Engineering · Reference
Chip load chart by tool diameter.
Recommended feed per tooth (chip load, in/tooth) for solid-carbide end mills across seven material groups and seven tool diameters. Conservative starting values per Machinery’s Handbook and major tooling makers — pair them with the speed & feed calculator to get spindle RPM and feed rate.
Data reference
Recommended chip load (in/tooth) by end-mill diameter
Values are feed per tooth in inches for solid-carbide square end mills at moderate radial engagement (roughly 30–50% of diameter). Use the lower end of each range for small or long-reach tools, finishing passes, and tough lots; the upper end for rigid setups, short tools, and roughing. At light radial stepover, increase feed for radial chip thinning (see below).
| Material group | 1/8″ | 3/16″ | 1/4″ | 3/8″ | 1/2″ | 3/4″ | 1″ |
|---|---|---|---|---|---|---|---|
| Aluminum (6061 / 7075) Free-cutting; high MRR. Sharp uncoated/polished or ZrN flutes, generous chip room. | 0.001–0.002 | 0.0015–0.0025 | 0.002–0.004 | 0.003–0.005 | 0.004–0.007 | 0.005–0.009 | 0.006–0.011 |
| Mild & low-alloy steel 1018, 1045, 4140/4340 (prehard ≤ ~32 HRC). Coated carbide; flood or MQL. | 0.0005–0.001 | 0.001–0.0017 | 0.0015–0.0025 | 0.002–0.0035 | 0.0025–0.004 | 0.0035–0.0055 | 0.004–0.007 |
| Stainless & PH steel 304/316L, 17-4PH, 15-5PH. Keep the tool cutting — too light a chip work-hardens the surface. | 0.0004–0.0009 | 0.0008–0.0014 | 0.0012–0.002 | 0.0018–0.003 | 0.002–0.0035 | 0.003–0.0045 | 0.0035–0.0055 |
| Titanium (Ti-6Al-4V) Low thermal conductivity; high cutting pressure. High-pressure coolant, avoid dwell. | 0.0003–0.0007 | 0.0005–0.001 | 0.0007–0.0015 | 0.001–0.002 | 0.0014–0.0025 | 0.002–0.0035 | 0.0025–0.004 |
| Nickel superalloy (Inconel) Inconel 718, 625. Severe work-hardening; rigid setup, positive geometry, never rub. | 0.0003–0.0006 | 0.0005–0.0009 | 0.0007–0.0013 | 0.001–0.0018 | 0.0012–0.0022 | 0.0016–0.003 | 0.002–0.0035 |
| Brass / Bronze C360 brass, C932 bronze. Free-machining; sharp tools, watch for grabby zero/negative rake. | 0.001–0.002 | 0.0015–0.0025 | 0.002–0.0035 | 0.0025–0.0045 | 0.003–0.006 | 0.004–0.0075 | 0.005–0.009 |
| Plastics (Delrin / PEEK / Ultem) Sharp single/two-flute or O-flute; clear chips fast to avoid melting and re-cutting. | 0.001–0.003 | 0.002–0.004 | 0.003–0.006 | 0.004–0.008 | 0.005–0.01 | 0.006–0.012 | 0.007–0.014 |
Representative carbide ranges compiled from Machinery’s Handbook (31st ed.) and published charts from Harvey Tool, 6GTools, and Inconel-machining references. Coatings, helix angle, flute count, runout, and rigidity all shift the working value — always confirm against your specific tool manufacturer’s data sheet and run a test cut.
How to use this chart
From chip load to feed rate.
Chip load is the thickness of material each cutting edge removes per revolution. It is the parameter that actually governs tool life and finish — pick it first, then solve for feed rate.
- The feed formula
IPM = RPM × flutes × chip load. Pick the chip load for your diameter and material from the chart, get RPM from cutting speed, multiply by the number of flutes. Example: a 1/2″ 4-flute carbide end mill in 6061 at 6,000 RPM and 0.005″/tooth → 6,000 × 4 × 0.005 = 120 IPM.
- Radial chip thinning (RCT)
When radial depth of cut (stepover, ae) drops below half the tool diameter, the actual chip comes out thinner than the programmed chip load, so you must feed faster to keep the edge cutting. The factor is RCTF = 1 / √(1 − (1 − 2·ae/D)²). Worked values: about 1.15× at 25% stepover, 1.4× at 15%, 1.67× at 10%, and ~2.3× at 5%. Multiply the chart chip load by RCTF before computing IPM.
- Small and long tools cut less per tooth
Chip load scales down with diameter because a thin shank deflects and a small flute has little chip room. Long-reach or necked tools deflect more still — drop to the low end of the range (or below) and lighten axial depth to keep the tool stable.
- Too light is as bad as too heavy
An over-light chip load makes the edge rub instead of shear — generating heat, chatter, and work-hardening (especially in stainless and Inconel). An over-heavy chip load packs the flutes and breaks tools. Stay inside the range and tune from there.
Related references
Build the full cut.
Chip load is one input. Pair it with these tools and datasheets to lock in spindle speed, feed, material removal rate, and cycle time.
- Speed & feed calculator — turn a chip load plus diameter and flutes into SFM, RPM, and IPM.
- Material removal rate (MRR) calculator — combine feed with width and depth of cut to size the cut for your spindle.
- Cycle time calculator — convert feed rate and path length into machining minutes.
- How to machine 6061 aluminum and Inconel 718 — material-specific tooling and parameter notes.
- How to machine Ti-6Al-4V — why low chip loads and high-pressure coolant matter on titanium.
- Drill size chart and tap drill calculator — for the hole-making side of the job.
Keep exploring
Related tools & references
Turn chip load and SFM into spindle RPM and feed rate.
Combine feed, width, and depth into an MRR figure.
Estimate run time once feeds and depths are set.
How feed per tooth drives the achievable Ra.
Machinability notes by alloy family to set a starting chip load.
Technically reviewed by the True Precision Machining engineering team · Last reviewed June 2026
Have a part that needs to be made right?
Tell us about your part and we'll quote within 24 hours. Aerospace, medical, and defense work welcome.
Quotes in 24 hours