Sheet Metal Fabrication vs CNC Machining: Choosing a Route for Enclosures and Brackets
An enclosure that starts life as a milled billet is often the most expensive version of itself. Cut the same box from 1.5 mm 5052-H32 and the material cost drops, the cycle time drops, and the only thing you give up is the ±0.02 mm bore you did not actually need. The reverse also happens: a bracket with a tapped boss, a sealed face and two coaxial bearing seats gets routed to laser and press brake, then comes back with hole-to-hole position wandering ±0.3 mm and a sealing face that will not hold a gasket. Both outcomes come from the same mistake — picking the process before reading the tolerance stack. This one walks through where each route wins on geometry, tolerance, volume and finish, using the numbers that show up on real prints.
What Each Process Actually Produces
Sheet metal works from a blank of constant thickness. Cutting defines the outline, the press brake defines the bends, and everything else — hardware, welding, finishing — happens after. Wall thickness is fixed by the sheet you buy, so a 1.5 mm bracket stays 1.5 mm everywhere, including the flanges you wish were thicker. Tolerances accumulate through the bend sequence, and every bend you add moves the features downstream of it.
CNC machining removes material from solid stock, so thickness becomes a dimension you control feature by feature. A pocket can be 3 mm deep in one region and 8 mm in another; a boss can be raised where a bearing sits and milled flush where a cable passes. That freedom costs machine time, and machine time is the dominant cost driver at every quantity. Our CNC machining cost guide breaks down how setup, cycle time and inspection split the quote.
Tolerance: Where the Two Routes Separate
Process capability is the honest place to start. A laser-cut blank followed by a brake bend holds dimensions in the tenths-of-a-millimetre range; a machining centre holds hundredths. The gap sounds small until you stack four bends and three hole patterns into one assembly.
| Feature | Sheet metal, typical | CNC machined, typical | What drives the difference |
|---|---|---|---|
| Overall profile | ±0.2 to ±0.5 mm | ±0.05 mm | Kerf width and bend springback versus cutter position |
| Hole-to-hole | ±0.1 to ±0.3 mm | ±0.02 to ±0.05 mm | Stack-up across bends versus single-setup machining |
| Bore diameter | ±0.1 mm (laser), ±0.05 mm (punched) | ±0.01 mm (reamed/bored) | Laser kerf taper versus a reamer sized to the fit |
| Flatness on a 300 mm panel | 0.5 to 1.5 mm | 0.05 to 0.1 mm | Residual stress from rolling and bending versus a faced surface |
| Perpendicularity of a flange | 0.5° to 1° | 0.05° | Brake tooling and material springback |
| Surface roughness, as produced | Ra 1.6–3.2 µm | Ra 0.4–1.6 µm | Mill finish versus as-rolled sheet |
Two consequences follow. First, if your drawing calls out positional tolerances tighter than ±0.1 mm across a folded assembly, sheet metal needs a secondary machining step — or the design needs to move to solid stock. Second, sheet metal parts that truly need a precision bore get one locally: laser the pilot hole, then ream it in a fixture. That hybrid is common and cheap. For parts where the bore is the function, read up on tight tolerance machining of aluminium alloys before committing to a route.
Cost Structure: Tooling Versus Cycle Time
The two processes invert each other on cost. Sheet metal carries almost no tooling at low quantity — a laser program and a brake setup — and then scales down sharply with volume once you add a progressive die. CNC carries the same setup cost at one part as at five hundred, because the cycle time per part barely moves.
| Quantity band | Usually cheaper | Reason |
|---|---|---|
| 1–20 pieces | Sheet metal or CNC, decided by geometry | No tooling either way; cycle time and material removal dominate |
| 20–300 pieces | Sheet metal (laser + brake) | Cycle time per part falls well below milling a pocket from solid |
| 300–1,000 pieces | Either, depending on features | Fixture investment in CNC starts paying back against bend-handling time |
| 1,000+ pieces | Stamped sheet metal | Progressive die amortises tooling across the run; per-part time drops to seconds |
Those bands are rules of thumb, not a quote. The crossover point moves with part size, number of bends, material, and whether secondary machining is required. A 40 mm clip with two bends crosses over far earlier than a 400 mm chassis with twelve forming stations. Where the volume is genuinely uncertain, prototype in sheet metal and keep the CNC route open — see how we handle low volume CNC production runs for that middle ground.
Material and Thickness Limits
Sheet metal constrains you to standard mill thickness, and each alloy has a bend limit that decides whether your flange cracks:
- 5052-H32 — bends down to roughly 1× material thickness, the safe default for brackets and chassis in the 0.8–3 mm range.
- 6061-T6 — needs about 1.5–3× thickness for a clean bend; strong and anodizes well, but a tight radius in T6 temper will crack along the grain.
