Guide
Thread milling or tapping: which should make the threaded holes on your part?
Thread milling is a CNC process in which a rotating cutter, smaller than the hole, travels a helical path around the bore and generates the thread one orbit per pitch. Tapping does the same job with a tool that already carries the finished thread size and form, driven straight into the hole and reversed out.
By Saola Manufacturing engineering team · Published · Updated
Both methods can produce a thread that passes the same go/no-go gauge, so the choice is about risk, cycle time and the hole itself. This guide covers where each method fits, what the thread standards control, how cast aluminum and zinc change the picture, and when a drawing should name the method at all. It describes processes and standards, not the equipment of any particular shop.
On this page
What is the practical difference between thread milling and tapping?
A tap is a one-size tool: its diameter, pitch and form are fixed, so one tap makes one thread. A thread mill is a profile tool: the machine’s program sets the diameter, so one cutter can make any size with the same pitch, internal or external, right-hand or left-hand.
A tap removes the whole thread in one stroke, which makes it fast and simple to program, but the full cutting load sits on one slender tool buried in the hole. If it binds and snaps, a broken tap in a finished part is often the end of that part.
A thread mill takes the thread in light, interrupted cuts while the machine interpolates a helix. The cutter is smaller than the hole, so chips have room to leave and a broken cutter usually comes out without damaging the bore. The cost is time: the tool has to orbit the hole, sometimes more than once, and the machine needs three-axis helical interpolation and a program for every thread.
Form taps, also called roll taps, are a third route: they displace material into the thread shape instead of cutting it, and are common in ductile aluminum and zinc alloys.
When is tapping the better choice?
Tapping is usually the right default for small and medium standard threads in free-cutting materials at production volume. It is the quickest way to make a thread, needs no special programming, and a rigid-tapping cycle on a modern CNC holds pitch well.
Tapping wins most clearly in these cases:
- Many identical small holes. A bolt pattern of fine threads in a cover or bracket taps in a fraction of the time a thread mill would need to orbit each hole.
- Small diameters. Below a certain size, a thread mill small enough to fit the hole is fragile and deflects, while a tap of the same size is comparatively robust.
- Soft, ductile alloys with form taps. Cast and wrought aluminum and zinc alloys are commonly form tapped, producing a chip-free thread with a work-hardened surface.
The limits of tapping are the same things that make it fast. One tap fits one size and one class, so a thread that needs its pitch diameter nudged, for instance to leave room for plating, needs a different tap. Blind holes need extra drilled depth below the last full thread, because the chamfered lead of the tap cannot cut a full profile at the bottom.
When does thread milling make more sense?
Thread milling pays off when the part is valuable, the thread is large or unusual, or the hole is awkward for a tap. It trades cycle time for control and for lower risk of losing the part to a broken tool.
- Large diameters. Big taps need high spindle torque and are costly to stock; one thread mill can cover a range of large sizes that share a pitch.
- Expensive or late-stage parts. When a thread is one of the last features on a heavily machined housing, the lower risk of a jammed tool is worth the extra seconds.
- Tapered pipe threads. A tapered thread such as NPT per ASME B1.20.1 can be milled with a profile cutter that follows the taper in the program, instead of a taper tap that must cut the full taper at once.
- Pitch-diameter control. Because the program sets the size, the machinist can move the pitch diameter within the class limits with a tool offset, which helps with a close class or a thread that will be coated afterward.
- Interrupted or thin-walled holes. Cross-drilled bores and thin bosses tolerate the lighter radial load of a thread mill better than the torque of a tap.
Thread milling has its own limits. A long, slender cutter deflects, which can leave the thread slightly tapered along a deep hole unless the program adds spring passes. The cutter also cannot reach a full thread right at the bottom of a blind hole. Neither limit is a reason to avoid the process, but both are reasons to state the full-thread depth on the drawing. On lathe work the question often does not arise at all, because internal threads on turned parts are commonly single-point threaded with a boring-bar style tool.
Does the threading method change the thread class or strength?
No: the class is defined by the limits in the thread standard and proven by the gauge, not by the tool that made the thread. A tapped 2B thread and a milled 2B thread are the same thread if both pass the same gauges.
| Class | What the standard says | What it means for method choice |
|---|---|---|
| 1B | For quick, easy assembly where a liberal allowance is needed, even with slightly bruised or dirty threads | Rare on new drawings; any method works |
| 2B | The most commonly used class for general applications, including bolts, screws and nuts; minimum diameters are basic, with no allowance, whether or not plated | Tapping with a standard tap is normal; milling where the part or hole calls for it |
| 3B | For applications where closeness of fit and accuracy of lead and angle matter; obtainable consistently only with high-quality equipment and efficient gauging | Either method, but milling makes size adjustment easier; gauging matters more than the tool |
| 6H (metric) | A tolerance class in the ISO 965-1 system for internal threads: grade 6 with fundamental deviation H, which places the minimum pitch diameter at basic | The usual general-purpose metric callout; standard taps are made for it |
One practical consequence follows from the table. Per the class definitions in NBS Handbook H28, internal classes 1B, 2B and 3B have basic minimum diameters and no built-in allowance for coating. A plated or anodized internal thread therefore needs its pre-coating size stated, and a thread mill makes that easier to hit than a stock tap does. The finishing comparison guide covers how much each coating adds.
Strength is also a function of geometry, not method. The pull-out formula in NASA Reference Publication 1228 ties the load a tapped hole can carry to the pitch diameter, the length of engagement and the shear strength of the weaker material. In practice that means a weak thread in a soft casting is fixed by more engagement length or a thread insert, not by switching from a tap to a thread mill. Form tapping is the one method choice that can change the surface itself, because it cold-works the flanks instead of cutting them.
