use ER collets specifically designed for taps with a square-drive feature. Excessive movement may cause chipping or breakage. Therefore, tension-compression float holders and conventional quick-change tap adapters should be avoided.
Taps have a unique problem when exiting a hole, unlike drills. Because taps must reverse direction and back out of the hole, they encounter stringy or continuous cut chips. Through-coolant for blind-hole tapping is highly recommended to flush the chips from the hole. This prevents the chips from becoming entangled with the tap teeth and causing chipping and breakage. If the workpiece material produces very short, broken chips or powdery chips (such as with gray cast iron), through coolant is not required.
Because carbide taps are designed to run faster, machine tools should have at least 250 SFM or higher tapping speed capability.
NOTE: The machine tool’s rated maximum RPM is usually for drilling and milling, not tapping. When tapping, the machine may be capable of only one-third of stated RPM value.
AccordianPage
HOW TO BUY
Contact Kennametal US Representative 800.446.7738
Contact Kennametal UK Representative +44/1384 408060
