Tooling basics

CNC Tool Selection Guide: 7 Essential Checks Before You Cut Metal

This guide covers how we pick a cutter for a specific feature, material and tolerance band. It is written for design engineers and buyers who approve a process, not for tool crib staff. Read it and you can tell whether a quoted tool path makes sense, and where a cheap cutter will cost you rework.

Get Instant Quote Talk to an Engineer

±0.005 mm toleranceØ400 mm rotary table3–5 day shipping

Custom auto spare parts machined with CNC tool selection for 5 axis work

On this page

Key takeaways

Start from the feature, not the catalogSlot width, corner radius and depth decide cutter diameter before any brand name enters the room.

Coating follows the materialAluminium runs uncoated or ZrN; steel and stainless want AlTiN or TiAlN; titanium wants sharp edges and low heat.

Runout eats tolerance0.03 mm of runout on a 6 mm cutter removes the finish you paid for.

Reach drives chatterPast 4:1 length-to-diameter, slow down or switch to a stub cutter.

Cheap tools suit soft geometryFor one-off brackets in 6061, a modest cutter often beats coated carbide on cost per part.

Selection matrix

Cutter choice by material and feature

Ratios assume a rigid setup on a 3-axis or 5-axis machine.

Work material	First-choice cutter	Coating	Watch out for
6061 / 6082 aluminium	2–3 flute carbide end mill	Uncoated or ZrN	Built-up edge at low rpm
7075 aluminium	3 flute, polished flutes	ZrN	Chips weld if coolant is weak
304 / 316 stainless	4–5 flute carbide, AlTiN	AlTiN or TiAlN	Work hardening on light passes
4130 / 4140 steel	4 flute carbide, AlTiN	AlTiN	Heat at the tip without flood coolant
17-4PH stainless	4 flute, tough substrate	AlTiN	Notch wear at the depth line
Ti-6Al-4V titanium	Sharp 4 flute, high helix	AlTiN, low speed	Heat kills edges fast
Inconel	6 flute, heavy core	AlTiN or AlCrN	Rubbing instead of cutting
POM / PEEK plastic	2 flute, polished, sharp	Uncoated	Melting and stringy chips

Check 1–2

Feature geometry sets the cutter before anything else

CNC tool selection starts with a drawing, not a catalog. The smallest internal corner radius on the part sets the maximum cutter diameter for that feature. A pocket with an R3 corner cannot be finished with a Ø12 mm end mill; the corner will be left as a step unless you add a smaller tool or a radius in the design. We read every drawing this way before quoting.

Slot width works the same way. A 6 mm slot cut with a 5 mm cutter takes two passes and leaves a witness line. A 6 mm cutter in a 6 mm slot rubs and breaks. The practical rule is a cutter between 60% and 90% of the slot width for roughing, then a full-width finishing pass if the tolerance is tight.

Depth decides flute length, and flute length decides rigidity. A cutter hanging 40 mm out of the holder in a Ø6 mm shank is a spring, not a tool. When the length-to-diameter ratio passes 4:1, expect to reduce feed per tooth by 30–50% and accept a lower material removal rate. On deep ribs we often switch to a stub cutter plus a longer neck tool for the last few millimeters.

1
Corner radius firstSmallest internal radius caps the finishing cutter diameter.
2
Slot ruleRough at 60–90% of slot width, then finish full width.
3
L:D over 4:1Reduce feed per tooth by 30–50% or change the setup.

Check 3–4

Coating and substrate must match the material

Coating is not a quality upgrade; it is a chemistry decision. Aluminium is soft and gummy, so a smooth, sharp edge with a thin ZrN layer or no coating at all cuts cleanest. A thick AlTiN coating rounds the cutting edge slightly, which raises cutting forces and encourages built-up edge on 6061.

Steel and stainless are the opposite case. At the tip, temperatures pass 600 °C in a cut. AlTiN and TiAlN form an aluminium oxide layer that slows diffusion wear and lets the edge survive longer. For 304 and 316 stainless the substrate matters as much as the coating; a tough, fine-grain carbide grade resists the chipping that comes with interrupted cuts.

Titanium and nickel alloys are the hard cases. Ti-6Al-4V conducts heat poorly, so the heat stays in the edge. Sharp geometry, low surface speed and plenty of coolant matter more than any coating. Inconel pushes this further, and we run AlCrN-coated tools at low speed with a heavy core to avoid rubbing. If a shop quotes Inconel with the same parameters as 4140, the tool life numbers in that quote are fiction.

1
AluminiumUncoated or ZrN; keep the edge sharp.
2
Stainless and steelAlTiN or TiAlN on a tough carbide grade.
3
Titanium and InconelSharp edge, low speed, high coolant pressure.

Check 5–6

Runout, holder choice and machine limits

Runout is the quiet killer of tolerance. On a 6 mm cutter, 0.03 mm of runout means one flute does most of the cutting. That flute wears twice as fast, the surface finish drops, and the hole diameter drifts. We check runout with a dial indicator at the tool tip before a finishing pass, and we keep it under 0.01 mm for work at ±0.005 mm.

