CNC Chip Load Reference Worksheet
Chip load is the thickness of the chip each tooth takes, and getting it right is the difference between a cut and a rub. This worksheet gives a quick starting-point chart by material and cutter diameter and a form to record the numbers you end up proving.
Fill in
CNC Chip Load Reference Worksheet
Cutting Data Record
Company: Acme Precision Ltd Job: WO-24817 Part: BRK-1001 Rev C Material: 6061 aluminum Tool: 1/2 in 4 flute carbide square end mill, TiB2 coated Machine: VMC-04, 12,000 RPM spindle Programmer: J. Rivera Date: 2026-10-20
Typical Chip Load Starting Points, Carbide End Mills (inch per tooth, side milling)
| Material | 1/8 in | 1/4 in | 3/8 in | 1/2 in | 3/4 in |
|---|---|---|---|---|---|
| Aluminum alloys | 0.0015 | 0.003 | 0.004 | 0.005 | 0.006 |
| Mild steel (1018) | 0.0007 | 0.0015 | 0.002 | 0.003 | 0.004 |
| Alloy steel (4140, pre-hard) | 0.0006 | 0.0012 | 0.0018 | 0.0025 | 0.0035 |
| Stainless (304, 316) | 0.0005 | 0.001 | 0.0015 | 0.002 | 0.003 |
| Titanium (Ti-6Al-4V) | 0.0004 | 0.0008 | 0.0012 | 0.0018 | 0.0025 |
| Gray cast iron | 0.0008 | 0.0016 | 0.0024 | 0.0032 | 0.0045 |
Adjustments
Slotting (full width): reduce the table value by about 20 to 30 percent. Light radial engagement (under half the diameter): chips thin out, so feed per tooth can often be raised to compensate. Finishing passes: use roughly half of the table value and verify surface finish. Long stickout or weak fixturing: reduce feed and depth first, then speed. Always defer to the tool manufacturer's published data for the exact cutter and coating.
Proven Cutting Data for This Job
| Operation | Tool dia | Flutes | SFM | RPM | Chip load | Feed IPM | Result |
|---|---|---|---|---|---|---|---|
| Rough | |||||||
| Semi-finish | |||||||
| Finish | |||||||
| Drill |
Observations
Slot cut chattered at 0.005 in/tooth, reduced to 0.003. Finish pass at 0.002 in/tooth gave 32 uin Ra.
Sign-off
Values are typical starting points for coated solid carbide end mills in side milling, not guarantees. Chip loads vary with cutter geometry, coating, radial engagement, machine rigidity and coolant. Use the speeds and feeds calculator to convert chip load into feed rate.
Keep proven cutting data with the part record
Optional: we can discuss storing job-proven cutting data alongside routings and part masters in your ERP.
Optional. The tool and every export work without this. No spam.
How to use the worksheet
Fill in the job, material, tool and machine fields so the sheet identifies the conditions. Find your material row and cutter diameter in the chart, and use the value as a starting chip load. Then apply the adjustments for slotting, light radial engagement or finishing. Enter the speed, RPM, chip load and feed you actually run in the proven data table and note any chatter, finish or tool wear observations. Export the sheet to PDF or Word and keep it with the setup documentation for repeat orders.
Why chip load matters
If the chip is too thin, the edge rubs instead of cutting, which causes heat, work hardening in stainless and titanium, and fast wear. If it is too thick, cutting force and deflection rise and the tool can chip or break. The chart rises with diameter because larger cutters have more strength and flute space, and falls with harder or gummier material. Chip load also feeds directly into feed rate: IPM equals RPM times flutes times chip load.
- Too light: rubbing, heat, work hardening, short life
- Too heavy: chatter, deflection, chipped edges
- Larger diameter: larger allowable chip load
Reading the chart
The chart is for solid carbide end mills with a typical four flute or similar geometry in side milling. A half inch cutter in aluminum starts around 0.005 inch per tooth, while in stainless it is nearer 0.002. Where your cutter diameter lies between columns, interpolate. If your tool manufacturer publishes a different value for that exact cutter, use theirs; it reflects their geometry and coating. The sheet is meant to speed up the first pass and keep your own proven data in one place.
Common mistakes
Using a sheet value for the wrong tool is the most frequent error: a high-feed mill, a roughing end mill and a micro tool all have very different ranges. Another is copying a feed rate between machines without recalculating, even though RPM limits differ. Finally, many shops fail to write down the final proven numbers, so the next programmer starts from scratch. Recording them on this sheet fixes that.
Frequently Asked Questions
What is chip load in machining?
Chip load, or feed per tooth, is the thickness of material each cutting edge removes per revolution. It is measured in inches or millimeters per tooth and drives feed rate along with RPM and flute count.
How do I calculate chip load from feed rate?
Chip load equals feed rate divided by RPM times the number of flutes. For example 32 IPM at 2,674 RPM with 4 flutes gives about 0.003 inch per tooth. This is the inverse of the feed rate formula.
Why reduce chip load when slotting?
In a slot the cutter is fully engaged, so chips are packed into a tight space, heat builds up and cutting forces are highest. Reducing chip load by roughly a fifth to a third lowers load and improves chip evacuation.
Can I use these values for HSS end mills?
Not directly. High speed steel tools usually take lower chip loads and much lower surface speeds than carbide. Start from the manufacturer's data for the HSS cutter and use this sheet only to record what you prove.
If proven cutting data is trapped in paper travelers and individual memory, Netray can help connect it to part and routing records in your ERP so it is reusable.
Related Tools
CNC Speeds and Feeds Calculator
Turn a surface speed and chip load into spindle RPM and table feed for any end mill, capped at your machine's maximum RPM.
Discrete ManufacturingMaterial Removal Rate Calculator
Calculate milling MRR from width of cut, depth of cut and feed, then estimate the spindle horsepower the cut will need.
Discrete ManufacturingTool Life Taylor Equation Calculator
Use the Taylor equation V x T^n = C to predict tool life at a new cutting speed or find the speed that gives a target tool life.
Discrete ManufacturingSurface Finish Ra to RMS Converter
Convert Ra to RMS in microinches or micrometers and estimate the theoretical Ra a turning insert leaves from feed and nose radius.