Hole deformation near a bend: why the hole moves

A Ø10 hole that comes back 10.4 mm one way and 9.9 mm the other, and half a millimetre off its dimension, has failed in two independent ways. The ovality is hole deformation near a bend: the material on the bend side of the hole was stretched around the radius while the material on the flat side was not. The position error is a separate fault, because the flat pattern consumed more or less material in the bend than the die actually needed.

Both errors appear after forming, so both are blamed on the press brake. The brake is rarely the cause. A hole either sat inside the zone the die deforms plastically, or it was placed from a bend allowance that did not match the tooling on the machine. One is a geometry decision made in CAD, the other a flat-pattern decision made in CAD, and both are cheaper to fix there than on the shop floor.

This is written for design engineers placing holes on parts that will be bent on a press brake, usually in 1–4 mm CRCA, stainless or aluminium. It separates the two failure modes, gives the strain arithmetic behind the ovality, quantifies the movement a K-factor mismatch produces on its own, and sets out the callouts that let a supplier inspect the requirement that matters. The design and CAD hub holds the related rules on bend relief, datum strategy and drawing notes.

Hole deformation near a bend: form error and position error are not the same fault

The deformation is a form error and the movement is a location error. A hole that has gone oval has been strained, and no back-gauge adjustment recovers it. A hole that is still round but half a millimetre from its dimension was developed from the wrong flat, and no amount of forming control recovers that either.

Three measurements separate the cases, and they need three different controls on the drawing:

• Form. Measure the diameter along the bend direction and across it. A difference of 0.40 mm is a circularity error of 0.20 mm, because circularity is the radial separation between two concentric circles, not the diameter spread.
• Position. Measure the centre from the datums. Measuring from the nearest edge folds the edge's own tolerance into the result and hides which feature moved.
• Size. Plastic flow moves the mean diameter as well as the spread. A hole that grows 0.15 mm in both directions is a size problem, not an ovality problem, and it usually means the hole was too close to the bend for the strain it carried.

A hole inside the bend zone often shows all three at once. That is why a single ±0.2 mm note on the hole diameter does not describe the requirement, and why a first article that measures one diameter across the hole can pass a part that will not assemble.

The keep-out comes from the die opening, the strain from the radius

The distance that keeps a hole out of the deformed zone is R + V/2 + t, measured from the bend line to the nearest point on the hole. For 3 mm CRCA on a 24 mm V die with a 3 mm inside radius that is 18 mm. Add the 5 mm hole radius and the centre has to sit 23 mm from the bend line. The formula and its table by thickness belong to the hole-to-bend distance guide, which owns that rule; this article is about what happens inside it.

The strain that does the damage is set by the radius-to-thickness ratio, not by the die opening. For a bend of inside radius R, thickness t and K-factor K, the neutral axis sits R + Kt from the inside surface and the outer surface is (1 − K)t further out. The engineering strain at that surface is:

ε = (1 − K)t / (R + Kt)

With K = 0.44 it collapses to ε = 0.56 / (R/t + 0.44). The ratio decides everything:

• R/t = 1 gives 0.56 / 1.44 = 38.9% strain.
• R/t = 2 gives 0.56 / 2.44 = 23.0%.
• R/t = 4 gives 0.56 / 4.44 = 12.6%.
• R/t = 6 gives 0.56 / 6.44 = 8.7%.

Cold-reduced steel only survives the R/t = 1 case because the strain is a gradient through the thickness rather than a uniform pull. The outer surface is at the limit, and a hole edge sitting in that surface has no reserve left. That is the physical reason a tight bend is the worst place to put a hole, and why the same hole on a 6 mm radius comes back much closer to round.

What a hole near a bend does, by position

The table applies the two mechanisms to a Ø10 hole in 3 mm CRCA at an R/t of 1, formed on a 24 mm V die with K = 0.44. Values are for the hole only; tooling wear, material yield spread and back-gauge repeatability add on top.

The first row is the one design engineers under-use. A hole outside the zone is a pure flat-pattern question, and it can be solved by agreeing a bend deduction with the supplier rather than by moving the hole. The third row is the one that cannot be solved by tolerance at all: a hole that crosses the tangent line is asking a flat feature to exist on a curved surface.

A worked example: a Ø10 hole at 20 mm from the bend

Take a 200 mm wide bracket in 3 mm CRCA with a 90° bend at a 3 mm inside radius, formed on a 24 mm V die. A Ø10 hole on the first flange has its centre 20 mm from the bend line, and a second Ø10 hole on the other flange has its centre 40 mm from the same line. K is 0.44.

The near edge of the first hole sits at 20 − 5 = 15 mm, which is 3 mm inside the 18 mm keep-out. The flat length between the two hole centres is the sum of the flange distances minus the bend deduction:

• BA = (π/2)(R + Kt) = 1.5708 × 4.32 = 6.79 mm
• OSSB = (R + t) tan 45° = 6.00 mm
• BD = 2 × 6.00 − 6.79 = 5.21 mm
• Flat centres = 20 + 40 − 5.21 = 54.79 mm

Now form it with a die that produces K = 0.33, which a tighter V and a springier grade can do. The bend allowance falls to 1.5708 × 3.99 = 6.27 mm and the deduction rises to 5.73 mm. At the same flat length the formed centres are 54.79 + 5.73 = 60.52 mm against a nominal 60.00 mm. The holes are 0.52 mm too far apart, and neither one was touched by the bend zone.

