Guides /

Milling Inconel and nickel alloys: end mill speeds and feeds

Published carbide end mill SFM and chip load for Inconel 718 and 625, Hastelloy, Waspaloy, Monel, Incoloy and A-286 from Harvey Tool, 6GTools, MariTool and Sandvik Coromant, plus work hardening, minimum chip thickness, coolant, flute count and worked examples.

Nickel alloys are where a feeds and speeds chart stops being a suggestion. Harvey Performance describes them as materials that work harden, keep heat in the cutting zone instead of carrying it off in the chip, and make gummy chips that weld to the cutting edge as built-up edge [4]. Sandvik Coromant, writing about heat resistant super alloys (HRSA) for jet engine parts, adds that cutting speeds are generally low and that the tool must keep a real chip going to avoid hardening the surface it will cut next [5].

The published numbers are low and they cluster. Harvey Tool's general guidelines put Inconel 718, Hastelloy, Waspaloy and Rene alloys at 40-60 SFM and Inconel 600/625, Monel and pure nickel at 45-100 SFM [1]. 6GTools gives 100 SFM for uncoated carbide in Inconel 625 and 718 [2], and MariTool charts its TiAlN-coated fine-pitch rougher at 60 SFM in 625/718 [3]. Sandvik Coromant gives solid carbide a much wider window of 30-100 m/min, about 98-328 SFM, which for 8-16 mm cutters means roughly 4,000 down to 600 RPM, and says carbide inserts are normally limited to about 40 m/min [5]. The top of Sandvik's window comes from high-speed machining with a very small radial step, not from conventional slotting (see the last worked example).

Bars are published SFM ranges, open dots single published values. Sandvik values converted from m/min (1 m/min = 3.28 SFM). The 328 SFM point is a Sandvik tool-life test at 0.5 mm radial engagement in 42 HRC Inconel 718. Cobalt-base alloys are not charted: Harvey lists two cobalt-base rows at 40-80 and 60-100 SFM [1], and 6GTools gives Stellite 100 SFM [2]. Sources [1]-[3], [5].

Quick reference by alloy

Alloy group (Harvey row)	Harvey SFM [1]	Harvey chip load, 1/4" / 1/2" [1]	Other published SFM	Notes from the sources
Inconel 718, X, W; Hastelloy C, B, X; Waspaloy; Rene 41-95	40-60	.001 / .002	100 uncoated, 625/718 [2]; 60 TiAlN rougher, 625/718 at 280-320 Bhn [3]	The slowest group in Harvey's table. Sandvik's 718 tests were on 42 HRC material [5].
Inconel 600, 625; Nickel 200-270; Monel 400-405	45-100	.001 / .002	100 uncoated, 625 [2]	Sandvik: solution-treated nickel alloys such as Inconel 625 usually machine easier than nickel- and cobalt-based superalloys [5].
A-286, Haynes 556 (iron-base)	50-80	.001 / .002		Sandvik: iron-based superalloys also machine easier [5].
Incoloy 600-802	80-100	.001 / .002	125 uncoated, Incoloy 800-802 [2]	Harvey's 3/8" chip load here is .0015, vs .001 for the nickel rows [1].

Chip load by diameter

Published chip load per tooth for Inconel 718. Harvey Tool's nickel and iron-base rows share the same chip loads except at 3/8" [1]. 6GTools lists the same chip loads for all its high-temperature alloy rows [2]. MariTool's values are for a 1 x D slot with its 4-flute rougher [3]. The diamond is Sandvik's fz 0.05 mm (.002") for a high-speed, light-radial cut in 42 HRC 718, plotted at 10 mm [5].

At 1/2" the three tables nearly agree: .002 in/tooth from Harvey and 6GTools and .0018 from MariTool's slotting chart [1]-[3]. At 1/4" they spread from .0006 (MariTool) to .0012 (6GTools), and at 1/8" every source is at or below .0005 [1]-[3]. MariTool says its numbers assume a 1 x D slot, that profiling cuts up to 2 x D deep and .25 x D wide can run higher feed and speed below .25 x D radial, and that long-flute roughers should come down 10-20% in SFM and 30-60% in feed per tooth [3].

Work hardening and minimum chip thickness

Sandvik's milling advice for super alloys is to combine a fairly low cutting speed with a moderately high feed per tooth, aiming for a chip thickness of not less than 0.1 mm (about .004") to prevent work hardening, a target written mainly for indexable cutters [5]. Small solid end mills can't carry a chip that thick (Harvey's 1/2" value is .002 [1]), but the principle carries over: don't reduce the feed to "be gentle". A tool that rubs instead of cutting hardens the surface it has to cut next. Sandvik also calls for down (climb) milling, so the chip is thinnest where the edge exits and is less likely to stick, sharp edges with optimized edge rounding, and as many teeth in the cut as stability allows [5]. Harvey also recommends climb milling and a coated tool [4].

