Applications · Aluminum and Non-Ferrous Alloys
Aluminum Machining: Choosing the Cutter and the Cutting Data for Wrought and Cast Alloys
Aluminum is the material that makes a machine look quick and a finish look bad. It cuts at surface speeds several times those of steel, it removes metal faster than any other common material, and it fails on the two things a steel-minded tool choice does not expect: the metal welds itself to the cutting edge, and the part moves as it warms up. Silicon content decides which of the two dominates. Below roughly 12% silicon a wrought or low-silicon alloy is soft and gummy, and the edge has to stay sharp and polished to stop the chip welding to it. Above that figure the alloy carries hard silicon particles that grind the edge away, and the cutting material has to be hard enough to survive being abraded. What changes between the two is set out below, with the cutting speeds published for aluminum turning, milling and drilling and where those figures stop being reliable.
Failure Modes
Three failure modes that decide how you cut aluminum
Aluminum problems rarely arrive as a worn edge. They arrive as a finish that looks smeared, a cutter that loads up in a deep pocket, a tool that dulls slowly with no warning, or a dimension that was right on the machine and wrong an hour later. Reading which of the three below applies settles the geometry, the cutting material and the order of operations before anything is bought.
Failure mode 01
Built-up edge and welded chips on wrought alloys
What actually fails
Below roughly 12% silicon, aluminum is soft and gummy rather than brittle. Under pressure the chip welds to the cutting edge and to the flutes behind it, and the built-up edge that forms is not cutting the metal so much as smearing it. The edge then breaks away and takes tool material with it. In a pocket the same welding packs chips against the wall, so the cutter recuts them instead of throwing them clear, and the load climbs until the cutter or the part gives way.
What to look for in the tool
Look for the sharpest edge available and a polished flute rather than a coating that adds friction: on aluminum, edge sharpness and rake angle do the work that a hard coating does on steel. Flute space and a helix steep enough to lift the chip out of the cut matter as much as the grade once the pocket gets deep, and a higher surface speed keeps the cut ahead of the weld, which is why the aluminum rows in the table below run at several times the steel figures.
Failure mode 02
Abrasive wear from silicon in cast alloys
What actually fails
Cast aluminum carries silicon as hard particles rather than as a dissolved element. Above roughly 12% silicon those particles are hard enough to grind the edge instead of deforming against it, and the failure is progressive edge rounding with a finish that goes dull by degrees. There is no chipping to warn the operator, and an ordinary coated carbide insert run at high speed behaves like a tool cutting an abrasive rather than a metal.
What to look for in the tool
Look at cutting material rather than at coating. The harder the cutting material, the longer the edge holds on a high-silicon alloy, and polycrystalline diamond exists for exactly this case. Because the wear is abrasive and steady rather than sudden, a high-silicon job usually rewards a planned tool change at a fixed number of parts over an attempt to reach the tool life a wrought alloy would give.
Failure mode 03
Thermal expansion and a dimension that will not sit still
What actually fails
Aluminum expands roughly twice as much as steel for the same temperature rise and carries heat away from the cut faster, so a part that feels warm to the hand has already grown. A bore measured while it is hot is not the bore that comes off the machine an hour later. A thin wall pockets heat, bows under the cut and then moves again when the fixture is released, and removing the material around a pocket lets internal stress go in a way that is invisible until the finished part is measured.
What to look for in the tool
Look at the order of operations and the coolant before the insert grade. Rough and finish in separate passes with a settling period between them, keep coolant on the cut rather than over the whole part, and measure at the temperature the drawing assumes. A free-cutting geometry that generates less heat in the first place is the cheapest way to stop the part from moving.
One boundary is worth stating plainly. Aluminum and magnesium alloys in the ISO N group are what the figures below cover; the harder non-ferrous materials sometimes grouped with them are not. There is no separate row for thread cutting: tapping and thread milling in aluminum are carried out far below the speeds in the table and the governing figure is the one published with the specific tap or thread mill.
Magnesium needs its own warning rather than a row in a table: fine magnesium chips ignite, and the coolant and housekeeping rules for magnesium are a safety matter before they are a cutting matter. Tell us if the part is magnesium and we will answer it as a separate question rather than as another aluminum job.
