Design stamped parts with holes at least 1× material thickness in diameter (1.5–2× for stainless), holes at least 1.5× thickness from an edge, an inside bend radius of at least 1× thickness for mild steel, and holes at least 2.5× thickness plus the bend radius from a bend. Expect ±0.002–0.005 in (±0.05–0.13 mm) on pierced features and ±0.010 in (±0.25 mm) across bends.
SSG MFG · design guideDG-02 · 13 rules
13 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 | Design to a stock thickness0.005–0.250 in (0.13–6.4 mm) typical; use standard mill gauges | 0.005–0.250 in (0.13–6.4 mm) typical; use standard mill gauges |
| 02 | Radius outside corners of the blankCorner radius at least 0.5× thickness; sharp corners only where the die cuts them in one hit | Corner radius at least 0.5× thickness; sharp corners only where the die cuts them in one hit |
| 03 | Keep slots and tabs wide enoughWidth at least 1.5× material thickness; length no more than 5× width for narrow punches | Width at least 1.5× material thickness; length no more than 5× width for narrow punches |
| 04 | Size holes to the punchDiameter at least 1× thickness for mild steel and aluminum; 1.5–2× for stainless | Diameter at least 1× thickness for mild steel and aluminum; 1.5–2× for stainless |
| 05 | Space holes from edges and each otherHole to edge at least 1.5× thickness; hole to hole at least 2× thickness | Hole to edge at least 1.5× thickness; hole to hole at least 2× thickness |
| 06 | Set the inside bend radius by materialAt least 1× thickness for mild steel and 5052-H32; 1.5–3× for 6061-T6, half-hard and spring tempers | At least 1× thickness for mild steel and 5052-H32; 1.5–3× for 6061-T6, half-hard and spring tempers |
| 07 | Bend across the rolling directionBend lines perpendicular to the grain where possible; add about 0.5–1× thickness to the radius when bending parallel | Bend lines perpendicular to the grain where possible; add about 0.5–1× thickness to the radius when bending parallel |
| 08 | Make flanges long enough to formAt least 2.5× thickness plus the inside bend radius | At least 2.5× thickness plus the inside bend radius |
| 09 | Add relief where a bend meets an edgeRelief width at least 1× thickness; depth at least thickness plus bend radius | Relief width at least 1× thickness; depth at least thickness plus bend radius |
| 10 | Keep holes clear of bendsEdge of hole at least 2.5× thickness plus the inside bend radius from the bend | Edge of hole at least 2.5× thickness plus the inside bend radius from the bend |
| 11 | Allow for springback on formed anglesTypical springback 1–2° for mild steel, 2–4° for 304 stainless, more for 6061-T6 and spring tempers | Typical springback 1–2° for mild steel, 2–4° for 304 stainless, more for 6061-T6 and spring tempers |
| 12 | Tolerance across bends more loosely±0.002–0.005 in (±0.05–0.13 mm) on pierced features; ±0.010 in (±0.25 mm) across one bend | ±0.002–0.005 in (±0.05–0.13 mm) on pierced features; ±0.010 in (±0.25 mm) across one bend |
| 13 | Call out burr side and heightNote the burr side on the drawing; expect burr up to 10% of thickness | Note the burr side on the drawing; expect burr up to 10% of thickness |
These build on the short list on the stamping process page, with the failure each rule prevents and a drawing for each.
Change the inside bend radius against thickness and material to see where the outside of the bend starts to crack, how springback grows, how the flat blank length moves, and how far a hole has to sit from the bend line.
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
0.005–0.250 in (0.13–6.4 mm) typical; use standard mill gauges
Rule 02
Corner radius at least 0.5× thickness; sharp corners only where the die cuts them in one hit
Rule 03
Width at least 1.5× material thickness; length no more than 5× width for narrow punches
Rule 04
Diameter at least 1× thickness for mild steel and aluminum; 1.5–2× for stainless
Rule 05
Hole to edge at least 1.5× thickness; hole to hole at least 2× thickness
Fig. 1Hole 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 06
At least 1× thickness for mild steel and 5052-H32; 1.5–3× for 6061-T6, half-hard and spring tempers
Fig. 2Bend 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 07
Bend lines perpendicular to the grain where possible; add about 0.5–1× thickness to the radius when bending parallel
Rule 08
At least 2.5× thickness plus the inside bend radius
Fig. 3Minimum 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 09
Relief width at least 1× thickness; depth at least thickness plus bend radius
Fig. 4Bend 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 10
Edge of hole at least 2.5× thickness plus the inside bend radius from the bend
Fig. 5Hole 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 11
Typical springback 1–2° for mild steel, 2–4° for 304 stainless, more for 6061-T6 and spring tempers
Rule 12
±0.002–0.005 in (±0.05–0.13 mm) on pierced features; ±0.010 in (±0.25 mm) across one bend
Standard: 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.
