Material guide
6061 aluminum feeds and speeds for desktop CNC
Published chip loads and surface speeds for milling 6061 aluminum with 1/8", 1/4" and 1/2" end mills, how MillCaliber's estimates compare, and how to stop chips welding to the cutter on a router-class machine.
1. Quick answer
For a 1/4" two-flute carbide end mill in aluminum, published chip loads mostly fall between about 0.002 and 0.006 in per tooth (0.05–0.15 mm), depending on the tool series and the cut. Amana's aluminum-cutting chart lists 0.004 in per tooth for a 1/4" two-flute tool in a full-width slot at 600 SFM (9,200 RPM, 74 in/min).
Aluminum problems on light machines are usually about chips, not spindle speed: chips that are too thin, chips that are not cleared, and chips that weld to the cutter. Use one to three flutes, keep a real chip, clear chips with air or a mist, and reduce depth or stepover rather than feed when the machine struggles.
Open the calculator with 6061 aluminum selected2. Published chip loads
Each figure is for a specific tool series, cut and machine. Use the figure for the end mill you actually run.
| Tool (maker, series) | Diameter | Flutes | Chip load (in/tooth) | Stated conditions |
|---|---|---|---|---|
| Amana aluminum-cutting 55° helix end mill | 1/4" | 2 | 0.004 | Slot, 100% width, depth 25% of D; 600 SFM, 9,200 RPM, 74 in/min |
| Onsrud 63-600 aluminum series (as listed by CNC Router Store) | 1/8" · 1/4" · 1/2" | — | 0.002–0.004 · 0.003–0.006 · 0.008–0.010 | Ranges by diameter |
| Onsrud 63-000 single flute (as listed by CNC Router Store) | 1/8" · 1/4" · 1/2" | 1 | 0.006–0.008 · 0.007–0.009 · 0.009–0.011 | Ranges by diameter |
| Productivity RedLine 5-flute aluminum end mill | 1/4" | 5 | 0.0015 (slot) to 0.0024 (side roughing) | 600 SFM slotting, 800–1,000 SFM side roughing |
| University of Pennsylvania MEAM guide (carbide end mills) | 1/8" · 1/4" · 1/2" | — | 0.001 · 0.002 · 0.004 | General shop guidance, 600+ SFM |
| RobbJack A1-201 2-flute (6061 page) | 1/8" · 1/4" · 1/2" | 2 | 0.0032 · 0.0064 · 0.0128 | 60,000 RPM, rigid setup, roughing and profiling |
The spread is wide because these are different tools on different machines. CNC Router Store notes that the two Onsrud series it lists disagree, and RobbJack's figures assume a 60,000 RPM high-speed spindle and a rigid setup. None of these are results measured on a desktop or belt-driven machine.
3. Surface speed: why sources disagree
Published surface speeds for aluminum range from about 600 SFM (Amana slotting, Productivity slotting, UPenn "600+") through 720–1,080 SFM (Helical's aluminum parameters) to around 3,900 SFM for a 1/4" tool at 60,000 RPM (RobbJack). Carbide tools in aluminum are often limited by spindle speed and machine stiffness rather than by the tool's own speed limit.
On a typical 24,000 RPM router spindle, the maximum surface speed is set by the cutter diameter:
| Cutter | SFM at 24,000 RPM | RPM for 600 SFM | RPM for 1,200 SFM |
|---|---|---|---|
| 1/8" | 785 | 18,300 | above 24,000 |
| 1/4" | 1,571 | 9,200 | 18,300 |
| 1/2" | 3,142 | 4,600 | 9,200 |
CNC Router Store's guide to aluminum welding says 24,000 RPM is usually too fast on a router, and that 12,000–16,000 RPM often fixes welding on its own, provided the feed keeps a real chip. Helical's notes add that when the recommended speed can't be reached on small tools, the machine's maximum RPM is used.
MillCaliber's 1,200 SFM aluminum target is labeled unvalidated. It sits inside this published range, but no source checked so far specifies it for the cutter type MillCaliber assumes. Use your tool maker's surface speed, and enter your spindle's real minimum and maximum RPM in the calculator.
4. How MillCaliber's estimates compare
MillCaliber's 6061 baseline is 1,200 SFM and 0.0023 in per tooth for a 1/4" cutter on a rigid machine. Its estimates for a 1/4" two-flute end mill, adaptive pocketing at 50% width of cut, with each machine class's default limits:
| Machine class | RPM | Chip load (in/tooth) | Feed (in/min) |
|---|---|---|---|
| Rigid / ball-screw | 18,000 | 0.0023 | 82.8 |
| Semi-rigid benchtop | 18,000 | 0.0017 | 62.1 |
| Desktop / belt-driven | 18,000 | 0.0013 | 45.5 |
The rigid-machine chip load sits at the low end of the published 1/4" figures. The desktop and semi-rigid estimates are lower, because MillCaliber's machine factors (0.55 and 0.75) reduce chip load on less stiff machines. Those factors are unvalidated heuristics. RobbJack and CNC Router Store both list a chip load that is too low as a cause of chip welding in aluminum, so a lower chip load is not automatically gentler.
