DFM for Sheet Metal

Bend radius rules.
Hole distance rules.
Flat blanks work.

Sheet metal fabrication has its own DFM rules — violate them and parts crack at bends, tear at hole edges, or won't form at all. This is the reference you want beside you when designing for press brake + laser.

Free DFM Review Sheet metal fabrication

01 · Bend radius

Never bend sharper than this.

The minimum bend radius depends on material and thickness. Bending tighter causes cracking on the outside of the bend — irreversible damage.

Material	Min bend radius	Recommended	Notes
Aluminum 5052-H32	1.0 × t	1.5 × t	Good formability, general workhorse
Aluminum 6061-T6	3.0 × t	4.0 × t	Age-hardened — cracks on tight bends
Mild steel (1018)	0.8 × t	1.0 × t	Most forgiving material
304 Stainless	1.0 × t	1.5 × t	Work hardens during bending
316 Stainless	1.0 × t	1.5 × t	Similar to 304 for bending
Copper C110	0.5 × t	1.0 × t	Very formable
Brass C260	1.0 × t	1.5 × t	Good general formability
Galvanized steel	1.5 × t	2.0 × t	Zinc coating flakes on tight bends

02 · Hole to edge

Feature to edge distances.

Too close to an edge or bend, and features tear out or distort during forming. Critical dimensions vary by feature type.

2 × t

Hole to edge

Minimum distance from hole to part edge. Closer causes edge tear-out during punching or laser cutting.

2.5 × t

Hole to bend

Minimum distance from hole center to bend edge. Closer distorts hole during forming.

1.5 × t

Tab to edge

Tab width must exceed 1.5× material thickness for rigidity.

1 × t

Slot width

Minimum slot width equals material thickness for laser cutting.

4 × t

Slot length

Slot length for formed tab (with bend) should be at least 4× thickness.

2 × t

Notch width

For relief notches at internal bends — at least 2× thickness wide.

03 · K-factor

Flat pattern math.

K-factor defines where the neutral axis sits inside a bend. Affects the developed flat pattern length. Get K-factor wrong — parts are wrong length.

K-factor defined: During bending, material on the outside of the bend stretches, material on the inside compresses. Somewhere between these is the "neutral axis" — material that neither stretches nor compresses. K-factor is the ratio of the neutral axis location to the material thickness.

Typical values: K = 0.33 for soft materials (aluminum 5052, mild steel), K = 0.40 for standard steel bending, K = 0.44 for stiff materials (stainless). Material and tooling both affect actual K — we use customer-specified value if given, or our calibrated shop values for that material and thickness.

Bend deduction: Bend deduction = 2 × (inside radius + material thickness) - bend allowance. This is subtracted from the sum of the flange lengths to get the flat pattern length. For a box with 50mm flanges bent at 90°, with 1.5mm material and 3mm inside radius: bend deduction ≈ 2.8mm — so flat pattern is 50+50-2.8 = 97.2mm, not 100mm.

In practice: Modern CAD (Solidworks, Inventor, Fusion 360) handles K-factor calculations automatically if you specify material and bend parameters. Send us your 3D model — we'll generate flat pattern matching our tooling. For paper-drawing customers, we recalculate flat patterns based on shop-verified K-factors.

04 · Common mistakes

What we see go wrong.

Frequent DFM errors

• Holes too close to bend edges — distort during forming
• Sharp inside bend radii — cause cracking
• Long narrow tabs — flex and distort during forming
• Overlapping bend reliefs — weaken structure
• Dimensions specified before bending — forget to account for bend growth
• Required precision features on formed faces — forming tolerance limits
• Internal corners without relief cuts — distort into odd shapes
• Hardware (PEMs, threaded inserts) specified after bending — can't access

Good practice

• Include bend notes with radius specification
• Provide 3D model (flat pattern derivative automatic)
• Specify dimensions in finished state, not flat pattern
• Add relief cuts at internal corners
• Keep hardware installations planar — before or after bending
• Account for bend growth — overall dimensions plus/minus 0.1-0.2mm
• Consider forming sequence — may affect tool access
• Use formed edges for stiffness, not just aesthetic

FAQ

How exactly does bend radius cause cracking?

Outside of the bend stretches — material elongates. If the radius is too tight, the required elongation exceeds the material's ductility. Cracks start at the outer surface and propagate inward. The cracks are fatal — part cannot be repaired. Minimum bend radius is a function of material grade, temper, and thickness. Aluminum 6061-T6 (age hardened) has poor formability — needs 3× thickness minimum. Dead soft aluminum 1100 can bend to 0.5× thickness without cracking.

Laser cut vs water jet vs plasma?

Laser: fastest for thin sheet (under 6mm), best edge quality, limited to flat sheet. Water jet: any material, any thickness, slow, rough edge. Plasma: fast for thick steel (6-25mm), rough edge, heat-affected zone. We primarily use laser for most sheet metal work (4kW fiber lasers handle up to 20mm mild steel, 12mm stainless). For thick or specialty materials, water jet or plasma routed through partners.

Can I specify a hem or flanged edge?

Yes — hemmed edges (folded back on themselves) add stiffness and eliminate sharp edges. Standard hem: 180° fold with inside touching back to panel. Open hem: 180° fold with gap (for stiffener). Teardrop hem: partial fold (more visible, rounded). All add manufacturing cost vs simple edge but provide functional and cosmetic benefits. Specify explicitly — not automatic.

What about welding?

Welding: joining sheet metal panels for larger assemblies. Options: spot welding (fast, small heat affected zone, limited strength), seam welding (continuous weld, leak-tight), TIG welding (precision, aerospace quality), MIG welding (fast for thicker material). Design implications: weld locations must be accessible to operator, weld joint types (butt, lap, corner) each have specific fit-up requirements, post-weld distortion is a concern for precision parts.

PEM nuts and hardware?

PEM self-clinching hardware (nuts, studs, standoffs) pressed into sheet metal for threaded features. Alternative to tapping or welding nuts. Requires: specific hole size per PEM part number, hole in sheet before forming (for accessibility), minimum edge distance per PEM spec. We install PEM hardware as standard capability. Specify by PEM part number for exact part.

Tolerance expectations for sheet metal?

Sheet metal tolerances are looser than CNC. Typical: ±0.2-0.5mm on cut features, ±0.5-1° on bend angles, ±1mm on overall formed dimensions. Tighter tolerance possible but expensive — requires precision tooling, controlled temperature, additional setup. Specify tolerances based on actual functional need. Over-specified sheet metal gets quoted at CNC prices.