Sheet Metal Design Guidelines: Bend Radius, K-Factor, Holes and Reliefs

Design Guide3 October 2026·By The Sarjan Solution Team

Sheet metal looks simple on screen: draw a flat profile, add a few bends, export a DXF. On the shop floor, small design choices decide whether a part bends cleanly, cracks, distorts, or cannot be formed at all. The guidelines below are the ones we apply when designing and checking sheet metal parts for fabricators. They are rules of thumb. Your fabricator's machines, tooling and materials always have the final say, so confirm critical values with them.

In the rules below, t means material thickness.

1. Inside bend radius

• For mild steel and most stainless steels, an inside bend radius of about 1 × t is a safe default.
• Harder or less ductile materials need more. Tempered aluminium alloys such as 6061-T6, for example, often need several times the thickness to avoid cracking on the outside of the bend, while softer alloys such as 5052 bend much tighter.
• Use one radius throughout a part where you can. Every different radius can mean a tool change.
• Match the radius to the tooling your fabricator actually has. In air bending, the radius you get depends mostly on the V-die opening, not on the punch.

2. K-factor and bend allowance

When sheet bends, the inside compresses and the outside stretches. The neutral axis, the layer that keeps its length, moves towards the inside of the bend. The K-factor is the position of that axis as a fraction of the thickness. It is usually between about 0.3 and 0.5, and it decides how long the flat blank must be.

• CAD defaults (often 0.5 or similar) are a starting point, not a fact.
• The correct value depends on material, thickness, bend radius and tooling. Ask your fabricator for their K-factor or bend-deduction table and set it in your CAD template.
• A wrong K-factor makes every bent dimension slightly off. On parts with many bends the errors add up.

3. Minimum flange length

A flange has to be long enough to sit across the V-die while it is bent. A common rule of thumb is a minimum flange length of about 4 × t, but the real limit is set by the die opening your fabricator uses for that thickness. Shorter flanges need special tooling or a different process, so check before designing them in.

4. Holes and slots near bends

• Keep holes at least about 2.5 × t plus the bend radius away from a bend line. Closer holes stretch into ovals as the bend forms.
• If a hole must sit closer, cut a relief slot or move the hole to a secondary operation after bending.
• Keep holes at least about 2 × t from the edge of the part, and hole diameters at least equal to t where they will be punched.
• Slots that cross a bend line should run perpendicular to it, and extend clear of the bend zone.

5. Bend reliefs and corner reliefs

Where a bend ends at an edge, or two bends meet at a corner, the material has nowhere to go. It tears or bulges. A bend relief (a small notch at the end of the bend) avoids this. Typical relief width is at least t, and depth extends just past the bend radius. Most CAD sheet metal tools add reliefs automatically. Check that the size suits the material instead of accepting the default.

6. Hems, joggles and countersinks

• Hems: an open or teardrop hem is kinder to the material than a fully closed one, especially on thicker or harder sheet.
• Joggles: keep the offset height and length in proportion to thickness. Ask what your fabricator's joggle tooling can do.
• Countersinks: on thin sheet, a deep countersink can go right through. Consider dimpling or a pan-head fastener instead.

7. Grain direction

Rolled sheet has a grain. Bends across the grain are less likely to crack than bends parallel to it. This matters most for tight radii and less ductile materials. Note the grain direction on the drawing when it matters, and remember that it affects how parts can be nested on the sheet.

8. Tolerances that fabricators can hold

• Features cut in the flat (laser, punch, waterjet) are accurate relative to each other, because they are made in one operation.
• Dimensions across bends collect error from every bend in between, so they cannot be held as tightly.
• Dimension critical features from the same face, or from a single datum, rather than in a chain across several bends.
• Apply tight tolerances only where the function needs them. Over-tolerancing bent parts makes them expensive to make and to inspect.

9. Drawings and flat patterns

• Include the flat pattern with overall flat size, bend lines, bend direction (up/down) and bend angle.
• State material, thickness, inside radius and the K-factor or bend table used.
• Supply a clean DXF of the flat pattern, with bend lines on a separate layer, for the cutting machine.
• Dimension the formed part as it will be inspected, not as it was modelled.

A quick pre-release checklist

1. One bend radius, matched to available tooling?
2. K-factor or bend table confirmed with the fabricator?
3. All flanges at least the minimum length for the die?
4. Holes clear of bends, or relieved?
5. Bend and corner reliefs sized for the material?
6. Critical dimensions taken from one face or datum?
7. Flat pattern, DXF and bend data on the drawing?

We design, detail and check sheet metal parts and enclosures, and prepare flat patterns and DXFs, for fabricators in the UK, USA, Netherlands, Belgium and worldwide. See our modelling and drafting service and our sheet metal fabrication project.

Frequently asked questions

What is a good default inside bend radius for sheet metal?

For mild steel and most stainless steels, about one times the material thickness is a safe default. Harder or less ductile materials, such as tempered aluminium alloys, need a larger radius. Always confirm with your fabricator’s tooling.

What K-factor should I use for sheet metal?

K-factor is usually between about 0.3 and 0.5, depending on material, thickness, bend radius and tooling. Use the value or bend table supplied by your fabricator rather than the CAD default.

How far should a hole be from a bend?

A common rule of thumb is at least 2.5 times the material thickness plus the bend radius. Closer holes tend to distort into ovals during bending.

What is the minimum flange length in sheet metal?

A common rule of thumb is about four times the material thickness, but the real minimum depends on the V-die opening used for that thickness.