Guide
Parallelism in GD&T vs flatness: which does a sealing or mounting face need?
Flatness is a form tolerance that limits how far a single surface may depart from a perfect plane, judged on its own with no datum. Parallelism is an orientation tolerance that does the same job and one more: it holds the surface between two planes that must also be parallel to a datum, so a parallelism GD&T callout always points at another feature of the part.
By Saola Manufacturing engineering team · Published · Updated
Designers mix the two up in both directions. Some put parallelism on a gasket face that only needs to be flat, which forces a datum, a fixture and a slower inspection for no functional gain. Others put flatness on a spacer whose two faces must agree, and then wonder why a part that passed inspection tilts the assembly. This guide covers the tolerance zones, the datum question, how each control is measured, and a decision rule for sealing and mounting faces. Both controls are defined in ASME Y14.5-2018 and in ISO 1101:2017; only their public descriptions are paraphrased here.
On this page
How do the flatness and parallelism tolerance zones differ?
Both zones are two parallel planes separated by the tolerance value, and the surface must lie between them. The flatness zone may float to any angle and any height, while the parallelism zone is locked parallel to the datum plane and may only move up and down.
That single difference explains everything else. Because the flatness zone can tilt freely, it measures only the shape of the surface: bow, twist, waviness and local high spots. A face can be perfectly flat and still sit at an angle to the rest of the part. Because the parallelism zone is tied to a datum, it measures shape plus tilt relative to that datum. A face that is flat but tilted fails parallelism; a face that is parallel is automatically flat to at least the same value. The one exception is a parallelism frame carrying the ASME tangent plane modifier, which checks only the plane resting on the high points and so leaves form uncontrolled.
Neither control fixes where the face sits. The distance between two faces, for example the thickness of a spacer, is still controlled by a size or location dimension. The parallelism zone floats inside those size limits; it does not replace them.
The hierarchy on a single face is therefore size or location first, orientation second and form last, and each refinement is only worth adding if it is tighter than the control above it. Under the ASME envelope principle (Rule #1), a feature of size such as a plate thickness already limits form at maximum material, so a parallelism or flatness callout between those two faces only does something if its value is smaller than the size tolerance. ISO drawings work on the independency principle of ISO 8015:2011 by default, so there the size tolerance does not control form unless the envelope symbol is added, and an explicit flatness or parallelism callout matters more.
Why does parallelism need a datum and flatness never takes one?
Parallel means parallel to something, so a parallelism frame must name a datum, usually a flat face labeled A. Flatness describes one surface in isolation, so a datum letter in a flatness frame is an error under both ASME and ISO rules.
In practice the datum choice is where most parallelism callouts go wrong. The datum should be the face the part actually rests on or bolts against in the assembly, because that is the plane the function is measured from. If the drawing picks a convenient machined face instead, the part can pass inspection and still sit crooked in service.
A datum face also inherits a quiet requirement: its own form. When the datum is a rough or bowed surface, the inspector has to decide how to rest it on the plate, and two shops will get two answers. The usual fix is a flatness callout on datum A itself, sized tighter than the parallelism value on the controlled face. Datum establishment rules, including how a datum feature is simulated by a surface plate, are covered by ASME Y14.5 and by ISO 5459:2024. The guide to datums on cast parts covers datum choice when the part starts as a casting.
What flatness and parallelism apply when the drawing gives no callout?
ASME Y14.5 sets no default flatness or parallelism, so unless a general note adds one, an unspecified face is limited only by its size dimension and Rule #1, which gives no form limit at all to a face that is not part of a feature of size. On an ISO drawing with a general note such as ISO 2768-mK, the K class sets a default flatness, and the default parallelism follows from it.
