Resources
Threads in aluminium: tap, form tap, or insert?
Published 2026-08-27
Threads are the feature drawings skim over: a size, a depth, and the rest is left to the shop. Yet they fail more often than most features, and they usually fail in the customer's hands — the third time someone opens the housing in the field, the thread strips. This is a walk through the three routes into an aluminium thread, and the handful of lines your drawing is probably still missing.
Three routes: cut it away, push it aside, or bring in another material
Cut tapping removes material — the tap shears the thread groove out and turns it into chips. It is the universal option: any position, any size, any material, and the lowest cost. Two prices come with it. Aluminium is gummy, so with the wrong cutting conditions the flanks tear and built-up edge appears. And chips in a blind hole have to be evacuated properly, because any that stay behind ride into your assembly.
Form tapping does not cut at all. The tap displaces material and lets it flow into the thread profile, producing no chips whatsoever. The displaced metal work-hardens and the grain flow follows the form, so a rolled thread in the same alloy is generally stronger and stands up better to repeated tightening than a cut one. The ductility of the 6xxx alloys sits right inside the window form tapping wants, which is why it is far more common in aluminium than in steel.
An insert changes the material altogether: a steel threaded element is set into the aluminium hole, so a steel screw now engages steel threads and the aluminium only carries the load. It costs the most and adds an operation, but it takes the weakest link — the aluminium thread itself — out of the load path. None of the three is better than the others; they are matched or mismatched to the job.
Answer one question first: how many times will this thread be tightened?
That question splits the decision more sharply than load does. Aluminium threads rarely fail by pulling out; they fail by being worked. Every tighten-and-release cycle wears the flanks, and since aluminium is much softer than the steel screw, the part always yields before the fastener does. For a joint made once and never touched again — structural joints, brackets that get bolted down permanently — a cut or formed thread in the aluminium is entirely adequate. For anything opened repeatedly — a housing serviced in the field, a mechanism with a consumable, a test fixture — design for an insert from the first drawing, rather than retrofitting one after the returns start.
The second question is whether anyone controls the tightening torque. If assembly uses a torque wrench and a specified value, aluminium threads have a predictable life; if it is an air gun and an operator's feel, design for the worst case. This belongs on the drawing as a line of its own: state the assembly torque if you have one, and if you do not, write that the supplier should propose it. A question parked on the drawing survives; one parked in a phone call does not.
Third is engagement length. At the same thread size, aluminium needs more engagement than steel to reach a comparable joint strength, because the aluminium flanks strip first. How much more depends on alloy, temper, fastener grade and the actual load — it is not a number you can lift from a formula. If material thickness is already tight in that area, do not invent an engagement depth on your own; write down what the joint has to carry and let the shop work it out while they are quoting.
When form tapping gives the better thread — and when it is not an option
Three advantages are real in aluminium. No chips, so blind holes carry nothing out with them — which matters most on parts headed for anodizing, where trapped chips are a contamination source in the tanks. The flanks are dense and work-hardened, so they take repeated tightening better. And form taps last far longer, which on a production quantity makes the per-part cost lower rather than higher. On volume aluminium work it is frequently the default, not a special request.
It does come with conditions. The pre-drilled hole matters far more than it does for cutting: undersize and the tap will break, oversize and the crest never fills, leaving an incomplete thread. Cut tapping forgives a loose pre-hole; form tapping does not — which is why it suits planned production better than a one-off part machined from a drawing that changed yesterday. It also demands more torque, so very small sizes and hard tempers get difficult. And it only works on material with enough ductility: aluminium alloys are ideal, castings and brittle materials are not.
One more point is worth settling in advance, because it starts arguments at inspection. A formed thread leaves a fine seam along the crest, where the displaced material closed up at the top. It looks like an incomplete form. It is not — it is inherent to the process, and it does not affect a go/no-go gauge result. Inspectors seeing it for the first time regularly reject the parts. If your drawing permits form tapping, add a note saying the crest seam is a normal feature of a formed thread and save everyone a round trip.
