The example above reads: True Position tolerance of ⌀0.5mm at Maximum Material Condition (MMC), referenced to datums A, B, and C.

1. Cell 1 — Geometric Characteristic: The symbol tells you what type of tolerance (form, orientation, location, profile, or runout).
2. Cell 2 — Tolerance Value: If preceded by ⌀, the zone is cylindrical/circular. If no ⌀, the zone is two parallel planes. The value is always in the drawing units (mm or inches).
3. Material Condition Modifier: Ⓜ (MMC), Ⓛ (LMC), or Ⓢ (RFS). If absent, RFS applies by default (ASME Y14.5-2018).
4. Datum References: Listed in order of precedence — primary (A), secondary (B), tertiary (C). Not all tolerances require datums (form tolerances do not).

Select each cell below to compose a real FCF. The live preview updates instantly and the decoder explains every cell in plain English.

The canvas above shows a schematic engineering drawing view of your selected FCF applied to a hole feature, with leader line, datum triangles, and basic dimensions. Changes update when you modify the builder above.

This means: a shaft specified as ⌀20.000 ± 0.050 has MMC = ⌀20.050mm. At that size, the shaft must be perfectly straight, perfectly round, and perfectly cylindrical — zero form error is allowed at MMC. As the shaft shrinks from MMC toward LMC (⌀19.950mm), form error equal to the departure from MMC is permitted.

Drag the Actual Size slider to see how the perfect-form envelope shrinks away from MMC — and how much form error is then permitted. The right chart shows the allowed form error as a function of actual size.

• GO gauge must be full form — it verifies the perfect-form-at-MMC envelope
• NO-GO gauge need only check one cross-section — it only verifies the LMC size limit
• If a straightness or cylindricity callout is added to a sized feature, it can override Rule #1 and relax the envelope requirement

Drag the slider to set the allowed position deviation. The left zone shows traditional ± square tolerancing. The right shows the equivalent GD&T circular zone. Watch how many more parts pass with GD&T.

Typical industry data. GD&T reduces scrap by recovering parts that pass functionally but failed ± inspection. Rework reduction comes from unambiguous measurement frames. Inspection cost reduction comes from hard gauging vs CMM measurement per part.

Drag the slider to change tolerance. Click Randomize to generate a new surface profile. The green band shows the tolerance zone; each measured line element must stay within it.

• Straightness ≤ size tolerance (surface elements cannot violate Rule #1 / Taylor Principle)
• Axis straightness with ⌀ can exceed size tolerance when MMC is specified
• Measured by placing part on surface plate and using dial indicator along element
• Do NOT confuse surface straightness with axis straightness — they are measured very differently

Adjust tolerance and surface waviness. The 3D heatmap and cross-section both update live. Green zone = within tolerance; red points = violation.

Enter measured surface heights at 4 corners + center. Computes flatness error and checks against tolerance.

• Flatness error ≤ size tolerance of the surface (Rule #1)
• Tighter flatness → better sealing, better bearing contact, more machining cost
• Typical ground surface: 0.005–0.025mm; milled: 0.025–0.1mm
• Flatness does NOT control location or orientation of the surface — add parallelism or perpendicularity for that

The inner and outer dashed circles define the annular tolerance zone. The coloured profile is the measured cross-section. Drag sliders to see how lobing and tolerance interact.

• Circularity ≤ half the size tolerance (it is bounded by the size limits)
• Measured with roundness tester (Talyrond) or CMM in circular scan mode
• Evaluated per cross-section — axis can still be bent (use cylindricity to control both)
• Micrometer measurement does NOT detect odd-lobe roundness errors — a 3-point micrometer reads constant on a 3-lobed part

The unwrapped cylinder shows all surface points. X-axis = angular position (0°–360°), Y-axis = axial position. Colour = radial deviation. Green band on profile plot = tolerance zone. Drag sliders to see combined form errors.

• The most comprehensive form tolerance for cylindrical features
• If cylindricity is specified, individual circularity and straightness callouts are redundant (and should be removed)
• Expensive to inspect — requires CMM or specialized roundness/cylindricity measuring machine
• Cylindricity cannot be applied with material condition modifiers (Ⓜ/Ⓛ) — it is always RFS
• Rarely specified on production drawings due to inspection cost; used for precision spindles and hydraulic cylinders

Drag sliders to adjust the wall tilt and tolerance. The left view shows the physical part (wall on datum plane) with the tolerance zone. The right graph shows the angular deviation measured at the wall axis.

