CNC stainless steel cutting: key parameters
Stainless steel work hardens faster and pulls more heat into the edge than carbon steel. This page explains which parameters actually control that, how they interact, and where the practical limits sit for 303, 304, 316L, 17-4PH and 440C. Written for engineers and buyers who have to judge a process window, not just read a feed chart.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
Why stainless steel punishes the wrong cutting data
Carbon steel cuts the way most people expect: the chip carries heat away, the edge stays cool, and a light pass is usually a safe pass. Austenitic stainless does the opposite. It has low thermal conductivity, around one third that of plain carbon steel, so heat that cannot leave with the chip builds up in the cutting zone and travels into the tool.
The second problem is work hardening. When the edge rubs instead of cutting, the surface deforms, its hardness climbs, and the next tooth meets a harder layer than the one before. This is why a timid depth of cut on 304 is often worse than an aggressive one. Feed per tooth has to stay above the hardening threshold, roughly 0.05 mm per tooth for most solid carbide tools in the Ø8–Ø16 mm range.
Third, stainless is gummy. It tends to smear and built-up edge forms on the rake face at moderate speeds, then breaks off and takes a piece of the coating with it. The result is inconsistent surface finish and unpredictable tool life, which is harder to manage than simple flank wear.
These three effects are coupled, so you cannot fix stainless cutting with one setting. Speed, feed, depth of cut, tool geometry and cooling have to be chosen together.
Cutting speed and feed rate in CNC stainless steel cutting
Cutting speed sets the temperature. Too high and the edge softens, diffuses and wears on the flank; too low and the material work hardens ahead of the edge. For coated carbide in 304, the practical window is roughly 120–180 SFM (37–55 m/min) for roughing and 200–260 SFM (60–80 m/min) for finishing. Free-machining 303 tolerates more, around 250–350 SFM.
Feed rate sets whether the edge cuts or rubs. It is expressed as feed per tooth, and the number matters more than the inches-per-minute figure on the screen. Under about 0.05 mm per tooth, the tool pushes the material instead of shearing it, and hardness rises with every pass. Above roughly 0.15 mm per tooth on a small cutter, chip thinning stops helping and the edge starts chipping.
One trap is slowing the feed to improve finish. On stainless that raises tool pressure, increases work hardening and usually makes the finish worse. If the finish is poor, the first thing to check is whether the insert or end mill is still sharp, not whether the feed is too fast.
Speed and feed should be moved together. Raising speed without raising feed just adds heat to a rubbing edge, and raising feed without enough speed loads the tool mechanically without helping chip evacuation.
Depth of cut and radial engagement
Axial depth of cut controls how much of the flute is in the material and how well heat can escape through the tool body. Radial engagement, sometimes called stepover, controls how much of the cutter diameter is loaded at one time. The two trade off against each other.
A conservative stainless strategy uses shallow axial depth with a high radial stepover, typically 50–70 percent of the diameter. It is stable and forgiving, but the cutting edge spends more time in the hardened layer. A high-feed strategy does the opposite: deep axial passes of one to two times the diameter with 5–10 percent radial engagement. Heat leaves with the chip, the hardened layer is cut through in one pass, and tool life on 316L often improves noticeably.
The catch is machine and holder stiffness. Deep axial passes on a long tool will deflect and chatter, and chatter on stainless damages the surface and the edge at the same time. If the setup is light, stay with the shallow strategy and accept shorter tool life.
Radial engagement also determines whether the tool is climb milling or conventional milling on the entry. Climb milling is the default for stainless because it starts the cut with a thick chip and avoids rubbing on entry.
Cooling, chip evacuation and tool geometry
Coolant on stainless has two jobs: remove heat and clear chips. Recutting a chip is one of the fastest ways to chip an edge, because the chip is already work hardened. Through-spindle coolant at 40–70 bar is the reliable answer for deep pockets and holes deeper than three times the diameter. Flood coolant is acceptable for open face milling if the flow reaches the cut zone.
Coolant concentration matters too. A weak mix loses lubricity exactly where built-up edge forms. Most shops run 8–10 percent for stainless, checked weekly rather than once a month.
Tool geometry should be specific to stainless. A positive rake angle of 12–20 degrees reduces cutting forces; a sharp, honed-but-not-rounded edge resists built-up edge; and a coating such as AlTiN or AlCrN holds up to the temperature. Uncoated carbide works for finishing passes on 303, but it wears quickly on 316L and 17-4PH.
