Form Tolerances
Flatness, straightness, circularity and cylindricity: what each controls, Rule #1, how to choose and how to inspect them, with worked examples.
Form tolerances control the shape of a single feature on its own: how flat a surface is, how straight a line or axis is, how round a section is, and how cylindrical a cylinder is. They are the simplest geometric controls and the only ones that never use a datum. This page covers all four, the rule that links size and form (Rule #1), how to choose between them, how each is inspected, and worked examples with numbers. It is part of the GD&T guide and follows ASME Y14.5-2018, with ISO differences noted.
What form tolerances do
| Symbol | Characteristic | Zone | Applies to | Datum? |
|---|---|---|---|---|
| Flatness | Two parallel planes t apart | A flat surface, or the derived median plane of a feature of size | No | |
| Straightness | Two parallel lines t apart (a flat view), a cylinder ⌀t (an axis), or two parallel planes (a median plane) | Line elements of a surface, or the derived median line of a feature of size | No | |
| Circularity | Two concentric circles t apart (radially) in each cross-section | A circular cross-section of a cylinder, cone or sphere | No | |
| Cylindricity | Two coaxial cylinders t apart (radially) | A whole cylindrical surface | No |
- No datum: the feature is checked against its own best shape, wherever it sits on the part. That is why form tolerances are inspected without a datum reference frame.
- A form tolerance is a refinement. It must be smaller than the size tolerance of the feature (and, for a diameter, you should aim well inside half of it, because circularity and cylindricity are measured on the radius and size on the diameter).
- Form is also limited by orientation, location and profile. A flatness tolerance on a surface and a parallelism tolerance on the same surface both apply, and the flatness has to be smaller than the parallelism tolerance, because parallelism already contains flatness.
Rule #1: size controls form
Before any form symbol is added, ASME Y14.5 gives every feature of size (a pin, shaft, hole, slot, tab) a built-in form limit called Rule #1, or the envelope principle:
- At its maximum material condition (MMC) a feature of size must have perfect form. A shaft whose largest allowed size is ⌀10.10 must fit inside a perfect ⌀10.10 envelope; a hole with a smallest size of ⌀10.00 must accept a perfect ⌀10.00 gage.
- Away from MMC, form can vary, but the whole surface must stay inside the MMC envelope, and no local size may fall outside the limits of size.
Largest allowed axis deviation (diametral zone) = MMC size − actual size (for a shaft)
Largest allowed axis deviation (diametral zone) = actual size − MMC size (for a hole)
Where Rule #1 does not apply
- Stock such as bar, sheet, tube and structural shapes made to their own standards (mill tolerances rather than the drawing).
- Parts marked “perfect form at MMC not required”, or with the independency symbol Ⓘ on the size.
- Flexible parts in the free state, and features that are not features of size (a plain flat surface, for example, has no envelope).
- ISO is different. ISO 8015 assumes the independency principle by default: size and form are checked separately, and the envelope applies only if the drawing adds the Ⓔ symbol. A drawing to ISO therefore needs explicit form tolerances where ASME would rely on Rule #1.
Flatness
Flatness says how much a surface may deviate from a plane. The tolerance zone is the space between two parallel planes t apart, and the entire surface has to lie in it. The zone floats: it can tilt and move to enclose the surface in the best way, so no datum is needed.
- How it is written. The feature control frame is attached to the surface by a leader or to its extension line, with no ⌀ and no datum: | ▱ | 0.05 |.
- Per unit area. A second compartment can limit local waviness on top of the overall limit, for example 0.05 overall and 0.01 on any 25 × 25 mm area. This stops a surface that is “flat overall” but rippled.
- Flatness of a derived median plane. When the frame is attached to the dimension of a width (a slot or tab), it controls the center plane of the feature, which can be flat even when each face is not. Add Ⓜ to allow bonus tolerance.
- Limits. Flatness must be less than the size tolerance. The size limits still apply to every point of the surface.
- Typical uses: sealing and gasket faces, mounting faces, bearing surfaces, surface plates, machine ways, datum features (a flat primary datum gives a stable set-up).
