Free cheat sheet · print it

GD&T cheat sheet. Print it, pin it up.

All 14 symbols, what each one controls, whether it needs a datum or can take MMC, and how it's usually checked on the floor. Then the modifiers, and how to read a feature control frame left to right.

Free shop calculators

Based on ASME Y14.5-2018. Prints on two Letter or A4 pages, black and white.

GD&T cheat sheet

ASME Y14.5-2018 · getdeburr.com/gdt-cheat-sheet

The 14 geometric characteristics

Form controls never use a datum. Profile can go either way. Orientation, location and runout always need one. MMC and LMC only make sense on a feature of size: a hole, pin, slot or tab.

Form no datum, ever

Straightnessform

Each line element of a surface, or the axis of a pin or hole, must be straight within the zone.

Datum
Never
MMC
Only on a feature of size (its axis or median plane)
Check
Straightedge and feelers, or indicator along a surface plate. Axis: go gauge at MMC or CMM.

Flatnessform

The whole surface must lie between two parallel planes the tolerance apart.

Datum
Never
MMC
Only on a feature of size (derived median plane)
Check
Part on three jacks on a surface plate, level it, sweep an indicator. Or CMM. Indicating the top face against the plate checks parallelism, not flatness.

Circularity (roundness)form

Each cross-section must be round within two concentric circles.

Datum
Never
MMC
No
Check
Roundness tester or CMM. Mics only catch oval; a V-block hides odd-lobe shapes.

Cylindricityform

The whole surface must lie between two coaxial cylinders. Roundness, straightness and taper in one.

Datum
Never
MMC
No
Check
CMM or roundness machine with many sections. Hard to do well with hand tools.

Profile datum optional

Profile of a lineprofile

Each cross-section of a surface must follow the true shape within a band.

Datum
Optional. Without one it controls form only.
MMC
Not on the tolerance. Datums can take MMB.
Check
Optical comparator with an overlay, contour tracer, or CMM.

Profile of a surfaceprofile

The whole surface must sit in a band around the true CAD shape. Can control size, location, orientation and form at once.

Datum
Optional. With datums it also locates the surface.
MMC
Not on the tolerance. Can use U for an unequal band.
Check
CMM against the model, or a fixture plus indicator zeroed on a master.

Orientation datum required

Angularityorientation

A surface or axis must sit at the basic angle to the datum, within a zone. Not an angle in degrees: a width.

Datum
Required
MMC
Yes, on a feature of size
Check
Sine plate or bar with gauge blocks, then sweep with an indicator. Or CMM.

Perpendicularityorientation

A surface or axis must be at 90° to the datum, within a zone.

Datum
Required
MMC
Yes, on a feature of size
Check
Datum face on the plate, run an indicator up the feature against a square or cylinder square. Or CMM.

Parallelismorientation

A surface or axis must be parallel to the datum, within a zone.

Datum
Required
MMC
Yes, on a feature of size
Check
Datum face down on a surface plate, sweep an indicator over the controlled face. Total indicator movement is the result.

Location datum required

Positionlocation

The axis or center plane of a hole, pin or slot must sit within a zone around its true position, set by basic dimensions from the datums.

Datum
Required (except some pattern-to-pattern cases)
MMC
Yes, MMC or LMC. Bonus tolerance applies.
Check
CMM. At MMC, a functional gauge with pins at virtual condition. Open setup: height gauge and pin gauges.

Concentricityremoved 2018location

The median points of a round feature must sit within a cylinder around the datum axis. Still on many older drawings.

Datum
Required
MMC
No, RFS only
Check
Needs median points, so CMM. Checking runout instead is common but agree it with the customer first.

Symmetryremoved 2018location

The median points of a slot or tab must sit within two planes centered on the datum plane. Still on older drawings.

Datum
Required
MMC
No, RFS only
Check
CMM, measuring both sides at matching points. Today the drawing would use position or profile.

Runout datum axis required

Circular runoutrunout

Rotate the part on the datum axis: the indicator reading at each single section must stay within the tolerance.

Datum
Required (an axis)
MMC
No, RFS only
Check
Part between centers, in V-blocks or a collet on the datum, one indicator, read each section separately.

Total runoutrunout

Same, but the indicator travels the full length while the part turns. One reading for the whole surface.

Datum
Required (an axis)
MMC
No, RFS only
Check
Between centers or in V-blocks, traverse the indicator along the surface while rotating. Max minus min over everything.

How to read a feature control frame

Read it left to right like a sentence: what control, how big a zone, under what condition, measured from which datums, in what order.

