Busbar tolerances: what to specify

Tolerance is a cost decision

A busbar drawing with every dimension tight does not get a better part. It gets a slower process, more inspection and a higher price. A tight call has to be measured, and if the process cannot hold it comfortably, the supplier has to add a step, a fixture or a rework loop.

The useful question is not 'how tight can this be made' but 'what does the assembly need'. A hole that locates a joint needs a tighter position than a hole that passes a cable. A bend that sets a joint face needs a tighter angle than a bend that only routes a cable. The drawing should show that difference, so the supplier knows where to spend the effort.

The calls that decide fit

The table below gives a practical starting set for a copper busbar. The values are illustrative and should be adjusted for the assembly, the process and the customer standard. They are grouped by the feature that drives the fit, not by the order of the drawing.

Use a general tolerance for the rest

A title block call such as ISO 2768-m covers the dimensions that do not locate anything. It gives the supplier a default and keeps the drawing readable. The alternative, a tolerance on every dimension, hides the critical calls in a wall of numbers and invites the supplier to treat them all as equally important.

The general tolerance should match the process. A cut length on a saw or a shear can hold a wider band than a machined edge. A punched hole can hold a tighter position than a flame-cut edge. If the drawing calls a class the process cannot meet, the supplier will either quote a higher price or ask for a deviation.

State the standard and the class in the title block, and say that untoleranced dimensions fall under it. If a feature is reference only, mark it as reference. If a feature is critical, give it its own tolerance and, where useful, a datum.

Twist and flatness

Twist is a rotation about the long axis. It is easy to miss on a drawing because the bar still looks straight in plan. A twisted bar will not sit flat on a joint face, and the bolt load will try to pull the twist out, which puts a bending stress on the joint. A call of 1 mm per 300 mm is a practical starting point for a panel bar.

Flatness is a different call. It says how far the surface may deviate from a plane. A bar can be straight along its length and still be bowed across its width. If the joint face is machined, flatness is controlled by the machining. If the bar is used as rolled, the mill flatness and the forming process decide the result.

Measure both on a surface plate or in a fixture that holds the datum. A twist measured with the bar resting on a bench can be misleading, because the bar may rock rather than show its true rotation. The inspection method belongs on the drawing or in the inspection plan.

Hole position and the bend

Hole position is usually the tightest call on a busbar because it sets the joint alignment. A pair of holes that is 0.5 mm out can make a bolted joint difficult to assemble, especially when two bars and a lug share the same bolts. A position tolerance of ±0.2 mm is common for a locating hole, while a clearance hole can be wider.

If the bar is bent after punching, the hole moves. The bend stretches the material on the outside and compresses it on the inside, and a hole near the bend can become oval or shift. The drawing should dimension the hole from a datum that survives forming, such as the finished end or a hole in a flat leg, and the first article should check it after the bend.

For a two-hole joint, check the pitch as well as the position. Two holes can each be within position tolerance and still be too far apart if the pitch is wrong. A functional gauge with two pins at the correct pitch is a quick way to prove the joint will assemble.

Bend angle, radius and springback

A bend angle tolerance of ±1 degree is a reasonable starting point for a formed busbar. The angle is measured on the formed leg, from a datum leg or a surface plate, not from the tool. Springback means the tool angle and the part angle are different, so the supplier has to compensate.

The radius call should be an inside radius, because that is what the tool controls and what the strain calculation uses. An outside radius call is ambiguous once the thickness tolerance is included. Give the inside radius with a tolerance and say whether it is a minimum or a nominal.

If the bend sets a joint face, the angle and the radius both matter. A part can be within angle tolerance and still have the joint face out of position because the radius is at the wrong end of its band. For a critical bend, give the angle, the radius and the leg length to the joint face, and inspect all three.

Plan the inspection with the tolerance

Every tight call needs a method. A tolerance without a method is a request for an argument at goods-in. Decide whether the feature is checked with a calliper, a pin gauge, a CMM, a fixture or a functional gauge, and put that method in the inspection plan.

For a first article, check the critical features on the actual part after forming and finishing. Record the datum, the instrument and the result. If a feature is measured on a sample rather than every part, say so. The inspection plan should also say what happens when a result is at the edge of the band: rework, concession or reject.

The Qumek first article inspection report builder can hold the feature list and the results, but the tolerance decisions still come from the assembly. Keep the drawing, the inspection plan and the first article on the same revision so the evidence matches the part.

• Give every tight call a datum and a measurement method.
• Check hole position after forming, not on the flat blank.
• Check twist in a fixture, not on a bench.
• Record the instrument and the result on the first article.
• State the general tolerance standard and class in the title block.
• Review the tolerance set when the assembly or the process changes.