42CrMo4 / 4140 alloy 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.

Open interactive calculator →

42CrMo4 turns at 150-240 m/min (about 490-790 SFM) with 0.25 mm/rev of feed, drills at 105-180 m/min and taps at 53-108 m/min, always on coated carbide. It is a chrome-moly steel supplied quenched and tempered at around 280 HB, and its behaviour shifts noticeably with every point of hardness. Before you program anything, find out what hardness the bar actually is.

EN 42CrMo4 / 1.7225 · AISI 4140 · 280 HB · ISO group P

Recommended speeds and feeds

Operation	Vc (m/min)	Feed	Shop note
Turning	150–240	0.25 mm/rev	At 280 HB run 180-220 m/min with 0.25 mm/rev on a tough substrate; if the bar is above 310 HB drop to 150 m/min and switch to a geometry with a negative land, because at that hardness a sharp edge simply crumbles.
Milling	150–240	0.09 mm/tooth	Mill at 150-240 m/min with 0.09 mm per tooth, always climb milling and trochoidal in pockets: 42CrMo4 is tough enough to break insert corners every time a tooth enters with chip thickness building up from zero.
Drilling	105–180	0.16 mm/rev	105-180 m/min with a carbide drill and decent through-coolant pressure; HSS is a miserable experience here (35-60 m/min and fast corner wear), and the point should be 140 degrees so the drill does not skate on entry.
Threading	53–108	0.16 mm/rev	53-108 m/min, and forget form tapping: at 280 HB the material will not flow enough and the roll tap bursts. Use a coated carbide cut tap or, better, a thread mill, which does not scrap the part if it breaks.

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

42CrMo4 normally ships quenched and tempered, 280 HB nominal, though the same grade can turn up anywhere from 250 to 340 HB depending on the temper. That hardness plus the toughness of chrome-moly means high cutting forces and a lot of heat concentrated right at the edge. The chip is short and hard, so chip control is easy, but it abrades the rake face and craters it at the same time. Once hardness climbs past 300 HB you start seeing plastic deformation of the edge, which is the polite way of saying the insert nose is being squashed flat.

Real hardness beats any table

42CrMo4 is not one material, it is a family of conditions. The same part number can arrive at 250 HB with a high temper or 340 HB tempered for strength, and between those extremes the right cutting speed varies by more than 40%. Check it with a portable tester before you set up a run, or at least take a test pass and watch: violet-blue chips and a high-pitched note mean you are over-speeding it. As a rule of thumb, take about 10 m/min off for every 10 HB above 280, and reinforce the edge with a land instead of cutting feed.

Plastic deformation: the classic failure here

When you push 42CrMo4 too hard, the insert nose does not wear - it squashes. Heat and pressure together soften the substrate, the edge loses its geometry, and parts start drifting oversize while the finish degrades gradually rather than failing suddenly. The tell is a rounded, shiny nose, sometimes with a blue tint on the top face. Cure it with a more heat-resistant carbide substrate, an AlTiN coating, plenty of coolant aimed at the edge, and speed pulled back towards 150-180 m/min - not by touching the feed.

Workholding and cutting force on big parts

42CrMo4 shows up in drive shafts, crankshafts, spindles and heavy sections, and on that kind of work cutting force is the real limit. A 4 mm depth of cut at 0.25 mm/rev and 280 HB demands power and flawless clamping: let the part move a tenth and the insert breaks. Before you raise parameters, check the chuck, the overhang and the tailstock. In milling, a trochoidal path with small radial engagement and deep axial cuts spreads wear along the whole flute length, so you can hold speed without frying the corner.

Quick shop tips

Measure the bar's real hardness before programming: 260 HB and 330 HB are a world apart in cutting speed.
If the insert nose comes out rounded and shiny rather than worn, that is plastic deformation: pull speed, not feed.
No form taps in hardened and tempered 42CrMo4: the material will not flow and the tap snaps in the hole.
In milling, always enter on a ramp or an arc; a straight full-width entry chips insert corners in this steel.
Reinforce the edge with a negative land before you reduce feed once hardness goes past 300 HB.
For drilling, a carbide drill with through-coolant pays for itself against HSS by about the second hole.

Frequently Asked Questions (FAQ)

What cutting speed do I use on 42CrMo4 at 320 HB?

Stay at the bottom of the range, around 150 m/min turning, with a reinforced-edge insert and plenty of coolant. Above 300 HB the failure mode shifts from wear to plastic deformation, and speed is the variable that triggers it.

Can I drill 42CrMo4 with an HSS drill?

You can, at 35-60 m/min with generous coolant, but drill life is short and the corners round off quickly. Past a couple of holes, a through-coolant carbide drill at 105-180 m/min works out cheaper.

Which coating works best on 42CrMo4?

PVD AlTiN for anything with impact (milling, interrupted cuts) and CVD with an aluminium-oxide layer for continuous turning at speed. What matters is hot hardness: in this steel the edge works well above 800 degrees.

How do I tap 42CrMo4 without breaking taps?

Tap drill for 60% thread engagement, a coated carbide tap, speed inside the 53-108 m/min range and coolant that actually reaches the bottom. In a blind hole, a thread mill is the safe choice because it cannot get trapped if something goes wrong.

Are 42CrMo4 and 4140 the same steel?

Yes, EN 42CrMo4 / 1.7225 is the equivalent of AISI 4140. For picking cutting parameters they are interchangeable; what you need to compare is the supply condition and the hardness, not the designation.

Similar materials

C45 / 1045 steel: cutting speed and feed rate

Speeds and feeds for C45 / AISI 1045 steel: Vc and feed per operation, and how much changes when the bar arrives quenched and tempered, not normalised.

16MnCr5 case hardening steel: cutting speed and feed rate

Cutting speed and feed for 16MnCr5 by operation, with the grinding stock and the precautions a case hardening steel needs before it ever sees the furnace.

Hardened steel 50-55 HRC: cutting speed and feed rate

Cutting speed and feed in hardened 50-55 HRC steel: Vc per operation, CBN and ceramic inserts, and the light passes and rigidity that hard turning needs.

Related tools

RPM, feeds and machining time calculator

Calculate cutting speed, RPM, feeds and pass time for milling, turning and drilling. Adjust values with linked scales and look up starting values by material.

Calculate cycle time

Estimate CNC turning and milling cycle time from G-code. Calculate parts per hour with a breakdown of cutting, rapids, canned cycles and tool changes.

Machining quote

Instant machining quote: material, machine time, setup per batch, secondary operations and margin. Free, no sign-up.