Sheet Metal Fabrication
Sheet metal fabrication cuts, bends and joins flat stock into a finished assembly, typically laser cutting followed by press braking, hardware and welding.
- Part
- Forming
- Revised
- 2026-08-11
At a glance
- Family
- Metal
- Typical tolerances
- ±0.005 in (±0.13 mm) on laser-cut features; about ±0.010 in (±0.25 mm) per bend, accumulating across bends; welded assemblies are substantially looser unless fixtured or machined after welding
- Surface finish
- Inherits the incoming sheet finish; commonly grained, then powder coated, anodized, or plated
- Typical volumes
- 1–10,000 parts per year; above about 10,000 stamping or roll forming usually wins
- Lead time
- 3–10 business days typical, 1–3 days for quick-turn simple parts; no tooling lead time
- Materials
- Metal
What it is
Sheet metal fabrication is the job-shop workflow that turns flat stock into a finished assembly: cut the flat pattern, bend it, install hardware, weld what needs joining, and finish it. No part-specific tooling is involved at any step, so a design can go from a CAD model to parts in hand in days, and change again the following week.
It is the default for enclosures, chassis, brackets, panels, racks, and machine guarding, in 0.024–0.250 in (0.6–6 mm) cold-rolled steel, galvanized, 304 and 316 stainless, and 5052 and 6061 aluminum. Volumes run from one prototype to about 10,000 a year, above which stamping's hard tooling starts to win.
The cost structure is entirely setup and labor: cut time, bend count, weld inches, and hardware count. Every one of those is a design variable, which is why sheet metal parts respond so strongly to design-for-manufacture work.
How it works
- Flat pattern. The 3D model is unfolded into a flat blank. This is not just geometry — bend allowance depends on material, thickness, inside radius, and the shop's tooling, expressed as a K-factor or a bend deduction table. Send the 3D model, not someone else's flat pattern; the fabricator's numbers differ from yours.
- Cutting. Fiber laser cutting dominates for its speed and edge quality; CNC turret punching is competitive for parts with many repeated holes and can add forms such as louvers, extrusions, and countersinks in the same operation. Waterjet handles thick plate and heat-sensitive materials.
- Deburring. Sheared and punched edges carry a burr, laser edges carry dross. Deburring is a separate operation, whether by timesaver machine, tumbling, or hand.
- Forming. Press braking makes one bend per stroke against a CNC backgauge. Bend sequence matters: a part must never be trapped by its own geometry before the last bend is reached.
- Hardware. Self-clinching nuts, studs, and standoffs are pressed into the flat or partially formed part, cold-flowing the sheet into a groove on the fastener. Each type has a minimum sheet thickness and a minimum edge distance.
- Joining. MIG, TIG, and spot welding, plus riveting and adhesive bonding. Welding sheet metal distorts it — heat input has to be controlled and sequenced, and weld shrinkage moves the assembly out of tolerance if it is not planned for.
- Finishing. Grinding welds, graining, then powder coating, anodizing, plating, or passivation.
Tolerance stacks up along that chain. Cut features hold to about ±0.005 in, a single bend to roughly ±0.010 in, and a multi-bend welded assembly to something much looser — which is why critical dimensions belong on cut features rather than across welded joints wherever possible.
Design guidelines
One thickness, one bend radius
Design the whole assembly in one material and gauge, and use the same inside bend radius everywhere. Every change of thickness is a different setup and a different flat pattern rule; every different radius is another tool change on the brake. Pull working thicknesses from the sheet metal gauge chart.
Bend radius
Inside radius of at least 1× material thickness for mild steel and annealed aluminum; 6061-T6 typically needs 2–4×, and more when bending parallel to the grain. Flat pattern development from the bend radius and K-factor chart.
Hole size, spacing, and distance from bends
Punched holes should be at least 1× material thickness in diameter (1.5–2× in stainless), at least 2× thickness from an edge, and at least 2.5× thickness plus the bend radius from a bend line. Laser cutting relaxes the diameter rule but not the distortion rule near bends.
Minimum flange length
About 4× material thickness. Shorter flanges cannot sit on both shoulders of the V-die and need special tooling.
Bend relief and corner relief
Provide a relief notch at the end of any bend that terminates at an edge — at least one material thickness wide and deeper than the bend radius plus thickness. At the intersection of two bends, add a corner relief so the material does not pile up and tear.
Hardware
Self-clinching fasteners need a minimum sheet thickness (check the specific part number), a minimum distance to the nearest edge, and clearance on the back side for the installation anvil. Installing hardware after forming is often impossible because the press cannot reach — plan installation before the bends that would block it.
