Cutting data per Stepcraft's official milling-parameter chart. Metric, single-flute to 4-flute end mills.
Defaults: AMB 1400 FME-P DI milling motor — 3 500 to 25 000 rpm, ER16 collet system (max 10 mm shank).
Spindle speed n
–rpm
How fast the spindle turns. Calculated from the material's cutting speed and the effective tool ø: n = vc·1000/(π·d). Set this on your spindle / milling motor. If it exceeds your spindle's max, it's capped — and the feed below is recalculated to keep the chip load correct.
Feed rate vf
–mm/min
How fast the machine travels through the material while cutting (XY). vf = rpm × flutes × chip load. Use as cutting feed in your CAM. Too slow: tool rubs, heats up and dulls. Too fast: overload, deflection, breakage. When unsure, keep rpm and reduce feed slightly — never crawl.
Plunge rate (≈⅓ feed)
–mm/min
Rule of thumb — ramp in where possible
Feed for straight-down Z moves. End mills cut poorly straight down (center of the tool barely cuts), so plunge at roughly ⅓ of the cutting feed — or better, let CAM ramp or helix into pockets and avoid straight plunges entirely.
Ramp entry
–
The better way into a pocket: descend at a shallow angle while moving, instead of drilling straight down. Set both in your CAM's lead-in/ramp settings. Shallow angles for metals (the tool can't clear chips going down), steeper is fine in wood and foam. A helix with the same angle works even better — constant engagement, chips fall clear. If your CAM asks for a ramp feed, use the value shown; the vertical component stays well below the plunge limit.
Stepover
–
How far the tool steps sideways between passes. Depends on the operation: • Slotting: 100% engagement by definition — respect the depth-per-pass limit. • Adaptive / trochoidal clearing: 10–15% of ø at full cutting depth. • Conventional pocket / facing: 40–50% of ø at reduced depth. • Contour finishing: 25% of ø at full depth (Stepcraft's recommendation) — the value shown. • Ballnose 3D finishing: stepover sets scallop height: s = √(8·r·h). Shown for h = 0.02 mm scallop — halve it for showroom surfaces.
Max depth per pass (slot)
–mm
How deep to cut in one pass when slotting (full-width groove). Stepcraft M-Series guideline: wood/plastics 0.75 × ø, non-ferrous metals 0.2 × ø. Deeper passes load and deflect the tool more. Alternative: full-depth contour passes with only 25% ø sideways engagement.
Effective cutting ø–
The diameter actually engaged in the cut. Flat end mills cut at full ø. Ballnose and V-bits cut on a curve/taper, so at shallow depth the working diameter is much smaller — rpm and chip load here are computed from this value, not the shank ø.
Cutting speed vc (effective)–
Surface speed of the cutting edge through the material, in m/min. It's a material constant from Stepcraft's chart (adjusted for cut type and HSS). Shown here is the actual value at the displayed rpm — if rpm was capped by your spindle, this is lower than the chart target. Harmless: the cut is just slower.
Chip load fz (from chart)–
Thickness of the chip each cutting edge takes per revolution, mm/tooth. From Stepcraft's chart for the material, interpolated for your effective ø. The single most important number for tool life: too small and the tool rubs instead of cutting (heat, dulling); too large and it chips or snaps.
Formulasn = vc·1000/(π·d) · vf = n·z·fz
Reference chart — Stepcraft benchmark values
Source: Stepcraft milling parameters (SC_milling-parameters.pdf). Depth-per-pass uses M-Series factors: non-ferrous metals 0.2×ø, wood/plastics 0.75×ø. Values are starting points — listen to the cut.