Tool Matrix
Which tool family for which aluminum operation
Milling is where most aluminum is cut, so it leads the matrix here, followed by turning and then the hole and the thread. Every card stops at the level of tool family, geometry and cutting material, because the specific cutter is decided against the machine, the fixture and the finish the drawing asks for.
Two facts run through all three blocks. The first is that aluminum rewards sharpness over hardness until silicon is present, and rewards hardness over sharpness once it is. The second is that the chip has to leave the cut immediately: an aluminum chip that stays under the cutter is recut, and a recut chip welds.
Milling
Milling aluminum is a chip evacuation problem wearing a metal removal problem as a disguise. The geometry that suits it is chosen as much for the space behind the cutting edge as for the edge itself.
Milling inserts for aluminum
Polished, high-rake coated carbide inserts for face and shoulder milling of wrought and low-silicon cast alloys, where the cutting edge needs to be sharp and the surface in front of the chip needs to be slippery rather than hard.
Solid carbide end mills for aluminum
Two and three flute geometry with wide flute space and a polished finish, so the soft chip clears instead of packing. High-helix and variable-pitch options where a deep pocket or a thin wall would otherwise chatter.
Cutting material for high-silicon aluminum
Polycrystalline diamond is the answer to abrasive silicon: the hardest edge available, chosen for face milling and boring of high-silicon cast alloys where coated carbide rounds off far too quickly to be economic.
Turning
Turning aluminum is fast, and it is the operation where the difference between a wrought alloy and a cast one shows up in the tool life most sharply.
Turning inserts for aluminum
Sharp positive-rake inserts with polished faces for roughing and finishing wrought and low-silicon alloys. The cutting edge is deliberately keen rather than strong, because on aluminum a keen edge is what keeps the chip from welding to it.
PCD inserts for high-silicon and finishing work
Diamond-tipped inserts for cast alloys above roughly 12% silicon and for finishing passes on soft alloys where a mirror finish and a long, predictable tool life both matter.
All turning shapes and cutting materials
The ISO turning shapes available in aluminum grades and in diamond, with the note that belongs to each, so a shape can be settled before the cutting material is chosen.
Drilling, threading and workholding
The hole is where a soft, gummy chip does the most damage, because it has nowhere to go. Workholding comes last for the same reason it does on steel: the holder decides whether the cutter runs at the speed it was bought for.
Drill bits for aluminum
HSS, HSS-Co and HSS-E-PM drills with polished flutes for general work, and solid carbide drills with internal coolant for deep holes and for the high-silicon cast alloys that wear a drill out quickly.
Threading tools for aluminum
Thread mills and taps for aluminum, including forming taps for chipless threads in the softer wrought alloys, where displacing the material avoids producing a chip that will weld inside the hole.
Tool holders for high-speed aluminum cutting
Holders that hold concentricity at the spindle speeds aluminum is cut at, where a collet pushed to its limit is often the reason a finish stops repeating.
Cutting Data
Published cutting speeds for turning, milling and drilling aluminum
The table gives the surface speed published for aluminum in each operation, drawn from the same source data as the cutting speed reference so the two cannot disagree. The spread between the rows is the point: a wrought alloy and a high-silicon casting are not the same machining problem, and the published windows are far apart because of it.
Milling spans the widest range of any operation here, from a cautious figure for a high-silicon casting to a window for a soft wrought alloy that most machine tools cannot reach at the cutter diameter they are using. That is not an error in the data: it is the reason spindle speed, holder balance and coolant delivery decide the result on aluminum as much as the insert does.
