A bend looks like the cheapest feature on a sheet-metal drawing — just a line where the flat turns a corner. On the floor it is nothing of the kind. A press brake forces metal past its yield point over a die, and the material fights back: it stretches on the outside, compresses on the inside, springs back when the ram lifts, and cracks if you turn it tighter than it wants to go. Almost all of that is decided not at the brake but on the screen, weeks earlier, by a handful of design choices that are cheap to get right and expensive to get wrong.
This guide covers the ones that matter most — radius, relief, feature spacing, flange length, flat-pattern math, and tolerance — from the designer's seat. The numbers are general engineering guidelines, not guarantees; every one flexes with material, temper, and tooling. But designing with them in mind is the difference between a part that forms clean on the first hit and one that comes back cracked, short, or out of tolerance.
Start with the inside bend radius
The most useful default in bend design: make the inside radius at least equal to the material thickness. Roughly 1T is a forgiving starting point for common mild steels and is where much standard tooling lands. Go tighter and you stretch the outer surface harder — and stretched metal only tolerates so much before it fractures, showing up as cracking, orange-peel, or fine splits along the outside of the bend. The risk climbs with harder tempers and heavier gauge, and it is worse when the bend runs parallel to the grain rather than across it. Call out a radius rather than leave it blank; "sharp bend" forces the shop to guess. Our press-brake forming page covers tonnage and tooling; the design side starts with a radius the material can actually make.
Give inside corners a relief cut
Where two bends meet, or a flange stops partway along an edge, the metal at the inside junction has nowhere to go — without relief it tears, bunches, or leaves a ragged distorted corner. A bend relief is a small notch cut into the flat pattern before forming that gives the metal room to move so the flange forms cleanly to the corner. A common guideline is a relief at least as wide as the material thickness and slightly deeper than the inside radius, so it clears the bend zone. Because these are cut in the flat by the laser before anything is formed, they cost essentially nothing up front and are painful to retrofit later.
Keep holes and features away from the bend
A hole or slot too close to a bend gets dragged into the deformation zone and distorts — the round hole pulls oval, the slot skews, the edge bulges. The fix is distance. A widely used rule of thumb keeps the near edge of a hole at least about 2.5 times the material thickness plus the bend radius from the bend line. Stay outside it and the hole forms where you drew it. When a feature genuinely has to live near the bend, you can form first and machine the hole afterward, or add a relief to isolate it — deliberate choices with a cost. Decide them on purpose rather than finding the distortion at first-article inspection.
Respect the minimum flange length
A press brake needs enough material on both sides of the bend to sit on the die. A flange that is too short slips into the die opening, forms partially, or will not form at all. As a rough guide the minimum outside flange runs on the order of four times the material thickness plus the bend radius, though it depends heavily on die width — wider dies need longer flanges. A stubby flange looks reasonable in CAD and is physically un-formable at the brake. Very short legs can be formed long and trimmed, or made with special tooling, but that adds operations, so check flange length against die geometry before the quote.
Design to the flat pattern: bend allowance and K-factor
The fact that trips up more drawings than any other: the flat blank is not the sum of the finished outside dimensions. When metal bends, the outer surface stretches and the inner compresses, and between them sits a neutral axis that neither grows nor shrinks. The flat develops along that axis, so you cannot add up the finished leg lengths and expect the part to come out to size. The bend allowance is the material consumed in the bend; the K-factor — roughly 0.3 to 0.5 for most sheet metal — locates that neutral axis as a fraction of thickness. Modern sheet-metal CAD handles this automatically once the part is built as real sheet metal with the correct thickness and radius. The trap is a part modeled as generic solid geometry, or with a placeholder radius that does not match the tool — the flat comes out wrong and no one notices until the formed part measures off. Send the 3D model, not just a flat DXF, so the shop can verify the flat against the tooling it will actually run.
The principleDesign to the tool and the flat pattern, not just the finished shape.
Be realistic about tolerances
Forming is repeatable, but it is not precision machining, and asking a bend to hold a machined tolerance is where cost quietly explodes. Angular tolerances of about ±1° per bend are a reasonable general expectation; tighter is achievable but demands more setup, better tooling, and sometimes in-process gauging a routine part should not pay for. The bigger trap is stack-up: every bend carries its own tolerance, and on a multi-bend part those errors accumulate, amplified by the leg length reaching the last feature. A hole-to-hole dimension spanning four bends cannot hold the same tolerance as one spanning none. Dimension from a single datum where you can, avoid chaining critical dimensions across bends, and reserve tight tolerances for the few features that truly need them. Stamping ±0.005" on every dimension does not make the part more accurate — only more expensive.
