You are here:

Machining Inconel 718: What It Actually Takes

Views: 0 Publish Time:
Renjie Precision
Precision CNC Machining, Sheet Metal & Injection Moulding
specializes in precision CNC machining, rapid prototyping, sheet metal fabrication, laser cutting, plastic injection molding, and surface finishing
follow me on:


Machining Inconel 718: What It Actually Takes

Inconel 718 is the material that turns a normal machining job into a project. It keeps its strength at 650 °C, resists oxidation and creep, and is used in turbine discs, rocket engine components, nuclear valves and high-pressure wellhead parts. It is also one of the least cooperative metals to cut: it work-hardens, it conducts heat badly, and it destroys tools that are not set up for it.

A part that costs $40 in 17-4 PH can cost $400 in 718 — not because the material is ten times dearer, but because the process is.

Why It Is Difficult

Four properties compound:

  • Work hardening. The surface hardens as it is cut. A tool that rubs instead of cutting hardens the next layer, and the next pass cuts through hardened material — a spiral that ends in a broken tool.
  • Low thermal conductivity. About 11 W/m·K, against 167 for aluminium. Heat stays at the cutting edge, so tool life is governed by temperature, not by force.
  • High hot strength. It does not soften when hot — the property that makes it useful is the property that makes it hard to cut.
  • Abrasive carbides and a gummy chip. Chips tend to weld to the edge, causing notching and built-up edge.

Tooling: Where the Money Goes

Carbide, fine grain, with a heat-resistant coating. AlTiN and AlCrN are common; PVD coatings outperform CVD for sharp edges. Positive rake geometry with a strong edge hone, and a chip breaker designed for nickel alloys.

OperationSurface speedFeedNotes
Rough milling (carbide)30–45 m/min0.08–0.12 mm/toothRadial depth 25–40% of diameter, axial 1–2× D
Finish milling40–60 m/min0.05–0.1 mm/toothSmall step-over, climb milling only
Turning (rough)25–40 m/min0.15–0.25 mm/revDepth of cut below the hardened layer
Drilling (HSS-Co or carbide)8–12 m/min0.05–0.08 mm/revPeck, through-coolant essential
Tapping3–6 m/min—Thread mill instead of tap wherever possible

These speeds feel absurdly slow next to aluminium. They are not conservative — running 718 at 80 m/min will destroy a $60 cutter in minutes.

The Rules That Keep Tools Alive

Never rub

Every pass must cut. A tool that dwells or takes a 0.02 mm depth of cut in work-hardened material generates heat and hardens the surface further. Keep the feed per tooth up and the radial engagement generous; a lighter pass is not a safer pass in 718.

Cut below the hardened layer

Depth of cut should be at least 0.5 mm, and ideally deeper, so the edge is always in fresh material rather than skimming the work-hardened skin left by the previous pass.

High-pressure coolant, aimed at the edge

Through-tool coolant at 70 bar is the single biggest tool-life improvement in 718. It breaks the chip, cools the edge and prevents built-up edge. Flood coolant at low pressure is much less effective.

Climb mill, always

Conventional milling in 718 produces a work-hardened, smeared surface and rapid flank wear. Every finishing path should be climb.

Expect to change tools

Tool life is measured in minutes, not hours. A shop quoting 718 will plan for several tools per part and will price them in. If a quote looks cheap, ask how many tools it assumed.

Machining Strategy

Rough with a large tool and a trochoidal path. Dynamic or trochoidal milling keeps radial engagement small and constant, which spreads heat and lets the tool cut rather than rub. It is slower per pass but far more predictable, and in 718 predictability is worth more than speed.

Leave 0.5–1 mm for finishing. More than that and the finish pass becomes a roughing pass in hardened material; less and the finish cannot clean up the roughing marks.

Minimise setups. Every re-fixture is a chance to cut into a hardened surface. Five-axis or multi-sided fixtures pay for themselves on this material.

Drill with care. Deep holes in 718 are the most common failure point — chip packing, then breakage. Peck, use through-coolant, and consider drilling undersize then boring.

Heat Treatment and Stress

718 is usually supplied in the annealed or solution-treated condition and aged after machining (720 °C for 8 h, then 620 °C for 8 h, typical). Aging causes shrinkage of roughly 0.04–0.08%, and distortion if the part is asymmetric.

The consequence for the drawing: decide whether tolerances apply before or after aging. If a bore must be H7 in the finished part, either machine it undersize and finish after aging, or accept that the aging will move it.

Stress relief before finish machining is common on thin or asymmetric parts: solution treat, rough machine, stress relieve, finish machine, age.

