A speeds & feeds chart gives you two numbers for each material: a surface speed (SFM) and a feed per tooth (IPT). Your machine needs RPM and feed rate (IPM). Here's how to get from one to the other.
The formulas
| To find | Formula |
|---|---|
| Spindle speed (RPM) | RPM = SFM × 3.82 ÷ tool diameter (in.) |
| Feed rate (IPM) | IPM = RPM × number of flutes × feed per tooth |
| Surface speed (SFM) from RPM | SFM = RPM × tool diameter × 0.262 |
The 3.82 and 0.262 come from converting the tool's circumference from inches to feet (12 ÷ π and π ÷ 12).
For metric: m/min = SFM × 0.3048, and mm/min = IPM × 25.4.
Worked example
A 1/2" 4-flute Majac Mills Ultra High Performance end mill in low carbon steel:
- The UHP chart gives 300–600 SFM. Start in the middle: 450 SFM.
- RPM = 450 × 3.82 ÷ 0.5 = 3,438 RPM.
- The chart's feed per tooth at 1/2" is 0.0040".
- IPM = 3,438 × 4 × 0.0040 = 55 IPM (about 1,400 mm/min).
Fine-tuning
- Start in the middle of the range. If the tool runs well without vibration or significant noise, increase SFM and/or feed per tooth in 5–10% steps.
- Check depth of cut. The charts assume a maximum depth. General Purpose tools, for example, are rated for up to 1× diameter when profiling and 0.5× diameter when full slotting. Each series' limits are shown in the calculator.
- Adjust for light radial cuts. Below 50% radial engagement, raise the feed per tooth to make up for chip thinning; see HEM explained.
- Ramp and plunge at about half the feed.
- Mind your machine. If the RPM is above your spindle's maximum, run at the maximum and reduce the feed rate in proportion, so the chip load stays the same.
Optimum speeds and feeds always depend on the material, setup, machine condition and tool deflection. If a job isn't running the way it should, call our technicians.
Questions about your application? Our technicians are happy to help. Call +1 705 728 8665 or .