| Aluminum condition | Operation | Tool family | Cutting speed (m/min) | Cutting speed (SFM) | Basis of the range | Source (as recorded) |
|---|---|---|---|---|---|---|
| Wrought aluminum | Turning | coated indexable carbide | 490-490 | 1605-1605 | published as a single starting figure | single starting value |
| Low-silicon aluminum and magnesium alloys (Si under 12.2%) | Turning | coated indexable carbide | 60-440 | 200-1450 | published as one window for the group | N2 row |
| High-silicon aluminum and magnesium alloys (Si over 12.2%) | Turning | coated indexable carbide | 30-290 | 100-950 | published as one window for the group | N3 row |
| Wrought aluminum alloys, non-hardened, 60 HB | Milling | solid carbide, aluminum geometry | 375-430 | 1230-1411 | the two figures are the published slotting and roughing values | p.42 cutting data, slotting 375 / roughing 430; SFM converted |
| Aluminum, general | Milling | coated indexable carbide | 500-1500 | 1640-4921 | published as a wet window and a dry window; the range spans both | p.11 (dry 800-1500 / wet 500-800); SFM converted |
| Cast aluminum alloys up to 12% Si | Milling | solid carbide, aluminum geometry | 200-230 | 656-755 | published as one value for the cast alloy group | p.42; SFM converted |
| Cast aluminum alloys over 12% Si, 130 HB | Milling | solid carbide, aluminum geometry | 160-160 | 525-525 | published as a single figure for the high-silicon group | p.42; SFM converted |
| Aluminum under 12% Si | Drilling | HSS and HSS-Co drills | 45-75 | 148-246 | two published grades; the range spans both | 811505 · 820902 |
| Aluminum under 12% Si | Drilling | HSS-E-PM drills | 70-90 | 230-295 | published as a window for the grade | 810434 |
| Aluminum over 12% Si | Drilling | HSS-E-PM drills | 30-35 | 98-115 | published as a window for the grade | 810434 |
Sources: recommended cutting speeds are taken from the published application data of tool makers — Ingersoll IMC Cutting Data and Parameters handbook, Kennametal TopSwiss MBS and inserts application data, Guhring RF 100 AL and RF 100 series, OSG VGM7 / VG446 / HSS-Co datasheets, Uddeholm Unimax cutting data, SSAB Hardox machining recommendations and Dormer Pramet workpiece material groups. The reference recorded for every row — as it is logged in our data, which is a document page, a column, a document number, or the grade breakdown the document itself prints — is carried in the last column of the table, so each figure can be taken back to what it came from without asking us for it. Values published only as surface feet per minute were converted at 1 m/min = 3.28084 SFM and are marked as converted. The rows in the table are the extremes of the published range for each aluminum condition and operation, with no interpolation between them. ISO P / M / K / N / S / H group letters follow ISO 513:2012.
Read the row that matches your alloy and operation, take a figure from the lower half of the window for an unfamiliar setup, then move up while the chip leaves clear and the finish stays uniform. On aluminum the ceiling is usually the machine rather than the tool: check the spindle speed the window implies for your cutter diameter before planning around it.
The table gives surface speed only. Feed per tooth and depth of cut are properties of the cutter geometry and the machine, not of the alloy, and a number printed here would be wrong for most readers. Thread cutting follows the same rule: tapping and thread milling in aluminum run far below the speeds above, and the figure that governs is the one published with the specific tap or thread mill for the thread form and depth you are cutting. Send us the thread callout and the alloy and we come back with that figure rather than a general one.
From surface speed to spindle speed
- Spindle speed in metric: n = (vc x 1000) / (pi x D), with vc in m/min and D the diameter in millimetres.
- Spindle speed in imperial: n = (SFM x 3.82) / D, with D the diameter in inches.
Worked from the table above
- Milling with a 16 mm cutter: at 1,200 m/min, n = (1200 x 1000) / (3.14159 x 16) = 23,873 rpm — a spindle speed few machines reach, which is why the upper end of the milling window is a target rather than a setting.
- The same window on a 50 mm face mill: at 1,200 m/min, n = (1200 x 1000) / (3.14159 x 50) = 7,639 rpm, which is inside the reach of a modern machining centre.
- Turning a 60 mm aluminum bar: at 400 m/min, n = (400 x 1000) / (3.14159 x 60) = 2,122 rpm.
- A 3 inch face mill: at 2,500 SFM, n = (2500 x 3.82) / 3 = 3,183 rpm.
Put it on the machine
The same arithmetic is on the cutting speed reference, with drill and tap diameters from every series rather than the aluminum rows above, so a figure read here can be turned into a spindle setting for any tool in the job without leaving the site.
Where the table gives a window rather than a figure, start at the bottom of it on an unfamiliar setup and move up while the chip breaks cleanly and the finish holds. The machine, the holder and the part decide how far up the window you can go; the table only says where the window is.
Data and Service
Where the figures come from
Every figure here carries its origin, and the three kinds of source are kept apart: published standards named by number and year, industry figures named by the document they were read from, and customer feedback written up as what it is.
Published standards
The ISO P / M / K / N / S / H application groups used to describe the tooling come from ISO 513:2012, which fixes what each letter covers. Where a figure comes from a standard, it is named with the standard and the year it was issued, per row.