- 304 / 316 stainless — work hardens fast, springs back heavily, and needs over-bend compensation worked out on the first article.
- Cold-rolled steel — forgiving to form, but every exposed edge needs a coating decision before the part leaves the shop.
Aluminium sheet and plate composition is governed by ASTM B209, which is the specification to cite on a print rather than a trade name. Grain direction matters too: a bend running parallel to the rolling direction on 6061-T6 is the classic crack site, and rotating the blank 90° on the nest usually fixes it at zero cost.
Geometry That Fights Sheet Metal
Some features simply do not belong on a folded part. Watch for these before the RFQ goes out:
- Coaxial bores on opposite walls — two bends of accumulated error between them.
- Deep tapped holes — a 1.5 mm sheet gives you about one thread of engagement; you need a PEM nut, a welded boss, or a thicker local section.
- Sealing faces for gaskets or O-rings — flatness from a brake will not hold a compressible seal across a long flange.
- Blind pockets with tight depth — a mill can hold ±0.05 mm depth; a formed feature cannot.
- Thick sections next to thin ones — sheet metal cannot vary thickness without welding on a second piece.
None of these are disqualifying. They are decisions: move the feature to a machined insert, relax the tolerance to what the assembly actually needs, or change process. A short design for manufacturability review before tooling usually finds the cheap version of all three.
Finishing Changes the Answer
Finish thickness is not cosmetic — it is dimensional. Powder coat builds 60–120 µm per side, which will close a clearance fit or make a threaded PEM stud hard to start. Type II anodizing builds 5–25 µm, roughly half of which grows outward. Chem film adds essentially nothing, under 1 µm, which is why it is specified on parts with tight fits and grounding requirements.
Sheet metal brings its own finishing problems. Weld seams and heat-affected zones discolour under anodizing, so a welded corner that looks fine bare turns into a visible band on a black anodized panel. Laser-cut edges hold coating poorly at sharp corners, and recesses shield the Faraday effect during powder application, leaving thin film inside deep channels. Define cosmetic zones on the drawing before production, not after first article. Our powder coating service and anodizing service pages cover what each finish needs from the substrate, and the CNC surface finishing overview ties the options together.
Hybrid Routes That Usually Win
- Laser cut + CNC ream — cheap blanking, precision where the bearing sits.
- Stamped blank + machined bosses — volume economics on the flat features, machined accuracy on the interfaces.
- Folded chassis + machined front panel — the cosmetic, connector-bearing face is milled; the structural box is folded.
- Fabricated assembly, finished as one — cut, form, weld, then coat the whole unit so colour and film thickness match across parts.
Coordination matters more than any single process here. Fabrication, stamping and finishing run from one plan at JLYPT sheet metal fabrication, so bend relief, burr direction, hardware installation and masking get settled before material is cut instead of after the parts come back wrong. High-volume programs move to dedicated OEM production cells once the process is validated.
What to Send With the RFQ
| Item | Why it changes the quote |
|---|---|
| STEP or DWG with tolerances marked | Separates cosmetic dimensions from functional ones |
| Quantity now and per year | Decides laser + brake versus progressive die |
| Material and temper | Sets bend radius, springback and coating compatibility |
| Cosmetic zones identified | Determines handling, masking and inspection level |
| Finish specification with thickness | Feeds back into fit tolerances and masking plan |
| Assembly interfaces | Shows which features need local machining |
Frequently Asked Questions
Is sheet metal always cheaper than CNC?
No. Below roughly 20 pieces the difference is driven by how much material a mill has to remove, and a deep, chunky part can be cheaper from solid than from a welded assembly of five folded pieces. Sheet metal wins clearly once the part is genuinely a folded shell.
Can a folded part hold ±0.05 mm?
Not across bends. Locally, yes — machine the feature after forming. Anything measured from a datum on the other side of a bend inherits that bend’s variation.
Do sheet metal parts anodize well?
Aluminium sheet anodizes fine; welds and heat-affected zones do not match. If appearance matters, either design the welds out of the cosmetic faces or pick a finish that hides the variation.
What thickness range makes sense?
0.5–6 mm covers most fabricated parts. Below 0.5 mm, handling and distortion dominate; above 6 mm, machining from plate usually beats forming. Material data from ASM International is a good reference when you are choosing between tempers.
Sending One In
Send the model and the drawing with the functional tolerances marked, and state the annual quantity even if the first order is small — that single number decides whether we quote laser and brake or a die. If you are unsure which route fits, request a quote with both options noted and we will price them side by side. For enclosures specifically, the machined electronic enclosure route is worth comparing before you commit to a folded design.
Four inputs decide most quotes: the drawing, the material grade, which features carry tolerance, and target quantity. Put those through the JLYPT quote form and pricing comes back tied to them, with bend radius against grain direction priced in rather than averaged. The production setup behind it is described on the sheet metal fabrication shop.
