CNC Milling Aluminum: 7 Tips That Hold Tolerance
Aluminum cuts fast, which is exactly why it goes wrong so quickly. This guide is for engineers and buyers who need parts that measure right the first time. Read it and you can judge whether a shop is running aluminum properly, or just running it fast.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
- 8
Key takeaways
Start with the alloy and the tool, not the spindle
Aluminum is not one material. 6061-T6 machines cleanly, welds well and holds ±0.005 mm on most features. 7075 is stronger and gummier; it cuts well but punishes poor chip evacuation. 2024 tends to move after machining when you remove a lot of stock from one side. 5052 and 5083 are softer and prone to built-up edge. Choosing the wrong grade is the most common reason a first article fails, and no speed or feed change fixes it.
Tool geometry matters more here than in steel. Use 2-flute or 3-flute carbide end mills with polished flutes and a 10–15° helix for roughing. The wide gullet carries the large chip volume aluminum produces. A 4-flute tool that works fine in 4140 will plug in 6061 at the same chip load. For finishing, a 3-flute tool with a higher helix and a small corner radius leaves a better floor finish and reduces chatter on thin features.
Coatings are a secondary choice. Uncoated polished carbide is often the best aluminum cutter because it has the sharpest edge. ZrN and DLC coatings reduce built-up edge on 5052 and 5083. Avoid thick AlTiN coatings; they round the cutting edge, and a rounded edge rubs instead of shearing. If your shop only stocks one aluminum tool, it should be an uncoated 3-flute with a 45° helix for finishing.
- 16061-T6General purpose. Good finish, predictable dimensions.
- 27075-T6High strength. Needs rigid setup and strong chip clearance.
- 32024-T4Aerospace use. Expect stress relief issues on heavy stock removal.
- 45052 / 5083Soft and gummy. Polished flutes and ZrN help.
Speeds, feeds and heat in CNC milling aluminum
Aluminum conducts heat away from the cut faster than steel, so you can run high surface speeds. A 10 mm carbide end mill in 6061 typically runs at 300–500 m/min surface speed, which on a 10,000 rpm spindle is the top of the range. The limit is usually spindle speed, not the material. Set the surface speed at the top of what your machine allows, then set the feed from the chip load.
Feed per tooth is where most programmers get it wrong. For a 10 mm 3-flute cutter in 6061, a chip load of 0.05–0.10 mm per tooth is normal for roughing. Too low and the edge rubs, work-hardens the surface and dulls the tool. Too high and you overload the flute on a light-duty machine. Watch the chip: a proper aluminum chip looks like a small comma, not dust. Dust means you are rubbing.
Heat is not the main failure mode in aluminum, but it still matters on deep pockets and long finishing passes. If the part gets warm to the touch, dimensions drift as it cools. Rough with air blast, then let the part stabilize before finishing. On thin floors, a warm part can warp 0.05 mm or more between roughing and finishing. Measure at a stable temperature, not straight off the machine.
Chip evacuation and workholding decide the finish
Deep pockets are where aluminum milling fails. The tool re-cuts a chip, the chip welds to the edge, and the next tooth hits a lump of built-up material. Use a high-pressure air blast or through-tool air if you have it. Flood coolant can work, but in a blind pocket it can pool chips at the bottom. If you use coolant, use a high-flow, low-pressure setup and direct it to sweep the pocket floor.
Workholding has to be rigid without crushing the part. Aluminum is soft; a vise with sharp jaws can mark a finished face. Use soft jaws machined to the part profile, or a vacuum plate for thin plates. For a part with a 2 mm wall, the fixture often needs more design time than the tool path. That is normal, and it is the difference between a part that measures right and one that springs after unclamping.
Vibration shows up as chatter marks and as a dimensional error. If you hear a ringing sound, reduce radial engagement before you reduce speed. Increasing spindle speed slightly can also move you out of a resonant frequency. On long, thin end mills, reduce the axial depth and use a shorter tool. A stub-length tool with 3× diameter reach is far stiffer than a 6× diameter tool.
- 1Recut chipsCause built-up edge, poor finish and tool breakage.
- 2ChatterFix radial engagement and tool stick-out before changing speed.
- 3Thin wallsSupport the wall, then take light finishing passes.
Finishing, deburring and inspection before the part ships
A sharp cutter leaves a better finish than a slow one. For a Ra 0.8–1.6 μm finish on 6061, use a 3-flute tool with a 0.4–0.8 mm corner radius, a 0.1–0.2 mm finish allowance, and a feed per tooth around 0.03–0.05 mm. Too light a finishing pass rubs the surface and produces a smeared look that anodizing will show. If the drawing calls for Ra 0.2–0.8 μm, plan a separate finishing step rather than trying to get there in one pass.
Deburring is not cosmetic. A 0.1 mm burr on a mating face changes the assembly stack. Break edges with a chamfer tool or a hand tool, and check holes for burrs at both ends. For anodized parts, note that hardcoat adds 0.05 mm or so per surface and changes hole size. Specify the finish before machining, not after.
Inspection should match the drawing. Check critical dimensions on a CMM or a height gauge, and record the tool, program revision and offset. If a feature is out, correct it with a small step-over pass rather than re-cutting the full depth. Reports are available on request, and every part is inspected before shipment.
How to tell whether a shop can mill aluminum well
Ask about tooling, not just machine count. A shop that runs aluminum daily will have polished 2 and 3-flute carbide in stock and will talk about chip load before spindle speed. If the answer to a deep-pocket question is only about coolant pressure, the shop probably cuts aluminum occasionally rather than as a core process.
