Aluminum Extrusion Tolerance: A Stage-by-Stage Guide

An as-extruded aluminium profile typically holds ±0.15 to ±0.50 mm on a functional dimension, depending on its circumscribing circle and wall thickness. Machine it and you can reach ±0.02 to 0.05 mm — but only on features cut from a machined datum, in a single setup, where the wall is thick enough not to move under the tool.

Those two sentences answer the question most drawings get wrong. Not because the numbers are hard, but because a drawing carries one tolerance while the process chain carries four, and each stage eats a different share of it.

What are you actually specifying when you write a tolerance?

Three different things get called "tolerance" in a typical RFQ, and mixing them is where projects lose money.

Die tolerance is what the extrusion press can hold as the profile leaves the run-out table. It is a function of the die, the alloy, the quench rate and the wall-thickness spread. It is the loosest of the three and the hardest to improve after the die is cut.

Machining tolerance is what a second operation can hold on features it cuts. It is a function of fixture rigidity, tool deflection and thermal stability — not of the machine's brochure accuracy.

Assembly tolerance is what survives after parts are stacked, bolted and aligned. It is the sum of everything upstream, plus the joint itself.

The failure pattern is consistent: a design engineer needs ±0.05 mm at assembly, writes ±0.05 mm on the profile drawing, and sends it to an extruder. The extruder quotes it. Two things then happen, and both are bad. Either the price doubles because the shop plans to inspect and sort every piece, or the shop quietly ships standard tolerance and the problem surfaces at the customer's assembly line three months later.

A drawing that separates the three stages costs nothing to produce and removes that entire failure mode.

Where does the tolerance go, stage by stage?

The table below is what we quote against. Every value is a reference capability, not a guarantee — the value that applies to your order is set by your drawing, and we confirm in writing what we can hold before quoting.

Stage	Typical achievable	What actually governs it
As extruded — dimension	±0.15 – 0.50 mm (0.006 – 0.020 in)	Circumscribing circle, wall spread, alloy, quench
As extruded — straightness	1 – 3 mm/m	Cooling uniformity, stretcher setup
As extruded — twist	1 – 2°/m	Wall symmetry, die balance
Sawn length	±0.1 mm (0.004 in)	Saw stop, blade condition, feed rate
CNC milled feature	±0.02 – 0.05 mm	Fixture, tool deflection, thermal drift
Hole position, same setup	±0.02 mm	Machine positioning, not the cutter
Hole position, across setups	±0.05 – 0.10 mm	Datum transfer, fixture repeatability
Bent — radius position	±0.4 mm (0.016 in)	Springback, mandrel, temper
Bent — angle	±0.2 – 0.5°	Temper consistency, tooling compensation
Anodised — per surface	+0.010 – 0.025 mm	Film thickness spec (10 – 25 µm)

One row deserves emphasis because it is misread more often than any other: straightness and dimension are not interchangeable. A profile can be dead-on ±0.2 mm in section and still bow 2 mm over a metre. If the drawing specifies only section tolerance and the application is a linear rail, the part will be rejected for a reason nobody wrote down.

Why is the as-extruded tolerance so wide?

Because the profile is formed at roughly 500 °C and measured at 25 °C, and the difference has to be built into the die.

Aluminium 6xxx expands about 23.4 × 10^-6 per °C. Over a 475 °C drop that is a 1.11% linear contraction. A 200 mm circumscribing circle shrinks 2.2 mm on cooling. The die is cut oversize by that factor, but the factor is only exactly right for one wall thickness — and a real profile has four or five different wall thicknesses cooling at different rates.

That asymmetry is the origin of most twist and bow. A section with a 3 mm wall on one side and a 1.2 mm wall on the other does not cool evenly, does not shrink evenly, and does not come out straight. No amount of die polishing fixes a section that is thermally unbalanced by design.

Three more contributors stack on top:

• Stretching. Profiles are pulled 0.5 – 1.5% after quenching to straighten them. This fixes bow and twist but moves dimensions by 0.1 – 0.2 mm, so it trades one tolerance for another.
• Die wear. A die runs 5 – 20 tonnes of aluminium in its life. By end of life, bearing wear can shift a dimension 50 – 100 µm. A part made on day 1 and a part made on month 18 are not identical.
• Quench rate. Faster quenching buys strength (T6) but increases residual stress, which shows up later as distortion during machining. Slower quenching is straighter but softer.

This is why EN 755-9 and GB/T 6892 exist as they do: they describe a commercial envelope, not a precision target. Quoting inside that envelope is normal. Quoting well inside it is a different conversation with a different price.

What can actually reach ±0.02 mm?

Four conditions, all required:

1. One setup. Everything that must relate to each other is cut without unclamping. Cross-setup position error is 2–5× the same-setup error.
2. A machined datum. The reference surface is cut, not extruded. An extruded face carries the die's tolerance plus 1–3 mm/m of bow; using it as a datum injects that error into every feature measured from it.
3. Adequate wall. Below about 1.2 mm, cutting force deflects the wall more than the tool. See CNC milling of aluminium profiles for the deflection arithmetic.
4. Short tool overhang. A Ø12 mm cutter at 40 mm overhang deflects roughly 0.09 mm under a 300 N cut — four times the positioning accuracy of the machine doing the positioning.

