GD&T · Lesson 3 of 4 · ~13 min read

The feature control frame

Learning outcomes

• You’ll be able to name every compartment of a feature control frame and say what each one tells you, reading left to right.
• You’ll be able to read a frame aloud as one plain sentence, including its datum order.
• You’ll be able to tell which dimensions are basic, and say where their tolerance comes from.

Prerequisites: Lesson 1: Reading engineering drawings, Lesson 2: Datums and the datum reference frame

Example part used in this lesson: AH-101 mounting bracket (fictional, Rev D). Rev D keeps Rev C’s geometry and datums and adds two frames. All values are decimal inches.

Axes: X runs along the 3.00 length, Y runs front to back, Z runs up.

What it is

Lesson 1 called a feature control frame (FCF) a boxed callout that holds a geometric tolerance symbol, its value and its datum letters. Lesson 2 said the datum order lives in it. This lesson opens the box.

An FCF is a rectangle split into compartments, read left to right like a sentence:

• Geometric characteristic symbol: what kind of control this is, such as position or flatness.
• Tolerance compartment: the shape and size of the tolerance zone, the region the feature must stay inside. A diameter symbol (Ø) in front of the value means a cylindrical zone, as for AH-101’s hole positions. Without Ø, the zone shape depends on the symbol: for flatness it’s the space between two parallel planes. Lesson 4 shows the other form and orientation zones, and Lesson 5 shows profile.
• Datum reference compartments: zero to three datum references, in order of precedence: primary, secondary, tertiary. A compartment can also carry a modifier, or two letters joined as a common datum (later lessons).

A count such as “2X” means each of those features gets its own zone. The basic dimensions lock all the zones to the datums and to each other, so the holes are controlled as a pattern.

A frame never works alone when it locates something. Basic dimensions, shown in a rectangle such as 1.25 in a box, give the theoretically exact location or shape. Basic dimensions say where the zone sits; the FCF says how big it is (Figure 3.1).

Where you’ll see it on the job

• A quality intern programming a coordinate measuring machine (CMM) reads each frame to decide which datums to set up, in which order, and what zone to report against. On AH-101 that’s A, B, C and a Ø.028 zone per hole.
• A manufacturing intern quoting a part scans the frames to spot tight tolerances that need a better machine or an extra operation.
• A machine shop intern sees flatness .002 on the bottom face and asks whether the saw-cut plate needs a facing pass before anodize.
• A design intern in a design review is asked to read a frame aloud. Doing it cleanly shows you know what the part has to do.
• An intern answering a supplier question finds that the supplier ignored the basic dimensions and applied the title-block default. The frame settles it.

Step-by-step how-to

Use these six steps on every frame.

1. Find what the frame controls. Follow its leader, or see what it sits under. Under a size callout such as 2X Ø.257 ±.003 THRU, it controls each hole’s axis. With a leader to a surface, or to an extension line from it, it controls that surface.
2. Read the symbol. Name the control and its family. Figure 3.4 groups the symbols into families. The family tells you what to expect next. Form symbols never take datums, orientation and runout always do, position normally does, and profile may or may not.
3. Read the tolerance compartment. Note the zone shape (Ø or not), the value in drawing units and any circled letter after the value. An Ⓜ means maximum material condition (MMC) and an Ⓛ means least material condition (LMC). Lesson 5 covers them. Other letters, such as Ⓟ or Ⓕ, are less common modifiers; look them up when you see one. With no modifier, the tolerance applies regardless of feature size (RFS). That’s the default in ASME Y14.5-2009 and -2018, and it has no symbol. Very old drawings may show a circled S for it. An unmodified datum feature of size, such as a hole or pin, works the same way on the datum side, called regardless of material boundary (RMB). Lesson 5 covers that.
4. Read the datum compartments. Left to right is primary, secondary, tertiary, as in Lesson 2. The letters are labels, so A|C|B means C is secondary. Some frames, such as flatness, have no datums at all.
5. Find the basic dimensions. Look for boxed numbers that run from the datums to the feature. They set the true position, the exact spot the zone is centered on, and the title-block defaults don’t apply to them. On AH-101 Rev D they are the boxed 1.25, 1.25 and 1.00.
6. Say it aloud. Join the pieces into one sentence: what feature, what control, what zone, relative to which datums in which order (Figure 3.3). Start with the feature, not the symbol. If you can’t finish the sentence, you’ve missed a compartment.

