Use one inside bend radius of about 1× material thickness on every bend, flanges at least 4× thickness long, holes at least 1× thickness in diameter, and holes at least 2.5× thickness plus the bend radius from a bend. Laser-cut features typically hold ±0.005 in (±0.13 mm), and each bend adds about ±0.010–0.015 in (±0.25–0.38 mm) and ±1° of angle.
SSG MFG · design guideDG-13 · 12 rules
12 rules, in the order you meet them on a model. Every value is typical; the principal quoting your part confirms its own limits.
| # | Rule | |
|---|---|---|
| 01 | Pick a standard gaugeSteel 0.036, 0.048, 0.060, 0.075, 0.105, 0.120 in (20–11 ga); aluminum 0.040, 0.063, 0.080, 0.090, 0.125 in | Steel 0.036, 0.048, 0.060, 0.075, 0.105, 0.120 in (20–11 ga); aluminum 0.040, 0.063, 0.080, 0.090, 0.125 in |
| 02 | Use a standard inside bend radiusAbout 1× thickness, or the shop's standard tooling radius; 1.5–3× for 6061-T6 | About 1× thickness, or the shop's standard tooling radius; 1.5–3× for 6061-T6 |
| 03 | Keep one radius per partSame inside radius on every bend in the part | Same inside radius on every bend in the part |
| 04 | Let the shop develop the flat patternSend the 3D model; K-factor is typically 0.3–0.5 and varies by shop, tooling and material | Send the 3D model; K-factor is typically 0.3–0.5 and varies by shop, tooling and material |
| 05 | Make flanges long enough for the V-dieAt least 4× material thickness | At least 4× material thickness |
| 06 | Add bend relief at edges and cornersRelief width at least 1× thickness; length at least bend radius plus thickness | Relief width at least 1× thickness; length at least bend radius plus thickness |
| 07 | Keep holes and slots away from bendsAt least 2.5× thickness plus the inside bend radius from the bend line | At least 2.5× thickness plus the inside bend radius from the bend line |
| 08 | Size holes at least material thicknessDiameter at least 1× thickness; hole to edge at least 1× thickness, 1.5× preferred | Diameter at least 1× thickness; hole to edge at least 1× thickness, 1.5× preferred |
| 09 | Respect hardware spacingFollow the fastener maker's minimum distance to edge and to bend; sheet at least the hardware's minimum thickness | Follow the fastener maker's minimum distance to edge and to bend; sheet at least the hardware's minimum thickness |
| 10 | Self-fixture welded assembliesTab-and-slot joints with slot clearance about 0.005–0.010 in (0.13–0.25 mm) over the tab | Tab-and-slot joints with slot clearance about 0.005–0.010 in (0.13–0.25 mm) over the tab |
| 11 | Control weld distortionStitch weld long seams on thin sheet, for example 1 in (25 mm) welds on 3–4 in (75–100 mm) centers | Stitch weld long seams on thin sheet, for example 1 in (25 mm) welds on 3–4 in (75–100 mm) centers |
| 12 | Dimension from one datum per viewTolerance across bends ±0.010–0.015 in (±0.25–0.38 mm) per bend; angles ±1° | Tolerance across bends ±0.010–0.015 in (±0.25–0.38 mm) per bend; angles ±1° |
These build on the short list on the sheet metal process page, with the failure each rule prevents and a drawing for each.
Move the inside bend radius against gauge and material to see where a press brake bend cracks, how much it springs back, how the flat pattern length changes, and how far a hole must sit from the bend to stay round.
6061-T6 · T 0.060 IN · R 0.120 IN (2T)
Works: forms clean
2T meets the typical 2T minimum for 6061-T6. Keep this one radius on every bend so one tool does the whole part.
Typical values for a 90° air bend. K-factor and minimum radius vary by shop, tooling, temper and grain direction; send the 3D model and the shop sets the flat pattern.
Each rule with its typical value, the reason behind it and what happens on the floor when it's ignored. Switch any drawing between Do and Avoid; point at a callout to pick it out.
Rule 01
Steel 0.036, 0.048, 0.060, 0.075, 0.105, 0.120 in (20–11 ga); aluminum 0.040, 0.063, 0.080, 0.090, 0.125 in
Rule 02
About 1× thickness, or the shop's standard tooling radius; 1.5–3× for 6061-T6
Fig. 1Bend radius
Do. Inside radius at or above the material's minimum, often 1× T for mild steel and 5052: the outside fibers stretch without tearing.
Avoid. Below the minimum radius the outside of the bend stretches past the material's elongation and cracks, worst across the grain.
Rule 03
Same inside radius on every bend in the part
Rule 04
Send the 3D model; K-factor is typically 0.3–0.5 and varies by shop, tooling and material
Rule 05
At least 4× material thickness
Fig. 2Minimum flange length
Do. The flange is long enough to rest on both die shoulders through the whole stroke, so the bend forms where it's drawn.
Avoid. A short flange slips into the V-opening mid-stroke: the bend walks, the angle is off and the part may kick.
Rule 06
Relief width at least 1× thickness; length at least bend radius plus thickness
Fig. 3Bend relief
Do. A relief notch at least T wide, running past the bend line by at least T plus the inside radius, lets the flange fold cleanly.
Avoid. Without relief the metal at the end of the bend has to tear or bulge; you get a ragged corner and a flange that won't sit square.
Rule 07
At least 2.5× thickness plus the inside bend radius from the bend line
Fig. 4Hole to bend distance
Do. Holes at least 2.5 T plus the bend radius from the bend stay round and on position.
Avoid. A hole inside the bend's deformation zone stretches into an oval and moves as the flange forms, or it has to be pierced after forming.
