Machining Cutting Parameters
Machining quotes rarely disagree because the arithmetic is wrong; they disagree because nobody can say what cutting data the part should run at. This page puts turning, milling and drilling side by side — speed, feed and depth of cut for eight common materials — and adds the feed limits behind each Ra target and which coolant belongs where. Every row says what fails outside the range: tool life, surface finish, or that stainless habit of getting harder the more you cut it.
Cutting data moves with machine rigidity, holder overhang, cutter grade and cooling. The values below are a digest of common handbook ranges: general starting points, not mandatory clauses. Final numbers come from a trial cut and the cutter supplier's recommendation. The references at the foot of the page cover cutting data and metal cutting principles — they are not the basis for one particular machine's set points.
1. Turning: continuous cutting, so speed can run high
Turning is continuous, edge temperature is steady, which is why a lathe can use a step more speed than a mill on the same material. Separate three things first: cutting speed vc (m/min, sets edge temperature and tool life), feed f (mm/rev, sets surface roughness and chip thickness) and depth of cut ap (mm, sets cutting force and machine load). They cannot all be maxed at once — that is the root of every "the parameters will not dial in" story.
| Material | Rough vc m/min | Finish vc m/min | Feed f rough / finish mm/rev | Depth ap rough / finish mm | What fails outside the range |
|---|---|---|---|---|---|
| Aluminium 6061 | 250–500 | 350–700 | 0.15–0.35 / 0.05–0.12 | 1–4 / 0.2–1 | Too slow builds a built-up edge and tears the surface; too fast welds chips onto the insert |
| Aluminium 7075 | 200–450 | 300–600 | 0.15–0.35 / 0.05–0.12 | 1–3 / 0.2–1 | Zinc-bearing 7075 runs one step below 6061, otherwise flank wear climbs quickly |
| Carbon steel 45# | 120–200 | 200–300 | 0.2–0.4 / 0.08–0.15 | 1.5–4 / 0.2–1 | Too fast gives crater wear and drifting dimensions; too slow gives a built-up edge and poor Ra |
| Stainless 304 | 60–120 | 100–180 | 0.1–0.25 / 0.05–0.12 | 1–3 / 0.2–0.8 | Too fast burns the edge; too light a feed rubs the surface and grows the work-hardened layer |
| Brass H62 | 250–450 | 300–600 | 0.15–0.35 / 0.05–0.12 | 1–4 / 0.2–1 | With too little rake the chip jams at the edge — chatter and a dug-in finish. Brass does not need high speed to finish well |
| POM | 250–500 | 400–700 | 0.1–0.3 / 0.05–0.12 | 1–3 / 0.2–0.8 | A dull edge friction-melts the chip into stringers on the part; cool with air, never with emulsion |
| ABS | 200–400 | 300–600 | 0.1–0.3 / 0.05–0.1 | 1–3 / 0.2–0.8 | Too slow actually sticks; too light a feed heats by friction and leaves a melted edge |
| Titanium TC4 | 30–60 | 40–80 | 0.1–0.2 / 0.05–0.1 | 0.5–2 / 0.2–0.5 | Too fast puts all the heat in the edge and burns it in seconds; too slow rubs the hardened layer and burns it just as fast |
The handbook gives cutting speed; the machine takes rpm: n = 1000 × vc ÷ (π × D). A Ø50 carbon steel part at 150 m/min roughs at about 955 rpm; the same row on a Ø10 part means 4,775 rpm — nearly a five-fold difference from one line of a table, and the first place "just copy the table" goes wrong.
Speed and tool life are not linear. Taylor's equation gives carbide an exponent near 0.25, so a 20% speed increase roughly halves tool life. That conversion decides which of the two lines in machining cost — machine time or tooling — climbs first. A quote that raised rpm without looking at tool cost usually starts overspending in the third week of production.
