Custom CNC Speeds & Feeds Chart: Complete Reference & Calculator
Build a custom speeds and feeds chart for your operation — turning, milling, drilling, threading, grooving — across steel, stainless steel, cast iron, aluminum, HRSA, and hardened steel. Includes 3 core formulas, 6 material-specific Vc tables, chipbreaker selection, coolant strategy, and a free calculator.
Why a Custom Chart Beats Generic PDF Catalogs
Manufacturer PDF catalogs give you one speed per material — but real shops need more. Your custom chart should adjust for:
- Material sub-class — 304 vs 316 stainless need 10-15% Vc adjustment; 17-4 PH needs 40% drop from 304
- Insert grade family — CVD vs PVD runs at 15-20% different Vc on the same material
- Operation type — turning vs milling vs drilling use different formulas (f vs fz)
- Machine rigidity — older or smaller machines need 10-15% Vc reduction
- Coolant capability — flood vs HP coolant allows different Vc bands
- Surface finish requirement — Ra < 0.8 µm requires lower Vc + smaller ap
For the complete framework (material × operation × grade × coolant), see our Speeds & Feeds Hub. The reference below is the starting point.
The 3 Core Formulas
Memorize these three equations and you can troubleshoot any cutting problem on the shop floor.
Where D = tool diameter (or insert engagement diameter), n = spindle speed. This is the surface speed at the cutting edge. Higher Vc → more heat → faster wear.
Where Vf = feed rate, n = spindle speed, z = number of effective teeth. For turning, this is f (mm/rev) = Vf ÷ n. Higher fz → larger chips → higher MRR but more cutting force.
Direct value, no formula. ap × fz × Vc = Material Removal Rate (MRR, mm³/min) — the productivity metric.
Material-Based Speed Chart
These are starting recommendations for carbide inserts. Adjust ±20% based on your specific grade, setup rigidity, and surface finish requirement. Always test on 5-10 pieces before committing to production.
Steel (ISO P05-P45) — 150-250 m/min
| Operation | Grade Family | Vc (m/min) | f / fz | ap (mm) |
|---|---|---|---|---|
| Rough turning | CVD (US7020, GC4325, YBC151) | 150-200 | 0.20-0.40 mm/rev | 2.0-8.0 |
| Medium turning | CVD | 180-230 | 0.15-0.25 mm/rev | 1.0-3.0 |
| Finish turning | CVD or PVD | 200-250 | 0.05-0.15 mm/rev | 0.3-1.0 |
| Face milling | CVD | 180-250 | 0.10-0.25 mm/tooth | 1.0-4.0 |
| Drilling | CVD or PVD | 120-180 | 0.05-0.15 mm/rev | — |
Stainless Steel (ISO M10-M30) — 100-180 m/min
| Operation | Grade Family | Vc (m/min) | f / fz | ap (mm) |
|---|---|---|---|---|
| Rough turning | PVD (VP15TF, GC2025, TT9080) | 80-130 | 0.15-0.30 mm/rev | 2.0-5.0 |
| Medium turning | PVD | 120-160 | 0.10-0.20 mm/rev | 1.0-2.5 |
| Finish turning | PVD sharp | 150-180 | 0.05-0.12 mm/rev | 0.3-1.0 |
| Milling | PVD | 100-150 | 0.08-0.20 mm/tooth | 1.0-3.0 |
| Drilling | PVD + HP coolant | 80-130 | 0.04-0.10 mm/rev | — |
Cast Iron (ISO K10-K25) — 120-220 m/min
| Operation | Grade Family | Vc (m/min) | f / fz | ap (mm) |
|---|---|---|---|---|
| Rough turning | CVD (MP8015, YBD102, KF5800) | 120-180 | 0.20-0.40 mm/rev | 2.0-8.0 |
| Medium turning | CVD | 150-200 | 0.15-0.30 mm/rev | 1.0-3.0 |
| Finish turning | CVD | 180-220 | 0.10-0.20 mm/rev | 0.3-1.0 |
