Unilateral vs Bilateral Tolerance in Machining
What each tolerance type means, worked examples, when to use each for fits and general dimensions, the GD&T equivalents, and why unilateral can cost more to hold.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 8 min read
On this page
Quick Answer
Bilateral tolerance lets a dimension vary on both sides of nominal — 10 ±0.05 means 9.95 to 10.05. Unilateral tolerance lets it vary in only one direction — 10 +0.1/−0.0 means 10.00 to 10.10, never under. Use bilateral for general dimensions, and unilateral for fits and mating parts where one boundary is a hard limit. Unilateral is usually harder to hold because the process must stay entirely on one side of nominal.
The Direction of the Tolerance Matters
Most people read a tolerance as "how much can this vary" and stop there. But there is a second question that matters just as much: which direction can it vary in? Bilateral tolerance allows variation on both sides of nominal; unilateral tolerance allows it in only one direction, pinning the other side to zero. That single choice encodes the intent of the part — whether a shaft must only ever be at-or-under nominal, or a bore at-or-over. Getting it right is the difference between a drawing that describes a working fit and one that just describes a size.
The Three Callouts, Side by Side
The same nominal size, toleranced three different ways:
| Callout | Meaning | Acceptable range |
|---|---|---|
| 10 ±0.05 (bilateral, equal) | ± both sides | 9.95 to 10.05 |
| 10 +0.1/−0.0 (unilateral) | Material only | 10.00 to 10.10 |
| 10 +0.0/−0.1 (unilateral) | Metal only off | 9.90 to 10.00 |
Notice the difference between the two unilateral examples: one allows only material (bigger), the other allows only material removal (smaller). That direction is the whole point of choosing unilateral over bilateral.
Reading the Callout: Four Worked Examples
The bands above read easier as metal. Four callouts you will actually see on drawings, worked on one Ø25 bore-and-shaft pair — the same size our press fit guide uses for its H7 numbers, so the two pages read together. (The same band written as limit dimensions, 24.98/25.00, changes nothing at the machine; the notation section above covers that.)
| Callout on the drawing | What it allows | What it means at the machine |
|---|---|---|
| Ø25 +0.05/0 | Bore at-or-over nominal only: 25.00–25.05 | Aim at 25.03 and never touch 24.99. The floor is the fit boundary — this is the hole logic behind every H-class bore. |
| Ø25 0/−0.02 | Shaft at-or-under nominal only: 24.98–25.00 | Aim under nominal. Paired with the bore above, clearance is guaranteed by construction — no selective assembly, no measuring pairs. |
| Ø25 ±0.05 | Either side of nominal: 24.95–25.05 | Aim dead-on 25.00 and normal process spread passes. The cheapest band on this page to hold. |
| Position Ø0.14 (GD&T) | Round zone — versus the 0.1 square that ±0.05 coordinate gives | Same hole location, about 57% more passing area, and radial is how a drill actually misses. The corners of the square were never functional. |
Unilateral: One Side Pinned to Zero
A unilateral tolerance allows variation in only one direction, with the other side set to zero. 10 +0.1/−0.0 means the part can be 10.00 to 10.10, but never under 10.00. This is the callout for fits, clearances, and mating parts — a shaft toleranced to only ever be at-or-under nominal, mating with a bore toleranced to only ever be at-or-over, guarantees clearance by construction. Unilateral tolerance communicates that intent directly, which is why it shows up on functional features rather than cosmetic ones.
Precise bores and holes are where tolerance classes get real — see our reaming guide and thread sizes chart.
Those one-sided limits are what produce clearance and interference — see our engineering fits and press fit guides.
Bilateral: Both Sides Allowed
A bilateral tolerance splits the allowed variation on both sides of nominal. It can be equal — 10 ±0.05, giving 9.95 to 10.05 — or unequal — 10 +0.1/−0.05, giving 9.95 to 10.10. Equal bilateral is the workhorse for general dimensions, where small variation either way is harmless and the part still functions. Because it accepts normal process variation in both directions, bilateral is also the easier and cheaper tolerance to hold — the machine can land anywhere in the band and the part passes.
Limit Dimensions and the GD&T Equivalent
The same tolerance band shows up in three notations on real drawings. Plus/minus (10 +0.1/−0.0), limit dimensions (10.00/10.10), and GD&T — where unilateral and bilateral become equally disposed versus unequally disposed tolerance zones inside a feature control frame. They all describe the same allowable band; the notation is just a matter of which system the drawing uses. Our GD&T symbols guide and machining tolerances guide cover the GD&T side in depth.
