Sheet Metal Fabrication in China: Process, Materials, and DFM

Sheet Metal · Fabrication in China Sheet Metal Fabrication in China: Process, Materials, and DFM Sheet metal is how enclosures, brackets, chassis, and panels get made — flat stock cut, bent, punched, welded, and finished into a 3D part in days, with no mold and no minimum run. Here is the process, the materials, the tolerances, and the DFM rules that decide whether your part is cheap or a rework loop. Request a quoteDFM rules What sheet metal fabrication is Sheet metal fabrication is the set of processes that turn flat sheet stock — steel, stainless, or aluminum — into three-dimensional parts by cutting, forming, and joining. There is no mold and no chip-cutting; the material starts as a coil or a blank and gains its shape through bending, punching, and welding. It is the default method for anything mostly thin wall: enclosures, brackets, panels, chassis, RF shields, and cabinets. The economics are the reason it dominates. Tooling is cheap — a press-brake die set or a turret-punch tool costs a fraction of an injection mold and changes in minutes — and lead time is measured in days, not weeks. The process scales from one prototype to thousands of pieces without a step change. The trade is geometry: sheet metal likes flat patterns and bends, not solid three-dimensional contours. A solid block belongs in CNC machining; a thin-walled, folded part belongs here. The design artifact that matters is the flat pattern — the unfolded outline of the part before bending. Every bend consumes a predictable length of material, accounted for by the bend allowance. Get that allowance wrong and holes drift and flanges come out short, no matter how carefully the shop bends. We return to that math in the DFM section. The process, step by step A sheet metal part moves through a fixed sequence, and each step has its own tolerance and failure mode. Understanding the sequence is how you read a quote and spot where a supplier cuts corners. 1. Cutting (laser or turret punch) The flat pattern is cut from sheet stock, usually on a fiber laser, which is tooling-free and holds a profile tolerance near ±0.1 mm with a clean, dross-free edge — the right choice for prototypes and complex outlines. For higher volume, a turret punch presses the profile with hardened tooling and adds formed features in the same cycle — louvers, embosses, knockouts, and countersinks a laser cannot make. Punching is faster at volume but needs tooling and leaves a slightly wider tolerance band. 2. Bending (press brake) Bending is the heart of sheet metal. A press brake drives a punch into a V-shaped die, folding the sheet along a straight line. The dominant method is air bending, where the punch does not bottom out and the angle is set by depth of stroke — fast and flexible, but sensitive to springback. Coining bottoms the punch into the die and stamps the angle, more accurate but slower and harder on tooling. Every material springs back a little after the bend, so the operator compensates by over-bending. The bend radius you specify is set by the tooling, not chosen freely — more on that below. 3. Welding and hardware insertion Where the design needs a closed seam or a structural joint, the formed pieces are welded — MIG for steel and stainless, TIG where the joint is thin or cosmetic. Beyond welding, this stage adds the mechanical hardware the part needs: PEM inserts (self-clinching nuts and studs pressed into the sheet), rivets, and weld studs. These are installed before finishing so the coating covers the hardware edge. 4. Finishing The part is cleaned, then coated, anodized, plated, or blasted to its final surface. Finishing is a separate discipline with its own quality risks, and it is the step most likely to be subcontracted — which is why vetting the finisher matters as much as vetting the fabricator. Materials: steel, stainless, or aluminum Three families cover the vast majority of sheet metal work, and the choice is driven by corrosion, strength, weight, and formability — in roughly that order. MaterialCommon gradesBest forWhat to watch Cold-rolled steelSPCC, CRS, DC01Internal brackets, painted enclosures, chassisRusts — needs powder coat or plating Galvanized / galvannealedSGCC, DX51D+ZOutdoor panels, corrosion without post-coatZinc fumes when welding; cosmetic marks Stainless steel304, 316Corrosion, food, medical, high strengthSpringback, higher cost, harder to form Aluminum5052, 6061Light weight, anodized cosmetics6061 cracks on tight bends; use 5052 for forming Cross-check any grade against the ASM Handbook before committing a drawing — grade chemistry and formability limits are material science, not opinion. Cold-rolled steel is the