Per ISO 2768-2, the general parallelism tolerance equals the size tolerance or the flatness tolerance, whichever is greater, with the longer of the two features taken as the datum. The flatness values in the table below grow with the length of the surface, which is why a general note can be loose on a large plate and quite reasonable on a small bracket. ISO 2768-2 has been withdrawn and replaced by ISO 22081:2021, but the “mK” note remains common on drawings, so it is worth knowing what it implies. If a face seals or locates, do not lean on the general note: give it its own frame.
| Nominal length (mm) | Class H (mm) | Class K (mm) | Class L (mm) |
|---|---|---|---|
| up to 10 | 0.02 | 0.05 | 0.1 |
| over 10 to 30 | 0.05 | 0.1 | 0.2 |
| over 30 to 100 | 0.1 | 0.2 | 0.4 |
| over 100 to 300 | 0.2 | 0.4 | 0.8 |
| over 300 to 1000 | 0.3 | 0.6 | 1.2 |
| over 1000 to 3000 | 0.4 | 0.8 | 1.6 |
How are flatness and parallelism measured?
Parallelism is the simpler check: rest the datum face on a surface plate and sweep an indicator across the controlled face, and the total indicator movement is the parallelism error. Flatness needs the tilt removed first, by leveling the part on adjustable supports or by fitting planes to measured points, because the zone is not tied to anything.
The most common inspection mistake follows directly from that difference. An inspector who lays a part on the plate with its opposite face down and sweeps the top face has measured parallelism of the top face to the bottom face, not flatness of the top face. If the bottom face is bowed or the part rocks, that reading can be far larger than the true flatness error, and a good part gets rejected. The reverse error also happens: a thin part pressed flat against the plate by its own weight or by a clamp reads better than it is in the free state.
Methods you will see on inspection reports:
- Surface plate and indicator, part on three jacks. The part is leveled until three reference points read the same, then the face is swept. The total reading approximates flatness; it is not exactly the minimum-zone value but is the usual shop check.
- Surface plate and indicator, datum face down. The plate simulates datum A. The total indicator movement over the controlled face is the parallelism error. Use the ASME tangent plane modifier if only the high points should count.
- Coordinate measuring machine. Points are probed and a plane is fitted. The standards define flatness by the minimum zone, two parallel planes as close together as possible; a least-squares fit reports a slightly different number, so ask which fitting method the report uses when results are close to the limit.
- Optical flat. Used for small, lapped faces such as seal rings, where interference fringes show form errors far below what an indicator can resolve.
Point density matters with every method. A sweep along two diagonals and the edges finds bow and twist; a sparse grid can miss a local dip at a bolt hole. If a dip at one location is what causes leaks, say so on the drawing or the inspection plan.
Which control does a sealing face or a mounting face need?
A face that seals against a gasket or O-ring usually needs flatness only, because the seal cares about gaps across the face, not about the angle to anything else. A face whose angle to another feature drives the function, such as both faces of a spacer or a rail seat that must match its base, needs parallelism to a datum.
A quick decision rule:
- Gasket or O-ring face on a cover or flange. Flatness. The mating part is also free to sit at whatever angle the bolts pull it to, so tilt is absorbed. Size the value from the seal manufacturer’s data for the gasket type and clamp load, not from habit.
- Mounting face that is the primary datum. Flatness on that face, labeled datum A, because everything else on the part is measured from it.
- Second face that must stay level with datum A. Parallelism to A, for example the top of a spacer, shim or riser block, a bearing seat on a housing that bolts down on A, or a machine-tool way pad.
- Face that must be square to a bore or shaft. Neither one. That is perpendicularity to the axis, or total runout on a turned face; see the runout guide.
- Large face where local dips matter more than overall bow. Flatness per unit area on top of an overall value, for example a looser value over the whole face and a tighter value over any small square.
Over-specifying in either direction costs real money. Parallelism on a face that only seals adds a datum, a fixture plan and often a dedicated setup to machine both faces in a known relationship. Flatness alone on a spacer lets two flat but wedge-shaped faces pass, and the wedge shows up as a tilted assembly.
How should the callout look on the drawing?
A flatness frame carries the symbol and a value and nothing else. A parallelism frame carries the symbol, a value and a datum letter, and the datum feature must be identified with a datum symbol somewhere on the drawing.
