DFM for Sheet Metal:
12 Design Rules
That Reduce Cost

Minimum Bend Radius

Design bends with an inside radius of at least 1× material thickness (1t) for SPCC, and 1.5t for SGCC. Going below this cracks the outer face of the bend and produces inconsistent angles. Sharp corners (0 radius) are achievable but reduce tooling life and require special setup — avoid unless structurally necessary.

Minimum Flange Length

The flange (the bent leg) must be long enough for the press brake tooling to grip and form correctly. Minimum flange length = 4× material thickness, with an absolute minimum of 3.0 mm. Short flanges cause the part to slip during bending, producing variable angles.

Consistent Bend Radii Across the Part

Use the same bend radius for all bends on a single part wherever possible. Each different radius requires a tooling change — which adds setup time and cost, especially in batch production. If your design has three different radii, rationalise to one or two.

Keep Bends Parallel or Perpendicular

Non-orthogonal bends (angled, non-90°) require special tooling setup and longer cycle times. Design bend lines to be parallel to each other and perpendicular to the primary axis of the blank. If an angled bend is needed, confirm with your fabricator before finalising.

Minimum Hole-to-Edge and Hole-to-Bend Distance

Holes placed too close to edges or bends distort during processing. Follow these minimum distances:

Holes closer than these limits will deform when the nearby edge is cut or when the bend is formed. This is especially critical for precision-located holes (mounting holes, connector cutouts).

Minimum Hole Diameter

Laser-cut holes with a diameter smaller than the material thickness produce poor edge quality and accumulate dross. For punching, the minimum is approximately 1× material thickness. As a general rule: minimum hole diameter = 1.2× material thickness.

Use Standard Hole Sizes for Hardware

Design holes for standard hardware sizes (M3, M4, M5, M6, M8 clearance holes; PEM insert dimensions). Non-standard hole sizes require custom tooling or slower laser cutting — both increase cost. Reference ISO 273 for metric clearance hole tables.

Place PEM Inserts Away from Bends

PEM self-clinching nuts, studs, and standoffs are pressed in after forming. The insert needs a flat bearing surface and access for the press tool. Minimum distance from insert centre to any bend line: 3× insert diameter, plus at least 5 mm clearance. Inserts placed in flanges shorter than this cannot be installed correctly.

Consolidate Hardware to One Side

PEM inserts installed on multiple faces of an enclosure require repositioning the part in the press multiple times. Consolidating hardware to one or two faces reduces setup time linearly. Where inserts on multiple faces are required, note it clearly on the drawing so it is accounted for in quoting.

Add Relief Cuts at Intersecting Bends

Where two bend lines meet at a corner (e.g. a box corner), material bunching causes distortion and cracking without a relief cut. Add a circular or square notch at the intersection — typically 1.5–2× material thickness wide. This is mandatory for box-form parts; without it, corners will never close cleanly.

Minimise Tight Inside Corners on Cutouts

Laser cutting produces sharp inside corners well, but if the corner is in a location that sees stress, cracking initiates there. For structural cutouts, add a minimum radius of 0.5 mm at inside corners. For non-structural cutouts (ventilation, access holes), sharp corners are fine.

Uniform Material Thickness Throughout

Parts that require two different material thicknesses (e.g. a thick base plate welded to a thin enclosure body) must be manufactured as separate components and joined. Designing a single-thickness part that is then locally reinforced by a welded plate is more production-friendly than specifying varying thickness — which is not achievable in sheet metal.