Menu

Sheet Metal DFM

Sheet Metal DFM: The Enclosure That Bends Right the First Time

Notes · Mechanical designNovember 19, 202617 min readSenova Systems Research

Your enclosure came back 7 millimetres too wide, with a cracked bend and a hole stretched into a slot. Sheet metal is not machining, the flat pattern is the part, and the bend is where the size lives. Twelve rules, in the order you meet them on a model.

Example Labs is a made-up company we use for worked examples.

Picture the Example Labs field sensor hub on the bench. The board is built, the battery is in, the firmware boots. The sheet-metal tray that holds it all arrived from the fabricator this morning, and it does not fit.

The tray is 7 millimetres too wide for the opening it was drawn to fit. One bend has a crack running along the outside of the radius. And the mounting hole nearest the bend is no longer round, it stretched into a slot when the sheet wrapped around the punch, so the screw that was supposed to hold the board down has nothing to bite into.

Three defects, one cause: the part was designed as if sheet metal were machining. It is not. In machining, you cut away what you do not want and the size you draw is the size you get.

In sheet metal, you cut a flat pattern and then bend it, and the bend is where the size lives. The flat pattern is the part. Everything in this article is about getting the flat pattern right, twelve rules, in the order you meet them on a model, each one verified against a published design guide.

It builds on the pieces that came before it: the enclosure article, which set the size, the IP rating, and the heat path for the hub this tray holds; and the injection moulding article, which taught the same DFM discipline, design determines most of the cost and quality before production starts, applied to the process that bends instead of moulds.

Why sheet metal is not machining

A sheet-metal part starts as a flat sheet of uniform thickness. A laser or a punch cuts the flat pattern. A press brake bends it. That is the whole process, and it has three consequences that catch every engineer the first time.

First, the thickness is fixed. You do not choose a thickness per feature; you choose one gauge for the whole part, and every rule in this article is written as a multiple of that thickness. A part that needs a thick wall in one place and a thin wall in another is not a sheet-metal part.

Second, the bend consumes material. When a sheet bends, the outside of the bend stretches and the inside compresses, and the length of material the bend uses up, the bend allowance, has to be accounted for in the flat pattern, or the formed part comes out the wrong size. The naive flat pattern, the sum of the outside dimensions, is always too long. The demo below shows by how much: 7.2 millimetres on a part 180 millimetres across.

Third, the bend is the least accurate part of the process. Laser-cut features in the flat hold ±0.005 inches (±0.13 mm). Each bend adds about ±0.010–0.015 inches (±0.25–0.38 mm) of position error and ±1° of angle. A dimension that crosses two bends carries twice that error, plus the angle error at the end of a 40 mm flange, which is another 0.70 mm. Sheet metal is not machining, and asking for machining tolerances on formed features raises the price without improving anything.

The twelve rules, in the order you meet them on a model

The twelve rules below follow SSG Manufacturing's design guide DG-13, "Sheet Metal Design Guidelines", which lists the same twelve in the same order, with the K-factor and bend-allowance detail filled in from the Partwork, Sekkei-Tech, Sinbo, and Anebon guides. Every value is typical; the shop that quotes the part confirms its own limits.

Rule 1, Pick a standard gauge. Steel 0.036, 0.048, 0.060, 0.075, 0.105, 0.120 inches (20 to 11 gauge); aluminium 0.040, 0.063, 0.080, 0.090, 0.125 inches. A non-standard thickness is a special order: it costs more, it takes longer, and the shop may not have the tooling for it. The hub tray in the demo uses 0.080-inch aluminium, 2.0 mm, which is a standard gauge, and that is not a coincidence. Pick the gauge first, and every other rule follows from it.