Worked examples

All three use AH-101 Rev D (Figure 3.2). As Lesson 1’s Step 7 says, check the revision first: the block ends with “D | HOLES LOCATED BY POSITION; ADDED FLATNESS ON DATUM A”.

Example 1: Read the position frame on the holes

Given: Under “2X Ø.257 ±.003 THRU” sits the frame: position | Ø.028 | A | B | C.

• Find what the frame controls: It sits under a hole size callout, so it controls the axis of each of the 2 holes.
• Read the symbol: Position, from the location family.
• Read the tolerance compartment: Ø.028 means a cylinder .028 in across. No modifier follows, so the zone stays .028 whatever size each hole is made within .254 to .260.
• Read the datum compartments: A primary, B secondary, C tertiary. A is primary, so each zone cylinder stands square to the bottom face.
• Say it aloud: “Each hole’s axis must lie in a cylinder .028 in across, centered on its true position. Set the part up on A, then B, then C.”

Answer: Each of the two hole axes must stay in its own Ø.028 cylinder, square to A and located from B and C. The Ø.257 ±.003 size still applies separately. Bolt-clearance holes like these often get Ⓜ, which Lesson 5 adds (Figure 3.3 breaks down the sentence).

Example 2: Read the flatness frame on datum feature A

Given: In the front view, a frame reads flatness | .002, with its leader on the bottom edge line of the base.

• Find what the frame controls: The leader lands on a surface edge line, not a dimension line, so it controls the bottom face itself.
• Read the symbol: Flatness, from the form family.
• Read the tolerance compartment: No Ø, so the zone is the space between two parallel planes .002 in apart.
• Read the datum compartments: None. Flatness compares a surface only with itself.
• Say it aloud: “The bottom face must lie between two parallel planes .002 in apart.”

Answer: The whole bottom face, which is also datum feature A, must fit between two parallel planes .002 in apart. Those planes can tilt any way; they don’t have to line up with anything else. This limits the wobble Lesson 2’s surface plate had to absorb.

Example 3: Find the true positions and their tolerance

Given: Rev D shows boxed 1.25 from B to the first hole, boxed 1.25 spacing, boxed 1.00 from C and (2.50) from B. A supplier asks whether the boxed 1.25 spacing carries the title block’s ±.01.

• Find what the frame controls: The position frame controls both hole axes.
• Find the basic dimensions: The first hole’s true position is X = 1.25, Y = 1.00 from B and C. The second is X = 1.25 + 1.25 = 2.50, Y = 1.00, because both holes sit on the same centerline (an implied basic zero offset). The (2.50) reference agrees exactly, because basic dimensions don’t stack up tolerance.
• Say it aloud: “Each hole’s axis stays within Ø.028 of its exact spot at (1.25, 1.00) or (2.50, 1.00), measured in the A, B, C frame.”

Answer: No. Boxed dimensions have no tolerance of their own, so the title-block ±.01 doesn’t apply. The only location tolerance is each hole’s Ø.028 zone from the position frame.

Easy mistakes

Applying the title-block default to a basic dimension

A bare-looking 1.25 tempts you to add ±.01, because Lesson 1 trained you to. Check for the box first. Boxed values get their tolerance from a frame (or occasionally a note), never from the title block.

Missing the Ø

The Ø is small and easy to skip on a crowded print. For position, a zone of .028 with Ø is a cylinder; without it, a band .028 wide. Read the zone shape before the number.

Reading the datums alphabetically

A|C|B looks like a typo for A|B|C. It isn’t: C is secondary. Set up in the order the compartments show.

