CNC Cutting Parameters by Material
Cutting speed, feed and depth of cut for turning and milling eight CNC materials with carbide inserts, plus coolant and depth-of-cut strategy each one needs.
Turning — cutting speed, feed and depth of cut (carbide inserts)
| Material and condition | Cutting speed (m/min) | Feed (mm/rev) | DOC roughing (mm) | DOC finishing (mm) | Coolant | Source |
|---|---|---|---|---|---|---|
| Aluminum 6061-T6 (wrought, heat-treatable, ~95 HB) | 300–1000 | 0.1–0.3 | 0.5–3.0 | 0.2–0.5 | Flood emulsion, high volume | S4 — ISCAR ISOTURN P25 (wrought hardenable) |
| Aluminum 7075-T6 (wrought, heat-treatable, ~150 HB) | 300–1000 | 0.1–0.3 | 0.5–3.0 | 0.2–0.5 | Flood emulsion, high volume | S4 — ISCAR ISOTURN P25 (lower half of the range for 7075) |
| Aluminum 6061 / 7075 (PCD tooling, reference row) | 600–2500 | 0.1–0.3 | 0.05–0.3 | 0.05–0.2 | Flood or oil mist | S4 — ISCAR ISOTURN P31 (PCD column) |
| Carbon steel 1045 (180–280 HB) | 160–275 | 0.4–1.2 | 2.0–8.0 | 0.3–1.0 (est.) | Emulsion | S3 — Mitsubishi B045, P group (UE6110 / MC6025) |
| Alloy steel 4140 (180–280 HB, quenched and tempered) | 160–275 | 0.4–1.2 | 2.0–10.0 | 0.3–1.0 (est.) | Emulsion | S3 — Mitsubishi B045, P group |
| Stainless 304 (≤200 HB) | 75–140 | 0.4–1.1 | 1.5–8.0 | 0.3–1.0 (est.) | Flood emulsion, high volume | S3 — Mitsubishi B045, M group (US735) |
| Stainless 316 (≤200 HB) | 75–140 | 0.4–1.1 | 1.5–8.0 | 0.3–1.0 (est.) | Flood emulsion, high volume | S3 — Mitsubishi B045, M group |
| Titanium Ti-6Al-4V (annealed, ~33–36 HRC) | 40–60 | 0.20–0.40 | 1.0–3.0 | 0.3–0.8 | High-pressure coolant (HPC) — mandatory, not optional | Sandvik titanium machining guidance (~60 m/min roughing); Machinery's Handbook 27 ed., Table 7 (29–76 m/min at 0.20–0.43 mm/rev) |
| Brass C36000 (free-cutting, ~90 HB) | 180–400 | 0.1–0.3 | 0.5–3.0 | 0.2–0.5 | Dry or minimal oil mist | S4 — ISCAR ISOTURN P25 (brass column) |
| Brass C36000 (PCD tooling, reference row) | 600–800 | 0.1–0.3 | 0.05–0.3 | 0.05–0.2 | Dry or oil mist | S4 — ISCAR ISOTURN P31 (PCD column) |
How to read this table. All values are carbide. The speed and feed bands come from heavy-cutting insert catalogues (the ap 1.5–12 mm roughing class), so take the lower-middle of the range for a conventional roughing pass and the finishing column for the last pass. Values marked (est.) have no citable catalogue table — they are shop experience, kept separate from the sourced numbers.
Face Milling (Carbide)
Feed per tooth is quoted for a Ø12 mm cutter (the source chart lists the 1/2 in column); scale it with cutter diameter for other sizes. Depths marked ×DC are the source's proportion-of-cutter-diameter figures converted to mm — treat them as fractions of your cutter, not as absolute limits.
| Material | Cutting speed (m/min) | Feed per tooth (mm, Ø12) | DOC roughing (mm) | DOC finishing (mm) | Coolant | Source |
|---|---|---|---|---|---|---|
| Aluminum 6061-T6 / 7075-T6 | 244+ (from 800 SFM) | 0.15–0.19 | 1.0–3.0 | 0.3–0.5 | Flood or MQL | S1 — Data Flute, Aluminum 6061/7075 column |
| Carbon steel 1045 | 61–137 | 0.076 | 1.0–3.0 (×DC) | 0.3–0.5 (×DC) | Emulsion | S1 — Data Flute, carbon steels <32 Rc |
| Alloy steel 4140 | 46–91 | 0.064 | 1.0–2.5 (×DC) | 0.3–0.5 (×DC) | Emulsion | S1 — Data Flute, alloy steel 40XX/41XX |
| Stainless 304 / 316 | 46–107 | 0.071 | 1.0–2.5 (×DC) | 0.3–0.5 (×DC) | Flood emulsion, high volume | S1 — Data Flute, stainless 300 series |
| Titanium Ti-6Al-4V | 43–61 | 0.064 | 0.5–1.5 | 0.2–0.5 | High-pressure coolant (HPC) | S1 — Data Flute, titanium cast/wrought 6AL4V |
| Titanium Ti-6Al-4V (IC830 face mill, reference row) | 51–55 | 0.13–0.18 | 1.5 | — | High-pressure coolant (HPC) | S5 — ISCAR Machining Titanium p32 (Vc=55, Km=1, Ke=0.92) |
| Brass C36000 | 152–274 | 0.165 | 1.0–3.0 (×DC) | 0.3–0.5 (×DC) | Dry or oil mist | S1 — Data Flute, brass (yellow/red/leaded) |
End Milling (Carbide)
Chip load is the Ø12 mm reference value; the depth-of-cut cells keep the source's ×D wording on purpose, because the mm figure only holds for a 12 mm cutter. On a 6 mm cutter the 0.3×D ceiling is 1.8 mm, not 3.6 mm.