When the radial step drops, the actual chip gets thinner than the programmed feed per tooth. 6GTools publishes multipliers for this: 1.0 at 50% radial, 1.1 at 30%, 1.2 at 20%, 1.4 at 15%, 1.8 at 10%, 2.3 at 5% and 5.0 at 1% [2]. Harvey ties chip thinning correction directly to reducing rubbing [6]. See the chip thinning guide.

Coolant

Harvey Performance calls high-pressure coolant of 1,000 psi or more mandatory for nickel alloys and prefers water-based fluids [4]. Sandvik recommends generous coolant at the edge when cutting speeds are low, to reduce chip adhesion, through-spindle coolant for HRSA, and says high-pressure coolant gives better tool life [5]. Sandvik's flank wear limits are 0.2 mm for its R390 inserts and 0.3 mm for round carbide inserts, past which the chance of a catastrophic failure rises rapidly [5].

How many flutes?

The sources disagree here. Harvey Performance recommends higher flute counts in nickel alloys: 6 or more flutes for traditional roughing and 8 flutes for finishing and high-efficiency milling, with variable-pitch geometry [4]. Sandvik's tool-life test in 42 HRC Inconel 718 (100 m/min, 10 mm axial, 0.5 mm radial, fz 0.05 mm) found four flutes optimum for 8-12 mm cutters, and warns that extra-close multi-flute end mills like those used in hardened steel are not recommended, because Inconel's sticky chips can clog the flutes and break the tool [5]. Harvey's high flute counts are paired with high-efficiency, light-radial toolpaths and high-pressure coolant [4], so match the flute count to the toolpath and coolant you actually have. See also choosing flute count.

Worked example: 1/2" 4-flute carbide in Inconel 718, Harvey numbers

50 SFM (middle of Harvey's 40-60): 50 × 3.82 ÷ 0.5 = 382 RPM, and 382 × 4 × .002 = 3.1 IPM [1]. That feed looks alarmingly slow next to steel, and it's meant to.

Worked example: same tool, 6GTools numbers at 10% radial

100 SFM uncoated: 100 × 3.82 ÷ 0.5 = 764 RPM, and at a 50% step 764 × 4 × .002 = 6.1 IPM [2]. Drop the step to 10% (0.05") and the 1.8 multiplier gives .0036 in/tooth programmed, so 764 × 4 × .0036 = 11.0 IPM for the same actual chip [2].

Worked example: 1/2" fine-pitch rougher slotting 625 or 718

MariTool 1010 at 60 SFM: 60 × 3.82 ÷ 0.5 = 458 RPM, and 458 × 4 × .0018 = 3.3 IPM in a 1 x D slot [3]. With a long-flute version, MariTool says to cut SFM 10-20% and feed per tooth 30-60% [3].

Worked example: Sandvik's high-speed test conditions on a 10 mm end mill

Sandvik's flute-count test ran 100 m/min, fz 0.05 mm, 10 mm axial and 0.5 mm radial [5]. On a 10 mm 4-flute cutter that is 100,000 ÷ (π × 10) = 3,183 RPM and 3,183 × 4 × 0.05 = 637 mm/min (about 25 IPM), at about 328 SFM. That is far faster than the conventional tables because the radial step is only 5% of the diameter; the cutter spends most of each revolution out of the cut and cooling.

FAQ

What SFM should I use to mill Inconel 718 with a carbide end mill?

Harvey Tool lists 40-60 SFM for Inconel 718 (with Hastelloy, Waspaloy and Rene alloys). 6GTools gives 100 SFM for uncoated carbide in Inconel 625/718, and MariTool charts its TiAlN fine-pitch rougher at 60 SFM in 625/718. Sandvik Coromant gives 30-100 m/min (about 98-328 SFM) for solid carbide in heat resistant super alloys, and its high-speed test in 42 HRC Inconel 718 ran 100 m/min with only 0.5 mm radial engagement.

What chip load should I use for a 1/2" end mill in Inconel?

Harvey Tool and 6GTools both list .002 in/tooth at 1/2" diameter (Harvey .001 at 1/4"; 6GTools .0012). MariTool lists .0018 for its 1/2" rougher in a 1 x D slot. 6GTools raises chip load as radial engagement drops, by 1.8x at 10% and 2.3x at 5%, to correct for chip thinning.

Why does Inconel work harden when I mill it?

Harvey Performance says nickel alloys work harden, hold heat in the cut and make gummy chips that weld to the edge. Sandvik Coromant recommends a fairly low cutting speed with a moderately high feed per tooth, so the chip is not too thin, to prevent work hardening, and climb milling for the thinnest chip at the exit. Light, rubbing cuts and dwelling make it worse.

Should I use coolant when milling Inconel?

Yes. Harvey Performance calls high-pressure coolant (1,000 psi or more) mandatory for nickel alloys and prefers water-based fluids. Sandvik Coromant recommends generous coolant at the edge, through-spindle coolant for heat resistant super alloys, and says high-pressure coolant gives better tool life.

End mill calculator Chip thinning math

Related guides

Tooling for this job

Amazon links are affiliate links. As an Amazon Associate I earn from qualifying purchases.