Straightness
Straightness has two different meanings, and which one applies depends on where the frame is attached.
| Frame attached to… | What is controlled | Zone | Written as |
|---|---|---|---|
| A surface (leader to the line in the view) | Every line element of the surface in the direction of the view | Two parallel lines t apart, in the plane of the view | | — | 0.02 | |
| The size dimension of a cylinder | The axis of the feature (its derived median line) | A cylinder of diameter t | | — | ⌀0.05 | (the ⌀ is required for an axis) |
| The size dimension of a width | The center plane of the feature | Two parallel planes t apart | | — | 0.05 | |
- Surface elements is the control for a rail, a guide bar or the edge of a tube: each line along the length must stay within the zone, so the surface cannot be dished or bowed.
- An axis is the control for a shaft or pin that must pass through a long bore, or a rod that must not bow. The zone is a cylinder and its size can grow with Ⓜ (bonus tolerance).
- Per unit length. A second compartment can limit the bend over a short length: for example 0.05 over the whole part and 0.01 over any 25 mm. A long slender part that is acceptable overall can still have a sharp kink.
- Straightness vs Rule #1. When Rule #1 applies, straightness of the axis is already limited by the size tolerance. An explicit straightness tolerance only helps when it is tighter than Rule #1 at the sizes where it matters (see Example 3 below).
Circularity (roundness)
Circularity controls the shape of a single cross-section of a round feature. At each section perpendicular to the axis (or to the center line of a cone), the outline must lie between two concentric circles whose radii differ by t. Each section is checked on its own, and the circles can be different from one section to the next.
- Radial, not diametral. A circularity of 0.01 means the radius changes by 0.01 at most around the section, so the diameter measured at different angles can differ by up to 0.02.
- Applies to cylinders, cones and spheres (a sphere is checked in every plane through its center).
- Lobing. A part can have a constant diameter and still not be round (a three-lobed shape from centerless grinding is the classic case). A caliper or micrometer cannot see it, and the part will not roll or fit as a round part should. Use a roundness tester, or a V-block set-up that is designed to find odd lobes.
- Typical uses: bearing journals, seal surfaces, piston bodies, valve stems, thin rings that distort when clamped.
Cylindricity
Cylindricity controls the whole cylindrical surface at once. The zone is the space between two coaxial cylinders t apart, and the entire surface must lie inside it. It combines circularity, straightness of the surface elements and taper into a single requirement.
- It is a bigger control than circularity. Every cylindricity tolerance already limits circularity to the same value, so you would only add a separate circularity tolerance when it is smaller than the cylindricity tolerance.
- Cylinders only. Cylindricity does not apply to cones, spheres or other shapes.
- It is demanding and costly to inspect (a roundness tester measuring several levels, or a scanning CMM). Use it when the whole surface has to be a good cylinder, for example the bore of a hydraulic cylinder or a sleeve for a seal, and use circularity (or plain size) elsewhere.
- Typical uses: honed bores, hydraulic and pneumatic cylinder tubes, piston pins, precision shafts.
Choosing a form control
| The need | Use | Why |
|---|---|---|
| A sealing or mounting face must touch evenly | Flatness | Controls the whole surface; add a per-area limit for waviness |
| A long rod or shaft must pass through a bore without binding | Straightness of the axis (⌀t) | Controls the bow of the axis, not the surface finish |
| A guide rail’s edge must be true along its length | Straightness of surface elements | Controls each line along the surface |
| A bearing seat must be round at every section | Circularity | Cheaper than cylindricity, since sections are independent |
| A honed bore must be a good cylinder from end to end | Cylindricity | Controls roundness, straightness and taper together |
| A surface must be flat and square to something | Perpendicularity or parallelism (Orientation Tolerances) | Orientation already contains flatness, so one control does both |
| A surface must follow a curved or free-form shape | Profile of a surface (Profile and Runout) | Form alone cannot describe a curve |
What processes can hold
These are typical values for good practice in common materials, to help choose a realistic tolerance. They vary widely with the machine, the material, the size and the set-up, so confirm them with your supplier before you commit.
