Worked Drawing Examples
Five complete parts with their feature control frames, the function behind each control, and how each is inspected: bracket, shaft, flange, housing and sheet-metal cover.
The best way to learn GD&T is to read finished drawings. This page works through five complete parts. For each one it lists the controls that would be on the drawing, in the form of real feature control frames, and gives the function behind each control, the reason for the choice, and how it would be checked. The numbers are examples, not recommendations for a specific product, and the layout follows ASME Y14.5-2018. It is part of the GD&T guide.
How to read these examples
- Function first. Every control exists because of something the part has to do: seal, locate, turn, assemble. Start from the function, then choose the control.
- Datums come from how the part is used. The primary datum is the surface or axis that the part actually sits on or turns about; the later datums are the next contacts.
- Fewest controls that do the job. A control that is not needed costs money to make and check.
- Each table lists the frame, the function, why this control, and how it is inspected. See the other pages for the detail: datums, form, orientation, position, profile and runout, modifiers and inspection.
Example 1: a mounting bracket
An L-shaped steel bracket bolts to a frame through four M6 clearance holes in its base, and a vertical flange carries a sensor on two slots. The base sits on the frame, the long edge pushes against a stop, and the short edge against another.
| Feature | Frame | Function and reason | Inspection |
|---|---|---|---|
| Base underside (datum A) | It is the mounting face. Flatness stops it from rocking on the frame, and it is the primary datum. | Surface plate and indicator | |
| Long edge (datum B) | The stop face. It is the secondary datum, so it needs to be square to A first. | Square on the plate; indicator | |
| Short edge (datum C) | The third contact, square to A and B. Looser, as it only stops rotation. | CMM | |
| Four M6 holes ⌀6.6 to 6.8 | Floating bolts: T = H − F = 6.6 − 6.0 = 0.6. MMC lets the hole move as it gets larger. | Functional gage with ⌀6.0 pins (virtual condition 6.6 − 0.6) | |
| Sensor slots 8 wide | The sensor has to be aligned to the long edge, not to the short edge. | Gage pin or CMM | |
| Vertical flange face | The sensor looks along this face, so it has to be square to the base. | Square and indicator |
- Why Ⓜ on the holes? The bolts are loose in the holes, so a larger hole leaves room for more position error. The bonus makes the part cheaper without hurting assembly.
- Why no modifier on the slot position? A sensor is aligned by its slot; with MMC the sensor could end up shifted. Where precise alignment counts, RFS is the safe choice.
- What the drawing does not need: flatness of the flange face, the edge straightness, or a location of the flange to C. Each would add cost without changing function.
Example 2: a stepped shaft
A ⌀25 shaft turns in two bearings (the journals), carries a ⌀30 bearing seat for a third bearing, a shoulder that a gear pushes against, and a keyway.
| Feature | Frame | Function and reason | Inspection |
|---|---|---|---|
| Journals ⌀25 (two, datum A and B) | The shaft turns on these two diameters. Together they define the datum axis A-B, so their form matters. | Roundness tester | |
| Bearing seat ⌀30 | The third bearing must run true to the journals. | V-blocks and indicator, or between centers | |
| Shoulder face | The gear sits on this face. Total runout combines flatness and squareness to the axis. | Indicator across the face while turning | |
| Gear seat ⌀40 | Gear mesh depends on the gear running true. | Same set-up | |
| Keyway 8 wide | It has to be centered on the axis so the key sits symmetrically. ASME 2018 uses position (no symmetry symbol). | CMM or keyway gage |
- Why a common datum axis A-B? Two short journals define the axis better than any one of them: a shaft turns about the line through both bearings.
- Why runout and not position? The surfaces are round and they rotate. Runout reads the thing that causes vibration, and it can be checked on the lathe.
- Size and form of the journals are covered by the limits of size (Rule #1), so only cylindricity is added, and only where a tighter form than the size tolerance is needed.
