Aluminum Speeds and Feeds: 6061, 7075, and 7050 Milling Starting Points
By Yoda
Aluminum is forgiving enough that you can machine it badly and still get a part, which is exactly why so many shops leave real cycle time on the table. The three alloys we stock behave differently: 6061 is soft and gummy and wants speed, 7075 is harder and wants a bit less of it, and 7050 sits close to 7075 but shows up in thick sections where rigidity and heat become the actual constraint. Here are practical carbide starting points for all three, the two formulas that generate every number you need, and the failure modes specific to each alloy.
In Short
- →Two formulas do all the work: RPM = SFM x 3.82 / diameter, and feed IPM = RPM x flutes x chip load.
- →Carbide starting points: 6061-T651 at 800 to 1,000 SFM, 7075-T651 at 600 to 900, 7050-T7451 slightly lower still. The 7xxx alloys run 10 to 25% slower than 6061.
- →Chip load scales with tool diameter, roughly 0.002 to 0.004 in per tooth on a 1/4 inch tool and 0.003 to 0.006 on a 1/2 inch.
- →Use 2 or 3 flutes in aluminum. Chip evacuation, not tooth count, is the limiting factor, and a packed flute is how you break tools and weld chips to the cutter.
- →These are starting points, not gospel. Coating, rigidity, holder runout, DOC, and whether you are slotting or side milling all move the safe answer. Validate on your machine.
The Two Formulas
Every speeds-and-feeds number comes out of these two equations. Surface speed is a property of the material and the cutter, and RPM is what your machine actually needs, so you convert between them using the tool diameter. Then feed rate is just how fast you advance given how many teeth are cutting and how big a chip each one should take.
Spindle speed and feed rate
RPM = SFM x 3.82 / tool diameter (in) feed (IPM) = RPM x number of flutes x chip load (in per tooth)
= 1/2 in 3-flute in 6061 at 900 SFM: RPM = 900 x 3.82 / 0.5 = 6,875, feed = 6,875 x 3 x 0.006 = 124 IPM
- SFM
- Surface feet per minute. A material and tooling property, the number you look up.
- 3.82
- 12 / pi, the unit conversion from surface feet to revolutions
- chip load
- Inches of material each tooth removes per revolution, also called IPT or feed per tooth
- IPM
- Inches per minute, the feed rate you program
Surface Speed by Alloy
6061 is the softest and fastest of the three. The 7xxx alloys are substantially harder, roughly 73,000 psi tensile in 7075-T651 against 42,000 in 6061-T651, and that hardness translates directly into lower surface speed and more heat at the cutting edge. 7050-T7451 is marginally more conservative again, partly because it is overaged and partly because it is usually being cut in thick sections where you have more material and more heat to manage.
Carbide milling surface speed, conservative to aggressive (SFM)
| Alloy | Roughing SFM | Finishing SFM | Relative to 6061 | Main constraint |
|---|---|---|---|---|
| 6061-T651 | 800 to 1,000 | 1,000 to 1,500 | Baseline | Gummy chips, built-up edge |
| 7075-T651 | 600 to 900 | 900 to 1,200 | 10 to 20% lower | Hardness, heat at the edge |
| 7050-T7451 | 550 to 850 | 850 to 1,100 | 15 to 25% lower | Thick sections, heat, rigidity |
Chip Load by Tool Diameter
Chip load scales with tool diameter because a bigger tool has more core strength to resist deflection and breakage. Running a 1/4 inch cutter at the chip load appropriate for a 1/2 inch one is a reliable way to snap it. Conversely, running too light a chip load is not safe either: it rubs instead of cutting, which generates heat and work hardens the surface, and in aluminum it promotes built-up edge where material welds itself to the cutting edge.
