Which Cutting Tools Should Be Used for 13 Metal Materials

• 1
  Tool and Cutting Data by Material Group
• 2
  Tool substrate and coating first, geometry second
• 3
  Aluminum, copper, brass, and magnesium
• 4
  Carbon steel, alloy steel, and tool steel
• 5
  Stainless 303, 304, 316, and 17-4PH
• 6
  Inconel, Monel, and other nickel alloys
• 7
  Coolant, rigidity, and when tool choice is not the problem

When engineers ask which cutting tools should be used for a new part, the answer starts with the workpiece, not the catalog. Aluminum cuts clean with a sharp uncoated carbide edge and lots of clearance. Steel needs a tougher substrate that survives interrupted cuts and heat. Stainless work-hardens the moment a dull edge rubs instead of shears. Titanium and nickel alloys run hot and pull heat into the tool, so coating choice and coolant pressure matter more than spindle speed.

A good rule: match the coating to the temperature at the edge. Uncoated carbide works below roughly 400 °C. TiAlN and AlTiN coatings hold up from 700 °C to 900 °C, which is where alloy steel, stainless, and titanium sit during a real cut. For aluminum and copper, coating is usually a liability because it rounds the sharp edge and traps chips.

Geometry follows the material. Aluminum likes 2 or 3 flutes with a 45° helix and polished flutes for chip evacuation. Steel and stainless run better with 4 or 5 flutes so the feed rate stays high without chatter. Titanium needs a sharper rake and a stronger core, which is why a dedicated Ti-6Al-4V end mill outperforms a general-purpose one on the same part.

If you are unsure, start with a tough PVD-coated carbide in a 4-flute geometry. It will cut most steel and stainless acceptably, and it will show you where the material fights back before you commit to a specialty tool.

• 1
  Uncoated for non-ferrousAluminum, brass, copper, and magnesium cut best with a polished uncoated edge.
• 2
  PVD TiAlN for steel and stainlessHandles the 700-900 °C range where these materials sit.
• 3
  AlTiN for titanium and InconelBetter hot hardness when the tool tip glows under load.

Aluminum is the easy material until it is not. 6061 and 7075 cut at 300-600 m/min with uncoated carbide and a 2 or 3 flute cutter. The failure mode is chip welding, not tool wear. If the flutes load up, increase feed per tooth and add air blast or a mist. Do not slow the spindle down; that makes it worse. A polished flute and a high helix help chips leave the cut.

Copper and brass behave similarly but brass is abrasive. C36000 free-machining brass cuts fast, though the zinc content wears the edge over long runs. Beryllium copper is a different animal: it is abrasive and the dust is a health hazard, so it needs containment, not just a coating change. Use uncoated carbide with a high rake angle and expect shorter tool life.

Magnesium AZ31B and AZ91D cut at 400-800 m/min and leave a fine finish with a sharp uncoated tool. The hard rule is coolant. Never run water-based coolant on magnesium because chips can ignite. Use mineral oil or a dry cut with air and keep the chip load heavy enough to avoid fine dust.

Common mistake: choosing a coated tool for aluminum because it looks more durable. The coating dulls the rake face and the aluminum starts to smear. If your surface finish drops on 6061, check the coating before you change the speed.

• 1
  Watch chip weldingIncrease feed per tooth and use air blast on aluminum.
• 2
  No water on magnesiumUse mineral oil or dry cutting with air only.

Low-carbon steel like 1018 is forgiving. A PVD TiAlN carbide in 4 flutes at 120-180 m/min handles most jobs. The risk is built-up edge on gummy low-carbon stock, so keep the feed per tooth above 0.05 mm and avoid dwelling in the cut. If the finish looks torn, the tool is rubbing, not cutting.

Alloy steel 4130, 4140, and 4340 give a cleaner chip and a better finish, but they are harder on the edge. Drop to 80-140 m/min and use a tough substrate with TiAlN or AlTiN. Pre-hardened 4140 at 30 HRC is a common turning and milling material, and it rewards a negative rake insert in turning with a strong edge. For milling, a variable helix end mill reduces chatter on deep pockets.

Tool steel D2 and H13 are usually machined in the annealed state at 50-90 m/min. The carbide needs a negative rake and an AlTiN coating to survive the abrasion from carbides in the steel. If the part is already hardened above 45 HRC, carbide struggles and you should consider whether the feature can be ground or EDM instead. Choosing the wrong process here costs more than choosing the wrong tool.