Rule 2, Use a standard inside bend radius, about 1× material thickness. The minimum bend radius is the tightest inside radius a sheet takes without cracking on the outside of the bend. Bending stretches the outer surface in tension; below the material's minimum radius, that tension exceeds what the metal can take, and it cracks, first when the bend runs along the grain. The working rule is about 1× thickness for mild steel, stainless steel, and soft aluminium. For 6061-T6, the rule is 1.5–3× thickness, and some guides go further, 2–3×, 1.5–4×, and 3–6× for thicker gauges all appear in published guides, so treat 1.5–3× as the working rule and check the shop's chart for thick material. Bend across the grain for 6061-T6, never along it. The material table below gives the numbers per grade.

Rule 3, One radius per part. Use the same inside radius on every bend, so one tool makes every bend. A part with three different radii needs three tool changes, three setups, and three chances for the flat pattern to be wrong, and the press-brake operator will quietly standardise them anyway, which changes the flat pattern after the part is already cut. One radius is a discipline, not a limitation: pick the radius the largest bend needs, and use it everywhere.

Rule 4, The K-factor is not a material constant. When a sheet bends, the neutral axis, the layer inside the metal that neither stretches nor compresses, is the only layer that keeps its length, and the bend allowance is the arc length of that layer through the bend. The K-factor is where the neutral axis sits, as a fraction of the thickness measured from the inside face: K = δ / t, where δ is the distance from the inside face to the neutral axis and t is the thickness. For a perfectly elastic bend the neutral axis would sit at mid-thickness and K would be 0.5. In practice, plastic deformation pulls it toward the inside, so real values fall between about 0.3 and 0.5. It is not a property of the metal alone. It moves with the bend radius, the yield strength, the thickness, the angle, and the method, tighter radii and harder materials push it lower, looser radii and softer materials push it toward 0.5. A common starting table, from Partwork: for an inside radius up to 1× thickness, K is 0.33 for soft materials (aluminium, copper), 0.38 for medium (mild steel), 0.40 for hard (stainless); for 1–3× thickness, 0.40, 0.43, 0.45; above 3×, 0.50 for all three. Those are starting values, not a property of the material. The fabricator's value is the one that matters, because the fabricator's tooling and method set the neutral axis, and if your CAD model assumes K = 0.50 while the shop uses K = 0.40, the fabricated part will be dimensionally different from the model. The demo below prices that difference: 0.63 mm on a 173 mm flat pattern.

Rule 5, The bend allowance is the arc length of the neutral axis. The formula is BA = A × (R + K × T), with A the bend angle in radians, R the inside radius, K the K-factor, and T the thickness. Add one bend allowance per bend to the straight flanges, measured to where each bend starts, and you have the flat blank. There is a second formula that describes the same blank from the other side: the bend deduction, BD = 2 × OSSB − BA, where the outside setback OSSB = tan(A / 2) × (R + T). The deduction is what you subtract from the sum of the flange lengths measured to the outside mould line. Both formulas give the same flat pattern; use whichever matches how the drawing is dimensioned, and do not mix them. The demo uses both, and they agree.

Rule 6, Make flanges long enough for the V-die: at least 4× material thickness. A flange has to be long enough to sit on the shoulders of the press-brake V-die while the punch folds it. Too short, and the sheet slips into the die opening instead of folding cleanly, the bend comes out in the wrong place, or not at all. The SSG rule is at least 4× thickness. Several other guides write it as 4× thickness plus the bend radius, which for a 1× radius is 5× thickness, the safer number, and the one to use when the flange is short and the tolerance matters. The demo's 6 mm flange on 2 mm material is 2 mm short of the 4× rule and 4 mm short of the 4× + radius rule. It cannot be gripped, and the shop will either refuse it or form it badly.

Rule 7, Add bend relief at edges and corners. Where a bend terminates at the edge of a face, or where two bends meet at a corner, add a relief cut, a small notch that isolates the bend zone. Without it, the metal tears at the corner of the bend, because the material at the end of the bend has nowhere to go. The rule is: relief width at least 1× thickness, length at least the bend radius plus the thickness. On the hub tray, that is 2 mm wide and 4 mm long. A rectangular relief works on a laser or a turret punch; a circular or teardrop relief reduces stress further at the end of the cut.