Example 3: a bolted flange
A round pump flange has a central bore that locates on a spigot, a face that seats on a gasket, and six M8 bolt holes on a bolt circle. See the datums page for the datum scheme.
| Feature | Frame | Function and reason | Inspection |
|---|---|---|---|
| Mating face (datum A) | It seals on a gasket. The primary datum, and it needs to be flat. | Surface plate | |
| Central bore ⌀50.000 to 50.025 (datum B) | It locates the flange on the spigot, so it must be square to the face. | Pin gage (⌀49.95) square to the face | |
| Six M8 holes ⌀9.0 to 9.2 on a ⌀100 circle | T = H − F = 9.0 − 8.0 = 1.0 for floating bolts. B at MMC lets the pattern shift as the bore gets larger. | Functional gage on a ⌀49.95 locating pin with six ⌀8.0 pins | |
| Rim face | The flange spins on a shaft in some uses, so the face must not wobble. | Indicator on a mandrel | |
| Outer diameter ⌀140 | The outline only needs to be near nominal, not tight. | CMM |
- Bolt hole tolerance: the six holes on the bolt circle are a pattern, so a single frame applies to all of them (“6X”). The pattern is located to the datum bore, not to one hole.
- Why bore B with MMC? It is a datum at MMC (Ⓜ): the bore can be as large as ⌀50.025, and the bore may float around the ⌀49.95 gage pin by up to 0.075 in total (50.025 − 49.95), and the pattern moves with it. That keeps good parts from failing.
- Fixed-diameter gage: a gage with a ⌀49.95 locating pin (the virtual condition of the bore with 0.05 of perpendicularity: 50.0 − 0.05) and six ⌀8.0 pins is a one-step check.
Example 4: a housing with parallel bores
A gearbox housing has two parallel bores ⌀32.000 to 32.025 (H7) that carry the shafts of a gear pair. Their distance and parallelism decide how the gears mesh. The base is datum A and the side face datum B.
| Feature | Frame | Function and reason | Inspection |
|---|---|---|---|
| Base (datum A) | The housing bolts to a plate by this face. | Surface plate | |
| Side face (datum B) | The second contact, square to the base. | Square, indicator | |
| Bore 1 | Locates the first shaft in the housing. | Gage pin at ⌀31.95 (virtual condition) and a CMM | |
| Bore 2 | Locates the second shaft. The same frame means the center distance is controlled by the two. | Same gage | |
| Bore 2 to bore 1 (in the gear plane) | The axes must be parallel, or the teeth would not make contact over the full width. | CMM, or two precision pins at a set distance | |
| Cover face | It seals with a gasket. | Surface plate |
- Center distance: each bore may be 0.05 from nominal at MMC. The center distance can vary by ±0.025 + ±0.025 = ±0.050 at MMC. At LMC (⌀32.025) each bore gains the 0.025 bonus, so the zone is ⌀0.075 and the center distance may vary by ±0.075 in the worst case. The designer should check that the gears accept it.
- Datum C in the parallelism frame is bore 1’s axis, so bore 2 is aligned to the first shaft.
- Would a ⌀0.05 position be too tight? For a ground or bored H7 it is typical of a precision housing; for a casting it would not be reachable and a larger value (0.15 to 0.3) would be used.
Example 5: a formed sheet-metal part
A 2 mm aluminum cover is bent from a flat blank, with a flange and four screw holes. It does not sit on a precise flat face, because the part springs back, so it is located on datum targets.
| Feature | Frame | Function and reason | Inspection |
|---|---|---|---|
| Datum targets A1, A2, A3 (three points), B1, B2 (two points), C1 (one point) | Targets (no frame) | Hold the part the way it will be held in the assembly: three points for A, two for B, one for C. Real surfaces are not flat. | A fixture with pins at the target points |
| All surfaces (general profile) | A loose general profile keeps the shape near the model. Marked “all over” on the drawing. | CMM or fixture with a scan | |
| Flange face | The face that seals against the housing must be tighter than the rest. | CMM | |
| Four screw holes ⌀4.5 to 4.7 | Screws M4 float; T = H − F with H = 4.5 (ISO 273 medium fit) and F = 4.0 gives 0.5. | CMM; or a gage with ⌀4.0 pins | |
| Whole part | Ⓕ in the notes | Springy parts are measured free (no clamping), and again restrained, with separate limits. | Fixture, with and without clamps |
- Why datum targets? A bent surface is not flat; three points define a plane exactly where the part will really sit. This repeats between inspectors.
