GD&T Basics: Flatness, Perpendicularity, and Position for CNC Parts

Why GD&T exists

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.

Flatness: controlling 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

Perpendicularity: controlling 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.

Position: controlling 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.

Datums: the reference frame that makes it all 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.

Practical guidance for drawing callouts

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.

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.