7075 / AlZnMgCu 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 →

7075 aluminium turns at 350-900 m/min (about 1,150-2,950 SFM) with 0.22 mm/rev, mills at 220-550 m/min with 0.13 mm per tooth, drills at 245-675 m/min and taps at 122-405 m/min. It is the aerospace and motorsport alloy: it cuts better and finishes better than 6082, but it distorts from residual stress and punishes any lapse in coolant without mercy. Strategy matters as much as the numbers.

EN AW-7075 · 150 HB · ISO group N

Recommended speeds and feeds

OperationVc (m/min)FeedShop note
Turning350–9000.22 mm/rev350-900 m/min at 0.22 mm/rev with a polished edge; 7075 will take spectacular finishes with a small nose radius and 0.05-0.08 mm/rev, but it needs continuous coolant because the moment the nose heats up it loads with aluminium.
Milling220–5500.13 mm/tooth220-550 m/min with 0.13 mm per tooth. Run light radial engagement and deep axial cuts on a trochoidal path: you spread wear along the whole flute length, keep temperature down and can push the feed without chatter.
Drilling245–6750.22 mm/rev245-675 m/min at 0.22 mm/rev with a polished-flute drill. Program pecks in deep holes: 7075 makes a shorter chip than 6082, but if it packs in the flute it welds just as fast.
Threading122–4050.22 mm/rev122-405 m/min. Form tapping works in 7075 but less well than in 6082 because the material is less ductile; on critical aerospace threads use a carbide cut tap or a thread mill and check the thread with a gauge.

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

With zinc, magnesium and copper, 7075 reaches about 150 HB in T6, well above any other common aluminium alloy. That extra hardness breaks the chip better and gives a mirror finish, but it also raises cutting forces and temperature. It still has aluminium's affinity for tooling: if the edge heats up because coolant is not reaching it, the material welds instantly and the cutter loads up. And above all, 7075 bar and plate carry manufacturing stress that is released as soon as you remove material, bowing parts that came off the machine perfectly flat.

Residual stress: the part that bows on its own

The classic case is a 7075 plate that comes off the machining centre flat and, five minutes later off the fixture, has bowed two tenths. The material carries residual stress from rolling and heat treatment, and hollowing out one face unbalances that state. The cure is strategy, not parameters: rough leaving 0.5 to 1 mm all over, release the part, let it relax, reclamp lightly and finish. On symmetric parts, alternate pockets on both faces. And always clamp with the minimum force needed, because a tight vice hides the distortion until you open it.

Real high speed machining: edge, coolant and evacuation

7075 is the material where high speed machining pays off most obviously: big axial depths, radial engagement of 5 to 15% of diameter, high feeds and trochoidal paths with no sharp direction changes. With that strategy a three-flute carbide cutter with a 45 degree helix runs cool and at constant load. What it will not forgive is a coolant interruption or a trapped chip: the moment one revolution recuts an old chip, aluminium welds to the edge and within two passes the tool is loaded and the part is scored.

Mirror finish and dimensional control

7075 in T6 will give finishes that need no polishing afterwards: with a polished-edge insert, a small nose radius and a fine feed you get comfortably below Ra 0.4. That level of finish does demand two things. First, part temperature: aluminium expands more than twice as much as steel, so a part measured hot shrinks back and lands out of tolerance the other way. Second, the tool: save a fresh edge for the final pass, because the smallest amount of built-up material shows on the surface immediately.

Quick shop tips

  • Rough leaving 0.5-1 mm, release the part, let it relax, then finish: 7075 bows as stress is released.
  • Clamp with the minimum pressure; a tight vice hides the distortion until you open the machine.
  • Trochoidal with light radial engagement and deep axial cuts is the strategy that pays best in this alloy.
  • If coolant drops out for a moment, stop: aluminium welds to the edge before you notice.
  • Measure with the part cold; aluminium expands more than twice as much as steel and will fool you on tight sizes.
  • Save a fresh tool for finishing; any built-up edge shows on the surface immediately.

Frequently Asked Questions (FAQ)

Why does my 7075 part distort after machining?

Residual stress from rolling and heat treatment, released as you remove material. Rough leaving stock, release the part and let it relax, then finish with light clamping. It is not a cutting speed or cutter problem.

Does 7075 machine faster than 6082?

Slightly slower: 350-900 m/min turning against 400-1,000 for 6082, and 220-550 milling against 250-600. In exchange, being harder it gives shorter chips, fewer burrs and a better finish.

What feed per tooth do I use on 7075 with an 8 mm cutter?

Around 0.13 mm per tooth as a catalogue starting point, adjusted for radial engagement: on trochoidal paths with light engagement raise it to compensate for chip thinning, and in full-width slotting drop it about 30%.

Can 7075 be machined dry?

In very open cuts with an air blast you can, but it is not recommended. 7075 generates more heat than 6082 and as soon as temperature rises the aluminium welds to the edge. Normal practice is plenty of coolant or well-aimed MQL.

Which tool works best in 7075: uncoated, DLC or diamond?

Fine-grain carbide with a polished uncoated edge works very well; DLC extends life and cuts adhesion, and PCD is the choice for long runs. What you must never use is a titanium-bearing coating, because aluminium sticks to it.

Similar materials

6082 / AlMgSi1 aluminium: cutting speed and feed rate

Cutting speed and feed for 6082 / AlMgSi1 aluminium: Vc per operation, chip evacuation and why the real limit is almost always your spindle 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.

Ti-6Al-4V (grade 5) titanium: cutting speed and feed rate

Cutting speed and feed for Ti-6Al-4V grade 5 titanium: Vc per operation, high pressure coolant and why you never let the cutting edge dwell in the cut.

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.