• Perpendicularity refines orientation only — a separate dimension still locates the feature
• Can be applied with Ⓜ for assembly — bonus tolerance at MMC is common for tapped holes
• Measured with angle plate, CMM, or precision square + dial gauge
• Squareness ≠ perpendicularity — a tapered surface can appear square but still fail GD&T

Set the basic angle and tolerance. The angled surface (inclined block) is shown sitting on datum A. The green tolerance band is centred on the true basic angle. Drag the actual angle slider to see when the surface falls inside or outside the zone.

• The angle (60°, 45°, 30°) is a basic dimension — not toleranced directly
• Angularity controls orientation variation, not the angle value itself
• Measured by setting part at basic angle with sine bar or CMM, then checking deviation
• Never tolerance the angle ± AND add an angularity callout — they conflict. Use GD&T with basic angle only.

The bottom face is Datum A. The top surface (toleranced feature) should be exactly parallel to it. Drag sliders to simulate taper/bow/roughness errors and see the tolerance zone in action.

• Parallelism is always measured relative to datum — not self-referencing like flatness
• A perfectly flat surface can still fail parallelism (if the whole surface is tilted relative to datum)
• A surface can pass parallelism but fail flatness (if bow is within the parallel zone)
• Parallelism tolerance must be ≤ size tolerance between the surfaces (Rule #1)

Drag the Actual X/Y sliders to move the hole. The circular GD&T zone and the equivalent ± square zone are both shown. Toggle between single-hole and bolt-circle (6-hole) pattern views.

Shows whether a bolt (fixed diameter) can physically pass through the displaced hole. MMC bonus tolerance directly corresponds to extra assembly clearance. Drag the bolt size and see how position error interacts with assembly fit.

• GD&T circular zone accepts 57% more parts than equivalent ± square zone at same corner allowance
• TP = 2 × radial deviation — the factor of 2 converts radius to diameter to match ⌀ zone
• With Ⓜ: total tolerance = stated tol + bonus (hole growth from MMC)
• Basic dimensions locating the hole are theoretically exact — all tolerance comes from the FCF, not from ± on the dimension

Each Z-slice has a median point. All median points must fall within the ⌀tol cylindrical zone centred on datum A. Left: XY cross-section with median point cloud. Right: axial scatter.

Concentricity is used when rotating mass balance matters. This simulation shows the relationship between eccentricity (off-centre mass) and the dynamic imbalance force at speed. Drag sliders to see why concentricity matters for turbines and crankshafts.

• Concentricity: use only when rotating mass balance matters (turbine discs, crankshafts) — the median axis must be coaxial to avoid unbalanced rotating mass
• For most assembly fit applications use circular runout instead — it is far easier to inspect and controls the same assembly effect
• Concentricity inspection requires finding median points from diametrically opposed CMM measurements at each Z-slice — not a shop-floor test
• Coaxiality (3D version) is the preferred ASME Y14.5-2018 term for cylindrical features

A slot is shown with Datum A as the center plane. CMM measures opposing surface pairs and computes median points. All median points must lie within ±t/2 of datum A. Drag sliders to offset and tilt the slot.

Shows a key mating with a shaft slot. Symmetry error shifts the slot centre — if the shift exceeds the assembly clearance, the key binds or won't fit. Drag sliders to see the relationship between symmetry tolerance and key fit.

• Symmetry is the planar equivalent of concentricity — applied to width features (slots, keys, tabs)
• Requires CMM measurement of mid-points between opposing surfaces at multiple stations
• ASME Y14.5-2018: Position with two-plane zone achieves the same control and is easier to inspect — preferred for production
• Retained in ISO 1101 — important on drawings following ISO standards

Drag sliders to shape the true profile (spline curve) and set tolerance. Switch between bilateral and unilateral zones. Each measured point on the cross-section must fall within the offset tolerance band.

• Profile of a line is evaluated at each individual cross-section — there is no constraint between cross-sections
• Use when a surface is extruded (constant cross-section) or when only 2D form matters
• Use profile of a surface for full 3D control
• Without a datum reference, controls only form. With datum — controls form + orientation + location.

Drag the sliders to set the total tolerance and see how the same value splits differently between bilateral and unilateral zones. Unilateral zones are used when material removal in one direction only is permitted (e.g. aerodynamic surfaces where adding material outward is not allowed).

Shows a free-form airfoil cross-section. The green uniform-thickness zone surrounds the true CAD profile. Each CMM probe point is colour-coded. Drag sliders to simulate machining deviation and see which regions fail.