Typical patterns for a cover that seals on one face and bolts down on the other:
- Seal face: ⏥ 0.05, with the value chosen from the seal data, no datum.
- Bolt-down face: datum symbol A, plus ⏥ 0.03 if A must be a stable datum.
- Top face of a spacer: ∥ 0.02 | A, and a flatness frame on A tighter than the parallelism value.
- Large plate: ⏥ 0.1 overall, with a second line limiting flatness per unit area over any small square, so a local dip at a fastener is caught.
Common mistakes to remove before the drawing goes out:
- A datum letter in a flatness frame. It is not valid, and a supplier will either ignore it or call to ask which one you meant.
- Parallelism and flatness on the same face with the same value. The flatness line does nothing, because parallelism already limits form to that value (unless the parallelism frame uses the tangent plane modifier).
- Flatness or parallelism looser than the size tolerance between the same two faces under ASME Rule #1. The callout is redundant.
- No note on coating. Anodize, plating or powder coat add thickness unevenly, so state whether the value applies before or after finishing.
- No free-state or restrained-state note on a thin part that will be bolted flat in assembly. If the function is measured bolted down, say so and describe the restraint.
What should a flatness or parallelism requirement include on an RFQ?
Send the drawing with each frame tied to a clearly identified face, the datum feature named, the state of the part at inspection, and whether the value applies before or after finishing. With those four items, a quote and an inspection plan can be built from the drawing alone.
Add three things that a drawing rarely shows. First, which faces actually seal or locate, so the shop knows where the tight values earn their cost. Second, how the part will be held in your assembly, because a part that is checked free and used clamped is being judged on the wrong condition. Third, which inspection method you expect on the report, surface plate or coordinate measurement, so both sides read the same number.
On machined parts, flatness and parallelism on related faces are decided largely by how the part is set up and how much stress is released when material comes off. Locating on datum A when the controlled face is cut, from a single consistent datum scheme, is what keeps parallelism in check. Saola’s CNC milling cell machines datum faces flat for downstream assembly on die-cast and sand-cast parts, and the milling page notes that every GD&T call-out gets measured and logged. On the quality page, the first article is measured against every toleranced dimension, and you can mark the control dimensions on your drawing so the inspection is built around them. To check a specific face, send the drawing for a quote.
Frequently asked
Does parallelism control flatness?
Yes, in the plain case. Because the whole surface must lie inside the parallelism zone, its form error cannot exceed the parallelism value. A separate flatness callout on the same face is useful only if it is tighter. If the frame carries the ASME tangent plane modifier, only the contacting plane is checked, and flatness needs its own callout.
Does flatness control parallelism?
No. Flatness has no datum, so a face can be perfectly flat and tilted to every other feature. An orientation or profile control to a datum, or a size dimension between two opposed faces, is what limits that tilt.
Can parallelism apply to a hole or a shaft?
Yes. Parallelism can be applied to an axis or a median plane as well as a surface, for example a bore axis parallel to a mounting face. When applied to a feature of size, a material condition modifier may also be used under ASME Y14.5.
Is flatness the same as a surface finish callout?
No. Surface roughness measures the fine texture left by the tool over a short sampling length, while flatness measures the overall shape of the face. A gasket face often needs both; see the surface roughness guide.
Why did my part pass flatness at the supplier and fail at incoming inspection?
Usually the two sides used different methods: one leveled the part and the other rested it on the opposite face, which measures parallelism. Coating added after the check, or a free-state versus clamped difference, are the next things to compare.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)
- ISO 1101:2017, GPS — Geometrical tolerancing — Tolerances of form, orientation, location and run-out, ISO, 2017
- ISO 5459:2024, GPS — Geometrical tolerancing — Datums and datum systems, ISO, 2024
- ISO 8015:2011, GPS — Fundamentals — Concepts, principles and rules, ISO, 2011
- ISO 2768-2:1989, General tolerances — Part 2: Geometrical tolerances for features without individual tolerance indications, ISO, 1989 (withdrawn)
- ISO 22081:2021, GPS — General geometrical specifications and general size specifications, ISO, 2021