Home » Milling » Why Stainless Steel Work Hardens (and How to Stop It From Killing Your End Mills)

Why Stainless Steel Work Hardens (and How to Stop It From Killing Your End Mills)

Filed under ,
work-hardening-stainless-steel

The first pass in 304 cut clean. The second pass squealed, the wall came back shiny, and the end mill had a notch at the depth of cut line. The program didn’t change. The material did.

Category: Milling  •  Reading Time: ~8 minutes  •  Audience: Intermediate to Advanced Machinists


QUICK ANSWER

Austenitic stainless like 304 and 316 gets harder as it is deformed, so each pass can leave a harder skin for the next one. Keep the tool cutting instead of rubbing: hold a real chip load, keep the feed constant, climb mill, take fewer and deeper passes, correct your feed for chip thinning on light radial cuts, keep edges sharp and keep coolant on the cut. Then run a tool built for stainless.

What Work Hardening Actually Is

Work hardening is the metal getting harder because it was plastically deformed. Seco Tools puts the mechanism plainly: austenitic stainless work hardens during deformation. Harvey Performance compares the result to heat treating, with the largest change in hardness right at the surface.

Heat is the other half of the problem, mostly for the tool. Seco notes that austenitic alloys combine low thermal conductivity with high resistance to deformation, so the heat of the cut tends to stay in the cutting zone instead of leaving with the chip. Harvey adds that when speeds and feeds are off, the tool does more rubbing and less cutting, and more of that heat goes into the part.

The part that catches people is that it compounds. A 2020 study in the Journal of Manufacturing Science and Engineering, run as drilling and planing tests on a cast heat resistant austenitic grade, traced the rise in hardness to plastic strain and found that each cut hardens the layer beneath it, so the tool is never cutting the material in its original state. The test was not milling 304, but the lesson carries: your second pass is cutting what your first pass left behind.

Left alone, it gets expensive. Harvey warns that a workpiece can harden until it rivals the hardness of the cutting tool, and that if the tool keeps getting fed the same way, heavy wear and eventual breakage follow.

Diagram of a work hardened layer left under a machined stainless surface, with the next pass cutting through it.

Which Stainless Grades Do It Worst

Stainless is not one material. Harvey’s stainless machining guide sorts it into five families, and they do not behave the same in the cut.

Family Common grades What to expect in the cut
Austenitic 304, 316 The family this post is about. Work hardens during deformation and holds heat in the cutting zone (Seco).
Ferritic 430, 446 Seco rates ferritic alloys as not much harder to machine than plain steels.
Martensitic 416, 420, 440 Hardened by heat treatment. Seco groups them with ferritic as not much harder to machine than plain steels. Read that as annealed stock; hardened 420 or 440C is a different job.
Precipitation hardened (PH) 17-4 PH, 15-5 PH The strongest family and heat treatable (Harvey). Behavior depends on the condition, so pull parameters for the condition on your cert.
Duplex 2304, 2507 Work hardening is less significant than in austenitic grades, but it is still there, and higher strength means higher cutting forces and lower speeds (AMTIL, writing on Sandvik Coromant’s stainless turning grades).

Not every 300 series grade is equally stubborn. One Haas Tooling speed and feed sheet, for example, groups 303 and 416 as free machining stainless and lists 304 and 316 as difficult.

Five Ways Shops Cause It

1. Feeding Too Light

Backing off the feed feels safe in stainless. It tends to do the opposite. A light feed lets the edge rub instead of shear, and Harvey ties rubbing directly to heat going into the workpiece. The research side agrees. A 2012 review of austenitic stainless machining by Kaladhar and co-authors, as cited in a 2023 International Journal of Metalcasting paper, concluded that low feed rates should be avoided to limit work hardening.

2. Light Radial Cuts With No Chip Thinning Correction

This one hides in good looking toolpaths. Helical’s Machining Guidebook explains that when the radial depth of cut drops under 50% of the cutter diameter, the chip being formed is much thinner than the programmed feed per tooth, which leads to tool rubbing and early wear. A finishing pass or a high efficiency toolpath can be rubbing while the feed on the screen looks right. The fix is to raise the feed to make up for the thinning. The SFM chart guide covers the base numbers.

