GD&T Straightness: Surface vs Axis Tolerance Explained
One straightness symbol (—), two very different controls — line elements on a surface, or the derived median line of a feature of size with the ⌀ modifier and MMC bonus tolerance.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 15 min read
On this page
Quick Answer
In GD&T, straightness (symbol —) is a form tolerance that never references a datum. It works in two distinct ways. Surface straightness controls individual line elements on a surface: each measured line must fit between two parallel lines separated by the tolerance value. Axis straightness applies to a feature of size — a pin, shaft, or hole — and is marked with the ⌀ modifier in the feature control frame: the derived median line of the feature must fit inside a cylindrical zone of the stated diameter. The ⌀ version overrides Rule #1, so the straightness tolerance may exceed the size tolerance, and when Ⓜ (MMC) follows the value, the feature earns bonus tolerance as its actual size departs from maximum material condition — guaranteeing assembly at the worst-case virtual condition boundary.
What the Straightness Symbol Controls
The straightness symbol is a single horizontal line (—) drawn in the first compartment of a feature control frame, followed by the tolerance value. It belongs to the form family of GD&T controls — alongside flatness, circularity, and cylindricity — which means it governs shape only. A straightness callout never contains a datum letter. If a datum appears in the frame, the control is something else entirely, usually position or an orientation tolerance, and it behaves under different rules. For the full symbol vocabulary, see our GD&T symbols explained reference.
What makes straightness unusual is that one symbol encodes two different requirements depending on how the frame is attached to the drawing. Placed with a leader pointing at a surface — or under a dimension that is not a size dimension — it controls line elements of a surface. Placed under the size dimension of a feature of size (a pin, shaft, boss, or hole) with the diameter symbol ⌀ before the tolerance value, it controls the derived median line of that feature — what machinists loosely call axis straightness. Same symbol, different tolerance zone shape, different verification method, and different relationship to the size tolerance. Reading which one the drawing means is the first skill; getting it wrong produces a tolerance zone with the wrong shape and an inspection plan that cannot work.
Straightness also sits downstream of the size dimension and interacts with Rule #1, the envelope principle that a feature of size may not violate a perfect-form boundary at maximum material condition. Our GD&T basics for CNC machining guide covers that vocabulary; the rest of this article assumes it.
Surface Straightness: Line Elements, Not the Whole Surface
Surface straightness is the simpler of the two forms. The tolerance zone is two parallel lines separated by the tolerance value, and each line element of the controlled surface — taken in the direction shown in the view where the callout is placed — must lie between those two lines. On a cylindrical surface the elements run parallel to the axis, which is why surface straightness is the standard way to control bow or taper along a turned shaft without invoking anything fancier. On a flat face, the elements are straight lines across the surface in the indicated direction; callouts in two views control both directions independently.
Two properties follow directly. First, surface straightness is evaluated element by element: neighboring lines can tilt, step, or drift relative to each other as long as each one is individually straight. A surface could be gently twisted and still pass. That makes it cheaper to meet than flatness, and also weaker — choose it when only one direction of deviation matters to function. Second, because the callout has no ⌀ modifier, Rule #1 still applies: the size tolerance keeps governing the overall form envelope, so the straightness value must be smaller than the size tolerance and adds a refinement, not an override. It is a tightening of what size already controls, never a relaxation.
Typical uses: a guide rail swept with a dial indicator, a long turned shaft where bow would cause vibration, a plate edge that locates against a fence — in each case only one direction of deviation matters, and paying for flatness or cylindricity would buy control nobody needs. For how straightness values fit into an overall tolerance scheme, see CNC machining tolerances.
Axis Straightness: The ⌀ Modifier, Rule #1 Override, and MMC Bonus
Axis straightness — feature-of-size straightness — is where the callout earns its keep. The frame is attached to the size dimension of a pin, shaft, or hole, and the tolerance value carries the ⌀ modifier: the tolerance zone becomes a cylinder whose diameter is the stated value, and the derived median line of the feature must stay inside it. The derived median line is the line you get by connecting the centers of infinitely many cross sections measured along the feature — it captures the actual bow of the part, independent of local diameter variation.
