Short answer: if you're running a 1/4" 4-flute solid-carbide end mill in 4140 prehard (around 28–32 HRC) with flood coolant, start at 280 SFM, 4,280 RPM, ~26 IPM, 0.0015 in/tooth, and step the depth-of-cut according to whether you're slotting, profiling, or cutting trochoidal. Below is the full math, the SFM ranges for the three common conditions of 4140 (annealed, prehard, hardened), the chip-load adjustments, and the conservative DOC + WOC you can hand to a new operator.

The formulas

RPM  = (SFM × 12) / (π × D)
IPM  = RPM × Z × Fz
MRR  = IPM × DOC × WOC

D    = tool diameter (inches)
Z    = number of flutes
Fz   = chip load per tooth (in/tooth)
DOC  = axial depth of cut (inches)
WOC  = radial depth (width) of cut (inches)

SFM ranges for 4140 with carbide

4140 ships in three common conditions. Pick the row that matches what you actually have in the chuck:

• 4140 annealed (~22 HRC) — 350–500 SFM with carbide, flood coolant.
• 4140 prehard / HT (~28–32 HRC) — 250–350 SFM. This is the bay default.
• 4140 heat-treated (40+ HRC) — 100–180 SFM, and only with rigid holders + AlTiN coatings.

Coatings push the high end of each range up by ~10–15%. AlTiN + flood coolant on prehard 4140 will run 320 SFM all day on a Haas VF with a CAT40 holder. Drop to TiN-only or no coolant and pull back to 240–260.

Chip load (Fz) for a 1/4" 4-flute

• 1/4" 4-flute carbide in steel — 0.0010–0.0020 in/tooth.
• Conservative starting point (new tool, average rigidity): 0.0015 in/tooth.
• Aggressive (production, rigid setup, known tool): 0.0020 in/tooth.
• Below 0.0010 in/tooth you start rubbing — the tool work-hardens the chip and the edge dies fast.

Worked example: 1/4" 4FL carbide in 4140 prehard, profiling

Material:   4140 prehard (~30 HRC)
Tool:       1/4" 4-flute carbide, AlTiN
Operation:  Profiling (light radial)
Coolant:    Flood

SFM (carbide on prehard 4140):  280 (mid-range)

RPM = (280 × 12) / (π × 0.25)
    = 3360 / 0.7854
    = 4,278 RPM   →  round to 4,280

Fz  = 0.0015 in/tooth (conservative start)

IPM = 4280 × 4 × 0.0015
    = 25.7 IPM

Axial DOC:   0.50 × D = 0.125"
Radial DOC:  0.40 × D = 0.100"

MRR = 25.7 × 0.125 × 0.100
    = 0.32 in³/min

Slotting vs profiling vs trochoidal

The recipe above is for profiling (cutter is engaged on one side, ~40% of diameter wide). Two adjustments matter:

• Full slot (1.0 × D radial): drop axial DOC to 0.25 × D and reduce feed by ~30% — the cutter is engaged on both sides, heat is twice as bad.
• Trochoidal / dynamic milling: radial 5–10% of D, axial 1.5–2.0 × D. You can raise SFM 30–50% because the chip has time to evacuate heat before the next pass.
• Finish pass: radial 5–10% of D, full flute axial, cut feed by 20% to clean the wall.

If the spindle complains

The whole table at a glance

1/4" 4-flute solid carbide, AlTiN coated, flood coolant

                   SFM     RPM      Fz       IPM    Axial   Radial
4140 annealed       420   6,420   0.0020    51.4   0.125"  0.100"
4140 prehard        280   4,280   0.0015    25.7   0.125"  0.100"
4140 hardened       150   2,290   0.0010     9.2   0.060"  0.060"

Slotting (1.0 × D radial): cut IPM by 30%, axial = 0.25 × D
Trochoidal (0.05 × D radial): SFM ×1.4, axial = 1.5 × D
Finish pass: cut IPM by 20%, radial = 0.05–0.10 × D

Why a single number isn't enough

Forum threads will give you "run 1/4" carbide in 4140 at 5000 RPM and 30 IPM" and that's exactly half the inputs. You need the diameter, flute count, material condition, coolant condition, operation type, and chipload to compute a recipe that won't scrap the tool. The math takes 10 seconds; the recovery from a wrong-feed broken tap takes 30 minutes.

Run it on your phone

The ShopCalc app holds the SFM ranges for every common steel, aluminum, stainless, brass, and titanium grade, plus chip-load presets by tool diameter and material. Type the diameter, pick the material, and it gives you RPM, IPM, axial/radial DOC, and an MRR — with ±50% SFM and chip-load sliders if you want to push or pull from the default. 100% offline. Free on the App Store and Google Play.

Related

• Speeds and feeds — the formulas and chip-load chart in full
• Tap drill chart for 1/2-13 UNC at 75% engagement
• ShopCalc — machinist calculator on iOS + Android

Note: Starting points only. Always verify on a test cut, especially for production runs and unfamiliar tooling.