workhorse: cheap, stiff, weldable, and formable, but it corrodes, so it ships with a powder coat or zinc plate. Galvanized steel arrives pre-coated and skips post-finishing, at the cost of weld-fume control and a surface that shows marks. Stainless 304 is the default corrosion answer — formable and weldable, but it springs back more than steel, so tight angles cost extra care. Aluminum splits by grade: 5052 is the formable one, 6061 the strong one that cracks on a tight inside radius, so formed parts default to 5052. The full material-selection guide. Tolerances: what sheet metal can honestly hold Sheet metal is looser than machining, and that is by design — the process trades a few tenths of tolerance for speed and a near-zero tooling bill. Expect these bands: Laser-cut profile: ±0.1 mm on a laser, closer to ±0.25 mm on a turret punch. Bend angle: ±0.5° to ±1°, depending on material and tooling. Hole position: ±0.25 mm typical across a flat pattern. Flange length: ±0.5 mm, because bend radius and material thickness both vary. The sources of that looseness are physical, not careless: material thickness varies within its mill tolerance, the bend radius is set by whatever tooling is on the brake, and springback shifts the angle on every stroke. So you do not put a ±0.05 mm callout on a sheet metal drawing — you would be paying for a process that cannot deliver it. When a feature genuinely needs tight tolerance — a dowel-pin bore, a bearing seat, a datum face — machine that feature after bending or make it a separate machined insert. That is the handoff where a partner with in-house CNC earns its keep: the sheet metal holds the shape, and the mill holds the tenths. DFM: bend radius and the k-factor The two numbers that decide whether a sheet metal part forms cleanly are the bend radius and the k-factor, both set at the drawing, and both where parts silently go wrong. Bend radius is the inside radius of the fold, and it has a floor set by the material. The rule of thumb is roughly one material thickness (1T) for mild steel, 1.5–2T for stainless, and 1.5–3T for aluminum — 6061 at the higher end because it cracks readily. Bend sharper than the floor and the outer surface stretches past its elongation limit and tears. Specify a radius at or above the floor, and keep one consistent radius across the part so the brake does not swap dies mid-run. k-factor is the position of the neutral axis — the imaginary line inside the material where the metal neither stretches nor compresses during the bend. Expressed as a fraction of the material thickness, it lands near 0.4–0.45 for steel, drifting with the ratio of bend radius to thickness. The k-factor feeds the bend allowance, the length of material consumed by the fold: Bend allowance = bend angle × (inside radius + k-factor × material thickness). That allowance, summed across every bend, converts your formed model into the flat pattern. Get the k-factor wrong and the flat pattern is the wrong length — holes land off-position and flanges come out short, errors that surface only after the first article comes back from the brake. A competent shop states the k-factor it assumes up front and corrects it from the first article, so ask for a flat-pattern check before production. Two more rules keep bends from cracking. First, bend across the grain whenever the shape allows — sheet stock has a rolling direction, and bending parallel to it concentrates stress along the weakest path, especially in aluminum and stainless. Second, keep bend lines away from hole edges and notches, because a bend running through a cut edge is a guaranteed crack starter. DFM: relief, holes, and the details that catch you The bend is the expensive part of sheet metal, and most DFM failures happen at the intersection of a bend and a feature. These rules separate a part that forms first-try from one that tears or distorts. Bend relief. Where a bend runs into a corner or a perpendicular edge, cut a small relief notch so the material can fold without tearing. The relief is roughly one material thickness wide — cheap insurance against a crack at the flange corner. Minimum hole diameter. A punched hole should be at least one material thickness in diameter — 1.5T is the comfortable floor — because smaller holes deform on the exit side. A hole smaller than the sheet thickness is a machining operation wearing a sheet metal price tag. Hole-to-edge distance. Keep a hole at least two material thicknesses from a cut edge, or the web between the hole and the edge distorts and can tear under the punch. Holes near bends. Keep holes at least 2.5× material thickness plus the bend radius away from a bend line, or the hole stretches into an oval as the bend pulls material past