C45 / 1045 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 →

C45 steel turns at 180-280 m/min (about 590-920 SFM) with 0.28 mm/rev on coated carbide, drills at 126-210 m/min with 0.18 mm/rev and taps at 63-126 m/min. It is the shaft and machine-part steel, and one of the most cooperative materials in the shop. The one variable that changes the game is delivery condition: normalised and quenched-and-tempered do not cut alike.

EN C45 / 1.0503 · AISI 1045 · 180 HB · ISO group P

Recommended speeds and feeds

OperationVc (m/min)FeedShop note
Turning180–2800.28 mm/rev180-280 m/min at 0.28 mm/rev is the sweet spot for roughing with a CVD-coated insert; if the stock came in quenched and tempered above 220 HB, stay near 180-200 m/min or you will see cratering and plastic deformation of the edge.
Milling180–2800.1 mm/toothUse the same 180-280 m/min window with 0.1 mm per tooth, and climb mill: C45 is tough enough that conventional milling, where each tooth enters rubbing at zero chip thickness, will chip insert corners on you.
Drilling126–2100.18 mm/rev126-210 m/min and 0.18 mm/rev with a carbide drill and through-coolant; past five diameters deep, back the speed off 20% and program pecks, because the hot chip packs into the flute.
Threading63–1260.18 mm/rev63-126 m/min. C45 taps nicely with a cut tap, but it is the material where dropping to 60-65% thread engagement pays off most: you cut the torque by a third and the thread still outlives the bolt going into 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

With 0.45% carbon and around 180 HB, C45 sits right in the sweet spot for machining: enough carbon for the chip to break on its own, not enough hardness to punish the edge. Chips come off segmented and tidy, without the welding tendency of S235. It does generate more heat in the cutting zone than a low-carbon steel, and that heat opens a crater on the rake face if you overspeed it. Quenched and tempered it can reach 250 HB, and then it behaves far more like 42CrMo4 than like a plain carbon steel.

Normalised, cold drawn or Q&T: not the same C45

The same grade can reach you at 170 HB hot-rolled and normalised, 200 HB cold drawn, or 250 HB quenched and tempered, and that spread matters more than any fine tuning of insert grade. If you do not know the condition, check it with a portable hardness tester or take a test pass: dark blue chips and a heavy cut mean you are above 220 HB and need to drop towards the bottom of the range, 180-200 m/min. Q&T stock also pushes cutting forces up, so review the workholding and reduce depth of cut before you touch the feed.

Crater wear: the tell that you are running too fast

In C45 the dominant high-speed wear mode is cratering: a diffusion-worn hollow on the rake face a couple of millimetres behind the edge. When the crater creeps close enough, the edge loses its backing and lets go all at once, usually mid-pass and usually marking the part. Fight it with a thick CVD aluminium-oxide coating, speed in the middle of the range, and coolant aimed where it matters. If you index an insert and see a bright groove on the top face instead of even flank wear, take 30 m/min out.

Finish and tolerance on C45 shafts

C45 is the classic long-shaft material, and there the enemy is deflection, not cutting. Once the length between centres passes ten times the diameter, the part walks away from the tool and you get taper or chatter. Use a tailstock or a steady rest, a small nose radius (0.4 mm) for finishing to cut radial force, and a feed matched to that radius. For Ra 1.6 with a 0.4 mm nose you want around 0.1 mm/rev. And remember the part comes off hot: measure once it has settled, or the tolerance will close up on you as it cools.

Quick shop tips

  • Check the real hardness before you program: normalised and Q&T C45 are 80 HB apart, which is a whole speed range.
  • A bright groove on the insert's rake face is crater wear: pull speed, not feed.
  • Finish long shafts with a 0.4 mm nose radius; a big radius pushes the part away and leaves taper.
  • Let the part cool before measuring the final diameter: C45 comes off a lathe genuinely hot.
  • Tapping C45 by hand or on the machine, drop to 60-65% thread engagement and you will stop snapping taps.

Frequently Asked Questions (FAQ)

What Vc should I use drilling C45 with HSS?

Between 45 and 75 m/min, roughly a third of the carbide range of 126-210 m/min. With a 10 mm HSS drill that is about 1,400-2,400 rpm, and it wants plenty of coolant plus a peck every three diameters.

Does quenched and tempered C45 machine like normalised C45?

No. Q&T can reach 250 HB, so drop towards 180-200 m/min, reduce the depth of cut and use an insert with a reinforced edge. Run normalised parameters on it and the edge deforms plastically within minutes.

Which insert coating works best in C45?

A CVD coating with an aluminium-oxide layer is the roughing standard, because it resists crater wear at speed. For finishing or interrupted cuts, a PVD TiAlN with a sharper edge takes the impact better.

Why do my taps keep breaking in C45?

Excess torque, usually from a tap drill that is too tight. Go from 75% down to 60-65% thread engagement, use a spiral-flute tap in blind holes, and make sure the drilled depth runs two or three pitches past the usable thread.

Are C45, 1045 and F-114 the same material?

Yes, they are equivalent designations for the same medium-carbon steel: EN C45 / 1.0503 and AISI 1045. For speeds and feeds you can treat them interchangeably; what actually changes the result is the heat treatment of the bar in your hand.

Similar materials

S235 / St37 mild steel: cutting speed and feed rate

Cutting speed and feed for S235 / St37 / 1018 mild steel in turning, milling, drilling and tapping, with real Vc ranges and how to beat built-up edge.

42CrMo4 / 4140 alloy steel: cutting speed and feed rate

How to machine 42CrMo4 / 4140 quenched and tempered: cutting speed and feed per operation, coatings that survive and Vc matched to the bar's real hardness.

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.

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.