CNC Routers and Hobby Machines
Feeds and speeds for routers, small mills and desktop CNCs: limited rigidity, high RPM, plastics, wood and aluminum.
What is different about a router
A CNC router (or a desktop mill) has a high-speed, low-torque spindle (10 000 to 24 000 rpm, 0.5 to 2.2 kW), a lighter frame and a gantry that flexes more than a milling machine. So the surface speeds you can reach are high, the cutting forces you can take are low, and the feed rate is often limited by the machine and not by the tool. The rules of the earlier pages apply, but you choose small depths of cut, small stepovers and a chip load the machine can actually deliver.
- Speed is easy; force is the limit. Even a small spindle can spin a 6 mm tool fast; the frame flexes long before the spindle stalls.
- Lower the depth first, then the feed, when anything goes wrong.
- Plastics and wood are the natural materials; aluminum is possible on a good machine with a sharp tool, a light cut and lubrication.
Starting values for a 6 mm router bit
| Material | Tool | Speed | Chip load | Feed rate | Depth per pass |
|---|---|---|---|---|---|
| MDF | 6 mm two-flute up-cut carbide | 18 000 rpm (339 m/min) | 0.150 mm | 5 400 mm/min | 6.0 mm |
| Plywood | 6 mm two-flute compression | 18 000 rpm (339 m/min) | 0.120 mm | 4 320 mm/min | 6.0 mm |
| Hardwood | 6 mm two-flute up-cut | 16 000 rpm (302 m/min) | 0.100 mm | 3 200 mm/min | 4.0 mm |
| Cast acrylic | 6 mm single-flute O-flute | 16 000 rpm (302 m/min) | 0.120 mm | 1 920 mm/min | 3.0 mm |
| HDPE and polyethylene | 6 mm single-flute O-flute | 16 000 rpm (302 m/min) | 0.150 mm | 2 400 mm/min | 4.0 mm |
| Aluminum (6061) | 6 mm two-flute polished carbide, mist | 12 000 rpm (226 m/min) | 0.040 mm | 960 mm/min | 1.5 mm |
| Brass | 6 mm two-flute carbide | 10 000 rpm (188 m/min) | 0.030 mm | 600 mm/min | 1.0 mm |
Chip load is per flute; the feed rate is RPM × flutes × chip load (see Cutting Speed, Spindle Speed and Feed Rate). For other diameters scale the chip load with the diameter and the speed to the same surface speed (see Speeds and Feeds by Material). Start at 70 % of the feed.
When the machine cannot feed fast enough
Worked example: MDF on a machine limited to 3 000 mm/min
- A two-flute 6 mm bit at 18 000 rpm and 0.15 mm per tooth wants a feed of 18 000 × 2 × 0.15 = 5 400 mm/min, but the machine tops out at 3 000 mm/min.
- At that feed and the full RPM the chip load would be only 3 000 ÷ (18 000 × 2) = 0.083 mm: the edge rubs, heats and burns the MDF and dulls quickly.
- Lower the RPM instead, not the feed: at 12 000 rpm the chip load is 3 000 ÷ (12 000 × 2) = 0.125 mm and the surface speed 226 m/min is still plenty for wood.
- This is the opposite of the advice for a machine that is spindle-limited (see Cutting Speed, Spindle Speed and Feed Rate): ask whether the machine or the spindle is the limit, then change the other one.
Aluminum on a router
Worked example: pocketing 6061 with a 6 mm two-flute bit
- The ideal speed for 150 m/min is 7 958 rpm; a router spindle that cannot run below 10 000 rpm gives 12 000 rpm (226 m/min), which is acceptable for aluminum.
- With a chip load of 0.04 mm the feed rate is 12 000 × 2 × 0.04 = 960 mm/min. A 1.5 mm deep, 3 mm wide cut removes 4.3 cm³/min and needs only 0.13 kW at the cutter (see Cutting Force, Power and Torque): power is not the limit; stiffness is.
- The stepover of 3 mm is half the diameter, so no thinning correction. A 1 mm stepover would need a multiplier of 1.34 (see Chip Load, Chip Thinning and Engagement).
- Use mist or an air blast with a lubricant (or a little WD-40-type oil), a polished two-flute tool, shallow passes and a sacrificial board under the work; clamp it rigidly.
Rigidity: where the flex is
A machine’s stiffness is a chain of springs in series: the total compliance is the sum of the compliances, so the weakest link dominates. 1 ÷ ktotal = Σ (1 ÷ ki).
Worked example: a hobby router
| Part | Stiffness (N/µm, typical) |
|---|---|
| Tool (6 mm, 25 mm stick-out) | 15 |
| Collet and spindle | 60 |
| Gantry and linear bearings | 20 |
| Frame and table | 40 |
| Work holding | 50 |
- Total stiffness: 1 ÷ (1/15 + 1/60 + 1/20 + 1/40 + 1/50) = 5.6 N/µm, weaker than any single part. The weakest link is the tool (6 mm, 25 mm stick-out) (15 N/µm).
- A side force of 30 N deflects the tool tip by 30 ÷ 5.6 = 5.4 µm.