| Material | Cutting speed (m/min) | Feed per tooth (mm, Ø12) | DOC roughing (mm) | DOC finishing (mm) | Coolant | Source |
|---|---|---|---|---|---|---|
| Aluminum 6061-T6 / 7075-T6 | 244+ | 0.19 (HP) / 0.29 (finishing) | ≤0.3×D ≈ 3.6 | ≤0.05×D ≈ 0.6 | Flood or MQL | S1 + S2 (depth-of-cut basis S2) |
| Carbon steel 1045 | 61–137 | 0.076 | ≤0.3×D ≈ 3.6 | ≤0.05×D ≈ 0.6 | Emulsion | S1 + S2 |
| Alloy steel 4140 | 46–91 | 0.064 | ≤0.3×D ≈ 3.6 | ≤0.05×D ≈ 0.6 | Emulsion | S1 + S2 |
| Stainless 304 / 316 | 46–107 | 0.071 | ≤0.2×D ≈ 2.4 | ≤0.05×D ≈ 0.6 | Flood emulsion, high volume | S1 + S2 |
| Titanium Ti-6Al-4V | 43–61 | 0.064 | ≤0.15×D ≈ 1.8 | ≤0.05×D ≈ 0.6 | High-pressure coolant (HPC) | S1 + S5 |
| Brass C36000 | 152–274 | 0.165 | ≤0.3×D ≈ 3.6 | ≤0.05×D ≈ 0.6 | Dry or oil mist | S1 |
Two Valid Speed Bands — Do Not Average Them
For stainless and carbon steel the two sources disagree by a factor of 2–4. Both are correct for their own strategy: the lower band is the tool-life-first shop value at a deep engagement, the higher band is the coated-insert value at a shallow engagement. Quote the band that matches your depth of cut.
| Case | Vc (m/min) | Feed per tooth (mm, Ø12) | DOC strategy | Applies when | Source |
|---|---|---|---|---|---|
| End milling, stainless 304/316 (US/EU shop basis) | 46–107 | 0.071 | ≤0.2×D | Solid carbide end mill, heavy roughing, tool life first | S1 (SSDH/MH-RO, 150–350 SFM) |
| End milling, stainless 304/316 (Japanese insert basis) | 100–200 (nominal 150) | 0.2 (≤0.4) | ≤0.05×D | VP15TF coated insert, shallow depth, high rpm, stable setup | S2 — Mitsubishi SRF/SUF |
| End milling, carbon steel 1045 (US/EU shop basis) | 61–137 | 0.076 | ≤0.3×D | Solid carbide end mill, tool life first | S1 |
| End milling, carbon steel (Japanese insert basis) | 80–300 (nominal 200) | — | ≤0.05×D | Coated insert, shallow depth, high rpm | S2 — Mitsubishi SRF/SUF |
How to Use These Numbers
- For Ti-6Al-4V the coolant is a precondition, not an option: the 43–61 m/min window only holds under high-pressure coolant or heavy flood. Cut dry and the insert craters and the surface burns within 30 seconds, with tool life commonly down more than 50%.
- Do not apply steel depth-of-cut logic to aluminium: at 244+ m/min and 0.15–0.19 mm per tooth (Ø12), a face-milling roughing pass of 1–3 mm is limited by spindle power and chip evacuation, not by tool life. Use a 2–3 flute polished-flute cutter with flood coolant.
- The two stainless speed bands pair with two different depths: 46–107 m/min at ap ≤ 0.2×D, 100–200 m/min at ap ≤ 0.05×D. Pairing the high band with a deep cut chips the edge.
- Every value in these tables is carbide. HSS runs at roughly 30–50% of the carbide speed (1045 turning 160–275 → about 50–90 m/min; 6061 milling 244+ → about 80–120 m/min). That conversion is shop convention, not catalogue data, so keep HSS figures out of the carbide table.
- C36000 cuts dry at 152–274 m/min and 0.165 mm per tooth (Ø12), but it contains more than 1% lead — fit dust extraction for dry cutting, and move to a lead-free copper alloy (e.g. C27450) at the lower end of the speed band when food or medical compliance applies.