Weld design
Specify weld length, not continuous beads, wherever strength allows: stitch welds put in a fraction of the heat and cause a fraction of the distortion. Keep welds away from tightly toleranced features, and give the fabricator a datum scheme that does not run across a welded joint.
Tolerances
Do not stack tolerances across bends. Dimension from a single datum edge, and put the tight dimensions on laser-cut features in the flat.
| Feature | Recommended | Limit | Why |
|---|---|---|---|
| Inside bend radius | 1× thickness | 2–4× for 6061-T6 | Outer fiber cracks at tighter radii in hard tempers |
| Minimum flange | 4× thickness | Half the V-die opening plus thickness | Flange must span both die shoulders |
| Hole diameter | ≥ 1× thickness | 1.5–2× in stainless | Punch strength; relaxed for laser cutting |
| Hole to edge | ≥ 2× thickness | 1.5× thickness | Thin webs bulge and tear |
| Hole to bend line | ≥ 2.5× thickness + radius | — | Metal stretching around the bend ovals the hole |
| Bend relief | Width ≥ thickness, depth > radius + thickness | — | Prevents tearing at the end of the bend |
| Cut feature tolerance | ±0.005 in (±0.13 mm) | — | Laser and turret accuracy |
| Bend dimension tolerance | ±0.010 in (±0.25 mm) per bend | Accumulates across bends | Springback and gauging variation stack up |
Cost drivers
With no hard tooling, cost is machine time plus labor plus material. Cutting time scales with cut length, not part area, so a part covered in small holes costs more than a solid one of the same size. Bend count is the largest single driver on formed parts, because each bend is a separate handling cycle. Welding is more expensive still — weld inches, plus grinding, plus the distortion correction that follows. Hardware is priced per piece installed. Material utilization matters at volume: parts that nest tightly on a sheet cost meaningfully less per piece.
Volume breakpoints: 1–10 pieces is prototype territory where setup dominates completely and the per-part price barely falls with quantity. From 100 to 1,000 the setup amortizes and the price drops sharply. Above roughly 10,000 a year, stamping or roll forming begins to win on cycle time despite the tooling investment.
- Cut the bend count. Every bend removed is handling time on every part, forever.
- Replace welds with tabs and slots or hardware. Self-locating tabs also improve assembly accuracy by removing fixture dependence.
- Nest-friendly outlines. Rectangular-ish parts nest far better than parts with sprawling arms; nesting efficiency shows up directly in the material line.
- Standardize gauge and hardware across the assembly. One thickness and one fastener type across five parts collapses setups and purchasing.
- Tolerance realistically. ±0.005 in on cut features is free; ±0.005 in across a welded joint requires fixturing, straightening, or machining after welding.
Questions
6 questionsWhat tolerance can sheet metal fabrication hold?
About ±0.005 in (±0.13 mm) on laser-cut features and roughly ±0.010 in (±0.25 mm) per bend, with bend tolerances accumulating across a multi-bend part. Welded assemblies are looser still. Put critical dimensions on cut features in the flat rather than across bends or welds.
What is the minimum bend radius for sheet metal?
At least 1× material thickness for cold-rolled steel and annealed aluminum. 6061-T6 typically needs 2–4× thickness, and more when the bend runs parallel to the rolling direction. Using one radius throughout the assembly avoids tool changes on the press brake.
How close can a hole be to a bend?
At least 2.5× material thickness plus the inside bend radius, measured from the hole edge to the bend line. Closer holes distort into ovals as the metal stretches around the bend. If a hole must be closer, either machine it after forming or extend it into a slot that crosses the bend entirely.
Why do I need to send a 3D model instead of a flat pattern?
Bend allowance depends on the fabricator's specific tooling, material, and measured K-factor. A flat pattern developed with different assumptions will produce a part whose flange lengths are wrong by a few hundredths of an inch per bend, and the error accumulates.
When should I switch from fabrication to stamping?
Around 10,000 parts a year for a simple part, sooner if it has many bends or holes. Stamping trades a multi-month tooling investment for a cycle time measured in fractions of a second; fabrication trades zero tooling for minutes of labor per part.
How do I avoid distortion when welding sheet metal?
Use stitch welds instead of continuous beads wherever the strength allows, alternate weld locations to balance heat input, keep welds away from tightly toleranced features, and avoid running the datum scheme across a welded joint. Weld shrinkage is predictable in direction but hard to hold to tight numbers.