Rule 8, Keep holes and slots away from bends: at least 2.5× thickness plus the inside bend radius from the bend line. Features inside the bend zone stretch as the sheet wraps the punch. A hole placed too close to a bend deforms into an oval, and a threaded hole distorts so the fastener will not start. The rule is measured from the edge of the feature to the bend line: 2.5× thickness plus the inside radius. On the hub tray, that is 7.0 mm. The mounting hole in the demo sits 3 mm from the bend line, 4 mm inside the limit, and it stretched into a slot. When space is tight, use an obround slot oriented along the bend, or add a relief cut along the bend line, but do not put a round hole in the stretch zone and hope.

Rule 9, Size holes at least material thickness, and keep them from the edge. Hole diameter at least 1× thickness, a smaller hole is hard to punch cleanly, and a laser will cut it but the slug may not fall out. Hole to edge at least 1× thickness, 1.5× preferred, closer than that and the edge bulges or tears when the hole is punched. On 2 mm material, that is a 2 mm minimum hole and 2 mm to the edge, 3 mm preferred. A hole that is also a fastener hole has a second constraint: the fastener maker's minimum distance to the edge and to the bend, and the sheet must be at least the hardware's minimum thickness. The fastener maker's chart wins over the general rule.

Rule 10, Pick the material for the bend, not for the brochure. Three grades cover nearly every enclosure, and they bend differently:

GradeMin. inside radiusWhat it means
Aluminium 5052-H321.0× thicknessExcellent formability; the industry standard for enclosures
Aluminium 6061-T61.5–3× thicknessProne to cracking if bent too tightly; bend across the grain; needs larger radii
Stainless steel 3041.0× thicknessHigh springback; work-hardens rapidly during forming

5052-H32 is the enclosure grade because it bends at 1× thickness without cracking, and its 12–18% elongation gives the bend room to stretch. 6061-T6 is stronger, 276 MPa yield against 5052's 193 MPa, but its 8–10% elongation is what cracks, and a 6061-T6 enclosure drawn with a 1× radius will come back with a crack along the outside of the bend. Stainless 304 has the best elongation of the three, 40–70%, but it springs back more than the others, so the brake has to over-bend it, and it work-hardens rapidly, each bend makes the next bend harder.

Pick 5052 unless the strength or the environment demands otherwise, and if the strength demands 6061-T6, pay for the larger radius.

Rule 11, Tolerances: the flat is precise, the bend is not. Laser-cut features in the flat typically hold ±0.005 inches (±0.13 mm). Each bend adds about ±0.010–0.015 inches (±0.25–0.38 mm) of position error and ±1° of angle. A dimension that crosses two bends carries the error of both, and the angle error at the end of a 40 mm flange is 0.70 mm at the tip. The consequence is a rule about where to put the tolerance: tolerance the flat pattern, not the folded envelope. Put the tight tolerance on the features cut in the flat, the hole positions, the slot widths, and leave the folded dimensions loose, because the folded dimensions are the sum of the bend errors and no amount of inspection will make them tighter.

Rule 12, Dimension from one datum per view, and do not stack tolerances across bends. A dimension chain that runs across three bends accumulates three bend errors, and the last feature in the chain is the one that does not fit. Dimension each feature from the same datum, one datum per view, so each feature carries one bend error, not three. And never dimension a feature across a bend from another feature across a bend. The flat pattern is where the accuracy lives; the folded part is where the errors add up.

Springback and grain: the two things the drawing cannot show

Two things about bending do not appear in the twelve rules, because they are properties of the process rather than the geometry, and both of them bite the first time.

Springback is the metal's elastic recovery after the punch lifts. The bend is formed past 90 degrees and springs back toward 90, and how far it springs back depends on the material, the radius, and the thickness. Stainless 304 springs back the most of the three enclosure grades. The brake operator compensates by over-bending, and the amount of over-bend is a shop setting, not a drawing dimension, which is another reason the folded angle carries a ±1° tolerance and not a tighter one. A part that needs an exact angle needs a secondary operation, not a tighter tolerance on the bend.

