CNC Feed & Speed Starting Ranges
Starting cutting-speed and feed ranges for aluminum 6061, 1018 and 1045 steel, 304 and 316 stainless, Ti-6Al-4V, and C360 brass.
These are starting points, not limits. In the five most common CNC alloys, published cutting-speed ranges differ by a factor of four between a general carbide chart and a modern coated solid-carbide chart for the same metal. The table below pulls those published ranges into one place and names the tooling behind each one. The rest of the page covers how a shop tunes away from them. For how the processes themselves work, see CNC machining and CNC milling.
What feed and speed mean
Two numbers drive everything a control runs. Cutting speed (vc) is how fast the cutting edge passes through the material, in surface meters per minute (m/min) or surface feet per minute (SFM). Feed per tooth (fz) is the thickness of chip each edge removes on its pass, stated in millimeters per tooth for milling and millimeters per revolution (fn) for drilling and turning.
Turning speed and feed into machine numbers
Spindle speed comes from cutting speed and cutter diameter: n = vc x 1000 / (pi x Dc). Table feed comes from feed per tooth, tooth count, and spindle speed: vf = fz x z x n. RobbJack publishes the same arithmetic in imperial form, RPM = SFM x 3.82 / tool diameter, with feed rate = RPM x chip load per tooth x number of flutes.
A worked example shows the scale. A 10mm four-flute carbide end mill in 6061 at 300 m/min runs at 300 x 1000 / (3.14 x 10), which is 9554 rpm. At fz 0.05 mm/tooth the table feed is 0.05 x 4 x 9554, or 1911 mm/min. Run the RobbJack formula on a chart-real diameter and the practical catch shows: 6061 at SFM 1000 on Harvey Tool’s smallest chart diameter, 1/8in, asks for 1000 x 3.82 / 0.125, about 30,560 rpm, which no shop spindle delivers. When the arithmetic outruns the spindle, radial engagement and depth of cut have to carry the load instead of speed.
Reading the starting ranges
Each range spans published charts from at least two tooling manufacturers, and every row names its source. Start at the low end of both the speed range and the feed range, make a cut, then tune.
Why the published ranges are wide
The spread between manufacturers is real, not carelessness. Sandvik Coromant lists wrought aluminum alloys (CMC 30.12) at 680 to 1140 m/min depending on radial engagement, because a coated solid carbide taking a light cut carries far more speed. Harvey Tool lists 6061-T6 at 800 to 1500 SFM, which is 244 to 457 m/min. Both describe a real tool honestly. The table shows the span of both so a reader can see the whole published range and then judge where their own tool sits inside it.
Engagement moves speed as much as coating does. Sandvik’s own sheet gives one aluminum alloy three speeds: 680 m/min at full-width slotting, 835 m/min at half the cutter width, 950 m/min at a tenth of it. Same tool, same metal, three answers.
How to adjust from the starting point
Machine rigidity, workholding, tool overhang, coolant pressure and through-spindle delivery, toolpath strategy, and tool wear all move the right answer away from any printed chart. Two habits keep the adjustment safe.
Chip load thinking
The chip has to be thick enough to cut rather than rub. RobbJack puts it plainly: too light rubs and work-hardens the cut, too heavy overloads the edge. For titanium the same source gives chip load per tooth as tool diameter x 0.0048, so a 10mm cutter in Ti-6Al-4V wants about 0.048mm per tooth. That agrees with Sandvik’s 0.046 mm/tooth for titanium alloys at a 10mm cutter. Stainless needs the same treatment for a different reason: a feed too light to cut cleanly rides on the work-hardened skin and wears the tool out fast.
When to cut the numbers back
Drop speed and feed together for deep slots, thin walls, long reach, and anything that chatters. RobbJack’s trochoidal guidance for slots gives the shape of it: tool about half the slot width, axial depth 1.5 to 2 diameters, and radial engagement of 3 to 10 percent of diameter in difficult alloys against 25 to 50 percent in non-ferrous work. Titanium and austenitic stainless have the narrowest workable window of the five materials here, so change one parameter at a time and in small steps.