The holder is part of the tool. An ER collet chuck is fine for general milling. Heat-shrink holders give better runout and clearance for deep pockets, and hydraulic holders absorb some vibration on long reach tools. If a job needs a Ø400 mm rotary table on a 5-axis center, the holder and tool assembly must clear the fixture through the whole tool path, not just at the start.

Machine travel also constrains the plan. Our largest envelope is 4,000 × 400 × 150 mm, with medium platforms at 750 × 1,150 × 550 mm and 600 × 600 × 600 mm. A tool long enough to reach the bottom of a deep cavity may exceed the Z travel once the holder is included. That is a fixture question as much as a tooling question.

1
Runout targetUnder 0.01 mm for finishing at ±0.005 mm.
2
Holder choiceHeat-shrink for deep pockets, hydraulic for long reach.
3
Check Z travelTool plus holder must fit the machine envelope.

Check 7

Cost per part, not cost per cutter

A Ø10 mm coated carbide end mill costs several times a cheap HSS cutter. On a 200-part run in 4140, the carbide tool usually wins because it holds size longer and needs fewer changes. On a single bracket in 6061 with loose tolerances, the cheap cutter can finish the job and the saving is real. The decision is cost per part, not cost per tool.

Tool cost is also a small slice of the total. Setup, inspection and the risk of a scrapped part dominate. A cutter that saves 20 minutes of cycle time but adds a 0.02 mm taper to a bore is a bad trade. We track tool changes and scrap per operation, which is why a quote may specify a more expensive cutter than the drawing seems to require.

For prototypes, the calculus shifts again. One or two parts rarely justify a custom form tool or a special insert. We would rather use a standard cutter and accept a slower cycle than make the customer pay for tooling they will never reuse. When a design moves to 10,000+ parts, a form tool or a custom insert starts to pay back.

1
Runs under 10 partsStandard cutters, accept slower cycle.
2
Runs over 200 partsCarbide or custom form tooling pays back.
3
Watch scrap riskA cutter that adds taper can cost more than it saves.

How we do it

Step by step: building a tool plan

The order matters; skipping a step usually shows up as chatter or a scrapped feature.

1
Read the drawing for the tightest featureFind the smallest internal radius and the tightest tolerance. That pair sets the finishing cutter diameter and the machine class before anything else is chosen.
2
Fix the setup and workholdingDecide how the part sits in the vise or fixture. If the tool cannot reach a face without a second op, note it now. Five-axis work often removes a second setup, which changes the tool count.
3
Pick the cutter family by materialAluminium: 2–3 flute uncoated or ZrN. Stainless and steel: 4–5 flute AlTiN. Titanium: sharp 4 flute, low speed. Plastic: 2 flute polished.
4
Set the length-to-diameter ratioKeep reach under 4:1 where possible. Past that, plan a stub cutter for roughing and accept 30–50% lower feed per tooth on the long tool.
5
Choose the holder for runout and clearanceHeat-shrink for deep pockets, hydraulic for long reach, ER collet for general work. Measure runout at the tip; keep it under 0.01 mm for tight finishing.
6
Set speeds and feeds from the tool data, then trimStart at the manufacturer's surface speed for the material, then adjust for setup rigidity. Reduce feed before speed when chatter appears; raising speed usually makes it worse.
7
Verify the finish on the first partMeasure the critical feature, check Ra, and inspect the tool edge under magnification. Catching a wear pattern on part one is cheaper than on part fifty.

FAQs

Questions engineers ask before approving a tool plan

When should we use high-speed steel instead of carbide?

HSS cutters tolerate shock better and cost far less. They make sense on low-volume aluminium or plastic parts, on manual setups, and where a broken cutter is likely because the setup is flexible.

Carbide wins on production runs in steel and stainless, and on any feature where size must hold across hundreds of parts. The harder the material and the longer the run, the clearer the carbide case.

Does a coating always extend tool life?

No. On aluminium, a thick coating can round the edge and increase built-up edge, which lowers finish quality. Uncoated or lightly coated polished tools often run cleaner.

On steel, stainless and titanium alloys, the right coating reduces diffusion and oxidation wear at the cutting edge. The gain is real but it comes from matching coating to material, not from buying the most expensive option.

How much runout is acceptable for precision work?

For general milling, 0.02 mm at the tool tip is workable. For finishing at ±0.005 mm, keep it under 0.01 mm and check with a dial indicator before the finishing pass.

Runout loads one flute harder than the others. That flute wears first, hole diameters drift, and the surface finish becomes uneven. Correcting the holder is usually faster than compensating in the program.

Can we cut deep pockets without a long, thin cutter?

Often yes. A stub cutter handles the bulk of the material, and a necked or reduced-shank tool reaches the last few millimeters. This keeps the stiff part of the setup doing most of the work.

If the design allows, adding a draft angle or a larger corner radius removes the need for a long tool altogether. That is a design change, so raise it before the drawing is frozen.

What matters most when we compare supplier quotes?

Look at the tool plan behind the number. A quote that names the cutter family, holder type and inspection method is easier to trust than a single price. Ask what tolerance the process holds on your tightest feature.

Volume, material and certification requirements change the plan. A medical part under ISO 13485 and an automotive part under IATF 16949 carry different documentation, and that shows up in the quote structure.