What Is a Tolerance Stack-Up?

Every dimension on an engineering drawing has a tolerance -- a range of acceptable variation. A hole might be called out as 0.500" ±0.005", which means any finished hole between 0.495" and 0.505" is acceptable. That range exists because no manufacturing process produces a perfect part every time, and designing to an exact size with zero tolerance is not practical or necessary for most applications.

The problem is that tolerances do not exist in isolation. Parts mate with other parts. Holes line up with shafts. Faces seat against faces. When you have multiple dimensions in a chain -- each with its own tolerance band -- those tolerances add up. That accumulation is a tolerance stack-up, and it is one of the most common ways a design that looks correct on a drawing fails in production.

The basic idea with a shaft and hole

Here is the simplest version. You have a shaft and a hole that need to fit together with a small clearance.

The shaft is designed at 0.495" with a tolerance of ±0.005". That means the shaft can be anywhere from 0.490" to 0.500".

The hole is designed at 0.500" with a tolerance of ±0.005". That means the hole can be anywhere from 0.495" to 0.505".

At designed size, the shaft is 0.005" smaller than the hole. There is 0.0025" of clearance all around the shaft -- tight, but it goes together.

Now consider the worst case. The shaft is made at its maximum allowable size: 0.500". The hole is made at its minimum allowable size: 0.495". Both parts are within tolerance. Both parts would pass inspection. But the shaft is now 0.005" larger than the hole. It will not go in. The assembly fails.

Neither part is defective. The design did not account for what happens when both parts are at their worst-case ends of the tolerance band at the same time.

Size is only half of it -- position matters too

Most engineers who are new to tolerance analysis look at size and stop there. That misses the other half of the problem.

Consider two parts that each have a hole. A shaft at 0.490" needs to pass through both holes at the same time. Each hole is sized at 0.500" ±0.005" -- plenty of clearance on size alone.

But each hole also has a position. Both holes are dimensioned at 2.000" ±0.005" from Edge A and 1.000" ±0.005" from Edge B.

In the worst case, one hole is at 2.005" from Edge A and 1.005" from Edge B. The other hole is at 1.995" from Edge A and 0.995" from Edge B. Both parts are within tolerance. Both pass inspection. But the two holes are now 0.014" apart from each other -- the diagonal distance between (2.005, 1.005) and (1.995, 0.995). The 0.490" shaft will not pass through both holes simultaneously.

The size was fine. The position stack-up is what killed the assembly.

Where else stack-ups cause problems

Shaft-and-hole fits are the easy example, but stack-ups show up in every type of assembly.

Press fits and bearing fits. A press fit depends on an interference between a shaft and a bore -- the shaft is intentionally larger than the hole by a controlled amount. If the tolerance band is too wide, the worst-case low end of the interference becomes a clearance fit. The bearing spins in the housing instead of pressing in. At the other extreme, the worst-case high end becomes an interference so tight that you crack the housing pressing it in.

Coatings and surface treatments. Anodizing, Cerakote, electroless nickel, and similar coatings add material to every coated surface. If a bore gets coated, the bore shrinks. If a shaft gets coated, the shaft grows. Those changes are small -- typically 0.0005" to 0.002" per surface -- but they stack directly onto the existing dimensional tolerances. A fit that had 0.002" of clearance can come back from the coating shop at zero clearance or interference, with every individual part still technically in spec.

Assemblies with multiple parts in a chain. The more parts in a chain, the wider the worst-case stack. If you have five parts each contributing ±0.005" of variation in a single direction, the worst-case stack at the end of that chain is ±0.025". A gap that was designed at 0.030" could be as small as 0.005" or as large as 0.055" in production. Whether that is acceptable depends entirely on what that gap is doing.

The most common mistake

The most common thing I see when reviewing a design with a stack-up problem: the engineer checked whether the parts fit at nominal size and stopped there. They confirmed that a 0.495" shaft fits a 0.500" hole and moved on. Nobody asked what happens when the shaft is 0.500" and the hole is 0.495".

The second most common mistake is not accounting for position at all. Designers dimension holes from edges and assume the position is controlled by the dimension. It is not -- the dimension has a tolerance, and that tolerance contributes to the stack just like the size tolerance does. GD&T positional controls exist specifically to handle this more rigorously, but even a basic worst-case analysis using the dimension tolerances directly is better than nothing.

How to fix a stack-up problem

There are two levers. You use one or both depending on what is practical.

Tighten the tolerances. Narrowing the tolerance band on one or more parts in the chain reduces the worst-case stack. A hole at 0.500" ±0.001" instead of ±0.005" is much less likely to create an interference with a shaft at 0.495" ±0.005". The tradeoff is cost -- tighter tolerances mean slower machining, more careful setups, and higher scrap rates. Tighten only what actually needs to be tighter, not every dimension in the chain.

Change the nominal dimensions. If the tolerance bands are appropriate for the manufacturing process, the other option is to adjust the designed sizes so that even the worst-case stack leaves acceptable clearance or interference. Instead of designing the shaft at 0.495" and the hole at 0.500", you might design the shaft at 0.490" and the hole at 0.500". The nominal clearance is now 0.010". The worst case is still 0.000" -- but you are no longer in interference, just a line-to-line fit.

In practice, fixing a real stack-up problem usually involves both: reviewing which dimensions are driving the worst-case scenario, adjusting those nominal values to open up the margin, and tightening tolerances only where the function genuinely requires it.

When to do the analysis

A tolerance stack-up analysis is most useful -- and cheapest -- at the design stage, before any parts are cut. Once you have production tooling, changing a nominal dimension or tightening a tolerance on a machined feature means retooling. That cost is measured in thousands of dollars and weeks of delay, not hours and drawing revisions.

If you are within a month of sending files to a manufacturer and have not walked through the worst-case stack on your critical fits, that is the time to do it. A DFM review that includes stack-up analysis is one of the better ways to spend engineering budget before a production run.