Frequently Asked Questions
What cutting speed should I use for turning 6061 aluminum?
300–1,000 m/min with carbide inserts, and 600–2,500 m/min with PCD tooling. Take the lower half of the band for 7075 and for interrupted cuts.
300–1,000 m/min with carbide inserts, and 600–2,500 m/min with PCD tooling. Take the lower half of the band for 7075 and for interrupted cuts.
What feed rate for turning 304 stainless steel?
0.4–1.1 mm/rev at 75–140 m/min, with flood emulsion at high volume. That feed band comes from heavy-cutting inserts; take the lower half on a lighter setup.
0.4–1.1 mm/rev at 75–140 m/min, with flood emulsion at high volume. That feed band comes from heavy-cutting inserts; take the lower half on a lighter setup.
How deep can I rough-turn 4140 steel?
2–10 mm depth of cut at 160–275 m/min with heavy-cutting carbide inserts, at feeds of 0.4–1.2 mm/rev.
2–10 mm depth of cut at 160–275 m/min with heavy-cutting carbide inserts, at feeds of 0.4–1.2 mm/rev.
What cutting speed for milling Ti-6Al-4V?
43–61 m/min with carbide end mills (51–55 m/min with an IC830 face mill), and high-pressure coolant is mandatory — the speed window does not exist without it.
43–61 m/min with carbide end mills (51–55 m/min with an IC830 face mill), and high-pressure coolant is mandatory — the speed window does not exist without it.
What chip load for a 12 mm carbide end mill in 1045 steel?
About 0.076 mm per tooth (0.003 in/tooth) at 61–137 m/min. Scale the chip load with cutter diameter when you change size.
About 0.076 mm per tooth (0.003 in/tooth) at 61–137 m/min. Scale the chip load with cutter diameter when you change size.
Why do two sources give different speeds for 304 stainless?
46–107 m/min is the tool-life-first shop value for a solid carbide end mill at 0.2×D depth of cut; 100–200 m/min is the coated-insert value at 0.05×D depth of cut. Use the band that matches your depth strategy — do not average them.
46–107 m/min is the tool-life-first shop value for a solid carbide end mill at 0.2×D depth of cut; 100–200 m/min is the coated-insert value at 0.05×D depth of cut. Use the band that matches your depth strategy — do not average them.
Can I machine C36000 brass without coolant?
Yes: 152–274 m/min milling (180–400 m/min turning) and 0.165 mm per tooth on a Ø12 cutter, dry or with minimum-quantity lubrication — with dust extraction, because C36000 contains more than 1% lead.
Yes: 152–274 m/min milling (180–400 m/min turning) and 0.165 mm per tooth on a Ø12 cutter, dry or with minimum-quantity lubrication — with dust extraction, because C36000 contains more than 1% lead.
What depth of cut for finishing 6061 aluminum?
Keep the finishing pass at or below 0.05 × tool diameter — 0.6 mm on a 12 mm cutter. In turning, the finishing band is 0.2–0.5 mm.
Keep the finishing pass at or below 0.05 × tool diameter — 0.6 mm on a 12 mm cutter. In turning, the finishing band is 0.2–0.5 mm.
Standards & Sources
- S1 — Data Flute, Technical Document, feeds and speeds chart (per-tooth chip load by diameter); source units SFM and inch/tooth, converted with m/min = SFM × 0.3048 and mm/tooth = inch × 25.4
- S2 — Mitsubishi Carbide, B065 SRF/SUF end mill, recommended cutting conditions
- S3 — Mitsubishi Carbide, B045 heavy-cutting inserts, recommended cutting conditions (heavy roughing class: ap 1.5–12 mm, f 0.4–1.3 mm/rev)
- S4 — ISCAR, ALUMINUM MACHINING catalogue, ISOTURN machining data P25/P28/P31
- S5 — ISCAR, Machining Titanium guide, Ti-6Al-4V milling example (IC830 face mill Vc = 55 m/min; solid carbide end mill 75 m/min)
- Titanium turning speed cross-checked against Sandvik Coromant titanium machining guidance and Machinery's Handbook, 27th edition, Table 7
- Turning finishing depths of cut (0.3–1.0 mm) and the HSS 30–50% conversion are shop estimates, marked (est.) in the tables
Related Pages
- /wiki/tooling/feeds-and-speeds-guide/ — Long-form feeds and speeds guide, including how to convert between rpm and cutting speed
- /wiki/tooling/titanium-machining-guide/ — Titanium machining in detail: heat management, coolant strategy and tool choices
- /wiki/tooling/stainless-steel-machining-guide/ — Stainless steel machining: work hardening and the depth-of-cut decisions behind the two speed bands
- /wiki/reference/thermal-expansion-coefficients/ — Sibling quick table: thermal expansion coefficients for the same materials
- /wiki/reference/material-density/ — Sibling quick table: density for weight and material cost estimates