Milling inserts are chosen differently from turning inserts. In turning the tool is continuously engaged, so heat builds steadily. In milling each tooth cuts and then runs free in air, so the tool is thermally cycled — hot in the cut, cool out of it. That single fact explains most of the choices below.
Step 1 — Match the insert to the cutter type
| Cutter | What it does | Typical insert families |
|---|---|---|
| Face mill (45°) | General face milling, light chips, good surface | SEHT, SDMT, ADMT, ONHU |
| Square shoulder mill (90°) | True 90° walls, steps, pockets | APKT, APMT, RDMT, LNHU |
| High-feed mill | Very high table feed at small ap | HNGX, LNGX, HNMX |
| Round insert mill | Roughing, hard skins, dies | RDMW, RPMT, RPMW |
| Slot / copy mill | Full-width slots, profiling | SDMW, ODMT, SEKT |
| Chamfer / dovetail | Edges, T-slots, chamfers | APHT, AOHT, specials |
Step 2 — Lead angle changes everything
The lead angle (entering angle) is the angle between the cutter’s axis and the cutting edge. It decides how the chip thins and where the force goes:
- 45° — chips thin out, so you can run higher feed per tooth. Axial force is higher, so it pushes the workpiece down. Good all-round face milling, good surface finish, can mill up to a shoulder with a small step.
- 90° — true square shoulder. Radial force dominates, so it is hard on slender setups and the surface finish at the wall is worse. Use it when you need 90°.
- Small lead (10–25°, high-feed) — the chip is extremely thin and the force is directed almost entirely into the spindle axis. This is how high-feed milling reaches 3–4 mm feed per tooth at 0.5–1 mm depth of cut.
Step 3 — Geometry: light, medium, heavy
Most milling insert ranges offer the same shape in two or three geometries. The code letters at the end of the designation (for example MM4, MR2, MM3) mark the intended duty:
- Light / finishing (L) — sharpest edge, lowest force, best finish. Will chip on scale or interrupted cuts.
- Medium (M) — the default. Handles most work. In our range the most stocked milling chipbreakers are PB1, PC2, KC2, MM4, MC3, MM3.
- Heavy / roughing (H or R) — strongest edge, needs high feed to work. Use on castings, scale, and interrupted cuts.
Step 4 — Grade from the material group
Same ISO 513 logic as turning, but milling grades need thermal-shock resistance because of the cycling:
| Group | Grades most stocked | Note |
|---|---|---|
| P – Steel | AP251U, AC152P, AC252P, AT210A | Mainstream steel face and shoulder milling |
| M – Stainless | AP200M, AP301M, AP351M, AP403M | Use sharp edge, avoid rubbing |
| K – Cast iron | AC151K, AC301K, AP251K, AT202 | Dry cutting normal; watch the casting skin |
| N – Aluminium | HS6120, HS7125, HS8115, PD20 | Polished, sharp, no steel-style coating |
| S – Superalloys | AP100S, AP351M, AC200M | Low speed, constant feed |
| H – Hardened | PB30, PB60, AP153H | Hard milling above ~45 HRC |
Step 5 — Feed per tooth, not feed per revolution
This is where most milling problems start. In turning you set mm/rev; in milling you must think in mm per tooth (fz):
vf = fz × z × n where z = number of teeth, n = rpm
The average chip thickness is what the edge actually sees, and it is smaller than fz whenever the radial engagement is small:
havg ≈ fz × √(ae / Dc)
So with a 50 mm cutter taking a 5 mm radial cut, √(5/50) = 0.32 — the real chip is under a third of your programmed fz. If you program 0.05 mm/tooth in that situation, the edge is effectively rubbing at 0.016 mm, work-hardens the surface, and wears out fast. When ae is small, increase fz. This is the single most useful milling rule.
Climb milling versus conventional
Use climb (down) milling by default: the chip starts thick and ends thin, the tool is pushed away from the finished surface, and tool life is better. Conventional milling is only preferable on very hard skins, on old machines with backlash, or when the fixture cannot take the climb force.
Frequently asked
Should I use coolant in milling?
For steel, usually yes for tool life — but watch that you are not thermally shocking the insert. Cast iron, run dry. Aluminium, use flood or air blast to clear chips. Hardened steel and most high-temperature alloys, run dry: coolant causes thermal cracking of the edge.
Why does my insert chip at the start of the cut?
Almost always the entry. Switch to climb milling, reduce the radial engagement, or use a tougher geometry. Chipping on exit is the opposite problem — the chip welds to the edge as it thins out, so raise fz.
How many teeth should the cutter have?
Enough that at least one tooth is always engaged (otherwise the feed is interrupted and the tool hammers), but not so many that chips cannot clear. For roughing with limited spindle power, a coarse-pitch cutter with fewer teeth lets you take a deeper cut.
Related guides
- ISO 513 material groups explained
- Carbide grades explained
- Chipbreaker selection guide
- Cutting parameters calculator
- Browse all milling inserts
Standards and further reading
The material group definitions used throughout this site follow ISO 513. The manufacturer links below are independent technical references.