Speeds and Feeds: Practical Starting Points by Material
Short answer: Start with surface speed, not RPM. For aluminum use 300–500 m/min carbide surface speed and 0.05–0.15 mm/tooth feed; for mild steel 120–180 m/min and 0.05–0.12 mm/tooth; for 304 stainless 60–100 m/min and 0.04–0.10 mm/tooth; for brass 200–350 m/min and 0.05–0.15 mm/tooth; for titanium 30–60 m/min and 0.03–0.08 mm/tooth. Convert to RPM with n = 1000 × Vc ÷ (π × D). Then set depth of cut: roughing 0.5–1.0 × tool diameter radially, finishing 0.2–0.5 mm. These are starting points — dial in with chip color, sound and tool wear.
Every machinist has a speeds and feeds story that ends with a broken tool or a scrapped part. The numbers below are the ones we hand to new programmers on the floor at our Dongguan plant, where four production lines run CNC machining, metal stamping, custom springs and heat sinks under one ISO9001 roof. They are not laws of physics. They are safe, productive starting points that get you into the right neighborhood so you can tune from evidence rather than guesswork.
Why surface speed matters more than RPM
RPM is a machine setting. Surface speed (Vc, in m/min) is what the cutting edge actually experiences. A 6 mm end mill at 10,000 RPM and a 20 mm end mill at 10,000 RPM are doing wildly different things to the material — the small tool is running at roughly 188 m/min, the large one at about 628 m/min. Same spindle speed, three times the thermal load at the edge.
That is why tool catalogs are organized by surface speed. The formula to convert:
n (RPM) = 1000 × Vc ÷ (π × D)
where Vc is surface speed in m/min and D is tool diameter in mm.
Feed, meanwhile, is usually expressed per tooth, because a 3-flute and a 6-flute cutter at the same RPM remove very different amounts of material. Feed rate:
Vf (mm/min) = n × fz × z
where fz is feed per tooth in mm and z is the number of flutes.
The three variables you actually control
1. Cutting speed (Vc) — drives heat and tool life. Too high, the edge breaks down; too low, you get built-up edge and poor finish.
2. Feed per tooth (fz) — drives chip thickness. Too low, the tool rubs and work-hardens the surface; too high, you overload the edge.
3. Depth and width of cut (ap, ae) — drives radial and axial engagement. This is where most shops leave money on the table.
Starting parameters by material
The table below assumes solid carbide tooling, coated for steel and stainless, uncoated or ZrN for aluminum, and good rigid workholding. Treat every number as a starting point.
| Material | Surface speed Vc (m/min) | Feed per tooth fz (mm) | Typical coolant | Notes |
|---|---|---|---|---|
| Aluminum 6061/7075 | 300–500 | 0.05–0.15 | Flood or MQL | High speeds fine; watch chip evacuation |
| Brass / copper alloys | 200–350 | 0.05–0.15 | Flood or dry | Free-machining; tends to grab if fed too light |
| Mild steel (1018, 1045) | 120–180 | 0.05–0.12 | Flood | Coated carbide essential |
| Alloy steel (4140, 4340) | 90–150 | 0.05–0.10 | Flood | Reduce Vc as hardness rises |
| 304 / 316 stainless | 60–100 | 0.04–0.10 | Flood, high pressure | Work-hardens; never dwell |
| Tool steel (D2, H13) | 50–90 | 0.04–0.08 | Flood | Annealed only; consider roughing at lower Vc |
| Titanium Grade 5 (Ti-6Al-4V) | 30–60 | 0.03–0.08 | Flood, high pressure | Heat goes into the tool, not the chip |
| Cast iron | 100–200 | 0.05–0.15 | Dry or air blast | Graphite dust; avoid flood if possible |
For turning, the same surface speed logic applies, but feed is expressed per revolution (mm/rev) rather than per tooth. Typical roughing feeds run 0.2–0.4 mm/rev for aluminum, 0.15–0.3 mm/rev for steel, and 0.1–0.2 mm/rev for stainless and titanium. Finishing passes drop to 0.05–0.15 mm/rev with a 0.4–0.8 mm nose radius.
