Aluminum Milling: Feeds, Speeds, and Tooling That Beat Built-Up Edge
Aluminum is the fastest metal to mill and the easiest to get wrong. Feeds-and-speeds starting points by operation, the alloy behavior that changes them, and the tooling rules that keep edges clean.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 10 min read
On this page
Quick Answer
Mill 6061-T6 aluminum with 2–3 flute polished carbide at 800–1,500 SFM roughing and 1,500–3,000 SFM finishing, chip load 0.002–0.005 in per tooth to start. The number one failure is built-up edge — aluminum welding to the tool — and the cure is counterintuitive: go faster, feed a real chip, and keep the tool sharp. Avoid AlTiN-coated tools, never let chips sit in the cut, and treat soft alloys (5052, 1100, O-temper) with more respect than hard ones.
Aluminum Milling: Fast, Forgiving, and One Trap
Aluminum is where milling is fun: cutting speeds an order of magnitude above superalloys, low cutting forces, and material that forgives mediocre setups. 6061-T6 — density 2.70 g/cm³, tensile 310 MPa — is the default stock for a reason. But one failure mode dominates every aluminum-machining conversation: built-up edge (BUE), where aluminum pressure-welds to the cutting edge and quietly ruins your finish and dimensions. Nearly every rule in this guide — the speeds, the chip loads, the tool coatings — exists to keep that from happening.
Aluminum Feeds and Speeds: The Starting Table
These are proven starting ranges for carbide in 6061-T6, compiled from tooling-vendor and shop references. Treat them as a first pass: prove them against tool life and finish, then climb. The two formulas that turn the table into a program: RPM = (SFM × 3.82) ÷ tool diameter, and feed rate (IPM) = RPM × chip load × flute count. A worked example: a 1/4″ 3-flute carbide end mill at 700 SFM runs 10,696 RPM; at a 0.0025″ chip load that is 80 IPM.
| Operation (6061-T6, carbide) | Cutting Speed (SFM) | Chip Load per Tooth | Notes |
|---|---|---|---|
| Rough milling | 800–1,500 | 0.002–0.005 in | Higher end needs rigidity + good chip evacuation |
| Finish milling | 1,500–3,000 | 0.001–0.003 in | Sharp 2-flute for finish + evacuation |
| Drilling (carbide) | 500–800 | 0.006–0.008 in/rev class | Spot first — aluminum grabs |
| Drilling (HSS) | 200–400 | 0.004–0.008 in/rev class | Polished flutes, peck on deep holes |
| Conservative start (any op) | 300–800 | 0.002–0.005 in | If in doubt, start here and climb |
Note what the table does not say: “slower is safer.” In aluminum the opposite is true — BUE forms at low surface speed, and raising SFM past roughly 820 (250 m/min) is the standard cure. If the finish suddenly goes cloudy and the edge looks lumpy, speed up before you slow down.
The Alloy Changes the Answer
“Aluminum” on a drawing covers alloys that mill very differently. The counterintuitive part: the soft alloys are the difficult ones. 5052 and 1100 are ductile and BUE-prone; pure 1100 is the worst built-up-edge offender of the common alloys despite being the softest. The hard tempers — 7075, and 6061 kept at proper speed — chip cleanly.
| Alloy | Milling Behavior | Watch Out For | Typical Parts |
|---|---|---|---|
| 6061-T6 | The benchmark — clean chips, forgiving | T651 temper runs gummier than expected; keep speeds up | Brackets, plates, frames, most prototypes |
| 7075-T6 | Harder, chips break cleaner than 6061 | Higher cutting forces; not weldable | Aerospace and high-stress parts |
| 2024-T3/T4 | Good chips, fatigue-rated | Poor corrosion resistance — plan the finish | Aircraft structures |
| 5052 / 1100 | Soft and ductile — the BUE champions | Built-up edge, smearing; raise SFM, sharpen tools | Enclosures, formed-and-milled sheet parts |
| Cast plate (MIC-6 class) | Stable, stress-free, machines flat | Porosity under the skin on critical faces | Fixture and tooling plate |
Grade-by-grade material details live on our aluminum CNC machining page, and the head-to-head decisions are in 6061 vs 7075 and 6061 vs 5052.
End Mills for Aluminum: What Actually Matters
Flute count first: 2- or 3-flute carbide, because aluminum’s big fast chips need open gullets to escape — a packed flute is a broken tool. Helix: high-helix geometry (35–45°) shears cleaner and lifts chips out. Coating: none, or an aluminum-specific one (ZrN, TiB2, DLC). Avoid AlTiN and other steel-oriented coatings — aluminum has a chemical affinity for them and welds on faster. Edge: polished flutes and a keen edge beat every other variable combined; a dull tool in aluminum plows, rubs, and builds up.
Hold the work like you mean it, too: aluminum’s low cutting force tempts light clamping, but thin walls and floor features chatter the moment rigidity slips. Trochoidal or adaptive toolpaths at 5–15% of tool diameter stepover keep engagement constant, cut chatter, and routinely deliver 2–4× the material removal rate of full-width step-downs.
