Stainless steel processing skills for CNC machined parts

• 1
  Key takeaways
• 2
  Stainless steel processing skills start with grade behavior
• 3
  Tool selection drives stainless steel processing skills
• 4
  Speeds, feeds, and heat control
• 5
  Workholding and machine setup for stainless
• 6
  Deburring, passivation, and finish control
• 7
  Step by step: running a stainless job
• 8
  Stainless grade selection for CNC work

Stainless is a ferrous alloy with at least 10.5% chromium. That chromium oxide layer gives the corrosion resistance, and it also changes how the material cuts. Austenitic grades such as 304 and 316L are the common ones, and they work harden quickly. Once the tool rubs instead of cutting, the surface gets harder than the base metal and the next pass is worse.

Ferritic and martensitic grades behave differently. Grade 430 is softer and gummy in a different way. Grades 420, 431, and 440C respond to heat treatment, so you can cut them in the annealed state and harden later. The trade is distortion during heat treatment, which often means grinding or a finish pass after hardening.

Precipitation hardening grades such as 17-4PH (SUS630) sit in the middle. In the annealed condition they machine close to 304, but the final properties come from aging. If you machine to final size before aging, plan for a small growth in the range of 0.0005 to 0.002 in per inch. That number moves with section thickness, so confirm it with the heat treater.

Free machining 303 is the exception. It contains sulfur, which breaks chips and lowers cutting forces. It is the right pick for shafts, fittings, and parts that do not need to be welded. For welded or highly corrosive parts, use 304 or 316L and accept slower cutting.

• 1
  Work hardening is the first riskIt appears when the edge rubs, when the feed is too light, or when the tool dwells in the cut.
• 2
  Chloride resistance316L has molybdenum for pitting resistance. Choose it for marine and medical parts.
• 3
  Magnetic responseAnnealed 304 is largely non magnetic. Cold work can make it slightly magnetic, which matters for sensor housings.

Carbide grade and coating matter more than brand. Look for a submicron grain carbide with a PVD coating such as TiAlN or AlTiN. The coating resists the built up edge that forms when stainless sticks to the insert. An uncoated insert can work on 303, but on 304 and 316L the edge breaks down faster and the finish suffers.

Geometry should be sharp and positive. A positive rake face lowers cutting force and reduces the tendency to work harden. For turning, that often means a positive insert with a small nose radius, around 0.4 mm for finishing and 0.8 mm for roughing. A large nose radius spreads the cut over more material, which raises radial force on thin walls.

For milling, use variable helix or unequal flute spacing. Stainless vibrates more than aluminum, and the uneven spacing breaks the harmonic that causes chatter. Four flutes is a good starting point for roughing, and a high feed mill can move a lot of metal if the machine has the spindle speed to support it.

Drilling is where most scrap starts. Use a 135° or 140° point with a split point for self centering. Through coolant helps, mainly on deep holes where chip evacuation is the limit. Peck depth of one diameter is a safe start. Deeper pecks raise the risk of work hardening at the bottom of the hole.

• 1
  CoatingsTiAlN and AlTiN handle the heat. Use them for 304, 316L, and 17-4PH.
• 2
  Nose radiusSmall radius for finish and thin walls. Larger radius for heavy roughing on rigid parts.
• 3
  Corner protectionA honed or chamfered edge lasts longer in interrupted cuts.
• 4
  Avoid reground drillsA hand reground point can lose its split and wander on entry.

Surface speed for stainless is lower than for aluminum, and the window is narrower. A common starting range for carbide turning is 120 to 180 m/min (400 to 600 sfm) on 304, and 100 to 150 m/min (330 to 500 sfm) on 316L. Run fast and the edge glows, run slow and the material work hardens. The feed per tooth needs to stay high enough to cut under the hardened skin.

On a 12 mm carbide end mill in 304, a starting feed of 0.05 to 0.08 mm per tooth at 1,500 to 2,000 rpm is reasonable. That is a starting point, not a rule. Listen to the cut and watch the chip color. Straw colored chips mean the heat is going into the chip, which is what you want. Blue or dark chips mean the edge is too hot.

Coolant should be flood and aimed at the cut, not at the part in general. High pressure through tool coolant, around 70 bar, helps with deep holes and pockets because it clears chips. On finishing passes, keep the tool moving. A dwell of even half a second in 304 can leave a hard spot that the next pass will not cut cleanly.

Roughing should remove the work hardened layer from a previous operation. If a part was saw cut or waterjet cut, the top 0.2 to 0.5 mm is often harder than the core. Take a first pass deep enough to get under it, rather than skimming the surface and rubbing.

• 1
  Start conservativeBegin at the low end of the speed range and raise feed before raising speed.
• 2
  Chip colorStraw is good. Blue or gray means the edge is running too hot.
• 3
  No dwellKeep the tool moving. A pause in the cut hardens the surface.
• 4
  Depth of cutRoughing depths of 0.5 to 2 mm per pass are common on rigid setups.

Stainless pushes back. Cutting forces are higher than aluminum or mild steel, and thin walls deflect. Support the part as close to the cut as the geometry allows. On a 5-axis setup, a low profile vise or a custom fixture with a machined nest gives better support than a standard vise on tall jaws.

Thermal growth is real on long parts. A shaft 300 mm long can grow a few hundredths of a millimeter as it warms during roughing. Rough, let the part cool, then finish. That sequence costs one extra setup but saves rework on tight bores and bearing fits.

On a lathe, a Ø400 mm rotary table or a mill turn center can cut a part in one setup, which removes the re-chucking error that shows up as concentricity problems. For parts up to 4,000 mm, plan the setup so the finishing passes happen after the part has reached a stable temperature.

Cleanliness between operations matters. Stainless chips work their way into fixtures and leave marks on the next part. Blow out the nest, wipe the jaws, and check the locating face before loading the next blank. Embedded chips are a common source of a 0.02 mm size error.

• 1
  Rough then finishLet long parts cool between passes to control thermal growth.
• 2
  One setup when possibleFewer chuckings means better concentricity and less handling damage.
• 3
  Clean locating facesA chip under the part shows up as a size error or a witness mark.

Machined stainless usually has a burr on the exit edge. A sharp burr is a handling hazard and a fatigue crack starter. Hand deburr with a fine file or a ceramic stone, then blend the edge. For cross holes and small features, a controlled brush or a thermal deburr process gives a more consistent edge than hand work.

Passivation removes free iron from the surface and lets the chromium oxide layer rebuild. It is not a coating. For 304 and 316L, a typical passivation bath follows ASTM A967, with a nitric or citric acid step and a rinse. Parts that will see salt spray or medical cleaning should be passivated, especially after grinding or bead blasting.

Surface finish targets drive the process. As machined surfaces run Ra 1.6 to 3.2 μm. A careful finishing pass with a sharp insert and a light feed gets to Ra 0.8 to 1.6 μm. Below Ra 0.8 μm, plan on a secondary operation such as polishing or lapping, because turning alone gets expensive fast.

Bead blasting, brushing, and polishing change the look and the finish. Bead blasting gives a uniform matte surface and hides small tool marks, but it can leave a roughness that needs passivation after. Keep the blasting media dedicated to stainless. Carbon steel media leaves iron particles that rust on the part.

• 1
  Deburr before passivationA burr traps contamination and creates a sharp edge.
• 2
  Dedicated mediaDo not bead blast stainless with media used on carbon steel.
• 3
  Finish targetsRa 0.8–1.6 μm from turning. Ra 0.2–0.8 μm needs polishing or lapping.