For stainless-steel milling, a useful starting value depends on the actual alloy, tool geometry, engagement, and machine setup. Haas publishes one such tool-specific reference for its six-flute HEPM solid-carbide end mills. The table below reproduces only the sheet’s ISO 13 stainless-steel group and listed inch diameters, so readers can choose a starting row without treating the numbers as universal stainless-steel settings.

Haas HEPM stainless-steel milling speeds and feeds

Definitions and units

Cutting speed is surface feet per minute (SFM); spindle speed is revolutions per minute (rpm); feed per tooth is inches per cutting edge per revolution; table feed is inches per minute. Haas lists 480 SFM for this material group. For the 1/2-inch tool, the sheet gives 3,680 rpm, 0.0041 in/tooth, and a table feed of 91 in/min. Because the end mill has six flutes, the basic feed relation is Vf = n × z × fz: 3,680 × 6 × 0.0041 is about 90.5 in/min, which rounds to the published 91.

The Haas sheet’s side-cutting conditions are 0.05D radial engagement and 3.0D axial depth. Those conditions matter: a full slot, a long-reach tool, or a different toolpath can impose very different cutting loads. The sheet also gives a specific adjustment when the tool’s length of cut is below 3D; consult that instruction rather than assuming the listed table feed applies unchanged.

Choose the correct row

Match the cutter diameter and confirm the workpiece belongs to the listed ISO 13 stainless-steel group. “Stainless” includes a wide range of austenitic, ferritic, martensitic, precipitation-hardening, and duplex grades. The source does not separate every grade or hardness. It is therefore a tooling-family reference, not a complete material database. If your alloy is heavily work-hardening, hardened, or difficult to chip, follow current Haas or cutter-maker recommendations for that exact grade.

Worked example and setup checks

For a 3/8-inch HEPM cutter on a machine capable of 4,910 rpm, start with the table’s 0.0035 in/tooth and 102 in/min under the stated engagement. Verify that the machine can hold the programmed speed, the workholding is rigid, and coolant reaches the cut. Check chip shape, sound, spindle load, and tool wear on a controlled first pass. A catalog setting does not certify tool life or surface finish.

If the part requires a slot rather than side cutting, do not use this table without checking the appropriate slotting guidance. If the cutter’s length of cut differs from the source condition, apply the manufacturer’s adjustment. Reduce the starting load when the setup has long stickout, weak workholding, interrupted engagement, or poor chip evacuation.

Two common mistakes

One mistake is copying the 480 SFM value to a different end mill or stainless alloy. The number belongs to the HEPM series and this material group. Another is calculating table feed with the wrong flute count. Use the actual cutting edges and the source’s feed-per-tooth value; do not multiply by tool diameter or assume every end mill has the same number of flutes.

Source: Haas HEPM Speeds & Feeds. The maker’s sheet governs any current product-specific update.

Document the actual cut

Write down the exact cutter part number and flute count with the workpiece grade and hardness. Record radial and axial engagement, coolant, stickout, and programmed rpm and feed. Those details make the manufacturer starting point reproducible and help diagnose whether a poor result came from tooling, material, or setup. If you change cutter family, insert geometry, or toolpath, revisit the appropriate manufacturer table instead of carrying the same values forward.

Tool wear also changes the cut. A worn edge may rub and work-harden some stainless grades, while a fresh edge can behave differently under otherwise identical settings. Use a controlled trial, inspect the edge and chips, and track the number of parts or cutting time before adjusting values. This table does not specify a tool-life limit or surface-finish guarantee.