- Profile first, then size. Sheet-metal features follow the shape of the model, so profile (not ± dimensions) is the control: it gives a zone around the shape that includes bend angle and flange position.
- Free state. Springback makes the part different when clamped; stating free state in the notes says which one counts.
Drawing review checklist
- Datums: are they real features the part is held on, listed in an order that matches its use? Is the primary one a surface or axis that can be simulated (a gage or fixture)?
- Every dimension toleranced: each feature has a ± tolerance, a feature control frame or a general note; none is left open. Basic dimensions have a frame that controls them.
- Size and form: Rule #1 applies by default: add form controls only where they are tighter than the size limits imply.
- Material conditions: Ⓜ on features that assemble with clearance, Ⓛ where wall thickness matters, and RFS (no symbol) where the position must be exact.
- Zone shape: a diameter symbol on a hole’s position, none on slots and tabs.
- Patterns: “4X” or “6 HOLES”, a single frame, a common datum scheme. Composite or two single-segment frames if the pattern and the individual holes have different needs.
- Inspectable: could someone check each control with a gage or a CMM in a reasonable time?
- Cost: are there any tolerances that are tighter than the function needs? Use the loosest value that works.
- Fit: does the stack-up of the assembly work in the worst case? See Inspection and Tolerance Stack-up.
- Standard: is the standard and year named (ASME Y14.5-2018) on the drawing?
Common mistakes
| Mistake | Why it is a problem | Fix |
|---|---|---|
| Using ± on a located hole and also a position | The two controls conflict, and the square zone is a poor fit for a round hole | Basic dimension plus position |
| Datum that cannot be simulated (a small cast spot) | Inspectors set the part up differently and get different results | Use datum targets or a larger machined surface |
| Flatness larger than the size tolerance on a feature of size | The control is meaningless: the size limits already hold the form tighter | Make the form tolerance smaller, or remove it |
| Ⓜ on a feature that is pressed or must be exact | Bonus lets the part drift when the fit needs it fixed | RFS |
| Everything referenced to the same one datum | The part is not fully located, and parts can differ in the other directions | A full frame A | B | C where location matters |
| Tolerance tighter than the process can make | Scrap and cost | Check the process capability; loosen, or change the process |
| Concentricity or symmetry on a 2018 drawing | They were removed from ASME Y14.5 in 2018 | Position or runout |
FAQ
Can I copy these frames onto my own drawings?
Use them as a pattern, not a copy. The values depend on the function, the process and the fit of your own assembly.
How many controls does a typical part need?
A simple part might have five to ten frames, a complex housing twenty or more. If a part has fifty frames, it is probably over-specified.
Should every dimension be basic?
No. Size dimensions of features of size keep their ± limits. Basic dimensions locate features or define a true profile, and carry a tolerance in the frame.
What if the supplier cannot hold the tolerance?
Talk to them early: the process capability sets the least a feature can cost. Loosen the tolerance if the function allows, or choose a different process.
Do these examples follow ISO or ASME?
ASME Y14.5-2018. ISO 1101 uses the same symbols, but defaults differ (independency instead of Rule #1, for example), so check with the standard on the drawing.
Related
- GD&T: the overview and quick reference.
- Datums and Datum Reference Frames
- Position and Location
- Profile and Runout
- Inspection and Tolerance Stack-up
References
- ASME Y14.5-2018, Dimensioning and Tolerancing, including its figures of worked parts.
- ASME Y14.5.1M, Mathematical Definition of Dimensioning and Tolerancing Principles.
- ISO 1101, Geometrical tolerancing; ISO 5459, Datums and datum systems.
- Meadows, J. D., Geometric Dimensioning and Tolerancing: Applications, Analysis, Gaging and Inspection, CRC Press.
- ISO 273, Fasteners: clearance holes for bolts and screws.
Last reviewed: October 2026. The parts on this page are illustrations; numbers must be checked against the real design.