Annotated feature control frame A frame with five cells: the position symbol, tolerance diameter 0.25 with an MMC modifier, then datums A, B and C. Labels: the characteristic, the tolerance zone, the modifier, and datums primary, secondary and tertiary. Ø0.25 M A B C Characteristic position Tolerance zone Ø = cylinder 0.25 wide Modifier: MMC bonus allowed 1st 2nd 3rd Datums, in order
  1. Symbol. Position: control the location of the hole's axis.
  2. Ø0.25. The Ø makes the zone a cylinder 0.25 across, centered on true position. No Ø means two parallel planes.
  3. Circled M. The 0.25 applies when the hole is at its smallest size. As the hole grows, you get bonus.
  4. A | B | C. Set the part up on A first (3 points of contact on a face), then against B (2 points), then C (1 point). Basic dimensions run from there.
  5. In words: "Each hole's axis must be inside a Ø0.25 cylinder at true position, at MMC, measured from A, then B, then C."

Bonus tolerance in 20 seconds

Hole size 10.00 to 10.20, position Ø0.25 M to A|B|C. MMC of a hole is its smallest size: 10.00.

Measured hole: 10.12 → bonus = 10.12 − 10.00 = 0.12
Allowed position: 0.25 + 0.12 = Ø0.37
CMM says X off 0.10, Y off 0.08 → position = 2 × √(0.10² + 0.08²) = Ø0.256
Without the M: Ø0.256 > Ø0.25, reject · With the M: Ø0.256 ≤ Ø0.37, accept

For a pin, MMC is the largest size, so bonus = MMC − measured size. Position is always 2 × the radial offset. Run your own numbers in the true position calculator →

Modifiers and drawing symbols

The small marks that change what a number means. RFS is the default: with no modifier, the tolerance applies at any size and there's no bonus.

M
MMCMaximum material condition: smallest hole, largest pin. Tolerance grows as the feature leaves MMC. After a datum letter it means MMB.
L
LMCLeast material condition: largest hole, smallest pin. Used to protect wall thickness or edge distance.
none
RFS (default)Regardless of feature size. No modifier means the tolerance is the same at any size. No bonus.
S
RFS, old symbolOn pre-2009 drawings. Means the same as no modifier today.
P
Projected tolerance zoneThe zone sits above the part, as tall as the number shown. For threaded and press-fit holes, where the mating bolt or pin goes.
F
Free stateCheck the part unrestrained, as it sits. For thin or flexible parts.
T
Tangent planeControl the plane touching the high points, not every point on the surface.
U
Unequal bilateralProfile only. The number after the U is how much of the band is on the side that adds material.
ST
Statistical toleranceTolerance set by statistical process control. Expect capability requirements, not just pass/fail.
CF
Continuous featureTreat interrupted surfaces, like a bore broken by a groove, as one feature.
Ø
DiameterBefore a size: a diameter. Inside a frame: a cylindrical zone.
SØ
Spherical diameterSize of a sphere. In a frame: a spherical zone.
R
RadiusThe arc must be within the size limits. Flats and reversals are allowed.
CR
Controlled radiusLike R, but a smooth curve with no flats or reversals.
SR
Spherical radiusRadius of a sphere, like a ball end.
25
Basic dimensionTheoretically exact. Its tolerance comes from a feature control frame, not the title block.
(25)
ReferenceInformation only. Not inspected and not on the FAI.
4X
PlacesThe callout applies to 4 identical features. Each one gets checked.
CounterboreFlat-bottom bore, diameter then depth. Spotface is the same box with SF inside.
CountersinkCone, given as diameter at the surface and included angle.
DepthDepth of a hole or bore, to the end of the full diameter, not the drill point.
All aroundCircle at the leader bend: profile applies all the way around the outline in that view.
Between"A ↔ B": the profile applies only from point A to point B.

Datums on the floor

Datums are how the part gets set up for measuring. Get the setup wrong and every reading after it is wrong.

Order matters

Primary datum first, with full contact (3 high points on a face). Secondary against 2 points, tertiary against 1. Swap the order and you get a different part.

Datum feature ≠ datum

The datum is the perfect plane or axis from your plate, chuck or gauge pin. The datum feature is the imperfect surface on the part that touches it.

Size datums

A hole or pin as a datum is held by the smallest pin or largest collar that fits (RFS). With a circled M after the letter (MMB), a fixed-size gauge pin is used and the part may shift.

getdeburr.com/gdt-cheat-sheet · Free AI drawing ballooner at getdeburr.com/balloon

Got a drawing full of these?

The free ballooner reads every dimension and GD&T frame on a PDF drawing, numbers them, and lists them in a Form 3 spreadsheet. No account needed.

Balloon a drawing free Shop calculators