Feeds and Speeds¶

In one sentence: Feeds and speeds are the two most critical cutting parameters — spindle RPM controls how fast the tool rotates; feed rate controls how fast it moves through the material — and choosing them correctly prevents tool breakage, poor surface finish, and wasted material.

The two fundamental parameters¶

Spindle speed (RPM) — how many revolutions per minute the cutter makes. Too slow: rubbing instead of cutting, built-up edge, poor finish. Too fast: thermal damage, tool breakage.

Feed rate (mm/min) — how fast the tool moves through the material. Too slow: re-cutting chips, work hardening (metals), heat build-up. Too fast: tool deflection, breakage, chatter.

The two parameters are linked: increasing RPM while holding feed rate constant means each cutting edge takes a smaller chip (lower chip load). Decreasing RPM while holding feed rate constant means larger chips (higher chip load). The target is a chip load in the manufacturer's recommended range.

Calculating spindle speed (RPM)¶

RPM is set by the desired surface speed (also called cutting speed — the speed of the cutter's edge as it passes through the material):

RPM = (Vc × 1000) / (π × D)

where:
  Vc  = surface speed  (m/min)
  D   = tool diameter  (mm)
  π   ≈ 3.1416

Simplified to a practical form:

RPM ≈ (Vc × 318.3) / D

Recommended surface speeds by material¶

Material	Surface speed Vc (m/min)	Notes
Aluminium (6061)	200–500	Use coolant or air blast; carbide preferred
Aluminium (cast)	150–350	More abrasive; reduce speed
Mild steel (1018)	30–60	Requires coolant; HSS or carbide
Stainless steel (304)	20–40	Work-hardens — maintain constant feed
Titanium	15–30	Coolant essential; carbide required
Hardwood	100–200	Dry; sharp tool critical
Softwood / MDF	150–300	Dry; chip-load larger than hardwood
HDPE	150–400	Dry or mist; avoid melting chips
Acrylic / PMMA	100–250	Sharp tools; allow chips to clear
Brass	80–200	Dry; free-machining alloys at the higher end
Carbon fibre (CFRP)	100–250	Dust extraction essential; wear PPE

Always verify against your tool manufacturer's data

These are starting values. The correct speed depends on tool coating, number of flutes, machine rigidity, coolant strategy, and depth of cut. Indexed insert tooling can run 2–5× faster than solid carbide figures above.

Example: 6 mm end mill in 6061 aluminium¶

Vc = 300 m/min (mid-range for aluminium)
D  = 6 mm
RPM = (300 × 318.3) / 6 = 15,915 RPM

Most hobby CNC routers run 10,000–24,000 RPM; the calculated value fits.

Calculating feed rate¶

Feed rate is set by the desired chip load — the thickness of material each cutting edge removes per revolution:

feed_mm_min = RPM × chip_load_mm × number_of_flutes

Recommended chip loads by material¶

Material	Chip load (mm) per flute
Aluminium (6061)	0.03–0.08 (3 mm tool) to 0.08–0.15 (12 mm tool)
Mild steel	0.01–0.04
Stainless steel	0.008–0.03
Hardwood	0.03–0.10
Softwood / MDF	0.05–0.15
HDPE	0.04–0.12
Acrylic	0.03–0.08

Chip load increases with tool diameter. A small tool requires a smaller chip load to avoid breakage; a large tool can take a bigger chip.

Example: 6 mm 2-flute end mill in 6061 aluminium¶

RPM       = 15,915 (from above)
chip_load = 0.05 mm (conservative for a 6 mm tool in aluminium)
flutes    = 2
feed      = 15,915 × 0.05 × 2 = 1,592 mm/min  ≈ 1600 mm/min

Plunge feed rate (VertFeed)¶

The plunge feed rate (Z-axis downward movement into the material) is typically 25–50 % of the horizontal feed rate:

VertFeed ≈ feed_mm_min × 0.3

Centre-cutting end mills can plunge directly; non-centre-cutting tools require a ramped entry — use a Ramp Entry dress-up.

Radial and axial engagement¶

The formulas above assume full-width radial engagement (slot milling). Reducing engagement multiplies the effective feed rate:

Radial engagement (% of diameter)	Feed rate multiplier
100 % (slotting)	× 1.0 (base values)
50 %	× 1.3–1.5
25 %	× 2.0–2.5
10 %	× 3.0–4.0

Adaptive Clearing automatically maintains a constant engagement angle, which is why it can run at significantly higher feed rates than conventional pocketing.

Setting feeds and speeds in FreeCAD¶

FreeCAD does not auto-calculate feeds and speeds. Values must be entered manually in the Tool Controller:

Field	Enter
`HorizFeed`	Horizontal feed rate (mm/min)
`VertFeed`	Plunge feed rate (mm/min)
`SpindleSpeed`	RPM
`SpindleDir`	CW for most end mills

SpindleSpeed defaults to 0

A new Tool Controller has SpindleSpeed = 0. The post-processor will write S0 in the G-code — the machine spindle will not start. Always set a non-zero RPM before post-processing.

Common problems and their causes¶

Symptom	Likely cause	Fix
Tool breaks immediately	Feed too high or plunge too fast	Reduce feed; use ramp entry
Chatter / vibration	RPM too low or feed too high	Increase RPM; reduce feed; shorten tool stick-out
Poor surface finish (rough)	Chip load too high (chips tearing)	Reduce feed or increase RPM
Melting chips (plastics)	RPM too high	Reduce RPM; clear chips actively
Rapid tool wear	Surface speed too high	Reduce RPM
Rubbing, built-up edge	Surface speed too low	Increase RPM
Work hardening (stainless)	Feed too low — tool rubbing	Increase feed; maintain constant engagement