GD&T Symbols Explained for Machined Parts
True position and MMC bonus tolerance, flatness, parallelism, perpendicularity, runout vs concentricity, profile, and datums — each symbol explained the way a machinist reads it.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 11 min read
On this page
Quick Answer
The symbols engineers actually put on machining drawings boil down to four jobs: location (true position), form (flatness), orientation (parallelism, perpendicularity), and runout. The one that matters most is true position — it controls where a hole or pin sits inside a cylindrical tolerance zone and, with an MMC modifier, earns “bonus tolerance” that lowers machining cost without loosening the fit. Concentricity is largely dead; use circular or total runout instead. This guide walks each symbol the way a machinist reads it, not the way a textbook lists it.
Why GD&T, and Why These Symbols
Traditional ± tolerancing stacks a coordinate box around every feature, and it mostly works — until holes must mate, faces must seal, or a bolt pattern must assemble every time. GD&T replaces the coordinate box with functional zones: a cylindrical zone for a hole’s axis, a planar zone for a face, a rotational limit for a shaft. The symbols below are the ones that actually appear on CNC machining drawings, grouped by the job they do. If you are new to the system, our GD&T basics guide covers the 14 symbols and the feature control frame first; this page is the deep dive on the ones that drive quotes.
For the full symbol vocabulary on a drawing — surface finish, holes, threads, and GD&T — see our engineering drawing symbols guide.
True Position: The Symbol That Replaces ±
True position controls where a feature’s axis, center, or derived median plane may lie relative to basic dimensions and datums — inside a cylindrical or two-dimensional tolerance zone rather than a square ± band. That shape is the whole point. A ±0.005 in tolerance on X and Y draws a 0.010 in square; a position tolerance of Ø0.010 in draws a circle of the same diagonal — it lets the hole’s center wander anywhere within a round zone that matches how a pin and hole actually fit. For holes, pins, and bolt patterns, true position usually wins over ± tolerancing because it separates size from location: a hole can be slightly larger yet still function if its center stays in the zone.
The modifier that makes position genuinely cost-effective is MMC — maximum material condition. With MMC, the tolerance grows as the feature departs from its worst-case size. For a hole, bonus tolerance equals actual hole size minus the MMC (smallest) size; for a shaft, it is MMC (largest) size minus actual size. The drawing still enforces worst-case assembly through the virtual condition boundary, but machining gets more room when the feature is not at its worst case. In practice, adding MMC to a position callout is the single cheapest edit on a drawing — it often drops a quote without changing the part’s fit.
Flatness: Form with No Datum
Flatness limits how far a surface may deviate from a perfect plane — and it references no datum, because it only cares about the surface’s own form, not its orientation. It is the callout for mating faces, sealing faces, and any surface that must sit uniformly without wobble or twist. Because flatness is independent of size and orientation, it is also one of the simplest controls to inspect — a surface plate and indicator do the job. On a machined part, a flatness of 0.005–0.010 in (0.13–0.25 mm) is routine; tighter than about 0.002 in (0.05 mm) and you are paying for a dedicated finishing pass, not just a good setup.
Parallelism and Perpendicularity: Orientation Controls
Parallelism controls how closely a surface, axis, or center plane stays parallel to a datum reference. It shows up when a face must stay aligned to a primary surface, or when a hole axis must run parallel to a datum axis. Applied to a feature of size with MMC or LMC it can gain bonus tolerance.
Perpendicularity controls a 90-degree relationship between a feature and a datum — faces that must stand square to a base, or holes that must be normal to a mounting surface so fasteners enter cleanly. Like parallelism it can pair with MMC on features of size.
These two are the workhorses of assembly drawings: a bracket that bolts to a plate needs its mounting face parallel to the plate and its holes perpendicular to it. The relationship between these and flatness is worth stating plainly — flatness is form (no datum), parallelism/perpendicularity are orientation (need a datum). A face can be perfectly flat yet tilted, or parallel yet wavy.
Runout (and Why Concentricity Is Gone)
Concentricity controls the coincidence of two axes, and in modern practice it is largely avoided — it is hard to measure, and ASME Y14.5-2018 no longer treats concentricity and symmetry as primary controls, in favor of more measurable alternatives. Circular runout controls the variation seen at one cross-section during rotation — the standard callout for journal surfaces, seals, and rotating fits. Total runout extends that control along the full surface length, which makes it stricter and the right choice when the whole cylinder must behave consistently during rotation. For non-rotating coaxial features, position is usually more practical than either. In short: if the part spins, reach for runout; if it just needs coaxial holes, reach for position.
Profile of a Surface: The Catch-All
Profile of a surface controls how far an actual surface may deviate from its exact, CAD-defined shape. It is the most flexible control in the system because it handles curved, blended, and freeform geometry that a simple plane or cylinder callout cannot describe — and it can be used with or without datums. On machined parts it is the go-to for contoured sealing surfaces and airfoil-like features, anywhere a ± linear tolerance cannot capture the intended form. A profile tolerance with no datums controls form only; add datums and it controls form plus location and orientation in one callout.
