Cutting Speeds And Feeds for Carbide Inserts: A Practical Guide

Cutting speed and feed are the two most important levers for productivity in CNC machining. Set them well and you maximize metal removal rate (MRR), surface finish and tool life; set them poorly and you get rapid wear, broken inserts or poor surface finish. This guide gives practical, authoritative steps to choose speeds & feeds for carbide inserts — using ISO insert nomenclature so you know exactly which insert you have, the formulas to convert speeds into RPM/feeds into IPM or mm/min, and the shop-floor tips engineers rely on.

How cutting speed (Vc) and RPM relate — formulas & worked example

Formulas (industry standard):

• RPM=1000×Vcπ×D\text{RPM} = \dfrac{1000 \times V_c}{\pi \times D}RPM=π×D1000×Vc​​ when VcV_cVc​ is in m/min and D in mm.
• RPM=3.82×SFMDin\text{RPM} = \dfrac{3.82 \times \text{SFM}}{D_{in}}RPM=Din​3.82×SFM​ and SFM=RPM×Din3.82\text{SFM} = \dfrac{\text{RPM} \times D_{in}}{3.82}SFM=3.82RPM×Din​​ (imperial). 

Worked example (metric):
You have a carbide turning insert for steel with recommended $Vc=180m/min$ and the work diameter D = 50 mm.
RPM=1000×180π×50≈180000157.08≈1146 RPM.\text{RPM} = \dfrac{1000 \times 180}{\pi \times 50} \approx \dfrac{180000}{157.08} \approx 1146 \,\text{RPM}.RPM=π×501000×180​≈157.08180000​≈1146RPM. 

Note: recommended Vc comes from the insert grade and the material group (P, M, K, N, S, H per ISO 513 / manufacturer tables). Use the grade data sheet (Sandvik, Kennametal, Iscar) for starting Vc. 

How feed (fz) and feed rate relate — formulas & worked example

Formulas:

• $Feed\; rate\; (mm/min)=RPM\times fz\times Z$
  where fzf_zfz​ = feed per tooth (mm/tooth), and Z = number of teeth (or for turning, use feed per revolution fff directly: mm/rev). 

Example (milling): Cutter with 4 teeth, RPM = 3000, desired chip load $fz=0.05mm/tooth$:
Feed rate = $3000\times 0.05\times 4=600mm/min.$

Turning note: turning feed is usually given as mm/rev; if your chart gives feed per revolution, multiply by RPM to get mm/min. 

• Cutting speed (Vc) — the speed of the workpiece relative to the cutting edge measured as surface meters per minute (m/min) or surface feet per minute (SFM). Think of it like car speed — how fast the metal slides past the insert. Typical units: m/min or ft/min. 
• RPM (n) — spindle revolutions per minute. Calculated from Vc and tool/work diameter.
• Feed per tooth / feed per revolution (fz or IPT) — how far each cutting edge advances per engagement. Like the step length each foot takes when walking; too big and you trip (tool overload), too small and you take forever (poor productivity).
• Feed rate (F or IPM / mm/min) — how fast the tool moves linearly (RPM × fz × number of teeth).
• Depth of cut (DOC) — how deep each pass removes material (radial and axial cuts).
• Chip load — the volume of material removed per cutting edge per second; controls cutting forces and temperature.
  Formulas and conversion examples are below.

ISO 1832 defines the standardized code for indexable inserts (first seven symbols are mandatory). The code tells you shape, clearance (relief) angle, tolerance class, fix/chipbreaker type, size (inscribed circle IC), thickness, and corner radius. Read the ISO standard when in doubt.

Common example and decoding (ISO practice): CNMG 120408 - MP
We’ll decode only the first 7 mandatory positions (the usual practical set):

1. C — shape. C = rhombic (80° included angle). (ISO table of shapes).

2. N — normal clearance/relief. N = 0° clearance (neutral / zero relief). Other letters map to 3°, 5°, 7° etc. (see ISO table 2). 