How should threads be made in aluminum and zinc die castings?
In most die castings the hole is cored close to size, then threaded by tapping or thread milling after casting. Internal threads are rarely cast in, because an internal thread needs an unscrewing core that slows the casting cycle.
The zinc die-casting design rules published by the International Zinc Association make the same point: machining an internal thread is usually cheaper than casting it, with exceptions for very coarse threads and single-turn threads. External threads can be cast when the parting line bisects them, but that asks for high die accuracy.
Cored holes carry draft, so they are slightly tapered. That taper matters for the threading method. A tap follows the hole it is given, so a tapered core produces a thread that is fuller at one end than the other. The same design rules suggest coring a hole to be tapped for about 60% of a full thread at the wide end and 75% at the narrow end where a full thread is not required, and removing the taper first where it is (IZA design rules). A thread mill, by contrast, cuts to the programmed diameter and position, so it can clean up a slightly shifted or tapered core in one operation, as long as enough stock is there.
Three habits help on cast parts sent for die casting and machining:
- Say which holes are cored and which are drilled. The supplier then knows whether the thread is cut into as-cast skin or into freshly drilled metal.
- Mark pressure-tight threads. Threading can open subsurface porosity near a core, so ports that must seal need that stated, and may need impregnation after machining.
- Allow for form tapping. ADC12 and Zamak 3 are both commonly form tapped. If a cut thread is required for a reason, write it down; otherwise let the method stay open.
Should the drawing specify thread milling or tapping?
Usually not: specify the thread, its class, its full-thread depth and how it is gauged, and leave the method to the supplier. Name a method only when the function of the part depends on it.
A complete callout already carries everything that governs fit. A metric thread reads like “M8x1.25-6H” per ISO 965-1, and an inch thread like “1/4-20 UNC-2B” per ASME B1.1, followed by the full-thread depth for blind holes. Naming a method on top of that constrains the supplier without improving the part, and it can force a slower or riskier route than the one the shop would pick.
There are legitimate exceptions, and each one should be written as a requirement with its reason:
- No form tapping, where the displaced crest of a formed thread would interfere with a seal or a mating part.
- A stated pre-plating size, where the thread is coated and must still gauge after finishing.
- A thread insert, where the design calls for helical coil inserts in a soft casting; the insert maker’s tap size then replaces the plain thread callout.
Left open, the method becomes a quoting decision: small holes are typically tapped on the CNC milling setup and large or tapered ones milled.
What should you ask an overseas supplier about threaded holes?
Ask how each thread will be gauged, not only how it will be made. A supplier in Vietnam or anywhere else should confirm the gauge standard, the class, and which threads are checked on every part and which are sampled.
- Gauges. Unified threads are gauged per ASME B1.2 and metric threads per ISO 1502. Ask whether go/no-go plug gauges for each size and class are on hand or need to be bought for the job.
- Coated threads. Ask whether the thread is gauged before or after finishing, and make sure both sides read the drawing the same way.
- Method flexibility. If the drawing leaves the method open, ask which holes will be tapped and which milled; the answer shows whether the supplier has thought about the large and tapered threads.
The RFQ package guide lists the rest of what to send with the drawing, and the tolerance guide covers the general notes that sit next to a thread callout. When the package is ready, send it for a quote; threads that need a method discussion are raised in the reply, feature by feature.
Frequently asked
Is a milled thread stronger than a tapped thread?
Not inherently. Thread strength depends on the thread size, the engagement length and the weaker material, as the NASA fastener manual’s pull-out formula shows. A formed thread has cold-worked flanks, which is the one method difference that changes the surface.
Can NPT threads be tapped instead of milled?
Yes. Taper taps are common for pipe threads, and the hole is often taper reamed or drilled first. Milling is an alternative that avoids the high torque of a full taper cut, particularly on larger sizes or valuable parts.
Do I need class 3B to get a precise thread?
Only if the fit needs it. Per the H28 class definitions, 2B is the general class for bolts, screws and nuts, and 3B is reserved for applications where closeness of fit and lead accuracy matter. A 3B callout raises gauging cost whether the thread is tapped or milled.
What are the downsides of thread milling?
On most small holes it takes longer than a tap, which cuts the thread in a single pass. It needs a machine that can run three-axis helical interpolation and a CAM or hand-written program for each thread, the smallest hole it can reach is limited by the cutter diameter, and on long threads the slender cutter can deflect, which shows up as taper or an undersize pitch diameter toward the bottom of the hole.
Can threads be cast directly into a zinc die casting?
External threads can, when the parting line splits them. Internal threads need an unscrewing core, so they are usually cored plain and threaded afterward, according to the International Zinc Association design rules.
Sources
- ASME B1.1-2024, Unified Inch Screw Threads (UN, UNR, and UNJ Thread Forms), ASME, 2024
- ISO 965-1:2026, ISO general purpose metric screw threads — Tolerances — Part 1: Principles and basic data, ISO, 2026 (replaces ISO 965-1:2013)
- Screw-Thread Standards for Federal Services, Handbook H28, Part I (section 4, classes of threads), National Bureau of Standards, 1969
- Fastener Design Manual, NASA Reference Publication 1228, R. T. Barrett, NASA Lewis Research Center, 1990
- Zinc die casting design rules (tapping, threads, cast screw threads), International Zinc Association, accessed September 2026