Right, plan, roundness, cylindrical tolerances: a machinist's read

• 1
  Right tolerance: perpendicularity and what it constrains
• 2
  Plan tolerance: flatness, parallelism, and the datum trap
• 3
  Roundness tolerance: lobing, ovality, and why a caliper lies
• 4
  Cylindrical tolerance: the one that covers the whole surface
• 5
  Comparing right, plan, roundness, and cylindrical tolerances

On a drawing, "right" usually means perpendicularity or squareness. It controls how far a surface, axis, or center plane may tilt away from a 90° relationship to a datum. The control is always measured against a datum, so the datum feature itself has to be established first. A face that is flat but sits 0.1° off square on a shaft will still fail a perpendicularity callout, even though a flatness check passes.

The tolerance zone depends on the feature. For a flat surface, it is two parallel planes 90° to the datum, separated by the tolerance value. For an axis, it is a cylinder 90° to the datum plane, with the axis diameter equal to the tolerance. A 0.05 mm perpendicularity callout on a Ø20 mm bore means the derived axis must stay inside a 0.05 mm cylinder over the full part length.

This is where right plan roundness cylindrical tolerances start to interact. A perpendicularity failure on a bore often comes from a roundness problem, not from setup error. If the bore is lobed, the center point moves as the probe rotates, and the derived axis wanders. Fix the roundness first, then recheck squareness.

Perpendicularity is not the same as an angular tolerance. An angular callout allows a specified tilt, such as 89.5°. A right tolerance demands exactly 90°, with the deviation bounded by the zone. Mixing the two on one drawing confuses inspectors and adds cost.

"Plan" on a print points to planarity, which engineers usually express as flatness or parallelism. Flatness is a form control. It needs no datum. It says every point on the surface must lie between two parallel planes separated by the tolerance value. A 0.02 mm flatness callout on a sealing face is common in hydraulic and vacuum work.

Parallelism is an orientation control. It is measured against a datum, so it ties the surface to another feature. Two faces 0.03 mm parallel to datum A can both be slightly bowed and still pass, as long as the distance between them stays inside the zone. Flatness alone cannot guarantee that.

For a machined plate, the practical limit is set by the machine, the fixturing, and the material. A 300 mm aluminum plate will move after clamping release. We rough it, let it relax, then finish it to hold 0.02 mm. On a thin wall under 2 mm, that number becomes hard to hold without stress relief between passes.

The datum trap is common. Engineers call parallelism to datum A, then dimension the feature from datum B. The inspector measures one way, the designer intended another, and the part gets rejected for the wrong reason. Put the datum that matters on the feature that seats first in the assembly.

Roundness, sometimes called circularity, controls how close a cross-section is to a true circle. It applies to each cross-section independently. There is no datum. The tolerance zone is the annular space between two concentric circles whose radii differ by the tolerance value. A 0.01 mm roundness callout means the radius varies by no more than 0.01 mm around the section.

A two-point caliper cannot see this. A three-lobe shape can measure the same diameter in every direction while sitting well outside a true circle. This is the classic reason a shaft feels tight in a bore even though the micrometer says the size is right. Three-point contact, a V-block, or a roundness tester is needed to catch lobing.

Roundness errors come from several places. Workholding with three jaws on a thin ring is one. Another is a spindle with runout. Centerless grinding can produce a three-lobe profile if the setup geometry is wrong. Turning a part between centers usually gives the best roundness on a cylindrical surface.

Roundness and size are separate requirements. A part can be within the diameter tolerance and still fail roundness. Rule 1 of GD&T handles this at maximum material condition, but a separate roundness callout is clearer when the function depends on sealing or bearing contact.

Cylindricity is the strictest of the four. It controls the entire cylindrical surface at once: roundness in every cross-section, straightness of the axis, and taper along the length. The tolerance zone is the space between two coaxial cylinders whose radii differ by the tolerance value. It is a form control, so no datum is required.

Because it covers everything, cylindricity is expensive to hold and expensive to verify. A roundness tester measures one section at a time. Full cylindricity needs a scanning CMM or a dedicated form tester with a helical path. On a 100 mm long bore, a 0.005 mm cylindricity callout is a grinding or honing operation, not a turning operation.

Use it when the function truly needs the whole surface. Hydraulic cylinder bores, bearing journals, and precision spindles are good candidates. For a simple locating pin, roundness plus a size tolerance is usually enough, and the part will cost less.

If you need both a location and a form control on the same bore, a position tolerance is a separate requirement, and the two must be checked independently. Adding cylindricity does not replace position, and position does not tighten the form.