Datums A/B/C: The Part’s Coordinate System
Every orientation and location tolerance needs a frame of reference, and that is what datums provide. Datum A is the primary, B the secondary, and C the tertiary — and the order matters, because it defines how the part is located before any geometric tolerance is evaluated. In fixture terms, A removes the first set of degrees of freedom, B the next, and C the last, so the part is held the same way every time it is inspected or assembled. When a drawing calls out A, B, and C, it is telling the machinist and the inspector exactly how to hold the part — which is why the datum scheme is the first thing a shop reads on any tight-tolerance print.
What Is Realistic to Machine
There is no universal machine-by-machine table, because the realistic number depends on rigidity, setup length, and inspection. But as a working rule for CNC: flatness, parallelism, and perpendicularity of 0.005–0.010 in (0.13–0.25 mm) are routine; true position of 0.005–0.010 in (0.13–0.25 mm) at MMC is typical for bolt patterns; and anything tighter starts to be dominated by setup and inspection rather than the machine itself. The highest-leverage drawing habit is restraint: reserve the tightest tolerances for features that actually affect fit or function, and let the cosmetic and non-critical surfaces stay loose. Over-tolerancing is the most common reason a quote comes back higher than the part deserves. Our machining tolerances guide and tolerances capability page cover the numbers in more detail.
For the two ways to write a tolerance band — plus or minus versus one-sided — see our unilateral vs bilateral tolerance guide.
FAQ
What is true position in GD&T?
True position controls where a feature's axis, center, or derived median plane may lie relative to basic dimensions and datums — inside a cylindrical or two-dimensional tolerance zone rather than a simple ± band. It beats ± tolerancing for holes, pins, and bolt patterns because it separates size from location: a hole can be slightly larger yet still function if its center lands within the allowed zone. In a drawing, it is the position symbol inside a feature control frame with the tolerance value, any MMC modifier, and the datum references.
What is bonus tolerance (MMC) in GD&T?
Bonus tolerance is the extra position allowance a feature earns as it departs from maximum material condition. For a hole, bonus tolerance equals the actual hole size minus the MMC (smallest) size; for a shaft or pin, it is the MMC (largest) size minus the actual size. The practical value: the drawing still enforces worst-case assembly through the virtual condition boundary, but manufacturing gets more room when the feature is not at its worst case — which is why adding MMC to a position callout usually lowers the machining cost without changing the fit.
Concentricity vs runout — which should I use?
Use runout. Concentricity controls the coincidence of axes, and in modern practice it is largely avoided because it is hard to measure and has been superseded — ASME Y14.5-2018 no longer treats concentricity and symmetry as primary controls. For rotating parts, circular runout controls the variation at one cross-section during rotation (good for journals, seals, and rotating fits), while total runout extends that control along the full surface (stricter, for when the whole cylinder must behave consistently). For non-rotating coaxial features, position is usually the more practical control.
What is the difference between flatness and parallelism?
Flatness is a pure form control with no datum reference: it limits how far a surface may deviate from a perfect plane, regardless of how that plane is oriented. Parallelism is an orientation control: it limits how closely a surface, axis, or center plane stays parallel to a datum. A face can be perfectly flat but tilted (bad parallelism), or parallel but wavy (bad flatness) — they constrain different things, which is why both often appear together on mating and sealing faces.
What GD&T tolerances are realistic for CNC machining?
There is no universal machine-by-machine table, because the realistic number depends on rigidity, setup, and inspection. As a working rule for CNC: flatness, parallelism, and perpendicularity of 0.005–0.010 in (0.13–0.25 mm) are routine; true position of 0.005–0.010 in (0.13–0.25 mm) at MMC is typical for bolt patterns; and tighter values push into the range where setup and inspection, not just the machine, determine success. The best drawing strategy is to reserve the tightest tolerances for features that actually affect fit or function.
When should I use profile of a surface?
Use profile of a surface when the geometry is more complex than a simple plane or cylinder and you want the whole surface to follow the intended CAD shape closely — curved, blended, or freeform features. It controls how far the actual surface may deviate from the exact modeled surface, and it can be used with or without datums. For machined parts it is the go-to control for contoured sealing surfaces, airfoil-like shapes, and features where a ± linear tolerance cannot capture the intended form.
Related Resources
CNC Machining Surface Finish: The Ra Chart, Explained
The CNC machining surface finish chart: Ra values in μm and μin, N1–N12 grades, what each process achieves, what…
Passivation of Stainless Steel: Process, Specs, and When Parts Need It
Passivation of stainless steel explained for machined parts: the chemistry, ASTM A967 and AMS 2700 methods, nitric…
GD&T Basics for CNC Machined Parts: The Symbols That Matter
GD&T basics for machined parts: the 14 symbols explained, feature control frames, datums, MMC bonus tolerance, true…
How to Outsource CNC Machining to China, Step by Step
How to outsource CNC machining to China, step by step: vet suppliers, compare landed cost, control quality remotely,…
Send the Drawing. We’ll Read the GD&T.
IsoCNC quotes against real GD&T — true position, runout, profile, and full datum schemes — and inspects on a CMM with first article reports. Send the drawing; an engineer reviews every RFQ, typically within 1–2 business days.