Key takeaways
- A hem is the cheapest stiffness and the cheapest safe edge you can buy — but only if the return length is at least four times the material thickness.
- Corner tearing is a relief problem, not a material problem. Width ≥ 1×t and depth ≥ R + t at every bend that ends on an edge.
- Closed hems trap pretreatment chemistry and water. Outdoors, specify a drain path or use a teardrop instead.
- Keep holes and slots out of the forming zone: 2.5×t + R for holes, 4×t + R for slots, measured to the tangent of the bend.
- A Z-bend needs at least 2.5×t of step height to clear the tooling; below that the part cannot be made on a press brake at all.
- Decide the corner joint before the flat pattern. Welded-and-dressed, folded interlock, riveted-and-sealed and corner-post are four different nests, not four finishes on the same part.
A food machinery customer lost 340 stainless doors to a single missing notch. The design was a 1.5 mm 304 lid with a 20 mm return on all four sides, laser cut and bent in one setup. On the first article, every corner split 3–5 mm down the bend line — not a crack you could see in the drawing, but a crack you could catch a fingernail on, and in a washdown plant that is a contamination trap and a rejected part. The fix took four minutes on the CAM station: a 1.5 × 3.0 mm relief notch at the end of each bend line. The rework cost was the 340 doors already cut.
Edge forms, reliefs and corner joints are the least glamorous decisions in an enclosure, and they generate a disproportionate share of scrap, rework and sharp-edge complaints. This guide covers the four edge forms and when each earns its money, the geometry rules for hems and curls, how to size bend and corner reliefs, the four ways to close a box corner, what joggles and Z-bends cost you in tooling, and the nine checks we run on every flat pattern before it goes to the laser. For the bend process itself — radii, springback, K-factor and tonnage — start with our sheet metal bending guide and the press brake calculator.
Four Edge Forms and When Each One Earns Its Money
An edge can be left raw, folded over, or rolled. The choice sets the stiffness, the safety of the handling, the corrosion behaviour and the price.
| Form | Geometry | What it buys | Watch out for |
|---|---|---|---|
| Open hem | Folded back with a gap; inside diameter ≥ 1×t | Safe edge, moderate stiffness, easy to form, tolerant of coating thickness | Leaves a visible slot; collects dust; not a sealing surface |
| Teardrop hem | Folded back with a rounded eye; inside diameter ≈ 1×t | Safe edge with no sharp slot; the best compromise for painted or coated sheet | Slightly taller than an open hem; needs the right punch nose |
| Closed (flat) hem | Folded flat against the panel; two-step forming | Maximum edge stiffness, doubles the local thickness — the standard move under an IK10 impact door edge or a latch strike | Traps pretreatment and water; highest tonnage; springback risk; can crack on high-strength or hard-temper alloys |
| Curl (rolled edge) | Rolled tube; outside radius ≥ 2×t, opening ≥ 1.5×t | Best hand-safe edge, high stiffness, no trap if left open | Needs 6×t + radius clearance from other bends; special tooling on thicker sheet |
Rule of thumb we quote with: leave the edge raw only where nothing touches it and it is inside the sealed volume. Every operator-accessible edge on a door, a lid or a removable panel gets at least an open hem or a teardrop.
Hem Geometry Rules
- Return length ≥ 4×t. Shorter than this and the punch slips off the flange instead of folding it. On bottom-bending tooling with a shallow die opening, allow 6×t.
- Inside diameter ≥ 1×t for open and teardrop hems. A zero-radius closed hem is a theoretical value, not a producible one.
- Keep holes, slots and extrusions out of the fold. Minimum edge-to-bend-tangent distance is 2.5×t + R for holes and 4×t + R for slots. Inside the fold, nothing is round afterwards.
- Allow for the coating. A 1.5 mm hem on pre-galvanised or pre-painted sheet closes on 1.5 mm plus two coats; specify the inside diameter from the coated thickness, not the base metal.
