CNC Machining vs Laser Cutting: Which Process Fits the Part

CNC machining and laser cutting are not two ways of doing the same job. A fiber laser melts a narrow path through sheet metal and produces a two-dimensional profile in one pass; a CNC mill drives a rotating cutter through solid stock and produces pockets, bores, threads, and contoured faces, feature by feature. So the choice starts with geometry, not accuracy: flat parts cut from sheet go to the laser, parts with machined features go to the mill, and parts that need both often run as a laser-cut blank followed by CNC finishing. Tolerance, thickness, and volume then refine the call, and this page works through each factor with concrete numbers.

The core trade: geometry before accuracy

Many comparisons frame CNC versus laser as a precision contest. That framing misleads buyers, because the two processes make different kinds of geometry, and almost every part clearly needs one kind or the other. A laser part is defined by its outline and its through-holes. A machined part is defined by features cut to depth: a pocket with a floor, a bore that fits a bearing, a thread, a face that must sit flat against another part.

Profiles versus features

A flat-bed fiber laser moves a focused beam in X and Y over a sheet, so every feature it produces goes all the way through the stock: the outer contour, holes, slots, and cutouts. It cannot cut partway through, cannot machine a surface flat or smooth, and cannot produce a thread. A milling machine spins a tool and positions it in X, Y, and Z, so it controls depth. It cuts pockets with real floors, counterbores, stepped features, tapped holes, and angled or contoured faces, and a 5-axis machine can reach several of those faces in one setup.

The tool shapes the limits, too. A laser’s kerf is narrow, 0.15 to 0.30mm, but the beam always burns through, and its heat leaves a thin heat-affected zone, 0.13 to 0.25mm on mild steel. A milling cutter is round, so every inside corner carries a fillet, typically 0.2 to 0.5mm for standard endmills, but the cutter leaves a machined surface rather than a cut edge, and it can hold depth to a few hundredths of a millimetre.

Where the two overlap

A flat bracket cut from 3mm sheet could come off either machine, and so could a simple plate with holes. The deciding callouts sit on the drawing. If the part shows a pocket, a counterbore, a thread, or a flatness callout on a face, laser alone cannot make it. If every feature is a through-hole or an outline, milling it wastes machine hours on geometry the laser produces in seconds at a fraction of the cost. Overlap exists, but the drawing resolves it fast.

When laser cutting is the right choice

Thin to medium sheet with profile geometry

Choose laser when the part is flat and its features go through. A 2mm stainless panel with a perforation pattern is the classic case: the laser holds about ±0.10mm on thin sheet (0.5 to 3mm), the narrow kerf preserves fine cutouts and small holes (minimum hole and slot size is about 1x the material thickness, tabs 2x), and the cut edge is clean enough to weld or coat as-cut when nitrogen assist is used. Brackets, gussets, enclosures, guards, and decorative screens all fit this description.

Speed compounds the advantage. On thin stock a fiber laser covers many metres of cut path per minute, so a full sheet of nested parts finishes quickly, and per-part cost falls steeply as the batch grows.

Volume and nesting economics

The laser’s economics come from the sheet, not the part. Parts nest tightly together, limited mainly by kerf compensation of about half the kerf per edge, so material utilization is high and the waste skeleton is thin. Setup is light: no fixtures to build, no tools to change, just a nesting program and a sheet. That is why laser-cut sheet parts stay cheap at quantity, and why buyers move flat work to the laser whenever the drawing allows it. The laser cutting thickness guide carries the tolerance-by-thickness detail.

When CNC machining is the right choice

Pockets, bores, threads, and faces

Choose CNC milling when the part has depth features. An aluminum housing with a deep pocket, bolt holes, and a mating flange is a milling job, full stop; no laser can cut the pocket or finish the flange. A valve block with cross-drilled passages, a fixture plate with reamed dowel holes, a shaft with a sealing groove: all machined parts. Drilled holes run practical to about a 4:1 depth-to-diameter ratio, threads come from taps or thread mills, and bores that must fit bearings get bored or reamed to size.

