The subject of threads and threading often relates to various aspects such as coarse and fine threads, tolerance classes, form, angle, and pitch. In this article, we will focus on the two primary methods for creating internal screw threads: tapping and thread milling and when to choose one over the other.
What is Tapping?
At first glance, a tap resembles a bolt or screw with grooves along its sides. These grooves serve to remove chips from the hole during machining, while the sharp edges on the end and periphery cut the threads. Taps function similarly to rotary tools, being held in a chuck, collet, or special “floating” tool holder and driven into the workpiece at a specific feed rate.
There are two important considerations: the presence of a hole slightly larger than the thread’s minor diameter (as taps only cut on the outer edges) and a feed rate precisely matching the thread’s pitch. For example, a 1/4″-20 tap must advance 0.05″ per revolution (or 20 threads per inch) to create a proper thread.
Taps come in various types. Plug taps are used for threading “through-holes,” while bottom taps can produce threads almost reaching the bottom of blind holes. Spiral point taps help drive chips forward, while spiral flute taps direct chips upward and out of the hole.
Forming or roll taps, unlike cut taps, don’t generate chips. Instead, they displace material similarly to the thread-rolling process mentioned earlier. Form taps follow the same rules as cut taps regarding feed rate and tool geometry but require a slightly larger pilot hole to accommodate the displaced metal. However, form taps are suitable for ductile materials like aluminum, stainless steel, and superalloys but not for cast iron or hardened steel.
TOOLIND spiral flute taps offer high performance for steel and steel alloys, stainless steel, cast iron, nickel- and cobalt-based alloys, titanium and titanium alloys, aluminum, and hard steel.
What is Thread Milling?
Thread milling also requires a pre-drilled hole. However, unlike cut and form taps, thread milling provides greater flexibility in terms of feed rates, thread sizes, and programming approaches. It functions like a milling cutter, removing material radially along its peripheral edges. The flutes of a thread mill mirror the thread form itself, creating the thread as they move.
Note the mention of “programming approach.” Unlike tapping, which can be performed on various machine tools or even manually, thread milling is only possible on CNC machining centers, Y-axis equipped mill-turn centers, or multitasking lathes. However, thread milling allows programmers more freedom in machining approaches, materials they can work with, and even the size of the threaded hole. For example, a single 20-pitch thread mill can create any thread size as long as it has 20 threads per inch and doesn’t exceed the tool’s maximum cutting depth.
A thread milling operation begins by driving the cutter into the center of the drilled hole at a relatively fast rate, followed by a small arcing motion to move the tool radially into the workpiece until it reaches the required diameter. The rotating thread mill then completes one full circle while moving upward (in the Z-axis) by an amount equal to the thread pitch. In the case of a 1/4″-20 thread, this would be 0.050″ or one complete turn. Once the thread is complete, the tool disengages by performing another small arcing motion back to its starting point before withdrawing from the hole.
The above description provides a generic programming outline. Tough materials like Inconel or titanium might require multiple passes or “spring passes.” Different arcing strategies can be employed, and since the feed rate is not dependent on the thread pitch as with tapping, programmers have the flexibility to adjust their strategies based on machining conditions and the type of tool being used. The example described a typical path for a “full profile” thread mill. However, some manufacturers offer “single-plane” thread mills that must trace the entire thread from top to bottom, circling round and round until reaching full depth.
TOOLIND high-performance solid carbide thread mills incorporate various design elements to enhance thread quality and tool production. Short chips that are easily evacuated generate less heat and friction, reducing the risk of threading damage. Moreover, superior carbide grades make threading easier and reduce machining times.
Which Method Should You Use?
As with many decisions in manufacturing, the choice between tapping and thread milling depends on several factors. Each method has its pros and cons, and selecting one over the other depends on production quantity, material hardness or toughness, available machine tool power, accuracy requirements, and personal preference. Here are some considerations to help you make a decision:
Speed: Generally, tapping is slightly faster than thread milling. Depending on the workpiece material, thread depth, and machine tool speed, tapping a 1/4″-20 thread, for example, might take around 4-5 seconds, while milling it with a full-profile cutter could take approximately twice that time. Single-plane thread mills that require multiple passes are much slower, but they are the exception rather than the rule. In most cases, the speed difference between milling and tapping is negligible unless dealing with high-volume production.
Power: Tapping requires significant torque to create a complete thread in a single pass, especially in tough materials. For threads larger than approximately 3/4″ in diameter, only powerful machining centers with geared heads can handle the task. Thread milling, on the other hand, doesn’t have such limitations and can machine threads of any size.
Size: There is a caveat to the previous point. Very small threads, such as those used in wristwatches and certain medical devices (e.g., #000 and smaller), may have limited availability for thread mills. In such cases, tapping might be the only viable choice, particularly if the threads are more than a few diameters deep.
Tool life: Thread milling has an advantage in tool life. Most taps are made of high-speed steel (HSS), while thread mills are typically made of carbide, providing longer tool life (and the ability to operate at higher spindle speeds). If a worn tap breaks inside the hole (a common occurrence), there is a high risk of damaging or scrapping the workpiece. Thread mills are more predictable in this regard, and if one breaks during operation, it is more likely that the workpiece can be salvaged.
Flexibility is the key advantage of thread milling. When tapped threads deviate from the desired tolerance, adjusting to a different “H-size” tap becomes necessary, which is available in small increments. However, thread milling allows for a simple offset adjustment to bring the threads back within specifications. Moreover, taps are designed for specific thread sizes and types, often tailored to specific materials. In contrast, a full-profile 16-pitch thread mill can cut any 16-pitch thread (as long as it fits in the hole), and the same applies to a 20-pitch thread mill for 20-pitch threads and so on. Single-plane thread mills can cut threads of any size or pitch by modifying the program.
However, it’s worth noting that this flexibility is also thread milling’s downside. The programming involved is admittedly more complex, which is why some shops tend to avoid it. Nevertheless, with the abundance of online programming calculators and widespread computer-aided manufacturing (CAM) support for thread milling, there’s no reason to avoid it, especially considering its enhanced flexibility and thread quality.
Regardless of the chosen method, it is crucial to adhere to best practices. Always use the appropriate toolholder. Machines without a rigid tapping function require a tension-compression holder or a self-reversing tapping head, while synchronous tap chucks like the one offered by TOOLIND should be used in other cases. Thread mills are best held in high-quality milling chucks, such as hydraulic, mechanical, or shrink-fit holders. It is advisable to avoid side-lock holders and collet chucks.
If through-the-tool coolant is available (a common feature with thread mills), it is recommended to use clean, high-pressure cutting fluid. On the other hand, when tapping, it may be necessary to stop the machine and apply a small amount of wax or specialty fluid into the hole to prevent seizing. Regardless of the chosen approach, it is essential to carefully consider the options and make informed decisions. Except for high-volume applications, thread milling often proves to be advantageous, although tapping still has its merits. If unsure, don’t hesitate to seek guidance from the experts at TOOLIND, as we specialize in threading.