- Doubling the stiffness of the gantry from 20 to 40 N/µm only raises the total to 6.5 N/µm: improve the weakest part first (a shorter tool, a larger-diameter tool), because the others barely matter.
- A short, thick tool is the cheapest stiffness: deflection ∝ L³ ÷ d⁴ (see Cutting Force, Power and Torque).
Acceleration and short moves
Worked example: the programmed feed is not the real feed
- A router that accelerates at 500 mm/s² takes v² ÷ 2a = (83.3)² ÷ (2 × 500) = 6.9 mm to reach 5 000 mm/min and as much to stop: a move shorter than 13.9 mm never reaches it.
- On a toolpath of 4 mm segments (a finely sampled curve) the speed is limited to about √(2 a × s ÷ 2) = 45 mm/s = 2 683 mm/min: the chip load falls and the tool rubs although the program says 5 000.
- Fixes: use arcs and smoothed paths (G64 or a blend tolerance), set the acceleration to what the machine can do, and calculate the chip load from the real speed in corners and small features.
Plastics, wood and dust
Worked example: acrylic that melts
- A single-flute 6 mm bit at 16 000 rpm and a chip load of 0.12 mm feeds at 1 920 mm/min; the chip carries the heat away.
- At a feed of only 480 mm/min (chip load 0.03 mm) the tool rubs, the acrylic melts and welds to the flute. For plastics a bigger chip is the cure: raise the feed or lower the RPM.
- Use a single-flute O-flute bit for plastics (large chip room, polished); up-cut bits clear chips and pull the work up, down-cut bits press the work down and give a clean top, compression bits give a clean top and bottom in plywood.
- Dust: MDF and wood make fine dust: use a dust shoe and extraction, wear a respirator and keep the machine in a ventilated space (see Dust, Fumes and Ventilation and Fire, Fuels and Explosion).
- Fire: never leave a router running unattended: a dull bit in wood can ignite.
Holding the work and tabs
- Vacuum table, screws or clamps: the work must not move or lift; hold-downs must be out of the toolpath.
- Tabs (small bridges left in the cut-out) hold a part until the end; cut them with a knife or a sander.
- Sacrificial board under the work: cut 0.2 to 0.5 mm into it so that the part is fully cut through; surface it flat in the machine.
- Zero the Z carefully: a touch plate or a probe, and re-check after a tool change.
- Runout: a collet runout of 0.03 mm makes one flute of a two-flute bit cut 0.08 mm and the other only 0.02 mm instead of 0.05 mm: 60 % more load on one tooth. Use a clean, good collet and tighten it properly.
Troubleshooting
| Symptom | Likely cause | Try |
|---|---|---|
| Wood or MDF burns | Feed too low for the RPM, dull bit | Raise the feed or lower the RPM; sharpen or replace the bit |
| Plastic melts and welds to the bit | Chip too small, heat builds | Larger chip load, single flute, air blast |
| Bit breaks in aluminum | Cut too deep or too fast, chips packed, stick-out too long | Reduce the depth to 1 mm, add mist or air, shorten the tool |
| Chatter and a rough wall | Flex in the machine or the tool | Smaller depth and stepover, shorter tool, change the RPM (see Dialling In: Chatter, Rigidity and Troubleshooting) |
| Corners are rounded or the part is the wrong size | Deflection and acceleration limits | Slow the feed in corners, take a spring pass |
| Part lifts or moves | Poor holding, up-cut bit pulling | Better clamping, tabs, a down-cut or compression bit |
| Steps are lost or the machine skips | Feed or acceleration too high, load too high | Lower the feed and the acceleration, reduce the depth |
Related
- Speeds and Feeds: the overview of this guide.
- Cutting Speed, Spindle Speed and Feed Rate: the formulas and the spindle-limit rule.
- Dialling In: Chatter, Rigidity and Troubleshooting: chatter and tuning.
- CNC Machines and Workflow, Machining Plastics, Wood and Composites and the CNC Feeds and Speeds Calculator.
FAQ
What feed rate should I use on my CNC router?
Feed rate = RPM × flutes × chip load; for a 6 mm two-flute bit in MDF at 18 000 rpm, about 5 000 mm/min if the machine can deliver it; otherwise lower the RPM to keep the chip load.
Why does my router burn the wood?
The feed is too low for the RPM (the chip is too thin and the bit rubs) or the bit is dull; raise the feed, lower the RPM or sharpen the bit.
Can I cut aluminum on a hobby router?
Yes with a sharp polished two-flute bit, light cuts (1 mm deep), a chip load of about 0.04 mm, lubrication and a rigid hold; the machine’s flex is the limit, not its power.
Why is the real feed lower than programmed?
The machine cannot accelerate fast enough on short moves: segments shorter than about 14 mm at 5 000 mm/min never reach the programmed feed.
References
- Tool makers’ guides for router bits and small end mills (Amana, Onsrud, Harvey Tool, Sandvik).
- Oberg, E., et al., Machinery’s Handbook (milling data); Altintas, Y., Manufacturing Automation (machine structural dynamics).
- Machine builders’ manuals (Shapeoko, Onefinity, Carbide 3D, Avid CNC) for feed and acceleration limits.
Last reviewed: October 2026. Chip loads and feeds are typical starting values for hobby machines: begin at 70 % and adjust.