This form of the callout deliberately overrides Rule #1. The feature may locally exceed the perfect-form envelope at MMC, because what the designer cares about is the boundary the feature presents to its mating part. That has two practical consequences. First, the straightness value may be larger than the size tolerance — a legitimate and common design choice when bow matters more than local diameter. Second, adding the Ⓜ modifier ties the requirement to maximum material condition and unlocks bonus tolerance: as the feature’s actual mating envelope departs from MMC, it gains an equal amount of additional straightness tolerance. The constant through all of it is the virtual condition boundary — the worst-case outline the mating part must clear: MMC plus the straightness value for an external feature (shaft), MMC minus the straightness value for an internal feature (hole).
| Actual Mating Envelope Size (mm) | Bonus Tolerance (mm) | Total Allowable Axis Straightness (mm) |
|---|---|---|
| ⌀20.10 (at MMC) | 0.00 | ⌀0.05 |
| ⌀20.08 | 0.02 | ⌀0.07 |
| ⌀20.05 | 0.05 | ⌀0.10 |
| ⌀20.00 (at LMC) | 0.10 | ⌀0.15 |
The example shows why designers reach for Ⓜ: every micrometer the shop holds under the size limit converts directly into extra form tolerance, so conforming parts assemble regardless of where they land in the size range. The shaft in the table always clears a ⌀20.15 mm boundary, which is exactly what the mating hole is sized around. This is the same bonus-tolerance arithmetic that applies to position at MMC — straightness is simply the form-level version of it.
Straightness vs Flatness vs Cylindricity
Engineers most often confuse straightness with its two form-control neighbors. Flatness is the area-level version of surface straightness — two parallel planes containing an entire surface — while cylindricity is the composite form control for a cylinder, simultaneously constraining roundness, straightness, and taper of the whole surface. Neither is interchangeable with straightness, and each costs more to achieve and to verify.
| Control | Applies To | Tolerance Zone | Datum? | Typical Verification |
|---|---|---|---|---|
| Straightness (surface) | Individual line elements of a flat or cylindrical surface | Two parallel lines separated by the tolerance value | Never | Straightedge and feeler gauge, dial indicator or height gauge sweep |
| Straightness (feature of size) | The derived median line of a pin, shaft, or hole | A cylinder whose diameter equals the tolerance value (⌀ modifier) | Never | CMM derived-median-line evaluation, functional ring or plug gauge at virtual condition |
| Flatness | An entire planar surface | Two parallel planes separated by the tolerance value | Never | Surface plate sweep, CMM point cloud |
| Cylindricity | The entire surface of a cylinder | Two coaxial cylinders separated by the tolerance value | Never | Roundness tester or CMM scanning |
The decision rule is functional. If only one direction of deviation matters — bow along a rail, bend along a shaft — straightness is sufficient and cheap. If the whole face seals, locates, or slides, specify flatness. If a cylindrical surface must stay uniformly round and straight over its full length for a precision bearing or sealing fit, the control is cylindricity — expensive, and worth it only on genuinely critical fits. Our GD&T cylindricity guide covers that callout and its measurement in detail.
How Straightness Is Measured
Verification splits along the same line as the callout itself. Surface straightness is shop-floor friendly. For loose tolerances, a precision straightedge laid on the surface with feeler gauges slipped under it gives a direct reading of the maximum gap. For tighter work, the part sits on a surface plate — cylindrical parts in V-blocks or between centers — and a dial indicator or height gauge sweeps along the controlled line element; the total indicator variation must stay within the tolerance value. Optical methods (laser alignment systems, autocollimators) handle long beds and machine-tool ways where a straightedge is impractical.
One caveat: a dial reading over a rotating shaft in V-blocks measures total indicator reading (TIR), which mixes straightness error with roundness error. It is a good shop proxy, but not a straightness measurement in the Y14.5 sense, and parts can dispute at the borderline.
Axis straightness cannot be read off the surface at all, because it governs the derived median line. The rigorous method is a CMM: the probe measures many cross sections along the feature, the software computes the center of each, and the resulting median line is evaluated against a cylindrical zone of the tolerance diameter. For production pass/fail on MMC callouts, the faster instrument is a functional gauge — a ring gauge for a shaft or a plug gauge for a hole, made at the virtual condition size. If the part enters the gauge, it assembles; that is the entire question the Ⓜ callout was written to answer. Our tolerance and inspection capability page covers the CMM and gauging equipment we use to verify these callouts.
When to Specify Axis Straightness (and When Not To)
Reach for feature-of-size straightness at MMC whenever the function of the part is assembly. Dowel pins, hinge pins, shafts sliding in bushings, pistons in bores, fastener shanks through clearance holes — in every case the failure mode is a part that measures in tolerance at every cross section yet will not assemble because its axis bows. The Ⓜ callout solves it economically: the mating features are sized around the virtual condition boundary, and the shop gets to trade size for form, holding whichever is easier. It is especially valuable on long slender turned parts, where some bow is physically inevitable and polishing local diameter to compensate is wasted money.
