Guide
What is the minimum hole-to-bend distance in a stamped metal part?
Hole-to-bend distance is the clear flat material between the edge of a pierced hole and the bend it sits next to, measured on the flat leg of a formed stamping. If that strip is too narrow, the metal that stretches and compresses during bending pulls the hole out of round and shifts it off its position.
By Saola Manufacturing engineering team · Published · Updated
No ISO, ASTM or DIN standard sets a single hole-to-bend number, because the answer depends on material, thickness, bend radius and die design. The published references do define the geometry of a bend, and this guide builds the rule of thumb from that geometry, then ends with a checklist for cold-rolled steel (SPCC), 304 stainless (SUS304) and cartridge brass. The multipliers here are typical industry guidance, not values from a standard and not the capability of any press shop.
On this page
Where is hole-to-bend distance measured from?
Measure it from the edge of the hole to the bend tangent line, the line where the flat leg stops and the curved part of the bend begins. On a drawing that is usually easier to dimension from the inside face of the formed flange, which sits one inside bend radius (R) beyond the tangent line.
The terms come from flat-pattern layout. The FAA’s airframe handbook defines the bend tangent line as the place where the metal starts and stops curving, and the setback as the distance from the outside mold line back to that tangent line; for a 90-degree bend the setback equals the inside radius plus the material thickness, R + T (FAA-H-8083-31A). For bends other than 90 degrees the handbook multiplies R + T by a factor equal to the tangent of half the bend angle.
That gives three reference faces for the same hole, differing by R or by T. The drawing has to say which face a hole is dimensioned from, and the design rule has to be applied to that same face.
Because the tangent line moves with the radius, check hole clearance again whenever the supplier proposes a larger radius to avoid cracking.
What is the minimum hole-to-bend distance for a stamped part?
Typical industry guidance keeps the nearest edge of a hole at least about two material thicknesses clear of the bend tangent line, which is the same as 2T + R from the inside face of the flange. Many design guides quote 2.5T + R instead, and that larger figure is the safer default for small holes and hard tempers.
The basis for the multiplier is physical rather than normative. During bending, the outer fibers stretch, the inner fibers compress and the sheet thins through the bend; the FAA handbook notes the bend area ends up thinner than the original sheet (FAA-H-8083-31A). That disturbance does not stop exactly at the tangent line. It fades out over a short band of flat material next to it, and the width of that band scales with thickness. A hole whose edge sits inside the band is pulled toward the bend and becomes a slot or a teardrop.
A worked example makes the numbers concrete. Take typical 1.5 mm cold-rolled steel bent to an inside radius equal to its thickness. Under the 2T + R rule of typical guidance, the hole edge should sit at least 4.5 mm from the inside face of the flange, or 6 mm from the outside face. Under the 2.5T + R rule it would be 5.25 mm from the inside face, which is typical of what a conservative drawing uses.
Slots parallel to the bend and square-cornered cutouts typically need more clearance than round holes, because a long edge parallel to the bend line sees the whole strain field at once.
What happens if a hole is too close to a bend, and how do you fix it?
The hole distorts, its center shifts toward the bend, and the bend line itself can wander along the weakened section. There are four standard fixes: move the hole, add relief, pierce the hole after forming, or accept a looser tolerance on that feature.
- Move the hole. Often the cheapest fix. A hole that only needs to be on the flange, not at a specific height, can move out of the deformation band without affecting the assembly.
- Add a relief cut. A slot or notch that runs across the bend line, or a relief hole where two bends meet, lets the metal move without dragging the hole with it. The FAA handbook describes relief holes at intersecting bends as a way to relieve stress and prevent tearing, and gives the bend radius as the most common basis for their diameter (FAA-H-8083-31A).
- Pierce after forming. In a progressive die, a hole can be pierced in a station after the bend, or with a cam-driven punch that pierces the formed flange. The hole is then round and in position regardless of the bend, but the die gets more complex, and that cost belongs in the quote discussion.
- Loosen the tolerance. If the hole is a clearance hole for a screw, slight ovality may be harmless. Say so on the drawing so the supplier does not add a die station to hold a tolerance nobody needs.
For a hole that locates the part or takes a pin, piercing after forming is usually worth it.
How close can a hole be to the part edge or to another hole?
Typical guidance keeps a pierced hole at least one to two material thicknesses from the blank edge and from the next hole. Below that, the web between them bulges or tears when the punch goes through, and the die section between the punches gets too thin to last.
Hole size follows the same logic. Typical guidance for punching holds the hole diameter at or above the material thickness in mild steel and brass, and somewhat larger in stainless, because a slender punch buckles or breaks when it has to shear a thick, strong sheet. Smaller holes are possible, but they are typically drilled, laser cut or pierced with special tooling, which changes the cost.
Two more features interact with hole placement. First, the burr: a punched hole has a clean shear side and a burr side, and the drawing should say which face must be burr-free if it matters. Second, the grain: the FAA advises laying bend lines across the rolling direction where possible, and its layout chapter explains that too small a radius cracks the sheet (FAA-H-8083-31A). A crack that starts at the bend will find a hole nearby, so grain direction and hole placement are reviewed together.
How do the bend radius and the material change the rule?
