Speeds & Feeds Chart Builder

Pick a material and tool, list your tool diameters, and get a printable table of RPM and feed rates for all of them at once. The material data is built in, so you do not need to look up a surface speed or chip load first. To work out a single tool from your own numbers, use the Speeds & Feeds calculator.

1. Material and tool

2. Tool diameters

Separate with commas. Fractions like 3/8 or 1-1/4 and decimals both work.

3. Where in the range

Low (safe start)MidHigh
Speeds & Feeds Chart – Machinist Central

Your speeds and feeds table

Open in Speeds & Feeds calculator
Surface speed
-
Chart range
-
Chip load
-
ISO group
-

    Conservative starting values for typical coated carbide and HSS tools, the same as the Speeds and Feeds Starting Chart. Check them against your tool maker's catalogue and adjust from test cuts.

    How the Speeds & Feeds Chart Builder Works

    The Chart Builder turns a material, a tool type and a list of your tool sizes into a ready-to-print speeds and feeds table: surface speed, RPM, chip load or feed per rev, and feed rate for every diameter.

    It is not the same tool as the Speeds & Feeds calculator. That calculator works out one tool from a surface speed and chip load you already know. The Chart Builder has a database of starting data for 17 materials built in, and builds a whole table for your end mills, drills or bar sizes at once, so you can pin it up next to the machine.

    The Method

    1. Look up the range
    For the material, tool material and operation it takes the low–high surface speed from the Speeds and Feeds Starting Chart, plus the chip load (end mills), feed per rev (drills, worked out from the drill diameter) or turning feed for that diameter.
    2. Pick a point in the range
    The slider sets how far from the low end to the high end to go. The same percentage is used for the surface speed and the chip load, so 0% is the gentlest start and 100% the most aggressive starting value.
    3. Work out RPM
    RPM is worked out for each diameter and rounded to a whole number. If it is above your machine's maximum, the maximum is used instead and the actual surface speed is shown.
    4. Work out the feed
    Feed rate comes from the RPM actually used, so a capped row gets a lower feed with the same chip load. The tool still takes a proper chip instead of rubbing or being overloaded.

    Formulas

    RPM = SFM × 12 ÷ (π × D) ≈ SFM × 3.82 ÷ D  (D in inches)
    RPM = Vc × 1000 ÷ (π × D)  (Vc in m/min, D in mm)
    Milling feed = RPM × chip load × flutes
    Drilling and turning feed = RPM × feed per rev
    Capped: RPM = machine max, actual SFM = RPM × π × D ÷ 12

    For turning, D is the workpiece diameter. On a CNC lathe use constant surface speed (G96) with a spindle limit, and program the feed per rev.

    Worked Example

    1018 steel, carbide end mill, 4 flutes, 50% of the range, 1/2 in diameter:

    • Chart range 250–450 SFM, so 50% gives 350 SFM.
    • RPM = 350 × 12 ÷ (π × 0.5) = 2,674 RPM.
    • Chip load at 1/2 in: 0.0020–0.0035 in, so 50% gives 0.0028 in per tooth (rounded).
    • Feed = 2,674 × 0.0028 × 4 = 29.9 IPM.

    Now a 1/8 in 3-flute carbide end mill in 6061 aluminium at 50% (1,050 SFM) on a 10,000 RPM machine: it wants 32,086 RPM, so the table shows 10,000 RPM, 327 SFM actual, the chip load stays at 0.0015 in, and the feed is 10,000 × 0.0015 × 3 = 45 IPM.

    Tips

    • Start low on a new set-up. Use 0–30% for HSS, long stick-out, light or hobby machines, thin walls and full-width slots.
    • Do not make up lost RPM with chip load. When the spindle tops out, keep the chip load and accept the lower feed rate, as the table does.
    • Light radial cuts can feed faster. Below about 30% stepover the chip is thinner than the chip load. Correct for it with the Chip Thinning Calculator.
    • Arcs need a feed correction. For internal circular moves use the Circular Feed calculator.
    • Check the power. Big tools in steel can need more power than a small machine has. Check with the MRR Calculator.
    • Copy as CSV pastes straight into a spreadsheet, so you can keep a tool-crib sheet for each machine.

    Frequently Asked Questions

    The Speeds & Feeds calculator works out RPM and feed for one tool from a surface speed and chip load you type in. The Chart Builder has the material data built in: pick the material, tool type and operation, and it builds a whole table for every diameter in your list, ready to print and pin up at the machine.

    Enter your spindle's maximum RPM. Any diameter that needs more is run at the maximum instead, the surface speed shown drops to match, and the feed rate is worked out again from the same chip load, so each tooth still takes the right size of chip. Those rows are marked in the table.

    Start at the middle (50%) for a normal job on a reasonably rigid machine. Use the low end for HSS tools, long stick-out, light machines, interrupted cuts or full-width slots. Move toward the high end only after test cuts show good chips, low noise and normal tool wear.

    They are the same conservative starting ranges as the Speeds and Feeds Starting Chart in the Handbook, rounded from Machinery's Handbook and published tool-maker starting data for typical coated carbide and HSS tools. Your tool maker's catalogue for the exact tool always takes priority.

    Yes. Switch to Metric and enter diameters in millimetres. Surface speed is then in m/min, chip load in mm per tooth and feed in mm/min, using RPM = Vc × 1000 ÷ (π × D).

    Results are conservative starting points, not guaranteed values. Machine rigidity, tool holding, stick-out, coolant and the exact tool all change what works. Always check against your tool manufacturer's data.