If your machine can hold it, the tool maker's chip load is the better reference. To reduce cutting force on a light machine, reduce depth of cut or stepover first, keep a real chip, and recalculate. See the Methodology for how the estimate is built.
5. From chip load to feed rate
Feed (in/min) = RPM × number of flutes × chip load (in/tooth)
Example from Amana's chart: 9,200 RPM × 2 flutes × 0.004 in ≈ 74 in/min. If your machine can't reach the feed for a given RPM, lower the RPM with it, so the chip stays the same. Lowering only the feed at the same RPM thins the chip.
6. Chip welding and built-up edge
Aluminum can cold-weld to the cutting edge under heat and pressure, forming built-up edge. Once a flute is packed, the tool usually breaks or ruins the part. The causes and fixes listed by RobbJack and CNC Router Store:
| Likely cause | Try first |
|---|---|
| Chip load too low (the edge rubs instead of cutting) | Raise the feed into the published range, or lower RPM with the feed |
| Chips not leaving the cut, so they are recut | Air blast into the cut; fewer flutes; adaptive clearing instead of full slots |
| No lubrication | Mist or minimum-quantity lubrication (MQL), see section 7 |
| Too many flutes for the chip room | One to three flutes; CNC Router Store says a 4-flute tool packs its gullets in aluminum on a router |
| Conventional milling | Climb milling, so the chip thins as it leaves the cut (RobbJack) |
| Uncoated or wrong coating | Polished uncoated or an aluminum coating such as DLC (RobbJack); RobbJack pairs AlTiN with steels, not aluminum |
Clean any built-up aluminum off the cutter before trying again; a tool with welded aluminum on its edge will keep welding.
7. Air, mist and coolant
Sources disagree on what is needed. RobbJack recommends flood coolant or air blast. CNC Router Store says air alone is not enough for aluminum on a router and recommends minimum-quantity lubrication: a small metered amount of lubricant carried by air, rather than flood coolant, which it considers impractical on most routers. Both agree that chips must be cleared from the cut.
Check what your machine maker allows before adding any liquid lubricant or coolant.
8. Choosing an end mill
- Flutes: one to three. At the same RPM, single-flute tools need half the feed of two-flute tools for the same chip, which suits machines with a low maximum feed. Onsrud's single-flute series lists heavier chips (0.007–0.009 in at 1/4").
- Geometry: aluminum-specific tools with a high helix and polished flutes are sold for chip evacuation (Amana's chart is for a 55° helix tool; RobbJack mentions 2–3 flute high-helix tools).
- Coating: uncoated polished, or an aluminum coating such as DLC (RobbJack). RobbJack pairs AlTiN coatings with steels, not aluminum.
- Length: use the shortest tool and stick-out that reach the depth. Deflection rises quickly with stick-out.
9. Slotting, adaptive clearing and depth
Full-width slots are the hardest cut for chip clearing. CNC Router Store suggests stepping over instead of full-width slotting at depth, and taking more, shallower passes. Amana's chart applies the same feed adjustment as its wood charts for deeper cuts:
- Depth of cut up to 1 × diameter: use the chart feed.
- 2 × diameter: reduce the feed by 25%.
- 3 × diameter: reduce the feed by 50%.
Adaptive clearing (constant engagement with a small stepover) keeps chips smaller and easier to clear. MillCaliber's chip-thinning compensation raises the feed at small stepovers so the chip stays at its target; see chip thinning.
10. Tools for aluminum
These links open Amazon search results for the tool types above. They are not specific products MillCaliber has tested. Compare the maker's data before you buy.
- 1/4" two-flute carbide end mills for aluminum (opens in a new tab)
- Single-flute carbide end mills for aluminum (opens in a new tab)
- DLC-coated end mills for aluminum (opens in a new tab)
- Mist and minimum-quantity lubrication systems (opens in a new tab)
As an Amazon Associate, MillCaliber earns from qualifying purchases. See the affiliate disclosure.
11. Sources
Accessed 18 October – 6 November 2026. These sources are cited for their published figures and guidance; they do not endorse MillCaliber.
- Amana Tool (via ToolsToday), 2 & 3 flute solid carbide aluminum cutting 55° helix end mills, speed chart (PDF): slot conditions, depth adjustments.
- CNC Router Store, Why is my aluminum welding to the router bit?: causes and fixes, RPM guidance, and the Onsrud 63-600 and 63-000 figures it lists.
- RobbJack, Speeds & feeds for 6061 aluminum: A1-201 2-flute values at 60,000 RPM.
- RobbJack, Chip welding & built-up edge: how to stop it.
- Helical Solutions, aluminum end mill speed & feed parameters (PDF): 720–1,080 SFM range and maximum-RPM note.
- Productivity Inc., RedLine 5-flute aluminum end mill speeds & feeds (PDF).
- University of Pennsylvania MEAM design lab, Feeds and speeds guide.