3. M — tolerance class (manufacturer use; commonly indicates medium tolerance class; ISO lists tolerance letter codes — consult ISO table). 

4. G — fixing/chipbreaker/edge style (G is often used for a particular chipbreaker style or ground edge — manufacturers add suffixes to clarify). 

5. 12 — inscribed circle (IC) in mm (12 mm → often shown as 120 or 12 depending on format; ISO and ANSI use metric/inch codes). 

6. 04 — thickness code (e.g., 04 corresponds to a specific thickness like 3.18 mm or per ISO tables). 

7. 08 — corner radius (0.8 mm nose radius). The last two digits (e.g., 08) designate the nose radius. 

Shop tip: Manufacturers often append short manufacturer codes (e.g., -MP, -CQ) to indicate chipbreaker and grade. Those are supplementary symbols (allowed by ISO if separated with a dash). Always check the manufacturer datasheet for the final two symbols. 

1. Insert grade (carbide substrate + coating): Grades are optimized per material group. P grades = steels, M = stainless steels, K = cast iron, N = non-ferrous, S = superalloys, H = hardened. Choose the grade first — it defines your recommended Vc and rough starting feeds. (See ISO 513 and vendor grade pages). 

2. Coatings (PVD vs CVD):

   • PVD (physical vapor deposition) coatings are thin and hard with good adhesion — they give lower built-up edge, better finish, and often allow higher cutting speeds for finishing and light roughing.

   • CVD (chemical vapor deposition) coatings are thicker and can provide thermal barrier and toughness — often used for heavy roughing at higher temperatures. Choose per manufacturer guidance. 

3. Chipbreaker design: Chipbreakers control chip shape at certain feeds and DOC. If chips are long and stringy, increase feed or choose a more aggressive chipbreaker. Manufacturer datasheets show the chipbreaker feed/DOC ranges. 

4. Insert geometry (clearance/rake/nose radius): Positive geometries and small nose radii reduce cutting forces — good for finishing or unstable setups. Larger radii and negative geometries increase strength for heavy cuts. Adjust feed accordingly. 

Practical shop approach (step-by-step):

1. Identify insert (ISO code) and the manufacturer data sheet for that insert (chipbreaker, grade). 

2. Pick material group (ISO 513) → choose appropriate grade family (P/M/K/N/S/H). 

3. Use manufacturer recommended Vc and chip load ranges as starting point (Sandvik/Coro, Kennametal, Iscar datasheets). 

4. Convert Vc → RPM and chip load → feed rate with formulas above. 

5. Start conservative: use 70–85% of recommended feed/speed for a new operation and ramp up if stability and tool life look good. Sandvik and other vendors recommend conservative startup to secure insert and machine. 

Rule of thumb for starting conservative: start at 70–85% of the recommended Vc and chip load, check chip shape, temperature and edge condition after a short trial cut; then tune up or down. Sandvik recommends starting conservatively to secure insert and surface finish. 

Example (turning mild steel, P-grade coated carbide):

• Suggested Vc: 180–250 m/min (finish → lower; high-feed/roughing → higher depending on grade)
• Starting feed: 0.10–0.30 mm/rev (depends on nose radius and desired finish)
• DOC (axial): 0.5–2.0 mm for finishing → 2–6 mm for roughing depending on insert type and clamping.
  (Always confirm exact numbers from the insert datasheet for that grade/chipbreaker.) 

• Built-up edge (BUE): reduce feed, increase cutting speed slightly, or switch to a PVD grade/coating.
• Poor chip control (long/stringy chips): increase feed or choose chipbreaker suited to smaller feeds; reduce depth of cut to get the chip into the breaker zone. 
• Edge chipping: reduce feed/impact, check runout, use a more robust (negative) geometry or tougher grade.
• High temperature / short tool life: reduce Vc or switch to a thermal-resistant grade or CVD coating for heavy cuts.