3. Stopping, Dwelling and Uneven Feed

Harvey recommends a constant feed rate that keeps the tool moving so heat can’t build in one spot, and Kennametal’s guidance is just as blunt about parking a tool against the work. In practice that means watching for the places a program slows down by itself: sharp inside corners, feed holds, a dwell at the bottom of a plunge. A tool sitting still against stainless is doing the one thing you are trying to avoid.

4. Too Many Shallow Passes

Every pass is another chance to harden the surface under it. Seco’s advice is to use the largest depths of cut and feeds that are practical, because fewer passes lowers the risk. An AMTIL article on Sandvik Coromant’s stainless turning grades gives the tool side of the same idea: with austenitic stainless, sharp edges that can cut under the work hardened layer work well. A skim pass that barely touches the wall is rubbing the hardest material on the part, so leave enough stock that the edge shears instead of rubs.

The same goes for spring passes. With almost nothing left to cut, the edge mostly skates, which is why Kennametal recommends skipping them when milling materials that work harden.

5. Running a Dull Tool One Part Too Long

Seco notes that a sharper edge cuts the material instead of deforming it, which makes less heat. A worn edge does the reverse. Kennametal lists tool maintenance among the ways to reduce work hardening. If you are not sure what the wear on your tool is telling you, see How to Diagnose Costly End Mill Wear Before It Scraps Parts.

Direction matters too. Harvey points out that conventional milling starts each chip at zero thickness and builds, which puts heat into the workpiece, while climb milling starts at full chip thickness and sends more of the heat out with the chip.


WARNING: THE NEXT TOOL PAYS FOR IT

A hardened surface does not only hurt the tool that made it. Kennametal points out that a run of broken taps can trace back to the hole, hardened by the drill that made it, with nothing wrong with the taps. If taps are snapping in stainless, look at the drill before you blame the tap: its condition, its feed and whether it dwelled at depth. Related reading: Why Taps Break at Reversal and Why the Drill Chart on Your Shop Wall Is Lying to You.


Reading the Evidence

What you see What it can point to First move
Wall or floor comes back with a glassy, polished look Kennametal gives a glazed finish as the visual sign of a work hardened surface Check feed per tooth and chip thinning before touching speed
Notch in the edge at the depth of cut line Seco ties notch wear to work hardening Vary the depth of cut from pass to pass to spread the wear (Seco)
Material stuck to the cutting edge Adhesion, or built-up edge. Seco notes austenitic steel tends to stick to the tool Seco points to lubricious coatings and higher cutting speed. Cutting Tool Engineering warns against very low speeds for the same reason
Second pass sounds and cuts worse than the first The pass is working in the skin the first pass left Fewer, deeper passes, and a sharp tool
Taps or reamers failing in drilled holes Possibly a work hardened hole (Kennametal) Check the drill’s condition and feed, and remove any dwell

stanlessStell-milled-finishes

Starting Parameters

These are Harvey Performance’s general guidelines for stainless, and they are starting points only. The grade, the condition, the tool and the setup all move the numbers.

Parameter Harvey Performance general guideline
Surface speed 100 to 350 SFM
Chip load, 1/8″ end mill .0005″ per tooth
Chip load, 1″ end mill .006″ per tooth

For a Helical end mill, run the exact tool number, material grade and machine through Helical’s Machining Advisor Pro instead of working from a general range.

On coolant, Harvey notes that flood coolant can help hold temperature in stainless and high temp alloys, that its lubricity helps flush chips so they are not recut, and that high pressure helps evacuation but can break miniature tools. Seco recommends an emulsion with at least 8% to 9% oil content for austenitic stainless, against the 3% to 4% it calls typical. Check that figure against your coolant maker’s sheet, and see Is Your Coolant Killing Your Tools? for the upkeep side.