- Overbend for springback. Closed hems are formed past 180° and flattened; the sharper the geometry, the more the material wants to open again.
| Thickness t | Min return length (4×t) | Min inside dia (1×t) | Hole-to-bend (2.5×t + R, R = t) | Typical hem die |
|---|---|---|---|---|
| 0.8 mm | 3.2 mm → use 4 mm | 0.8 mm | 2.8 mm | Standard flattening die |
| 1.0 mm | 4.0 mm | 1.0 mm | 3.5 mm | Standard flattening die |
| 1.5 mm | 6.0 mm | 1.5 mm | 5.3 mm | Standard flattening die |
| 2.0 mm | 8.0 mm | 2.0 mm | 7.0 mm | Hemming die, two hits |
| 3.0 mm | 12.0 mm | 3.0 mm | 10.5 mm | Roller hemming or press |
Two traps specific to closed hems on outdoor enclosures. First, the fold is a capillary: pretreatment and rinse water wick in and bleed out for days, staining the paint and undercutting adhesion. Second, in freezing climates the trapped water freezes and opens the hem. Where a closed hem is needed for stiffness, add a drain notch at the low end, or use a teardrop and accept the small penalty in stiffness. This interacts directly with the moisture strategy in our condensation control guide.
Bend Reliefs: Where Tearing Starts
When a bend line ends on a free edge, the material at that corner has nowhere to flow. It tears. A relief notch removes the constraint. The sizing rules are simple and they work:
- Relief width ≥ 1×t (measured perpendicular to the bend line).
- Relief depth ≥ R + t — the cut must pass the full bend zone, not just reach it.
- Round the inner corners of the notch where possible; a sharp notch corner is the next crack starter.
- Alternative to a notch: offset the flange so the bend line does not meet the edge at all — a "step-back" flange costs a little material and removes the relief, the tear risk and the extra laser path.
| Thickness | Inside radius R | Relief width (min) | Relief depth (min) | Laser or punch? |
|---|---|---|---|---|
| 1.0 mm | 1.0 mm | 1.0 mm | 2.0 mm | Laser, no burr |
| 1.5 mm | 1.5 mm | 1.5 mm | 3.0 mm | Laser |
| 2.0 mm | 2.0 mm | 2.0 mm | 4.0 mm | Laser or punch |
| 3.0 mm | 3.0 mm | 3.0 mm | 6.0 mm | Laser; allow for kerf |
On the laser, remember that the kerf eats into the relief: a 0.2 mm kerf on a 1.0 mm slot is a 20% error, which is why we draw reliefs in the CAM station against the actual kerf compensation rather than trusting the model dimension. Burr direction matters too — it is one of the indications ISO 13715 supports, and how to write it is set out in our edge break and deburring guide. A burr on the outside of a bend is a crack starter and a cut finger.
Corner Joints: Four Ways to Close a Box
Once the flanges are up, something has to close the vertical corner. This decision belongs in the flat pattern, because each option needs a different notch, tab or gap.
| Joint | How it closes | Strength | Sealing | Cost | Best for |
|---|---|---|---|---|---|
| Welded and dressed | Flanges meet, corner welded, ground and blended | Highest | Continuous, IP-capable | Highest | Outdoor, food-grade, IK08+, hygiene-critical |
| Folded interlock | Tab from one flange folds over the other | Medium | Needs sealant | Low-medium | Indoor covers, guards, light-duty housings |
| Riveted + sealant / PEM | Overlap flange, fasteners plus a bead | Medium | Good if the bead is continuous | Medium | Serviceable panels, mixed-material boxes |
| Corner post extrusion | Panels captive in an aluminium post | High | Gasketed by design | High unit, low at volume | Modular cabinet families, kiosks |
For a welded corner, leave a small weld gap at the flat-pattern stage rather than butting the flanges hard: a consistent 0.5–1.0 mm gap gives the weld somewhere to sit and keeps the outside dimension honest. For a folded interlock, check that the tab does not land on a bend radius. And in every case, the corner is the first place the plating or coating fails — see the corrosion resistance coatings guide for the edge-coverage issue, and the galvanic corrosion guide if the box mixes metals.
Joggles and Z-Bends
A joggle (Z-bend, offset) steps one plane past another so that two panels can overlap flush. Two rules govern whether it can be made:
- Step height ≥ 2.5×t for the punch and die to clear. Below that, the tooling collides with the first bend.
- Flange after the second bend ≥ 1.5×t to stay supported.
