Sheet Metal Fabrication Design Guide: 9 Rules That Cut Cost

Sheet metal parts are cheap to make and expensive to make badly. The difference is almost never the supplier's skill; it is whether the design respects how a flat blank becomes a folded part. A bracket with nine bends, a hole 1 mm from a bend line and a flange too short for the press brake will be quoted high, made slowly and inspected with difficulty, no matter who builds it.

This sheet metal fabrication design guide covers the nine rules that account for most of the cost gap between a well-designed fabricated part and a redesigned version of the same component. Each one is stated as a rule, followed by the reason and the practical limit.

Rule 1: Match the inside bend radius to the material thickness

The inside radius of a bend is not a free choice. Forming sheet over a sharp punch thins the outer surface and, in harder alloys, causes cracking along the bend line.

Aluminum 6061-T6 is the usual culprit. It is popular for machined parts and a poor choice for tight bends, because the temper that gives it strength also makes it crack. If the part is a bent 6061 bracket with a 1 mm inside radius on 2 mm sheet, expect either a cracked batch or a supplier who proposes 5052 instead.

Rule 2: Keep holes at least 2.5 × thickness plus the radius from a bend line

A hole placed close to a bend line distorts when the material is stretched. The practical minimum distance from the edge of the hole to the start of the bend is 2.5 × t + R. Anything closer will pull into an oval or tear.

When the design genuinely needs a feature near the bend, there are three options: move the hole to the other side of the bend and use a slot, punch the hole after bending (adds an operation), or add a relief cut that isolates the feature from the deformation zone.

Rule 3: Add bend relief wherever a flange ends inside the part

A flange that ends in the middle of a panel will tear at the corner unless material is removed. The relief is a small cut, typically as wide as the sheet thickness and as deep as the bend radius plus thickness, placed at each end of the bend line.

This is a two-minute change in CAD and a recurring defect if omitted. Lasers will cut whatever the flat pattern shows, including a crack initiation point.

Rule 4: Keep flange height at least 4 × thickness plus the radius

A press brake needs room for the punch and the die, and a very short flange cannot be formed because there is nothing for the tooling to bear against. As a working minimum, flange height should be at least 4 × t + R, and more for thick or high-strength material.

If a design needs a 3 mm flange on 2 mm steel, the realistic alternatives are a different process, a joggle, or accepting a secondary operation.

Rule 5: Keep hole diameter at or above sheet thickness

Laser cutting handles small holes better than punching, but a hole smaller than the sheet thickness is still slow and wears tooling. As a rule: hole diameter should be at least equal to thickness, and at least 1.5 × t for punched holes in production.

Slots are more forgiving than round holes in one dimension, but a slot narrower than the thickness will suffer the same problems.

Rule 6: Count the bends before you count the features

Bend count is the most reliable predictor of sheet metal cost. Each bend needs a press brake setup, a handling step and an inspection point, and a bend sequence that requires re-gripping the part adds labor without adding value.

Designs that fold a single blank into a complete enclosure usually beat designs that weld five flat panels, provided the bend sequence is possible. Two rules of thumb: fewer than six bends per part for economical small-batch work, and check whether any two bends conflict in direction and cannot both be formed in one setup.

Rule 7: Design weld joints for access and distortion

Welding is where fabricated parts lose tolerance. Two practical rules:

• Prefer lap and flanged joints to butt joints on thin sheet. They are more forgiving of fit-up error and easier to fixture.
• Keep welds away from machined or cosmetic faces, and specify the finish (grind flush, leave as-welded) explicitly. Undefined weld appearance is the most common reason a fabricated assembly is rejected on cosmetic grounds.

Where the drawing calls for flatness after welding, expect either stress relief, straightening, or machining of the critical face after fabrication.

Rule 8: Specify realistic tolerances

Fabricated parts accumulate tolerance through the process chain. A realistic drawing for a laser-cut and bent part states:

• Cut profile and hole positions: ±0.1 mm for laser cutting, ±0.2 mm for punching at larger sizes.
• Bend angle: ±0.5° to ±1° depending on part size and tooling.
• Overall dimensions across several bends: ±0.3 mm to ±0.5 mm, because each bend contributes angular error that projects over distance.
• Flatness after welding: specify the value and the measurement method, or accept that it will be negotiated at inspection.

Tightening a callout beyond these levels does not improve the part; it either raises the price to cover gauging and rework, or produces a supplier who accepts the drawing and then argues at delivery.

Rule 9: Plan the finish sequence, including threads and hardware

Finishing happens after fabrication, and it changes dimensions. Powder coating adds 60 to 100 µm per surface; anodizing adds roughly half the coating thickness per surface. A hole that must accept a pressed bearing cannot be finished inside it, so it needs masking, which is a manual operation and a cost line.

Decide in the design, not in the purchase order:

• Which faces are cosmetic, and therefore cannot carry weld marks, scratches or gate marks.
• Which holes and threads must be masked before coating.
• Whether threaded hardware is inserted before or after finishing (before is usually wrong, because paint bridges threads).
• Whether the part needs a note like "finish per drawing, do not coat bore Ø12 H7".

The K-factor question, briefly

Every flat pattern depends on the K-factor: the position of the neutral axis in the bend, expressed as a fraction of thickness. Bend allowance is calculated as:

BA = π × (R + K × t) × θ ÷ 180

where R is the inside radius, t is thickness and θ is the bend angle in degrees. A K-factor of 0.33 to 0.50 covers most air-bent parts, but the correct value depends on material, tooling and the bending method, and it is the supplier's tooling data that should drive the flat pattern, not a value copied from a textbook.

The design implication is simple: do not model the flat pattern yourself and send it as a manufacturing file. Send the folded 3D model with bend radii and let the fabricator generate the blank. Conflicting flat patterns are a reliable source of parts that are 1 mm out on the last flange.

Sheet metal fabrication pre-quote checklist

• Inside radii at or above the material minimum, especially on 6061-T6.
• Holes at least 2.5 × t + R from bend lines.
• Bend relief at every flange that ends inside the part.
• Flange heights at or above 4 × t + R.
• Hole diameters at or above sheet thickness.
• Bend count minimized and sequence feasible.
• Weld type and appearance specified.
• Tolerances within laser and press brake capability.
• Cosmetic faces, masking and hardware sequence defined.
• Material chosen from a stocked gauge and a bendable alloy.

Frequently asked questions

What is the minimum bend radius for 2 mm aluminum? For 5052, one times the thickness, so 2 mm inside radius. For 6061-T6, use 1.5 to 3 times the thickness, or anneal the material before bending, otherwise the bend line will crack. If a design needs a tight radius in 6061-T6, changing the alloy is usually cheaper than changing the process.

Do I need to supply a flat pattern with the 3D model? No, and it is usually better not to. The flat pattern depends on the fabricator's tooling, bend deduction and K-factor, so a pattern generated in your CAD system can disagree with theirs. Send the folded model with bend radii and let the shop generate the blank.

Can a welded sheet metal part still hold tolerance? Yes, if the critical features are machined after welding or if the tolerance is realistic for a welded assembly. Welding introduces distortion that no fixturing fully removes, so a design that needs ±0.05 mm across a welded joint should plan a post-weld machining operation.

Next step

If you have a fabricated part that keeps coming back expensive or slightly out of tolerance, send the 3D model and the drawing. We will return the flat pattern assumptions, the bend sequence and a note on which three features are driving the price, so the next revision can be cheaper without changing what the part does.