Adding datums to a form control

Flatness looks incomplete without letters, so people assume datums are implied. They aren’t. Form controls compare a feature only with itself, so the inspector never sets up a datum frame for them.

Thinking the frame replaces the size tolerance

One callout block holds both, so it’s easy to check one and forget the other. Position controls where the hole is, not how big. The Ø.257 ±.003 still has to be checked on its own.

Mixing up boxed and parenthesized numbers

Both look like “special” dimensions. A box means exact and controlled by a frame; parentheses mean reference and not inspected.

Practice questions with answers

Use Figures 3.1-3.2 unless a question says otherwise.

Q1. In what order are a frame’s compartments read?

A) Datums, symbol, tolerance
B) Symbol, tolerance, datums
C) Tolerance, symbol, datums
D) Any order

Q2. What does the Ø in “Ø.028” tell you?

Q3. What tolerance applies to the boxed 1.00 from datum C?

A) ±.01
B) ±.005
C) None of its own; the position frame’s Ø.028 zone
D) It isn’t inspected

Q4. A frame reads position | Ø.010 | A | C | B. Which datum is secondary?

Q5. Read the AH-101 flatness frame aloud.

Q6. Perpendicularity belongs to which family, and which lesson covers it?

A) Form, Lesson 4
B) Orientation, Lesson 4
C) Location, Lesson 5
D) Runout, Lesson 5

Q7. A supplier wants to write “A|B” after the flatness .002 “to be safe”. What do you say?

FAQs

How many symbols are there?

ASME Y14.5-2018 uses 12, in five families: form, orientation, location, profile and runout (Figure 3.4). The 2018 edition dropped concentricity and symmetry; position, profile or runout now do those jobs. You’ll still see them on older ASME drawings and on current ISO drawings.

Why Ø.028 for the holes?

Lesson 1’s ±.01 in X and Y gave the first hole a square zone. A circle through that square’s corners is about Ø.0283 (Lesson 1, Figure 1.5). Rounding down to Ø.028 keeps almost the same worst case (radius .014 vs .0141) and still gives about 54% more area than the square. Hole-to-hole, though, Rev D is looser than Rev C. Each hole’s zone is tied to the datums, and the two zones’ errors can add up between the holes. Each hole may sit up to .014 from its true position, so if they move apart, spacing grows by up to .028. Spacing can range from 1.222 to 1.278 in, against Rev C’s 1.24 to 1.26. That’s with no Ⓜ on the frame. Lesson 5 adds Ⓜ, which gives larger holes a larger zone, so the allowed spacing widens. Lesson 5 also shows how to tighten spacing where function needs it.

What do Ⓜ and Ⓛ do?

They let the zone grow as the feature departs from its MMC or LMC size. That extra is called bonus tolerance. Lesson 5 covers it.

Can one feature have more than one frame?

Yes. Frames can stack under one callout, and the feature must meet every one of them. Some special frames combine two rows that work together. Later lessons show when that helps.

Do ISO drawings use the same frames?

The layout looks very similar, and most symbols match. ISO rules differ in places, including some defaults. Check which standard the drawing’s notes call out, as AH-101’s Note 1 does for ASME Y14.5-2018.

What comes next?

Lesson 4 covers the form and orientation families, starting with flatness on datum A.

Sources (all checked 2026-10-28; used for facts only, no text or figures copied)

• GD&T Basics, Feature control frame and GD&T symbols
• GD&T Basics, Position, True position and Flatness
• GD&T Basics, Maximum material condition and Regardless of feature size
• GD&T Basics, Concentricity and Symmetry (removed in the 2018 edition)
• Drafter, Feature control frame builder
• Action Engineering, MBE dictionary: ASME Y14.5 terms
• WisTech Open, Blueprint Reading, Print symbols and notes
• Wikipedia, Geometric dimensioning and tolerancing (symbol table and 2018 removals)
• ASME, Y14.5 Dimensioning and Tolerancing product page (current edition 2018, reaffirmed 2024)