Speeds & Feeds for Carbide Inserts
Cutting parameters reference: Vc (cutting speed), fz (feed per tooth), ap (depth of cut) for steel, stainless, cast iron, aluminum, HRSA, and hardened steel. Includes formulas, charts, troubleshooting, and an interactive calculator.
The Three Core Formulas
Speeds and feeds all derive from these three equations. Memorize them, and you can troubleshoot any cutting problem on the shop floor.
Where D = tool diameter (or insert engagement), n = spindle speed. This is the surface speed at the cutting edge. Higher Vc → more heat → faster wear. Lower Vc → slower cutting → longer tool life but lower MRR.
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. Doubling ap doubles MRR but doubles radial force too.
Cutting Speed by Material (Vc Reference)
These are starting recommendations for carbide inserts. Adjust ±20% based on your grade, setup rigidity, and surface finish requirements. Always test on 5-10 pieces before committing to production.
Steel (ISO P05-P45) — 150-250 m/min
| Operation | Grade Type | Vc (m/min) | fz / f (mm/rev or mm/tooth) | ap (mm) |
|---|---|---|---|---|
| Rough turning | CVD (US7020, GC4325, YBC151) | 150-200 | 0.20-0.40 | 2.0-8.0 |
| Medium turning | CVD (US7020, GC4325) | 180-230 | 0.15-0.25 | 1.0-3.0 |
| Finish turning | CVD (GC4305, CA6515) or PVD (VP15TF) | 200-250 | 0.05-0.15 | 0.3-1.0 |
| Face milling | CVD (APKT 1604 grade) | 180-250 | 0.10-0.25 | 1.0-4.0 |
| Drilling (U-drill) | CVD or PVD | 120-180 | 0.05-0.15 | — |
| Threading | CVD (UE6020) or PVD | 100-180 | thread pitch driven | — |
Stainless Steel (ISO M10-M30) — 80-180 m/min
| Operation | Grade Type | Vc (m/min) | fz / f (mm/rev) | ap (mm) |
|---|---|---|---|---|
| Rough turning | PVD (VP15TF, GC2025, TT9080) | 80-130 | 0.15-0.30 | 2.0-5.0 |
| Medium turning | PVD (VP15TF, YBM151) | 120-160 | 0.10-0.20 | 1.0-2.5 |
| Finish turning | PVD (VP15TF, GC2025) | 150-180 | 0.05-0.12 | 0.3-1.0 |
| Milling (peripheral) | PVD (APMT 1135 VP15TF) | 100-150 | 0.08-0.20 | 1.0-3.0 |
| Drilling (SPMG U-drill) | PVD (VP15TF) | 80-130 | 0.04-0.10 | — |
| Threading | PVD (VP15TF) | 60-120 | thread pitch driven | — |
Cast Iron (ISO K10-K25) — 100-200 m/min
| Operation | Grade Type | Vc (m/min) | fz / f (mm/rev) | ap (mm) |
|---|---|---|---|---|
| Rough turning | CVD (MP8015, YBD102, KF5800) | 120-180 | 0.20-0.40 | 2.0-8.0 |
| Medium turning | CVD (GC3210, CA310) | 150-200 | 0.15-0.30 | 1.0-3.0 |
| Finish turning | CVD (GC3210, KF2500) | 180-220 | 0.10-0.20 | 0.3-1.0 |
| Milling | CVD (SPKN / SEKN style) | 120-180 | 0.10-0.25 | 1.5-5.0 |
Aluminum (ISO N10-N25) — 300-600 m/min
| Operation | Grade Type | Vc (m/min) | fz / f (mm/rev) | ap (mm) |
|---|---|---|---|---|
| Rough turning | Uncoated K10 (CCGT K10, YD201) | 300-500 | 0.15-0.40 | 2.0-6.0 |
| Finish turning | Uncoated polished or DLC-coated | 400-600 | 0.05-0.20 | 0.3-1.5 |
| Milling (high-Vc) | Uncoated polished APKT | 400-800 | 0.05-0.20 | 1.0-4.0 |
| Drilling | Uncoated polished | 200-400 | 0.05-0.15 | — |
HRSA / Inconel / Titanium (ISO S05-S25) — 30-50 m/min (carbide), 200-300 m/min (ceramic)
| Operation | Grade Type | Vc (m/min) | fz / f (mm/rev) | ap (mm) |
|---|---|---|---|---|
| Rough turning (carbide) | PVD high-toughness (TT9080, VP15TF) | 30-50 | 0.10-0.20 | 1.0-3.0 |
| Medium turning (carbide) | PVD (TT9080, IC807) | 40-60 | 0.08-0.15 | 0.5-2.0 |
| Finish turning (ceramic) | SiAlON or whisker (CC6190, GC1105) | 200-300 | 0.10-0.20 | 0.3-1.0 |
| Drilling (U-drill carbide) | PVD high-toughness | 30-50 | 0.04-0.08 | — |
Hardened Steel (ISO H05-H25) — 80-150 m/min (CBN) or 50-100 m/min (ceramic)
| Hardness (HRC) | Insert Type | Vc (m/min) | f (mm/rev) | ap (mm) |
|---|---|---|---|---|
| 48-55 HRC | Coated carbide (CA5525, GC4325) | 100-150 | 0.10-0.20 | 0.5-2.0 |
| 55-62 HRC | CBN (low-CBN content) | 120-180 | 0.10-0.15 | 0.3-1.0 |
| 62-68 HRC | CBN (high-CBN content) | 100-150 | 0.05-0.12 | 0.2-0.5 |
| 65+ HRC | Ceramic (SiAlON or whisker) | 50-100 | 0.05-0.15 | 0.2-0.5 |
Feed & Depth of Cut by Operation
| 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 requirement (Ra) |