| Milling | CVD | 120-180 | 0.10-0.25 mm/tooth | 1.5-5.0 |
Aluminum (ISO N10-N25) — 300-600 m/min
| Operation | Grade Family | Vc (m/min) | f / fz | ap (mm) |
|---|---|---|---|---|
| Rough turning | Uncoated K10 (CCGT, YD201) | 300-500 | 0.15-0.40 mm/rev | 2.0-6.0 |
| Finish turning | Uncoated polished or DLC | 400-600 | 0.05-0.20 mm/rev | 0.3-1.5 |
| Milling (high-Vc) | Uncoated polished APKT | 400-800 | 0.05-0.20 mm/tooth | 1.0-4.0 |
| Drilling | Uncoated polished | 200-400 | 0.05-0.15 mm/rev | — |
HRSA / Inconel / Titanium (ISO S05-S25) — 30-60 m/min (carbide) / 200-300 m/min (ceramic)
| Operation | Grade Family | Vc (m/min) | f / fz | ap (mm) |
|---|---|---|---|---|
| Rough turning (carbide) | PVD tough (TT9080, VP15TF) | 30-50 | 0.10-0.20 mm/rev | 1.0-3.0 |
| Medium turning | PVD | 40-60 | 0.08-0.15 mm/rev | 0.5-2.0 |
| Finish turning (ceramic) | SiAlON or whisker (CC6190, GC1105) | 200-300 | 0.10-0.20 mm/rev | 0.3-1.0 |
| Drilling | PVD + HP coolant 70+ bar | 30-50 | 0.04-0.08 mm/rev | — |
Hardened Steel (ISO H05-H25) — 60-180 m/min
| Hardness | Insert | Vc (m/min) | f (mm/rev) | ap (mm) |
|---|---|---|---|---|
| 48-55 HRC | Coated carbide | 100-150 | 0.10-0.20 | 0.5-2.0 |
| 55-62 HRC | CBN low-content | 120-180 | 0.10-0.15 | 0.3-1.0 |
| 62-68 HRC | CBN high-content | 100-150 | 0.05-0.12 | 0.2-0.5 |
| 65+ HRC | Ceramic | 50-100 | 0.05-0.15 | 0.2-0.5 |
Operation-Based Feed Reference
| Operation | Feed Unit | Typical Range | Driver |
|---|---|---|---|
| Turning (rough) | f (mm/rev) | 0.15-0.40 | Insert nose radius, machine power |
| Turning (finish) | f (mm/rev) | 0.05-0.15 | Surface finish (Ra) |
| Face milling | fz (mm/tooth) | 0.10-0.25 | Cutter diameter, machine rigidity |
| Peripheral milling | fz (mm/tooth) | 0.05-0.20 | Same + radial engagement |
| High-feed milling | fz (mm/tooth) | 0.30-0.80 | Small round inserts, low radial engagement |
| Drilling (U-drill) | f (mm/rev) | 0.04-0.15 | Hole diameter, drill body stiffness |
| Threading | Pitch (mm/rev) | 0.5-6.0 | Thread pitch standard |
| Grooving / Parting | f (mm/rev) | 0.05-0.20 | Groove width, chipbreaker geometry |
For operation-specific insert selection, see Carbide Inserts by Operation.
Insert Geometry Effect on Parameters
| Geometry Variable | Effect on Vc | Effect on fz | Effect on Force |
|---|---|---|---|
| Positive rake (vs negative) | +10-20% Vc | No change | -20-30% force |
| Sharp edge (vs honed 0.05 mm) | +5-15% Vc (stainless) | -10-15% fz | -15-25% force |
| Large nose radius (0.8 vs 0.4 mm) | No change | +30-50% fz | +40-60% radial force |
| Chipbreaker (vs flat top) | No change | +10-20% fz | +5-10% force |
Chipbreaker Selection
| Operation | Chipbreaker | Examples |
|---|---|---|
| Rough turning (ap >3 mm) | PM / MM | CNMG 120408-PM, CNMG 120412-MM |
| Medium turning (ap 1-3 mm) | PM / MF | CNMG 120404-PM, TNMG 160404-MF |
| Finish turning (ap <1 mm) | MF / GF / PF | CNMG 120404-MF, VBMT 160404-PF |
| Aluminum finishing | Sharp ground (no breaker) | CCGT 060204 K10 (polished) |
| High-feed milling | Special high-feed | RPMT 08T2-MJ, RDKT 0702-MJ |
For ISO code breakdown of insert shapes and chipbreaker codes, see Carbide Inserts by ISO Code.
