Wireform tolerances: what to put on the drawing and what to leave to the process

The principle: tolerance the function

A wireform drawing usually has fewer dimensions than a machined drawing, but each one carries more weight. A bend position controls the length of two legs and the position of everything after it. A bend angle controls the direction of a leg and the load path. If every dimension carries the same tight tolerance, the supplier has to assume that every feature is critical, and the price reflects that assumption.

The alternative is to identify the features that locate the part in the assembly and the features that carry the load, tolerance those, and let a general tolerance cover the rest. That is not a lower quality standard. It is a statement about where the variation matters, which is exactly what a supplier needs to choose a process.

This guide uses indicative bands for small formed wire parts in the 0.5 to 3 mm diameter range. They are starting points for a discussion, not a published standard. The supplier's capability and the part geometry will move them.

What the process holds without special measures

The table below gives indicative production bands for a CNC formed wire part. They assume a stable wire lot, a standard tool set and a general tolerance in the title block. A tighter call is possible, but it usually needs a different tool, a slower cycle, extra inspection or a selected wire lot.

How bend errors stack

Each bend has a position tolerance and an angle tolerance. The position errors add along the part in the same direction, so a chain of five bends at plus or minus 0.2 mm can put the last feature at plus or minus 1.0 mm in the worst case. The angle errors add in a different way: a small angle error at an early bend moves the tip of a long leg by the leg length times the angle in radians.

For an illustrative example, a 1 degree error at a bend with a 40 mm leg moves the tip by about 0.7 mm. That is larger than the bend position tolerance, which is why the angle call often matters more than the position call on a part with long legs. The same 1 degree error on a 10 mm leg moves the tip by about 0.17 mm.

A statistical stack, where the errors are assumed independent and combined as the root sum of squares, gives a smaller number than the worst case. For five bends at plus or minus 0.2 mm, the root sum of squares is about plus or minus 0.45 mm. The statistical number is useful for predicting the batch, but the worst case is the right number for a fit that must never fail.

Datums on a wire part

A wire part does not have a natural flat face to use as a datum. The practical datum is a leg, a bend centre or a pair of bend centres. Choose the feature that the assembly uses to locate the part. If the part hangs from a hook, the hook is the datum. If it sits in a groove, the two legs that touch the groove are the datum.

Once the datum is chosen, dimension the other features from it. A chain of dimensions from a single datum is easier to inspect and easier to program than a series of relative dimensions, but it can produce long tolerance chains. A mixed approach, with a primary datum and local dimensions for features that move together, is often the practical answer.

If the part is measured on a CMM, the fixture has to hold it in the same way the assembly does. A wire part that is measured free can distort under its own weight or under the probe force. Agree the fixture and the clamping with the supplier before the first article.

Angles, radii and linear dimensions

An angle call is more stable than a linear call across a bend, because it does not include the wire diameter. A dimension from one outside surface to another includes the wire twice, so the wire tolerance appears in the result. A dimension between bend centres avoids the wire diameter and is the better control for a multi-bend part.

Radius calls deserve care. The inside radius is set by the tool, but the finished radius depends on springback. If the radius is functional, give it a band and say what it controls. If it is not, give a minimum radius and let the supplier use a standard tool. A drawing that calls an exact radius with no tolerance is asking for a measurement that the process cannot hold without a trial.

For a spring, replace a stack of linear dimensions with the free length, the load at a stated deflection and the spring rate. Those three calls describe the function and let the supplier choose the wire and the coil geometry. They also let the inspector test the part in the way it will be used.

What to leave to the process

Some features are better left to the supplier. The exact tool radius, the overbend at each bend, the bend sequence and the position of a cut in the feed are process decisions. If the drawing specifies them, it removes the supplier's ability to optimise the setup and it usually adds cost without improving the function.

The same applies to the tip form on a cut end. A small chamfer or a deburr is often a process default. If the assembly needs a specific tip, call it. If it does not, let the supplier use the standard cut and deburr. A drawing that calls a chamfer on every end without a reason adds a handling step to every part.

Coating thickness is another example. If the coating is decorative, a standard thickness range is enough. If it is functional, for example for contact resistance or corrosion life, give the standard and the minimum thickness. Do not give a nominal thickness with no range, because no coating process holds a single value.

• Tool radius and overbend: supplier's process decision
• Bend sequence and feed position: supplier's process decision
• Standard cut and deburr: default unless the assembly needs a tip form
• Coating thickness: a range with a minimum, not a single value
• Bend radius: a minimum or a band, not an absolute

Agree the inspection before the first article

A tolerance is only useful if both sides agree how it will be measured. For a wireform, that usually means a mix of a functional gauge, a few dimensional checks and a load test. The gauge proves the assembly condition. The dimensional checks prove the bend positions that the gauge cannot see. The load test proves the spring function.

Agree the sampling and the record. For a stable part, a first article plus a periodic check may be enough. For a part that feeds an automated line, add a gauge check at the start of each shift and a load check at each lot change. Write the method into the control plan so that a new operator does the same thing.

If the part is measured on a CMM, agree the fixture, the datum scheme and the number of points on each feature. A wire is a curved surface, so the point count and the fitting method change the result. A report that gives a single number without the method is hard to defend when a batch is questioned.

A worked tolerance set

Take an illustrative retaining clip in 1.6 mm stainless 302, five bends, one long leg of 35 mm and a loop that passes a 4 mm pin. A practical set might be: bend positions at plus or minus 0.3 mm, bend angles at plus or minus 1 degree, the loop inside diameter at plus or minus 0.1 mm, the free length at plus or minus 0.5 mm, and a general tolerance of plus or minus 0.5 mm for the undimensioned features.

The loop and the long leg are the functional features. The loop gets the tight call because it must pass the pin. The long leg gets the angle call because a 1 degree error moves the tip by about 0.6 mm. The other bend positions carry the general tolerance, because the clip is compliant and the housing absorbs the variation.

That set is defensible, inspectable and cheaper than a drawing where every dimension is plus or minus 0.1 mm. It also tells the supplier where to spend the effort, which is the real purpose of a tolerance.