| Tool diameter | Chip load, 6061 | Chip load, 7075 / 7050 | 3-flute feed at listed SFM |
|---|---|---|---|
| 1/4 in | 0.002 to 0.004 in | 0.002 to 0.003 in | 6061 ~165 IPM at 900 SFM |
| 3/8 in | 0.003 to 0.005 in | 0.002 to 0.004 in | 6061 ~138 IPM at 900 SFM |
| 1/2 in | 0.003 to 0.006 in | 0.003 to 0.005 in | 6061 ~124 IPM at 900 SFM |
| 3/4 in | 0.004 to 0.007 in | 0.003 to 0.006 in | 6061 ~96 IPM at 900 SFM |
Worked Starting Points
Here are the three alloys run through both formulas at typical roughing speeds, for the tool sizes most shops reach for. Round to something your machine likes and adjust from there based on spindle load, sound, and chip color.
| Alloy and SFM | Tool | RPM | Chip load | Feed (IPM) |
|---|---|---|---|---|
| 6061 at 900 SFM | 1/4 in, 3 fl | 13,750 | 0.004 in | 165 |
| 6061 at 900 SFM | 1/2 in, 3 fl | 6,875 | 0.006 in | 124 |
| 7075 at 750 SFM | 1/4 in, 3 fl | 11,460 | 0.004 in | 138 |
| 7075 at 750 SFM | 1/2 in, 3 fl | 5,730 | 0.006 in | 103 |
| 7050 at 700 SFM | 1/4 in, 3 fl | 10,695 | 0.004 in | 128 |
| 7050 at 700 SFM | 1/2 in, 3 fl | 5,350 | 0.006 in | 96 |
Flute Count and Chip Evacuation
Steel practice says more flutes means more feed. Aluminum inverts that logic. Aluminum produces high volumes of soft, sticky chips, and if those chips cannot get out of the flute they pack, weld to the cutter, and either ruin the finish or break the tool. So you use 2 or 3 flutes with large polished gullets, and you accept fewer teeth in exchange for space to clear chips. Three flutes is the usual best compromise for plate work: enough teeth for good feed, enough gullet for evacuation.
- 2 flutes: maximum chip clearance. Best for deep slots, pockets, and full-width cuts where evacuation is worst.
- 3 flutes: the default for aluminum plate. Good feed rate with adequate gullet space. Start here.
- 4+ flutes: finishing passes and light radial engagement only, where chip volume per tooth is small.
- Uncoated or ZrN and TiB2 coatings. Avoid TiAlN in aluminum, it has an affinity for aluminum and promotes built-up edge.
- Polished flutes matter more in aluminum than in almost any other material. A rough gullet is where chips start sticking.
- Air blast or flood coolant aimed at chip evacuation, not just cooling. Recutting chips is a leading cause of poor finish in 6061.
Alloy-Specific Failure Modes
Each of the three fails differently, and knowing which failure you are looking at tells you which parameter to change.
| Alloy | Characteristic problem | What you see | Fix |
|---|---|---|---|
| 6061-T651 | Built-up edge and chip welding | Gummy finish, chips sticking to cutter | More speed, more chip load, better evacuation |
| 6061-T651 | Chip recutting | Scratched or torn surface finish | Air blast or coolant aimed at the flutes |
| 7075-T651 | Heat at the cutting edge | Discolored chips, rapid edge wear | Reduce SFM 10 to 20%, increase coolant |
| 7075-T651 | Edge chipping on entry | Chipped corners on the part edge | Ramp or arc in, avoid straight plunge entry |
| 7050-T7451 | Deflection in thick sections | Taper on wall, chatter | Shorter tool, reduce radial engagement |
| 7050-T7451 | Residual stress movement | Part moves after material removal | Rough, then let it rest, then finish |
Why Temper Matters as Much as Alloy
A drawing that says 6061 without a temper has not told you what you are cutting. T651 plate has been stress-relief stretched after solution heat treatment, which is what lets you take material off one face without the part bowing. T6 has not. Same alloy, same nominal hardness, very different machining behavior on anything long or thin. The same logic applies in the 7xxx alloys, where T7351 and T7451 are overaged and cut slightly differently than peak-aged T651.
- 6061-T651: stress relieved plate, the correct choice for machined parts. Stable during material removal.
- 6061-T6: sheet temper under 0.250 in, not stress relieved. Expect movement on long parts.
- 7075-T651: peak aged, hardest and strongest, most prone to heat and edge chipping.
- 7075-T7351: overaged for stress corrosion resistance, roughly 10 to 15% lower strength, slightly more forgiving to cut.