Coolant Strategy Matrix
| Material | Operation | Coolant | Pressure |
|---|---|---|---|
| Steel (P) | Turning / Milling | Flood | 5-15 bar |
| Stainless (M) | Turning | Flood or HP | 15-30 bar |
| Stainless (M) | Drilling / Threading | HP through-tool (mandatory) | 70-150 bar |
| Cast Iron (K) | Any | Dry or MQL | — |
| Aluminum (N) | Any | Flood or MQL | 5-15 bar |
| HRSA (S) | Carbide turning | HP through-tool | 70+ bar |
| HRSA (S) | Ceramic turning | Dry | — |
| Hardened (H) | CBN turning | Dry or light flood | — |
For tool holder selection to support high-pressure coolant, see Tool Holder Guide.
Frequently Asked Questions
How do I calculate cutting speed (Vc) for my CNC machine?
Cutting speed Vc (m/min) = π × D × n ÷ 1000, where D is tool diameter (mm) and n is spindle speed (RPM). For steel turning 150-250 m/min, stainless 100-180 m/min, cast iron 120-220 m/min, aluminum 300-600 m/min, HRSA 30-60 m/min. Use our free Speeds & Feeds Calculator to look up exact values.
What is feed per tooth (fz) for carbide milling?
Feed per tooth fz = Vf ÷ (n × z), where Vf is feed rate (mm/min), n is spindle speed (RPM), z is effective tooth count. Typical fz ranges: finishing 0.05-0.15 mm/tooth, medium 0.10-0.25 mm/tooth, roughing 0.20-0.50 mm/tooth. Multiply fz by tooth count to get table feed rate.
Can I use the same speeds and feeds for steel and stainless steel?
No — different grades and parameters. Steel uses CVD-coated grades (US7020, GC4325, YBC151) at 150-250 m/min. Stainless uses PVD-coated grades (VP15TF, GC2025, TT9080) at 100-180 m/min. Stainless requires sharp edges to prevent work hardening and high-pressure coolant. Steel tolerates honed edges and lower coolant pressure.
What is depth of cut (ap) for roughing vs finishing?
Depth of cut ap is how deep the insert cuts radially. For turning: roughing ap 2-8 mm, medium 1-3 mm, finishing 0.3-1.0 mm. For milling: roughing ap = full diameter engagement, semi-finishing 1/3-1/2 diameter, finishing 0.5-2.0 mm. Higher ap requires more rigid setup and tougher grade (more negative geometry). For high-Vc finishing (Ra requirements), use small ap + sharp edge.
What cutting speed should I use for carbide inserts on aluminum?
Aluminum (ISO N-class) requires very high Vc — 300-600 m/min for turning, 400-800 m/min for milling. Use uncoated polished grades (K10) or DLC-coated inserts with sharp ground edges to prevent built-up edge (BUE). Below 200 m/min, aluminum welds to the cutting edge causing rapid wear. Use coolant (flood or MQL) but avoid HP at these high Vc.
How do I optimize my CNC speeds and feeds for tool life?
Tool life optimization: (1) Start with manufacturer recommended Vc ±15% tolerance, (2) run 5-10 piece test batch, (3) inspect insert wear pattern at end of test, (4) crater wear = reduce Vc 15%, BUE = increase Vc 30%, chipping = switch to tougher grade (more negative rake, PVD instead of CVD), (5) optimize chipbreaker for actual chip shape — PM for medium, MF for finishing, MM for heavy roughing. Use Speeds & Feeds Calculator as starting point, then refine.
Get Your Custom Speeds & Feeds in 30 Seconds
Skip the math. Our calculator handles material, grade, operation, and machine specs — outputs RPM, Vc, fz, ap, and feed rate instantly.
Related: by Material · by Operation · by ISO Code · Grade Cross-Reference · Tool Holder Guide