Sheet Metal Fabrication
Also: sheet metal, precision sheet metal, sheet metal fab, metal fabrication, enclosure fabrication, sheet metal parts, fab shop
Sheet metal fabrication cuts, bends, welds and finishes flat stock into brackets, enclosures and chassis: no hard tooling, fast turns, one piece to thousands.
1,699 sheet metal fabrication companies in the Noramark directory
Sheet metal fabrication is a routing, not a single machine. A flat pattern is cut from sheet on a laser, a turret punch or a waterjet, deburred, bent on a press brake, fitted with hardware (PEM nuts and studs, rivets, weld nuts), welded or riveted into an assembly, and finished with powder coat, plating or anodize. Every step uses general-purpose tooling, so a new part costs programming time rather than a die.
It is the fastest, cheapest way to make thin-walled metal parts: brackets, enclosures, chassis, panels, guards, cabinets and frames from 0.5 to 6 mm (0.020 to 0.250") stock. Flat-pattern features come out at ±0.13 mm (±0.005") because the laser or punch is a precision machine. Bent features are looser, about ±0.25 mm (±0.010") per bend, because each bend depends on thickness variation, springback and the brake setup.
The limits come from the material form. Wall thickness is constant across the part, features sit on the surface or go through it, and tolerances stack across every bend. A part that needs a thick section next to a thin one, a bore held to ±0.025 mm (±0.001"), or a tight hole pattern across two bends is usually machined, cast, or built as a weldment with machined details.
At a glance
| Typical tolerances | Flat-pattern features (cut or punched) ±0.13 mm (±0.005"). Bend-to-edge ±0.25 mm (±0.010") standard, ±0.13 mm (±0.005") with care; bend angle ±1° standard, ±0.5° with care. Hole-to-hole across a bend ±0.38 mm (±0.015"). Welded assemblies ±0.8 mm (±1/32") as welded; ±0.13 mm (±0.005") only on features machined after welding. |
|---|---|
| Size limits | Sheet is stocked at 1,220 x 2,440 mm (4 x 8 ft) and 1,525 x 3,050 mm (5 x 10 ft), and lasers and brakes are sized to match, with 3-4 m (10-12 ft) brake beds common. Thickness 0.5-6 mm (0.020-0.250") is sheet metal; 6-25 mm (0.25-1") is plate work on heavier brakes with plasma or waterjet cutting. The tightest practical limit is usually a deep box or a narrow channel the brake tooling cannot reach into. |
| Surface finish | Mill finish as received: cold-rolled steel about 1-2 µm Ra (40-80 µin), stainless 2B or #4 brushed, aluminum mill finish. Laser-cut edges 3-6 µm Ra (125-250 µin) with slight dross on thick stock; punched edges carry a burr on the exit side. Deburring and grain sanding are standard; powder coat, zinc plating, chem film and anodize are the usual finishes. |
| Lead time | Prototypes in 5-10 business days; production runs in 2-4 weeks. Add 1-2 weeks when powder coating or plating goes to an outside finisher. |
Typical of U.S. job shops; confirm with the shop for your part.
Materials
Cold-rolled steel (ASTM A1008, called 1008/1010 or simply CRS), hot-rolled pickled and oiled for heavier gauges, galvanized and galvanneal, and A36 or A572 plate above 5 mm (3/16"). 5052-H32 is the aluminum sheet-metal alloy: it bends at a 1t radius and welds well. 6061-T6 cracks on tight bends and is used when the part needs machined features or T6 strength; 5083 for marine and cryogenic work. Stainless 304 and 316 (2B or #4 finish) bend and weld well but need about 50% more brake tonnage. Copper, brass and Grade 2 titanium are fabricated the same way for electrical, decorative and aerospace parts. Tool steels, 7075 and cast alloys are not sheet materials.
What drives the cost
- Number of bends: each is a press-brake hit and a setup
- Hardware count: every PEM nut, stud or rivet is a press operation
- Welding, grinding and cosmetic blending
- Finish: powder coat, plating, anodize, silk screening
- Material grade and thickness: stainless and thick plate cost more to cut and bend
- Quantity: nesting yield and setup are amortized across the run
- Tolerances tighter than ±0.25 mm (±0.010") on bent features
When to use it
- Enclosures, chassis, brackets, panels, guards and frames with a constant wall
- One piece to a few thousand: there is no hard tooling to pay for
- Fast turns: laser plus brake makes a new part in days
- Parts that would turn most of a machined blank into chips
- Assemblies that combine cut-and-bent parts with PEM hardware and welded details
When not to
- Sections that vary in thickness, or features that must be cut into a solid: machine or cast instead
- Tight bores and hole patterns across bends, unless the part is machined after welding
- Tens of thousands a year of a small part: a stamping die pays for itself
- Long constant profiles: roll forming or extrusion is cheaper per foot
- Compound curved surfaces: deep drawing, casting or molding
Design tips
- Keep the inside bend radius equal to the material thickness (1t) and use the same radius on every bend; a shop bends with the tooling it has.
- Make flanges at least four times the thickness long, and keep holes at least 2t plus the bend radius away from a bend line so they do not distort.
- Add bend reliefs where a bend ends inside the part, and keep tabs and slots at least one material thickness wide.
- Tolerance across as few bends as possible; dimension from a datum on the flat and accept ±0.25 mm (±0.010") per bend.
- Design for one thickness; if a boss or thick pad is needed, weld or press-fit a machined detail.
- Send a STEP model with the bends in it and a drawing with material, thickness, finish, hardware part numbers and the cosmetic surfaces.
- Call out PEM hardware by part number and installation side, and note where grain direction or weld spatter matters.
- Specify welds with AWS symbols and say which are structural, which are seal welds and which must be ground flush.
Frequently asked questions
- What is the minimum bend radius for sheet metal?
- For mild steel, 5052-H32 aluminum, copper and annealed stainless, one material thickness (1t) is a safe minimum with standard brake tooling. 6061-T6 needs 1.5-2.5t and still shows orange peel on the outside of the bend; 7075-T6 should not be bent cold. Thicker plate needs larger radii, and bending across the rolling direction helps at tight radii.
- What thickness counts as sheet metal?
- In U.S. shops, sheet metal runs from about 0.5 mm (0.020", 24 gauge) to 6 mm (0.250", 3 gauge); above that it is plate, cut by plasma or waterjet and formed on heavy brakes. Most enclosure and bracket work is 1.0-3.0 mm (0.040-0.125") steel or aluminum.
- How much does sheet metal fabrication cost?
- A simple laser-cut and bent steel bracket is $20-60 in singles and a few dollars at hundreds; an enclosure with hardware, welds and powder coat is $100-400 each in tens. Bends, hardware and finish drive the price more than the material does. The Noramark cost estimator gives a ballpark from flat size, bend count and quantity.
- What file format do sheet metal shops need?
- A STEP or native CAD model with the bends in it (the shop unfolds it with its own K-factors), plus a PDF drawing for material, thickness, finish, hardware and tolerances. A DXF of the flat pattern is only useful when you are sure of the bend allowances.