Cost: What to Expect

For an 80 mm diameter, 40 mm thick flange with a bore and eight holes, 10 pieces:

MaterialMaterial costMachiningTotal index
6061 aluminiumLowFast1.0
304 stainlessLowModerate2.5
17-4 PHModerateModerate4
Inconel 718HighVery slow, high tool wear12–20

The multiplier is mostly machine time and tooling. A 718 part that takes 3 hours of spindle time where aluminium took 20 minutes is normal, and at $60–90/hour that is the whole cost.

Design Rules That Save Money

  • Do not over-specify tolerance. 718 holds tolerance well, but every tight feature costs finishing time in a material that is already slow.
  • Avoid deep, narrow pockets. Depth-to-diameter above 4:1 in 718 is where tools break.
  • Use thread inserts or thread milling instead of tapping small threads; taps break and a broken tap in a $500 part is a scrap.
  • Keep the part shape balanced so aging does not bow it.
  • Specify the condition — annealed, solution treated + aged, or as-aged — because it changes both machinability and the sequence.

Reading Tool Wear in 718

Tool failure in Inconel is not random, and the wear pattern tells you which parameter is wrong. Learning to read it saves more money than any speed table.

  • Flank wear with a uniform band — normal progression. Change the tool at the planned interval and nothing else.
  • Notching at the depth-of-cut line — work hardening from the previous pass, or a depth that skims the hardened layer. Increase depth of cut so the edge stays in fresh material.
  • Cratering on the rake face — cutting temperature too high. Reduce surface speed 15–20%, and check coolant delivery is reaching the edge rather than the chip.
  • Chipping on the cutting edge — interrupted cut, vibration, or a tool that is too sharp for the load. A small edge hone and a more rigid setup fix it.
  • Built-up edge and a smeared finish — speed too low for the coating, or coolant starved. Increase speed slightly and raise pressure.

The pattern to watch for is a change in the pattern. A tool that suddenly notches where it previously wore evenly is telling you a fixture moved or a batch of material is different — both worth investigating before the next part.

Setup and Fixturing

Inconel punishes any flexibility in the setup. A part that moves by 0.05 mm under cutting load will produce a tool that rubs on one pass and bites on the next — and rubbing is how work hardening starts.

Three practices are standard:

  • Support the part under the cut. A jack or a support block beneath a thin floor is not optional; deflection changes the effective depth of cut and the edge load.
  • Minimise overhang. Tool overhang should be as short as the geometry allows. Every extra 10 mm of stick-out increases deflection and chatter, and chatter in 718 kills edges.
  • Prefer rigid workholding over fast workholding. Soft jaws are fine; a single clamp on a tall part is not. If the setup needs a fixture, build the fixture.

The cost of a fixture is small next to the cost of a scrapped 718 part or a weekend of broken tools, which is why experienced shops will quote a fixture on a first article even at low volume.

Coolant delivery deserves the same attention as tool selection. On a deep pocket, flood coolant from one nozzle never reaches the cutting edge, and the tool fails while looking correctly specified on paper. Through-spindle coolant, or a high-pressure jet aimed at the flank from close range, is what makes the parameter table achievable. If a shop says it machines 718 but has no high-pressure coolant, believe the equipment over the claim.

Frequently Asked Questions

Can Inconel 718 be machined without coolant?

No, not practically. Dry machining generates edge temperatures that destroy carbide in seconds. High-pressure coolant is the standard.

How much slower is 718 than stainless?

Typically five to eight times the cycle time, and three to five times the tool consumption. Some geometries are worse.

Is 718 harder to machine than titanium?

Different. Titanium's problem is heat and chatter with a tendency to gall; 718's problem is work hardening and abrasion. Most shops find 718 slower but more predictable than Ti-6Al-4V.

Can 718 be welded?

Yes, but it needs a controlled procedure and post-weld heat treatment. For machined parts, welding is usually avoided because it introduces distortion and residual stress into a part that is already difficult to hold.

Why did my tap break?

Work hardening in the hole, chip packing, or too high a speed. Thread milling avoids the problem entirely and is the recommended approach for anything above M6.

The Short Version

Slow speeds, heavy feeds, sharp coated tools, high-pressure coolant, climb milling and no rubbing. Those six rules are the difference between a 718 job that finishes and one that eats cutters and scrapped parts.

Budget for 12–20× an aluminium part and plan the heat treatment sequence before the first cut. The general rules for difficult materials are in our material guide, and the tolerance implications of post-machining heat treatment are covered in the tolerance breakdown.