By the end of this page you will have a short spec for one solid carbide end mill: flute count, end profile, length, coating and helix, matched to one material and one operation. It takes about ten minutes with a catalog open. Choose for the material first and the tool second, because a cutter that runs well in aluminum is not evidence it will survive stainless.

What you need

  • The workpiece material and its hardness

    Grade, not family. "Steel" is not a spec. Above HRC 50 the choices narrow sharply.

  • The operation and the depth of cut

    Slotting, roughing, finishing or HEM, plus the deepest feature measured in tool diameters.

  • The machine's top RPM and an honest read on its rigidity

    A knee mill and a VMC do not get the same answer.

  • A supplier catalog that publishes geometry

    It needs helix angle, core, coating and flute length per item. If the listing gives only diameter and price, it is not enough to choose from.

The steps

1. Write down the material and hardness. You have it when one row of the table below applies and you are not torn between two.

2. Name the operation. Pick one of slotting, traditional roughing, finishing or high-efficiency milling. If the job needs two of them, you are buying two tools.

3. Pick the flute count from the table. Harvey Performance gives 2 or 3 flutes for non-ferrous work. For ferrous work it gives 4 for slotting, 3 to 5 for roughing, 5 to 7 for HEM and 5 to 14 for finishing. Fewer flutes clear chips better and more flutes leave a better finish. Count flutes against the radial engagement, not on their own. A 6-flute tool buried in a full-width slot has nowhere to put the chips.

4. Choose the end profile. Square for flat-bottom slots and 90° shoulders. Corner radius wherever the print allows it, because the corner is where carbide chips first. Ball for 3D surfacing. Above HRC 50, use corner radius or ball only. The check: the corner the tool leaves matches the corner on the drawing.

5. Choose the shortest length that reaches the feature. Shorter tools are stiffer and cheaper. Past about 5x diameter of reach, Harvey recommends a necked tool over a long-flute one. Done right, the holder clears the part with the least stickout that clears it.

6. Choose the coating. Use the table. If no coating in the table suits the material, a sharp, polished uncoated tool is a legitimate answer for aluminum.

7. Choose the helix. General-purpose tools sit around a uniform 30°. Suppliers cite 35° to 45° high helix for lifting chips in aluminum, which buys sharpness at the price of more axial pull on the holder. Variable helix, for example flutes alternating 37° and 35°, is there to break up chatter. Buy it if the machine or setup is the weak link.

8. Decide general-purpose or high-performance. Per Cutting Tool Engineering, general-purpose mills (2 to 4 flutes, AlTiN or TiCN) cost 20% to 40% less than high-performance tools (5 to 12+ flutes, variable helix, TiAlSiN or AlCrN). The premium tools are built for repetitive production with trochoidal and adaptive clearing toolpaths. A job shop with varied work and conservative parameters gets most of the result from the cheaper tool. Price both now rather than from memory. The AMT/USCTI market report for July 2026 attributed double-digit carbide cost increases to a carbide materials shortage, hitting larger diameters hardest.

Material Flutes Coating Helix / notes
Aluminum, brass, plastics 2 to 3 (1 to 2 on a router) TiB2, ZrN, DLC, or polished uncoated High helix, polished flutes
Carbon and alloy steel 4 to 6 AlTiN, TiAlN, AlCrN Standard helix; variable if it chatters
Stainless steel 3 to 5 AlCrN over AlTiN for sustained heat Sharp edge, stable core
Hardened steel 4 to 8 TiAlSiN for HRC 45+ Corner radius or ball above HRC 50, short overhang
Highly abrasive non-metallics Per operation Amorphous or CVD diamond Diamond runs cooler: 600 to 800°C max

The flute ranges are a composite of supplier guides, and the suppliers disagree at the edges. The coating temperatures come from Sonic Tools: AlTiN to 900°C, AlCrN 900 to 1,100°C, TiAlSiN 1,000 to 1,200°C. These are vendor figures, not independent tests.

If it did not work

Check the coating first. AlTiN reacts with aluminum, so a 'premium' AlTiN tool is the wrong tool here. Switch to TiB2, ZrN or polished uncoated, and drop to 2 or 3 flutes for chip room.

Geometry cannot cancel overhang or spindle runout. Shorten the stickout, move to a stub or necked tool, then reassess. On a low-rigidity machine, variable flute and variable helix tools are still the forum consensus for full-width cuts.

Look for recut chips. Machinists on Practical Machinist describe edge failure as near-instant once chips get wedged back into the cut. Fix evacuation with fewer flutes, more coolant or air, or less radial engagement. Then add a corner radius.

Check the spindle. Carbide needs surface speed that RPM-limited knee mills often cannot reach, and forum machinists report quality HSS roughers outperforming carbide there. Coated cobalt is the forgiving option for setups that are less than rigid.

Done, and then

You now have a tool spec you can defend line by line and order against. The next decision is the toolpath that tool will run, since flute count and HEM only pay off together.

Match the tool to the toolpath

Climb versus conventional, trochoidal and adaptive clearing, and where each one fits.

CNC machining techniques