it. Minimum flange height. A flange shorter than about four material thicknesses plus the bend radius cannot be gripped by the die and will not form cleanly. If the design needs a tiny flange, expect it to be formed with a secondary operation or machined instead. Inside corner radii on the profile. Laser-cut internal corners should carry a radius at least equal to the material thickness, so the profile cuts cleanly and the bend does not start from a sharp notch. None of these rules add cost; they remove it. A part drawn with relief, sensible hole clearances, and one consistent bend radius drops straight onto the brake, while the same part drawn without them spends an extra cycle being re-cut and re-formed. The complete DFM guide. Finishes: powder coat, anodize, and plating Finishing is where a sheet metal part gets its corrosion resistance and its cosmetics, and the choice is set by the base metal: steel is coated or plated, aluminum is anodized, stainless is usually bare or passivated. Pick wrong and you pay for protection you do not need or ship a part that rusts in the crate. FinishBase metalWhat it givesNotes Powder coatSteel, aluminumTough, thick (50–100 µm), any colorDefault for enclosures; hides minor surface flaws Anodize (Type II)Aluminum onlyThin oxide, cosmetic color, corrosionDyeable; won’t hide scratches Hard anodize (Type III)Aluminum onlyThick, wear-resistant oxideGrows into the surface; changes dimensions slightly Zinc platingSteelSacrificial corrosion, low costOften chromate passivated on top Nickel / chrome platingSteelDecorative, hard, corrosionCosts more; used for visible hardware PassivationStainlessRestores the passive oxide, no coatingASTM A967; not a coating Powder coat is the general-purpose answer for steel: a dry polymer sprayed electrostatically and oven-cured into a film thick enough to take abuse and hide minor marks. Anodizing builds an aluminum-oxide layer directly into the surface — Type II for cosmetics and color, Type III hardcoat for wear — but it only works on aluminum and grows the surface by a few microns, so tight fits need allowance. Plating covers steel: zinc is the sacrificial workhorse, nickel and chrome are the decorative and hard options. Passivation is not a coating — it restores the chromium-oxide film on stainless so the metal protects itself. For texture without chemistry, bead blasting and brushing are the defaults. The full surface-finish reference. Sheet metal vs CNC machining vs injection molding The three processes compete for enclosures and housings, and the choice comes down to three questions: how thin is the wall, what volume, and what tolerance. Sheet metal wins for thin walls (0.5–3 mm), low-to-medium volume, and geometry that is fundamentally folded. Tooling is near-free, lead time is days, and design changes cost nothing. It loses when the part is solid, the tolerance is tight, or the shape has no bend lines. CNC machining wins for solid geometry, thick sections, and tolerances in the ±0.01 mm range. A machined enclosure is more rigid and precise than a folded one, but it costs more per part and wastes billet material, so it is reserved for low volume or where stiffness and tolerance dominate. Injection molding wins at high volume for plastic parts with complex shapes and thin walls. The mold is expensive and takes weeks, but amortized over thousands of pieces the per-part cost collapses. It loses at low volume and whenever the part must be metal or change quickly. The practical pattern for hardware teams: folded sheet metal for the first enclosures and brackets through EVT → DVT → PVT, because it iterates in days and carries no tooling commitment; then, only if volume or aesthetics demand it, move to molded or die-cast housings once the design is frozen. Die casting vs CNC for comparison. Why China for sheet metal Sheet metal is a cluster business, and China’s manufacturing belts run the densest clusters of it anywhere. In the Pearl River Delta — Dongguan and its surrounding towns — laser cutting, bending, welding, and finishing sit minutes apart, and the sheet stock, hardware, and coating lines that feed them live in the same radius. That density changes the economics three ways. First, tooling is cheap and local: press-brake dies and punch tooling are made down the road, so a custom bend radius or a formed feature is a same-week order, not an import. Second, labor depth: press-brake operators in the cluster have run your exact part geometry thousands of times, which turns a ±1° angle into a ±0.5° one. Third, finishing is a shared service: the powder-coat line, the anodizer, and the plater are specialists serving every shop in the district, so a small fabricator delivers a finished part without