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.
CuZn39Pb3 brass: 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.
CuZn39Pb3 brass turns and mills at 200-500 m/min (about 650-1,640 SFM) with 0.2 mm/rev or 0.1 mm per tooth, drills at 140-375 m/min with 0.2 mm/rev and taps at 70-225 m/min. It is the benchmark for machinability: chips break themselves into small pieces and tool wear is almost an afterthought. The one real problem with brass is that it grabs the tool and pulls it in.
EN CW614N · CuZn39Pb3 · 110 HB · ISO group N
Recommended speeds and feeds
Operation
Vc (m/min)
Feed
Shop note
Turning
200–500
0.2 mm/rev
200-500 m/min at 0.2 mm/rev with a neutral or slightly negative geometry; very positive aluminium inserts dig in and leave chatter marks. The chip breaks on its own, so the chipbreaker hardly matters.
Milling
200–500
0.1 mm/tooth
200-500 m/min with 0.1 mm per tooth and 3 or 4 flute cutters. Brass takes high feeds without hurting the finish, and because the chip is short you do not need the huge gullets aluminium demands.
Drilling
140–375
0.2 mm/rev
140-375 m/min at 0.2 mm/rev with a brass-specific drill, its rake dubbed off on the cutting lips: a standard drill self-feeds, grabs and can lift the part out of the vice or snap.
Threading
70–225
0.2 mm/rev
70-225 m/min. Brass taps beautifully with a straight-flute cut tap and needs almost no lubricant, but forget form tapping: the lead makes the material insufficiently ductile and the rolled thread comes out cracked.
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
The lead in free-machining brass does not dissolve in the matrix: it sits as fine particles that act as an internal lubricant and a built-in chipbreaker, so the chip fractures into short flakes with no special geometry needed. At 110 HB, cutting forces are low and the edge barely wears. The odd behaviour shows up with very positive tooling: brass is so soft and cuts with so little resistance that the tool tends to dig in and self-feed, especially a drill, which screws itself into the hole and grabs. Lead-free brasses, increasingly common under drinking water rules, behave very differently: gummy and sticky.
The drill that grabs: the signature brass defect
It is the classic surprise for anyone drilling brass for the first time with a standard steel drill. Near breakout the drill screws itself into the material, self-feeds and grabs: the part spins in the vice, the hole comes out triangular, or the drill snaps. It happens because a standard drill's rake angle is far too positive for a material that offers so little resistance. The fix is to stone that rake back on the cutting lips until the face is practically at zero degrees, or simply buy drills ground for brass. And clamp the part properly, always.
Leaded and lead-free brass: not the same job
Traditional CuZn39Pb3 is the industry's machinability benchmark, but drinking water regulations have pushed work towards lead-free and low-lead alloys containing silicon or bismuth. Without lead's chipbreaking effect, those brasses produce long gummy chips, stick to the edge and demand lower speeds with sharper geometries and better evacuation. If a program that ran perfectly suddenly throws bird's nests and a poor finish, check the material designation before you touch anything: odds are your supplier switched to a lead-free alloy.
Finish, tolerance and screw machine work
Brass gives bright finishes in a single pass and very tight tolerances, because cutting forces are minimal and the part barely deflects or heats up. That is why it is the benchmark material for screw machine work: fittings, bushings, valves and connectors hold size over thousands of parts. The one thing worth watching is the internal burr in cross-holes and grooves, which in brass is thin and razor sharp and stays inside the part unless deburring is planned. On hydraulic parts, that burr ends up in the customer's valve.
Quick shop tips
Dub off the drill's rake or buy a brass-specific drill: a standard grind self-feeds and grabs.
Avoid very positive aluminium geometries when turning; brass digs in and leaves chatter marks.
If the material changed to lead-free brass, expect long chips, adhesion and a lower speed.
Brass gives a bright finish in one pass: do not take a spring cut, you do not need it.
Plan for internal deburring in cross-holes; brass burrs are thin, sharp and stay inside the part.
Do not use form taps: leaded brass is not ductile and the rolled thread comes out cracked.
Frequently Asked Questions (FAQ)
Why does my drill grab and dig in when drilling brass?
Because a standard drill's rake angle is far too positive for such a soft material: the drill self-feeds and screws itself in. Stone the lip faces back to near zero degrees, or use a drill ground specifically for brass.
What cutting speed do I use on brass with HSS?
Between 70 and 175 m/min, a third of the carbide range. Brass is so unabrasive that HSS holds up very well, and on form tooling in screw machine work it remains a classic combination that still works.
Does brass need coolant?
Very little. It can be machined practically dry or with minimum lubrication, because the lead acts as an internal lubricant and cutting forces are low. A coolant stream mainly helps wash the short chips out of the working area.
Why does lead-free brass machine so much worse?
Because lead was what fragmented the chip and lubricated the cut. Without it the alloy is ductile and gummy: chips stretch out, stick to the edge, and you have to drop the speed and use sharper geometries with better evacuation.
Can I use brass parameters on bronze or copper?
No. Bronze is harder and more abrasive, and pure copper is extremely ductile and sticky, nothing like leaded brass. CuZn39Pb3 is an exceptionally favourable case among copper alloys.
