Datum
All skills
GD&TRev. Q3 2026

GD&T callout review

Review a drawing's GD&T scheme for legality and intent under ASME Y14.5: datum precedence, degrees of freedom actually constrained, redundant or missing controls, modifier misuse, and whether each callout can be inspected. Use whenever the user shares drawing callouts, asks if their GD&T is correct, asks how to apply position or profile, mentions datum selection, MMC/LMC, composite tolerances, or gets pushback from a machine shop or CMM programmer about a callout.

Kenji Aoyama portraitKenji AoyamaGD&T SpecialistMitutoyo logoMitutoyo

Likes are peer vetting. Like this skill if it held up in your work.

GD&T Callout Review

Reviews geometric tolerancing the way a checker does: first is it legal, then does it constrain what the function needs, then can anyone actually measure it.

Required inputs

  1. The callouts, transcribed or listed: feature, feature control frame contents, and datum definitions. If the user has an image of the drawing, work from what is visible and list anything illegible as an open question.
  2. What the part does: mating features, which surfaces locate it, which features must align with what. Function drives datum selection; without it the review is only a legality check, and say so.
  3. The standard in force (default ASME Y14.5-2009 or 2018; ask if ISO GPS, because rules differ, notably the envelope requirement).

Review sequence

Run these checks in order and report findings grouped by severity: ILLEGAL (won't survive a checker), FUNCTIONAL RISK (legal but doesn't protect function), INSPECTION RISK (hard or ambiguous to measure), and COST (tighter or more complex than function requires).

  1. Datum reference frame
    • Do the datums correspond to how the part is located in the assembly? Primary should be the surface that dominates orientation in use, not the largest convenient face.
    • Count degrees of freedom constrained by each datum in precedence order. Flag over-constraint (a tertiary datum that constrains nothing) and under-constraint (rotation left free that function needs controlled).
    • Datum features of size referenced RMB vs MMB: is the choice deliberate? MMB implies a functional gage condition.
  2. Legality of each frame
    • Form tolerances (flatness, circularity) must not reference datums. Position must reference datums (with rare pattern exceptions). Profile without a datum controls form only; is that intended?
    • Modifier legality: MMC/LMC only on features of size. Diameter symbol present when the tolerance zone is cylindrical. Projected tolerance zone on tapped holes that receive studs or long fasteners; flag if missing.
    • Composite vs. two-single-segment frames: does the lower segment reference repeat the intent (pattern-to-pattern vs. feature-to-feature)? This is the most common misuse; explain the difference in one sentence when flagged.
  3. Coverage
    • Every surface should be controlled by something: a directly toleranced dimension, a profile, or a general note. Hunt for orphan surfaces.
    • Are refinements ordered correctly (each refining control tighter than the one it refines, e.g., perpendicularity tighter than the position it refines)?
  4. Inspectability
    • Can each callout be verified with the shop's likely equipment? Flag callouts that require a CMM but will go to a shop with calipers and pins, and callouts where the datum feature is too small or rough to establish a repeatable frame.
    • Position at MMC enables hard gaging; note where a functional gage would pay off at volume.
  5. Cost
    • Identify tolerances tighter than the process typically holds (e.g., position dia 0.05 on a drilled hole) and totals that could be met with a looser tolerance plus a bonus from MMC.

Output format

  • Findings table: callout, finding, severity, recommended rewrite (full feature control frame text, e.g., "position dia 0.25 (M) | A | B (M) | C")
  • Rewritten datum strategy in three or four sentences if datum selection is the root problem
  • Open questions where drawing information was missing

Guardrails

  • Never invent tolerance values. Propose the structure of the fix and ask for, or reason from, the functional requirement to set the number.
  • If the user's shop or customer is on ISO GPS and the drawing is ASME (or mixed), flag it as a finding on its own; mixed-standard drawings cause real disputes.
  • When a callout is legal but unusual, say "legal but will generate shop questions" rather than calling it wrong.

More GD&T skills