• Most commonly inspected on a CMM with CAD comparison — the true profile comes from the 3D model
• Can replace all other controls (position, perpendicularity, flatness) for complex features
• Bilateral zone is default; use Ⓤ modifier for unilateral zone specification
• Requires datums for full constraint — without datums, only form is controlled

Simulates a CMM scanning a turbine blade cross-section. The probe path sweeps across the surface, measuring deviation at each point normal to the true profile. Watch how tool wear (global offset) and chatter (waviness) produce different failure patterns — and see the pass/fail map update in real time.

Simulates a dial indicator riding on a rotating shaft cross-section. The gauge trace sweeps 360°. Left panel shows the physical shaft cross-section view. Right panel shows the full indicator reading (FIM) chart — the measurement technician sees this.

• Circular runout includes both circularity (form) and coaxiality (location) errors combined
• Easiest runout to inspect — one indicator, one rotation per cross-section
• Preferred over concentricity for most rotating assembly applications
• Cannot separate form errors from location errors — if this distinction matters, use circularity + position separately

Circular runout directly affects lip seal life and leakage. As the shaft rotates, each FIM cycle flexes the seal lip. Higher runout = larger flex amplitude = faster seal fatigue. This simulation estimates seal contact pressure variation and relative wear rate for a given runout error.

Shows the same shaft inspected by both methods. A tapered or barrel-shaped shaft may pass circular runout at every individual cross-section, but fail total runout because the annular cylinder must encompass the entire surface simultaneously.

• Total runout = cylindricity + coaxiality — orientation + location + form all together
• Measured by sweeping the indicator over the full surface during continuous rotation
• Common on precision spindles, turbine rotors, camshafts
• Total runout tolerance must always be ≥ circular runout tolerance on the same surface

Total runout on a bearing journal directly causes periodic radial displacement of the spindle during rotation. This shows the vibration waveform seen by the bearing and how taper/wobble creates additional axial-sweep errors that circular runout misses. The displacement amplitude = total FIM / 2.

A rigid body in 3D space has 6 degrees of freedom (DOF): 3 translations (X, Y, Z) and 3 rotations (Rx, Ry, Rz). The 3-2-1 rule fully constrains all 6 DOF using three datums:

• Primary datum: largest, most stable surface — 3 highest points contact the datum plane
• Secondary datum: longest edge perpendicular to primary — 2 points contact
• Tertiary datum: short edge, stop — 1 point contact
• Datum order matters — always qualify parts in A → B → C order (same as the FCF)

• True DRF (Theoretically Exact): Three mutually perpendicular planes derived from the datum features. Exists as a mathematical construct, not a physical object.
• Datum Feature Simulator: The physical surface or tool that establishes the datum (surface plate, pin, CMM probe, fixture locator). Must be of higher accuracy than the tolerance it establishes.
• Basic Dimensions: Theoretically exact dimensions (TED) — boxed numbers — that locate features relative to the DRF. They have no tolerance themselves; all tolerance comes from the GD&T callout.
• Datum features must be identified on the highest-quality surfaces that are accessible for measurement and stable for fixturing — not free-floating or deformable surfaces.

Bonus tolerance makes physical sense: a larger hole can be further off-center and still accept a bolt. As the hole grows (moves away from MMC), the mating pin has more clearance — hence more positional tolerance is allowed.

• Use Ⓜ on position tolerances for clearance holes that accept fasteners (bolts, screws)
• Use Ⓜ on orientation tolerances (perpendicularity of threaded holes) for assembly fit
• Functional gauge concept: an MMC callout can be verified with a hard gauge (fixed size pin gauge)
• Do NOT use Ⓜ on form tolerances (flatness, circularity, cylindricity) — they are always RFS
• Do NOT use Ⓜ on runout tolerances — always RFS

• Less commonly used than MMC — primarily for minimum edge distance and wall thickness control
• Cannot be verified with a simple hard gauge — requires variable measurement
• LMC is often misunderstood on the shop floor — add a note explaining the intent when using it

• RFS is the default in ASME Y14.5-2018 — no symbol needed (the Ⓢ symbol is rarely used in practice)
• Form tolerances (flatness, circularity, cylindricity, straightness) are always RFS — no modifiers allowed
• Runout tolerances are always RFS — no modifiers allowed
• Profile tolerances are typically RFS unless combined with a size feature
• In older drawings (ANSI Y14.5M-1982), RFS had to be explicitly called out — be careful reading legacy prints

Enter basic dimensions, measured actual locations, and tolerance. The calculator computes the diametral position error and pass/fail result.

Enter hole size limits and stated position tolerance. A table shows bonus tolerance at each size step.

Enter up to 8 dimensions with nominal value and bilateral tolerance ±. The calculator computes the resultant gap/interference using both methods.