Add 0.5° of bend angle error, which is inside what a manual setup holds on a short flange. The second hole, 40 mm from the bend, moves 40 × sin 0.5° = 0.35 mm. A laser position tolerance of ±0.10 mm and a back-gauge repeatability of ±0.15 mm bring the worst case to 0.52 + 0.35 + 0.10 + 0.15 = 1.12 mm against a ±0.5 mm drawing. The part fails on the flat and the angle, not on the hole.

If the hole has to stay, the cheaper fix is to state the bend deduction and the die opening on the drawing so the model and the machine agree. If it cannot stay, move the first hole to 23 mm from the bend line, which puts its edge exactly at the 18 mm limit, and recalculate the flat from the die that will actually run.

Why the hole goes oval instead of uniformly larger

The strain is not uniform across the hole. Material on the bend side is pulled onto the arc and thins as it travels; material on the flat side keeps its original thickness. The hole edge between them is a free boundary, so it cannot carry the membrane load and yields locally instead. The diameter grows along the bend and contracts across it by roughly Poisson's ratio, 0.3 for steel.

Take the 0.4 mm growth from the table. The contraction across the bend is 0.3 × 0.4 = 0.12 mm, so the hole measures about 10.40 mm by 9.88 mm. Circularity is the radial separation, not the diameter spread: (10.40 − 9.88) / 2 = 0.26 mm. The area barely changes. That is how a hole passes a plug gauge and still gives a bolt head a poor seat.

The plastic zone is also narrower than the V/2 keep-out. Air bending concentrates plastic strain near the punch nose and leaves the material beside the die shoulder largely elastic, so a hole a millimetre outside the nominal zone often comes back round, and one a millimetre inside sometimes distorts very little. Do not design to that scatter. The keep-out exists so the scatter lands on the safe side.

What to put on the drawing

• Bend line positions on the flat and the bend deduction, with the die opening the flat was developed for.
• True position of each hole to named datums A, B and C, and which features set B and C.
• A circularity callout on every hole within 40 mm of a bend line, typically 0.10–0.20 mm, to ISO 1101 or ASME Y14.5.
• Diameter tolerance stated separately from position; a Ø10 clearance hole is not the same requirement as Ø10 ±0.05 mm.
• A process note for holes that must be pierced after forming, with the operation sequence.
• Flatness of 0.10 mm over the washer face where a bolt head seats.
• Bend angle tolerance, ±0.5° for a short flange and ±0.25° where a hole sits far from the bend.
• Material grade and temper, because yield spread moves both springback and the developed length.

ISO 2768-1 covers general tolerances for linear and angular dimensions where the drawing gives no individual tolerance, and it is a fair default for the outline. It covers neither circularity nor position, so a drawing that says only "general tolerances ISO 2768-1 class m" has not specified the feature that fails. The K-factor guide covers how to agree the bend deduction with the supplier instead of carrying a CAD default into production.

What Ganesh actually runs

Bending is on a 200 T, 5-axis CNC press brake with a 4,450 mm bed and Delem control, forming to 10 mm. The bed length matters here: a part that fits in one setup avoids the repositioning step where the relation between hole and bend drifts. Die openings are recorded against the job, so hole distances are calculated from the tool that runs rather than from a CAD default.

Cutting is a 12 kW fibre laser with a 40 ft × 16 ft bed, with 6 kW and 3 kW support machines, in CRCA, mild steel, stainless, aluminium, brass and copper. When a hole has to sit inside the bend zone, the in-house tool room builds the post-form pierce tool and the fixture, and the hole is pierced after forming on a press from 20 T to 300 T. Three CLOOS robotic MIG cells and more than 30 manual MIG, spot and SPM stations take the welded assemblies that follow.

Typical sheet metal tolerance is ±0.5 mm, tighter on critical features by agreement, and PPAP plus first article inspection are available. Where the drawing asks for both, the first article report gives roundness and position as separate results rather than a single diameter reading. The bending capability page lists the machine and tool set.

When moving the hole is the wrong fix

Sometimes the hole has to stay where it is because the mating part or the envelope is fixed. Moving it 3 mm may push it into a rib, a weld nut or a cable path, and the drawing change costs more than the process change.

In that case the honest options are to pierce after forming, to add a relief slot at the bend line on a non-cosmetic part, or to move the bend by shortening the flange. What does not work is tightening the position tolerance and expecting the brake to deliver it: the error sits in the flat and the bend angle, and neither responds to a tolerance.

We do not run tube laser cutting or five-axis laser trimming, so a formed part needing a hole in a position only reachable after forming is outside the route here. A hole that crosses the bend line is not a tolerance problem either; it needs a different part, a post-form operation, or a stamping tool that makes the hole and the form in one station.

Holes near bends are decided in CAD, and the two decisions are separate: where the hole sits relative to the deformed zone, and how the flat is developed for the die that will run. Send the flat pattern with the bend lines, the die opening and every hole within 40 mm of a bend to request a quote, and the pattern can be checked against the die set before the job is scheduled.