Chip evacuation is the hidden parameter. If chips pile up in a pocket, no amount of speed tuning will save the tool. Program the path so chips exit the cut zone, and prefer air blast plus minimum quantity lubrication over a flooded pocket that traps chips.
Starting parameters by stainless grade
Solid carbide tooling, coated, coolant on. Verify on the machine before committing to a production run.
| Grade | Roughing speed | Feed per tooth | Typical use |
|---|---|---|---|
| 303 (free machining) | 250–350 SFM | 0.08–0.15 mm | Shafts, fittings, high-volume turning |
| 304 / 304L | 120–180 SFM | 0.05–0.12 mm | Brackets, housings, general parts |
| 316 / 316L | 100–160 SFM | 0.05–0.10 mm | Marine, medical, chemical exposure |
| 17-4PH (SUS630) | 100–150 SFM | 0.04–0.10 mm | Aerospace, high-strength shafts |
| 420 / 431 | 150–220 SFM | 0.06–0.12 mm | Valves, pump parts, wear surfaces |
| 440C | 100–140 SFM | 0.04–0.08 mm | Bearings, knives, high hardness |
| Austenitic, deep pocket | Reduce 20 percent | Keep above 0.05 mm | Long reach, weak setup, chatter risk |
Two cutting strategies and when each one wins
| Item | Shallow and wide | Deep and narrow |
|---|---|---|
| Axial depth | 0.5–1 × diameter | 1–2 × diameter |
| Radial engagement | 50–70 percent | 5–10 percent |
| Heat removal | Moderate | Better, chip carries heat |
| Work hardening | Repeated light passes | Cut through in one pass |
| Setup stiffness needed | Low | High |
| Best for | Thin walls, long tools, first article | Rigid setups, 316L, 17-4PH |
| Main risk | Built-up edge, poor finish | Chatter and tool deflection |
The rule we machine by
If the setup is rigid and the tool is short, run deep axial passes with light radial engagement and keep feed per tooth above 0.05 mm. If the part is thin-walled or the tool has to reach, go shallow and wide, slow the speed 20 percent, and accept shorter tool life rather than chase a finish that the setup cannot hold.
Questions we get on stainless cutting data
Can I use the same parameters for 304 and 316L?
Not quite. 316L adds molybdenum, which raises hot strength and lowers thermal conductivity a little further. Start about 15–20 percent slower than your 304 numbers and keep feed per tooth the same or slightly higher.
If tool life drops sharply when you switch from 304 to 316L on the same program, the speed is usually the culprit, not the feed.
Why does my surface finish get worse when I slow the feed down?
On stainless, a lower feed per tooth means the edge rubs instead of shearing. The surface work hardens, built-up edge grows on the rake face, and the finish becomes torn rather than cut.
Check for a dull edge first. If the tool is fresh and the finish is still poor, raise feed per tooth toward 0.08 mm and see whether it improves.
Do I need through-spindle coolant for every stainless job?
No. Open face milling with good flood coverage is fine. Through-spindle coolant earns its cost on holes deeper than three times the diameter, deep pockets, and any operation where chips would otherwise be recut.
If you are drilling 304 without through coolant, use a peck cycle and pull the tool clear often enough to clear chips.
How do I know the material has work hardened?
The signs are a sudden rise in cutting noise, a finish that turns from bright to dull, and chips that come off as fine dust instead of curled segments. On a previously machined surface it often shows as a hard skin that dulls a new edge within minutes.
Once a layer is hardened, a light pass will not remove it cleanly. Take a deeper pass below the hardened zone or change the tool geometry.
Which coating holds up best on stainless?
AlCrN and AlTiN are the usual choices because they resist the temperatures stainless generates. TiAlN also works but tends to break down earlier at higher speeds.
The coating matters less than edge preparation. A sharp edge with a light hone resists built-up edge better than a heavily rounded edge, whatever the coating.
Can stainless parts be held to ±0.005 mm?
Yes, on rigid setups with temperature-stable material and in-process checking. Stainless moves with heat, so rough, let the part cool, then finish. Measuring a warm part and adjusting the offset is a common source of drift.
We inspect 100 percent of parts before shipment and can supply reports on request.
Send us the drawing, get the process window back
We machine 303, 304, 316L, 17-4PH and 440C daily on 127 CNC machines, including 16 simultaneous 5-axis centers. Upload your files and we return a quotation with free DFM analysis within 12 hours.
Quotation in 12 hours±0.005 mm toleranceFrom one prototype to 10,000+ partsNDA on request
Follow GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
