GD&T Examples: 10 Real Engineering Drawings Annotated and Explained

Theory Makes Sense When You See It on a Drawing

GD&T (Geometric Dimensioning and Tolerancing) textbooks teach you the rules. But the real learning happens when you look at an engineering drawing and can read, interpret, and explain every callout in the feature control frames.

The following 10 examples represent the types of GD&T applications you will see on real production drawings. Each one covers a specific scenario, the GD&T applied, why that tolerance was selected, and how you would inspect it. The examples progress from simple to complex.

Example 1: Flatness on a Mounting Plate

Scenario: A steel mounting plate bolts to a machine frame. The bottom surface is the primary contact face and must sit flush against the frame to distribute clamping load evenly.

GD&T applied: [⏥ | 0.05] on the bottom surface.

Why this tolerance: Flatness controls the surface shape independently. No datum is needed because the concern is the surface’s own planarity, not its relationship to other features. The 0.05 mm tolerance prevents the plate from rocking or creating uneven contact when bolted down.

How to inspect: Place the plate on a granite surface plate. Sweep a dial indicator across the bottom surface. The difference between the highest and lowest readings is the flatness error. On a CMM (Coordinate Measuring Machine), take a grid of points across the surface and evaluate using minimum zone or least squares fitting.

Example 2: Perpendicularity of a Dowel Pin Hole

Scenario: A cast aluminum housing has two dowel pin holes used to locate it on a mating component. The holes must be perpendicular to the mounting face so the pins engage straight and the housing aligns correctly.

GD&T applied: [⟂ | ⌀0.05 | A] on each dowel hole, where datum A is the mounting face.

Why this tolerance: Perpendicularity ensures each hole axis is within 0.05 mm of being perfectly perpendicular to datum A. If the holes are tilted, the pins won’t engage properly and the housing will be misaligned.

How to inspect: On a CMM, measure multiple points along the bore of each hole to establish the actual axis. Calculate the deviation of the axis from perfect perpendicularity to datum A. The axis must lie within a ⌀0.05 mm cylindrical zone perpendicular to the datum plane.

Example 3: Parallelism of Opposite Faces

Scenario: A machined steel block has top and bottom faces that mate with other components in a stack. The top face must be parallel to the bottom face to maintain consistent stack height and prevent tilting.

GD&T applied: [∥ | 0.03 | A] on the top surface, where datum A is the bottom surface.

Why this tolerance: Parallelism controls both the orientation and the flatness of the top surface relative to the bottom. The 0.03 mm tolerance ensures the two faces are within 0.03 mm of being perfectly parallel.

How to inspect: Place the bottom face (datum A) on a surface plate. Sweep an indicator across the top surface. The total indicator variation is the parallelism error.

Example 4: True Position of a Single Hole

Scenario: A bracket has a single clearance hole for a mounting bolt. The hole must be in the correct location relative to the edges of the bracket so the bolt aligns with the mating threaded hole in the assembly.

GD&T applied: [⊕ | ⌀0.50 Ⓜ | A | B | C] on the hole. Datum A is the back face, datum B is the bottom edge, datum C is the left edge. Basic dimensions of 25.00 mm from B and 15.00 mm from C locate the theoretically exact hole center.

Why this tolerance: True position with a cylindrical tolerance zone at MMC (Maximum Material Condition) is the standard approach for clearance holes. The ⌀0.50 mm zone at MMC means that when the hole is at its smallest allowable size, the center must be within 0.50 mm of the true position. As the hole gets larger, bonus tolerance increases the allowable deviation.

How to inspect: Measure the hole’s actual diameter and center location relative to datums A, B, and C. Calculate the positional deviation: 2 × √(ΔX² + ΔY²). Add the bonus tolerance (actual hole size minus MMC size) to the stated tolerance. Compare the deviation to the total allowable tolerance.

Example 5: Circular Runout on a Bearing Journal

Scenario: A motor shaft has a bearing journal that supports a ball bearing. The journal surface must run true to the shaft’s axis to prevent vibration and premature bearing failure.

GD&T applied: [↗ | 0.02 | A-B] on the bearing journal surface, where datum A-B is the shaft axis established by two bearing surfaces at opposite ends.

Why this tolerance: Circular runout checks the eccentricity at each cross-section independently. A 0.02 mm FIM (Full Indicator Movement) ensures the bearing seat is round and concentric enough at every point to support the bearing without excessive radial load variation.

How to inspect: Mount the shaft between centers (representing datum axis A-B). Place a dial indicator on the bearing journal. Rotate the shaft one full turn. Record the FIM. Repeat at several cross-sections along the journal length. The highest FIM reading is the result.

Example 6: Profile of a Surface on a Cast Part

Scenario: An injection-molded plastic housing has a complex curved exterior surface that must match the CAD model closely for proper fit with adjacent panels in the assembly.

GD&T applied: [⌓ | 0.50 | A | B | C] on the exterior surface, with datums establishing the part’s location and orientation in the assembly.

Why this tolerance: Profile of a surface is the right choice for complex 3D shapes that cannot be described by simple geometric controls. The 0.50 mm tolerance creates a zone 0.25 mm on each side of the true profile (the CAD surface). With datums referenced, the profile tolerance controls not just shape but also orientation and location of the surface.