| Process | Flatness (about 100 mm) | Roundness / cylindricity |
|---|---|---|
| Milling or routing | 0.02 to 0.05 mm | n/a |
| Turning and boring | n/a | 0.005 to 0.02 mm |
| Surface grinding | 0.002 to 0.01 mm | n/a |
| Cylindrical grinding | n/a | 0.001 to 0.005 mm |
| Honing | n/a | 0.001 to 0.003 mm (cylindricity) |
| Lapping | 0.001 to 0.002 mm | 0.0005 to 0.002 mm |
| Sheet-metal laser cutting and forming | 0.5 to 2 mm (varies with thickness, residual stress) | n/a |
| FDM 3D printing | 0.2 to 0.5 mm | 0.1 to 0.3 mm |
How form is inspected
| Control | Common methods | Watch out for |
|---|---|---|
| Flatness | Granite surface plate with a dial indicator or height gauge; CMM scanning with a least-squares or minimum-zone fit; autocollimator and level for large machine beds | A spread of readings is an upper bound; a best-fit plane can give a smaller true flatness |
| Straightness | Straightedge and feeler gauge; indicator while rotating the part between centers or on V-blocks (for an axis); CMM scanning; laser or optical alignment for long axes | Rotating a bowed part measures the surface’s runout, not exactly its straightness |
| Circularity | Roundness tester (rotating spindle or table, a trace of radius against angle); V-block and indicator; CMM with many points | Few CMM points miss lobes; the filter and number of undulations per revolution affect the result |
| Cylindricity | Roundness tester measuring several heights, or a scanning CMM | Needs enough levels to see taper and bow, and a good part set-up |
A common rule is that the measuring system’s uncertainty should be about a tenth of the tolerance (4:1 at the very least). A tolerance of 0.005 mm is not meaningful if the equipment cannot resolve better than 0.003 mm.
Worked examples
Example 1: Rule #1 on a pin
A pin is drawn ⌀10.00 ±0.10, so its limits are 9.90 and 10.10. The MMC is 10.10, and no explicit form tolerance is given. How much can the axis be out of straight at each actual size?
| Actual size | Allowed axis deviation (= 10.10 − size) | Meaning |
|---|---|---|
| 10.10 | 0.00 | Perfect form at MMC |
| 10.05 | 0.05 | The axis may bow within a ⌀0.05 zone |
| 10.00 | 0.10 | The axis may bow within a ⌀0.10 zone |
| 9.95 | 0.15 | The axis may bow within a ⌀0.15 zone |
| 9.90 | 0.20 | The axis may bow within a ⌀0.20 zone |
At the smallest size the pin can be 0.20 out of straight and still be inside the limits. If that is too loose for the function, an explicit straightness tolerance tightens it (Example 3).
Example 2: checking flatness with a dial indicator
A 100 × 100 mm face has a flatness tolerance of 0.05. It rests on a surface plate and a dial indicator reads the height at nine points (in micrometers, µm, relative to the lowest reading):
| Column 1 | Column 2 | Column 3 |
|---|---|---|
| 0 | 12 | 8 |
| 5 | 30 | 18 |
| 2 | 14 | 9 |
- Highest reading 30 µm, lowest 0 µm: the spread is 30 µm = 0.030 mm.
- Flatness is the width of the narrowest pair of parallel planes that contains every point. The two horizontal planes through the highest and lowest readings contain every point and are 0.030 apart, so the narrowest pair can only be that wide or narrower: the true flatness is no more than 0.030.
- 0.030 is less than 0.05, so the face passes with no further analysis.
- If the tolerance were 0.02, the spread would exceed it, but the face might still pass: a CMM minimum-zone fit tilts the planes to find the narrowest pair. The simple spread can only prove a pass, not a fail.
Example 3: straightness tighter than Rule #1
A shaft is ⌀20.00 down to 19.90 (MMC 20.00) with an explicit axis straightness of ⌀0.05, regardless of feature size. The allowed axis deviation is the smaller of Rule #1’s allowance and 0.05:
| Actual size | Rule #1 allows | Explicit tolerance | Allowed (smaller of the two) | Which controls |
|---|---|---|---|---|
| 20.00 | 0.00 | 0.05 | 0.00 | Rule #1 governs |
| 19.98 | 0.02 | 0.05 | 0.02 | Rule #1 governs |
| 19.95 | 0.05 | 0.05 | 0.05 | Both equal |
| 19.92 | 0.08 | 0.05 | 0.05 | The ⌀0.05 tolerance governs |
| 19.90 | 0.10 | 0.05 | 0.05 | The ⌀0.05 tolerance governs |
The explicit tolerance only makes a difference on shafts at 19.95 and below. At MMC the part must still be perfectly straight, and Rule #1 keeps that.