A larger radius moves the tangent line away from the flange, and a harder temper needs a larger radius, so the hole must move with it. The FAA’s published radius table for aluminum shows how quickly the required radius grows with temper and thickness.
| Alloy and temper | t = 0.032 in | t = 0.064 in | t = 0.128 in |
|---|---|---|---|
| 5052-H32 | 0 | ½t–1t | ½t–1½t |
| 6061-T4 | 0–1t | ½t–1½t | 1t–2t |
| 6061-T6 | ½t–1½t | 1t–2t | 1½t–3t |
| 2024-T3 | 2t–4t | 3t–5t | 4t–6t |
| 7075-T6 | 3t–5t | 4t–6t | 5t–7t |
Read the table together with the hole rule. In 6061-T6 at the thickest column the recommended radius can reach three thicknesses, so a hole at 2T + R from the inside face needs about five thicknesses of flange before it, not three.
The same logic applies to steel, stainless and brass, although the FAA table covers aluminum only. For steel plate and flat bar, German drawings often cite DIN 6935 for cold-bending radii; for sheet, the supplier’s material certificate and a bend test in the sense of ASTM E290 are the practical evidence that a radius will not crack. In every case, choose the radius first, then place the holes.
What should a DFM checklist cover for SPCC, SUS304 and brass stampings?
For each material, confirm the designation and temper, the inside radius, the hole-to-bend and hole-to-edge clearances, the grain direction and which face must be burr-free. The table lists what typically changes from one material to the next.
| Check | SPCC cold-rolled steel | SUS304 stainless | C26000 brass |
|---|---|---|---|
| Name the spec on the drawing | JIS SPCC, or the ASTM A1008 designation you accept as equal | JIS SUS304 or ASTM A240 Type 304, with finish | ASTM B36 C26000, with temper |
| Inside radius | Often about 1T; confirm with supplier | Often larger than steel; work hardens | Soft tempers bend tight; hard tempers need more |
| Hole-to-bend start point | 2T + R from inside face | 2.5T + R or more | 2T + R; more in hard tempers |
| Smallest punched hole | About 1T | Larger than 1T | About 1T |
| Springback | Moderate | High; die must overbend | Rises with temper |
| Grain and burr | Bend across rolling direction; mark burr side | Same; protect cosmetic face | Same; burr side matters for plated contacts |
Two cross-reference traps are worth checking before the RFQ goes out. SPCC is a Japanese designation that many Asian mills and shops use by default; a US drawing that calls out ASTM A1008 should say whether SPCC is acceptable, because the two specifications are organized differently and are not automatically interchangeable. Brass needs its temper stated, because the same alloy in a hard temper behaves like a different material at the bend.
If the part is plated or coated after stamping, allow for the coating in hole sizes near bends; the finishing comparison guide covers how each finish affects dimensions.
What should the drawing and RFQ say about holes near bends?
Dimension every critical hole from a stated face of the formed part, mark which holes locate or mate, and give a general tolerance for the rest. A supplier in Vietnam, Mexico or anywhere else can then decide at the quote stage which holes are pierced flat and which after forming.
- One datum scheme. Dimension holes on a flange from that flange’s own features where possible. A hole dimensioned across a bend picks up the bend angle tolerance as well as the piercing tolerance.
- Flat pattern as reference only. Send the STEP model of the formed part and treat any flat pattern as reference, because the supplier’s bend allowance for its own tooling will differ from the CAD default.
- Functional holes flagged. List the holes that locate the part or take a pin, so they are reviewed for piercing after forming instead of discovered at first article.
- General tolerance named. Cite a general tolerance class such as ISO 2768-1 m, or your title-block convention; the tolerance guide explains the options.
Saola Manufacturing places stamping with partner plants it manages, and a drawing sent for a quote gets a design-for-manufacturing reply that names any hole sitting inside a bend zone before tooling is discussed. The RFQ package guide lists what else to include, and the quote form takes STEP and PDF files.
Frequently asked
Is there an ISO or ANSI standard for hole-to-bend distance?
Not as a single required value. Standards define the materials, the bend test and the drawing conventions, while the hole-to-bend multiplier is industry guidance derived from bend geometry. That is why the drawing should state the dimension and its reference face rather than rely on a rule both sides assume.
Should I use 2T + R or 2.5T + R?
Use the larger clearance where you have room, and especially for stainless, hard tempers, small holes and slots parallel to the bend. Where space is tight, ask the supplier to review the feature; piercing after forming is usually the way to keep the hole close.
Does the rule change for a hem or an offset?
Yes. A hem folds the metal back on itself and an offset puts two bends close together, so the deformation zones add up. Keep holes away from both bends of an offset and review any hole near a hem individually.
What tolerance can a stamped hole hold relative to a bend?
It depends on the material, thickness, die design and whether the hole is pierced before or after forming, so it is answered part by part in the quote. Holes pierced after the bend typically hold position better than holes pierced flat.
Sources
- Aviation Maintenance Technician Handbook — Airframe, Volume 1 (FAA-H-8083-31A), Chapter 4: layout and forming terminology, setback, relief holes, Federal Aviation Administration, 2018
- Advisory Circular AC 43.13-1B, Acceptable Methods, Techniques, and Practices, paragraphs 4-55 and 4-56 and Table 4-6, Federal Aviation Administration, 1998
- ASTM E290-22, Standard Test Methods for Bend Testing of Material for Ductility (scope), ASTM International, 2022
- ASTM A1008/A1008M-24, Standard Specification for Steel, Sheet, Cold-Rolled (scope), ASTM International, 2024
- ASTM A240/A240M-24, Chromium and Chromium-Nickel Stainless Steel Plate, Sheet, and Strip (scope), ASTM International, 2024
- ASTM B36/B36M-18, Standard Specification for Brass Plate, Sheet, Strip, and Rolled Bar (scope and alloy list), ASTM International, 2018