Why Unilateral Can Cost More to Hold
The cost difference comes from control, not geometry. Bilateral tolerance accepts process variation on both sides, so a standard setup usually lands in the band naturally. Unilateral tolerance forces the process to stay entirely on one side of nominal — the machine cannot wander to the wrong side at all. That often means tighter control, more careful setups, and higher scrap risk, which shows up in the quote. It is not that unilateral is automatically more expensive in every job; it is that it is more demanding to hold, and demanding tolerances are where machining cost comes from. The takeaway for drawings: reserve unilateral for the fits that need it, and let general dimensions stay bilateral.
FAQ
What is the difference between unilateral and bilateral tolerance?
Bilateral tolerance splits the allowed variation on both sides of the nominal size — it can be equal (10 ±0.05) or unequal (10 +0.1/−0.05). Unilateral tolerance allows variation in only one direction, so one side is zero — 10 +0.1/−0.0 means the part can be 10.00 to 10.10 but never under 10.00. Bilateral is the general default; unilateral is used when one boundary must be protected for fit or function.
When should I use unilateral tolerance?
When one limit is a hard boundary for fit, clearance, or assembly — mating parts, shafts and holes with a specific allowance, or any feature where going under (or over) nominal breaks the assembly. For example, a shaft that must slide into a bore is often toleranced to only ever be at or under nominal, while the bore is toleranced to only ever be at or over. Unilateral tolerance expresses that intent directly.
Is unilateral tolerance harder to machine than bilateral?
Usually yes, in the sense that it demands more control. Bilateral tolerance accepts normal process variation on both sides of nominal, so hitting it is easier. Unilateral forces the process to stay entirely on one side of nominal, which often requires tighter control and can raise machining difficulty and cost. It is not automatically more expensive in every job, but it is generally more demanding to hold.
What are limit dimensions?
Limit dimensions are just the upper and lower acceptable sizes written directly instead of as a plus/minus callout — for example, 10.00/10.10 instead of 10 +0.1/−0.0. They express the same tolerance band, just in a different notation. You will see all three forms on drawings: plus/minus, limit dimensions, and GD&T symbols.
How do unilateral and bilateral tolerances appear in GD&T?
In GD&T the same concept appears as equally disposed versus unequally disposed tolerance zones. A profile or position tolerance can have its zone split evenly around nominal, or biased to one side. The principle is identical to the plus/minus version — it is just expressed through a feature control frame. Our GD&T symbols guide covers how these zones are defined.
Which tolerance type should I use on a drawing?
Use bilateral (usually equal) for general dimensions where small variation either way is acceptable. Use unilateral for mating features, fits, and clearance-critical dimensions where one boundary is a hard limit. The rule of thumb: if the part still works when the dimension wanders a little either way, bilateral is fine; if it only works when the dimension stays on one side, unilateral is the correct call.
Is ±0.1 the same as 0/+0.2?
No. The band width is identical — 0.2 in both cases — but the band sits in a different place. ±0.1 spans 0.1 below to 0.1 above nominal, while 0/+0.2 spans nominal to nominal+0.2. The middle of the band moves by a full 0.1, so a process centered for one callout fails the other half the time. At the machine, ±0.1 says aim at nominal; 0/+0.2 says aim at nominal+0.1 and never cut under nominal. Equal width is not equal meaning.
When should a unilateral tolerance be switched to bilateral?
When no fit pins either side. If over and under nominal are equally harmless — non-mating faces, clearance features, covers and brackets that touch nothing — bilateral accepts normal process spread on both sides and is the cheaper band to hold. Keep unilateral only where one boundary is functional: a mating surface, a fit floor, an assembly edge. Everything else can go bilateral, and the quote will usually agree.
Related Resources
CNC Machining Surface Finish: The Ra Chart, Explained
The CNC machining surface finish chart: Ra values in μm and μin, N1–N12 grades, what each process achieves, what…
Passivation of Stainless Steel: Process, Specs, and When Parts Need It
Passivation of stainless steel explained for machined parts: the chemistry, ASTM A967 and AMS 2700 methods, nitric…
GD&T Basics for CNC Machined Parts: The Symbols That Matter
GD&T basics for machined parts: the 14 symbols explained, feature control frames, datums, MMC bonus tolerance, true…
How to Outsource CNC Machining to China, Step by Step
How to outsource CNC machining to China, step by step: vet suppliers, compare landed cost, control quality remotely,…
Sources
Standards and references behind the numbers on this page.
- ASME Y14.5-2018 (R2024), Dimensioning and Tolerancing — the controlling standard for ± and position callouts
- Xometry, True Position Tolerance — the 57% usable-area difference between square and cylindrical tolerance zones
Tolerance Read Right, Machined Right
IsoCNC reads your unilateral, bilateral, and GD&T callouts the way they are meant — and quotes the fit, not just the number. Send the drawing; an engineer reviews every RFQ, typically within 1–2 business days.