GD&T basics for machined parts
Connect datums, feature controls and inspection to how a machined part assembles. Understand position, basic dimensions and material-condition modifiers through practical examples.
Start with function and the governing drawing standard
Geometric dimensioning and tolerancing describes permitted variation in shape and feature relationships. It helps a drawing communicate why a part must fit, locate, rotate or seal; it does not require every surface to receive the tightest possible control.
Assembly
Identify the interfaces
Mark the seating face, locating bore or pin, mating shoulder and clearance features. A cosmetic outside edge may need much less control than a locating feature.
Drawing
Choose one interpretation system
State the governing standard and edition. ASME identifies Y14.5-2018 (R2024) as its current reaffirmed edition. ISO GPS uses a coordinated set of standards, not simply interchangeable symbols.
Verification
Make the requirement measurable
Consider access to the datum features and controlled surfaces. Include the material condition and whether the drawing applies after coating, heat treatment or assembly.
An important default differs between systems: ASME Rule #1 generally couples size and perfect form at maximum material condition for applicable regular features of size, subject to its exceptions. ISO GPS generally applies independence unless a relationship such as an envelope requirement is specified. Do not translate an existing drawing by changing only the standard named in its title block.
The examples below are introductory ASME-style explanations. They are original teaching examples, not extracts from a standard or a complete specification for a production part.
Choose references that reproduce how the part seats
Make the setup follow the assembly
For this simple block, a primary seating face A, secondary side B and tertiary end C establish a repeatable orientation. The letters name actual datum features; the reference planes are theoretically exact.
Flatness and orientation are separate
A flatness zone may float around one surface. A parallelism zone is oriented to a referenced datum. A flat mounting face can still be tilted relative to another interface.
A datum feature is a physical feature on the part. The datum is the theoretically exact reference established from it. A fixture surface or measurement construction helps simulate that relationship; it does not make the manufactured face perfectly flat. Datum precedence matters: A then B then C can establish a different reference frame from B then A then C.
| Reference | Functional choice | What to resolve |
|---|---|---|
| Primary A | The mounting face that seats on the assembly. | Its actual contact region, access and required form. |
| Secondary B | The side that guides the part after it is seated. | Which direction it locates and whether it is actually the assembly interface. |
| Tertiary C | The end stop that establishes the remaining location. | Whether it is necessary for the controlled feature and accessible for inspection. |
For this simple planar arrangement, the familiar three-two-one concept constrains six rigid-body degrees of freedom. Cylindrical datums, patterns, targets and flexible parts require different reasoning; three arbitrary faces are not a universal datum system.
- Use a locating bore when that is how the part works. A turned housing may locate on a cylindrical interface and shoulder. Choosing an unrelated outer flat merely because it is easy to clamp can hide the functional relationship.
- Avoid references that disappear. A temporary machining face, burr or surface later removed by grinding is a poor final datum unless the drawing intentionally defines that intermediate state.
Use the control that answers the functional question
| Need | Control to consider | Important distinction |
|---|---|---|
| One mounting surface must be flat | Surface flatness. | A form control; it does not reference a datum or orient the face to another feature. |
| A face must remain parallel to a seat | Surface parallelism to the functional datum. | Orients its zone to a datum; it does not set the separation between the faces. |
| A hole must stand square to a seat | Axis perpendicularity, or a position control that also locates it. | Define whether the controlled feature is the axis or the surface. |
| A hole pattern must assemble to pins or screws | Position with appropriate basic dimensions and datum references. | Hole size, position and assembly clearance are separate but connected requirements. |
| A contoured face must follow CAD geometry | Profile with appropriate datum references and zone definition. | The references and definition determine whether form, orientation and location are controlled. |
| A turned surface must run accurately about a functional axis | Circular or total runout, as function requires. | Runout evaluates surface behavior about a datum axis; it is not simply another name for hole position. |
A roughness requirement is also different from flatness or profile. A surface can be smooth and bowed, or geometrically flat with visible tool marks. See surface roughness for texture requirements and the CNC design guide for tool access and finished fits.
Read the size, basic dimensions and position zone together
A diametral zone is not a ± radius
In a simple cross-section, a position zone of diameter 0.20 mm has radius 0.10 mm. Coordinate offsets of 0.08 mm and 0.06 mm lie exactly on that boundary; the whole axis still needs evaluation.
