EUCylindricity is the form tolerance for cylindrical surfaces. It checks whether the entire surface of a shaft, bore, or pin stays within an acceptable shape envelope. On parts like hydraulic cylinders, bearing journals, and valve stems, poor cylindricity leads to seal failure, vibration, uneven wear, and assembly problems.
This guide covers the cylindricity symbol, feature control frame, tolerance zone, measurement methods, typical tolerance values, and differences from related controls such as circularity and runout.
What is Cylindricity?
Cylindricity is a form tolerance that evaluates how closely a cylindrical feature matches an ideal cylinder. Unlike simpler checks, it examines the entire surface at once rather than a single cross-section or a single line element.
Think of cylindricity as the three-dimensional version of circularity. Circularity checks whether one cross-section is perfectly round. Cylindricity checks whether the full cylinder, from end to end, stays within the tolerance.
Cylindricity is a form control applied to an individual feature. It does not reference a datum. It does not control the size of the feature, and it does not use material condition modifiers (MMC or LMC). It controls only the shape of the cylindrical surface.
Cylindricity Symbol and Feature Control Frame
1. Cylindricity Symbol:
The cylindricity symbol is a circle between two oblique (slanted) lines, representing a simplified side view of a cylinder. This symbol appears in the first compartment of the feature control frame on engineering drawings.
The symbol tells manufacturing and inspection that all surface elements of the cylindrical part must be evaluated, not just individual cross-sections or line elements. In geometric dimensioning and tolerancing, this cylindricity GD&T symbol is one of four form control symbols, alongside straightness, flatness, and circularity.
2. Feature Control Frame
The feature control frame for the cylindricity callout contains two compartments only. There is no datum block because cylindricity does not reference a datum feature.
| Compartment 1 | Compartment 2 |
| Cylindricity symbol (⌭) | Numerical tolerance value (e.g. 0.05) |
The first compartment contains the cylindricity symbol. The second compartment contains the tolerance amount in millimetres or inches. There is no third compartment because cylindricity does not reference any datum feature or require reference points.
The tolerance value specifies a radial gap, not a diameter. The diameter sign (Ø) is never used inside the frame.
The feature control frame connects to the controlled surface with a leader arrow. The leader must point directly to the physical cylindrical surface or its extension line. It must never point to a size dimension line.
3. Diameter Symbol and Size Tolerance
The diameter symbol (Ø) often appears near a cylindricity callout, but they serve different purposes. The diameter dimension and its diameter tolerance control the feature size. The cylindricity tolerance controls only the shape.
The cylindricity tolerance value must always be smaller than the size tolerance. If it were equal to or larger, the form control would add nothing meaningful. A cylindrical part is considered acceptable only when it satisfies both the size limits and the cylindricity tolerance zone.
4. General Notes on Drawings
Some drawings include general tolerance notes in a tolerance block that cover basic form requirements. However, cylindricity should be specified through a feature control frame on each specific feature. A general tolerance block alone cannot adequately control cylindricity, because it applies to an individual surface without a datum reference.
If multiple cylindrical features on the same part require identical cylindricity GD&T control, each feature needs its own feature control frame and cylindricity callout.
Cylindricity Tolerance Zone
The cylindricity tolerance zone is a 3D boundary defined by two concentric cylinders (also called two coaxial cylinders). Every point on the actual part surface must lie between the inner and outer cylinders. The tolerance zone controls roundness, axis straightness, taper, and waviness at the same time.
Key Characteristics
Shape: The cylindricity tolerance zone consists of two concentric cylinders sharing a central axis. The actual surface must fit entirely within the radial gap between them.
Tolerance value: The tolerance amount in the feature control frame represents the radial distance (gap width) between the two concentric cylinders. For example, a cylindricity tolerance of 0.05 mm means the two coaxial cylinders are separated by 0.05 mm in the radial direction. This is a radial value, not a diameter value. No diameter symbol (Ø) is used.
No datums required: Cylindricity is a pure form tolerance. It does not reference any external datums or datum features. The two concentric cylinders are mathematically fitted to the actual surface to minimise the radial separation that contains it.
What it controls: The cylindricity tolerance zone captures all cylindrical form errors at once: ovality, lobing, taper, barrel shape, hourglass shape, straightness deviations, and waviness along the axial portion of the cylindrical part. The total variation of the surface must fall within the tolerance zone.
The golden rule: The cylindricity tolerance value must always be smaller than the size tolerance (diameter tolerance) of the feature. If it were equal to or larger, the form control would add nothing meaningful.
No bonus tolerance: Cylindricity does not receive bonus tolerance at maximum material condition or LMC. The tolerance amount is fixed regardless of the feature size or actual produced size.
