Laser Cutting vs CNC Machining: A Decision Framework for Plates

A 3 mm aluminum bracket, 120 × 80 mm, four 5 mm holes, one 20 mm slot. At 200 pieces, laser cutting produces it for around $1.40 each. CNC milling the same part from 3 mm plate costs about $7. Now change one detail: one of the holes becomes a 12 mm counterbore 2.5 mm deep. Laser cannot make that feature, the part now needs a second operation or a different process, and the two routes converge in price.

That is the whole shape of this decision. Laser and CNC machining are not competitors on thickness or on speed — laser is dramatically faster on flat profiles and cannot make a three-dimensional feature at all. They compete on the narrow band of parts that are flat but need something more than a through-cut.

If you buy brackets, plates, mounting panels and chassis parts, the cost difference between choosing correctly and incorrectly is usually a factor of three to five on the first order and a factor of two at volume.

What each process does to a plate

A fiber laser cuts a 2D outline. The beam melts and ejects material along a path, producing a through-cut with a kerf of 0.1 to 0.5 mm depending on thickness and lens. Everything the part needs must be reachable from one side, and everything must go all the way through.

A CNC mill works in three dimensions. It can profile an outline, but it can also pocket, counterbore, tap, chamfer, face and drill at an angle. It is slower per metre of cut by an order of magnitude, but it produces features that a laser physically cannot.

So the first filter is simple. If every feature in the part is a through-hole or a profile, laser is a candidate. If any feature has a floor — a pocket, a counterbore, a blind slot, a tapped hole with a specified thread depth — the part needs a machining operation somewhere, and the question becomes whether to cut the outline by laser and machine the rest, or machine the whole thing.

Edge quality, and where laser edges matter

A laser cut edge in mild steel is clean and square for the first few millimetres of thickness, with a fine striation pattern that most applications accept. As thickness increases, the striations coarsen and the kerf develops a taper, typically 0.05 to 0.15 mm per side on 6 mm plate and more above 10 mm.

Surface roughness on a laser cut edge runs Ra 3 to 6 µm, compared with Ra 0.8 to 1.6 µm from a milling cutter. For a bracket that is painted or powder coated, that difference is invisible. For a part with a sliding fit, a seal, or a visible edge on an anodized housing, it is not.

Two edge conditions matter most at design stage:

Dross. On thick steel and aluminum, laser cutting leaves a hard dross on the underside that must be removed by grinding or tumbling. That is a real cost, often $0.20 to $0.60 per part.

Heat affected zone. The cut edge has a narrow HAZ, roughly 0.1 to 0.3 mm on 6 mm steel. For most structural parts this is irrelevant. For parts that will be fatigue loaded or subsequently bent, it can matter.

The hole-size rule that catches designers

A laser cannot cut a hole much smaller than the material thickness without a penalty. The practical rule is that hole diameter should be at least equal to thickness, and preferably 1.2 times. A 3 mm hole in 6 mm stainless is possible but will come out tapered and out-of-round, and the pierce point will leave a mark.

The reason is the pierce. The laser must start each hole by punching through the material, which leaves a small crater and spatter before the cut establishes. On a hole near the thickness limit, the pierce consumes a large fraction of the circumference.

Milling has no such rule. A 3 mm hole in 6 mm plate is a drilling operation, held to ±0.05 mm and round within 0.02 mm.

Thickness limits worth knowing

CNC machining has no equivalent table. It will cut any of these materials at any thickness, limited only by the machine's Z travel and the length of the tool.

Where the cost curves cross

This is the part buyers actually want. The numbers below are for a 120 × 80 × 3 mm aluminum bracket with four 5 mm holes, quoted at typical Shenzhen rates.

There is no crossover on a flat part. Laser wins at every quantity, because its setup is trivial and its cut speed is measured in metres per minute rather than millimetres.

The crossover appears when features force a second operation. Add a 12 mm counterbore to that bracket and the routes look like this:

Now the answer depends on volume, and on whether the laser shop and the machine shop are the same company. If they are, the counterbore gets done in a second setup on a mill with the parts still nested, and the combined route wins above about 100 pieces.

When the right answer is both

The most common production route for plate parts is laser blanking followed by CNC finishing. The laser cuts the outline and all through-holes in one fast pass; the mill then machines the counterbores, tapped holes and any face that needs a flatness or finish specification.

That hybrid only works well when one supplier controls both steps, because the laser-cut outline becomes the datum for the milling operation. If two vendors split it, the mill has to find the outline again, and positional tolerance between the laser profile and the machined features is typically ±0.15 mm instead of ±0.05 mm.

Frequently asked questions

Can a laser cut a pocket that does not go through?

No. Laser cutting is a through-cut process. A pocket requires milling, or in some cases a laser ablation process that removes material layer by layer at a much higher cost per part.

Is laser cutting more accurate than CNC machining?

Generally no. A fiber laser holds ±0.1 mm on hole position and ±0.15 mm on profile, while a CNC mill holds ±0.02 to ±0.05 mm routinely. Laser is faster, not more precise.

What thickness can a fiber laser cut?

Production shops routinely cut mild steel to 20 mm, stainless to 12 mm and aluminum to 10 mm. Above those numbers the edge quality drops and machining becomes competitive even for flat parts.

Do laser cut parts need deburring?

Usually a light tumble or vibratory finish is enough to remove dross and soften the edge. On thick steel and aluminum, manual or robotic grinding of the underside is often needed, and that cost should be in your quote comparison.