| Face milling | fz (mm/tooth) | 0.10-0.25 | Cutter diameter, insert size, machine rigidity |
| Peripheral milling | fz (mm/tooth) | 0.05-0.20 | Same as face milling, plus radial engagement |
| High-feed milling | fz (mm/tooth) | 0.30-0.80 | Small round inserts, low radial engagement |
| Drilling (indexable 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 (ISO, UN, BSW, etc.) |
| Grooving / Parting | f (mm/rev) | 0.05-0.20 | Groove width, chipbreaker geometry |
Insert Geometry Effect on Parameters
The same insert grade can run at ±20-30% different Vc depending on geometry. Four geometry variables matter:
| Geometry Variable | Effect on Vc | Effect on fz | Effect on Cutting 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 by Operation
| Operation | Chipbreaker Type | Examples | Best For |
|---|---|---|---|
| Rough turning (ap >3 mm) | PM / MM | CNMG 120408-PM, CNMG 120412-MM | Steel, stainless at high fz |
| Medium turning (ap 1-3 mm) | PM / MF | CNMG 120404-PM, TNMG 160404-MF | General purpose, steel |
| Finish turning (ap <1 mm) | MF / GF / PF | CNMG 120404-MF, VBMT 160404-PF | Low Ra surface finish |
| Aluminum finishing | Sharp ground (no breaker) | CCGT 060204 K10 (polished) | BUE prevention |
| High-feed milling | Special high-feed | RPMT 08T2-MJ, RDKT 0702-MJ | fz >0.5 mm/tooth |
| Stainless finishing | Sharp ground (no breaker) | CCMT 060204, DCMT 070204 | Sharp edge for low work hardening |
Coolant Strategy by Material & Operation
| Material | Operation | Coolant Type | Pressure | Reason |
|---|---|---|---|---|
| Steel (P) | Turning / Milling | Flood (8-12% emulsion) | 5-15 bar | Heat dissipation, tool life |
| Steel (P) | Drilling | Flood or HP through-tool | 10-30 bar | Chip evacuation |
| Stainless (M) | Turning | Flood + HP option | 15-30 bar | Prevent work hardening, +30% tool life with HP |
| Stainless (M) | Drilling / Threading | HP through-tool (mandatory) | 70-150 bar | Chip evacuation in gummy material |
| Cast Iron (K) | Turning / Milling | Dry or MQL (preferred) | — | Avoid thermal cracking |
| Aluminum (N) | Turning / Milling | Flood or MQL | 5-15 bar | Prevent BUE welding to edge |
| HRSA (S) | Turning (carbide) | HP through-tool | 70+ bar | Heat dissipation, +50% tool life |
| HRSA (S) | Turning (ceramic) | Dry | — | Ceramic + coolant = thermal shock fracture |
| Hardened (H) | CBN turning | Dry or light flood | — | CBN tolerates heat; coolant optional |
Troubleshooting: Wear Pattern Recognition
The fastest way to diagnose cutting parameter problems is to read the wear pattern on a used insert. Here is a diagnostic reference:
| Wear Pattern / Symptom | Likely Cause | Fix |
|---|---|---|
| Crater wear (concave depression on top face) | Vc too high / chemical reaction with workpiece | Reduce Vc by 15-20%, switch to CVD with thicker Al2O3 |
| Flank wear (uniform band on clearance face) | Normal gradual wear; excessive = Vc too high | Reduce Vc 10-15%, or switch to more wear-resistant grade |
| Built-up edge (BUE) (material welded on rake) | Vc too low for aluminum / stainless, edge too dull | Increase Vc 30-50%, use sharper edge, more coolant |
| Chipping (small fractures on edge) | Vc too high for grade, interrupted cut, vibration | Reduce Vc 10-15%, switch to tougher grade (PVD), check rigidity |
| Notch wear (wear at depth-of-cut line) | Oxidation at high temp (steel), or coolant infiltration | Reduce Vc, switch to Al2O3-rich CVD grade |
| Plastic deformation (edge deformed under heat) | Vc way too high, inadequate coolant | Reduce Vc 30%+, add HP coolant, switch to ceramic if heat persists |
| Thermal cracking (cracks perpendicular to edge) | Coolant on hot insert (thermal shock), cast iron dry machining mistake | Pre-heat insert with light cut, switch to dry for cast iron |
| Chips purple / blue (overheated) | Vc way too high, chip evacuation poor | Reduce Vc 20-30%, increase coolant pressure, check chip breaker geometry |
| Chips stringy / long | fz too low, chipbreaker ineffective | Increase fz 20-30%, switch chipbreaker to more aggressive (PM/MM) |
