316 / 1.4401 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 →

316 stainless turns at 100-180 m/min (about 330-590 SFM) with 0.2 mm/rev, mills at 60-100 m/min with 0.07 mm per tooth, drills at 70-135 m/min and taps at 35-81 m/min. Those numbers sit below 304 for a reason: molybdenum makes it tougher, stickier and quicker to work harden. If you are coming off a 304 job, pull the parameters back before you press cycle start.

EN X5CrNiMo17-12-2 / 1.4401 · AISI 316 · 215 HB · ISO group M

Recommended speeds and feeds

Operation	Vc (m/min)	Feed	Shop note
Turning	100–180	0.2 mm/rev	100-180 m/min at 0.2 mm/rev, a sharp-edged PVD insert and a depth of cut above 0.5 mm; on fine finishing passes the hardened layer is thicker than the cut, and the nose ends up rubbing itself round.
Milling	60–100	0.07 mm/tooth	60-100 m/min with 0.07 mm per tooth, climb milling, entering on an arc or a ramp. Avoid close-pitch cutters in pockets: 316 does not clear chips well, and whatever stays between tooth and wall gets recut and chips the edge.
Drilling	70–135	0.1 mm/rev	70-135 m/min at 0.1 mm/rev, carbide drill with through-coolant and no pauses in the feed. Past three diameters deep, 316 attacks the drill margin through adhesion; back the speed off 20% and raise coolant pressure.
Threading	35–81	0.1 mm/rev	35-81 m/min. This is the material that breaks the most taps: drill for 60% thread engagement, use a coated tap with good lubrication, and if the hole is blind and the part is expensive, thread mill it - no argument.

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

316 is a molybdenum-bearing austenitic at 215 HB, and everything that happens in 304 happens here amplified. It work hardens more readily, the chip is tougher and springier, and adhesion on the edge is strong enough to weld chip material onto the rake face on the very first pass. Thermal conductivity is lower still, so essentially all the heat generated stays at the tool tip. Deep holes and tapping are where the difference against 304 really shows up.

Why 316 costs more than 304

The molybdenum that gives 316 its pitting resistance also gives it more hot toughness and more affinity for the tool material. In practice that means a speed window 15 to 20% below 304 across every operation: 100-180 m/min against 120-200 turning, and 60-100 against 70-120 milling. It also wants a slightly lower feed, 0.2 mm/rev, not because the material is hard but because cutting forces are high and the nose takes a beating. Reuse a 304 program untouched and you will see the difference in tool life.

Coolant pressure: the variable that changes the most

In 316 lubrication is not a comfort item. A properly mixed coolant with good EP additives, delivered under pressure to the cutting zone, does more for tool life than any speed adjustment. Pressure breaks the chip, stops it welding to the edge and carries away heat the material refuses to conduct. In deep drilling and parting off, where the chip has nowhere easy to go, through-coolant is literally the difference between a finished hole and a snapped drill. Check the emulsion concentration too: below 8% and 316 starts sticking.

Part distortion and thin walls

316 shows up in tube, tanks, flanges and food and chemical industry parts, very often with thin walls. Two problems meet there: cutting forces are high and the part is not rigid, so it deflects away from the tool, chatters, and ends up with a hardened surface that never got cut. The fix is to reduce radial force - a lead angle close to 90 degrees, a small nose radius - clamp with soft jaws that spread the pressure, and finish in one clean pass. Taking a second cut on a thin 316 wall never improves the size, it just hardens it.

Quick shop tips

Coming off a 304 job, take 15-20% off the speed before you run the first 316 program.
Check emulsion concentration: below 8%, 316 welds to the edge on the first pass.
Finish with a depth of cut above 0.5 mm; below that you are rubbing the hardened layer.
Index the insert as soon as you see welded material on the rake face, even if the edge still looks whole.
For tapping, drill for 60% thread engagement; no fastener will ever miss the 15 points you gave up.
Use a variable-pitch cutter and arc entry: 316 chatters easily, and chatter hardens it.

Frequently Asked Questions (FAQ)

What is the difference between machining 304 and 316?

316 contains molybdenum, is slightly harder (215 HB against 200) and noticeably stickier and quicker to work harden. That translates into a 15-20% lower speed range in every operation and a much bigger demand for coolant pressure.

Why do my drills break in 316?

Usually one of two things: stopping the feed inside the hole, which hardens the bottom, or letting chips pack in the flute. Use a carbide drill with through-coolant, continuous feed at 0.1 mm/rev, and reduce speed past three diameters of depth.

What cutting speed do I use on 316 with HSS?

Between 35 and 60 m/min, a third of the carbide range, and always with plenty of lubrication. HSS only works in 316 with a perfectly sharp edge; the moment it rounds off it starts rubbing and hardening the material instead of cutting it.

Can I use steel-grade inserts on 316 stainless?

They work badly. Steel (ISO P) geometries are blunter with tight chipbreakers, and 316 needs a sharp edge, a big rake angle and an open breaker. Use ISO M geometries with a PVD coating.

What is the minimum sensible feed in 316?

Turning, do not go below 0.12-0.15 mm/rev; milling, do not go below 0.05 mm per tooth. Under those values chip thickness is smaller than the edge radius, and the tool stops cutting and starts burnishing and hardening the material.

Similar materials

304 / 1.4301 stainless steel: cutting speed and feed rate

Cutting speed and feed for 304 / 1.4301 stainless by operation, plus the tricks that stop the surface work hardening and the chip welding to the 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.

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.