More hole size can permit more position variation
For the illustrated hole at MMC, diameter 6.00–6.20 mm and position diameter 0.20 mm at MMC give a 5.80 mm virtual-condition boundary. At the idealized 6.10 mm mating size, total position allowance is 0.30 mm.
For a simple hole, the size limits control its permitted diameter. Boxed basic dimensions define theoretically exact locations; they do not mean the hole must be manufactured with zero error. A geometric tolerance defines the allowed departure from that ideal relationship. A reference dimension, normally shown in parentheses, serves a different purpose and is not a substitute for a basic dimension.
For this simple cross-section, the diametral position result is 2 × √(ΔX² + ΔY²). Offsets of 0.08 mm and 0.06 mm give a 0.10 mm radial offset and a 0.20 mm diametral result. They sit on the edge of a diameter 0.20 mm zone. This coordinate calculation alone does not evaluate the whole hole axis, form, datum establishment, uncertainty or any material-boundary requirement.
| Drawing element | Example | Meaning |
|---|---|---|
| Hole size | Diameter 6.00–6.20 mm. | The independent size limits still apply. |
| Basic location | Theoretically exact X and Y offsets from the stated datum system. | Defines the ideal location; do not add an unrelated ± tolerance to the same location. |
| Position zone | Diameter 0.20 mm, relative to A, B and C. | A diametral cylindrical zone for the controlled axis, with the applicable standard interpretation. |
| Material modifier | No modifier, or MMC when function justifies it. | Determines whether the tolerance can vary with departure from the material limit. |
The circular cross-section of a position zone differs from independent ±X/±Y limits, which produce a rectangular zone. Replacing one with the other at the same printed number changes the acceptance region.
Keep feature tolerance and datum boundaries separate
Maximum material condition means the feature contains the most material allowed by its size limits: the smallest permitted hole or the largest permitted shaft. The placement of the modifier matters.
| State | Calculation | Result |
|---|---|---|
| At hole MMC | 6.00 mm hole; zero departure from MMC. | Diameter 0.20 mm position allowance. |
| At a 6.10 mm mating size | 0.10 mm departure + 0.20 mm stated position. | Diameter 0.30 mm total position allowance. |
| Virtual condition for this internal feature | 6.00 mm MMC − 0.20 mm position at MMC. | Diameter 5.80 mm functional boundary. |
The simplified example assumes the appropriate mating-size evaluation and an otherwise conforming feature. One caliper reading does not establish the mating envelope or prove compliance; the size limits and applicable boundary requirements remain in force.
- A modifier after the tolerance applies to the controlled feature. In ASME practice, MMC can permit additional geometric tolerance as the feature departs from MMC. Do not automatically apply it to a bearing bore or other interface whose function requires tight alignment regardless of size.
- A modifier after a datum reference applies to its boundary. For an eligible datum feature of size, maximum material boundary concerns the datum simulator and may permit datum-reference-frame mobility. It is not an extra tolerance to add independently to every controlled hole.
- No modifier also has a meaning. For an applicable ASME position tolerance, the default is regardless of feature size; an eligible datum feature reference defaults to regardless of material boundary. RFS and RMB describe different parts of the requirement.
Tie the drawing to the delivered manufacturing state
| Situation | Clarify | Why it affects the plan |
|---|---|---|
| Anodized or plated locating bore | Final size and geometric requirements after the specified finish; identify masking. | Deposits and conversion layers affect the delivered interface differently. |
| Heat-treated shaft | Which diameters, shoulders and datum surfaces are finished after treatment. | A pre-treatment inspection does not establish the final geometry. |
| Thin plate clamped during inspection | Free or restrained state and defined support/clamping conditions. | Clamping can hide distortion or create a different result from assembly. |
| Part machined in several setups | Functional references that remain available throughout the route. | The manufacturer may use process datums, but final acceptance must address the drawing datums. |
| Hole used to locate a long mating pin | Functional engagement, orientation and any necessary projected requirement. | Checking one circle near the entrance may miss axis tilt over the engagement length. |
Specify the result without prescribing an unnecessary machine or fixture. The shop can propose a manufacturing route; changing the datum system or acceptance condition requires design approval.
