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.
16MnCr5 case hardening steel: 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.
16MnCr5 turns at 160-250 m/min (about 525-820 SFM) with 0.25 mm/rev, mills in the same window at 0.09 mm per tooth, drills at 112-188 m/min and taps at 56-113 m/min. It is the gear and splined-shaft steel, machined soft at around 210 HB and then carburised and quenched. Everything you program has to allow for that second life in the furnace.
EN 16MnCr5 / 1.7131 · AISI 5115 · 210 HB · ISO group P
Recommended speeds and feeds
Operation
Vc (m/min)
Feed
Shop note
Turning
160–250
0.25 mm/rev
160-250 m/min with 0.25 mm/rev and a positive insert with a polished edge; working below 120 m/min in this steel is the fastest route to built-up edge and a surface that will not case harden evenly afterwards.
Milling
160–250
0.09 mm/tooth
160-250 m/min at 0.09 mm per tooth. When roughing gear teeth, spread the wear by avoiding repeated passes at the same radial depth: the chromium abrades, and the notch forms in exactly the same spot every time.
Drilling
112–188
0.16 mm/rev
112-188 m/min with 0.16 mm/rev. On holes that get carburised afterwards, leave stock or mask them: an H7 hole finished before heat treatment closes up and hardens, and then only grinding or EDM will save it.
Threading
56–113
0.16 mm/rev
56-113 m/min. Always thread before carburising, and protect the thread with stop-off paint or leave stock to be removed later; a thread carburised to 60 HRC is brittle and will not tolerate so much as a chase with a tap.
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
With just 0.16% carbon plus manganese and chromium, 16MnCr5 is more ductile than its 210 HB suggests. Chips come off long and slightly gummy, with a tendency to build up on the edge at low speed like any low-carbon steel. The chromium adds some abrasiveness, so insert flank wear runs faster than in C45 at the same speed. It leaves a substantial burr on exit edges and, above all, it holds internal stress that is released during carburising and quenching, moving the part.
Grinding stock for heat treatment: the forgotten allowance
16MnCr5 is carburised and quenched after machining, and in that process the part changes both size and shape. A gear can grow a tenth or two and go out of flat, and a long shaft bows. That is why functional surfaces get grinding stock, typically 0.2 to 0.4 mm on diameter depending on size and geometry, and why critical dimensions are only signed off after heat treatment. Machining to final size in the soft state is the classic beginner's mistake with this material: the part leaves the lathe perfect and comes out of the furnace out of tolerance.
Built-up edge and the surface you take into the furnace
At 0.16% carbon, 16MnCr5 sticks to the tool if you run slow. Built-up edge does not only ruin the finish: it leaves an uneven surface that carburises unevenly and can give you variable case hardness. Work the top half of the range, 200 to 250 m/min, with a positive sharp geometry and feed above 0.15 mm/rev, and use plenty of coolant. If you see welded material on the rake face when you index, raise the speed before you change anything else.
Internal stress and the order of operations
Case hardening steel accumulates rolling and machining stress that the quench releases all at once. On thin-walled or strongly asymmetric parts it pays to rough, let the part rest, or even stress relieve in between, and only then finish. Sequence matters: rough everything first, then finish, rather than completing one feature before you touch the next. On shafts with keyways or splines, cutting the slot last reduces later distortion, because every cut that breaks the symmetry of the section is an invitation for the part to move in the furnace.
Quick shop tips
Leave 0.2-0.4 mm of grinding stock on surfaces you will grind after hardening; the part grows and distorts in the furnace.
Cut the threads before carburising and mask them: a carburised thread is brittle and cannot be chased.
If chips weld on and the finish tears, push the speed towards 200-250 m/min instead of cutting the feed.
Rough the whole part before finishing any feature, so the stress is released before you go to size.
On precision holes that get carburised, leave stock and finish them after heat treatment.
Expect slightly faster flank wear: the chromium in this steel abrades more than a plain carbon steel.
Frequently Asked Questions (FAQ)
Do you machine 16MnCr5 before or after case hardening?
Before, in the soft condition at around 210 HB. After carburising the surface sits at 58-62 HRC and only grinding or CBN tooling will touch it, so all conventional machining is done beforehand with stock left on.
How much grinding stock do I leave for after hardening?
As a guide, 0.2 to 0.4 mm on diameter for medium-sized parts, more on long or asymmetric parts that distort further. Confirm it with whoever runs the heat treatment, because it depends on case depth and quench method.
What Vc do I use on 16MnCr5 with an HSS end mill?
Around 55-90 m/min, a third of the carbide range. With a 12 mm HSS cutter that is roughly 1,500-2,400 rpm; keep feed per tooth above 0.05 mm so the edge cuts instead of rubbing.
Why do my 16MnCr5 gears come out of tolerance after hardening?
Because carburising and quenching change both size and form. The answer is not in the soft machining but in leaving grinding stock, stress relieving between roughing and finishing, and using an operation order that does not break the part's symmetry at the end.
Can I use 42CrMo4 parameters on 16MnCr5?
They are close, but 16MnCr5 is softer (210 HB against 280 HB) and takes more speed: 160-250 m/min against 150-240. The bigger practical difference is that 16MnCr5 forms built-up edge and 42CrMo4 does not.