Turning extends the same logic to round parts. Diameters, tapers, and threads around a centerline belong on a lathe, where standard work holds about ±0.025mm. Nothing about a laser enters that conversation, because a lathe part has no flat profile to cut.

Tolerances and finishes a laser cannot hold

Milling holds ISO 2768-1 fine class as a working default: ±0.05mm on features from 0.5 to 3mm, ±0.10mm from 6 to 30mm, ±0.15mm from 30 to 120mm. Precision setups reach ±0.025mm, and high-precision work can hold ±0.013mm on rigid machines. Surface finish is a separate lever the laser does not have at all: a standard as-machined face runs about Ra 3.2µm, a fine-finishing pass can reach Ra 0.8µm, and grinding reaches Ra 0.4µm or better. Sealing faces, bearing seats, and sliding surfaces are specified this way, and only machining delivers them.

Worked examples

Three parts show the routing logic. First, a batch of 2mm aluminum mounting brackets with slots and holes, tolerance ±0.2mm: laser, without hesitation, nested ten-up on a sheet. Second, an aluminum actuator housing with a 12mm-deep pocket, two tapped M5 holes, and a ±0.05mm bore: CNC milling, because the pocket, threads, and bore are machined features no laser can form. Third, a 12mm steel fixture plate with a laser-friendly outline but also a central pocket, two bearing bores at ±0.05mm, and four tapped M6 holes: the hybrid route, which the next section unpacks.

The third example is the common trap. Buyers quote the plate as a machining job and pay to profile the outline on the mill, or quote it as a laser job and discover the bores cannot be cut. Splitting the process solves it.

The hybrid workflow: laser-cut blank plus CNC finishing

Many production parts need both processes, and running them in sequence is standard shop practice for plates and panels that carry machined features.

Which step carries which features

The laser cuts the near-net outer profile, lightening holes, and any large through-holes, because through-profiles are what it does cheaply and fast. Add a small machining allowance to the profile so the mill can finish critical edges to size. The mill then handles everything with depth: facing the plate flat, milling pockets, boring holes to ±0.05mm or tighter, tapping threads, and machining faces that must seal or locate. Bulk material removal happens at laser cost, and precision happens only where the drawing demands it.

A worked hybrid example

Take that 12mm mild-steel fixture plate again, 300 by 200mm. The laser cuts the outline, a large central relief, and corner holes in minutes from nested plate. The mill then faces the plate, mills the central pocket, bores the two bearing holes, taps the M6 pattern, and finishes the datum edges. Compared with milling the whole plate from oversize stock, the mill spends its hours only on the features that need it, and the profiling work happens on the machine built for it. Shops that run both processes route this way by default; shops that run only one will sub-contract the other step, and the drawing should anticipate the split.

Tolerance and edge quality compared

On thin sheet the tolerance gap between the processes is small: the laser holds about ±0.10mm at 0.5 to 3mm, and standard milling holds ±0.13mm with routine precision to ±0.025mm. The gap widens with stock thickness, because the laser’s tolerance is thermal and drifts as heat disperses into more material: about ±0.15mm at 3 to 6mm, ±0.25mm at 6 to 12mm, and ±0.50mm at 12 to 25mm in mild steel. Milling tolerance, by contrast, depends on the machine, the setup, and the feature, not on the stock thickness in the same way.

What each process leaves on the surface

The edge each process leaves is a category difference. A laser cut edge has a kerf, a striation pattern, possible thin oxide (with oxygen assist on carbon steel), and a heat-affected zone of 0.13 to 0.25mm on mild steel. A milled surface is cut, not burned: Ra 3.2µm as-machined, smoother with a finishing pass or grinding. Neither substitutes for the other. A laser edge can be left as-cut for most welded or painted work, but a bearing bore or a gasket face must be machined.

Corners and features at the small end

At the feature scale the processes trade again. The laser’s minimum inside corner radius is about 0.5mm, and holes and slots scale with thickness (1x minimum, 2x for tabs and bridges). Milling needs a corner fillet set by the tool, 0.2 to 0.5mm typical, but it can machine features far smaller than the stock thickness, cut threads, and hold depth. Small through-holes in thin sheet favor the laser; small features with depth favor the mill.