How to inspect: Scan the surface using a CMM, structured light scanner, or laser scanner. Align the scan data to the datum reference frame. Compare the scan data to the CAD model. Every point must fall within the 0.50 mm bilateral tolerance zone around the true profile.

Example 7: Angularity on a Chamfered Surface

Scenario: A precision machined part has a 30-degree chamfer on one edge. The chamfer angle is a functional feature that guides a mating component during assembly. The angle must be tightly controlled.

GD&T applied: [∠ | 0.10 | A] on the chamfer surface, with a basic dimension of 30° relative to datum A (the top face). Datum A is the flat surface adjacent to the chamfer.

Why this tolerance: Angularity controls how closely the actual chamfer conforms to the basic 30-degree angle. The 0.10 mm tolerance means the chamfer surface must lie between two parallel planes 0.10 mm apart, oriented at exactly 30° to datum A.

How to inspect: On a CMM, take points along the chamfer surface and calculate the plane. Evaluate the angular deviation from 30° relative to datum A. The surface must fit within the tolerance zone. Alternatively, use an angle plate and indicator setup referenced to datum A.

Example 8: True Position of a Four-Hole Bolt Pattern

Scenario: A flange has four bolt holes on a 75.00 mm bolt circle diameter, equally spaced at 90 degrees. The flange bolts to a mating flange, and all four holes must align with the corresponding holes in the mating part.

GD&T applied: [⊕ | ⌀0.40 Ⓜ | A | B] on all four holes. Datum A is the flat face of the flange. Datum B is the center bore. Basic dimensions locate each hole at 90° intervals on the 75.00 mm bolt circle relative to datum B.

Why this tolerance: True position at MMC is the standard method for bolt patterns. The cylindrical tolerance zone accounts for the fact that holes are round and bolts are round. MMC allows bonus tolerance as the holes open up, reflecting the additional assembly clearance that larger holes provide.

How to inspect: Measure each hole’s actual diameter and center coordinates relative to datums A and B. For each hole, calculate the positional deviation from its basic location. Apply bonus tolerance based on actual hole size. All four holes must individually pass the tolerance requirement.

Example 9: Total Runout on a Precision Shaft

Scenario: A stainless steel roller shaft for a printing machine must produce even contact pressure across its entire length. Any combination of eccentricity, taper, or surface irregularity would cause uneven print quality.

GD&T applied: [↗↗ | 0.025 | A-B] on the roller surface, where datum A-B is the shaft axis established by the two journal bearings.

Why this tolerance: Total runout captures all surface variation during rotation across the entire length of the roller. Unlike circular runout, which checks one cross-section at a time, total runout detects taper and axial waviness as well as eccentricity. The 0.025 mm tolerance ensures the entire roller surface runs true enough for consistent print contact.

How to inspect: Mount the shaft between centers (datum A-B). Place an indicator on the roller surface. Slowly sweep the indicator along the entire length while rotating the shaft. The total FIM across all positions is the total runout result.

Example 10: Composite Position on a Connector Pattern

Scenario: An electronic enclosure has a rectangular pattern of four holes for an electrical connector. The pattern must be reasonably well located on the enclosure (so the connector aligns with the cutout), but the holes within the pattern must be very precisely positioned relative to each other (so the connector pins engage all four mounting holes).

GD&T applied: A composite feature control frame with two lines:

• Upper line (PLTZF – Pattern Locating Tolerance Zone Framework): [⊕ | ⌀0.80 Ⓜ | A | B | C] — locates the pattern as a group relative to the datums.
• Lower line (FRTZF – Feature Relating Tolerance Zone Framework): [⊕ | ⌀0.25 Ⓜ | A] — controls the position of holes relative to each other.

Why this tolerance: Composite position separates two requirements: the pattern-to-datum relationship (which can be looser) and the hole-to-hole relationship within the pattern (which must be tight). The upper line allows the pattern to shift up to ⌀0.80 mm from its nominal position. The lower line requires each hole to be within ⌀0.25 mm of its nominal spacing relative to the other holes in the pattern.

How to inspect: Measure all four hole locations relative to datums A, B, and C. First evaluate each hole against the upper line tolerance (pattern location). Then evaluate each hole against the lower line tolerance (hole-to-hole spacing), which only references datum A for orientation. Both requirements must be satisfied.

Lessons from These Examples

Across these 10 scenarios, several patterns emerge:

• True position dominates. It appears in more examples than any other symbol because hole and pin location is the most common geometric control in manufacturing.
• Datums matter. Every non-form tolerance references datums, and the choice of datums directly affects how the part is set up for inspection and whether it passes or fails.
• MMC is common for assembly features. Clearance holes and pin locations almost always specify MMC because bonus tolerance reflects how the parts actually assemble.
• Measurement method follows from the GD&T. The tolerance type dictates the inspection approach. Runout uses indicators on rotating parts. Position uses CMM coordinate data. Profile uses surface scanning.
• Simpler is better. The best GD&T application uses the simplest tolerance that captures the functional requirement. Over-tolerancing adds cost. Under-tolerancing allows non-functional parts.

Frequently Asked Questions