GreatLight CNC Machining Factory logo
CNC Machining
Rapid Prototyping
Materials
Industries
News
About GL

Get Instant Quote

Drawing interpretation

GD and T Symbols on Machining Drawings

This page explains what the symbols in a feature control frame actually require, how datum references and the T symbol change inspection, and where GD&T beats plus/minus tolerancing. Written for engineers and buyers who sign off on drawings before the chips fly.

ASME Y14.5 / ISO 110114 characteristicsDatum targetsMMC gauging
Feature control frame showing GD and T symbols on a machining drawing
Why symbols replace stacked limits

What GD and T symbols on machining drawings actually control

A drawing can state size two ways. The old way stacks a limit on every dimension: 12.00 ±0.10 mm, then 40.00 ±0.10 mm, and so on down the sheet. GD and T symbols replace most of that with a frame that says what the feature must do in function: stay flat within 0.05 mm, stay perpendicular to datum A within 0.1 mm, or hold its axis inside a 0.2 mm diameter zone.

The shift matters because a size limit and a functional limit are not the same requirement. A bore can be perfectly on size and still be unusable if its axis is skewed enough to bind a mating pin. A face can sit inside its thickness band and still rock on a housing. GD and T symbols on machining drawings describe the geometry that makes the assembly work, not just the caliper reading.

Two standards sit behind the symbols. ASME Y14.5 governs most of North America, and ISO 1101 covers much of Europe and Asia. They agree on the core symbols and diverge in places, so the title block has to name one. Mixed-standard drawings are a common source of argument at first article.

Every symbol answers one question: which degrees of freedom does this feature have to give up? Form symbols constrain the surface itself. Orientation symbols constrain it against a datum. Location symbols constrain it against two or three datums at once. Once you read a frame that way, the symbols stop looking arbitrary.

  • 1
    Size is not functionA within-limit part can still fail to assemble.
  • 2
    Title block rulesASME Y14.5 or ISO 1101, not both.
  • 3
    One question per symbolWhich degrees of freedom are removed.
Frame anatomy

Reading a feature control frame left to right

The first compartment holds the characteristic symbol. The second holds the tolerance zone: a number, sometimes preceded by Ø, which tells the inspector whether the zone is a cylinder or a pair of parallel planes. A position callout of Ø 0.2 mm means the axis must lie inside a cylindrical zone 0.2 mm in diameter, oriented and located by the datums that follow.

After the number comes the material condition modifier, if the designer wants one. A circled M means the tolerance applies at maximum material condition, so the allowed deviation grows as the feature departs from that size. A circled L does the same at least material condition. No modifier means the tolerance holds regardless of feature size, and the inspector must measure size and geometry separately.

The last compartments list datum references in order of precedence. Primary datum first, then secondary, then tertiary. Precedence is not cosmetic. It sets the order in which the part is fixtured, so a frame that names B before A tells the inspector to seat the part on B and clock it to A.

Basic dimensions appear in rectangles with no tolerance. They are not inspection targets on their own. They feed the true profile or the true position that the frame controls, and the frame carries the entire allowance.

  • 1
    Ø before a numberCylindrical zone, not parallel planes.
  • 2
    Circled MBonus tolerance as the feature departs from MMC.
  • 3
    Datum orderPrimary, secondary, tertiary. It sets the setup.
  • 4
    Boxed numbersBasic dimensions, tolerance lives in the frame.
The five families

The 14 geometric characteristics and when each applies

Form covers straightness, flatness, circularity, and cylindricity. None of them needs a datum, because they compare a surface only to itself. Flatness on a sealing face or cylindricity on a hydraulic spool are typical. If a shop can measure the feature on a surface plate with no fixturing, the callout is probably a form characteristic.

Orientation covers perpendicularity, parallelism, and angularity. All three need at least one datum, because an angle only means something relative to a reference. These show up on faces that mate with other faces: a motor mounting face perpendicular to a pilot bore, a rail face parallel to a base.

Profile of a line and profile of a surface control form and location together. Profile of a surface is the only characteristic that can tie a free-form surface to basic dimensions across the whole face, which is why it dominates castings, covers, and impeller blades. Location covers position, concentricity, and symmetry. Position is the workhorse for holes and pins; the other two are rare and often replaced by position or profile in new drawings.

Runout covers circular runout and total runout, and it is the only characteristic that requires rotation of the part about a datum axis. Use it on shafts, bearing journals, and anything that spins. It checks the combined effect of form and location in one pass, which is why a lathe part with a bearing seat often carries total runout instead of separate cylindricity and concentricity callouts.

  • 1
    No datum neededStraightness, flatness, circularity, cylindricity.
  • 2
    One datum minimumPerpendicularity, parallelism, angularity.
  • 3
    Free-form workProfile of a surface with basic dimensions.
  • 4
    Spinning partsCircular and total runout about a datum axis.
Datum letter T

What the T symbol means on a drawing

The capital T shows up in two different places, and mixing them up causes real scrap. The first is inside a datum feature symbol: a boxed letter with a leader, with a T added. That T means the datum is established at the tangent plane of the feature, not at its actual surface. The inspector contacts the high points of a rocking or irregular face instead of averaging over the bumps.

That distinction matters on castings and weldments. A raw cast face touches a fixture only at its high spots. A tangent-plane datum tells the inspector to simulate exactly that contact, which is how the part actually sits in the assembly. Without the T, the datum is the real surface and the setup can shift.

