6082 / AlMgSi1 aluminium: cutting speed and feed rate

Optimize your machining processes with our online cutting parameters calculator. Select the operation type (turning, milling, drilling or threading) and instantly get the critical calculations for your shop: cutting speed (Vc), revolutions per minute (RPM), feed per revolution or per tooth, machining time and the theoretical roughness (Ra / Rz) based on the insert nose radius. To fine-tune those values live at the machine, use the interactive machining calculator.

Cutting calculator

Step 1

Which operation are you machining?

Do you want to adjust these values live?

Here you get the recommendation (Vc, feed, roughness, threading). In the interactive machining calculator you can move Vc, diameter, RPM and feed with linked scales, locks and time/power estimation.

Open interactive calculator →

6082 aluminium turns at 400-1,000 m/min (roughly 1,300-3,300 SFM) with 0.25 mm/rev, mills at 250-600 m/min with 0.15 mm per tooth, drills at 280-750 m/min and taps at 140-450 m/min. With numbers like that the material is almost never the limit: your spindle rpm is, along with how fast you can get the chips out of the cut. In 6082 the program is dictated by evacuation, not by Vc.

EN AW-6082 · AlMgSi1 · 95 HB · ISO group N

Recommended speeds and feeds

Operation	Vc (m/min)	Feed	Shop note
Turning	400–1000	0.25 mm/rev	400-1,000 m/min at 0.25 mm/rev with a polished-edge insert, uncoated or PCD for long runs; no steel geometries, whose blunt edge does nothing but load up with aluminium.
Milling	250–600	0.15 mm/tooth	250-600 m/min at 0.15 mm per tooth with a 2 or 3 flute cutter, high helix and a big chip gullet: a 4 flute cutter has nowhere to put the chips you are making. A 10 mm cutter at 500 m/min needs 16,000 rpm, so the spindle is usually the real ceiling.
Drilling	280–750	0.25 mm/rev	280-750 m/min at 0.25 mm/rev with a polished-flute drill and a 130-140 degree point. Through-coolant, or at least a jet that pushes the chip out; an aluminium chip left in the flute welds and snaps the drill.
Threading	140–450	0.25 mm/rev	140-450 m/min. 6082 is the form tapping material par excellence: the thread comes out smooth and stronger, there is no chip to clear, and M4 and M5 stop breaking taps. Always use a lubricant made for aluminium.

Starting values for coated carbide in medium cutting. Fine-tune them in the calculator for your tool, type of pass and safety margin.

How it behaves when cutting

6082 is an aluminium-magnesium-silicon alloy at about 95 HB, soft, very ductile and with excellent thermal conductivity that carries nearly all the heat away. That is why it takes enormous surface speeds without cooking the edge. Its weakness is affinity: aluminium welds readily to the tool and forms built-up edge the moment the edge is less than sharp or lubrication runs short. Temper matters a lot: in T6 it cuts clean and the chip breaks reasonably well, while in O or T4 the material is gummy, leaves long burrs and the chip tangles.

Chips rule: why aluminium needs room

At 500 m/min and 0.15 mm per tooth, a cutter removes a chip volume that looks nothing like steel. If that chip does not leave the slot it gets recut, welds to the cutter and breaks the edge in seconds. That is why aluminium cutters have two or three flutes with very open gullets and a 40 to 45 degree helix, and why compressed air or pressurised coolant is not a luxury. In deep pockets and slots, evacuation matters more than any cutting parameter: when in doubt, cut radial engagement before you cut speed.

Built-up edge and coatings that do not belong here

Aluminium has a chemical affinity for titanium, so a TiN or TiCN coating - excellent in steel - is about the worst thing you can put in 6082: the aluminium welds to the coating and grows a built-up edge that ruins the finish and eventually breaks the tool. What works is fine-grain uncoated carbide with a polished edge, carbon-based coatings such as DLC, or PCD for long runs. Add continuous lubrication to that: 6082 will accept MQL or air mist, but it will not tolerate running fully dry in slotting or drilling.

T6, T4 or annealed: not every 6082 cuts alike

6082 in T6, solution treated and aged, is the one that gives a good finish and manageable chips, and it is what you normally get in machined bar and plate. In O (annealed) or T4 the material is markedly more ductile and sticky: chips come off in endless strings, big burrs form on every edge, and the finish suffers. If you are stuck with soft stock, raise the feed per tooth to thicken the chip, use the sharpest edge you can get and budget time for deburring. Expecting T6 finish from T4 stock only leads to shop arguments that go nowhere.

Quick shop tips

Do not use titanium-bearing coatings (TiN, TiCN) in aluminium: the material welds to them and builds up on the edge.
Use a 2 or 3 flute cutter with a high helix; with 4 flutes the chip has nowhere to go and gets recut.
Work out the rpm before you fix the Vc: 500 m/min with a 10 mm cutter is 16,000 rpm, which many spindles cannot reach.
Form tap whenever the thread allows it; in 6082 it gives a stronger thread with no chip to jam the hole.
Air blast or coolant aimed into the slot: in aluminium, evacuation beats surface speed.
If the stock is T4 or annealed, raise the feed per tooth and expect burrs; it is not the cutter's fault.

Frequently Asked Questions (FAQ)

How many rpm is 600 m/min in 6082 aluminium?

It depends on diameter: about 19,100 rpm with a 10 mm cutter and about 9,500 rpm with a 20 mm cutter. That is why in aluminium the practical ceiling is usually the spindle rather than the material; if you cannot reach those rpm, use the largest diameter the part allows.

What cutting speed do I use on 6082 with an HSS cutter?

Between 140 and 350 m/min, roughly a third of the carbide range. HSS cuts aluminium well with a polished, sharp edge, but it loads up quickly without lubrication and gets nowhere near the material's potential.

Why is aluminium sticking to my end mill?

Affinity plus a lack of lubrication, made worse by a dull edge or the wrong coating. Use polished uncoated carbide or DLC, keep the feed per tooth high so the chip comes off thick, and make sure there is a continuous air or coolant stream in the slot.

Can I machine 6082 dry?

In open face milling with good evacuation, yes, with compressed air. In slotting, deep pockets and drilling, no: the chip stays in, welds and breaks the tool. There you need coolant or MQL.

What is the difference between machining 6082 and 7075?

7075 is harder (150 HB against 95), gives shorter chips and a better finish, but wants slightly less speed (350-900 turning against 400-1,000) and carries residual stress that distorts the part after roughing. 6082 is softer, stickier and far more prone to burrs.

Similar materials

7075 / AlZnMgCu aluminium: cutting speed and feed rate

Cutting speed and feed for 7075 aluminium: Vc per operation, keeping residual stress from bowing the part and an edge that will not load up at high rpm.

CuZn39Pb3 brass: cutting speed and feed rate

Cutting speed and feed for CuZn39Pb3 / CW614N brass, the drill grind that stops it self-feeding and grabbing, and how lead-free brass behaves instead.

S235 / St37 mild steel: cutting speed and feed rate

Cutting speed and feed for S235 / St37 / 1018 mild steel in turning, milling, drilling and tapping, with real Vc ranges and how to beat built-up edge.

Related tools

RPM, feeds and machining time calculator

Calculate cutting speed, RPM, feeds and pass time for milling, turning and drilling. Adjust values with linked scales and look up starting values by material.

Calculate cycle time

Estimate CNC turning and milling cycle time from G-code. Calculate parts per hour with a breakdown of cutting, rapids, canned cycles and tool changes.

Machining quote

Instant machining quote: material, machine time, setup per batch, secondary operations and margin. Free, no sign-up.