Skip it when the feature is short (L/D near or below 1, where bow is negligible), when Rule #1’s default envelope already protects the fit, or when the real requirement is orientation or location — a pin that must be perpendicular to a face needs perpendicularity or position, not straightness. And avoid stacking tight values reflexively: like all geometric tolerances, straightness costs metrology time, and an unnecessarily fine number on a non-critical feature raises piece price without buying function. A good rule of thumb is to start from the assembly math — worst-case clearance divided between the mating features — and tighten only where the budget demands it.
If you are adding GD&T to production drawings, the symbols reference and tolerancing guide in this cluster cover the surrounding framework, and our engineering team reviews callouts on every quote — flagging controls that are over-tight, unmeasurable, or cheaper expressed another way.
FAQ: GD&T Straightness
What does the straightness symbol mean in GD&T?
The straightness symbol is a short horizontal line (—) placed in the first compartment of a feature control frame. It is a form tolerance, meaning it controls the shape of a feature only — never its location or orientation — and it never references a datum. Read two ways, it either limits how much individual line elements of a surface may deviate from a perfect line, or, when the diameter symbol ⌀ precedes the tolerance value on a feature of size, it limits how much the axis or derived median line of a pin, shaft, or hole may bow or bend within a cylindrical zone of the stated diameter.
What is the difference between surface straightness and axis straightness?
Surface straightness applies to individual line elements on a surface — on a cylinder, lines parallel to the axis; on a flat face, lines in the direction shown. Each line element must fit between two parallel lines separated by the tolerance value, and the surface itself stays bound by the Rule #1 size envelope. Axis straightness applies only to a feature of size and carries the ⌀ modifier: the derived median line of the whole feature must fit inside a cylindrical zone. Because it overrides Rule #1, the tolerance can exceed the size tolerance, and with Ⓜ it earns bonus tolerance as the feature departs from MMC.
Can a straightness tolerance be larger than the size tolerance?
Yes — but only when the callout is applied to a feature of size with the ⌀ modifier. Normally, Rule #1 of ASME Y14.5 says the size tolerance alone controls form: a perfect-form boundary at MMC that the surface cannot violate. A straightness callout with ⌀ overrides that envelope requirement, so the axis is allowed to bow by the full stated value even if that pushes material outside the size limits at a local cross section. This is the standard way to toleranced a shaft or pin whose assembly function depends on axis bow more than on local diameter. Without ⌀, straightness can never exceed the size tolerance.
Does a straightness callout use a datum?
No. Straightness is a pure form control and never references a datum — if you see a datum letter in the frame, the callout is a different control entirely (most likely position or an orientation tolerance). Straightness only says how straight a line element or a derived median line must be relative to its own ideal geometry; it says nothing about where that feature sits on the part. If you need to control both form and location — for example, a dowel pin that must be straight and in position — you stack two frames: straightness (optionally at MMC) above, and position relative to datums below.
How is straightness measured?
Surface straightness is checked with a straightedge and feeler gauges for loose tolerances, or with a dial indicator or height gauge sweeping along the controlled line element on a surface plate — the total indicator variation must stay within the tolerance value. Axis straightness is harder, because it governs the derived median line rather than the visible surface: a CMM probes many cross sections, computes the center of each, and fits the resulting line inside a cylindrical zone. For production pass/fail at MMC, a functional gauge — a ring gauge for shafts, a plug gauge for holes, sized at virtual condition — confirms assembly directly.
What is the difference between straightness and flatness?
Straightness controls line elements one at a time: each measured line on the surface must individually fall within two parallel lines. Flatness controls the entire surface at once: every point must fall between two parallel planes separated by the tolerance value. A surface can pass straightness in one direction while being twisted or dished — it would fail flatness — because straightness says nothing about how neighboring lines relate to each other. Flatness is therefore the stronger, more expensive control and is common on sealing faces and datum surfaces, while straightness suits long edges, rails, and cylindrical features where only one direction matters.
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,…
Straightness Callouts on Your Drawing? Send It Over.
IsoCNC machines precision shafts, pins, bores, and guide features to GD&T prints every day — with CMM verification of derived-median-line straightness, functional gauging at virtual condition, and full inspection reports on every lot. An engineer reviews every drawing, typically within 1–2 business days.