The second place is a datum target. Targets are drawn as a circle split horizontally: the size of the target area or point in the upper half, the identifier in the lower half, such as T1 or T2. Three target points on a primary plane simulate the same constraint as a full surface, which is useful when the surface is too large or too rough to fixture reliably.

A datum target is not a datum feature. A datum feature is the physical surface of the part. A target is a defined point, line, or area on it, with a stated size. If a drawing shows T1, T2, T3, the inspector needs three contact points of the stated diameter, not a flat pad.

  • 1
    T in a datum boxTangent plane simulation, not the real surface.
  • 2
    T1, T2, T3Datum targets with a stated contact size.
  • 3
    Why it existsRough castings and large weldments fixture repeatably.
Two tolerance philosophies

GD&T versus traditional plus/minus tolerancing

Plus/minus tolerancing assumes a square or rectangular zone. A hole at X ±0.1 and Y ±0.1 has a 0.2 by 0.2 mm box, and the corners of that box allow about 0.141 mm of radial error. If the mating pin only needs 0.1 mm of clearance, the corner of the box is a reject that the drawing permits.

A position callout of Ø 0.2 mm gives a round zone of the same nominal width. The corner is gone. The zone matches the clearance the fastener actually has, so the drawing stops rejecting parts that would assemble fine. That is the main engineering argument for position over coordinate tolerancing on hole patterns.

The trade-off is inspection cost. A caliper cannot verify a position callout. You need a CMM with the right probe and software, or a functional gauge built to the virtual condition boundary. For a two-hole bracket, plus/minus is cheaper to check. For a 24-hole pattern on a transmission housing, the round zone pays for itself in accepted parts.

Tolerance values should track process capability. A CNC mill holds position to roughly ±0.025 mm routinely and ±0.013 mm with care; a lathe holds ±0.013 mm on diameter without heroics. Asking for 0.05 mm position on a hole 100 mm from the datum in soft aluminum is achievable, but it invites rework and sorting. Surface finish interacts too: a 0.8 μm Ra bore usually needs boring or reaming after drilling, and that second operation changes the setup and the position stack.

  • 1
    Square zoneCorners allow 1.41 times the radial error.
  • 2
    Round zoneMatches fastener clearance, fewer false rejects.
  • 3
    Inspection costCMM or functional gauge, not a caliper.
  • 4
    Match the processDo not ask for tighter than the machine holds.
Pick the callout

Choosing between plus/minus and GD&T callouts

Use the left column when the feature is simple and the right column when function depends on geometry.

SituationPlus/minus worksGD&T is the better callInspection method
Single hole, loose clearanceYes, ±0.1 mm on X and YNot neededCaliper or pin gauge
Hole pattern, mating pinsMarginal, corner wastePosition Ø 0.2 mm at MMCFunctional go-gauge
Sealing face flatnessNo control of formFlatness 0.05 mm, no datumSurface plate and indicator
Bearing journalPartial, needs two calloutsTotal runout 0.02 mm to A-BBetween centers, indicator
Cast housing faceFixtures at high spotsDatum with T, tangent planeThree-point target setup
Free-form coverCannot express itProfile of a surface 0.3 mmCMM scan against CAD
Spool boreSize only, no axis controlCylindricity 0.01 mmRoundness gauge or CMM

The short version

If the feature mates with a fastener pattern or a free-form surface, use GD&T and accept the CMM cost. If it is a single hole or a simple step with generous clearance, keep plus/minus and save the inspection time.

FAQs

Questions we get at first article

Can a shop reject a part that is within size but out of GD&T?

Yes. Size and geometric tolerance are separate requirements. A bore can measure inside its diameter limits and still fail a position or cylindricity callout.

The drawing is the contract. If the frame is there, the part has to meet it, whatever the caliper says.

Does a circled M always give bonus tolerance?

Only when the feature departs from maximum material condition. The bonus equals the amount of departure, added to the stated tolerance.

If the part is produced exactly at MMC, the bonus is zero and the stated number is the whole allowance.

What does a boxed dimension without a tolerance mean?

It is a basic dimension. It defines the true location or true profile and carries no tolerance by itself.

The tolerance comes from the feature control frame that references it. Never inspect a basic dimension on its own.

Is ISO 1101 the same as ASME Y14.5?

Close, not identical. The core symbols match, but defaults differ on things like profile and some modifier usage.

The title block should name one standard. If it does not, ask before quoting.

Why does my drawing show T1 and T2 on a face?

Those are datum targets. The inspector must contact the part at those defined points or areas, at the diameter stated in the target symbol.

It is common on castings and large weldments where the full surface is too rough to seat reliably.

How tight a position tolerance can CNC milling hold?

Roughly ±0.025 mm routinely, and ±0.013 mm with careful setup on a stable part. Beyond that, expect extra fixturing, temperature control, and more inspection time.

We work to ±0.005 mm on parts that need it, but the drawing and the process have to agree before the first cut.

Send us the drawing, symbols and all

We read the feature control frames before quoting, flag callouts that fight the process, and return a DFM note with the quote.

12-hour quoteFree DFM analysis100% inspection

Follow the shop

More from GreatLight

We publish setup notes, tooling trials and inspection data from the factory floor.

FacebookTikTokYouTubeLinkedInInstagramThreadsPinterest

Trusted by engineers and manufacturers worldwide

Tesla Ford Motor Company BYD Auto Denso Magna International Boeing Airbus Medtronic KUKA FANUC