Pick a Tool Built for Stainless

A general purpose end mill will cut stainless. A stainless tool gives you more room before the trouble starts. Harvey’s guide matches flute count to the toolpath like this:

Toolpath Harvey’s recommendation Example on the store
Traditional roughing 4 or 5 flute. The 5 flute allows higher feed rates Helical 88342, 1/2″ 5 flute variable pitch, 1″ LOC, Tplus
Slotting 4 flute, for chip room. Chipbreaker geometry helps Helical end mills for stainless
Finishing 5 or more flutes, helix angle over 40°. Aggressive finishing can run 7 to 14 flutes Helical 88691, 3/8″ 7 flute variable pitch, 1-1/4″ LOC, Tplus
High efficiency milling (HEM) 5 or 7 flute chipbreaker roughers, or standard 5 to 7 flute variable pitch end mills Helical 88344, 1/2″ 5 flute variable pitch, 1-5/8″ LOC, Tplus

Three features are worth checking on the listing:

  • Coating. Helical coats its stainless and high temp line in Tplus, which it describes as offering heat resistance and high hardness for reduced abrasion. Harvey notes that coatings for ferrous materials cut friction, which moves heat into the chip. More in Cutting Tool Coatings Explained.
  • Variable pitch. Helical builds variable pitch into this line to reduce vibration. The why is in Killing Chatter.
  • Flute count for the toolpath. The table above is the short version.

[PLACEHOLDER: IMAGE 4, PRODUCT PHOTO: Helical end mills for stainless, 4, 5 and 6 or 7 flute side by side, end view if possible. Alt text: “Helical Solutions Tplus coated end mills for stainless steel in 4, 5 and 6 flute.”]

What Our Reps See

[PLACEHOLDER: JAY: add field input from inside sales. For example, the stainless call you get most (which grade, which operation), what the customer was running, and what they switched to.]

A Checklist Before You Run

  1. Know the grade and condition. 303 and 304 are not the same job, and neither is 17-4 in two different conditions.
  2. Set chip load first, then speed. Start from the tool maker’s numbers for that exact tool.
  3. Correct for chip thinning any time radial engagement is under half the diameter.
  4. Climb mill, and look through the program for dwells and slow corners.
  5. Plan fewer, deeper passes. Leave the finish pass enough stock that the edge shears instead of rubs.
  6. Start with a sharp tool and change it on a schedule, not on a failure.
  7. Coolant on the cut, at a concentration your coolant maker recommends for stainless.

[PLACEHOLDER: IMAGE 5, OPTIONAL: printable version of this checklist as a shop card. Alt text: “Stainless steel work hardening checklist for CNC milling.”]

Stainless Work Hardening FAQ

What causes stainless steel to work harden?

Plastic deformation. Austenitic stainless hardens as it is deformed, and heat that stays in the cutting zone adds to it. Rubbing, light feeds, dull edges and repeated shallow passes all make it worse.

Does 304 or 316 work harden more?

Both are austenitic, and that is the family known for it. A Haas Tooling speed and feed sheet puts both in the same difficult group, apart from free machining grades like 303.

Can you machine through a work hardened surface?

Often, yes. The advice in AMTIL’s piece on Sandvik Coromant’s stainless grades is a sharp edge that cuts under the hardened layer. That means a fresh tool and a real depth of cut, not another light pass. If the layer is deep, it can take more than one pass to clear.

Should I slow down in stainless?

Slowing surface speed can help with heat, but dropping the feed is where shops tend to get hurt. Keep a real chip load. For stainless in general, Harvey Performance gives 100 to 350 SFM as a starting range.

Why do my taps keep breaking in stainless?

The taps may be fine. Kennametal points to the hole: if the drill hardened it, the tap is cutting a harder material than you planned for. Check the drill’s condition and feed, and take out any dwell at depth.

Chapman Can Help

If stainless is eating tools on one job, do three things before the next run: read the chip load off the program instead of the setup sheet, check the radial engagement on every pass under half the diameter, and put in a fresh end mill made for stainless. Start with those three before you touch the speed.

If it still fights you, call with the grade, the tool and the toolpath and we will work through it with you: 410.686.6860. Stocked items ordered by 4:30 PM ET ship the same day, and non-stock items ship factory direct.

Order online or talk to the team

The store is open around the clock. The sales desk is open Monday through Friday, 7:30am to 5:00pm EST.

Call (410) 686-6860 or write sales@wcchapman.com.