Agree how the tolerance will be evaluated
A CMM report is useful only when its alignment, sampled features and evaluation match the requirement. GD&T defines product requirements; it does not automatically select a complete measurement plan.
Establish
Reproduce the datum system
Identify contact surfaces, precedence, datum targets or material boundaries. Record the relevant part condition and support arrangement.
Measure
Sample the feature that matters
Plan probe access and coverage of the controlled surface or axis. A few convenient points may miss form error or a tilted bore.
Evaluate
Report the requirement and result
Connect results to drawing identifiers, limits, units, datum references and material modifiers. Include the agreed treatment of measurement uncertainty near an acceptance limit.
A functional gage may be useful for a repeated assembly-boundary requirement; a CMM may provide richer location information; a surface-plate setup may suit some simple checks. Choose a capable method for the characteristic instead of requesting a machine name as proof of quality. A functional gage by itself may not verify every local-size or form requirement.
Review one real assembly before releasing the drawing
- Identify the functional chain. Show what seats first, what locates second and where motion or clearance is intended. Tie each critical control to that assembly need.
- Resolve the drawing system. State the standard/edition, units, general notes, CAD/drawing precedence and revision. Remove contradictory title-block or legacy notes.
- Check every control for completeness. Verify the feature attachment, zone shape, value, basic dimensions, datum order and appropriate modifier. Avoid an undefined datum or a missing location.
- Review the tolerance together with the mate. Check worst-case size and location effects, not just nominal CAD alignment. Consider whether the fastener floats, is fixed or must locate the assembly.
- Confirm final-state inspection. Include finish/heat treatment, measurement state, required report and inspection scope before ordering. Keep non-functional features proportionate to their role.
Use the machining design guide to check access and geometry, then carry the accepted datum and fit requirements into the quotation package.
Frequently asked questions
What does GD&T add to ordinary dimensions?
Size dimensions define permitted size; geometric controls define permitted form and feature relationships. A mounting face can meet a thickness dimension and still be tilted or bowed. Use the controls that reflect the assembly function under the selected drawing standard.
Does a basic dimension have zero manufacturing tolerance?
No. A basic dimension is theoretically exact and locates or defines the ideal geometry. The related geometric tolerance provides the allowed variation. It should not be confused with a reference dimension or treated as a zero-error coordinate.
Is position diameter 0.20 mm the same as ±0.20 mm?
No. In a simple cross-section, a diameter 0.20 mm circular zone has a radius of 0.10 mm. Independent plus/minus coordinate limits produce a different-shaped acceptance zone. Evaluate the actual control, datum system and full feature.
Should every hole use maximum material condition?
No. MMC is useful when the assembly function permits greater geometric variation as the feature departs from maximum material. A precision alignment or bearing interface may need control regardless of size. Choose the modifier from function, not as an automatic cost-saving label.
Can I use ASME and ISO GD&T interchangeably?
No. Similar symbols can carry different defaults or interpretation rules, including the relationship between size and form. Name the governing standard and edition, and deliberately translate requirements when changing systems.
Does requesting a CMM report guarantee the drawing is verified?
No. The method must use the correct datum system, feature coverage, evaluation and acceptance conditions. Agree what the report covers and how results correspond to drawing requirements; a machine name alone does not establish a valid inspection.
Sources and further reading
- ASME — Y14.5 Dimensioning and TolerancingOfficial listing of Y14.5-2018 (R2024); consult the applicable standard for complete rules and exceptions.
- ISO 8015 — GPS fundamentalsOfficial scope of the ISO GPS interpretation framework.
- Mitutoyo — CMM and GD&T measurement planningMeasurement planning and ASME/ISO default differences; this educational handout predates the current ASME edition.
- KEYENCE — datum fundamentalsDistinguishes the physical datum feature and exact reference.
- KEYENCE — form tolerancesForm-control zones; illustrations here are independently drawn.
- KEYENCE — orientation tolerancesDatum-related orientation and its difference from flatness.
- KEYENCE — maximum material conditionMaterial condition and additional geometric allowance; use the governing standard for detailed evaluation.
- PTC — ASME datum feature material-boundary modifiersDatum boundaries and the distinction between MMC/MMB and feature tolerance.
Specify the details that make the part work.
Upload your CAD and drawing with the material, quantity, finishing and critical dimensions. Confirm the manufacturing route before production.