Gdandt Basics

GDandT Basics (cross-cutting/tolerancing/gdandt-basics)

Use when the task is the geometric dimensioning and tolerancing fundamentals behind an ASME Y14.5 drawing: reading a feature control frame, establishing the datum reference frame, telling a form, orientation, position, profile, or runout tolerance apart, applying the material condition modifiers (MMC, LMC, RFS), and computing the bonus tolerance that becomes available when a feature departs from its maximum material condition size. This leaf is the foundation for the tolerancing pack; it is distinct from cross-cutting/tolerancing/position-tolerance-calc (which runs the full position verification with virtual condition), from cross-cutting/tolerancing/tolerance-stackup (which sums tolerance contributions across an assembly), and from cross-cutting/tolerancing/datum-reference-frames (which builds and evaluates datum reference frames in detail).

Domain quick reference

• Feature control frame: the drawing symbol that carries the tolerance. It reads, in order: geometric characteristic symbol, tolerance value (diameter symbol when the zone is cylindrical), optional material condition modifier, then up to three datum references. Example: position | diameter 0.5 (M) | A | B (M) | C.
• Geometric characteristic categories: form tolerances (flatness, straightness, circularity, cylindricity) control shape alone and carry no datum; orientation tolerances (perpendicularity, parallelism, angularity) control orientation relative to a datum reference frame; position controls location relative to the true position; profile controls a boundary offset from the true profile; runout controls coaxiality relative to a datum axis.
• Tolerance zone types: flatness is two parallel planes; circularity is an annulus between two concentric circles; cylindricity is the annular space between two coaxial cylinders; position is a cylindrical zone, expressed as a diameter, about the true position; perpendicularity, parallelism, and angularity are planes or cylinders oriented to the datum frame.
• Datum reference frame: the ordered set of datum features (primary, secondary, tertiary) that locates and orients the tolerance zones. The frame is read left to right in the feature control frame.
• Material condition modifiers, applied to the tolerance in the frame: M means maximum material condition (MMC), the most material the feature can have (smallest hole, largest pin); L means least material condition (LMC), the least material (largest hole, smallest pin); S, or no modifier at all, means regardless of feature size (RFS).
• Bonus tolerance at MMC: the stated tolerance applies at the MMC size; any departure of the actual feature size from the MMC size adds bonus. For a hole (MMC = smallest size) the bonus is actual - mmc; for a pin (MMC = largest size) the bonus is mmc - actual. Total tolerance = stated tolerance + bonus.
• LMC bonus works in the opposite direction: for a hole the bonus is lmc - actual, for a pin it is actual - lmc.
• Zero tolerance at MMC is legitimate: a position callout of diameter 0 (M) means the feature must sit exactly at true position when at MMC, and every unit of departure from MMC becomes the available tolerance.

Workflow

1. Read the feature control frame off the drawing and parse it with parse_feature_control_frame; the result carries the symbol, the tolerance value, the diameter flag, the modifier, and the datum list.
2. Identify the tolerance category with tolerance_category (form, orientation, location, profile, or runout) and the zone shape with tolerance_zone_type.
3. Read the material condition modifier with material_condition_modifier and explain it with modifier_meaning (MMC, LMC, or RFS default).
4. From the size limits and the part type, derive the boundary sizes with mmc_size and lmc_size.
5. When the modifier is M, compute the bonus tolerance with bonus_tolerance_at_mmc from the actual feature size, and the total budget with total_tolerance_at_mmc.
6. For an LMC callout, use bonus_tolerance_at_lmc instead.
7. Assemble the full interpretation with interpret_feature_control_frame, which includes the bonus and total tolerance whenever the modifier is M and the sizes are supplied.
8. Confirm the deterministic checks with the contract test scripts/test_gdandt_basics.py.

Worked example

Interpret the feature control frame "position | diameter 0.5 (M) | A | B | C" for a hole with size limits 10.0 to 10.3 mm:

• parse_feature_control_frame returns symbol "position", tolerance 0.5, diameter True, modifier "M", and datums A, B, C in order.
• tolerance_category is "location"; tolerance_zone_type is the cylindrical zone of diameter 0.5 about the true position.
• modifier_meaning("M") is "maximum material condition (MMC): the stated tolerance applies at the MMC size and grows with departure from MMC".
• mmc_size((10.0, 10.3), "hole") is 10.0; the bonus is zero when the hole measures 10.0 and grows as the hole grows.
• If the actual hole measures 10.3, bonus_tolerance_at_mmc gives 10.3 - 10.0 = 0.3 and total_tolerance_at_mmc gives 0.5 + 0.3 = 0.8; the acceptance zone diameter is 0.8 at that size.
• A hole measuring 9.9 is below MMC, violates the size limits, and the logic raises ValueError rather than returning a negative bonus.

A second example: "flatness | 0.2" is a form tolerance, so tolerance_category returns "form", the zone is two parallel planes 0.2 apart, and parse_feature_control_frame raises if a datum is added, because form tolerances reference no datum.

Pitfalls

• Adding a datum to a form tolerance callout: parse_feature_control_frame raises, because form tolerances reference no datum.
• Reading the zone as a cylinder for every symbol: only location tolerances such as position with the diameter flag get a cylindrical zone; "flatness | 0.2" is two parallel planes 0.2 apart.
• Forgetting that MMC bonus grows with departure from MMC: the bonus is zero at the MMC size (10.0 for a hole with limits 10.0-10.3) and grows as the feature departs toward LMC.
• Passing a size outside the size limits: a hole at 9.9 is below MMC and violates the limits, so the logic raises ValueError instead of returning a negative bonus.
• Applying the MMC bonus machinery to an LMC callout (or assuming a bonus under RFS): LMC callouts use bonus_tolerance_at_lmc, and the RFS default grants no bonus at all.
• Treating the stated tolerance as the zone at every size: with the M modifier the acceptance zone is stated tolerance plus bonus (0.5 + 0.3 = 0.8 for a 10.3 hole), so the zone grows with the feature.

Related leaves

• cross-cutting/tolerancing/position-tolerance-calc: full position verification, deviation from true position, virtual condition, and the acceptance verdict.
• cross-cutting/tolerancing/tolerance-stackup: summing tolerance contributions across an assembly.
• cross-cutting/tolerancing/datum-reference-frames: datum reference frame construction and evaluation in detail.

Behavior contract (gate 3)

Run the deterministic contract test (stdlib unittest, offline):

python3 scripts/test_gdandt_basics.py

The test covers feature control frame parsing (symbol, tolerance, diameter flag, modifier, datums), category and zone classification, modifier meanings, MMC and LMC bonus tolerance including size-limit violations, boundary sizes, total tolerance at MMC, zero tolerance at MMC, the full frame interpreter, and invalid-input edge cases.

Compliance

• Standards referenced, not reproduced: ASME Y14.5 is proprietary (ASME); the feature control frame structure, the tolerance categories, the MMC/LMC/RFS modifiers, and the bonus tolerance rule are common GD&T methodology, name and paraphrase only per standards-map.yaml.
• compliance: STANDARDS-REF, gated: false (reference-only listing).