A part can measure within tolerance on every basic size dimension and still fail at assembly. The holes are the right diameter. The plate is the right thickness. But the hole pattern sits a few thousandths off from where the mating part expects it, and the bolts will not drop through.
That is the gap GD&T for CNC machining is meant to close. For buyers sourcing machined parts, understanding GD&T basics helps explain why two parts with similar dimensional tolerances can perform very differently in an assembly.
What GD&T Controls
GD&T stands for Geometric Dimensioning and Tolerancing. It is a language of symbols used on engineering drawings to define how part features must relate to one another and to the function of the finished component.
In U.S. manufacturing, GD&T commonly follows ASME Y14.5-2018. International drawings may instead use the ISO Geometrical Product Specifications system, including ISO 1101. Both address geometric tolerancing, although they differ in some details.
Conventional dimensional tolerances tell a machinist how large or small a feature may be. GD&T adds control over characteristics including form, orientation, location, profile, and runout.
Datums are another important part of understanding GD&T basics for machined parts. A datum is a theoretically exact reference. The datum feature is the physical surface or feature on the part used to establish that reference. Under ASME Y14.5, Feature control frames identify datums with letters, typically A, B, and C.
Datums create the reference framework for geometric controls that depend on relationships between features. Form controls such as flatness and circularity generally do not require a datum.
Why GD&T Matters for CNC Machining
When dimensions are chained together, their allowable variation can accumulate. That tolerance stack may create more variation at the end of the chain than the assembly can accept.
On a simple bracket, that may not matter. On a housing that must locate a bearing, seal against a mating face, and bolt accurately to another structure, it can matter a great deal.
GD&T also establishes a clearer reference framework for inspection.
A true position tolerance referenced to datums A, B, and C establishes a common framework for locating and measuring a feature. That gives the machine shop and the customer’s inspection team the same basis for interpreting what the drawing requires.
It also tells the manufacturer which relationships matter most to function. If a bearing bore controls how the assembly operates while another feature only provides clearance, the machining and inspection plan can reflect that difference.
Common GD&T Symbols on Machined Parts
Flatness. Controls how much a surface may deviate from a perfect plane. It is commonly used on sealing faces, mounting surfaces, and other surfaces that need to sit flush. Flatness is a form control and does not require a datum.
Circularity. Controls roundness of a circle at individual cross sections of a cylindrical feature. It may be used on shafts, bores, and features involved in rotating or sealing applications.
Perpendicularity. Controls how square a surface, center plane, or axis is relative to a datum. Typical applications include bores that must remain square to a mounting face and walls that must stand perpendicular to a base.
Parallelism. Controls how well a surface, center plane, or axis remains parallel to a datum. It can be important on clamping faces, slide surfaces, and opposing surfaces that must maintain a consistent relationship.
Position. Controls the variation of a feature’s axis or center plane relative to its location defined by basic dimensions to a datum reference frame. Position is commonly used for bolt patterns, dowel holes, locating pins, and other features that must align with mating components.
Runout. Controls variation in a surface as the part rotates around a datum axis. Circular runout evaluates individual cross sections, while total runout controls variation across the full surface. Typical applications include shafts, spindles, and bearing-related features.
Profile. Controls a surface or contour relative to its theoretically exact shape. Profile is particularly useful for complex geometry that would otherwise require numerous individual dimensional controls.
GD&T and Plus-Minus Tolerances Work Together
GD&T and conventional dimensional tolerancing are not competing systems. Most machined-part drawings use both.
Feature size is often controlled with conventional dimensional tolerances. GD&T adds control over characteristics such as form, orientation, location, profile, and runout.
One GD&T concept that can directly affect manufacturability is maximum material condition (MMC).
When MMC is applied to a positional tolerance, it links the feature’s location deviation to its actual manufactured size. This grants “bonus tolerance”, which is positional tolerance that is added to the stated tolerance as the actual size of the feature moves away from maximum material condition.
Consider a hole. For the hole, MMC is its smallest allowable diameter. As the actual hole becomes larger, additional positional tolerance may become available while ensuring the assembly can still function.
For example, a hole has a size limit of 5.00 mm to 5.20 mm (MMC is 5.00 mm) and a positional tolerance of Ø 0.10 mm Ⓜ. If manufactured at 5.00 mm, bonus tolerance is 0.00 mm, so total positional tolerance is still 0.10 mm. If manufactured at 5.10 mm, bonus tolerance is 0.10 mm, so total positional tolerance is 0.10 + 0.10 = Ø 0.20 mm.
That gives the manufacturer more room to produce an acceptable part without compromising the functional requirement.
When GD&T Makes Sense
GD&T is most valuable when a feature has a functional relationship that needs to be controlled.
Common examples include:
- Bolt hole patterns that must align with mating components
- Sealing surfaces and gasket faces
- Bearing bores and bushing fits
- Rotating components where runout matters
- Locating features such as dowel holes and pins
- Stacked assemblies where variation can accumulate across several parts
- Complex profiles where multiple surfaces must maintain a defined relationship
It does not need to be applied to every feature on every part.
The test is simple: ask what happens if the feature is off. If there is no functional relationship that requires geometric control, a conventional dimensional tolerance may be enough.
GD&T Mistakes That Can Increase Machining Cost
Missing or unclear datums. Position and other geometric controls generally require appropriate datum references to establish how features are located and oriented. Missing or poorly selected datums can make a part harder to manufacture and inspect consistently.
Poorly selected datum features. Datum features should provide a stable, repeatable reference and reflect how the part functions or mates in the assembly. A rough saw-cut edge or a surface that disappears during machining may create unnecessary setup problems.
Tolerances tighter than function requires. If a clearance hole only needs 0.010″ of positional control to function, specifying 0.0005″ creates additional machining and inspection demands without improving the assembly.
Conflicting or redundant requirements. Combining geometric controls and dimensional tolerances that impose competing requirements on the same geometry can create uncertainty during machining and inspection. Profile, for example, is normally defined using basic dimensions rather than competing plus-minus dimensions on the same geometry.
Overuse. Adding geometric controls to features that do not need them adds quoting, machining, and inspection work without improving part performance.
How GD&T Affects Machining Cost
GD&T for CNC machining can either reduce manufacturing cost or increase it. The difference is how well the tolerances match the actual function of the part.
Tighter or more complex geometric requirements can change how a part must be fixtured, how many machining operations are required, which processes are appropriate, and how much inspection is needed. Scrap risk can increase as the allowable manufacturing window gets smaller.
Applied well, GD&T can work the other way.
Datum structures built around part function can make manufacturing and inspection planning clearer. MMC can provide additional tolerance where the assembly allows it. Controlling the relationships that actually matter can provide more manufacturing freedom than simply tightening every dimension on the print.
For reference, Kiski Precision Industries holds 0.002″ true position across 150-piece military production runs, 0.003″ profile over 50″ on aerospace work, and 0.0003″ flatness and parallelism directly from CNC machining without a grinding operation. Finished parts are verified with in-house CMM inspection.
The best drawing gives the manufacturer more than numbers. It communicates what the part has to do.
When requesting a quote, identify the features that must fit, seal, locate, or run true and the features that are less critical to function. That context helps the manufacturing team understand where precision matters most and quote the part accordingly.