Is CNC Machining Used for Nitinol?

• 1
  Why Nitinol Cuts Differently From Other Metals
• 2
  Tool Geometry and Coating Choices That Hold Up
• 3
  Cutting Parameters: What Actually Works
• 4
  Heat, Transformation Temperature and Phase Damage
• 5
  Where CNC Fits and Where It Does Not
• 6
  Matching Nitinol Geometry to the Right Process

Nitinol is roughly 55% nickel and 45% titanium by weight. Those two elements form an intermetallic phase that is hard, abrasive and a poor conductor of heat. When a carbide insert shears a chip off a 6061 aluminum block, most of the heat leaves with the chip. With nitinol, a large share of the heat stays in the cut zone because the alloy conducts heat at roughly one third the rate of titanium and a fraction of steel. The edge gets hot while the chip stays cooler than you would expect.

The alloy also has a low elastic modulus, around 30–40 GPa in the austenite phase. Push it with a dull tool and it springs away from the edge instead of forming a clean chip. That springback is the root cause of most chatter, poor finish and tool breakage on nitinol jobs. A sharp edge with a positive rake keeps the cut compressive and reduces the load that feeds back into the part.

Nitinol work-hardens fast. Once a surface layer has been deformed, hardness climbs and the next pass has to shear through a harder skin. That is why depth of cut and feed per tooth matter more than spindle speed in most setups. Take a light pass at low feed and the material rubs, hardens, then fights the following pass. Take a proper bite and the cut stays below the hardened zone.

• 1
  Low thermal conductivityHeat concentrates at the edge instead of leaving with the chip.
• 2
  Low elastic modulusThe part deflects away from the tool, which drives chatter and poor finish.
• 3
  Rapid work hardeningLight rubbing passes harden the surface and shorten tool life.

Carbide is the starting point for CNC machining used for nitinol parts, but not every grade works. Use a submicron or ultrafine grain carbide with high hot hardness. Uncoated micrograin carbide often outperforms coated grades here, because many PVD coatings break down chemically against titanium-rich alloys and leave a rough edge that tears the surface. If you do coat, choose an AlTiN or AlCrN layer and expect to test it on scrap first.

Geometry matters more than grade. A sharp, positive rake angle reduces cutting forces and limits springback. High helix angles, usually 40–45 degrees, pull the chip up and out of the slot instead of letting it pack. Polished flutes help chip evacuation because nitinol chips are stringy and tend to weld to the tool. A small edge hone, in the 5–10 μm range, adds edge strength without making the tool dull.

For small features, a four-flute end mill with a 0.5–1.0 mm diameter is common, but chip clearance becomes the limiting factor. Two-flute cutters clear chips better and are the safer choice in deep pockets under 3× diameter. Above that depth, use air blast and pecking passes rather than flooding coolant alone. Flood coolant still helps, but it cannot reach the bottom of a deep slot on its own.

Tool life on nitinol is short by metalworking standards. Expect to change cutters several times on a job that would use one tool in stainless. Track wear with a microscope every few parts and set a hard replacement limit. A worn 0.2 mm corner radius will rub, harden the surface and push your finish past Ra 1.6 μm before you notice it visually.

• 1
  Micrograin carbideUncoated grades often outlast coated ones on titanium-rich alloys.
• 2
  40–45° helixLifts stringy chips clear of the slot and reduces recutting.
• 3
  5–10 μm edge honeAdds edge strength without dulling the cutting edge.
• 4
  Replace on a scheduleInspect under magnification; do not run to visual failure.

There is no universal recipe for nitinol. Starting points are usually surface speed of 15–30 m/min for carbide, feed per tooth of 0.01–0.03 mm, and radial engagement of 5–10% of cutter diameter. These numbers sit far below what the same cutter would run in 316 stainless. The goal is to keep the cut in a narrow band where the chip forms cleanly and the edge does not rub.