How to Measure Cylindricity
Measuring cylindricity requires data from the entire surface, not just a single cross-section. There are several methods, ranging from simple shop-floor checks to high-precision laboratory measurements. The key difference between methods is how many points and cross-sections they sample.
V-Block and Dial Indicator (Basic Method)
Place the cylindrical part on a V-block or a pair of precision rollers. Rotate the part slowly while recording dial indicator readings at several marked points along the axial portion. Repeat measurements at multiple axial positions along the entire length of the cylinder.
This method provides a rough estimate of the total variation. It is practical for quick checks but not suitable for tight tolerances, because the V-block setup mixes roundness errors with other geometric effects.
Roundness Measuring Instrument (Dedicated Method)
A dedicated roundness measuring instrument (such as a Taylor Hobson Talyrond or Mitutoyo Roundtest) rotates the cylindrical part on a precision spindle while a measuring probe traces the surface. Under computer control, the instrument takes point measurements at multiple cross-sections along the axial portion. Software then combines the data to calculate the total cylindricity error and the total variation across the entire surface.
Results are typically displayed on a polar graph showing deviation from a perfect cylinder. A polar graph can also be plotted manually from the recorded data when digital output is not available. This method provides high accuracy and is the standard approach for precision components in mechanical and automotive applications.
Coordinate Measuring Machine (CMM)
A coordinate measuring machine probes multiple marked points across the cylindrical surface, sampling several cross-sections at different heights along the axial portion. The machine’s software fits an ideal cylinder to the measured data and calculates the cylindricity deviation.
CMMs offer flexibility because they can measure cylindricity alongside other GD&T characteristics in a single setup. However, the number of probed points affects accuracy. More points give a more reliable result.
Whichever method you use, take repeat measurements and sample enough cross-sections to capture the full range of surface variation. A measurement taken at only one or two cross-sections may miss taper, barrel shape, or localised defects along the entire stack of measurements.
Typical Cylindricity Tolerance Values
The achievable cylindricity depends on the manufacturing process and part size. The table below gives general guidance for common processes.
| Process | Typical Cylindricity (mm) | Notes |
| Standard CNC turning | 0.02 to 0.05 | Depends on L/D ratio, clamping, and tool condition |
| Precision CNC turning | 0.01 to 0.02 | Short parts, stable setup, sharp tooling |
| Cylindrical grinding | 0.005 to 0.01 | Common for bearing seats and precision shafts |
| Honing | 0.002 to 0.005 | Used for cylinder bores, hydraulic cylinders |
| Lapping | 0.001 to 0.003 | High-cost, used for the tightest requirements |
These values are approximate. Actual results depend on machine condition, workholding, part geometry, and material.
Tighter cylindricity adds inspection time and cost. Specify only what the function requires.
Factors That Affect Cylindricity
Understanding what causes cylindricity form errors helps engineers write realistic tolerances and helps manufacturers control their processes. These factors affect the total variation of the cylindrical part surface.
Tool Wear and Deflection
A worn or deflecting cutting tool produces a tapered or barrel-shaped surface. On long cylindrical parts, tool deflection increases with distance from the chuck, creating a measurable taper along the axial portion.
Workholding
Three-jaw chucks apply uneven clamping force, which can distort thin-walled or soft parts into a tri-lobed cross-sectional shape. The distortion may spring back after unclamping but leaves residual form error. Collet chucks or soft jaws ground in place reduce this effect.
Thermal Effects
Heat generated during machining causes localised expansion. If the cylindrical part or machine heats unevenly, the resulting surface will deviate from the ideal cylindrical form. Coolant management and controlled cutting speeds help reduce thermal distortion.
Part Geometry (Length-to-Diameter Ratio)
Long, slender parts deflect under cutting forces and their own weight. The longer the unsupported length relative to the diameter, the harder it is to hold tight cylindricity. Steady rests, follower rests, or between-centres setups improve results on long shafts.
Machine Condition
Spindle runout, guideway wear, and central axis alignment errors in the machine tool all transfer directly to the workpiece surface. Regular machine calibration and maintenance are essential for holding tight cylindricity tolerances.
Applications of Cylindricity
Cylindricity is commonly applied in mechanical and automotive applications where cylindrical parts must maintain precise form for sealing, rotating, or sliding functions. Below are the most common uses.
Hydraulic and Pneumatic Cylinders
The bore of a hydraulic cylinder must be closely cylindrical to maintain a seal against the piston. Shape errors such as taper or ovality create gaps that allow fluid to bypass the seal. This leads to pressure loss, reduced efficiency, and accelerated seal wear. Typical cylindricity requirements for hydraulic bores range from 0.005 to 0.02 mm depending on pressure and bore size.
Precision Shafts and Bearings
Rotating shafts that run in bearings need consistent cylindrical form over their entire length. A shaft with a slight taper or barrel shape creates uneven loading on the bearing. This causes vibration, noise, and premature bearing failure. Cylindricity is commonly applied on bearing journals and seal surfaces.
