Bend radius and material thickness in sheet metal design
The bend radius is set by the material and the tooling, not by the designer. As a guide value, mild steel and stainless steel manage an inside bend radius roughly equal to the sheet thickness. Aluminium 5754 often needs 1–1.5 times the thickness, and hardened 6082-T6 considerably more, otherwise the outside of the bend cracks. Stainless steel also springs back more than ordinary steel, which the workshop compensates for by overbending.
In air bending on a press brake, the radius is in practice set by the die's V-opening, which is often 6–8 times the sheet thickness. The inside radius is then about 15 per cent of the V-opening. That is why we like to ask which sheet metal shop you plan to use and design to their tooling. The result is a part that is right without the workshop having to edit the file. Rolling direction matters too: bends across the rolling direction crack less, and for sensitive materials we state the direction on the drawing.
Flat pattern and K-factor
When sheet is bent, the outside stretches and the inside is compressed. The neutral line, which keeps its length, does not lie in the middle of the material but closer to the inside. The K-factor states where: 0.5 means in the middle, and in air bending the value is typically between 0.3 and 0.45 depending on material and radius.
The flat pattern is calculated with the K-factor, and a wrong value gives the wrong flange length on the finished part. We use the CAD software's sheet metal tools, so the flat pattern updates when a flange changes. If the workshop has its own bend allowance tables, we use them. You receive a DXF at 1:1 scale with outlines, holes and bend lines on separate layers. You can read which files workshops want in the guide file formats for CAD and manufacturing.
A flat pattern that is correct in CAD can still come out wrong if the workshop uses different tooling from the one we assumed. We therefore state on the drawing which radii and which K-factor the flat pattern is based on, so the workshop sees at once if anything needs adjusting.
Holes, flanges and reliefs
A hole too close to a bend gets pulled into an oval when the sheet is bent. The guide value is that the edge of the hole should be at least 2–2.5 times the sheet thickness plus the bend radius from the bend line. If the hole cannot be moved, it can be cut after bending or relieved with a slot.
The shortest flange is set by the die's V-opening, because the sheet must rest on both sides during bending. As a guide value, a flange needs to be at least 3–4 times the thickness. Where a bend ends at an edge, a bend relief is needed – a small notch at least as wide as the sheet thickness – which stops the material tearing. In corners where two bends meet, we add a corner relief so the sheet does not bulge.
Welded sheet metal assemblies need extra care. We design tabs and slots that lock the parts in the right position before welding, so no separate welding fixture is needed for simpler frames. That saves time in the workshop and gives better dimensional accuracy.
Photo etching for thin, detailed parts
Photo etching suits thin parts, typically 0.05–1 mm, with many small holes or fine outlines: meshes, sieves, shielding cans, spring contacts, nameplates and parts for model making. The metal is dissolved chemically from both sides through a mask, so the part is free of burrs and stresses. The cost is hardly affected by how many holes the part has, and even complicated outlines are quick to produce, because the mask is created directly from the drawing file.
Because etching also works sideways, there is a limit to how small the features can be. As a guide value, holes and slots should be at least as wide as the material thickness, often 1–1.2 times, and bridges between holes at least as wide as the thickness. The mask is compensated with an etch allowance specified by the etching supplier. Bend lines can be half-etched to about half the thickness, so the part can be bent by hand. Tolerance is typically around ±10–15 per cent of the thickness.
Common photo etching materials are stainless steel, brass, nickel silver, copper and spring steel. The choice is driven by function: spring contacts need spring-tempered material, shielding cans good conductivity and nameplates a material that withstands weather and cleaning.
Sheet metal or another manufacturing method?
A bent sheet metal part is often cheaper than a machined one, because laser cutting and bending are fast and the material is used efficiently. Electronics covers, brackets, angle brackets and front panels are typical examples. If you have a machined part that has become expensive, we can check whether it can be redesigned in sheet metal. Conversely, a small run of sheet metal covers can sometimes be replaced with 3D-printed covers, which we make ourselves. That is a good way to test shape and assembly before ordering the sheet metal part.