Grain direction is the direction the sheet was rolled, and it matters because the metal is weaker across the grain than along it. A bend that runs along the grain, the bend line parallel to the rolling direction, cracks first, and on 6061-T6 it cracks at radii that would be fine across the grain. The drawing should show the grain direction, and the flat pattern should be nested so the tightest bends run across it. A part with bends in two directions will always have one bend along the grain; that is the bend that gets the larger radius.

DEMO

The demo is the Example Labs field sensor hub tray: a U-channel in 5052-H32, 2.0 mm thick, with an outside base of 100 mm and two 40 mm flanges, 60 mm long, bent twice at 90 degrees. Inside radius 2.0 mm (1× thickness, per Rule 2). K-factor 0.40 (the Partwork starting value for soft aluminium at 1–3× radius). The arithmetic was run in Python before writing.

Step 1, the correct flat pattern. The bend allowance per bend is BA = A × (R + K × T) = 1.5708 × (2.0 + 0.40 × 2.0) = 4.398 mm. The bend deduction per bend is BD = 2 × OSSB − BA = 8.000 − 4.398 = 3.602 mm. The correct flat is the sum of the outside dimensions minus two bend deductions: 180 − 2 × 3.602 = 172.80 mm. Both formulas agree, the allowance and the deduction describe the same blank, and the flat pattern the shop should cut is 172.80 mm by 60 mm.

The outside setback is OSSB=tan(45°)×(R+T)=4.000 mm\text{The outside setback is OSSB} = \text{tan(45°)} \times \text{(R} + \text{T)} = \text{4.000 mm}

Step 2, the wrong flat pattern. The naive flat pattern is the sum of the outside dimensions: 100 + 40 + 40 = 180 mm. It is 7.20 mm too long, because it counts the material the bends consume twice, once in the base and once in each flange. The formed tray comes out 7.2 mm oversize, and the hub opening it was drawn to fit is 100 mm. The tray does not fit, and the error is not a tolerance. It is 19 times the per-bend tolerance of ±0.38 mm, and no amount of careful bending will fix a flat pattern that is 7.2 mm too long. The rework is a new blank, a new laser cut, and a new bend, and the wasted material is 432 square millimetres of 2 mm 5052 per part, before the labour.

Step 3, the K-factor error. If the CAD model assumes K = 0.50, the theoretical mid-thickness value, while the shop uses K = 0.40, the bend allowance becomes 4.712 mm per bend and the flat pattern 173.43 mm: 0.63 mm too long. If the CAD model assumes K = 0.33, the tight-radius value, the flat pattern is 172.36 mm: 0.44 mm too short. Both errors are larger than the per-bend tolerance of ±0.25–0.38 mm, so either one eats the whole tolerance budget before the first bend is made. The K-factor is the one number in the formula you cannot read off the drawing, and it is the number that decides whether the part fits. State it on the drawing, and use the fabricator's value.

Step 4, the hole and the flange. The mounting hole in the demo sits 3 mm from the bend line. The rule is 2.5× thickness plus the inside radius: 2.5 × 2.0 + 2.0 = 7.0 mm. The hole is 4 mm inside the limit, and it stretched into a slot when the sheet wrapped the punch. Move it to 7 mm and it stays round. The short flange in the demo is 6 mm long on 2 mm material. The rule is at least 4× thickness, 8 mm, and the stricter form, 4× thickness plus the radius, is 10 mm. The flange is 2 mm short of the first and 4 mm short of the second, and the brake cannot grip it. Lengthen it to 10 mm and the bend forms cleanly. The relief at the corner is 2 mm wide and 4 mm long, 1× thickness by radius plus thickness, and without it the corner tears.