Piston and Cylinder Bores
Engine and compressor performance depends on the fit between piston and bore. Poor cylindricity in either cylindrical part leads to blow-by, high oil consumption, and reduced compression. Controlling cylindricity ensures uniform clearance around the full circumference and along the full stroke length.
Valve Components
Valve stems and seats require precise cylindrical form for correct seating and sealing. A non-cylindrical valve stem may leak in one position and bind in another. This is especially critical in high-pressure or high-temperature applications where even small leaks compound over time.
Precision Hole Alignments
When a pin or shaft passes through multiple aligned holes, each hole must maintain cylindrical form over its full depth. A hole that is round at the entrance but tapered or oval deeper in will cause the pin to jam or misalign. Cylindricity control prevents this, which is particularly important in aerospace and tooling applications.
Threaded Components
On high-precision threaded parts, the cylindricity of the major and minor diameters affects thread engagement and function. Poor cylindricity causes inconsistent thread depth, which can lead to cross-threading, jamming, or weak joints. This matters most in critical fastening applications and precision instruments.
Cylindricity vs Circularity
Circularity and cylindricity are both form tolerances that do not require datums. The key difference is dimensional scope.
| Feature | Circularity (Roundness) | Cylindricity |
| Scope | 2D: one cross-section | 3D: the entire cylindrical surface |
| Tolerance zone | Two concentric circles in a single plane | Two coaxial cylinders along the full length |
| Controls | Ovality, lobing at one slice | Ovality, lobing, taper, barrel, bow, straightness |
| Datum required | No | No |
| Symbol | Single circle | Circle with two tangent lines |
| Inspection | Roundness tester or CMM at one cross-section | Roundness tester or CMM across multiple cross-sections |
A part can pass circularity at every cross-section but still fail cylindricity if it has a taper or bend along its length. Cylindricity is the stricter control because it captures both cross-sectional errors and axial errors.
Use circularity when only local roundness matters (for example, an O-ring groove cross-section). Use cylindricity when the full cylindrical form is functionally important.
Cylindricity vs Total Runout
Cylindricity and total runout both evaluate the entire cylindrical surface, but they work differently.
| Feature | Cylindricity | Total Runout |
| Datum required | No | Yes (requires a datum axis) |
| What it controls | Shape only (form tolerance) | Shape, orientation, and location relative to the datum axis |
| Tolerance zone | Two coaxial cylinders (best-fit axis) | Two coaxial cylinders centred on the datum axis |
| When to use | When shape alone matters | When the surface must also be concentric with another feature |
Total runout is a composite control. It includes cylindricity errors plus any eccentricity or tilt relative to the datum axis. If a shaft is perfectly cylindrical but offset from the datum axis, it will pass cylindricity but fail total runout.
Choose cylindricity when you care only about the surface form. Choose total runout when the cylindrical surface must also run true to a reference axis.
Frequently Asked Questions
What is circularity in GD&T?
Circularity (roundness) measures how closely a single cross-section matches a perfect circle. It is a 2D form control. All points on the measured cross-section must fall between two concentric circles. Circularity does not control taper or straightness along the length of a cylinder.
What is the difference between concentricity and cylindricity?
Concentricity checks whether the median points of a feature’s cross-sections lie on the datum axis. It is a location tolerance that requires a datum. Cylindricity checks whether the surface matches an ideal cylinder. It is a form tolerance with no datum reference. Concentricity controls axis alignment. Cylindricity controls surface shape.
What is the difference between cylindricity and surface profile?
Cylindricity applies only to cylindrical surfaces. Surface profile (profile of a surface) can control any shape, including complex curves, flat surfaces, and compound forms. Surface profile is more versatile but requires a defined nominal surface. Cylindricity is the simpler callout when the feature is a plain cylinder.
Can the cylindricity tolerance be larger than the size tolerance?
No. The cylindricity tolerance must be smaller than the size tolerance. If the cylindricity tolerance equalled or exceeded the size tolerance, the form control would be meaningless because any surface within the size limits would automatically satisfy the cylindricity requirement.
What standard governs cylindricity?
Cylindricity is defined in ASME Y14.5 (the US standard for geometric dimensioning and tolerancing) and ISO 1101 (the international standard for geometrical tolerancing). Both standards define the cylindricity symbol, tolerance zone, and application rules.
One key difference: ASME Y14.5 applies Rule #1 (the envelope principle) by default. This means the size tolerance automatically limits the maximum form error at maximum material condition. ISO 1101 follows the independence principle by default, so size and form are controlled separately unless the envelope symbol (Ⓔ) is added. This affects how cylindricity interacts with the size tolerance on your drawing.
