Bending tolerances and how to inspect a bend

Bending tolerances and inspection are two halves of one argument, and they only agree when the drawing says which tolerance it controls. A bend carries three: the angle between the two flanges, the position of the flange in space, and the shape the part settles into once it is released from the tool. A part can hold the first, miss the second, and never be checked for the third. That gap is where most bending disputes live.

The practical consequence is that a supplier and a customer can both be right and still disagree. The supplier measures 90.2° on a protractor against the flange; the customer measures the gap at the far end of a 400 mm panel and finds 5 mm. Both measurements are true, and they describe different things.

The bending and welded assemblies hub holds the rest of this cluster, including the distortion and fixture material that takes over once a formed part is welded into an assembly.

Answer first: what a bend tolerance is meant to control

A bend tolerance should control the position of the features that matter at assembly, expressed in a way the shop can measure. In practice that means choosing between angle, linear position and profile, and stating which one the drawing governs.

ISO 2768-1 is the default where the drawing gives no individual tolerance. Its scope is the dimensions of workpieces produced by metal removal or formed from sheet metal, and it provides four linear classes, f, m, c and v. For class m, the linear tolerance is ±0.3 mm over 30–120 mm, ±0.5 mm over 120–400 mm, ±0.8 mm over 400–1,000 mm and ±1.2 mm over 1,000–2,000 mm.

The angular table works differently, and this catches people out. ISO 2768-1 gives a single angular tolerance table for all four classes, indexed on the length of the shorter side of the angle: ±1° up to 10 mm, ±0°30′ over 10–50 mm, ±0°20′ over 50–120 mm, ±0°10′ over 120–400 mm and ±0°5′ over 400 mm.

Note the direction. The angular tolerance tightens as the flange gets longer. A 40 mm flange is allowed half a degree; a 400 mm flange is allowed five minutes. That is the reverse of the linear table, which loosens with length, and it exists because a fixed angular error produces a linear error proportional to the length. ISO 2768-1 keeps the tip movement roughly constant by tightening the angle.

The bending tolerances and inspection values that decide a pass

The gap between columns one and three is the point. General tolerances are a fallback for dimensions nobody thought about, and a bent part usually has several dimensions that somebody should have thought about.

Angle tolerance and linear tolerance do not move together

Take a 300 mm flange. Under ISO 2768-1 class m, the flange length is held to ±0.5 mm and the bend angle is held to ±0°10′. Convert the angle into the distance the tip can move:

Δ = L × tan(θ)

At 300 mm and 0.1667°: 300 × 0.002909 = 0.87 mm.

So the general angular tolerance permits nearly twice the tip movement the linear general tolerance would allow on the same dimension. A part can pass the general tolerance, pass the drawing, and miss the mating hole by almost a millimetre at the far edge of the flange.

Widen the callout to ±0.5° and the same 300 mm flange moves its tip 300 × tan(0.5°) = 2.62 mm. On a 600 mm flange, ±0.5° is 5.24 mm. This is the single most useful number in bending inspection: the angle tolerance is not an abstract quality grade, it is a linear displacement that grows with the flange and it lands exactly where the fixing holes are.

The response is not to tighten every angular callout. It is to decide which surface locates the part in the assembly and dimension that surface linearly, then use the angle only as a process control. A drawing that gives a flange-top-to-datum distance of 200 ±0.5 mm and an angle of 90° ±1° tells the shop what matters.

Where the bend error actually comes from

There are four sources, and they stack differently.

Bend allowance, and the K-factor behind it. The flat pattern is computed from BA = (π/180) × θ × (R + K·t). Differentiating with respect to K gives dBA/dK = 1.5708 × t for a 90° bend. On a 3 mm part, 0.02 of K-factor error costs 0.094 mm of flat length per bend. Six bends accumulate 0.57 mm, which breaks a ±0.5 mm callout before the material does anything unexpected. The K-factor explainer covers how the value is proved for a grade.

Thickness variation. A 0.10 mm coil variation changes the bend allowance by 1.5708 × 0.33 × 0.10 = 0.05 mm per bend, which is small. Its bigger effect is on springback: a thinner sheet recovers more, so the angle moves more than the length does.

Springback variation between coils. Two coils of the same nominal grade can spring back differently by a degree, which is why a bend table proved on one coil can be wrong on the next and why the angle, not the flat length, is the first thing to move.

Deflection in the machine. On a long bend the ram and bed deflect, the middle of the part gets less penetration, and the angle at the centre differs from the angle at the ends. The long panel article quantifies this and covers crown compensation.

Choosing a gauge that can actually resolve the callout

The rule of thumb is a tenth: the measuring instrument should resolve at least one tenth of the tolerance band. Apply it to the two callouts above.