| Spindle load fluctuating | Chip jamming, BUE forming, chip evacuation issue | Reduce fz, check chipbreaker geometry, increase coolant |
Decision Tree: From Material to Parameters
Material (workpiece) ├── Steel (P) → CVD grade → Vc 150-250 → f 0.10-0.40 → flood coolant ├── Stainless (M) → PVD grade → Vc 80-180 → f 0.05-0.30 → HP coolant ├── Cast Iron (K) → CVD grade → Vc 120-220 → f 0.10-0.40 → DRY / MQL ├── Aluminum (N) → Uncoated polished → Vc 300-600 → f 0.05-0.40 → flood or MQL ├── HRSA (S) → PVD high-toughness → Vc 30-60 → f 0.05-0.20 → HP 70+ bar └── Hardened (H) → CBN or ceramic → Vc 80-180 (CBN) → f 0.05-0.15 → dry/light flood Operation (geometry) ├── Rough (ap >3 mm) → negative rake, large nose → high fz ├── Medium (ap 1-3 mm) → either rake, medium nose → medium fz ├── Finish (ap <1 mm) → positive rake, small nose → low fz for Ra └── High-feed (fz >0.5) → round insert, low radial engagement → very high fz
Frequently Asked Questions
What is cutting speed (Vc) and how do I calculate it for carbide inserts?
Cutting speed Vc (m/min) is the surface speed at which the insert cutting edge engages the workpiece. Formula: Vc = π × D × n / 1000, where D = tool diameter (mm) and n = spindle speed (RPM). For carbide inserts, typical Vc ranges: steel 150-250 m/min, stainless 80-180 m/min, cast iron 100-200 m/min, aluminum 300-600 m/min, HRSA 30-50 m/min. Use our Speeds & Feeds Calculator to look up Vc by material and operation.
How do I calculate feed per tooth (fz) for carbide milling?
Feed per tooth fz (mm/tooth) is the chip thickness each tooth removes per revolution. Formula: fz = Vf / (n × z), where Vf = feed rate (mm/min), n = spindle speed (RPM), z = number of effective teeth. For carbide milling, typical fz: finishing 0.05-0.15 mm/tooth, medium 0.10-0.25 mm/tooth, roughing 0.20-0.50 mm/tooth. Multiply by number of teeth for total feed rate.
What is depth of cut (ap) for roughing vs finishing?
Depth of cut ap (mm) is how deep the insert penetrates radially. For turning: roughing ap 2-8 mm (full insert engagement), medium ap 1-3 mm, finishing ap 0.3-1.0 mm. For milling: roughing ap = full cutter diameter engagement possible, semi-finishing ap = 1/3 to 1/2 diameter, finishing ap = 0.5-2.0 mm. Higher ap requires more rigid setup and tougher grade.
Can I use the same Vc for stainless steel and aluminum?
No — stainless steel (ISO M) runs at 80-180 m/min with PVD grades, while aluminum (ISO N) runs at 300-600 m/min with uncoated polished grades. Stainless requires sharp edges to prevent work hardening; aluminum requires sharp edges to prevent built-up edge (BUE). Both need coolant but at different strategies: stainless = high-pressure coolant, aluminum = flood or MQL to prevent edge welding.
How does coolant affect carbide cutting parameters?
Coolant strategy directly affects Vc, tool life, and chip evacuation. Flood coolant (most common): 8-12% emulsion, 30-50 L/min flow, allows 10-20% Vc boost on steel. High-pressure coolant (HP): 70-150 bar, used for stainless drilling/threading and HRSA turning, enables 30-50% Vc increase. Dry/MQL (Minimum Quantity Lubrication): required for cast iron (avoids thermal cracking) and some HRSA operations. Never use coolant on cast iron unless grade is K-grade with thermal-stable CVD coating.
What are the symptoms of running cutting speed too high?
Excessive Vc symptoms: (1) insert cutting edge shows crater wear (concave depression on top face) within minutes, (2) workpiece shows discoloration (blue/purple = overheated), (3) chips are purple/red hot instead of straw/gold color, (4) spindle load drops (cutting force decreases as edge wears), (5) tool life drops 50%+ vs baseline. Reduce Vc by 15-20% and re-test. If problem persists, switch to a more wear-resistant grade (CVD instead of PVD, or higher hot-hardness grade).
Get Cutting Parameters in 30 Seconds
Stop cross-referencing PDF catalogs. Our calculator uses real-world data from Mitsubishi, Sandvik, Kyocera, and 5 other brands — input your material, insert grade, and operation, get Vc, fz, ap, RPM, and feed rate instantly.