2. Milling: interrupted cutting, so both speed and radial engagement give way
Every revolution runs entry, cut, exit and air cooling. The edge sees impact fatigue, so milling speed sits a step below turning on the same material, and radial (ae) and axial (ap) engagement are set as fractions of cutter diameter: ae at 0.3D loads the cutter gently and lasts; the shop that raises ae to raise removal rate pays first in chatter, then in chipped flutes.
| Material | Cutting speed vc m/min | Feed per tooth fz mm/z | Radial ae | Axial ap | What fails outside the range |
|---|---|---|---|---|---|
| Aluminium 6061 | 300–600 | 0.05–0.15 | 0.3–0.6 D | 0.5–1.0 D | Too much radial engagement starves chip evacuation and the cutter re-cuts its own chips |
| Aluminium 7075 | 250–500 | 0.05–0.12 | 0.3–0.5 D | 0.4–0.8 D | One step down from 6061; multiply by 0.7 again on long overhangs |
| Carbon steel 45# | 100–180 | 0.03–0.08 | 0.2–0.5 D | 0.3–0.8 D | Too small a feed per tooth burnishes instead of cutting and shortens tool life — the most common false economy |
| Stainless 304 | 50–100 | 0.02–0.05 | 0.15–0.3 D | 0.2–0.5 D | Keep the cutter moving: every pause leaves a hardened layer at that spot and the next pass cannot bite |
| Brass H62 | 250–500 | 0.05–0.12 | 0.3–0.6 D | 0.5–1.0 D | Brass grabs: climb milling pulls the cutter into the work, so reduce feed per tooth on machines with backlash |
| POM | 300–600 | 0.08–0.2 | 0.4–0.7 D | 0.5–1.0 D | Chip evacuation is the whole problem in slots — chips that cannot leave melt onto the wall, so take shallower, layered passes |
| ABS | 250–500 | 0.08–0.2 | 0.4–0.7 D | 0.5–1.0 D | High rpm friction heats the cut, which goes white and brittle; use single- or two-flute aluminium-style cutters |
| Titanium TC4 | 30–60 | 0.02–0.05 | 0.1–0.25 D | 0.2–0.5 D | Flood coolant through the tool is mandatory and conventional milling is out; at higher speeds the cutter fails in seconds and titanium chips can ignite |
Feed rate F = fz × flutes z × rpm n. A four-flute Ø10 end mill in carbon steel at 120 m/min and fz 0.05 gives n ≈ 3,820 rpm and F ≈ 764 mm/min. Dropping fz below 0.03 is not "safer": the chip gets thinner than the edge radius, the cutter rubs instead of cutting, and tool life halves. It is the most common false economy on a shop floor.
HSS cutters run at roughly half to a third of carbide speed on the same material; coated grades (TiAlN and friends) take another step up in steel. When unsure, start at 70%–80% of the cutter supplier's recommendation rather than at the top of a handbook range.
3. Drilling: the lowest speeds, and chip evacuation above all
Drilling is enclosed cutting: chips leave through two flutes and coolant struggles to reach the edge. Speeds are therefore the lowest of the three operations, and pecking matters more than the numbers — a deep hole without retraction grinds its own chips in the flutes until the drill snaps.