We do not make sheet metal parts ourselves, but we design for the workshop you choose and help you find one if needed. The drawing states general tolerances to ISO 2768-1, bend angles, bend direction and material designation, for example EN 1.4301 for stainless steel. Read more under technical drawings. Sheet metal housings for electronics are designed together with the circuit board, as described under electronics enclosures.
Guide values for sheet metal and photo etching
| Parameter | Guide value (t = sheet thickness) |
|---|---|
| Inside bend radius, steel and stainless | approx. 1 × t |
| Inside bend radius, aluminium 5754 | approx. 1–1.5 × t (6082-T6: considerably larger) |
| V-opening in air bending | approx. 6–8 × t; inside radius ≈ 15 % of V-opening |
| K-factor in air bending | typically 0.3–0.45 |
| Hole edge to bend line | at least 2–2.5 × t + bend radius |
| Minimum flange length | approx. 3–4 × t |
| Bend relief | width ≥ t, depth ≥ t + bend radius |
| Photo etching: smallest hole and slot | approx. 1–1.2 × t |
| Photo etching: half-etched bend line | approx. 50 % of t |
| Photo etching: tolerance | typically ±10–15 % of t |
Guide values. The sheet metal shop's tooling and the etching supplier's rules always take precedence over the table.
What we need from you
- Sketch, CAD model or an existing sample of the part
- Material and thickness, for example S235, EN 1.4301 or 5754
- The workshop's bend radii, V-openings or bend allowance table, if available
- Surface treatment requirements: powder coating, galvanising or anodising
- Critical dimensions and hole patterns against other parts
- Number of parts per order and per year
- For photo etching: material, thickness and whether the part is to be bent
Typical projects
- Bracket and angle bracket with hole pattern
- Cover and housing for electronics
- Front panel with cut-outs for display and connectors
- Guard plate over moving parts
- Welded frame of bent parts
- Photo-etched nameplate
- Photo-etched shielding can for a circuit board
- Photo-etched mesh or sieve
- Spring contacts and thin contact strips
- Etched parts for model making
What affects price and lead time
- Number of bends and how they affect each other
- Tolerance requirements and critical hole patterns
- Whether the part is to be matched to a particular workshop's tooling
- Welded assemblies of several sheet metal parts
- Redesign from a machined or cast part
- For photo etching: number of variants and half-etched areas
What you get
- DXF at 1:1 scale with flat pattern and bend lines on their own layer
- STEP of the finished bent part
- Drawing with bend angles, bend direction and tolerances
- Recommendation for material, thickness and surface treatment
- Photo etching artwork with half-etched areas
- 3D-printed test part for fit (optional)
Frequently asked questions
Which bend radius should I design with?
As a guide value, an inside radius equal to the sheet thickness for steel and stainless steel. It is best to use the workshop's own radii, because they depend on the press brake tooling.
What is the K-factor?
The K-factor states where the neutral line lies in the sheet during bending, as a proportion of the thickness. It is used to calculate the flat pattern. In air bending it is typically between 0.3 and 0.45.
Which file format does the sheet metal shop want?
Usually a DXF at 1:1 scale with the flat pattern and a STEP file of the finished part. A PDF drawing with bend angles and tolerances makes checking and quoting easier.
When is photo etching worth it?
When the part is thin and has many small holes or fine outlines. The cost is hardly affected by the number of holes, and the tooling is a simple photo mask instead of an expensive press tool.
How small can photo-etched holes be?
As a guide value, roughly as large as the material thickness, or slightly larger. In 0.2 mm sheet that means holes down to about 0.2–0.25 mm.
Do you make sheet metal parts yourselves?
No. We design and draw for laser cutting, bending and photo etching and help you find a workshop. We can print test parts for fit.