본문 바로가기
Guides

GD&T Symbol Chart

Spec chartsCNC machiningSep 10, 2026

Dimensional tolerances alone cannot say "how well do the holes line up" or "how flat is the surface." The language for specifying that is geometric tolerancing (GD&T). The 14 symbols are listed in a table, and the 6 most commonly used come with practical values.

GD&T Symbol Chart

SymbolNameCategoryDatum
⏤StraightnessFormNot required
⏥FlatnessFormNot required
○CircularityFormNot required
⌭CylindricityFormNot required
⌒Profile of a lineFormOptional
⌓Profile of a surfaceFormOptional
∥ParallelismOrientationRequired
⟂PerpendicularityOrientationRequired
∠AngularityOrientationRequired
⌖PositionLocationRequired
◎ConcentricityLocationRequired
⌯SymmetryLocationRequired
↗Circular runoutRunoutRequired
⌰Total runoutRunoutRequired

Form tolerances look at that one feature alone, while orientation, location, and runout tolerances need a reference feature (datum). A parallelism callout without a datum has nothing to be parallel to, so it cannot be inspected.

The 6 Most Used Symbols and Practical Values

SymbolWhereTypical valuePrecision value
⏥ FlatnessDatum and sealing surfaces0.050.02
⟂ PerpendicularityShafts, flanges0.05/1000.02/100
∥ ParallelismOpposing faces0.050.02
⌖ PositionBolt holes⌀0.2⌀0.1
◎ ConcentricityBearing seats0.030.01
↗ RunoutRotating shafts0.030.01

Typical values are what CNC milling and turning can hold without a separate operation. From the precision values onward, grinding or jig machining is added.

Where to Apply Them

  • Apply them only to functional features: surfaces where seals contact, bearing seats, and datum surfaces that mate with other parts
  • Leave the rest to general tolerances (ISO 2768). Writing ISO 2768-K in the title block also sets default geometric tolerances
  • Match the datum to the machining datum. If the surface held during machining differs from the inspection datum, the error doubles

Why Geometric Tolerances Raise Machining Cost

RequirementWhat gets added
Flatness 0.02Grinding or lapping operation
Position ⌀0.05Jig machining, CMM inspection
Concentricity 0.01Single-setup machining, grinding
Perpendicularity 0.01/100Precision fixtures, measurement time

Each time the value tightens one step, one more operation is added. If precision values are applied throughout a drawing, the whole part becomes a ground part.

Frequently Asked Questions

What happens if no geometric tolerance is specified?

The default geometric tolerances of the general tolerance standard apply. If the title block has no standard noted, the manufacturer assumes the medium class.

Should I specify concentricity or runout?

For rotating parts, runout is easier to inspect. It can be measured directly with a dial gauge. Concentricity requires CMM measurement, which adds cost.

If position is ⌀0.1, what is the hole position error?

The center must fall within a circle of diameter 0.1, that is, within a radius of 0.05. It is similar to a dimensional tolerance of ±0.05, but it also covers the diagonal direction.

See Also

Read them in this order to decide where to apply tolerances.

Source standard: KS A ISO 1101 (geometric tolerance symbols). Practical values are design practice, not standard values.

Have a part to machine?

Upload a drawing to see your quote.

Sponsorship & lab support

From competition prep to research projects,
we build alongside student teams and labs.

Questions?

KakaoTalk chat
031-509-0523