We use technical and security cookies and, only if you accept, analytics with no cross-site tracking. More in the Cookie policy and Privacy policy.
We use first-party cookies and technical storage to make the site work, Google reCAPTCHA security technology and, only if you accept, Vercel analytics (no cookies, no cross-site tracking). You can accept or reject analytics; both options are equivalent and you can change your choice at any time. More info: Cookie policy, Privacy policy, Legal notice and Terms and conditions.
Ti-6Al-4V (grade 5) titanium: cutting speed and feed rate
Optimize your machining processes with our online cutting parameters calculator. Select the operation type (turning, milling, drilling or threading) and instantly get the critical calculations for your shop: cutting speed (Vc), revolutions per minute (RPM), feed per revolution or per tooth, machining time and the theoretical roughness (Ra / Rz) based on the insert nose radius. To fine-tune those values live at the machine, use the interactive machining calculator.
Cutting calculator
Step 1
Which operation are you machining?
Do you want to adjust these values live?
Here you get the recommendation (Vc, feed, roughness, threading). In the interactive machining calculator you can move Vc, diameter, RPM and feed with linked scales, locks and time/power estimation.
Ti-6Al-4V turns and mills at 40-80 m/min (about 130-260 SFM) with 0.15 mm/rev or 0.06 mm per tooth, drills at 28-60 m/min with 0.08 mm/rev and taps at 14-36 m/min. Those speeds look brutally low next to steel and there is no shortcut: titanium conducts heat so poorly that everything you generate stays at the edge. The golden rule is constant feed plus coolant that genuinely reaches the cut.
EN Ti-6Al-4V · Grade 5 · 330 HB · ISO group S
Recommended speeds and feeds
Operation
Vc (m/min)
Feed
Shop note
Turning
40–80
0.15 mm/rev
40-80 m/min at 0.15 mm/rev, fine-grain carbide either uncoated or with a thin PVD coating, and high pressure coolant aimed right at the edge. Keep the nose radius and lead angle small to lower the temperature in the contact zone.
Milling
40–80
0.06 mm/tooth
40-80 m/min with 0.06 mm per tooth and a trochoidal strategy: light radial engagement, deep axial cuts and a short arc of contact so each flute has time to cool before it comes round again. Solid carbide cutters with many flutes and variable pitch.
Drilling
28–60
0.08 mm/rev
28-60 m/min at 0.08 mm/rev and uninterrupted feed to the bottom. Stop the drill in the hole and titanium hardens the floor, after which the drill never cuts again: it just rubs until it breaks.
Threading
14–36
0.08 mm/rev
14-36 m/min. Tapping titanium is delicate: drill for 60-65% thread engagement, coated carbide tap and high pressure lubrication. On expensive parts, thread mill - a broken tap in a titanium part usually means scrapping it.
Starting values for coated carbide in medium cutting. Fine-tune them in the calculator for your tool, type of pass and safety margin.
How it behaves when cutting
Ti-6Al-4V runs around 330 HB and its thermal conductivity is about one sixth that of steel, so heat does not leave with the chip: it concentrates at the tool tip and degrades it chemically. Titanium is also reactive at high temperature and welds readily to the edge, and its low elastic modulus lets the part push away from the tool and spring back, producing chatter and uneven chip thickness. The chip comes off in thin, very hot segments that can ignite if allowed to pile up. All of that forces a different approach: low speed, committed feed and high pressure coolant.
The heat has nowhere to go: why Vc is so low
In steel, a good share of the heat leaves with the chip. In titanium it does not: thermal conductivity is so low that heat accumulates at the edge, which can pass 1,000 degrees in ordinary cuts. At that temperature titanium reacts with the tool material and the edge degrades by diffusion, not abrasion. Hence the 40-80 m/min window, and hence the fact that pushing it 20% can halve tool life. Productivity does not come from surface speed here, it comes from depth of cut and feed, both of which can stay high.
Never let the edge dwell: notching and work hardening
Titanium work hardens, and its signature wear is a notch right on the depth of cut line, where the edge meets the outside surface. Any moment the tool turns without feeding, any accidental dwell, leaves a hardened zone that tears the edge apart later. In turning, vary the depth of cut between successive passes so the notch never forms in the same place, and always exit under feed. In drilling and tapping the rule is identical: continuous entry, continuous exit, and never stop the motion with the tool inside the material.
Rigidity, chatter and chip safety
The elastic modulus of Ti-6Al-4V is roughly half that of steel, so the part yields under cutting force and springs back, which means chatter, especially on thin walls and long overhangs. Keep tool overhang to a minimum, clamp as close to the cut as you can, and use variable-pitch cutters. There is also a genuine safety issue: fine titanium chips burn. Do not let chips pile up in the pan or machine dry with nests of swarf around the job, and keep the coolant running - besides cooling, it stops hot chips finding enough oxygen.
Quick shop tips
High pressure coolant aimed at the edge: in titanium it is the single biggest contributor to tool life.
Never stop the feed with the tool in contact; titanium hardens and the edge is ground away on the next pass.
Buy time with depth of cut and feed, not surface speed: past 80 m/min tool life falls off a cliff.
Vary the depth of cut between passes so the notch does not form on the same line every time.
Minimum overhang and clamping close to the cut: titanium yields under the tool and chatters easily.
Do not let fine titanium chips accumulate in the machine; they burn, and running coolant cuts that risk a long way.
Frequently Asked Questions (FAQ)
Why is the cutting speed for titanium so low?
Because its thermal conductivity is about six times lower than steel and the heat stays at the edge, which degrades by chemical diffusion. That is why the range is 40-80 m/min, and why in titanium you gain productivity with feed and depth of cut rather than rpm.
What Vc do I use on Ti-6Al-4V with HSS tooling?
Around 14-28 m/min, and only with plenty of lubrication. HSS loses hardness in exactly the temperature range titanium works in, so life is very short; for anything repetitive you need fine-grain carbide.
Why do my drills break in titanium?
Almost always from stopping the feed inside the hole or letting chips pack in the flute. Drill at 28-60 m/min with a continuous 0.08 mm/rev feed, high pressure through-coolant, and no pauses until you break through.
Coated or uncoated tooling in titanium?
Fine-grain uncoated carbide with a very sharp edge works very well, especially in milling. If you do coat, use a thin PVD such as AlTiN or AlCrN; thick coatings round the edge, and in titanium a dull edge means heat and notching.
Does Ti-6Al-4V machine like Inconel 718?
They share low thermal conductivity and work hardening, but Inconel is considerably worse: its turning range is 20-50 m/min against 40-80 for titanium, and it keeps its hardness hot. Run titanium parameters in Inconel and the edge is gone in minutes.
