Speeds & Feeds Reference by Material
This article is the master reference for surface speed (SFM), feed per tooth, and feed per revolution across all common workpiece materials. It covers carbide tooling (coated and uncoated) for both milling and turning. For HSS tooling, use roughly 40-50% of the carbide SFM values listed below.
Core Formulas
Every speeds-and-feeds calculation starts with these three formulas. Memorize them.
RPM from SFM
RPM = (SFM x 3.82) / Diameter (inches)
Where:
- SFM = surface feet per minute (the cutting speed for the material)
- 3.82 = constant (derived from 12 / pi)
- Diameter = tool diameter for milling, workpiece diameter for turning
Example: 400 SFM on a 0.500" end mill = (400 x 3.82) / 0.500 = 3,056 RPM
Feed Rate (IPM) for Milling
IPM = RPM x Feed Per Tooth (FPT) x Number of Flutes
Example: 3,056 RPM x 0.003" FPT x 4 flutes = 36.7 IPM
Feed Rate (IPR) for Turning
IPR = Feed per revolution (set directly on the CNC)
IPM = RPM x IPR
Example: 800 RPM x 0.008 IPR = 6.4 IPM
SFM Reference — Carbide Tooling by Material
These ranges assume coated carbide (CVD or PVD AlTiN/TiAlN) at standard conditions. Use the low end for roughing, interrupted cuts, long tool stickout, or poor rigidity. Use the high end for finishing, rigid setups, and good coolant delivery.
Carbon Steel (1018, 1045, 12L14)
| Operation | SFM Range | Notes |
|---|---|---|
| Turning — roughing | 500-700 | Coated carbide, CNMG/WNMG |
| Turning — finishing | 600-800 | Polished insert, light DOC |
| Milling — roughing | 400-600 | Coated carbide end mill |
| Milling — finishing | 500-700 | Reduce FPT for finish |
| Drilling — carbide | 350-500 | Through-coolant preferred |
- 12L14 (free-machining) can run 20-30% faster than 1045
- 1018 is gummy at low speeds — keep SFM above 400 to avoid built-up edge
Alloy Steel (4140, 4340, 8620)
| Operation | SFM Range | Notes |
|---|---|---|
| Turning — roughing | 350-500 | Coated carbide |
| Turning — finishing | 400-600 | Light DOC, sharp insert |
| Milling — roughing | 350-500 | 4 or 5 flute carbide |
| Milling — finishing | 400-550 | Reduce FPT |
| Drilling — carbide | 250-400 | Watch chip evacuation |
- Heat-treated 4140 (28-32 HRC): reduce SFM by 20-30%
- 4340 in normalized condition machines well at 400-500 SFM
- If insert life is short (under 15 minutes), SFM is too high — drop 15-20%
Stainless Steel — 304 / 316 (Austenitic)
| Operation | SFM Range | Notes |
|---|---|---|
| Turning — roughing | 250-350 | Maintain DOC > 0.010" to avoid work hardening |
| Turning — finishing | 300-400 | Sharp edge, positive rake |
| Milling — roughing | 250-350 | Climb mill only, no dwelling |
| Milling — finishing | 300-400 | Reduce stepover for finish |
| Drilling — carbide | 200-300 | Through-coolant, no pecking if possible |
- 303 (free-machining): Add 30-40% to these SFM values
- Never dwell in the cut. Stainless work-hardens instantly if the tool rubs without cutting
- Minimum chip load of 0.001" per tooth — going lighter causes rubbing and work hardening
- Use sharp, positive-rake inserts with honed (not chamfered) edges
Stainless Steel — 17-4 PH (Precipitation Hardened)
| Condition | SFM Range (Turning) | Notes |
|---|---|---|
| Condition A (solution treated, ~30 HRC) | 250-350 | Machines similar to 304 but less gummy |
| H1150 (~34 HRC) | 225-300 | Moderate |
| H1025 (~38 HRC) | 200-275 | Notch-sensitive, use round or large-radius inserts |
| H900 (~44 HRC) | 150-225 | Hard turning territory, use CBN or tough coated carbide |
- 17-4 PH is less prone to work hardening than 304 but tougher due to higher hardness
- Feed rates same as 304 ranges
- Milling SFM: 200-300 across conditions
Aluminum — 6061-T6 and 7075-T6
| Operation | SFM Range | Notes |
|---|---|---|
