Guide
Bend radius, K-factor and the flat pattern: what the sheet metal shop needs from your drawing
Most sheet metal questions a shop sends back before quoting are about bends: the inside radius is drawn sharper than the tooling makes, a hole sits inside the bend zone, or a flange is too short to hold on the press brake. All three are design choices, and all three are cheap to fix on the drawing and expensive to fix with a reject. This page is the short version of what the brake can and cannot do.
Send a drawingUpdated October 8, 2026
Inside bend radius
A press brake forms sheet by pushing a punch into a V die; the inside radius of the bend comes from the punch tip and the die opening, not from the CAD model. In air bending, the common method, the inside radius lands close to the material thickness for mild steel, stainless and 5052 aluminum. A drawing that calls out a radius smaller than the thickness gets a question, because the shop cannot make it without coining or a special punch.
The working default is inside radius equal to material thickness. If your model uses that, the shop's flat pattern will match your part. If a feature needs a larger radius, say so on that bend; if the whole part is at a larger radius, a general note covers it.
K-factor and bend allowance
When sheet bends, the inside compresses and the outside stretches; somewhere between them is a neutral axis whose length does not change. The K-factor is the position of that neutral axis as a fraction of the thickness, from the inside surface. It is what CAD uses to unfold a bent part into a flat pattern: the bend allowance, the length of material in the bend, is computed from the radius, the angle, the thickness and the K-factor.
A K-factor near 0.33 is typical for a tight air bend in mild steel, and values from about 0.3 to 0.5 cover most materials and radii. The exact number depends on the shop's tooling and the material lot, which is why the flat pattern is the shop's responsibility, not the designer's. Send the formed part as a STEP or the drawing with bent dimensions; let the shop unfold it with its own K-factor. A flat DXF you unfolded with a guessed K-factor will come back a few thousandths long or short on every flange.
Rules that keep the part makeable
These are the numbers shops design around; a given shop may hold tighter with its tooling, and the quote for your part is what counts. When a design needs to break one of them, say so on the drawing and expect a question or a tooling charge rather than a silent change.
| Feature | Common minimum | Why |
|---|---|---|
| Inside bend radius | 1 x thickness | The punch and die, and cracking on the outside of the bend |
| Flange length | About 4 x thickness plus the radius | Shorter flanges fall into the V die instead of forming |
| Hole or slot to bend | About 2.5 x thickness plus the radius, from the bend line | Holes in the bend zone stretch into ovals |
| Hole to edge | About 2 x thickness | The edge bulges or tears on punching |
| Bend relief | Width about thickness, depth to the bend | Stops tearing where a flange meets an unbent edge |
| Slot width for a tab | Thickness plus a clearance | Tabs are sized to the sheet they pass through |
Bend direction and grain
Rolled sheet has a grain. Bending parallel to the grain is more likely to crack on aluminum and on thicker steel; bending across it is safer. A shop nests parts on the sheet with that in mind, so a part with bends in both directions on a cosmetic face should say which face is the show face, and whether the grain direction matters for a brushed stainless panel.
What to put on the drawing
- Material and thickness, with the inside bend radius as a general note or per bend.
- Bent dimensions to the outside or inside of the flange, consistently, with the angle.
- A STEP of the formed part. The shop unfolds it; you do not need to send a flat pattern.
- Which face is cosmetic, and whether grain direction matters.
- Hardware (PEM nuts and studs) with the manufacturer's part number and the side it is installed from.
Questions buyers ask
- Should I send a flat pattern DXF?
- Send the formed part. A flat DXF is useful only if the shop confirms your K-factor and tooling match theirs; most shops prefer to unfold it themselves from the STEP or the bent drawing.
- What bend angle tolerance is normal?
- Air bending holds angles to about plus or minus one degree as a matter of course; tighter calls for a different method and a note on the drawing. The quote you receive states what the shop holds on your part.
- Can a shop bend a hole that is close to the bend line?
- It can, but the hole distorts. If the hole must stay round, move it, or draw it as a post-bend operation (drilled or punched after forming), which the shop prices accordingly.
About Amerigo. Amerigo is the sourcing network for American manufacturing. More about Amerigo