Which tolerances make a part expensive?

Which dimension costs money and which does not?

Most dimensions on a drawing have no tolerance of their own and fall under the general tolerance in the title block. ISO 2768-1 sets out in four classes how far linear and angular dimensions without an individual tolerance may deviate. You hold them with the operation you are running anyway, at no extra cost.

The money sits in a handful of dimensions with a dimensional tolerance of their own, and only when they change the operation, the gauge or the machine. Each one is a critical dimension for your estimate, whatever the drawing calls it.

Keep features, requirements and operations apart: a plate with 32 holes, 8 of them threaded and 2 as fits. The 8 call for tapping or thread milling, the 2 for a second operation and another gauge. The other 22 ride along in the drilling cycle.

When does a tolerance change the operation?

Tolerances on linear sizes are standardised as IT tolerance grades under ISO 286: the lower the number, the tighter the band. For a bore of 6 to 10 mm, IT7 is 15 microns. H7 places that band above the nominal size: a Ø 10 H7 bore may be up to 0.015 mm over size.

Every process holds an IT tolerance grade, and that is where the route switches. For most applications a drilled bore is accurate enough. When the drawing asks for more, you drill undersize and finish by reaming: reamed holes for dowel pins hold a band of two hundredths. Single-point boring, with one cutting edge, is the other road.

Below a few hundredths boring gets harder; at a few microns it only works in shallow bores, at high cost and with every part inspected. Grinding and honing take over, and honing only pays where the form of the bore matters.

What does a tight tolerance do to inspection time?

If you cannot measure a dimension reliably, you cannot deliver it. For the general tolerance a calliper and a sample will do. A fit needs a plug gauge or a bore gauge, often on every part. A band of a few microns goes to the coordinate measuring machine (CMM), in a room held at temperature.

The reason is measurement uncertainty. Every measurement has a spread, and it has to be small next to the tolerance, or you reject good parts and pass bad ones. Metrologists use rules of thumb such as 10 to 1 or 4 to 1 between tolerance and uncertainty; the guide JCGM 106 warns that such ratios are not always clearly defined.

Temperature counts. Drawing dimensions apply at 20 °C, the reference temperature in ISO 1, so an aluminium plate still warm from the machine cannot be measured to a few microns straight away. Waiting, conditioning and a first article inspection belong in the estimate, not in the margin.

How do tolerances stack up?

A dimension that follows from a chain inherits the tolerance of every link. Three stepped dimensions of ±0.1, end to end, can leave the end dimension out by ±0.3: that is worst-case analysis, every link at its limit.

A drawing dimensioned from one datum keeps each dimension independent: you machine and measure from the same face. A chain can force you to hold the end dimension separately, in an extra setup or with tighter tolerances on every link. Check whether your setup plan keeps that datum in one setup.

Designing to the worst case gives tight tolerances, and with them expensive machining and inspection. Statistical tolerancing opens them up. That choice belongs to the customer; the bill lands with you.

Worked example: one bore, three tolerances

An example with round numbers: one Ø 10 bore in an EN AW-6082 plate, a batch of 20, the machine at € 80 an hour. At ±0.1 you drill it in half a minute. At H7 you drill undersize and ream: a minute and a half. At ±0.005 you bore in several passes and probe between the last ones on the machine: four minutes. The part then cools before it goes to the CMM.

From ±0.1 to H7 the band gets about thirteen times tighter and the bore almost four times dearer. From H7 to ±0.005 the band narrows by only a third, yet the bore costs more than three times as much. An estimate that adds a fixed mark-up per tolerance class misses every time: the price jumps at each switch, a tool, a gauge, a chance of scrap. At a grinding shop it becomes a subcontracted line with its own price.

When do you ask the customer for a wider tolerance?

Ask when the tolerance has no function you can point to. A bearing fit has one; ±0.01 on the outside of a cover plate usually does not. Tight values often come from an older drawing or a template, and nobody remembers why.

Propose it, never change it quietly. Quote the requested tolerance and the wider one side by side, naming the operation that drops out. At the design stage that costs a stroke of the pen; after release, a new revision.

Once agreed, the new tolerance goes on a new revision of the drawing, not into an email. An ERP keeps the old price, not the reason the dimension could open up. Lose the reason and the repeat order is costed tight again.

How to read the tolerances in a request

Run through these before you price a part. Every answer that adds an operation or an inspection step becomes a line in your estimate or a question for the customer.

• Which dimensions carry their own tolerance, and which ride on the general one?
• Which fits are specified, and where?
• Which gauge measures each tight dimension, and how often?
• Are dimensions given from one datum or as a chain?
• At what temperature do the dimensions apply, and can you measure there?
• Which tight tolerance looks copied from an older drawing?