| Turning — roughing | 800-1200 | Uncoated or polished carbide |
| Turning — finishing | 1000-1500 | PCD for production |
| Milling — roughing | 800-1200 | 2 or 3 flute, polished |
| Milling — finishing | 1000-1500+ | High helix (45-degree), ZrN or DLC coated |
| Drilling — carbide | 500-800 | 130-degree point, through-coolant |
- 7075 is slightly harder (150 BHN vs 95 BHN for 6061) — use the low end of the range
- Aluminum is SFM-limited by the machine, not the tool — run as fast as your spindle allows
- At high SFM, chip evacuation becomes the limiting factor, not tool wear
- Use flood coolant or mist to prevent built-up edge
- Cast aluminum (A356, 380): reduce SFM by 20-30% due to silicon content abrasion
Titanium — Ti-6Al-4V (Grade 5)
| Operation | SFM Range | Notes |
|---|---|---|
| Turning — roughing | 100-175 | Uncoated or PVD coated carbide |
| Turning — finishing | 150-200 | Sharp edge, positive rake |
| Milling — roughing | 100-175 | 4-5 flute, variable helix |
| Milling — finishing | 150-200 | Reduce to 100-120 if chatter |
| Drilling — carbide | 80-150 | Through-coolant mandatory |
- Low SFM, high feed. Titanium has poor thermal conductivity — the heat stays in the cut. Keep speed low and push feed to move heat into the chip.
- Minimum chip load 0.002" per tooth (milling) to avoid work hardening
- Use flood coolant, high pressure (300+ PSI through-tool preferred)
- Commercially pure (CP) titanium: can run 20-30% faster than Ti-6Al-4V
Inconel 718
| Operation | SFM Range | Notes |
|---|---|---|
| Turning — roughing | 80-120 | Coated carbide, aggressive chipbreaker |
| Turning — finishing | 100-150 | Sharp insert, light DOC |
| Milling — roughing | 80-120 | 5+ flute, high feed strategy |
| Milling — finishing | 100-140 | |
| Ceramic turning | 600-1000 | Ceramic inserts, no coolant, light DOC |
| Drilling — carbide | 50-80 | Through-coolant, reduced peck |
- Inconel is the hardest common material to machine — heat, work hardening, and abrasion all fight you
- Minimum chip load 0.002" per tooth
- Replace inserts before they are visually worn — notch wear creeps up fast
- Ceramic inserts run at 5-10x the SFM of carbide but require rigid setup and no interruptions
D2 Tool Steel
| Condition | SFM Range | Tooling |
|---|---|---|
| Annealed (~20 HRC) | 100-150 | Coated carbide (TiAlN/AlCrN) |
| Hardened (58-62 HRC) | 150-250 | CBN inserts for turning |
| Hardened (58-62 HRC) | 100-200 | Ceramic end mills for milling |
- Annealed D2 machines at surprisingly low SFM because the high chromium carbides in the steel are abrasive — pushing speed burns tools
- Hardened D2 is hard milling territory — CBN inserts at 150-250 SFM, light DOC (0.005"-0.010"), low feed
- On a CNC lathe, CBN inserts can finish hard D2 to 8-16 Ra at 200 SFM
- EDM is often more cost-effective than hard milling for complex D2 geometry
Cast Iron (Gray and Ductile)
| Type | SFM Range (Turning) | SFM Range (Milling) | Notes |
|---|---|---|---|
| Gray cast iron (Class 30-40) | 300-500 | 250-400 | Produces powder chips, can run dry |
| Ductile cast iron (65-45-12) | 250-400 | 250-350 | Produces curled chips like steel |
| High-strength ductile (80-55-06) | 200-350 | 200-300 | More abrasive, tougher |
- Gray cast iron can be machined dry — the graphite flakes act as a lubricant
- Do NOT use coolant on gray cast iron if possible — the abrasive slurry (cast iron dust + coolant) destroys machine ways and screws
- Ductile cast iron benefits from coolant, especially at higher SFM
- Use coated carbide inserts with a K-grade (cast iron specific) or general-purpose P/K combination
Feed Per Tooth (FPT) — Milling Reference
These are starting-point chip loads for coated carbide end mills. Adjust based on tool diameter, flute count, radial engagement, and rigidity.
