Speeds, Feeds and Tool Life for Machining Invar 36

By Invar Machining editorial team· Updated September 26, 2026 · How we write these guides

Typical Invar 36 machining parameters sit close to those for 304 stainless: coated carbide milling at 30 to 60 m/min, HSS at 15 to 25 m/min, feeds held high enough that the edge always takes a real chip and flood coolant aimed at the cut. The alloy is gummy, prone to work hardening and hard on tool edges if the program is not built for it. The tables below are starting points a shop adjusts against the tool life and finish it actually sees, and the shop’s own program governs.

Why Invar 36 behaves the way it does

Invar 36 is about 64 % iron and 36 % nickel, and it shares the face-centered cubic structure that makes austenitic stainless gummy to cut. Annealed hardness is only about 70 to 80 HRB, roughly 130 to 160 HB, so the alloy is soft, and the trouble is not hardness. 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. Machinability ratings put it at roughly 40 to 50 % of a free-cutting steel, in the same band as 304 stainless.

The alloy also has lower thermal conductivity than carbon steel, so heat generated at the cutting edge does not move away from the tool as fast. That heat concentrates 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. Invar’s iron-nickel composition and its face-centered cubic structure explain most of this behavior, and why Invar work hardens covers the mechanism in more depth.

Typical milling parameters

Milling Invar 36 comes down to keeping the edge cutting, avoiding dwell and clearing chips before they are recut. Typical starting points:

Operation	Tool material	Speed, m/min	Feed per tooth, mm	Depth notes
Roughing, side milling	Coated solid carbide, AlTiN or similar	30 to 60	0.05 to 0.10	Axial up to 1x diameter, radial 25 to 40 % of diameter
Roughing, HSS	HSS-Co (M42 class)	15 to 25	0.04 to 0.08	Axial 0.5x diameter, shallower radial
Finishing	Coated solid carbide	40 to 70	0.03 to 0.06	Axial 0.2 to 0.5 mm, radial 0.1 to 0.3 mm, after stress relief
Face milling	Indexable carbide, positive rake	40 to 70	0.08 to 0.15	Axial 0.5 to 2 mm, full engagement avoided on thin plate

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. On pockets, a trochoidal or dynamic toolpath with a small radial step and a full axial depth keeps the load constant and the heat in the chip. Strategy choices are covered in Invar milling strategy.

Typical turning parameters

For carbide tooling on a rigid CNC lathe, shops run Invar 36 at lower surface speeds than 4140 steel, with a feed chosen to keep the tool cutting rather than rubbing. Typical starting points:

Operation	Tool material	Speed, m/min	Feed, mm/rev	Depth notes
Roughing	Coated carbide insert, positive chip breaker	40 to 70	0.15 to 0.30	1 to 3 mm, constant depth to avoid a work-hardened step
Roughing, HSS	HSS-Co	15 to 25	0.10 to 0.20	1 to 2 mm
Finishing	Coated carbide, sharp nose	60 to 90	0.05 to 0.15	0.2 to 0.5 mm, after stress relief
Parting and grooving	Carbide, narrow chip breaker	30 to 50	0.05 to 0.10	Coolant into the groove, feed never below the minimum chip

Turning brings its own trap: long chips wrap around the part and the chuck unless the insert breaks them. A chip breaker matched to the feed range, not a general-purpose one, is the usual fix. Invar CNC turning covers lens cells, spacers and other round parts in more detail.

Typical drilling and tapping parameters

Holes are where work hardening bites hardest, because a drill that pecks too lightly or dwells at the bottom builds a hard skin that the next peck or the tap has to cut. Typical starting points:

Operation	Tool material	Speed, m/min	Feed	Depth notes
Drilling	HSS-Co twist drill, 130° to 135° split point	10 to 15	0.05 to 0.12 mm/rev, rising with diameter	Peck 1x diameter, full retract to clear chips
Drilling	Solid carbide drill, through-coolant	30 to 50	0.08 to 0.15 mm/rev	Deeper pecks or none with through-coolant
Reaming	Carbide or HSS-Co reamer	8 to 15	0.15 to 0.30 mm/rev	Leave 0.1 to 0.2 mm, flood coolant
Tapping, cut	HSS-E spiral flute, TiN or TiCN	3 to 6	Pitch	65 to 70 % thread, drill at the large end of the size band
Tapping, form	HSS-E form tap	5 to 10	Pitch	Larger pre-hole, ductile alloy suits forming, oil or high-lubricity coolant
Thread milling	Solid carbide thread mill	25 to 40	0.03 to 0.05 mm/tooth	Preferred for blind holes and M6 and larger, no tap breakage risk

A tap that stalls in Invar costs the tap and often the part, which is why many shops thread mill what they can and specify thread inserts on repeat-assembled holes. See Invar drilling and tapping and thread inserts for Invar.

Tool wear and work hardening

Tool wear in Invar 36 follows a pattern. A sharp edge cuts cleanly for a while. As it dulls it begins to rub, the rubbing work hardens the surface, the hardened surface accelerates the wear and soon the edge is gone. The curve is flat then steep, which is why shops that cut Invar regularly change tools on a schedule rather than running them to visible failure.