Tool makers and industry data
The cutting-speed ranges in the table above are the values printed by the tool makers our data is taken from. They are used as published, at the extremes of the published window, and every row carries its document and page or column reference in our source file so any figure can be checked before it is used on a job.
Trial feedback
Where a customer tells us what a grade actually did on their machine, it is recorded as an attributed note rather than reworked into an illustrative story. We do not publish references we cannot point to.
What comes with a quotation
Two things we do go beyond the table. Both are actions rather than figures, and both are visible in a quotation before anything is ordered.
A starting cutting speed with the quotation
Send the aluminum alloy or its hardness, the operation, and the machine it runs on. The quotation comes back with a starting surface speed and a feed range for the insert family we propose. Treat it as the first setting rather than a guarantee of the result: the figure is decided by your setup, the holder and the part, and it is meant to be adjusted from the chip and the finish.
Trial quantities to prove it on the machine
The honest answer to "will this grade run on my aluminum" is a trial order, not a data sheet. Small quantities and mixed orders are welcome, and charges and freight are confirmed against the actual enquiry rather than published as a fixed number.
How we handle a tooling enquiry from first question to delivery
Questions Buyers Ask
Aluminum machining questions we are asked before quoting
The published windows in the table above run from 160 m/min for a high-silicon cast alloy to 1,500 m/min for aluminum cut dry, and the spread is mostly about silicon content and about how the chip clears. Take the lower half of the window for a deep pocket or an unfamiliar setup, and check the spindle speed the window implies at your cutter diameter: on small cutters the machine, not the tool, is usually the limit.
Because it is soft and gummy below roughly 12% silicon, and under cutting pressure the chip welds to the edge rather than flowing away from it. The welded material then smears the surface instead of cutting it. A sharper edge, a polished flute, more rake, a higher surface speed and enough flute space to throw the chip clear all push the problem back; a hard coating added for wear resistance does not help and can make the friction worse.
Below roughly 12% silicon, the alloy is soft and the dominant failure is a built-up edge and a smeared finish. Above it, hard silicon particles grind the cutting edge, so the dominant failure becomes wear and the answer becomes the hardest cutting material available rather than the sharpest one. The same cutter geometry does not serve both well, and the published cutting speeds differ by several times.
Sharpness and surface finish on the tool matter more than coating hardness, and that is the opposite of the rule for steel. Coatings chosen to add friction, such as the hard wear coatings used on steel, tend to encourage the chip to weld. What helps is a polished cutting face, a polished flute, high positive rake and a substrate fine enough to take a keen edge and hold it at high surface speed.
Two or three flutes with wide flute space for roughing, so the soft chip has somewhere to go, and a polished face and flute so it does not stick on the way out. High-helix and variable-pitch geometry comes into it when a deep pocket or a thin wall starts to chatter, because the fix for chatter on aluminum is usually the geometry rather than a slower cut. Tell us the pocket depth and the machine and we will say which of the two we would quote.
Aluminum expands roughly twice as much as steel over the same temperature rise, so a part that is warm from cutting is genuinely larger than the same part cold. Measuring hot and adjusting the offset will leave you undersize when the part cools. Let the part come back to room temperature before the finishing cut and before the measurement, keep the coolant on the cut rather than flooding the whole part, and expect thin walls to keep moving after the fixture is released.
Often, yes, and the published source data carries separate wet and dry windows for aluminum milling for that reason. Dry cutting relies on the chip carrying the heat away, so it needs enough air or chip clearance to do that, and it is a poor choice in a deep pocket where the chip has nowhere to go. What matters more than wet or dry is consistency: on aluminum, a coolant flow that reaches the edge intermittently causes more trouble than either extreme.
Yes. Send the alloy designation or its temper and hardness, the operation and the machine, and we come back with the cutter family, the cutting material and a starting surface speed for it. Where the alloy is one we have not quoted before, we confirm which side of the silicon line it falls on before naming a cutter, because that single question decides whether the answer is a sharp edge or the hardest one available.
Send the alloy and the operation — get the cutter and a starting speed
Tell us the alloy designation or hardness, what the part is and which machine it runs on. You get the cutter family and geometry we would quote, the holder for that spindle speed, and a starting surface speed for the combination, rather than a catalogue to search through.