What reliably reaches ±0.02 mm: milled faces, milled slots, bored holes, drilled holes in one setup, on sections with walls of 1.5 mm or more.

What does not: thin side walls, long-reach features, large flat faces (they move with temperature, not with the tool), and any dimension that spans two setups. Drilling and tapping has the same limits on hole position, and precision sawing is where the 0.1 mm length tolerance comes from before machining starts.

What do bending and anodising add?

Bending is the stage where tolerance is most often lost, because springback is not a machining error and cannot be dialled out at the control. 6063-T5 springs back 3–8° depending on the R/t ratio; the tool must be cut to over-bend by that amount. Radius position lands around ±0.4 mm and angle around ±0.2–0.5° in production. For a curved rail, a ±0.2° error on each side of a mitre compounds into a visible gap at the joint.

Anodising adds material, and the addition is not symmetric with your intent. Film builds 10–25 µm per surface, so every external dimension grows and every internal dimension shrinks by twice the film thickness.

Take a Ø20 H7 bore: the entire tolerance band is 21 µm (+0.021 / 0). A 15 µm film on each wall reduces the diameter by 30 µm — more than the whole band. The bore is out of tolerance before the part is even inspected. The fix is either to machine it after anodising, or to specify the pre-anodised dimension with the film allowance built in and say so on the drawing.

Sequence matters too. Bend, then stress-relieve, then anodise. Anodising a bent part and bending it afterwards cracks the film at the outside of the radius, and no touch-up hides it. Details are on the anodised aluminium profile page.

What should be on your drawing?

• Mark only the dimensions that function. Three to five tight tolerances is normal. A drawing with forty ±0.05 mm callouts is not a precision part, it is a part that will be quoted at three times the price and still argue at incoming inspection.
• Send everything else to a general tolerance. ISO 2768-m is the usual choice and removes 90% of the argument.
• Name the datum type. Write "machined datum" — not just a letter on an extruded surface.
• Say whether the dimension applies before or after finishing. This single note prevents more rejections than any other.
• On long parts, specify straightness per metre, not over the full length. A 6 m part at 0.5 mm/m is a reasonable call; 0.5 mm over 6 m is a different and much more expensive part.
• State the measurement method for parallelism, concentricity or position. If the method is not agreed, the first inspection becomes a negotiation.

If the drawing is not settled yet, the cheapest step is a DFM review before the die is cut — precision machining and die design interact, and a wall change at drawing stage costs nothing while the same change after tooling costs a new die.

Dónde esto no aplica

Small sections with thin walls. Below roughly 30 mm circumscribing circle with walls under 1.2 mm, both extrusion tolerance and machining tolerance widen. The material moves more than the numbers above allow.

Parts longer than about 5 m. Self-weight starts to matter in both measurement and fixturing. Straightness figures measured on a 6 m part include the sag of the part itself, and two inspectors with different support spacing will disagree.

7xxx alloys. The extrusion window is narrow and the quench sensitivity is high. A 7075 or 7050 profile will not hold a tighter tolerance than 6082-T6, and it will cost considerably more. If the requirement is strength rather than tolerance, that is a different decision — but do not expect tighter numbers from the harder alloy.

Blanket ±0.02 mm with 100% inspection. If every dimension on a part must be held at ±0.02 mm, the honest answer is that the part should be redesigned. Guaranteeing it by sorting means paying for the parts that get scrapped, and no supplier can promise the yield.

Preguntas frecuentes

Can you hold ±0.05 mm on an extruded profile?

On machined features, yes — that is inside the normal CNC band of ±0.02–0.05 mm. On the extruded surface itself, no. An as-extruded dimension runs ±0.15–0.50 mm. If a ±0.05 mm callout lands on an unmachined face, either the face gets machined or the tolerance gets relaxed.

Should the tolerance be specified before or after anodising?

State it explicitly, because the answer changes the part. A 20 µm film per surface moves an external dimension +40 µm and an internal dimension −40 µm. For bores and shafts that mate, specify the finished (post-anodising) dimension and let the shop carry the allowance.

How much does tightening a tolerance cost?

It is not linear, and it is not mainly machine time. Moving from ±0.10 mm to ±0.05 mm usually costs 20–40% more, mostly in fixturing and slower feeds. Moving below ±0.02 mm tends to double the price, because it changes the process — temperature-controlled room, in-process gauging, and often a second stress-relief cycle.

Is EN 755-9 the same as GB/T 6892?

They cover the same subject — extruded profile tolerances — and are broadly comparable in structure, but the tables are not identical and the grade naming differs. If a drawing cites one and the shop quotes against the other, the difference shows up at inspection, so name the standard and the grade on the drawing.

Qué enviarnos

Send the drawing with the tolerance intent marked and we will return a DFM note listing which callouts we can hold as drawn, which need a process change, and which are cheaper to redesign. That review happens before any tooling is committed, and it is where most of the avoidable cost sits.

Correo: linjunbing@truetrustlv.com  |  WhatsApp: +86 136 6644 0600

Sylvia Lin — Shanghai Truetrust Aluminum Industry Technology Co., Ltd.