Inconel 718 (UNS N07718): cutting speed and feed rate

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 →

Inconel 718 turns at 20-50 m/min (roughly 65-165 SFM) with 0.12 mm/rev on coated carbide, mills at 25-35 m/min with 0.05 mm per tooth, drills at 14-38 m/min and taps at 7-23 m/min. Those are the lowest speeds in the whole catalogue, and there is a reason: this nickel superalloy keeps its hardness at exactly the temperature the cutting edge works at. Here every parameter is chosen to make the edge survive, not to go fast.

EN NiCr19NbMo · UNS N07718 · 360 HB · ISO group S

Recommended speeds and feeds

OperationVc (m/min)FeedShop note
Turning20–500.12 mm/rev20-50 m/min at 0.12 mm/rev with a round insert or a small lead angle, a large edge hone and high pressure coolant. Always enter and exit on a ramp or an arc, never straight in, and vary the depth between passes so the notch does not repeat.
Milling25–350.05 mm/tooth25-35 m/min with 0.05 mm per tooth, climb milling, short arc of contact and trochoidal in pockets. Each tooth's entry is the critical moment: chip thickness has to build from a real value, not from zero, or every flute starts by rubbing already hardened material.
Drilling14–380.06 mm/rev14-38 m/min at 0.06 mm/rev, a short and very rigid carbide drill, through-coolant and continuous feed. No long drills and no unnecessary pecks: every re-entry into the hole meets a harder floor than the last one.
Threading7–230.06 mm/rev7-23 m/min. Thread mill with carbide wherever you can: a tap in Inconel works at enormous torque and, if it breaks off inside, you can neither drill it out nor pick it out. Drill for 60% thread engagement and lubricate under pressure.

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

Inconel 718 is a precipitation-hardened nickel superalloy at around 360 HB, designed specifically not to give way under heat: it keeps its strength at temperatures where any steel would have softened. It work hardens aggressively, so every pass leaves a layer far harder than the base material. It contains niobium and titanium carbides that abrade the edge, and its thermal conductivity is even lower than titanium's. The result is a very characteristic failure mode: depth of cut notching, a bite taken out of the edge exactly where it meets the part surface.

Depth of cut notching drives tool life

In Inconel 718 the edge does not die of uniform wear, it dies of a notch located exactly where the edge crosses the outside surface of the part. It is fed by material hardened on the previous pass, by the side burr that forms, and by the alloy's hard carbides. When the notch grows, the insert lets go and usually takes size and finish with it. The most effective countermeasure is to vary the depth of cut between successive passes so the notch never forms twice on the same line, and to use small lead angles or round inserts that spread the load over more edge length.

Constant feed and gentle entries: the discipline that saves edges

Inconel punishes any hesitation. A feed stop, a spring pass or a straight full-depth entry leaves a hardened zone that wrecks the edge. Program ramp or arc entries, exits under feed, radii on path corners, and no stretch where the tool is in contact without cutting. The feed must be enough for chip thickness to exceed the edge radius: 0.12 mm/rev turning and 0.05 mm per tooth milling are not conservative values, they are the minimum needed to cut rather than burnish. Backing the feed off to protect the tool achieves precisely the opposite.

High pressure coolant and overall rigidity

Coolant in Inconel is not only about temperature: it is chip control and contact-zone control. A high pressure jet aimed between chip and rake face lifts the chip, shortens the contact length and measurably reduces wear. This is the material where high pressure coolant most clearly justifies its cost. Add rigidity to that: short toolholders, firm clamping and a machine with real power available at low rpm, because cutting forces are very high. If the setup chatters, the notch arrives sooner and the whole strategy falls apart.

Quick shop tips

  • Vary the depth of cut between passes: it is the single most effective measure against edge notching.
  • Always enter and exit on a ramp or an arc; a straight entry in Inconel breaks the edge on the first part.
  • Do not reduce the feed to protect the tool: below the minimum the edge burnishes, hardens the material and dies sooner.
  • High pressure coolant aimed at the edge; in Inconel it is the improvement that buys the most tool life.
  • Short toolholders and rigid clamping; with the cutting forces in this material, chatter is not forgiven.
  • Prefer a thread mill to a tap: a broken tap in Inconel writes the part off.

Frequently Asked Questions (FAQ)

What cutting speed will Inconel 718 really take?

With coated carbide, 20-50 m/min turning and 25-35 m/min milling. Ceramic strategies go much higher, but they need the right machine, workholding and experience; with carbide, going over that range costs you edges immediately.

Why does a notch form on my insert turning Inconel?

Because at the depth of cut line you get material hardened by the previous pass, the side burr and the alloy's hard carbides all at once. Fight it by varying the depth between passes and using round inserts or small lead angles.

Can I drill Inconel 718 with an HSS drill?

In practice it is not viable for repetitive work: at 5-13 m/min an HSS drill lasts very little and the hole floor hardens with every pass. Use a short carbide drill with through-coolant at 14-38 m/min and a continuous 0.06 mm/rev feed.

What is the minimum feed in Inconel 718?

Turning, do not go below 0.10-0.12 mm/rev; milling, do not go below 0.05 mm per tooth. Under that, chip thickness is smaller than the edge radius, the tool burnishes instead of cutting, and work hardening takes off.

Will 316 stainless parameters work on Inconel 718?

No. 316 turns at 100-180 m/min and Inconel at 20-50: a factor of four or five. They share adhesion and work hardening, but Inconel also keeps its hardness hot and abrades with its carbides.

Similar materials

Ti-6Al-4V (grade 5) titanium: cutting speed and feed rate

Cutting speed and feed for Ti-6Al-4V grade 5 titanium: Vc per operation, high pressure coolant and why you never let the cutting edge dwell in the cut.

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.