- Avoid tight Z-bends in 316L stainless and 7075 aluminium — they crack at the tangent, and the fix is a larger radius or a welded-on shim, both of which cost more than designing the step correctly.
Where a joggle is used to hide a fastener head or to bring a door skin flush with a frame, check the tolerance stack: two bends each at ±1° plus a ±0.2 mm material variation will show as a visible lip on a 1 m door. Tolerances are set out in our sheet metal tolerance guide.
What It Does to the Flat Pattern
Every one of these features changes the developed length, and most of the surprises in first articles come from here:
- K-factor between 0.25 and 0.50 (about 0.42 for typical cold-rolled steel and aluminium with standard tooling). Bend allowance = (π/180) × angle × (R + K×t). Get it wrong and every flange moves.
- A hem adds material twice. The flat blank is longer by the return length plus two bend allowances, and the second bend is a 180° fold with its own allowance.
- Springback is compensated, not avoided — 5–10° on some alloys, handled by overbending, coining or in-process angle measurement.
- Reliefs reduce the nest yield marginally but reduce scrap a lot; the trade is almost always worth it.
Nine Checks Before the Flat Pattern Goes to the Laser
- Every bend that ends on an edge has a relief — width ≥ t, depth ≥ R + t.
- Hem returns ≥ 4×t, inside diameters ≥ 1×t, and coated sheet dimensioned from the coated thickness.
- Holes ≥ 2.5×t + R and slots ≥ 4×t + R from the bend tangent.
- Corner joint chosen, and the notch, tab or weld gap drawn accordingly.
- Z-bend steps ≥ 2.5×t with a flange ≥ 1.5×t after the second bend.
- Curl outside radius ≥ 2×t, opening ≥ 1.5×t, clearance ≥ 6×t + radius from other bends.
- Countersinks ≥ 3×t from bends, ≥ 4×t from edges, depth ≤ 0.6×t.
- Bend direction checked against material grain on 6061-T6, 7075 and hard-temper stainless.
- Deburr and edge-break requirements written on the drawing — a raw edge is a handling hazard under machinery safety rules, and a burr on an outdoor edge is a corrosion start.
What We Do With Your File
Send a step file or a PDF with a material callout and we will run the nine checks, return a marked-up flat pattern with the relief and hem corrections, and quote the parts — usually within 24 hours. Where a corner keeps cracking or a hem keeps opening, we will tell you which of the four joint or four edge forms to switch to and what it costs. Use the contact form or email gongtianbao@xhlmarketing.com. If you are earlier in the process, the sheet metal DFM guide sets the sequence, and the prototype-to-production guide shows how a first article turns into a repeatable run.
Two of the nine checks depend on information only the buyer has, so send it with the enquiry rather than waiting for a question. What to send with the enquiry so the flat pattern check starts on day one is a ten-item list that takes about thirty minutes to assemble.
Frequently Asked Questions
How long does a hem return need to be?
At least four times the material thickness, measured on the flat. A 1.5 mm panel needs a 6 mm return; a 2 mm panel needs 8 mm. With bottom-bending tooling and a shallow die opening, allow six times the thickness. Shorter than that and the punch slides off instead of folding the flange.
Why does my corner crack when I bend a box?
Because the bend line ends on a free edge and the material has nowhere to flow. Add a relief notch at least one material thickness wide and R + t deep, past the full bend zone. Round the inner corners of the notch, and check that the burr from cutting is not on the outside of the bend.
Open, teardrop or closed hem — which should I choose?
Open or teardrop for a safe edge on painted or coated sheet, and for anything outdoors, because they do not trap pretreatment chemistry or water. Closed hem where you need maximum edge stiffness or double thickness under a latch strike or an IK10 door edge — and then add a drain notch if the part lives outside.
Can I put a hole close to a hem or a bend?
Keep the hole edge at least 2.5×t + R from the bend tangent, and 4×t + R for slots. Closer than that and the hole will ovalise into a teardrop as the material flows through the bend, which shows up as an assembly mismatch rather than a visible defect.
What is the minimum step for a Z-bend?
About 2.5 times the material thickness, with a flange of at least 1.5×t after the second bend, so the tooling can clear the first bend. On 316L stainless and 7075 aluminium, increase both and use a generous radius — tight Z-bends crack at the tangent in those alloys.