Example 4: reading roundness
A roundness tester traces a ⌀30 journal and reports the largest radius as 15.0084 mm and the smallest as 15.0041 mm, after the tester has removed the part’s offset from the spindle (by fitting the best circle).
- The two concentric circles that just contain the trace are 15.0084 − 15.0041 = 0.0043 mm apart.
- Circularity is therefore 0.0043. It passes a 0.005 tolerance, and fails a 0.003 one.
- On the diameter this means two diameters across the section may differ by up to about 0.0086, which a micrometer with 0.001 resolution could see only if it happens to land on the high and low spots.
Troubleshooting
| Symptom | Likely cause | Try |
|---|---|---|
| Part is within size but rocks on a flat surface | Surface is not flat: no flatness control, or the control is too loose | Add or tighten a flatness tolerance; check where the part touches |
| Shaft passes a micrometer but binds in its bearing | Lobing (odd-lobed out-of-roundness) or axis bow | Measure on a roundness tester; add circularity and straightness |
| Ground face measures flat on the machine but not after release | The magnetic chuck clamped the part flat; residual stress or clamping then relieves | Measure unclamped, add a stress-relief or a free-state note, or reduce material removal in the final passes |
| Thin part changes shape every time it is clamped | A flexible part; the form depends on how it is held | Specify the restraint and the free-state condition (see Modifiers and Material Conditions) |
| Inspector A says flat, inspector B says not | One used the spread of three-point readings and the other a best-fit plane | Agree the method; a minimum-zone fit is the definition |
| Circularity fails on the CMM, passes on the tester | The CMM took too few points, so it missed a lobe or its filter differs | Use the same number of points per revolution; compare with a tester on the same section |
Related
- GD&T: the overview, symbols and a quick reference to the 14 characteristics.
- Datums and Datum Reference Frames: a good datum feature usually has a flatness tolerance.
- Orientation Tolerances: controls that include form and add a datum.
- Material Properties and Speeds & Feeds: what affects the form a process can hold.
FAQ
Why do form tolerances have no datum?
They control the shape of one feature against its own best-fit shape, so there is nothing outside the feature to measure from. The zone floats to wherever the feature is.
Is flatness the same as parallelism?
No. Flatness has no datum and only limits how far the surface departs from a plane. Parallelism has a datum and limits how far the surface tilts relative to it. A parallelism tolerance on a surface therefore also controls its flatness, so the flatness tolerance, if given, must be smaller.
Does flatness control size?
No. A flatness tolerance applies to the shape of the surface. The thickness of the part is still controlled by its size tolerance, and a surface can be perfectly flat and still the wrong thickness.
If I specify cylindricity, do I need circularity as well?
Usually not. Cylindricity already limits the circularity of every section to the same value. Add circularity only if you need a tighter round section than the overall cylindricity.
Can a form tolerance be bigger than the size tolerance?
Not for a feature of size under Rule #1: the size limits already force the form inside them. To allow more form than size (a flexible part), the drawing must override Rule #1 explicitly.
What does Ⓜ do on a straightness frame?
It lets the axis straightness tolerance grow as the feature gets smaller than MMC (bonus tolerance), and creates a virtual condition. It is used when the part must fit a gage or a mating bore. It is covered with the other modifiers on the Modifiers and Material Conditions page.
How tight should I make a form tolerance?
As loose as the function allows. Each step tighter raises cost: grinding instead of milling, a roundness tester instead of a micrometer. Start from what the part has to do (seal, bear, slide) and from the process that will make it.
References
- ASME Y14.5-2018, Dimensioning and Tolerancing (Rule #1, form tolerances and their zones).
- ASME Y14.5.1M, Mathematical Definition of Dimensioning and Tolerancing Principles.
- ISO 1101, Geometrical product specifications (GPS): Geometrical tolerancing: Tolerances of form, orientation, location and run-out.
- ISO 8015, Geometrical product specifications (GPS): Fundamentals: Concepts, principles and rules (the independency principle and the envelope requirement).
- ISO 12780 (straightness), ISO 12781 (flatness), ISO 12181 (roundness) and ISO 12180 (cylindricity): specification operators and verification.
- Meadows, J. D., Geometric Dimensioning and Tolerancing: Applications, Analysis, Gaging and Inspection, CRC Press.
Last reviewed: October 2026. Process capabilities are typical values only; always confirm with the manufacturer, and use the standard your drawing names.