Guide
Should you use a form tap or a cut tap in a cast aluminum hole?
A form tap is a fluteless tap that makes an internal thread by pushing metal sideways into the thread shape instead of removing it as chips; a cut tap is the conventional fluted tap that machines the thread and carries the chips out. In die-cast aluminum both work, but they need different hole sizes, react differently to draft and porosity, and leave different evidence in the finished thread.
By Saola Manufacturing engineering team · Published · Updated
This guide is for design engineers and sourcing managers who own a die-cast aluminum or zinc part with threaded holes and need to decide three things: whether the hole is cast (cored) or drilled, which kind of tap goes into it, and what the drawing has to say so any competent supplier makes the same thread. It draws on the thread standard and published design guidance listed at the end.
On this page
What is the difference between a form tap and a cut tap?
A cut tap removes metal with cutting edges and flutes, so the hole starts close to the thread’s minor diameter; a form tap displaces metal with rounded lobes, so the hole starts larger and the metal flows up into the thread crests. That single difference drives almost every practical consequence below.
Because nothing is cut away, a form tap produces no chips. In a blind hole that matters: chips packed at the bottom of a cut-tapped hole are a common cause of broken taps, short threads and loose debris that later falls into an assembly. Cold forming also leaves the thread flanks work-hardened and smooth, and a NASA fastener reference notes that cold-rolled threads gain fatigue resistance from compressive surface stress (NASA RP-1228). That statement is about rolled bolt threads, so treat it as the mechanism, not a rating for an internal thread in a casting.
The trade-offs run the other way too. A form tap needs more torque than a cut tap of the same size, and the pre-hole has to be held more closely, because the hole size decides how much metal is available to fill the thread. The formed thread also has a small seam at its crest where the displaced metal meets, which is normal and does not show on a go/no-go plug gauge, but surprises inspectors who have not seen it before.
Can you form tap die-cast aluminum like A380 or ADC12?
Yes, in most cored and drilled holes, provided the hole is sized for forming and the alloy is not one of the very low-ductility grades. The deciding factors are alloy, porosity near the hole wall, and how accurately the hole is made.
General forming guidance published in the tooling trade press asks for a workpiece elongation of about 8% and a hardness no higher than about HRC 30, yet the same source states that cored holes in die-cast aluminum and zinc form-tap readily when the core pins are sized for it (Cutting Tool Engineering, 1995). Bulk elongation figures for high-pressure die-cast aluminum-silicon-copper alloys are low, so do not read that guidance as a pass/fail test for a casting; read it as a warning that the less ductile the alloy, the more a trial matters.
Alloy choice shows up clearly at the extremes. NADCA describes alloy 390, the hypereutectic wear alloy, as having the lowest ductility of the die-casting alloys, with elongation under 1%, and notes that iron-rich intermetallic particles in aluminum alloys reduce ductility and act as fracture starting points (NADCA, aluminum alloys). In a 390 part, expect a formed thread to tear at the crests; a cut thread or an insert is the safer default. A380 and its close equivalent ADC12, covered in the ADC12 vs A380 guide, sit in the middle and are routinely threaded either way.
Porosity is the other factor. Forming presses the hole wall outward, so a gas pore just under the surface can collapse into the thread instead of simply opening, as it would with a cut tap. Both methods work best in the dense skin a cored hole keeps; drilling or reaming a cored hole oversize removes that skin before the thread is made.
What hole size does each type of tap need?
Per the percentage-of-thread formulas used by tap makers, a form tap needs a noticeably larger hole than a cut tap for the same thread, typically close to the thread’s pitch diameter rather than its minor diameter. Using a cut-tap drill chart for a form tap is the most common way to break form taps.
| Thread | Cut tap hole (in) | Form tap hole (in) | Difference (in) |
|---|---|---|---|
| #10-24 UNC | 0.155 | 0.172 | 0.017 |
| 1/4-20 UNC | 0.208 | 0.228 | 0.020 |
| 5/16-18 UNC | 0.266 | 0.288 | 0.022 |
| 3/8-16 UNC | 0.322 | 0.347 | 0.025 |
Two things follow from the table. First, the gap between the two holes is small in absolute terms, so a hole that is right for one tap is wrong for the other; the drawing or the process sheet has to say which tap the hole is for. Second, the form-tap hole is more sensitive: per the same formula, every thousandth of an inch of hole size moves thread engagement by roughly twice as much as it would with a cut tap, which is why forming asks for a better-controlled hole.