Rule 13
Note the burr side on the drawing; expect burr up to 10% of thickness
Fig. 7Burr direction
Do. The drawing names the burr side, and the burr faces away from mating, sealing and handled surfaces.
Avoid. A burr on the mating face holds parts apart, cuts hands and wiring, and can break off as loose debris.
Features cut in the same die station are held by the tool and repeat closely. Anything measured across a bend or between stations adds forming variation, so tolerance those features separately.
| Feature | Typical | Tight | Cost of tight |
|---|---|---|---|
| Pierced hole diameterTight needs shaving or a finish punch | ±0.002 in (±0.05 mm) | ±0.001 in (±0.025 mm) | Moderate |
| Hole to hole, same station | ±0.002 in (±0.05 mm) | ±0.001 in (±0.025 mm) | Moderate |
| Blank outline | ±0.005 in (±0.13 mm) | ±0.002 in (±0.05 mm) | Moderate |
| Dimension across one bendStacks with each added bend | ±0.010 in (±0.25 mm) | ±0.005 in (±0.13 mm) | High |
| Bend angleTight usually needs a restrike station | ±1° | ±0.5° | Moderate |
| FlatnessTight needs a flattening or coining station | 0.005 in/in of length | 0.002 in/in of length | Moderate |
| Formed or embossed height | ±0.005 in (±0.13 mm) | ±0.003 in (±0.08 mm) | Moderate |
| Burr heightTight usually means a deburr step | 10% of thickness | 5% of thickness | Low |
Basis: Industry-typical press tolerances; 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 stamping rules shift with the alloy or compound.
The default stamping steel. It bends at 1× thickness or tighter across the grain and pierces holes down to about 1× thickness with little springback.
Bends at about 1× thickness in common gauges but springs back more than steel for the same radius. Burrs are softer and it can gall on the die without lubricant.
Work hardens as it forms, so minimum holes go to 1.5–2× thickness and springback roughly doubles against mild steel. Expect faster die wear and higher press tonnage.
Ferritic and less ductile than 304 in bending. Keep the radius at 1–1.5× thickness and bend across the grain to avoid cracks on the outside of the bend.
Usually stamped in spring tempers for contacts and clips. Harder tempers need an inside radius of 1–3× thickness and bends across the grain, so specify temper and grain direction on the print.
Very ductile in soft tempers and bends at 0.5× thickness or less. It burrs heavily and smears, so tight punch clearance and burr callouts matter.
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
For cold-rolled 1008 steel, an inside bend radius equal to the material thickness is a safe default, and many parts bend tighter across the grain. Stainless 304 and 430 are usually kept at 1–1.5× thickness, while 6061-T6 aluminum and spring-temper bronze need 1.5–3×. Bending parallel to the rolling direction calls for a larger radius than bending across it.
Keep the edge of the hole at least 2.5× material thickness plus the inside bend radius from the bend line. For 0.060 in (1.5 mm) steel with a 0.060 in radius, that is about 0.210 in (5.3 mm). Closer holes sit in the stretch zone and distort into ovals, unless they are pierced after forming in a later station.
Hole edge to part edge should be at least 1.5× material thickness, and hole to hole at least 2× thickness. On 0.060 in (1.5 mm) steel, that is 0.090 in (2.3 mm) to the edge and 0.120 in (3.0 mm) between holes. Thinner webs bulge or tear as the punch goes through.
Springback is the elastic recovery of the metal after the forming load comes off. It grows with yield strength and with the ratio of bend radius to thickness. Typical values are 1–2° for mild steel and 2–4° for 304 stainless at a radius near 1× thickness. Dies overbend or restrike to compensate.
The burr forms on the side where the punch exits, the die side of the cut. Its height is typically up to 10% of material thickness. Show the burr side on the drawing so the toolmaker can orient the part in the die, and add a deburr note only where the edge touches people or a sealing face.
ISO 2768-1 medium (m) is a reasonable default for untoleranced linear dimensions on stampings, since it allows about ±0.004–0.008 in (±0.1–0.2 mm) in common sizes. Put explicit tolerances on holes and on any dimension that crosses a bend, because bend variation can exceed the general tolerance class.
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 stamping every day.