One practical note: 4340 at high hardness cuts more like stainless than like 1045. If your speeds and feeds work on 1045, back off 30 to 40 percent before touching 4340.

• 1
  1018, 1045: general purpose4-flute TiAlN carbide handles both at moderate speeds.
• 2
  4140 pre-hard: tough substrateNegative rake and variable helix reduce chatter.
• 3
  Hardened D2: consider grindingAbove 45 HRC, carbide life drops fast.

Stainless steel work-hardens if the tool rubs. That single fact drives every choice. You need a sharp edge, a rigid setup, and a feed rate high enough to stay under the hardened layer. 303 free-machining stainless cuts at 60-120 m/min with a TiAlN-coated 4 or 5 flute cutter. 304 and 316 are gummier and lower sulfur, so they need a slightly lower speed and a heavier feed per tooth.

17-4PH is precipitation-hardening stainless. In the solution-treated state it cuts like 316, but after aging to 40 HRC it becomes abrasive and notch-sensitive. Use an AlTiN coating, a tough fine-grain carbide, and high-pressure coolant. Do not let the tool dwell or the edge will chip at the depth-of-cut line.

Titanium Ti-6Al-4V is where tool selection separates shops. The material has low thermal conductivity, so heat stays at the cutting edge. Use uncoated fine-grain carbide or an AlTiN coating, 3 or 4 flutes, and 30-60 m/min. Feed per tooth stays low, 0.02-0.06 mm, because the edge is thin. High-pressure coolant through the tool is almost mandatory for deep pockets.

The classic titanium mistake is running too slow with a light feed. That polishes the surface, generates heat, and work-hardens the next pass. Keep the tool engaged and let the chip carry heat away.

• 1
  Never rub stainlessLight feeds harden the surface and kill the next pass.
• 2
  17-4PH after agingTreat it like a hard alloy: AlTiN and high-pressure coolant.
• 3
  Titanium runs hotThrough-tool coolant and a sharp edge beat a coated edge.

Inconel 718 is the hardest common material we cut. It keeps its strength at 700 °C, which is exactly where the cutting edge sits. Carbide with an AlTiN coating works at 20-40 m/min with a low feed. Whisker-reinforced ceramic inserts can run faster in turning, 200-300 m/min, but they are brittle and need a rigid setup with no interrupted cuts.

The main failure mode is notching at the depth-of-cut line, not flank wear. Vary the depth of cut between passes so the notch does not concentrate. Keep coolant flowing; Inconel does not conduct heat away from the edge well. If the tool squeals, the setup is not rigid enough, and no coating will fix that.

Monel and other nickel-copper alloys are softer than Inconel but still gummy. They work-harden like stainless, so the same rules apply: sharp edge, positive rake, and a feed rate that stays under the hardened skin. Speeds sit between stainless and Inconel, roughly 30-50 m/min.

For these alloys, plan the tool change before the part is done. One worn edge on Inconel can scrap a 6-hour roughing cycle. Touch the edge after each pass on the first article.

• 1
  Vary depth of cutStops notching at the same axial line every pass.
• 2
  Ceramic is fast but brittleTurning only, no interrupted cuts, rigid setup.

Coolant strategy is half the decision. Aluminum wants air or mist. Steel and stainless want flood or high-pressure through-tool coolant. Titanium and Inconel need high pressure, ideally 70 bar or more, to break the chip and reach the edge. Magnesium bans water entirely. If you use the wrong coolant, a perfectly good tool will fail.

Rigidity matters more than grade on difficult materials. A 4,000 mm machine with a long reach tool will chatter on 17-4PH no matter which insert you buy. Shorten the tool holder, reduce the overhang, and check the workholding before blaming the carbide. On 5-axis work, verify that the rotary table is clamped and the tool axis is not reaching past the stable zone.

Sometimes the tool is fine and the process is wrong. A deep 2 mm slot in Inconel is a wire EDM job, not a milling job. A hardened D2 die detail is a grinding job. Knowing when to switch processes saves more time than optimizing speeds and feeds on the wrong one.

Finally, measure. Tool life data from your own machine beats any catalog number. Log the material, tool, speed, feed, and the number of parts before the finish drops or the edge chips. After a few jobs you will have a starting point that is more accurate than the chart.

• 1
  Match coolant to materialAir for aluminum, flood or high pressure for steel and titanium.
• 2
  Rigidity before gradeReduce overhang before buying a more expensive insert.
• 3
  Know when to change processEDM and grinding beat milling on some features.