Step 5, the tolerance stack. Two bends at ±0.25–0.38 mm each give ±0.50–0.76 mm across the part, and the ±1° angle error on a 40 mm flange is 0.70 mm at the tip. A dimension that runs across both bends and out to the flange tip carries more than a millimetre of possible error, on a part whose flat pattern is held to ±0.13 mm. That is why the drawing dimensions from one datum per view, and why the tight tolerance goes on the flat, not on the folded envelope.

The decision test: five questions

A team that is wondering whether its enclosure has a sheet-metal problem can answer five questions in an afternoon. If it cannot answer three of them, it has one.

  1. What is the flat pattern length, and what K-factor was it calculated with? If nobody can produce the number, or if the CAD model and the shop are using different K-factors, the part's size is an accident.
  2. Is every inside radius the same, and is it at least 1× thickness, 1.5–3× for 6061-T6? If the radii differ, the part needs multiple setups; if any radius is below the minimum, it will crack.
  3. Is every flange at least 4× thickness long, and does every hole sit at least 2.5× thickness plus the radius from a bend? If not, the brake cannot grip the flange and the hole will stretch into a slot.
  4. Is there a relief cut wherever a bend ends at an edge or meets another bend? If not, the corner will tear, and the tear will be found at assembly, not at the brake.
  5. Are the tight tolerances on the flat pattern, dimensioned from one datum, with the folded dimensions left loose? If the drawing carries ±0.1 mm across three bends, the shop will either charge for fixtures and inspection or quietly ignore the tolerance, and either way the part will not fit.

Objections

"Our CAD software calculates the flat pattern." It does, with the K-factor you gave it. If you gave it 0.50 and the shop uses 0.40, the software will calculate the wrong flat pattern with complete confidence. The software is not the authority. The fabricator's K-factor is, and it belongs on the drawing.

"We can just bend it and check." You can, once, on the first article. Then the shop bends fifty, and the first article's correction does not transfer, because the correction was a guess about the K-factor rather than a measurement of it. The flat pattern is calculated, not iterated, and the iteration costs a blank, a laser cut, and a bend every time.

"6061-T6 is stronger, so we should use it." It is stronger, and it cracks. A 6061-T6 enclosure drawn with a 1× radius will come back with a crack along the outside of the bend, and the crack will be found at assembly or in the field, not at the brake. Use 5052-H32 for enclosures unless the strength or the environment demands otherwise, and if the strength demands 6061-T6, pay for the 1.5–3× radius and bend across the grain.

"Tight tolerances cost nothing, the laser is accurate." The laser is accurate, and the bend is not. A ±0.1 mm tolerance across three bends does not make the part more accurate; it makes the quote higher, because the shop has to fixture and inspect for a tolerance the process cannot hold. Tolerance the flat pattern, not the folded envelope, and the price comes down without the part getting worse.

"We don't need relief cuts, the corners look fine." The corners look fine in CAD, where the metal does not tear. On the brake, the material at the end of the bend has nowhere to go, and it tears. The relief cut is 2 mm wide and 4 mm long. The tear is a scrapped part.

Sources

  1. SSG Manufacturing, "Sheet Metal Design Guidelines"
    What we used

    Design guide DG-13, the twelve rules in the order you meet them on a model: standard gauges (steel 0.036–0.120 in, 20–11 ga; aluminium 0.040–0.125 in); inside bend radius about 1× thickness, 1.5–3× for 6061-T6; minimum flange 4× thickness; bend relief width at least 1× thickness, length at least bend radius plus thickness; holes at least 2.5× thickness plus the inside bend radius from a bend; hole diameter at least 1× thickness; hole to edge at least 1× thickness, 1.5× preferred; laser-cut features typically hold ±0.005 in (±0.13 mm); each bend adds about ±0.010–0.015 in (±0.25–0.38 mm) and ±1° of angle; dimension from one datum per view