Ask how thin-wall parts are held. The right answer mentions soft jaws, vacuum fixtures, or added support ribs. The wrong answer is slower feed rates. Rigidity comes from the setup, and a flexible setup will chatter no matter how slow the pass is.
Ask how the finish is specified. If the drawing says Ra 0.8 μm and the shop quotes one finishing pass, expect a smeared surface after anodizing. If the shop separates roughing and finishing and discusses the anodize build-up on holes, that is a shop that reads the drawing.
GreatLight runs 127 high-precision CNC machines, including 16 simultaneous 5-axis machining centers and 27 three-axis machines, across three wholly-owned plants with 7,600 m² of floor space. Aluminum work covers 6061, 7075, 2024, 5052, 5083, 6082 and ADC12. Quotation and DFM feedback come back within 12 hours, and production can start within 24 hours. There is no minimum order quantity, from one prototype to 10,000+ part runs.
Step by step: setting up a stable aluminum cut
- 11. Confirm the alloy and temperCheck the cert against the drawing before you touch the machine. 6061-T6 and 6061-T4 cut differently. If the cert is missing, hold the job.
- 22. Pick a 2 or 3-flute cutter for roughingMatch the diameter to the smallest internal radius. Never leave more than 5% of the cutter diameter as corner stock if you want a clean finish pass.
- 33. Set surface speed and chip loadTarget 300–500 m/min for 6061, 200–350 m/min for 7075. Feed per tooth 0.05–0.10 mm for a 10 mm cutter. Recalculate for smaller tools.
- 44. Use trochoidal or high-efficiency paths for pocketsKeep radial engagement at 8–15% of the cutter diameter and axial depth up to 1× diameter. This keeps the chip thin and the load even.
- 55. Clear chips with air blastAim the nozzle at the cut, not the part. Recut chips are the number one cause of poor finish and sudden tool breakage in deep pockets.
- 66. Support thin walls before the finishing passAdd a sacrificial rib, use a vacuum fixture, or leave a joining web. Removing support first and finishing later is how walls bow.
- 77. Measure at a stable temperatureLet the part cool, then check critical dimensions. Re-cut with a 0.05 mm finish allowance if needed, not with a full-depth pass.
When to use which aluminum milling approach
All values are typical ranges for 6061-T6 on a rigid 3-axis or 5-axis machine.
| Feature | Roughing | Finishing | When it fails |
|---|---|---|---|
| Flutes | 2–3 | 3 | 4-flute packs chips in deep pockets |
| Surface speed | 300–500 m/min | 300–450 m/min | Too slow rubs and work-hardens |
| Chip load | 0.05–0.10 mm/tooth | 0.03–0.05 mm/tooth | Dust chips mean rubbing, not cutting |
| Radial engagement | 8–15% of Ø | 5–8% of Ø | Full-width cuts chatter on thin walls |
| Cooling | Air blast | Air or light flood | Flood pools chips in blind pockets |
| Finish target | Ra 1.6–3.2 μm | Ra 0.8–1.6 μm | One pass cannot do both jobs |
| Inspection | In-process | Final CMM | Measuring a hot part hides drift |
The short version
Aluminum rewards a sharp tool, a stable setup and a clear chip. Get the alloy right, keep the flutes open, and support thin walls before you touch the speed override.
CNC milling aluminum: common questions
Should I use coolant or air blast when milling aluminum?
Air blast is usually better for roughing and for deep pockets because it clears chips and keeps the cut visible. Use high-flow flood coolant for heavy finishing cuts where heat builds up, or when the machine has no air supply.
Do not use a light mist in a deep pocket. It wets the chips without moving them, which makes recutting worse.
How many flutes should an end mill have for aluminum?
Two or three flutes cover most work. Two flutes give the largest gullet for roughing; three flutes give a better balance of finish and chip clearance. Four flutes can work for finishing at shallow radial engagement, but they plug easily in pockets.
On a 10 mm cutter in 6061, a 3-flute tool at 0.05–0.10 mm per tooth is a safe starting point.
Why does my aluminum part warp after machining?
Warping usually comes from residual stress in the stock, not from the cutter. Removing a lot of material from one side releases stress and the part bends. 2024 and 7075 are more prone to this than 6061.
Rough both sides evenly, leave 0.3–0.5 mm for finishing, and let the part rest before the final pass. Stress-relieved stock helps on tight parts.
What tolerance can you hold on aluminum parts?
GreatLight holds ±0.005 mm on critical features in aluminum, with 100% inspection before shipment. Achieving that depends on the feature, the wall thickness and the setup.
Very thin walls and long unsupported features need a tolerance review before quoting. Send the drawing and we will flag what is practical.
Does anodizing change the dimensions of a milled aluminum part?
Yes. Anodizing builds oxide on the surface, and hardcoat builds more than a standard clear coat. A hole that measures 5.00 mm before coating will measure smaller after it.
Tell the machine shop which finish you plan. Holes and threads can be cut with an allowance so the coated part fits. Laser marking needs a minimum character height of 1.5 mm.
Can you mill aluminum prototypes without a minimum order quantity?
Yes. There is no minimum order quantity, from a single prototype to 10,000+ part runs. Uploads are secure and confidential, and an NDA is available on request.
Quotation and free DFM analysis return within 12 hours. Production can start within 24 hours after approval, and parts typically ship in 3–5 days.
Send the drawing, get a milling plan
Upload your aluminum part and we will return a quote with DFM notes, tooling comments and a realistic tolerance call.
12-hour quoteNo minimum order quantity100% inspectionNDA on request
More machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
