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.
S235 / St37 mild 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.
S235 mild steel turns at 200-350 m/min (roughly 650-1,150 SFM) with 0.3 mm/rev of feed on coated carbide; drilling drops to 140-263 m/min and tapping to 70-158 m/min. It is the most common structural steel on the shop floor and also the one that gives the worst finish when you run it too slow. At 120 HB the limit is never spindle power - it is chip control and built-up edge.
EN S235JR · AISI 1018 · 120 HB · ISO group P
Recommended speeds and feeds
Operation
Vc (m/min)
Feed
Shop note
Turning
200–350
0.3 mm/rev
Work the top half of the range, 250-350 m/min, with a positive insert, a sharp edge and a roughing chipbreaker: below 150 m/min built-up edge forms and the surface tears even though the machine sounds perfectly happy.
Milling
200–350
0.12 mm/tooth
With an indexable face mill at 200-350 m/min, keep at least 0.12 mm feed per tooth so each insert really shears; dialling the feed back to improve the finish on S235 does the opposite, because the edge starts rubbing instead of cutting.
Drilling
140–263
0.2 mm/rev
Carbide drill at 140-263 m/min and 0.2 mm/rev with through-coolant; with HSS stay at 70-120 m/min and peck every 3-4 diameters, because the continuous chip winds around the shank and grabs.
Threading
70–158
0.2 mm/rev
Tapping runs at 70-158 m/min, and S235 is a textbook candidate for form taps: it has elongation to spare, the rolled thread ends up stronger, and there is no stringy chip left to jam the tap in a blind hole.
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
S235 carries only 0.17% carbon, so it is soft (120 HB) and very ductile. That ductility produces long, stringy, hot chips and makes the workpiece pressure-weld onto the rake face as built-up edge whenever surface speed is low. Because it conducts heat well, most of the heat leaves with the chip and the part, so the edge fails by adhesion rather than by temperature. It also throws a heavy burr on every exit edge: the material would rather fold over than shear off cleanly.
Built-up edge: why S235 tears instead of cutting
The number one defect in S235 is not wear, it is built-up edge. The workpiece cold-welds onto the rake face, grows, then breaks away taking coating with it and leaving a surface that looks like coarse sandpaper. It lives in the low and medium speed band, roughly 60 to 150 m/min, which is exactly where most programmers park out of habit. The fix runs against instinct: push the surface speed up towards 250-350 m/min, use a positive geometry with a polished edge, and never drop below 0.15 mm/rev. If it still shows up, check coolant flow before you blame the insert.
Chip control: bird's nests around the turret
At 0.3 mm/rev and a sensible depth of cut, S235 will happily produce a continuous chip that wraps the turret, scores the part and stops the cycle. Chips break when thickness and depth are enough to load the insert's chipbreaker, so the classic mistake is roughing with a shallow depth and a timid feed. Pick a medium roughing breaker, run a depth of at least two or three times the nose radius, and raise the feed before you raise the speed when the chip comes off long. In lights-out work, chip control outranks surface finish every time.
Mill scale, burrs and stress in hot-rolled stock
S235 almost always arrives hot-rolled, wearing a hard scale full of embedded sand that eats an edge far faster than the clean steel underneath. The first pass has to get under that layer, with at least 1.5 to 2 mm of depth and speed knocked back about 20%, rather than skimming the surface. Commercial sections also carry rolling stress: rough one face of a plate and it bows, so on flat parts rough both sides and leave stock for finishing. And plan the deburring - this steel raises a burr on every exit edge, and doing it by hand is expensive.
Quick shop tips
If the surface tears and the chips come off blue and welded, your problem is low surface speed, not a worn insert.
Do not cut the feed to chase a better finish: below 0.1 mm/rev in S235 the edge rubs and everything gets worse.
Knock 20% off the surface speed for the first pass over hot-rolled stock with mill scale on it.
Use form taps wherever you can: in a steel this ductile they give a stronger thread with no chip to evacuate.
Program the deburring operation; S235 raises a burr on every exit edge and hand work is the expensive way to fix it.
On long, slender shafts bring up the tailstock: the part deflects long before the tool feels anything.
Frequently Asked Questions (FAQ)
What cutting speed should I use on S235 with HSS tooling?
About a third of the carbide values: 70-120 m/min turning and milling, and a little less for drilling. HSS loses hardness with heat, so if you try the 300 m/min that carbide likes, the edge anneals itself in seconds.
Why does my S235 part come out with a torn surface?
Almost always built-up edge from running too slow. Move up to 250-350 m/min with coated carbide, keep the feed above 0.15 mm/rev and use a positive geometry with a sharp, polished edge.
Do I need coolant to machine S235?
Turning with carbide runs fine dry, but coolant helps break up built-up edge and flush chips clear. For drilling it is worth having, especially past three diameters of depth.
Is S235 the same thing as 1018 or St37?
They are working equivalents of the same low-carbon structural steel: EN S235JR, the old DIN St37 and American AISI 1018. For picking speeds and feeds treat them the same; cold-drawn 1018 usually finishes better simply because its surface is cleaner.
Can I run my S235 parameters on C45?
Not a good idea. C45 has more carbon and 180 HB, so drop the range to 180-280 m/min. Running S235 speeds in C45 accelerates crater wear on the insert.