For ±1°, the band is 2°, so the instrument should resolve 0.2°. A digital protractor reading to 0.1° meets that, just. For ±0°10′, the band is 0.333°, so the instrument should resolve 0.033°, and a protractor does not.

The workaround is to measure a chord instead of an angle. On a 300 mm flange, 0.033° corresponds to 300 × tan(0.033°) = 0.17 mm of tip movement. A height gauge on a surface plate, reading to 0.01 mm, resolves that with an order of magnitude to spare. Measuring the distance from the flange tip to a datum, rather than the angle itself, converts an impossible angle measurement into an easy length measurement.

For a repeat part, a checking fixture with a dial indicator at the flange tip is faster and more repeatable than either, provided the fixture is validated against a measured part and its wear points are controlled.

Measuring the errors that are not an angle

Twist and bow are the two failures that pass an angle check and fail the assembly, and both are easy to measure once the method is fixed.

Twist is a difference in elevation between two corners. Stand the part on three points and measure the gap under the fourth with a feeler gauge. The gap is the twist over the support span, so a 1 mm gap on a 1,000 mm span is 1 mm per metre regardless of how wide the part is. The trap is choosing support points arbitrarily: support at the corners of the shortest edge and the reading will describe the flange, not the part.

Bow is measured against a straight edge with a feeler gauge, or on a surface plate with a height gauge, and the result depends entirely on how the part is supported. A 3,000 mm channel supported at its ends will sag under its own weight; supported at the quarter points it will not. State the support positions in the inspection plan, then use the same positions at first article and in production.

Both measurements belong on the first article record. Neither belongs in a tolerance note that says "straight within commercial limits", because that phrase cannot be inspected and will be resolved by argument.

Proving it at first article and holding it in production

The first article record for a bent part should carry: the flat length as cut, the flange lengths, the included angle on both flanges measured clear of the radius, the tip position relative to the datum the assembly uses, twist, and the gauge used for each. Add the material coil or heat number, because the coil is the variable that most often explains a drift later.

In production, the meaningful check is the one that catches drift early. Measuring the first and last part of a run catches tool wear and thermal drift but misses a mid-run material change. Measuring the tip position on a sample every few hundred parts, using the same fixture the first article used, closes that gap for the cost of a few seconds.

Where the part is welded after bending, the bend tolerance stops being the controlling tolerance. Weld shrinkage moves the geometry by more than the bend ever did, and the welded assembly tolerances article works through the post-weld stack. The rule is to inspect the bend before welding, and the assembly after.

How Ganesh Multitech holds bending tolerance

Bending runs on the 200 T, 5-axis CNC press brake with a 4,450 mm bed and Delem control, to 10 mm. The Delem programme holds the bend table, the springback correction and the sequence per part, which is what makes a repeat order land where the first article landed rather than where the last operator left the machine. Material is cut on the 12 kW fibre laser with a 40 ft × 16 ft bed, and the cut edge quality that the brake locates against is classified under ISO 9013, so the edge the backgauge sees is a defined feature rather than an assumption.

Ganesh holds ±0.5 mm as a typical sheet metal tolerance, with tighter tolerance on critical features by agreement, and PPAP and first article inspection are available. Manufacturing runs across five units in Mumbai (Vasai) and Nagpur under ISO 9001:2015 and ISO 14001:2015.

The bending capability page carries the machine data and the bend allowance calculator reproduces the flat-length arithmetic used above with your own K-factor.

What to put on the drawing

• The datum, named, and whether it is a surface, a hole pattern or a formed feature.
• The locating interface dimensioned linearly from that datum, with the tolerance on the dimension rather than only on the angle.
• The angle callout, with the flange length it is measured over.
• Bend radius, stated explicitly, since ISO 2768-1 does not cover it.
• Flat length basis, or the requirement that the supplier proves it.
• Free-state or restrained-state inspection, stated.
• Twist and straightness callouts with the measuring method.
• Which surfaces are inspected before coating and which after.

Dimensioning practice for all of this is set out in ISO 129-1, which covers the presentation of dimensions and tolerances on technical drawings. Following it is not a formality: an ambiguous datum is the most common reason two inspectors produce two answers from one part.

When the tolerance conversation is the wrong one

If a bent part keeps failing at assembly, tightening the angle callout is usually the wrong first move. The cheaper fix is often to change the design so the locating feature is a hole rather than a flange edge, or to add a slot that gives the joint somewhere to move. A tolerance is a promise about variation; it cannot create clearance that the design never provided.

It is also the wrong conversation when the tolerance is tighter than the process can earn. Below ±0.2 mm on a formed feature, the correct answer is usually to form oversize and machine, or to move the feature to a second operation — and to say so at quotation rather than at the third rejected batch.

Send the drawing with the assembly interface marked, or request a quotation with the annual volume attached. The review will tell you which of the three tolerances the part actually depends on, and which callouts can be relaxed without the assembly noticing.