A sheet metal bracket can look perfect in CAD and still crack at the bend, pull a hole out of round, or refuse to fit the press brake tooling. Most of these problems are decided on the drawing, long before the blank is cut. If you quote or make sheet metal parts, a five-minute DFM check of a few dimensions saves rework, scrap and awkward calls with the customer.

The rules below are rules of thumb expressed as multiples of the material thickness, written t. They come from published shop guidance, not from any one standard, so always confirm them against your own tooling, material and the customer's requirements.

Minimum inside bend radius

The first number to check is the inside bend radius. A common rule is that the inside radius should be at least equal to the material thickness (1t). The Fabricator notes that air bending normally gives a radius of one to two times thickness for mild steel, and that coining can take mild steel close to zero radius.

Material changes the picture:

  • Mild steel and softer aluminium (such as 3003 and 5052) bend at roughly 1t.
  • Stiffer aluminium alloys such as 6061 and 2024 may need four to eight times thickness as the minimum inside radius, per the same source.
  • Keep radii consistent across the part, so the operator does not change tools for every bend.

A drawing that shows a sharp inside corner on a 3 mm 6061 bracket is a spec gap. Ask the customer whether the radius matters to function. If it does not, the article advises leaving the radius undimensioned rather than putting a tight tolerance on it.

Holes, slots and edges near a bend

Holes placed too close to a bend line stretch into ovals when the flange is formed. Two published versions of the rule are worth knowing:

  • Keep hole edges at least 2t from the start of the bend radius (The Fabricator).
  • A more conservative version is 2.5t plus the bend radius for holes and 4t plus the bend radius for slots (New Equipment Digest).

The same New Equipment Digest guide gives these spacing rules for flat features:

  • Hole to edge: at least 2t, to avoid bulging.
  • Hole to hole: at least 6t apart.
  • Minimum hole diameter: at least equal to thickness; higher-strength material needs larger holes. Punching usually cannot go smaller than t, so smaller holes push you to laser cutting.

Illustrative example: on a 2 mm CRCA bracket with a 2 mm inside radius, the conservative hole-to-bend distance is 2.5 x 2 + 2 = 7 mm. If the drawing shows a 5 mm gap, either the hole moves, or you pierce after bending, which adds an operation that belongs in your quote.

Bend relief and flange width

Where a bend runs into an edge or a cut-out, the material needs room to move. The Fabricator gives a simple formula: minimum bend relief = material thickness + inside bend radius. Without relief, the corner tears or bulges, which may or may not be acceptable on a hidden part. That is a question for the customer, not a decision for the operator.

Short flanges are the other common trap. Keep the flange width at least 4t, because the sheet has to span the die opening to bend cleanly. A 6 mm flange on a 2 mm sheet looks fine in the model, but it may need special tooling or a different method.

Hems, countersinks and corners

Secondary features have their own limits. New Equipment Digest lists, among others:

  • Open hem: inside diameter at least 1t and return length at least 4t.
  • Countersink distance from a bend: at least 3t; from an edge, at least 4t.
  • Relief cut width: at least one thickness and longer than the bend radius.
Treat every distance under these multiples as a question to raise before quoting, not a problem to discover at the press brake.

A quick pre-quote checklist

Before you price a sheet metal RFQ, run through the drawing with these questions:

  • Is the material grade and thickness clear, and is the inside radius suitable for it?
  • Are holes and slots far enough from bends, edges and each other?
  • Does every bend that meets an edge have relief, or does the customer accept tearing?
  • Is every flange at least about 4t long?
  • Are tolerances on bent dimensions realistic for press brake work, or will they need fixtures and extra inspection?
  • Are finish notes (powder coating, plating, deburring) stated, and is masking needed near holes?

Each "no" is either a clarification for the customer or a cost line in your quote: an extra operation, special tooling, laser cutting instead of punching, or slower inspection. Writing these down at quote stage protects your margin and your delivery date.

How SpecReview helps

Upload the drawing PDF, the STEP model, or both, and SpecReview lists spec gaps and unclear notes to clarify before quoting, along with DFM and rejection risks and a short reason why each matters. Each finding is tagged as coming from the spec, the geometry or an assumption, so you know which points to confirm with the customer first.