Inserts and rivet nuts are a design choice, not a rescue
Helical coil inserts are the most familiar: a steel wire coil wound into an oversized aluminium thread to create a steel internal thread. The benefit is not only that it is now steel — the coil has some give, so load spreads across more turns instead of concentrating on the first one or two. Note that it needs a larger tapped hole and its own tap, so the boss has to have material around it. And one common type has an installation tang that must be snapped off and retrieved after fitting; that is a genuine foreign-object risk, so the drawing should say who is responsible for removing it.
Key-locking inserts — a solid steel bushing with keys driven into the parent metal — are tougher and better under vibration, which suits high load and field-repairable joints. And when the wall is simply too thin to hold a thread at all (our thinnest wall runs down to the 0.7 mm class, where tapping stops being a meaningful conversation), the real answer is a blind rivet nut or a self-clinching nut: the first needs access from one side only and grips by deforming, the second is pressed into ductile sheet. Both are limited by the parent material, and both spin out if the hole is oversized or the wall too thin — so the hole tolerance ends up mattering more than the thread does.
One route gets overlooked. If the part is machined from an extrusion, check the section for a screw port before you specify anything. A screw port designed into the profile takes a thread-forming screw directly, with no secondary operation at all — the cheapest fastening available. The catch is that the joint location has to line up with the section at design time. Once the parts are machined, you are back to tapping or an insert.
The lines your drawing actually needs
The most common ambiguity in a thread callout is the depth of a blind hole. With a single depth figure on the drawing, the shop may read it as the drilled depth or as the full-thread depth, and the two differ by the incomplete threads the tap leaves at the bottom. Nothing about that surfaces during quoting; it surfaces when the first article is measured. Dimension the two depths separately and the problem never arises.
The other frequent one is process sequence. An anodic film grows on the surface, and it grows on both flanks of the thread, accumulating on the pitch diameter until a thread that was in tolerance is now tight — sometimes tight enough that a go gauge will not pass. There are three ways out: tap after anodizing, mask before it, or write the acceptance requirement for the post-anodize condition. Any of them works, but the drawing has to pick one; do not assume the shop will think of it for you. Functional threads especially — cosmetic ones can be left loose.
As for tolerance class, standard general practice covers almost everything and needs no call-out. Only when the fit is genuinely sensitive is it worth naming a class from ISO 965 explicitly — 6H for an internal thread, for instance. The finer you specify, the more gauging and labour you pay for, and the logic is exactly the same as with dimensional tolerances: tighten what has to be tight, and leave the rest alone.
| Put this line on the drawing | The problem it heads off |
|---|---|
| Drilled depth and full-thread depth dimensioned separately | One depth figure on a blind hole reads two ways — and a wrong read is a whole batch |
| State whether form tapping is permitted or prohibited | Settles whether the crest seam counts as a defect, before the rejection arrives |
| Say whether threads are cut before or after finishing | Anodizing thickens both flanks; the wrong order fails a go gauge |
| For inserts, give the full part call-out, who installs, who removes the tang | Fitting and tang removal are two separate costs and one FOD risk |
| Call for go/no-go gauging on threads that matter | Otherwise 'it screwed in by hand' becomes the acceptance criterion |
| State the assembly torque, or say the supplier should propose it | In aluminium the thread gives up on torque long before it gives up on load |
| Mark thin-wall areas as no direct tapping | Moves the rivet-nut-or-thicker-boss decision forward into quoting |
Not settled yet? Send the drawing before you fix the call-out
Thread choices depend heavily on the specifics. The same size behaves differently on a structural bracket than on a housing opened every quarter, and the same wall thickness leads somewhere else depending on whether there is room beside it for a boss. In our workflow every drawing gets an engineering read before it gets a price — which holes suit form tapping, which ones we would recommend an insert for, where the wall will not carry a direct thread, whether tapping should come before or after finishing — and those notes come back with the quote instead of surfacing at first article.
So there is no need to lock the process down for us in advance. Put the purpose of each threaded hole in a note, along with the expected number of assembly cycles, the fastener grade it mates with and the service condition, send the drawing with the STEP, and we will settle the rest together. Changing one line of a thread call-out at the quoting desk always costs less than replacing a stripped part at a customer site.
Keep reading