Rule 08
Diameter at least 1× thickness; hole to edge at least 1× thickness, 1.5× preferred
Fig. 5Hole size and spacing
Do. Holes at least T in diameter, at least 1.5 T from an edge and 2 T from each other: the punch shears clean and the web holds.
Avoid. Too close to an edge the metal bulges out; too close together the web between holes stretches or tears, and small punches break.
Rule 09
Follow the fastener maker's minimum distance to edge and to bend; sheet at least the hardware's minimum thickness
Rule 10
Tab-and-slot joints with slot clearance about 0.005–0.010 in (0.13–0.25 mm) over the tab
Rule 11
Stitch weld long seams on thin sheet, for example 1 in (25 mm) welds on 3–4 in (75–100 mm) centers
Standard: AWS D1.3 for sheet steel; D1.6 for stainless
Rule 12
Tolerance across bends ±0.010–0.015 in (±0.25–0.38 mm) per bend; angles ±1°
Standard: ASME Y14.5 datums; ISO 2768-1 m for untoleranced dimensions
Fig. 6A complete drawing package
Do. Every requirement is on the drawing: general tolerance, material by specification, finish by specification, critical dimensions and revision.
Avoid. Whatever the drawing leaves blank, the supplier decides, usually with the cheapest local equivalent.
Cut features come straight from the CNC program and hold closely. Each bend adds angle and position variation, and welding adds distortion on top, so tolerance by feature type rather than one block tolerance.
| Feature | Typical | Tight | Cost of tight |
|---|---|---|---|
| Laser or punched feature position | ±0.005 in (±0.13 mm) | ±0.003 in (±0.08 mm) | Moderate |
| Hole diameterTight usually means reaming | ±0.005 in (±0.13 mm) | ±0.002 in (±0.05 mm) | Moderate |
| Dimension across one bendStacks with each added bend | ±0.010–0.015 in (±0.25–0.38 mm) | ±0.005 in (±0.13 mm) | High |
| Bend angleTight needs angle measurement or bottoming | ±1° | ±0.5° | Moderate |
| Flatness of a cut panelTight needs leveled stock | 0.005 in/in of length | 0.002 in/in of length | Moderate |
| Self-clinching hardware position | ±0.005 in (±0.13 mm) | ±0.003 in (±0.08 mm) | Low |
| Welded assembly overallTight needs fixtures or post-weld machining | ±0.030 in (±0.8 mm) | ±0.015 in (±0.4 mm) | High |
Basis: Typical laser and press brake practice; ISO 2768-1 m for untoleranced dimensions. Put a general tolerance note on the drawing and tighten only the features that need it; every tight callout is priced. See the tolerance guide.
The same sheet metal rules shift with the alloy or compound.
Bends at 1× thickness or tighter with little springback and takes powder coat well. It rusts bare, so plan a finish.
Hot-rolled A36 is used for heavier brackets and frames from about 0.188 in (4.8 mm) up. Use an inside radius of 1–1.5× thickness and expect mill scale that needs blasting before paint.
The go-to aluminum for bent sheet. It bends at about 1× thickness in common gauges and welds well, with more springback than steel.
Stronger but crack-prone in bending. Use an inside radius of 1.5–3× thickness, more on heavy gauges, and bend across the grain, or switch to 5052-H32.
Springs back about twice as much as mild steel and work hardens at the bend. It cuts slower on the laser and shows heat tint at welds that needs pickling or passivation.
Bends very tight in soft tempers but reflects fiber laser energy, so cut speed drops and edge quality varies. Burrs smear and need a deburr step on bus bars.
Run these against the model before it goes out for quote. The builder's DFM check catches most of them on an uploaded part.
0 of 12 checked
Plan on a flange at least 4× material thickness long, measured from the outside of the bend. On 0.060 in (1.5 mm) steel, that is about 0.240 in (6 mm). Shorter flanges cannot span the V-die, which is typically 6–8× thickness wide, and slip during bending. Some shops can form shorter flanges with special tooling at added cost.
K-factor locates the neutral axis as a fraction of thickness and typically falls between 0.3 and 0.5. Air bending mild steel at a radius near 1× thickness often lands around 0.4–0.45. Treat any value in CAD as a starting point and send the 3D model, because the shop adjusts the flat pattern to its own tooling and material.
Make the relief at least 1× material thickness wide and deep enough to pass the bend radius plus the thickness. On 0.060 in (1.5 mm) steel with a 0.060 in radius, that is 0.060 in wide and at least 0.120 in (3 mm) deep. Round or obround ends reduce the crack risk at the relief root.
Metal in the bend zone stretches on the outside and compresses on the inside as it wraps the punch. Any hole inside that zone stretches with it and turns oval. Keep the hole edge at least 2.5× thickness plus the inside bend radius from the bend, or cut the hole after bending if it has to sit closer.
Most steel electronics enclosures use 16 gauge, 0.060 in (1.5 mm), or 14 gauge, 0.075 in (1.9 mm). Aluminum enclosures commonly use 0.063 in or 0.080 in 5052-H32. Choose the thinnest standard gauge that meets stiffness and hardware requirements, then add flanges or formed ribs for stiffness rather than a heavier gauge.
Each bend adds about ±0.010–0.015 in (±0.25–0.38 mm) of position variation and ±1° of angle. A feature across three bends can drift ±0.030 in (±0.8 mm) or more if dimensions are chained. Dimension critical features from one datum, and use floating hardware or slotted holes where parts must line up across several bends.
Check your part against these rules.
Drop a STEP file in the builder for an instant DFM check and a budgetary estimate, then send it to principals who run sheet metal every day.