owning any of those lines. The honest caveat applies to every process in China: the cluster holds world-class shops and shops that cut corners, often quoting similar prices. In sheet metal the risk concentrates in the finish — a powder-coat line with poor pretreatment passes visually and peels in a year — and in flat-pattern discipline, where a shop that never checks the k-factor ships parts whose holes drift. The fix: request a measured first article, confirm the finisher, and hold the partner to documented quality. Vetting a supplier without flying out. Nex-G: sheet metal through vetted partners, QA-managed Nex-G’s own floor is EMS and CNC under one roof in Dongguan Hengli — a 6,800 m² facility staffed by more than 100 people and running since 2006. Sheet metal fabrication and stamping are sourced through a vetted partner network and QA-managed by Nex-G, which matters: the enclosure, bracket, or chassis comes back to a shop that can machine to the same drawing, inspect to the same standard, and integrate the part into the same build the electronics live in. The anchor is the quality system behind the sourcing. Nex-G holds ISO 9001, IATF 16949 (build-to-print — design excluded under clause 8.3), and ISO 14001, with URS certification to 2027. SPC runs to a Cpk target of ≥1.67 on critical characteristics and a floor of ≥1.33, backed by real data. That discipline is applied to sourced sheet metal: incoming inspection, a measured first article against the flat pattern, and finish verification before the part enters your build. In-house, 80+ CNC machines from Mazak, Brother, TSUGAMI, and Sodick hold ±0.005 mm on milled and turned features and ±0.002 mm on grinding and wire EDM — the capacity that picks up any sheet metal feature needing a machined tolerance. The service runs no MOQ, carries programs from EVT → DVT → PVT, and quotes lead times of 3, 7, and 30 days by scope. One partner manages the sheet metal, the machining, and the board, so the fit is checked at the bench, not at your dock. See the full capability. Frequently asked questions What is the minimum order for sheet metal parts?None, through Nex-G’s sourced network. Because the tooling is press-brake dies and laser programs rather than a mold, a single prototype costs little more than material and machine time, and the same flat pattern scales to production with no step change. Per-unit cost is higher at low volume because setup is near-fixed. What tolerances can I realistically hold?Plan for ±0.1 mm on laser-cut profiles, ±0.5° to ±1° on bend angles, and ±0.5 mm on flange lengths. For a feature that needs tighter — a bearing seat or a dowel bore — machine it after bending rather than asking the brake for a tolerance it cannot deliver. Steel, stainless, or aluminum — how do I pick?Steel if cost and stiffness matter and the part will be powder coated or plated. Stainless 304 if the environment is corrosive or the part is food- or medical-contact. Aluminum 5052 if weight matters and the part is formed; 6061 only for flat work or generous radii, since it cracks on tight bends. What minimum bend radius should I specify?Roughly one material thickness for mild steel, 1.5–2T for stainless, and 1.5–3T for aluminum. Going sharper risks cracking the outer surface. Keep a single consistent radius across the part to avoid die changes, and bend across the rolling grain where the shape allows. Powder coat or anodize?It is decided by the base metal. Steel gets powder coat or plating; aluminum gets anodize. Powder coat is thick and hides minor flaws, anodize is a thin oxide that shows every scratch but wears well. You rarely choose between them — you choose the metal, and the finish follows. When should I machine a part instead of bending it?When the wall is thick, the geometry is solid rather than folded, or a tolerance drops below ±0.1 mm. A machined enclosure is more rigid and precise but costs more and wastes material, so it earns its place at low volume or where stiffness and tolerance dominate. Do you make sheet metal in-house?Nex-G sources sheet metal fabrication and stamping through a vetted partner network and QA-manages the result in-house — incoming inspection, a measured first article, and finish verification under the same ISO 9001 / IATF 16949 / ISO 14001 system and SPC discipline that runs the CNC floor. CNC and EMS are in-house, so the sheet metal, the machining, and the electronics integrate under one quality gate. Sourcing sheet metal for your build?Send the drawing and the finish spec — we will quote the fabrication and confirm the flat pattern before anything hits the brake.Request a quote Related articlesDie Casting vs CNC MachiningCNC Machining Cost in ChinaThe Complete Guide to Materials Selection