Thickness and stock limits

The laser is a sheet and plate process within a defined band: about 20mm practical in steel and stainless, about 15mm in aluminum, with tolerance and edge quality degrading toward the top of the range. Below that band nothing changes; the laser does not care whether the sheet is 0.8mm or 8mm, only how the parameters are set. Milling has no thickness band at all. The limits are the machine envelope and workholding: a mill can face a 100mm-thick block if the machine travels and the fixture allow it, while a laser cannot cut a 100mm block under any parameters. Very thin stock inverts the comparison, though. A 0.5mm shim cuts cleanly on a laser and is miserable to mill, because it deflects under cutting force and will not clamp rigidly. Thick plate beyond the laser’s range routes to plasma or waterjet, a choice the laser vs plasma and laser vs waterjet pages cover in detail.

Cost drivers compared

What makes a CNC part expensive

Machining cost is machine hours plus setup. The levers are the volume of material removed (deep pockets and full-profile work eat time), the number of setups (each new fixture adds labor and error risk), the tolerance callout (tightening every feature to ±0.025mm adds 20 to 50 percent through slower feeds, finer tooling, and more inspection), the finish callout, and the material itself: titanium machines at 20 to 30 percent of the rate of free-machining brass and needs carbide tooling and flood coolant, so the same part in titanium costs far more to cut than in aluminum. Setup amortizes across the batch, which is why machined parts suit prototypes through mid volumes.

What makes a laser part expensive

Laser cost is path, thickness, and material. The machine charges by cut length and pierce count; thicker stock cuts slower and needs more power and gas; high-pressure nitrogen assist, specified for clean oxide-free edges on stainless and aluminum, is a real consumable cost; and the sheet price and nesting efficiency set the material component. Tolerance barely moves the price, which is the mirror image of machining. The asymmetry matters for buyers: on the laser you pay for geometry you could simplify, on the mill you pay for precision you may not need everywhere.

Materials each process handles

The overlap covers the common sheet metals: mild steel, stainless, and aluminum all cut on fiber laser and all machine on CNC. Outside that overlap the processes diverge sharply. Copper and brass are poor fiber-laser materials, because they reflect the 1064nm beam; they machine beautifully, and free-machining brass C360 is the machinability benchmark. Titanium and the engineering plastics (acetal, PEEK, glass-filled nylon) are CNC materials with no laser-cutting story at all. On the other side, thin sheet in any laser-friendly alloy is a laser material, because milling thin sheet is slow and distortion-prone. Material alone rarely decides the process, but it can veto one.

When neither process fits

Some parts should not go to either machine. Stock thicker than the laser’s range (about 20mm steel) and looser than ±0.5mm is plasma work; reflective metals and any heat-sensitive work, where even a 0.13 to 0.25mm heat-affected zone is unacceptable, go to waterjet, which cuts cold. The process comparison matrix holds the summary rows across all processes. And simple parts at high volume, a flat washer, a bent clip, a molded housing, outgrow both: stamping, casting, and molding amortize tooling and win on per-part cost once volumes justify the tool. CNC and laser both pay machine time on every part, which is their strength at low and mid volume and their limit at scale.

How to choose

Four questions route almost every part. Does every feature go through the stock, or does the part need pockets, bores, threads, or machined faces? Through-features alone point to laser; depth features point to CNC or the hybrid route. What tolerance does the drawing call out? ±0.1mm-class work is comfortable on thin sheet either way; ±0.025mm work is machining. What is the stock? Sheet within the laser’s thickness band cuts economically; solid blocks and thick sections machine. And what is the volume? Laser unit cost falls fast with nesting; machining setup amortizes more slowly and rewards consolidated setups.

When a part answers both ways, split it: laser the blank, machine the features. The laser cutting and CNC machining hubs carry the full process detail behind each leg of that decision.