Face milling and turning
Face milling and turning run on the same cutting-speed logic with one change: a turning insert usually presents a single edge, so turning works in feed per revolution, while a face mill states feed per tooth across the inserts in the cutter. The public OEM charts we could verify cover all five materials only for end milling and drilling, so this section carries sourced worked examples for face milling and turning rather than an invented grid. Read them as illustrations of a complete parameter set from a named tooling maker, not as starting ranges and not as limits.
| Operation and material | Cutting speed | Feed | Setup behind the number |
|---|---|---|---|
| Face milling, unalloyed steel CMC 01.2, HB180 (Sandvik Coromant) | 270 to 325 m/min at HB150 across chip thickness 0.10 to 0.20mm; worked set 262 m/min at 0.17mm | fz 0.24 mm/tooth | 125mm cutter, 8 teeth, 45 degree entering angle, 667 rpm, 1281 mm/min |
| Face milling, grey cast iron GG20 (Mitsubishi Materials) | 125 m/min | fz 0.25 mm/tooth | 200mm cutter, 16 inserts, 200 rpm, 800 mm/min |
| Turning, mild steel | 120 m/min, Mitsubishi Materials | fn 0.2 mm/rev at 3mm depth, Mitsubishi Materials | Specific cutting force 3100 MPa and 4.65 kW required power at 80 percent efficiency (net cutting power about 3.7 kW), Sandvik Coromant Metalcutting Technical Guide |
| Drilling, alloy steel (Mitsubishi Materials) | 50 m/min | fn 0.15 mm/rev | 15mm drill, 1062 rpm |
Sandvik’s guide also shows how far hardness shifts a published speed. The chart values span 270 to 325 m/min at HB150, roughly 283 m/min at 0.17mm chip, and the HB180 correction factor of about 0.92 takes that to about 260 m/min; the worked set in the table runs 262 m/min, the same correction carried into its 667 rpm and 1281 mm/min figures (n = 262 x 1000 / (pi x 125)). A change of 30 Brinell moves the answer by eight percent, which is one reason a printed chart is only ever a first guess. For the lathe side of the same logic, see CNC turning.
Limits of this table
This is starting guidance only. Nothing here is a capability claim about any shop, and none of these numbers is a limit in either direction: a rigid machine with good coolant and a fresh coated tool often runs well above the top of a published range, and a worn tool in a marginal setup can fail below the bottom of one. Confirm against the tooling manufacturer’s own data for the specific tool, coating, and diameter before cutting, and give titanium and austenitic stainless the smallest steps. For what a finished part can hold dimensionally, see the CNC tolerances reference table.
About this data
- Methodology
- Starting-point guidance only, not limits and not a capability claim for any shop. End-milling values are for solid carbide end mills and span two tooling manufacturers: Harvey Tool General Machining Guidelines (SFM by material, chip load per tooth at 1/4in and 1/2in diameters) and Sandvik Coromant CoroMill Dura cutting data (vc in m/min by CMC material group and radial engagement, feed per tooth by cutter diameter). Drilling values come from Guhring speed and feed charts and span tool classes as the rows state: series 551 and 552 are HSS-class twist drills, series 546 is solid carbide. Where the two sources disagree, the published span of both is shown rather than one number. Feed values are quoted for a 10mm cutter or a 6 to 10mm drill; published feed per tooth rises with diameter. Ranges were read from the manufacturers charts in August 2026.
- Sources
- Sandvik Coromant CoroMill Dura cutting data: CMC 01.2 unalloyed steel, 02.2 low-alloyed steel, 05.21 austenitic stainless, 23.22 titanium alloys, 30.12 aluminum alloys, 33.2 copper and copper alloys; vc across ae 1.0 to 0.1 x DC and the finishing table; fz codes F01 to F08 at DC 10mm.
- Harvey Tool General Machining Guidelines: 6061-T6/T651 800 to 1500 SFM, 10XX steels 100 to 300 SFM, austenitic 100 to 350 SFM as the union of two chart rows (304 and 316 at 100 to 250; a second row including 200 series and 316L at 100 to 350), 6Al-4V 50 to 250 SFM, high-lead brass 800 to 1500 SFM, with chip load per tooth at 1/4in and 1/2in.
- Guhring speed and feed charts for drills: series 552 (295 SFM wrought aluminum, 115/90 SFM structural steels, 145 SFM long-chipping brass) and series 546 carbide (575 SFM wrought aluminum, 50 SFM austenitic stainless, 50 SFM titanium, 490 SFM short-chipping brass), feed per revolution by drill diameter.