Depth of cut: the multiplier most people miss
| Operation | Radial engagement (ae) | Axial depth (ap) | When to use |
|---|---|---|---|
| Heavy roughing | 0.5–1.0 × D | 0.5–1.0 × D | Strong setup, high-power spindle |
| Dynamic / trochoidal | 0.05–0.15 × D | 1.0–3.0 × D | Deep pockets, thin walls, hard material |
| Semi-finish | 0.3–0.5 × D | 0.3–0.5 × D | Leaving 0.3–0.5 mm for finish |
| Finish | 0.05–0.1 × D | 0.2–0.5 mm | Surface finish and tolerance control |
If you take one thing from this article: on modern CAM, a light radial engagement with a deep axial cut (trochoidal or dynamic milling) usually beats a heavy radial cut. It spreads tool wear along more of the flute, reduces radial deflection, and lets you run higher feed per tooth. On thin-wall parts this is not a preference, it is a requirement — see our notes on thin-wall machining strategies.
Worked example: 6061 aluminum bracket
Say you are milling a 6061-T6 bracket with a 10 mm, 3-flute carbide end mill, targeting a 0.5 mm finish allowance.
- Choose Vc = 400 m/min.
- n = 1000 × 400 ÷ (π × 10) = 12,730 RPM. If your spindle caps at 10,000, use 10,000 and accept Vc ≈ 314 m/min.
- Choose fz = 0.08 mm.
- Vf = 10,000 × 0.08 × 3 = 2,400 mm/min.
- Roughing: ae = 5 mm (0.5 × D), ap = 5 mm.
- Material removal rate ≈ 5 × 5 × 2,400 = 60,000 mm³/min.
That is a healthy, conservative aluminum cut. If the spindle load meter sits below 60% and the chips are clean and silver, push fz to 0.12 mm and ap to 7 mm. If you hear chatter, reduce ae before you reduce speed.
Worked example: 304 stainless shaft on a lathe
Turning a 40 mm 304 stainless shaft with a coated carbide insert, 0.8 mm nose radius.
- Choose Vc = 80 m/min.
- n = 1000 × 80 ÷ (π × 40) = 637 RPM.
- Roughing feed = 0.25 mm/rev → Vf = 159 mm/min.
- Depth of cut = 2 mm per side.
- Expect work hardening at the surface. Never let the tool dwell — keep the feed constant through the pass.
If the insert fails after 10 minutes, drop Vc to 65 m/min before you change anything else. If it fails after 2 minutes, you are probably running too slow and rubbing, not cutting.
How to tune from the starting point
A starting point is only useful if you have a feedback loop. Use this sequence:
1. Listen. A clean cut sounds steady. Chatter is a rising whine; a dull tool is a low growl.
2. Look at the chips. Aluminum should be bright and curled. Steel should be blue-grey and not dusty. Stainless chips should be short and silver, not long and straw-colored.
3. Check the load meter. Aim for 50–70% spindle load on roughing. Above 85%, back off ae first.
4. Inspect the edge. Flank wear should be even. Cratering means speed is too high. Chipping means feed is too high or the setup is not rigid.
5. Measure the part. If dimensions drift during a run, thermal growth is in play — check coolant delivery before touching the program.
Coolant choice interacts with all of this. High-pressure through-tool coolant transforms stainless and titanium drilling; on aluminum it is often unnecessary. We cover that trade-off in cutting fluid selection for CNC.
Tool holding and rigidity: the hidden variable
You can copy a parameter table exactly and still get chatter, because the table assumes a rigid setup. Tool holder runout of 0.02 mm turns an effective 3-flute cutter into a 1-flute cutter — one edge does most of the work and fails early. Hydraulic and shrink-fit holders hold runout under 0.005 mm, which is often worth more than a 20% speed increase.