Coolant and Chips: One Rule
The real coolant rule for aluminum is not “always flood.” It is never let chips stay in the cut. Re-cut chips are how flutes pack, edges build up, and tools snap. Soft wrought grades want MQL, mist, or flood to control built-up edge; harder alloys often run fine on a strong air blast. Deep pockets and slots need a chip-evacuation plan — through-tool air, coolant aimed at the flutes, and retractions on deep drilling. WD-40 on a manual mill is folk wisdom with a real mechanism (lubricity against BUE), but on a production CNC the answer is engineered coolant delivery, not a spray can.
From Feeds and Speeds to Finished Parts
If you landed here researching parameters for your own machine, the table above will get you cutting. If you landed here because the parts need to exist — prototypes this week, production next quarter — that is the other half of what we do. IsoCNC mills aluminum daily, from single 6061 brackets to 7075 aerospace parts in 5-axis cells, with anodizing and finishing under one roof. Our CNC milling service page covers capability and equipment, the quote guide covers what to send, and CNC vs 3D printing helps if you are still picking a process. Send the drawing — an engineer reviews every RFQ, typically within 1–2 business days.
FAQ: Aluminum Milling
What SFM should I use for milling aluminum?
For 6061-T6 with carbide: 800–1,500 SFM roughing and 1,500–3,000 SFM finishing are the production ranges, with 300–800 SFM as a conservative starting band for less rigid setups. Counterintuitively, going too slow is the common failure — built-up edge forms when surface speed is too low, and raising SFM past roughly 820 (250 m/min) is the standard cure. Convert to RPM with RPM = (SFM × 3.82) ÷ tool diameter; a 1/4-inch end mill at 700 SFM is about 10,700 RPM.
What chip load should I use milling aluminum?
Start at 0.002–0.005 inches per tooth for general work in 6061 — a 1/2-inch end mill can run 0.004–0.008 per tooth, and smaller tools scale down. The floor matters more than the ceiling: below roughly 0.0003 inches per tooth the tool rubs instead of shearing, which is exactly how built-up edge starts. Feed rate follows from chip load: IPM = RPM × chip load × flute count. If chips are dust instead of curls, feed harder.
What is the best end mill for aluminum?
A 2- or 3-flute carbide end mill with a high helix (35–45°), polished flutes, and either no coating or an aluminum-specific one (ZrN, TiB2, or DLC). Flute count is about chip room: aluminum’s big, fast chips need open gullets, which is why 2- and 3-flute tools beat 4-flute in aluminum. Avoid AlTiN and other steel-oriented coatings — aluminum has a chemical affinity for them and welds to the edge. Sharpness beats everything: a keen uncoated tool outperforms a dull coated one every time.
Why does aluminum stick to my end mill?
That is built-up edge (BUE): aluminum pressure-welds to the cutting edge, forming a false edge that ruins finish and dimensions. It happens when surface speed is too low, chip load is too thin (rubbing), the tool is dull, or the alloy is one of the gummy ones — 5052, 1100, and O-temper stock are the worst offenders. The fixes stack: raise SFM past 820, increase feed to a real chip, use a sharp polished-flute tool, and add lubrication (flood, MQL, or mist) so chips leave the cut zone.
Is 6061 or 7075 easier to mill?
6061 is easier on the machine and the budget; 7075 is easier on the chip. 6061-T6 is the forgiving default — moderate cutting forces, available everywhere, anodizes well. Its T651 temper runs gummier than many expect, so keep surface speed up. 7075-T6 is harder and stronger, and its chips actually break cleaner than 6061’s, but it costs more, cuts with higher force, and does not weld. For most parts, 6061 until the drawing’s strength numbers say otherwise. For what the stress-relieved temper actually changes on the machine, see 6061-T6 vs T651.
Can a CNC router mill aluminum?
Yes, within limits — routers mill aluminum successfully for plates, panels, and brackets, but they are RPM-limited and light on rigidity, so they live at the small-tool, light-DOC end of the parameter space. Trochoidal/adaptive toolpaths with 5–15% stepover help a lot. For structural parts, tight tolerances, or any real volume, a machining center with flood coolant is the right tool — that is the work our CNC milling service runs daily.
Related Resources
304 vs 316 Stainless Steel: Which Grade for Machined Parts?
304 vs 316 stainless steel compared for CNC machined parts: composition, corrosion resistance (PREN), machinability,…
How to Outsource CNC Machining to China, Step by Step
How to outsource CNC machining to China, step by step: vet suppliers, compare landed cost, control quality remotely,…
CNC Machining Surface Finish: The Ra Chart, Explained
The CNC machining surface finish chart: Ra values in μm and μin, N1–N12 grades, what each process achieves, what…
GD&T Basics for CNC Machined Parts: The Symbols That Matter
GD&T basics for machined parts: the 14 symbols explained, feature control frames, datums, MMC bonus tolerance, true…
Aluminum Milling, From Prototype to Production
IsoCNC mills 6061, 7075, 2024, 5052, and cast plate in 3- and 5-axis cells, with anodizing and plating in-house. Not sure whether your part needs simultaneous 5-axis or 3+2 would do? The 5-axis vs 3-axis decision guide breaks down which features justify the premium. Send the drawing; an engineer reviews every RFQ, typically within 1–2 business days.