Three 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 heat-resistant coatings outperform plain TiN in most shops’ experience. Uncoated sharp carbide can be the right choice for finishing when the coating’s edge hone is too large.
• Chip breakers matched to the feed. Invar produces long, stringy chips that wrap around the tool or the part if the geometry does not break them.

The feed is the lever most often set wrong. A finishing pass at 0.02 mm per tooth “to get a better finish” does the opposite in Invar, because the edge cannot get under the hardened skin and rubs instead. Keep the chip above the edge radius, roughly 0.03 mm per tooth for a carbide finisher, and take the finish from a sharp tool and a rigid setup rather than a light chip. What the work-hardened layer means for the part’s later stability is covered in why Invar work hardens and stress relief for Invar machined parts.

Coolant and chip control

Flood coolant aimed directly at the cutting edge, not the general work area, removes heat and helps prevent recutting of stringy chips. Through-spindle coolant on drilling and deep pockets serves the same purpose: the heat has to leave the cutting zone quickly or it stays in the tool and the part. Emulsion at a higher concentration than for steel, or a high-lubricity oil for tapping and forming, is typical. Dry cutting and minimum quantity lubrication are possible on roughing but rarely on finishing, where thermal growth of the part during the cut matters. The choice is covered in coolant strategy for Invar.

Chip evacuation is a setup consideration, not an afterthought. 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. Because the alloy is ferromagnetic, fine chips cling to the part and the fixture, so cleaning between setups is part of the process.

Worked example: starting point for a hypothetical 12 mm carbide end mill

Take a hypothetical Invar 36 mounting plate, 25 mm thick, pocketed with a 12 mm four-flute AlTiN coated solid carbide end mill on a rigid vertical machining center with flood coolant, roughed before stress relief and finished after. Values are typical starting points, not a program.

Roughing. Pick a surface speed of 45 m/min, mid-band. Spindle speed is speed times 1000 divided by π times diameter: 45 × 1000 / (3.1416 × 12) = about 1190 rpm, so call it 1200 rpm. Feed per tooth 0.08 mm. Table feed is feed per tooth times flutes times rpm: 0.08 × 4 × 1200 = 384 mm/min, so about 380 mm/min. Axial depth 12 mm, one diameter, radial step 3.6 mm, 30 % of diameter, climb milling with a dynamic toolpath. Material removal rate is about 12 × 3.6 × 384 = 16,600 mm3/min, or 16.6 cm3/min. Leave 0.5 mm on the walls and floor for the finishing pass, then send the part to stress relief.

Finishing. After the furnace, a fresh tool. Surface speed 55 m/min gives about 1460 rpm, call it 1450 rpm. Feed per tooth 0.05 mm gives 0.05 × 4 × 1450 = 290 mm/min. Axial depth 0.3 mm on the floor, radial 0.2 mm on the walls, two passes to remove the 0.5 mm stock. The chip stays above the edge radius, so the tool cuts the whole way and the floor finish comes from the sharp edge, not from a slow feed.

Pass	rpm	Feed, mm/min	Axial depth, mm	Radial depth, mm
Roughing	1200	380	12	3.6
Finishing	1450	290	0.3	0.2

From here the shop adjusts. If the chip comes off blue and the edge craters, it drops the speed by 10 to 15 % before it touches the feed. If the wall shows a rubbed, shiny band, the feed goes up, not down. If the corners chatter, the radial step comes down and the tool gets a larger corner radius.

What this means for your RFQ

None of this changes what shows up on your drawing, but it explains why an Invar 36 quote includes more machine time than the same geometry in steel, covered in why Invar 36 parts cost more, and why a shop with Invar experience asks about tolerances before it commits to a cutting strategy. A part that needs a fine finish or a tight position gets a slower finishing pass after stress relief than one that only needs to fit. The sequence is summarized on the Invar 36 machining page.

The parameters are the shop’s job. Your job is to give the shop what it needs to pick them: the alloy and spec, for example Invar 36 to ASTM F1684, the heat treatment sequence or “shop to recommend”, the surface finish on critical faces, the tolerances that control function and any thin walls or deep pockets that limit the tool. If a feature is hard to reach or awkward to fixture, say so. A shop that machines Invar regularly can often suggest a sequence that holds the tolerance without adding passes.

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

Frequently asked questions

Reviewed against

• Wikipedia, Invar
• ASTM F1684, Standard Specification for Iron-Nickel and Iron-Nickel-Cobalt Alloys for Low Thermal Expansion Applications

Values in this guide are typical handbook figures for planning. The mill certificate for your heat lot and the shop's quote for your geometry govern.

Keep reading

• Why Invar Work-Hardens and How Shops Control It During Machining · Materials
• Invar Milling Strategy: Toolpaths That Avoid Work Hardening · Process
• CNC Turning Invar 36: Live Tooling, Chip Control and Setup · Process
• Invar Drilling and Tapping: Hole Quality and Thread Practices · Process

All process guides