The same logic applies to workholding. A part hanging 80 mm out of a vise will deflect long before the tool does. For a deeper treatment, see tool holder selection for precision work.
At BQUQ we machine to ±0.005 mm on our CNC lines, and that tolerance is only achievable when speeds, feeds, tool holding and fixturing are treated as one system rather than four separate settings.
Speeds and feeds for common part families
| Part family | Material | Typical approach |
|---|---|---|
| Heat sink base and fins | Aluminum 6063/6061 | High Vc, low ae, deep ap; air blast often enough |
| Robot end-effector plates | 6061 or 7075 | Trochoidal roughing, 0.3 mm finish allowance |
| Stainless fittings | 304/316 | Low Vc, constant feed, high-pressure coolant |
| Brass gears and bushings | C360 brass | High Vc, avoid too-light feed to prevent grabbing |
| Titanium fasteners | Ti-6Al-4V | Low Vc, sharp edges, generous coolant, short tool life expected |
| Prototype housings | Mixed | Conservative first pass, measure, then optimize |
For parts like these, we run CNC milling for prismatic geometry and CNC turning for rotational features, often on the same order. If you need both plus finishing, our CNC machining service covers the full route from raw stock to inspection.
Frequently Asked Questions
Q: What surface speed should I use for aluminum on a CNC mill?
A: For 6061 and 7075 aluminum with solid carbide tooling, start at 300–500 m/min surface speed and 0.05–0.15 mm per tooth. Aluminum tolerates high speed well, so tool life is usually limited by chip evacuation and built-up edge rather than heat. If chips weld to the flute, increase feed per tooth before reducing speed.
Q: Why does my 304 stainless tool break so quickly?
A: Stainless work-hardens the moment the edge rubs instead of cuts. Keep feed per tooth at 0.04–0.10 mm and never let the tool dwell in the cut. Use coated carbide, high-pressure coolant directed at the edge, and reduce surface speed to 60–100 m/min. If the insert fails within minutes, you are likely running too slow, not too fast.
Q: How do I calculate RPM from surface speed?
A: Use n = 1000 × Vc ÷ (π × D), where Vc is surface speed in m/min and D is tool diameter in mm. For a 12 mm cutter at 350 m/min, that is 1000 × 350 ÷ 37.7, roughly 9,280 RPM. If your spindle cannot reach that, cap the RPM and accept a lower effective surface speed.
Q: Should I use trochoidal milling or conventional roughing?
A: Trochoidal or dynamic milling uses 5–15% radial engagement with axial depth up to 3× tool diameter. It reduces radial deflection, spreads wear along more flute length, and suits thin walls, deep pockets and hard materials. Conventional roughing at 50–100% radial engagement is faster to program and fine for open, rigid parts.
Q: Do these speeds and feeds apply to CNC turning too?
A: Yes for surface speed, but turning feed is per revolution rather than per tooth. Typical roughing feeds are 0.2–0.4 mm/rev for aluminum, 0.15–0.3 for steel, and 0.1–0.2 for stainless and titanium. Finishing drops to 0.05–0.15 mm/rev, usually paired with a 0.4–0.8 mm nose radius for surface finish.
Related Resources
- About BQUQ and our Dongguan production lines: /about/
- CNC machining, turning and milling capabilities: /cnc-machining/
- Industry trends in precision manufacturing: /industry-dynamics/
- Technical articles and machining guides: /bquq-blog/
- Frequently asked questions on quoting and tolerances: /faq/
- Case studies from production programs: /case/
- Request a quote or send drawings: /contact/
Authored by the BQUQ Engineering Team. BQUQ (Dongguan) runs CNC machining (±0.005 mm), metal stamping, custom springs, and heat sink production in one ISO9001 factory. Source-direct from Dongguan, China — quote in 12 hours: sc@bquq.com | WhatsApp +86 13713157787 | www.bquq.com
