420 / 1.4021 martensitic stainless: cutting speed and feed

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 →

Annealed 420 stainless turns and mills at 110-180 m/min (about 360-590 SFM) with 0.2 mm/rev or 0.07 mm per tooth, drills at 77-135 m/min and taps at 39-81 m/min. It is a martensitic stainless around 230 HB, harder than 304 but far less sticky: here the enemy is abrasion, not adhesion. If the part is already hardened, none of these numbers apply.

EN X20Cr13 / 1.4021 · AISI 420 · 230 HB · ISO group M

Recommended speeds and feeds

OperationVc (m/min)FeedShop note
Turning110–1800.2 mm/rev110-180 m/min at 0.2 mm/rev with a wear-resistant coating; flank wear dominates, so watch the width of the wear land and index on a size criterion rather than waiting for the edge to break.
Milling110–1800.07 mm/tooth110-180 m/min with 0.07 mm per tooth. In moulds and cavities, trochoidal paths keep the arc of engagement constant and avoid the temperature spikes that locally harden the surface and then destroy the finishing cutter.
Drilling77–1350.11 mm/rev77-135 m/min at 0.11 mm/rev with plenty of coolant; 420 does not pack the drill up the way 316 does, but the drill margin wears fast through abrasion and holes start coming out undersize without warning.
Threading39–810.11 mm/rev39-81 m/min. Threads in 420 are always cut in the annealed state: once it is hardened to 50 HRC no tap will enter. Use a carbide cut tap with good lubrication and drill for 65% thread engagement.

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

420 carries around 13% chromium and enough carbon to harden, which is why it ends up in cutlery, injection moulds and pump shafts. Annealed at 230 HB, its microstructure holds hard chromium carbides scattered through the matrix that act like tiny abrasive particles against the tool flank. The chip is shorter and better behaved than in the austenitics and it welds far less, but thermal conductivity is still low and heat piles up at the edge. Too much surface temperature can even harden the part locally, which is exactly what this steel is designed to do.

Annealed or hardened: two different materials

420 is supplied annealed between 200 and 240 HB and hardened afterwards to 48-54 HRC depending on the application. The parameters on this page are for the annealed condition. If the part is already hardened you are in hard machining territory: CBN or ceramic tooling, light passes, different speeds. In moulds it is normal to rough soft, harden, then finish with carbide cutters made for hardened steel at very small engagements. Always confirm the condition before loading the program: the gap between 230 HB and 52 HRC is not something the feed override will fix.

Abrasive wear: you can feel the chromium on the flank

Unlike the austenitics, tools in 420 do not die from adhesion but from straight abrasion. The chromium carbides spread through the matrix scrape the insert flank steadily and predictably, which has one advantage: wear is progressive and you can plan it per number of parts. Hard coatings, wear-resistant substrates and a speed in the middle of the range, around 140 m/min, give the most consistent life. Push past 180 m/min and temperature rises, adding plastic deformation of the edge on top of abrasion - and that one does fail suddenly.

Finishing cutlery and mould surfaces

420 is used where surface finish matters: mould cavities, blades, shafts that get polished afterwards. Match nose radius to feed (for Ra 0.8 with a 0.8 mm nose, around 0.07 mm/rev), use a polished-edge insert and take one finishing pass with no spring cuts. Watch the temperature: an overspeed finishing pass can leave a heat-affected surface layer that behaves differently on hardening and shows up as patchy hardness. Continuous coolant, never intermittent, and a fresh edge for the final pass.

Quick shop tips

  • Confirm whether the part is annealed or hardened before programming: two different worlds under the same name.
  • Wear in 420 is abrasive and progressive, so change tools on a part count rather than waiting for a failure.
  • Watch hole diameters: the drill margin wears and holes start coming out undersize.
  • Continuous coolant, never on and off: intermittent flood thermally cracks the edge in milling.
  • Cut every thread in the annealed state; after hardening there is no tap that will go in.
  • Save a fresh insert for the finishing pass in mould cavities; a worn edge leaves a heat-affected surface.

Frequently Asked Questions (FAQ)

Does 420 machine like 304?

No. 420 is martensitic: harder (230 HB), less sticky, and it wears tools by abrasion rather than adhesion. It takes slightly less speed than 304 in turning (110-180 against 120-200) but considerably more in milling, because it does not work harden like the austenitics.

Can I machine already hardened 420 with these parameters?

No. These values are for the annealed condition at around 230 HB. Hardened to 48-54 HRC you need CBN or ceramic tooling and very light passes, with hard turning logic.

What cutting speed do I use on 420 with HSS?

Between 39 and 63 m/min, a third of the carbide range, and only in the annealed condition. HSS suffers badly from chromium carbide abrasion, so expect short tool life and keep the coolant running continuously.

Why does my end mill wear out so fast in 420?

Chromium carbide abrasion, made worse if you are running above 180 m/min. Drop towards 140 m/min, use a hard AlTiN coating and go trochoidal in pockets so arc of engagement and temperature do not spike in the corners.

Can 420 be form tapped?

Annealed and carefully, yes, but it is not very ductile compared with a carbon steel and the thread crest can come out cracked. For threads that carry load, a carbide cut tap or a thread mill is far more reliable.

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.

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.

Hardened steel 50-55 HRC: cutting speed and feed rate

Cutting speed and feed in hardened 50-55 HRC steel: Vc per operation, CBN and ceramic inserts, and the light passes and rigidity that hard turning needs.

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.