Why does GD&T exist at all?

Coordinate dimensioning (plus/minus tolerances on X, Y, Z) describes where features should be, but it cannot control shape, orientation, or the functional relationships between surfaces. A plate can have every thickness dimension within ±0.05 mm and still rock on a surface plate because the face is not flat. A bolt hole pattern can be perfectly spaced in X and Y but tilted relative to the mounting face. GD&T solves this by defining tolerance zones that match how parts actually function.

ASME Y14.5 is the US standard; ISO 1101 is the European standard. Both use the same core concept: a symbol defines a tolerance zone within which the controlled feature must lie, datums define the reference frame, and material condition modifiers adjust tolerance based on feature size.

How does flatness control surface form?

Flatness (◆) is a form control. It defines two parallel planes separated by the tolerance value; the entire controlled surface must lie between them. Flatness does not reference any datum — it is purely about the shape of the surface itself.

On CNC-machined parts, flatness is critical for sealing surfaces, mounting faces, and any surface that acts as a datum. A typical achievable flatness on a milled face is 0.02 mm per 100 mm of length with a proper face mill in a rigid setup. Ground surfaces can hold 0.005 mm per 100 mm. Tighter than that requires surface grinding or lapping.

  • 0.1 mm / 100 mm: standard milled finish, acceptable for non-contact surfaces
  • 0.05 mm / 100 mm: good face mill result, adequate for most mounting faces
  • 0.02 mm / 100 mm: precision milling, suitable for gasket seals and datum surfaces
  • 0.005 mm / 100 mm: surface ground, for precision locating and O-ring sealing
  • 0.002 mm / 100 mm: lapped, for inspection fixtures and optical mounting

How does perpendicularity control orientation?

Perpendicularity (⊥) is an orientation control requiring a datum reference. For a surface, the tolerance zone is two parallel planes separated by the tolerance value, at exactly 90 degrees to the datum. For an axis (e.g., a bore perpendicular to a face), the zone is a cylinder of the tolerance diameter within which the feature axis must lie.

A common application is a hydraulic valve spool bore, which must be perpendicular to the mounting face within 0.02 mm per 100 mm or the spool binds. Coordinate checks alone cannot catch this because the bore can be tilted and still pass.

How does position tolerance control location?

Position (⌖) is the most used and most misunderstood GD&T symbol. It defines a tolerance zone (usually a cylinder for holes, two parallel planes for slots) located at the theoretically exact position given by basic dimensions. The center point, axis, or centerplane of the actual feature must fall within this zone.

When position is specified at MMC (Maximum Material Condition), tolerance increases as the feature departs from MMC size. For a hole at ø10 H7 (ø10.000 to ø10.015 mm) with ⌖ø0.1 MMC A|B|C, position tolerance is ø0.1 mm at the smallest hole size (ø10.000). If the hole measures ø10.012 mm, available position tolerance becomes ø0.112 mm. This bonus tolerance is why GD&T reduces scrap versus coordinate tolerancing.

GD&T SymbolControl TypeTolerance ZoneDatum?
◆ FlatnessFormTwo parallel planesNo
⎕ ParallelismOrientationTwo parallel planes/cylinderYes
⊥ PerpendicularityOrientationTwo parallel planes/cylinderYes
⌖ PositionLocationCylinder (holes) / planes (slots)Yes
⌒ Profile of a SurfaceProfile3D offset from CAD surfaceYes

Why do datums make GD&T work?

GD&T is meaningless without a properly specified datum scheme. Primary datum (A) is typically the mounting face (three degrees of freedom), secondary (B) orients on a second axis (two DOF), and tertiary (C) locks rotation (one DOF).

The 3-2-1 rule applies: three points on A, two on B, one on C. On real parts, pick the largest functional surface as A, a bore or perpendicular edge as B, and a feature that prevents rotation as C. Arbitrary datums make GD&T uninspectable.

How should you write GD&T callouts on a drawing?

Use GD&T where it matters functionally. Do not sprinkle position callouts on every hole with tighter tolerances than you need. A good rule: use ±0.1 mm position for general mounting holes, ±0.05 mm for dowel pin holes and bearing bores, and ±0.02 mm or tighter only for precision locating features. Every decimal place of tighter tolerance adds cost — and tighter inspection requirements.

How are flatness and parallelism measured, and what must the report show?

Flatness and parallelism cannot be verified with a caliper. Flatness is measured on a surface plate or on a coordinate measuring machine (CMM) as the distance between the two parallel planes that bound the surface. Parallelism is measured the same way, but always relative to the datum called out on the drawing — so the report has to state which datum was used, or the numbers cannot be compared with anyone else's inspection.

  • Feature and nominal: for example flatness 0.05 mm on face A, or position ⌖ 0.1 mm at MMC
  • Datum reference frame: A (primary), B (secondary), C (tertiary) — identical to the drawing
  • Measured value per feature, not just pass/fail — that is what shows the real process position
  • Instrument and traceability: CMM, surface plate or gauge, each with its calibration status
  • Who measured it and who released the part

Every TruPart inspection report comes with the CMM report listing measured values, an FAI on the first order and the material certificates, at no extra cost. List the critical features on your RFQ and they are prioritised in the inspection plan.

Frequently Asked Questions

  • What is the H7 tolerance zone for a 10 mm bore?

    H7 on a 10 mm nominal bore gives a tolerance of +0.015 mm / -0.000 mm per ISO 286-2, so the hole must measure between 10.000 mm and 10.015 mm. This is a close-running or precision-locating fit commonly used for dowel pins and bearing journals.

  • What does MMC mean on a position callout?

    MMC (Maximum Material Condition) is a modifier that grants bonus tolerance. For a hole at MMC (smallest allowable size), the stated position tolerance applies. As the hole grows larger within its size tolerance, position tolerance increases by the difference. This makes sense: a larger hole gives more assembly clearance.

  • Can flatness be inspected with a dial indicator?

    Yes, for non-precision work: a part on a surface plate with a dial indicator gives a reading from total indicator travel. However, this does not separate flatness from surface roughness effects. Below 0.01 mm, a CMM or optical flat is required.

  • How do I choose datums for a machined part?

    Choose A as the functional mounting surface (usually the largest flat face), B as a bore or edge perpendicular to A for orientation, and C as a feature that locks rotation. Datums should reflect how the part seats and functions in assembly.

  • What is the difference between profile of a surface and position?

    Position controls feature location (center point, axis, centerplane) but not shape. Profile of a surface controls the entire surface geometry — location, orientation, and form — via a 3D tolerance zone around the CAD model. Use profile for complex contours, position for holes and regular features.

  • How is flatness and parallelism measured and reported on a machined part?

    Flatness is measured on a surface plate or with a CMM as the distance between the two parallel planes bounding the surface; parallelism is measured the same way but relative to the datum on the drawing. The CMM report lists the measured value for each feature — not just pass/fail — together with the datum frame, the instrument and its calibration status.

  • What should a CMM inspection report contain?

    Per feature: nominal, tolerance and measured value; the datum reference frame used; the instrument with calibration status; the date and who measured and released the part. On TruPart orders the CMM report with measured values, the FAI on the first order and the material certificates ship with the parts at no extra cost.

Need this kind of part machined?

Send a drawing — quote in 48 hours. No minimum order; one piece is fine.