PICK YOUR TOOL. DIAL IN THE CUT.

Speeds & Feeds
Calculator

Find a starting spindle speed and feed rate for end mills, face mills, drills and lathe tools from any brand. Choose your material, tool and machine to see chip load, depth of cut and the spindle power the cut needs, with values ready to enter in Fusion. Works in inches or millimetres, from hobby routers to industrial machining centres.

General guidance from common shop references. Results are estimates; always check your setup and wear eye protection. Learn It! isn’t responsible for anything broken, damaged, etc but we’d love to hear what worked for you. Use these tools at your own risk.

Any tool brand / mill, drill + lathe

Find your starting point.

Work down the four steps: what you’re cutting, what you’re cutting with, your machine and how you’re cutting. The result updates as you go, with the values to enter in Fusion.

Units
Operation

1What are you cutting?

6061, 7075, 2024, 5052. Machines fast and easy. The danger is chips welding to the tool, not heat or force.

2What are you cutting with?

Tool material

Uncoated solid carbide or carbide inserts. 3–4 × faster than HSS. The best choice for aluminum, plastics and wood.

Tool shape
in
Stickout and flute length
in

Blank = 3 × diameter.

in

Caps the depth of cut.

3What’s your machine?

Fills in the fields below. Change any of them to match your machine.

hp
RPM
Speed and feed limits
RPM
in/min

Blank = no limit.

4How are you cutting?

Toolpath

Fusion Adaptive Clearing: small stepover, full flute depth, faster feed. The best choice on most machines.

Coolant
Approach

Start conservative on a new setup, a long tool or a part you can’t afford to scrap.

Set my own width and depth
in
in

Leave blank to use the recommended value (shown greyed out). Type a percentage like “10%” to use a share of the tool diameter.

19,100 RPM · 125 in/minSee result ↓

Starting point

Adaptive · 1/4 in 3-flute carbide end mill · Aluminum, wrought

Spindle speed 19,100 RPM 1,250 SFM · 381 m/min
Feed rate 125 in/min 3,175 mm/min
Feed per tooth (program)
0.0022 inReal chip 0.0014 in (chip thinning × 1.58)
Stepover
0.028 in11 % of D
Stepdown
0.200 in0.80 × D
Metal removal
0.703 in³/min
Ramp feed
47.4 in/minHelix or ramp at ≤ 3°
Plunge feed
19.7 in/minCenter-cutting tools only
Tool deflection (est.)
Low 0.0001 inStickout 0.750 in (3.0 × D)
Spindle power0.41 hp needed of 2.4 hp available (17 %)

Your spindle makes about 2.4 hp at 19,100 RPM (3.0 hp at full speed). The line marks 80 %, the most this calculator plans for.

  • In Fusion Adaptive Clearing, set Optimal load to the stepover and Maximum stepdown to the depth. Feed optimization is not needed: chip thinning is already included.
  • Clear chips with air or mist. Re-cutting chips is the most common way to break a tool in aluminum.
  • Use 2–3 flutes for slots and pockets (1 flute on light routers). Uncoated, ZrN or DLC tools; avoid AlTiN.

Enter these in Fusion
Spindle speed19,100 rpm
Surface speed1,250 SFM
Ramp spindle speed19,100 rpm
Cutting feedrate125 in/min
Feed per tooth0.0022 in
Lead-in / Lead-out feedrate125 in/min
Ramp feedrate47.4 in/min
Plunge feedrate19.7 in/min
Maximum ramp angle (Passes)3°
Optimal load0.028 in
Maximum stepdown0.200 in

Field names as they appear in Fusion’s tool library (Feed & speed tab) and toolpath Passes tab.

Starting chart: aluminum, wrought, carbide, adaptive
DiameterRPMPer toothFeedDepth
1/16 in24,0000.00072 in51.8 in/min0.050 in
1/8 in24,0000.0013 in90.2 in/min0.100 in
3/16 in24,0000.0017 in125 in/min0.150 in
1/4 in19,1000.0022 in125 in/min0.200 in
3/8 in12,7300.0030 in115 in/min0.300 in
1/2 in9,5500.0038 in109 in/min0.296 in
5/8 in7,6400.0045 in104 in/min0.205 in
3/4 in6,3700.0053 in100 in/min0.152 in
1 in6,0000.0066 in119 in/min0.094 in

Uses your machine, 3 flutes, coolant and approach, with the recommended width and depth for each size.

Show the math
  1. Surface speed: 1000 SFM base for carbide in aluminum, wrought × 1.25 (adaptive) × 1 (coolant) × 1 (balanced) = 1250 SFM.
  2. Chip load: 0.0040 in at ½ in, scaled for diameter (× 0.57), tool material (× 1), rigidity (× 0.60), stickout (× 1), approach (× 1) and toolpath (× 1) = 0.00138 in per tooth.
  3. Width and depth: stepover 11 % of D, depth 0.80 × D (from the material, toolpath, rigidity and approach).
  4. Chip thinning: at 11 % of D the chip is thinner than the feed per tooth, so the programmed feed per tooth goes up × 1.58 to keep the real chip at 0.00138 in.
  5. Spindle speed: 1250 × 12 ÷ (π × 0.2500) = 19,100 RPM.
  6. Feed: 19,100 RPM × 3 flutes × 0.00218 in = 125 in/min.
  7. Power: 0.703 in³/min × 0.3 hp per in³/min × 1.51 (chip thickness) × 1.1 (tool wear) ÷ 0.85 (drive efficiency) = 0.41 hp at the motor.
  8. Deflection: cutting force ≈ 9 lbf on a 0.650 in lever, tool core 0.8 × D, E = 87 Mpsi → 0.00012 in.
How to use these numbers
  1. These are starting points, not limits. If your tool maker publishes numbers for that exact tool, use theirs.
  2. Run the first cut at the speed shown and 70–80 % of the feed, then bring the feed override up while you watch and listen.
  3. Squealing or chatter: lower the RPM about 10 %, or reduce the stickout or width of cut. Don’t just slow the feed; that makes the tool rub.
  4. Blue or burnt chips in steel, or melted chips in plastic: too much heat. Lower the RPM or raise the chip load.
  5. Chips should come off clean, curled and the same colour as the material (light straw is fine in steel with carbide).

General guidance from common shop references. Results are estimates; always check your setup and wear eye protection. Learn It! isn’t responsible for broken tools, but we’d love to hear what worked for you.

Report a bug