Depth of cut depends on the operation. For roughing, an axial depth up to 0.5× diameter with light radial engagement keeps radial forces low and manages the heat. For finishing, drop to 0.05–0.1 mm radial and 0.2–0.5 mm axial. Climb milling is standard because it starts the cut at maximum chip thickness, which avoids the rubbing that work-hardens the surface.

Coolant choice matters less than delivery. High-pressure flood at 40–70 bar reaches the cut zone on most features. Air blast plus minimum quantity lubrication works well on thin walls where the part cannot take much side load. If you run dry, expect short tool life and watch for discoloration that signals overheating.

Rigidity in the setup is not optional. Nitinol parts are often thin and long, so they deflect under load. Support them with a tailstock, steady rest, or a sacrificial support that you machine away later. On a 5-axis machine, keep the part as close to the table as the geometry allows. Every millimeter of overhang amplifies the springback problem.

• 1
  Surface speed15–30 m/min with carbide; well below stainless practice.
• 2
  Feed per tooth0.01–0.03 mm to avoid rubbing and hardening.
• 3
  Radial engagement5–10% of cutter diameter for roughing and finishing.

The shape memory effect in nitinol depends on the transformation temperature, usually written as Af. That value sits near body temperature for many medical grades. If the cut zone rises above Af during machining, the material locally transforms to austenite and the crystal structure changes. It may transform back on cooling, but the surrounding stress state does not fully reset. Repeated thermal cycling can shift the Af by a few degrees, which is enough to change how a stent or guidewire performs.

This is why aggressive speeds and dry cutting are risky on functional nitinol parts. The surface may look fine under a loupe but behave differently in a bend test. For parts where the Af is specified, keep the bulk temperature below the transformation range and use coolant continuously. Do not let the part sit in a hot chip pile.

Heat also drives oxidation. Titanium-rich alloys form a hard oxide layer quickly above roughly 400 °C. That layer is brittle and can flake during later passes, leaving pits. On finishing cuts, keep the surface cool and avoid dwell. If you see a straw or blue tint on the chips, the edge is running too hot.

For parts where transformation behavior is critical, plan a stress relief or shape-setting step after machining. That step is outside the machining scope, but it affects how much stock you leave and how you fixture the part. Leave enough material for the heat treat vendor to work with, and document the as-machined condition so they can adjust the cycle.

• 1
  Af near body temperatureSmall thermal shifts change functional behavior in medical parts.
• 2
  Oxide above 400 °CBrittle scale can flake and leave pits on the surface.
• 3
  Leave heat-treat stockShape setting and stress relief need extra material to work with.

CNC machining used for nitinol works best on prismatic parts with moderate aspect ratios. Think bone anchors, catheter hubs, biopsy forceps components, orthodontic brackets and small robot grippers. These parts have features you can reach with a 0.5–3.0 mm cutter, walls above 0.3 mm thick, and tolerances in the ±0.005 mm to ±0.05 mm range. They also tend to be short, so deflection stays manageable.

The process struggles with very thin walls and long slender features. A 0.1 mm wall on a 20 mm long tube will deflect and chatter no matter how sharp the tool is. Nitinol is often better formed by laser cutting, wire EDM or photochemical etching for those geometries. Those processes avoid mechanical load entirely, which suits thin sections and complex outlines.

Deep holes and small internal channels are another weak spot. Drilling nitinol below 1 mm diameter is slow, and chip evacuation is poor. If your design needs a long internal lumen, consider gun drilling from both ends, EDM, or designing the part in two pieces joined later. Each route has trade-offs in cost and lead time, so bring the drawing to the quote stage early.

Surface finish is achievable but costly. A Ra 0.8–1.6 μm finish on nitinol is realistic on flat and gently curved surfaces with the right parameters. Mirror finishes below Ra 0.4 μm usually need lapping or electropolishing after machining. Plan those steps into the process rather than asking the mill to deliver them in one pass.

• 1
  Good fitPrismatic parts, walls above 0.3 mm, features reachable with small cutters.
• 2
  Poor fitVery thin walls, long slender sections, sub-millimeter deep holes.
• 3
  Consider alternativesLaser cutting, wire EDM and etching avoid mechanical load.