- 7050-T7451: overaged and quench insensitive, the thick-section choice. Cut it like 7075-T7351 but expect more heat because there is more material.
How to Dial It In on the Floor
Published numbers get you to a safe starting point. The last 30% comes from paying attention for ten minutes.
- Start at the conservative end of the SFM range with a mid-range chip load, then raise speed first, not feed.
- Watch chip color. Silver and curled is right. Blue, brown, or straw means too much heat, so reduce SFM before anything else.
- Listen for chatter, then shorten the tool or reduce radial engagement rather than slowing the feed. Chatter is usually rigidity, not speed.
- Check the cutting edge under magnification after a few parts. Material welded to the edge means increase speed and chip load, wear means reduce speed.
- Measure the chip. If it is dust rather than a recognizable curl, your chip load is too light and you are rubbing.
- Log what worked per alloy and per tool. This industry runs on the numbers in someone's notebook, and the notebook is usually more accurate than the catalog.
Two formulas and three surface speed ranges cover most aluminum plate work: RPM = SFM x 3.82 / diameter, feed = RPM x flutes x chip load, with 6061 at 800 to 1,000 SFM, 7075 at 600 to 900, and 7050 slightly below that. Use 2 or 3 flutes so chips can actually leave, keep chip load in range for the tool diameter rather than the machine's comfort, and read the chips instead of trusting the chart. And remember that temper is half the story: T651 and T6 are the same alloy and very different parts once you start removing material.
Frequently Asked Questions
What speeds and feeds should I use for 6061 aluminum?
For carbide in 6061-T651, start at 800 to 1,000 SFM for roughing and up to 1,500 for finishing. Convert to RPM with RPM = SFM x 3.82 / tool diameter, then set feed with IPM = RPM x flutes x chip load. A 1/2 inch 3-flute at 900 SFM works out to about 6,875 RPM and, at a 0.006 inch chip load, roughly 124 IPM. Use 2 or 3 flutes so chips can evacuate.
Do 7075 and 7050 need slower speeds than 6061?
Yes. 7075-T651 is roughly 73,000 psi tensile against 42,000 for 6061-T651, and that hardness means more heat at the cutting edge. Run 7075 about 10 to 20% slower than 6061, so 600 to 900 SFM for roughing. 7050-T7451 is slightly more conservative again, 550 to 850 SFM, partly because it is usually being cut in thick sections where heat and rigidity are the real constraints.
How many flutes should I use for aluminum?
Two or three. Aluminum makes large volumes of soft, sticky chips, and the limiting factor is getting them out of the flute rather than how many teeth are cutting. Three flutes is the default for plate work, giving decent feed rates with enough gullet space. Drop to two for deep slots and pockets where evacuation is worst. Save four or more flutes for light finishing passes.
What is the formula for RPM from SFM?
RPM = SFM x 3.82 / tool diameter in inches. The 3.82 is 12 divided by pi, which converts surface feet into revolutions. So a 1/2 inch tool at 900 SFM needs 900 x 3.82 / 0.5 = 6,875 RPM. Feed rate then follows from IPM = RPM x number of flutes x chip load per tooth.
Why are my aluminum chips sticking to the cutter?
That is built-up edge, and it is the classic 6061 problem. It usually means you are running too slow, taking too light a chip load, or not evacuating chips. Counterintuitively the fix is generally more speed and more feed, not less. Also check your coating: TiAlN has an affinity for aluminum and promotes the problem. Uncoated, ZrN, or TiB2 are better choices, and polished flutes help significantly.
Why does my part move after machining even though the plate was stress relieved?
Stress relief reduces residual stress, it does not eliminate the physics. When you remove a lot of material from one side of a plate, whatever stress remains is no longer balanced, so the part relaxes into a new shape. This is most pronounced in thick 7050 and 7075. The practical fix is to rough the part, let it sit, then take a finishing pass, so the movement happens before you cut your final dimensions rather than after.
Run the Numbers
Skip the arithmetic.
Our speeds and feeds calculator runs both formulas for your alloy, tool, and flute count. And when you need the plate itself, quote 6061, 7075, or 7050 in under 60 seconds with certs included.