For metric threads the same formulas apply with pitch in millimeters in place of 1/TPI. Whatever the system, check the finished thread against its class with gauges per ASME B1.1 (or ISO 965-1 for metric), not against the drill size.
Engagement above about 65% to 75% adds little strip strength but a lot of tap torque, which is typical shop guidance for both tap types. In soft or porous metal, strength comes more easily from a longer engagement length: NASA’s fastener manual sizes the depth of a tapped hole from the shear strength of the weaker material, so a steel screw in an aluminum casting simply needs more thread depth (NASA RP-1228).
How should a cored hole with draft be sized for tapping?
Size the core pin so its diameter at about half the required thread depth equals the target pre-hole for the chosen tap, and add a chamfer at the mouth to take the metal a form tap pushes up. That is the approach described for roll-form tapping of cored holes in Cutting Tool Engineering (1995).
The reason is draft. A core pin must taper so it can be pulled from the solidified casting, and NADCA notes that holes need more draft than any other die-cast feature because the metal shrinks onto the pin (NADCA, draft; NADCA, holes and windows). A tapered hole gives more thread at the bottom than at the mouth. Placing the nominal size at mid-depth splits that difference, so the mouth runs a little light and the bottom a little heavy.
Zinc die-casting guidance published by the International Zinc Association makes the same trade-off explicit: where a full thread is not needed, core the hole for about 60% thread at the large end and 75% at the small end; where a full thread is essential, remove the taper before tapping or use much less draft; and keep threaded depth within about twice the screw diameter (IZA, zinc die casting design rules). The same logic carries over to aluminum, where holes need more draft than in zinc.
For deep threads in drafted holes, a light drilling pass to a straight size before tapping is often the cleaner answer, at the cost of cutting through the cast skin. The die casting page covers how cast features and machined features are split on a part.
When should a threaded hole be cored, drilled, or fitted with an insert?
Core the hole when volumes justify the core pin and the thread is not a critical seal or locator; drill it when position, straightness or depth is critical; and add an insert when the thread must survive repeated assembly or carry more load than the parent aluminum can. The table summarizes the usual pattern.
| Situation | Hole | Tap | Why |
|---|---|---|---|
| Blind mounting hole, general fastening | Cored | Form | No chips to clear; keeps the dense cast skin; one operation |
| Through hole in a thin boss | Cored | Form or cut | Forming bulges thin walls; check boss wall before choosing form |
| Thread that locates or aligns a mating part | Drilled or cored and redrilled | Cut or form | Position and perpendicularity come from the machining setup, not the pin |
| Port that seals against pressure | Drilled | Cut (tapered threads) | Tapered pipe threads are cut; seal faces are machined; watch porosity |
| Thread assembled many times in service | Cored or drilled | Tap for insert | An insert gives a wear-resistant thread in soft metal |
| Hypereutectic or very low-ductility alloy | Either | Cut | Formed crests tend to tear in brittle alloys |
Inserts deserve a word of their own. NASA’s fastener manual describes them as the standard way to give a strong, wear-resistant tapped hole in soft materials such as nonferrous alloys, and as the usual repair for stripped threads (NASA RP-1228). Wire-thread inserts go into a hole tapped with a special oversize tap; some solid and thread-forming insert types go into a plain cored or drilled hole. Either way the insert type goes on the drawing, because the hole under it is not the hole for the screw.
Machining the hole after casting is a CNC milling operation on most housings, often combined with facing the boss so the thread starts square to a machined surface.
How should the drawing specify a tapped hole in a casting?
Call out the thread by standard and class, give the full-thread depth, and state separately whether the hole is cored or drilled and whether the thread may be formed, cut, or either. Leave out any of these and two suppliers can make two different holes from the same drawing.