| Material | FPT (inches) | Notes |
|---|---|---|
| Carbon steel (1018, 1045) | 0.003-0.006 | Higher for roughing, lower for finishing |
| Alloy steel (4140, 4340) | 0.003-0.005 | |
| Stainless 304/316 | 0.002-0.004 | Minimum 0.001" — less causes work hardening |
| 17-4 PH stainless | 0.002-0.004 | |
| Aluminum 6061/7075 | 0.004-0.010 | Chip evacuation is the limit |
| Titanium Ti-6Al-4V | 0.002-0.004 | Minimum 0.002" — less causes work hardening |
| Inconel 718 | 0.002-0.004 | Minimum 0.002" |
| D2 tool steel (annealed) | 0.002-0.004 | |
| D2 tool steel (hardened) | 0.001-0.002 | CBN or ceramic |
| Cast iron | 0.003-0.006 |
Important: These FPT values assume full-width or near-full-width cutting (radial engagement > 50%). When radial engagement drops below 50%, you must increase feed to compensate for chip thinning. See [[chip-thinning-and-hem]] for the adjustment formula.
Feed Per Revolution (FPR) — Turning Reference
| Material | FPR Roughing (IPR) | FPR Finishing (IPR) |
|---|---|---|
| Carbon steel | 0.008-0.015 | 0.003-0.006 |
| Alloy steel | 0.006-0.012 | 0.003-0.005 |
| Stainless 304/316 | 0.005-0.010 | 0.003-0.005 |
| 17-4 PH stainless | 0.005-0.010 | 0.003-0.005 |
| Aluminum | 0.008-0.015 | 0.004-0.008 |
| Titanium Ti-6Al-4V | 0.005-0.010 | 0.003-0.006 |
| Inconel 718 | 0.004-0.008 | 0.003-0.005 |
| Cast iron | 0.006-0.012 | 0.003-0.006 |
Chip Thinning Adjustment (Quick Reference)
When radial engagement is less than 50% of the cutter diameter, the actual chip is thinner than the programmed feed per tooth. You must increase feed to maintain proper chip thickness. See [[chip-thinning-and-hem]] for the full explanation.
| Radial Engagement (% of diameter) | Feed Multiplier |
|---|---|
| 50% | 1.0x (no adjustment) |
| 25% | 1.4x |
| 15% | 1.8x |
| 10% | 2.2-3.0x |
| 5% | 3.5-5.0x |
Surface Finish Formula (Turning)
The theoretical arithmetic average roughness in turning is:
Ra = f^2 / (32 x r)
Where:
- Ra = surface roughness in inches (multiply by 1,000,000 for microinches)
- f = feed per revolution (inches)
- r = tool nose radius (inches)
Example: 0.005 IPR feed with a 0.032" nose radius: Ra = (0.005)^2 / (32 x 0.032) = 0.000025 / 1.024 = 0.0000244" = 24.4 microinches Ra
Key insight: Halving the feed rate improves surface finish by 4x (because feed is squared). Doubling the nose radius improves finish by 2x.
For more on surface finish in turning, see [[surface-finish-turning]].
Common Mistakes
-
Running stainless or titanium too slow. This seems backwards, but running TOO slow causes built-up edge and work hardening. There is a minimum SFM below which things get worse, not better.
-
Running alloy steel too fast. 4340 at 600+ SFM with carbide burns through inserts in 10-15 minutes. The correct range is 350-500 SFM for general turning. If your CNMG432 in 4340 is failing at 15 minutes, SFM is too high — reduce to 400-500 SFM.
-
Ignoring chip thinning. Programming 0.003" FPT at 10% radial engagement means the actual chip is only 0.001" thick — you are rubbing, not cutting. Increase feed to compensate.
-
Using HSS feeds for carbide tools. Carbide can handle 2-4x the feed rate of HSS. If the manufacturer says 0.004" FPT, use 0.004" — not the 0.001" you learned on a Bridgeport.
-
Not adjusting for tool diameter. A 1/4" end mill at 400 SFM runs at 6,112 RPM. The same SFM on a 1" end mill is 1,528 RPM. Always calculate RPM from SFM, do not just enter a fixed RPM number.
Related Articles
- [[chip-thinning-and-hem]] — Chip thinning compensation and HEM/HSM strategies
- [[surface-finish-turning]] — Detailed surface finish control in turning operations
- [[insert-failure-analysis]] — Diagnosing insert wear to optimize speeds and feeds
- [[speeds-feeds-fundamentals]] — The complete beginner's guide to speeds and feeds concepts