  2. Partwork, "Bend Allowance & K-Factor Calculator for Sheet Metal"
    What we used

    BA = A × π/180 × (R + K × T); K-factor 0.33–0.50 by radius and material (soft 0.33/0.40/0.50, medium 0.38/0.43/0.50, hard 0.40/0.45/0.50); BD = 2 × OSSB − BA, OSSB = tan(A/2) × (R + T); minimum bend radius about 1× thickness for mild steel, stainless, and soft aluminium, 1.5–4× for hard aluminium such as 6061-T6; K-factor values are starting values, not a property of the material

  3. Sekkei-Tech, "Sheet Metal Design for Manufacturing: Bend Radius, K-Factor, and Flat Patterns"
    What we used

    Minimum radii by material (mild steel 0.5–1× thickness; 5052 aluminium 1×, 1.5–2× for thicker gauges; 6061-T6 3–6×; stainless 304 1×, 1.5–2× for heavier gauges); K-factor 0.30–0.50, 0.33–0.38 common; bend relief width at least the thickness, depth at least radius plus thickness; hole-to-bend distance 1.5× thickness plus radius (a looser form than the 2.5× rule, see Corrections)

  4. Anebon, "Bending of Metal: Engineering Guide & DFM Tips"
    What we used

    K = δ/t, range 0.33–0.50; material table: 5052-H32 1.0× thickness, "excellent formability; industry standard for enclosures"; 6061-T6 2.0–3.0× thickness, "prone to cracking if bent too tightly"; stainless 304 1.0× thickness, "high springback; work-hardens rapidly"; minimum flange 4× thickness plus radius; hole at least 2.5× thickness plus radius from the bend line; bend parallel to the grain cracks first

  5. Sinbo Machining, "Bend Radius and Bend Allowance"
    What we used

    BA = π × (R + K × T) × (A/180); flat length is the sum of flange lengths plus the bend allowances; K is not a property of the metal alone, it moves with radius and yield strength; K-factor table by material and radius; inside radius is not free, on standard air-bending tooling it is roughly one material thickness

  6. DeepLink Metal Fab, "Sheet Metal Fabrication Design Guide"
    What we used

    Minimum flange 4× thickness plus radius; hole-to-bend 2.5× thickness plus radius; relief width at least thickness, depth at least radius plus thickness plus 0.5 mm; laser-cut hole diameter at least 1.0× thickness

  7. Example Labs field sensor hub figures from the cluster: 100 × 60 × 40 mm, CR2032 230 mAh, STM32H7, 2 MB flash, 48 MHz clock, BLE radio (#28); the machined 6061-T6 hub lid from #27 is a different part
    What we used

    This article designs the sheet-metal tray that holds the same hub

More in design notes

The Clip That Doesn't BreakThe lid has to open for battery service and calibration, and every time it opens, the clip bends past its limit, because the clip is a spring, and the spring was sized by feel instead of by strain.21 minThe Screw That Doesn't StripThe housing has to open for battery service and calibration, and every time it opens, the joint gets weaker. A self-tapping screw holds 380 N on the first pass and is stripped by the eleventh; a brass insert still holds 1,056 N at pass 25. The strength does not come from the brass, it comes from plastic locked into the knurls.21 minThe Seal That Actually SealsYour enclosure passed IP65 on the bench and leaks in the field, because the gasket took a set after two years of temperature cycling and the joint designed at 30% compression is now working at 15%. The seal is a set of numbers, not a material.26 minTolerance Stack-UpEvery part is a little off, and the little offs add up. Ten parts at ±0.1 mm stack to ±1.00 mm worst case and ±0.32 mm statistically, and the difference between those two answers is the difference between a product that assembles and a product that doesn't. The fix is rarely a tighter tolerance. It is usually a shorter chain.14 minPower Design for Battery ProductsThe battery is a budget, not a box. A field sensor on a CR2032: the headline budget says 513 days, the measured budget says 44. The gap is sleep current, regulator losses, and a battery that is not a constant, and the fix is arithmetic, not a bigger cell. The power budget, the BMS, and the rules that make battery life honest.14 min