| Design feature | General guideline | Why it matters |
|---|---|---|
| Inside bend radius | ≥ material thickness (~1T) as a default | Tighter radii overstretch the outer fiber and crack, especially across grain or in harder material |
| Corner / bend relief | Width ≥ 1T, depth just past the bend radius | Gives metal room to move so inside corners form clean instead of tearing or bunching |
| Hole / feature to bend | Near edge ≥ ~2.5T + bend radius from the bend line | Features inside the deformation zone distort — round holes pull oval, slots skew |
| Minimum flange length | ~4T + bend radius (varies with die width) | Too-short flanges cannot sit on the die and will not form fully |
| Bend-to-bend spacing | Keep bends far enough apart to clear tooling and prior flanges | Crowded bends collide with the tool or the formed leg and cannot be reached in sequence |
| Angular tolerance | ~±1° per bend as a routine expectation | Tighter angles and long tolerance chains across many bends drive cost and stack-up risk |
The values above are general engineering guidelines, not SPF-specific guarantees — every one shifts with material, temper, tooling, and geometry, so treat them as a starting point for a design review, not a spec.
Design for consistency and grain
The cheapest part to form is a consistent one. Using the same inside radius on every bend lets the shop form the part with one tool instead of swapping mid-run; keeping bends to a few common angles, orienting features so the operator is not flipping and re-registering between hits, and grouping bends into a sensible sequence all shave setup time. Grain direction belongs in the same conversation: bending across the grain resists cracking, while a tight bend parallel to it can split, so on high-strength or heavy-gauge parts it is worth noting orientation on the print — and leaving it open elsewhere so the shop can nest for yield. None of this shows on the finished part; all of it shows on the price and lead time. Our in-house design and engineering team reviews for exactly these frictions, and the broader sheet metal fabrication workflow is built around parts designed to form.
What we see on the floor
At Southern Perfection, complete fabrication has run under one roof in Byron, GA since 1982, and models come in every day for review before anything is cut. The un-manufacturable submissions rhyme. The most common is the missing or too-tight radius — crisp sharp corners the material will not make without cracking. Close behind are inside corners with no relief, holes sitting on top of a bend line, and flanges too short for the die to grip. Every one is cheap to fix on the screen and costly to discover after the laser has cut the blanks. Because our press brakes form to 230 tons and the same building holds the TRUMPF fiber laser, plasma, plate rolling, welding, and CMM inspection, a bend problem caught in model review is solved without bouncing the part between shops. Our engineers work in SolidWorks, so when a flat pattern looks off or a radius does not match a tool we run, we flag it and propose a fix against the actual tooling.
Send your 3D model early — our engineers will flag any bend issues before we cut a single part.
When tight tolerances are the right call
None of this means loosen everything and hope. Plenty of parts legitimately need a tight bend angle, a precise hole-to-edge dimension, or a secondary operation after forming — a mating flange that has to seal, a bracket that locates a bearing, a bend that feeds automated assembly. Those requirements are real and worth specifying. The point of DFM is not to strip tolerance out of a part; it is to spend it deliberately. Put the tight tolerance on the feature that earns it, hold the rest to what forming comfortably delivers, and call out any secondary machining as its own operation rather than burying an implicit machined tolerance in a formed dimension. A part designed that way is the kind a custom manufacturing shop can quote accurately and build repeatably. For the wider context, our custom metal fabrication guide covers the process end to end.
Frequently asked questions
What inside bend radius should I use?
A safe default is an inside radius at least equal to the material thickness, about 1T, which suits common mild steels and standard tooling. Design tighter and you risk cracking the outer surface of the bend, and the risk grows with harder tempers, thicker gauge, and bends parallel to the grain. When in doubt, specify a radius rather than leaving it blank so the shop is not forced to guess.
Why do inside corners need a relief cut?
When a flange ends or two bends meet, the metal at the inside corner has nowhere to go and will tear or bunch into a distorted corner. A relief is a small notch cut into the flat pattern before forming that gives the material room to move so the flange forms cleanly to the corner. A common guideline is a relief at least as wide as the material thickness and slightly deeper than the inside radius, and because it is cut in the flat it adds essentially no cost.
How far should a hole be from a bend?
A widely used rule of thumb keeps the near edge of a hole at least about 2.5 times the material thickness plus the bend radius from the bend line. Inside that distance the hole gets pulled into the deformation zone and distorts, so a round hole can form oval and a slot can skew. If a feature must sit closer, form the part first and machine the hole afterward, or add a relief to isolate it.
Do I need to set the K-factor in my CAD model?
Your model must account for it, but modern sheet-metal CAD handles the K-factor automatically as long as the part is built as real sheet metal with the correct thickness and inside radius. The K-factor locates the neutral axis and drives the flat-pattern length; if the model uses generic solid geometry or a placeholder radius, the flat pattern comes out wrong at every bend. Sending the 3D model lets the shop verify the flat against the tooling it will run.
What angular tolerance is realistic for a press-brake bend?
About plus or minus one degree per bend is a reasonable routine expectation for press-brake forming. Tighter angles are achievable but require more setup, better tooling, and sometimes in-process gauging, which adds cost. Watch tolerance stack-up too: on a multi-bend part the angular and dimensional errors accumulate, so dimension from a single datum and reserve tight tolerances for the features that genuinely need them.