304 / 1.4301 stainless steel: 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 →

304 stainless turns at 120-200 m/min (roughly 390-660 SFM) with 0.22 mm/rev, mills slower at 70-120 m/min with 0.08 mm per tooth, drills at 84-150 m/min and taps at 42-90 m/min. The gap between turning and milling is not a typo in the table: in milling, every entry and exit multiplies both adhesion and work hardening. In 304, constant feed matters more than speed.

EN X5CrNi18-10 / 1.4301 · AISI 304 · 200 HB · ISO group M

Recommended speeds and feeds

OperationVc (m/min)FeedShop note
Turning120–2000.22 mm/rev120-200 m/min at 0.22 mm/rev and, above all, never stop the feed: every second the insert spins without advancing leaves a hardened band that will eat the edge on the next pass. Use a positive geometry with a sharp edge and a PVD coating.
Milling70–1200.08 mm/toothDrop to 70-120 m/min with 0.08 mm per tooth and climb mill; conventional milling starts each tooth at zero chip thickness, which means rubbing, and in 304 rubbing means hardening the surface before you cut it.
Drilling84–1500.12 mm/rev84-150 m/min at 0.12 mm/rev, through-coolant and continuous feed to the bottom. Stopping the drill inside the hole, even for a badly planned peck, is the number one cause of broken drills in 304.
Threading42–900.12 mm/rev42-90 m/min. Use coated spiral-flute taps to lift the chip up and out, and drill for 60-65% thread engagement: tapping torque in 304 is high and the thread still holds far more than the fastener needs.

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

304 is an austenitic stainless at 200 HB that work hardens as you cut it: the act of cutting leaves a hardened layer underneath, sometimes past 300 HB, so the next pass meets a different material from the one on the mill certificate. Thermal conductivity is low, so heat stays in the edge instead of leaving with the chip. The chip is long, tough and very keen to weld itself to the tool. And because the edge always works on the same depth line, you get the notch wear that stainless is famous for, right at the depth of cut.

Work hardening: the trap in 304

Austenite transforms partly as it deforms and gains hardness in exactly the layer you just cut. That is why a light finishing pass over an already hardened surface cuts worse than a deep roughing pass, and why spring passes destroy edges. The practical rule is simple: fewer, deeper passes, with the depth of cut always greater than the hardened layer left by the previous pass, on the order of two or three tenths of a millimetre. Never take a second cut in the same place to chase a tenth, and never let the tool dwell in contact without feeding.

Adhesion and built-up edge: the finish that never arrives

304 sticks to tooling with enthusiasm. The chip welds onto the rake face, grows, then tears coating away as it leaves, putting visible smears and irregular marks on the part. The answer is the sharpest possible edge, a very positive geometry, a thin PVD coating such as TiAlN, and coolant in volume - ideally under pressure and aimed straight at the cutting zone. A lazy stream that only wets the part is useless: the fluid has to get between chip and edge and break that weld before it forms.

Depth of cut notching and long chips

Wear in 304 is not uniform: a notch opens at the exact point where the edge meets the outside surface of the part, fed by hardened material and by scale on the bar. Beat it by varying the depth of cut between successive passes so the notch never forms twice on the same line, and by using a smaller lead angle that spreads the load. The chip, meanwhile, comes off long and springy: choose a chipbreaker made for stainless, with an open geometry, and do not drop below 0.15 mm/rev.

Quick shop tips

  • Never stop the feed with the tool in contact: the hardened band it leaves wrecks the edge on the next pass.
  • Fewer, deeper passes: if the cut does not get under the hardened layer, the tool rubs instead of cutting.
  • Vary the depth of cut between passes so the notch does not always form on the same line.
  • Coolant under pressure and well aimed; in 304 a stream that only wets the part is close to running dry.
  • In milling always climb cut, and switch to a variable-pitch cutter the moment chatter appears.
  • Index the insert when wear reaches the notch even if the flank still looks fine; that notch is what breaks the edge without warning.

Frequently Asked Questions (FAQ)

Why does 304 harden while I am machining it?

Because it is austenitic and work hardens: the zone deformed by the edge gains hardness and the next pass meets harder material. Avoid it by cutting underneath that layer with deeper passes, a constant feed and no spring passes.

What cutting speed do I use on 304 with an HSS drill?

Around 30-50 m/min, roughly a third of the carbide range of 84-150 m/min, with generous coolant and continuous feed. With an 8 mm HSS drill that is about 1,200-2,000 rpm, and you must not let the drill dwell in the hole.

Why is milling 304 slower than turning it?

Because in milling every tooth enters and exits, each entry hits an already hardened surface, and adhesion builds up on the edge. That is why the milling window drops to 70-120 m/min against 120-200 m/min for turning.

Which coating is best for 304 stainless?

A thin PVD, TiAlN or AlCrN, over a positive geometry with a sharp edge. Thick CVD coatings round the edge too much, and in 304 a dull edge means rubbing, hardening and sticking.

Can I machine 304 dry?

Not advisable. Low thermal conductivity concentrates heat in the edge and adhesion goes through the roof without lubrication. If you have no high-pressure coolant, at least use high volume well aimed; in milling, compressed air beats intermittent flood that thermally cracks the edge.

Similar materials

316 / 1.4401 stainless steel: cutting speed and feed rate

Speeds and feeds for 316 / 1.4401 stainless: Vc and feed per operation, why it sticks worse than 304 and how to keep notch wear off the cutting edge.

420 / 1.4021 martensitic stainless: cutting speed and feed

Cutting speed and feed for annealed 420 / 1.4021 martensitic stainless, the abrasive wear its chromium causes and what changes once the part is hardened.

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.