Guides / Process

Invar 36 Machining Parameters: Speeds, Feeds and Tool Wear

September 20, 2026

Invar 36 does not machine like a mild steel or an aluminum alloy of similar hardness. It machines more like an austenitic stainless: gummy, prone to work hardening and hard on tool edges if the program is not built for it. A shop that has cut Invar before sets speeds, feeds and tool geometry to match, and the difference shows up in tool life and surface finish, not just cycle time.

Why Invar behaves the way it does

Invar 36 is roughly 64 percent iron and 36 percent nickel, and it shares the face centered cubic structure that makes austenitic stainless gummy to cut. The material work hardens quickly under a dull edge or a light, rubbing cut, which raises cutting forces on the next pass. Left unmanaged, this turns into chatter, built up edge and a surface finish that gets worse instead of better as a tool wears.

The alloy also has lower thermal conductivity than plain carbon steel, so heat generated at the cutting edge does not move away from the tool as fast. That heat concentrates right where the tool is doing the most work, which is part of why tool life in Invar tends to be shorter than in a similarly hard steel.

Typical turning parameters

For carbide tooling on a rigid CNC lathe, shops commonly run Invar 36 at lower surface speeds than 4140 steel, with a feed rate chosen to keep the tool cutting rather than rubbing. As a starting point for roughing with a coated carbide insert:

Operation	Surface speed	Feed	Depth of cut
Roughing, coated carbide	40 to 70 m/min	0.15 to 0.3 mm/rev	1 to 3 mm
Finishing, coated carbide	60 to 90 m/min	0.05 to 0.15 mm/rev	0.2 to 0.5 mm

These are typical starting points, not fixed numbers. The right values depend on the insert grade, part rigidity and coolant delivery, and a shop tunes them against the tool life and finish it actually sees.

Typical milling parameters

Milling Invar 36 follows the same logic: keep the edge cutting, avoid dwell, and clear chips before they recut. Solid carbide end mills with a coating suited to nickel alloys are common. A shop typically starts with:

Operation	Surface speed	Feed per tooth	Axial depth
Roughing, solid carbide	30 to 60 m/min	0.05 to 0.1 mm/tooth	Up to 1x diameter
Finishing, solid carbide	40 to 70 m/min	0.03 to 0.06 mm/tooth	0.2 to 0.5 mm

Climb milling is the usual choice, since it keeps the chip thickness decreasing through the cut rather than starting the tooth on a thin, rubbing chip that encourages work hardening.

Tool geometry and coating

A few choices matter more in Invar than in steel:

• Sharp, positive rake edges. A negative or heavily honed edge rubs before it cuts, and rubbing is what hardens the surface.
• Coatings suited to nickel alloys. AlTiN and similar coatings that resist heat and built up edge outperform plain TiN in most shops’ experience.
• Chip breakers. Invar produces long, stringy chips that wrap around the tool or the part if the geometry does not break them.
• Consistent tool life tracking. Because wear accelerates once an edge starts to dull, shops that cut Invar regularly change tools on a schedule rather than running them to visible failure.

Coolant and chip control

Flood coolant aimed directly at the cutting edge, not just the general work area, removes heat and helps prevent the recutting of stringy chips. Some shops run through spindle coolant on drilling and deep pocket work for the same reason: the heat has to leave the cutting zone quickly or it stays in the tool and the part.

Chip evacuation is a real setup consideration, not an afterthought. On multi pass roughing, a program that pauses to clear chips or pecks deeper holes instead of drilling through in one pass avoids the recutting that shortens tool life.

What this means for your part

None of this changes what shows up on your drawing, but it explains two things buyers often ask about. First, why an Invar 36 quote includes more machine time than the same geometry in steel, covered in more detail in why Invar 36 parts cost more. Second, why a shop with Invar experience asks about tolerances before it commits to a cutting strategy: a part that needs a mirror finish or a tight position tolerance gets a different, slower finishing pass than one that only needs to fit.

If your drawing has features that are hard to reach or awkward to fixture, mention them on the RFQ. A shop that machines Invar regularly can often suggest a sequence that holds the tolerance without adding unnecessary passes. Invar’s iron-nickel composition and its face centered cubic structure explain most of the cutting behavior described above, if you want the metallurgy background.

Send your drawing through our RFQ form and we match it with shops that already run these parameters, so your quote reflects real cutting time instead of a guess.

Frequently asked questions

Keep reading

• Invar Drilling and Tapping: Hole Quality and Thread Practices
• Invar Fixturing and Workholding: Avoiding Distortion During Machining