- How to read this
- Find the material and the operation, then start at the low end of both the speed range and the feed range and tune upward on chip form, sound, and tool wear. These are starting points from tooling manufacturers charts, not limits and not a promise about any machine or shop.
| material | operation | cutting speed vc | equivalent SFM | feed starting point | tooling and source basis |
|---|---|---|---|---|---|
| Aluminum 6061 | End milling, solid carbide | 244 to 1140 m/min | 800 to 3740 | fz 0.05 to 0.08 mm/tooth (0.002 to 0.003in) on a 10mm cutter | Harvey Tool 800 to 1500 SFM for 6061-T6; Sandvik Coromant CMC 30.12, 680 to 1140 m/min |
| Aluminum 6061 | Drilling, twist drill to solid carbide | 90 to 175 m/min | 295 to 575 | fn 0.25 to 0.32 mm/rev (0.010 to 0.0125in/rev) on a 6 to 10mm drill | Guhring series 552 twist drill 295 SFM in wrought aluminum; series 546 carbide 575 SFM |
| Carbon steel 1018 and 1045 | End milling, solid carbide | 30 to 366 m/min | 100 to 1200 | fz 0.04 to 0.08 mm/tooth (0.0015 to 0.003in) on a 10mm cutter | Harvey Tool 100 to 300 SFM for 10XX steels; Sandvik Coromant CMC 01.2, 145 to 366 m/min |
| Carbon steel 1018 and 1045 | Drilling, HSS-class twist drill | 27 to 35 m/min | 90 to 115 | fn 0.20 to 0.25 mm/rev (0.008 to 0.010in/rev) on a 6 to 10mm drill | Guhring series 552, structural and free-cutting steels: 115 SFM under 150 BHN, 90 SFM under 32 HRC |
| Stainless 304 and 316 | End milling, solid carbide | 30 to 220 m/min | 100 to 722 | fz 0.013 to 0.08 mm/tooth (0.0005 to 0.003in) on a 10mm cutter | Harvey Tool 100 to 350 SFM across its two austenitic rows (100 to 250 for 304 and 316); Sandvik Coromant CMC 05.21, 70 to 220 m/min |
| Stainless 304 and 316 | Drilling, solid carbide | 15 m/min | 50 | fn 0.13 mm/rev (0.005in/rev) on a 6 to 10mm drill | Guhring series 546 carbide, austenitic stainless under 36 HRC |
| Titanium Ti-6Al-4V | End milling, solid carbide | 15 to 120 m/min | 50 to 394 | fz 0.013 to 0.046 mm/tooth (0.0005 to 0.0018in) on a 10mm cutter | Harvey Tool 50 to 250 SFM; Sandvik Coromant CMC 23.22, 105 to 120 m/min; RobbJack about 230 SFM |
| Titanium Ti-6Al-4V | Drilling, solid carbide | 15 m/min | 50 | fn 0.076 mm/rev (0.003in/rev) on a 6 to 10mm drill | Guhring series 546 carbide, titanium alloys under 43 HRC |
| Brass C360 | End milling, solid carbide | 130 to 457 m/min | 426 to 1500 | fz 0.05 to 0.08 mm/tooth (0.002 to 0.003in) on a 10mm cutter | Harvey Tool 800 to 1500 SFM for high-lead brass; Sandvik Coromant CMC 33.2 copper alloys, 130 to 294 m/min |
| Brass C360 | Drilling, twist drill to solid carbide | 44 to 149 m/min | 145 to 490 | fn 0.17 to 0.20 mm/rev (0.0065 to 0.008in/rev) on a 6 to 10mm drill | Guhring series 552 long-chipping brass 145 SFM; series 546 short-chipping brass 490 SFM |
Frequently asked questions
Are these feed and speed values limits?
Why does the same material show such a wide range?
Which end of the range should I start at?
What is chip load and why does it matter?
How do I turn a cutting speed into a spindle speed?
Do these numbers apply to face milling and turning?
Why is titanium so much slower than steel?
Does feed change with tool diameter?
Sources
Last reviewed: 2026-08-16