Speeds & Feeds Calculator
RPM and feed with the physics the paid tools hide: chip-thinning compensation, Kienzle cutting power and torque, tool deflection, and your machine's real limits. Free, no login, and every formula is one click away.
Cut definition
Aggressiveness
Scales book speed ±15% and chip load ±20%. Start standard; earn aggressive.
Machine limits
Power is checked at 80% drive efficiency. Limits produce warnings — never silent clamps.
Spindle speed
10,000 rpm
314 m/min
Feed rate
3,695 mm/min
chip load 0.0924 mm/t
Spindle load
20%
2.37 kW (3.18 hp) · 2.3 N·m (20 in·lb) · MRR 92.4 cm³/min
Every number, with its math
- Spindle speed
- 10,000 rpm
- Feed rate
- 3,695 mm/min
- Chip load (programmed)
- 0.0924 mm/tooth
- Avg chip thickness
- 0.0441 mm
- Material removal rate
- 92.4 cm³/min
- Specific cutting force
- 1,538 N/mm²
- Cutting power
- 2.37 kW
- Spindle torque
- 2.3 N·m
- Cutting force (est.)
- 498 N
- Tool deflection (est.)
- 0.0302 mm
Running ~42% under book speed ≈ 5.2× tool life (Taylor, n=0.33). Kienzle constants for Aluminum 6061: kc1.1 = 750 N/mm², mc = 0.25.
Starting values from mid-range handbook data + physics checks — not gospel. Your tool maker's cutting data beats any calculator; this tells you whether a number is sane and what limits you first. Everything runs in your browser.
Engagement — top view
The chip each tooth takes (exaggerated ~×20) — thin where the tooth exits at the surface, thickest at the bottom of the arc: hex 0.0800 mm, average hm 0.0441 mm against a programmed fz of 0.0924mm. Dashed circle = previous tooth's path.
Chip-thinning compensation
Feed multiplier vs. radial engagement (ae ÷ D). Below 50% stepover the chip comes out thinner than fz, so feed goes up to compensate — at your 25% stepover the target 0.0800 mm chip needs 0.0924 mm/tooth programmed. Right of the dashed line, no compensation.
Tool deflection — side view
Estimated tip deflection 0.0302 mm — OK for roughing, too much for finishing. Bend shown ~×94 exaggerated. Stiffness falls with stickout cubed: gripping 24 mm instead would cut deflection roughly in half.
What makes this one “advanced”
A basic calculator multiplies three numbers and stops. The expensive tools — and this one — keep going: they check whether each tooth is actually taking a chip thick enough to cut (chip thinning), whether your spindle has the power and torque to sustain the removal rate (Kienzle model), and whether the tool will bend enough to chatter or snap (deflection). Any of those can be the binding constraint, and the number that matters is whichever limit you hit first.
The difference here is that nothing is a black box. Every output row can show the formula with your numbers plugged in — the same equations from the tooling catalogs and machining handbooks. If a cut trips a limit, the warning says which one and what to change. That's also why the deflection estimate pairs well with the chatter simulator and the feed numbers with the G-code time auditor.
Where do the base numbers come from? Mid-range handbook cutting speeds and chip loads per material, adjusted for operation, coating, and how aggressive you tell it to be — deliberately conservative starting points, because the right way to use any calculator is to start sane and optimize from evidence. When your tool manufacturer publishes data for your exact tool, use theirs.
Frequently asked questions
How are speeds and feeds calculated?+
Spindle speed comes from the surface speed the material can sustain: RPM = (1000 × Vc) / (π × D), where Vc is cutting speed in m/min and D is tool diameter in mm. Feed rate is RPM × number of flutes × chip load per tooth. The advanced part is everything after that: compensating chip load for radial chip thinning, checking the cut against spindle power and torque, and estimating tool deflection — which is what this calculator does, with each formula shown.
What is chip thinning and why does it matter?+
When the radial width of cut is less than half the tool diameter, the chip that each tooth removes is thinner than the programmed feed per tooth. If you don't compensate, the tool rubs instead of cutting — generating heat and wearing out early. The compensation factor is 1 / (2 × √(r × (1 − r))) where r = ae/D; at 10% stepover it means running about 1.67× the book feed. This is the foundation of every HSM/adaptive toolpath strategy.
How is cutting power calculated?+
From the Kienzle specific cutting force model used in tooling catalogs: kc = kc1.1 × hm^(−mc), where kc1.1 and mc are measured material constants and hm is the average chip thickness. Power in kW is then material removal rate (cm³/min) × kc / 60000, and torque is 9550 × power / RPM. This calculator uses published kc1.1 values from roughly 700 N/mm² for aluminum up to 4600 N/mm² for hardened steel.
How accurate is the tool deflection estimate?+
It models the tool as a stepped cantilever — the fluted section at a reduced core diameter plus the shank — loaded with the estimated cutting force, which is the same approach professional calculators use. It's an estimate for judgment, not a simulation: below ~0.01 mm you're fine for finishing, up to ~0.025 mm is workable roughing, and beyond that expect chatter, taper, and broken tools. Stickout matters cubed, which is why shortening it is always the first fix.
Should I trust a calculator over my tool manufacturer's data?+
No — when you have the manufacturer's cutting data for your exact tool and material, use it. A physics-based calculator earns its keep everywhere else: unbranded tooling, materials not on the chart, sanity-checking whether a cut exceeds your machine's power, torque, or rigidity, and understanding which limit binds first. That's why every number here shows its formula.
Why is my calculated RPM higher than my spindle can go?+
Small tools in soft materials often want more RPM than the machine has — a 3 mm endmill in aluminum wants 30,000+ RPM at full surface speed. The calculator caps RPM at your machine limit and tells you the surface speed you're actually getting. Running slower than book speed is safe (tool life goes up); the mistake to avoid is keeping the feed calculated for the higher RPM.
Optimizing cycle times or building shop software?
This calculator is a taste of what I build — from feed optimization to full machine-data tooling.