| Material | Drill / cutting speed m/min | Feed f mm/rev | Deep hole | What fails outside the range |
|---|---|---|---|---|
| Aluminium 6061 | 60–100 (150–250 carbide) | 0.15–0.25 | Peck to clear chips; through-tool coolant for deep holes | Too heavy a feed jams the drill and the flutes scratch the bore on retraction |
| Carbon steel 45# | 20–30 (60–90 carbide) | 0.1–0.2 | L/D > 3: cut 10%–15% per extra diameter | Too fast burns the point and the hole closes in; too slow rubs the bottom and burrs the exit |
| Stainless 304 | 8–15 (cobalt HSS 12–18) | 0.08–0.15 | L/D > 3: cut 20% and peck every pass | The real problem is work hardening: a hole not drilled in one go often cannot be entered again |
| Brass H62 | 60–100 | 0.15–0.3 | Peck to avoid self-feeding | Brass screws itself into the work: too heavy a feed chips the entry and snaps the drill |
| POM | 60–120 | 0.15–0.3 | Peck frequently, air cooling | Chips wrap the drill, friction melts the wall and the hole ends up undersized |
| ABS | 60–120 | 0.15–0.3 | Peck frequently, air cooling | Above the softening point the hole entry collapses — most visible on clear parts |
| Titanium TC4 | 8–15 (carbide) | 0.05–0.12 | Through-tool coolant; never let the drill idle in the hole | Titanium conducts heat poorly, so it all stays at the edge: two or three seconds of rubbing destroys the point |
Feed per revolution also scales with drill diameter: below Ø3 use 0.05–0.1 mm/rev, around Ø6 use 0.1–0.15, above Ø12 up to 0.2–0.3. Applying one figure to a small drill snaps it; to a large drill it clogs. Drilling time follows depth and peck count, which the manual machining time tool estimates from hole count and depth.
4. Surface finish and coolant: fix Ra, then fix feed
Roughness is not produced by a slow last pass; it comes from feed and nose radius: theoretical scallop Ra ≈ f² ÷ (8R) × 1000 (f in mm/rev, R in mm). At Ra 0.8, once f passes 0.1 the cut cannot deliver it, and the rest is grinding or polishing — cost that has to be added as a separate operation instead of being hidden inside the turning rate.
| Target / case | Turning feed f mm/rev | Tool and nose | Cooling | What goes wrong |
|---|---|---|---|---|
| Ra 0.8 | ≤ 0.1 | R0.4 nose radius + wiper | Emulsion, flood | Above f 0.1 the theoretical scallop already exceeds 0.8 µm; polishing to rescue it moves the cost to a second operation |
| Ra 1.6 | ≤ 0.2 | R0.4 nose radius | Emulsion | This is the economical turning grade; quoting Ra 1.6 and delivering Ra 3.2 is the most common mismatch on quotes |
| Ra 3.2 | ≤ 0.35 | R0.4–R0.8 nose radius | Emulsion, or dry for cast iron | Roughing grade; for milling also watch feed per tooth and cutter runout |
| Carbon / alloy steel | — | Coated carbide (PVD/CVD) | Emulsion at 5%–10%, aimed at the edge | When concentration drops the first symptom is dimensional drift, not finish |
| Stainless / superalloys | — | Cobalt HSS or tough carbide grades | High flow, high pressure; never interrupt the coolant | Interrupted cooling thermal-shocks the edge until it chips |
| Aluminium alloys | — | Sharp, high-rake, polished flutes | Emulsion or kerosene; avoid sulphur EP additives (they stain the part) | Aluminium welds onto the edge as speed rises — poor cooling builds a built-up edge fast |
| Cast iron | — | Carbide, dry | Dry with extraction; no emulsion (graphite sludge) | Wet cutting turns graphite dust into mud that blocks flutes and filters |
| Titanium | — | Uncoated fine-grain carbide | High-pressure through-tool; no chlorine-bearing fluids | Titanium chips are flammable: clear them off the machine instead of letting them pile up |
| Engineering plastics | — | Single- or two-flute aluminium cutters, sharp edge | Air blast or MQL; no conventional emulsion | Plastics absorb water — dimensions and properties shift, and emulsion invites stress cracking |
The wrong coolant costs more than the wrong feed: wet cutting cast iron turns graphite into sludge that blocks flutes; sulphur EP additives stain aluminium; chlorine-bearing fluids stress-corrode titanium at temperature; emulsion swells and later stress-cracks plastics. When a tighter finish is needed, book the cost under surface finishing or grinding rather than pressing the turning parameters harder.
How the parameters become cost
- Removal rate → machine cost. Time = removal volume ÷ material removal rate (MRR, cm³/min). A 20% higher MRR cuts machine cost by about 17% (1 ÷ 1.2) — the only near-linear payoff in machining parameters. MRR is proportional to speed × feed × depth; the 40 cm³/min for aluminium 6061 built into the machining cost calculator is a mid-range composite.