- Thread and class. For example 1/4-20 UNC-2B per ASME B1.1, or M6x1-6H for metric. Class 2B or 6H is the normal choice for tapped holes in castings; tighter classes add cost without much benefit in aluminum.
- Full-thread depth, not drill depth. State the minimum depth of full thread. For a cored blind hole, also give the minimum cored depth so the pin leaves room below the last thread.
- Method note. “Thread may be cut or formed” gives the supplier freedom. “Formed thread required” or “Cut thread required” locks it, which is right when you have tested one method, for example for strip torque or leak behavior.
- Cored hole definition. If the hole is cored, show it as a cast feature with its own size at a stated depth and the draft direction, or reference the core pin drawing. A hole shown only as a thread callout leaves the pin size to the die designer.
- Gauging. Say the thread is accepted by go/no-go plug gauges for its class. Because a formed thread’s crest is shaped differently from a cut one, agree up front whether minor diameter is inspected, and with what.
Tolerance notes for the cast and machined features around the hole are covered in the ISO 2768 and NADCA tolerance guide.
What should you check when moving a threaded casting to a new supplier?
Ask for the core pin sizes and the tap type actually used, because neither is usually on the part drawing, and both decide whether the new supplier’s threads behave like the old ones. This matters most when a die is moved or rebuilt, for example when production shifts from China to Vietnam.
If the incumbent form-taps cored holes and the new source drills and cut-taps them, the parts will pass the same gauges but may differ in strip torque, in chips left in blind holes and in how porosity shows up in the thread. None of that is wrong, but it should be a decision, not a discovery. A short checklist for the first articles:
- Confirm the pre-hole method (cored or drilled) and the tap type for each threaded feature.
- Gauge every thread with go/no-go plugs and section one or two holes to see thread fill and any porosity at the crests.
- Run the assembly torque on sample parts, with the production screw, to the value your assembly line uses.
- Check blind holes for chips or loose flakes, especially where the part goes into a sealed or clean assembly.
The RFQ package guide lists what else to send with the drawing. When the package is ready, send it for a quote; the reply can call out, hole by hole, whether a thread is proposed as cored and formed or drilled and cut.
Frequently asked
Is a formed thread stronger than a cut thread in aluminum?
Often it is at least as strong, because the grain is displaced rather than cut and the flanks are work-hardened. In porous or low-ductility castings the advantage can disappear, so test strip torque on real parts before relying on it.
Can I use my normal tap drill chart for a form tap?
No. A form tap needs a larger hole than a cut tap for the same thread, so use the tap maker’s forming chart or the forming formula shown above. A cut-tap hole overloads a form tap and often breaks it.
Do form taps work in zinc die castings?
Yes. Zinc alloys such as Zamak 3 are generally well suited to forming, and zinc design guidance covers coring holes for tapping directly. Size the cored hole for the forming tap and keep draft low where a full thread is needed.
Why does my formed thread have a line at the crest?
That is the seam where metal flowing from both flanks meets. It is a normal feature of formed threads and does not affect go/no-go gauging; a very open seam usually means the pre-hole was too large.
Is a roll tap the same as a form tap?
Yes. Roll tap, roll-form tap, thread-forming tap and fluteless tap are names for the same tool: it displaces material into the thread shape instead of cutting it out as chips. That is why it needs a larger pilot hole than a cut tap of the same size.
Sources
- ASME B1.1-2024, Unified Inch Screw Threads (UN, UNR, and UNJ Thread Forms), ASME, 2024
- Fastener Design Manual, NASA Reference Publication 1228, R. T. Barrett, NASA Lewis Research Center, 1990
- Draft, NADCA Design, North American Die Casting Association, accessed September 2026
- Holes and windows, NADCA Design, accessed September 2026
- Aluminum alloys, NADCA Design, accessed September 2026
- Zinc die casting design rules, International Zinc Association, accessed September 2026
- Threads Will Roll, D. Gajdosik, Cutting Tool Engineering, 1995