Feed per tooth, written fz, is the distance advanced per cutting edge during one spindle revolution. A feed number in a manufacturer chart is an index that must be converted with the matching diameter row; it is not a feed rate by itself. The selected examples below come from Sutton’s E100 HSS Co.8 slotting guidance and its separate chip-load table. They cover a small subset of steel material groups and tool diameters, not every HSS endmill or milling condition.

HSS Milling Feed per Tooth Chart

How the two tables connect

The Sutton application guide identifies an E100 HSS Co.8 tool configuration and assigns a feed number to each listed material group. For the selected annealed steel groups, the first E100 entry uses cutting speed 30 m/min and feed number 6. The feed table then maps feed number 6 to chip load by nominal tool diameter. For example, a 6 mm cutter maps to 0.018 mm per tooth. It is important to join the material row and diameter table correctly; reading a feed number as millimetres per revolution would produce the wrong machine setting.

Convert chip load to table feed

For a milling cutter, calculate spindle speed from n = (1000 × Vc)/(π × D), where Vc is cutting speed in m/min and D is diameter in mm. Calculate feed rate from vf = fz × z × n, where fz is chip load in mm/tooth and z is the number of cutting edges. If the selected E100 6 mm example has Vc 30 m/min and a two-edge cutter, n is about 1,592 rpm and vf is about 57.3 mm/min using fz 0.018 mm/tooth. Actual spindle and feed commands must also respect machine limits and engagement.

Keep the conditions attached to the number

Sutton describes its guide values as recommendations. The table’s tool setup includes a named tool series, HSS cobalt material, geometry, slotting cut, and axial and radial engagement ratios. The same chip load should not automatically be applied to a different series, a coated tool, a long-reach tool, a different cut type, or a different engagement. Work material hardness and heat treatment also matter. Use the exact current tool catalogue entry when it is available and ask the supplier if the product code has changed.

Adjustments and signs of a poor starting point

The guide notes that long-series tools require a speed reduction of 40 percent and a feed reduction of 20 percent. Those reductions are specific to the source guidance and should not be stacked with unrelated rules without understanding the resulting cut. Chatter, rapid edge wear, built-up material, excessive spindle load, or a poor finish can indicate that the starting conditions do not suit the setup. Check runout, workholding, stick-out, flute count, coolant, chip evacuation, and the actual material before changing a value.

A feed-per-tooth table cannot determine a safe operation by itself. Radial engagement changes the chip thickness, axial depth changes cutting force, and a flexible setup can fail even at a nominally small chip load. Do not increase the programmed feed solely because a displayed value looks conservative. Begin with the product-specific recommendation, observe the cut, and make controlled adjustments within the tool and machine limits.

When documenting a setup, record tool series, diameter, flute count, material condition, Vc, fz, engagement, coolant, and the source guide revision. This lets a later operator distinguish a manufacturer starting value from a value tuned in production. For safety-critical work, use a qualified process review and validate the tool path and workholding before machining.

References

• Sutton Tools Application Guide: HSS Endmills, pages 194–195

These are selected Sutton manufacturer values for a named tool family and operation. Verify the actual cutter, work material, engagement, machine, and revised product data before use.