- Speed → tool cost. A 20% speed increase roughly halves carbide tool life, doubling tool cost per part. The 17% saved on machine time is easily eaten; judge by the sum of the two lines, not the best of them.
- Ra and coolant → secondary operations. Miss the finish and you add grinding, polishing or lapping; pick the wrong coolant and you add rework and scrap. Both hide in "other" on a quote, which is exactly where they get underestimated.
Machine rate changes the conclusion too: on a machine costing 120 per hour, 20% off the cycle is a real win; on one at 40 per hour, halving tool life for 20% of the cycle usually loses money. How to build the rate is in machine hour rate.
The seven numbers to ask for at quotation
- Material grade and temper (6061-T6 versus 6061-O run at completely different speeds)
- Stock form and allowance (bar, plate or casting — allowance sets the number of roughing passes)
- Cutter grade, diameter and overhang (anything past 3D needs derating, and this is the item most often withheld)
- Speed, feed per rev or per tooth, and depth of cut — separately, not as one "rpm" figure
- Cooling method (flood, through-tool, MQL or dry)
- Number of setups and whether a fixture is needed (setup is spread over the batch; on small batches it dominates)
- Ra acceptance and the gauge (visual comparator or profilometer)
A supplier who can answer all seven is usually cutting to the numbers; one who cannot is quoting an experience-based guess. For the full cost structure, start from process selection to check the part belongs in machining at all, and look unfamiliar terms up in the glossary.
Four common mistakes
- Putting cutting speed straight into the machine. Handbooks give m/min, machines take rpm; Ø50 and Ø10 differ five-fold. Get it wrong and you burn an edge — or crash.
- Running stainless on steel parameters. 304 work-hardens hard: too light a feed rubs the surface, the hardened layer deepens, and the second pass cannot bite. The fix is enough feed to keep the edge under the hardened layer, not slower and slower cutting.
- Assuming slower is safer. Titanium and stainless burn edges at low speed too — the edge rubs the hardened layer and all the heat stays in it. Titanium wants low speed, sufficient feed and high-flow coolant together; two out of three is not enough.
- Watching speed and ignoring overhang and rigidity. Stretching overhang from 2D to 4D often costs 30% of usable speed. Skip that and you get chatter, regular marks, and hand polishing to rescue it.
Frequently asked questions
The ranges are wide — which end do I start from?
Start in the lower-middle of the roughing band, step up 10%–15% per trial until finish or tool life fails first, then back off one notch and record the set. That trial ladder beats any table because it describes your machine.
Why does stainless want a heavier feed rather than a slow grind?
The work-hardened layer in stainless runs 0.1–0.3 mm deep. With too light a feed the edge only scrapes that layer and the layer deepens every revolution. Keeping feed high enough to cut beneath it is the only stable approach — which is why 304 has a floor of about 0.02 mm/tooth.
The same block turns to Ra 1.6 but mills worse — why?
Milled scallop height depends on feed per tooth and nose radius together, and every tooth takes an entry shock while runout multiplies the effective profile height. Getting Ra 1.6 from a milled face usually needs small feed per tooth, high rpm and a finishing cutter — or grinding instead.
Plastics have no tool life problem, so can I run any rpm?
No. Plastics fail by friction heating: high rpm, a dull edge and a light feed all pile heat into the cut and give melted edges, whitening and stress cracks. Go for a sharp edge, moderate speed, sufficient feed and air cooling — see the last two rows of the turning table.
Related: CNC machining cost calculator · Machine hour rate · Manual machining time · Surface finishing cost · Process selection · Glossary
References
- Concise Handbook of Cutting Parameters 机械工业出版社 · ISBN 978-7-111-05418-1
- Machinery's Handbook (31st ed.) Industrial Press · ISBN 978-0-8311-3631-1
Basis for the parameters above. Links go to the publisher or its search page; the standard text itself is sold by the publisher. Price references are public market ranges, not supplier quotations.