GD&T · Lesson 4 of 4 · ~13 min read

Form and orientation controls

Learning outcomes

• You’ll be able to describe the tolerance zone for flatness, straightness, circularity, cylindricity, perpendicularity, parallelism and angularity.
• You’ll be able to explain why form controls never take datums, while orientation controls need them but don’t locate anything.
• You’ll be able to judge a simple inspection reading against a form or orientation tolerance, and check size separately.

Prerequisites: Lesson 2: Datums and the datum reference frame, Lesson 3: The feature control frame

Example part used in this lesson: AH-101 mounting bracket (fictional, Rev D, unchanged from Lesson 3). 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 3 named five symbol families. This lesson covers two of them.

Form controls limit a feature’s shape compared only with itself, so they never take datum letters.

• Flatness: the whole surface must lie between two parallel planes the tolerance apart.
• Straightness: each line element of a surface must lie between two parallel lines. Applied to a pin’s size callout, it can instead control the derived median line, the bent “spine” through the centers of its cross-sections.
• Circularity: each cross-section of a round feature must lie between two concentric circles. The tolerance is the radial gap.
• Cylindricity: the whole round surface must lie between two coaxial cylinders.

Orientation controls limit a feature’s angle to datums, so they need datum letters.

• Perpendicularity: two parallel planes at 90° to the datum.
• Parallelism: two parallel planes parallel to the datum.
• Angularity: two parallel planes at a boxed basic angle to the datum.

Each zone can slide to wherever the feature sits. Orientation sets angle, never location; position does that in Lesson 5 (Figures 4.1 and 4.2).

Where you’ll see it on the job

• A quality intern in the inspection lab checks the .002 flatness on AH-101’s bottom face before the part’s first-article report goes out.
• A manufacturing intern sees perpendicularity on a secondary datum face and plans to cut both faces in one setup, so they come out square.
• A design intern is asked in review why a bonding face carries flatness but no datums. The answer is that it only needs to sit flat on structure.
• A test or integration intern traces a poor electrical bond reading back to a bottom face that bowed after machining, so it no longer seats fully on structure.
• An intern fielding a supplier question learns the supplier checked parallelism with calipers. The readings can’t show tilt, so the lab has to recheck.

Step-by-step how-to

Use these six steps for any form or orientation frame.

1. Name the control and its family. Read the symbol from Lesson 3. Form or orientation tells you whether datums are coming.
2. Picture the tolerance zone. Two planes, two lines, two circles or two cylinders, and how far apart. A Ø in front of the value means a cylinder around an axis instead.
3. Set up the datums. For orientation, seat the part on the datum simulators in frame order. For form, there’s nothing to set up; skip this step. Any leveling you do is only to make the reading easier.
4. Collect the readings. A dial indicator is a gage whose needle shows tiny movements of a probe tip. On a surface plate, it rides on a height gage, a precision stand that slides on the plate. Sweep the surface and note the highest and lowest readings. A coordinate measuring machine (CMM) can probe points instead. A roundness instrument spins a round part on a precise spindle and records its radius all the way around. For angularity, a sine bar tilts the part to the exact basic angle first, using gauge blocks (the trade name for precision spacer blocks) under one end.
5. Compare the spread with the tolerance. The total swing, high minus low, is called full indicator movement (FIM). If it fits inside the tolerance, that control passes. State any setup assumption, because the setup can inflate the spread. The true form value is the minimum zone: the narrowest zone of the right shape that holds every point.
6. Check size separately. Form and orientation don’t replace size limits. A micrometer checks local size at each spot, a two-point check. In ASME drawings, by default, a feature of size must also fit inside a boundary of perfect form at its maximum material size. That’s the envelope rule (Rule #1). A micrometer can’t verify it. It needs a full-form check, such as a gage, a CMM evaluation or a functional check.

Worked examples

All three use AH-101 Rev D (Figure 4.3). Examples 2 and 3 use “what if” frames that are not on the drawing, so you can practise without changing the revision.

Example 1: Check flatness .002 on datum feature A

Given: The inspector turns the part over and sets it on three adjustable jacks, tall enough for the upright to hang clear. They level the bottom face until three corner readings match, then sweep it. The highest reading is +.0009 in and the lowest is −.0008 in.

• Name the control and its family: Flatness, a form control.
• Picture the tolerance zone: Two parallel planes .002 in apart, free to tilt any way.
• Set up the datums: None. Flatness takes no datums, so leveling the face is just a measuring convenience.
• Collect the readings: High +.0009 in, low −.0008 in.
• Compare the spread with the tolerance: .0009 − (−.0008) = .0017 in. Leveling on three corners may not find the best tilt, so for the points you swept, the minimum-zone flatness is .0017 in or less. Dense enough sampling makes that a fair estimate for the whole face.

Answer: Measured flatness is .0017 in or less, inside .002 in. It passes.

Example 2: Check perpendicularity of face B to datum A (what if 1)

Given: This is the Lesson 2 part whose upright leans out .006 in at the top over 1.50 in. Assume, as there, that face B is flat and only tilted.

• Name the control and its family: Perpendicularity, an orientation control.
• Picture the tolerance zone: Two parallel planes .005 in apart, both square to datum A.
• Set up the datums: Seat the bottom face on the surface plate. That’s datum A, the only datum in the frame.
• Collect the readings: Run the indicator straight up the face on the height gage, from the bottom edge to the top. It reads 0 at the bottom and .006 in at the top. Repeat across the 2.00 in width; with a pure tilt, every line reads the same (Figure 4.4).
• Compare the spread with the tolerance: FIM is .006 in, more than .005 in.

Answer: The face fails perpendicularity by .001 in. That’s the same lean that shifted the hole reading in Lesson 2. A frame like this on datum B would catch it directly.

Example 3: Check parallelism of the base top, then its thickness (what if 2)

Given: The part sits on the plate on datum A. An indicator sweep over the top face of the base, avoiding the holes, gives a high of +.0013 in and a low of −.0013 in. A micrometer at six spots reads .2490 to .2512 in. Assume the bottom face meets its .002 flatness.

• Name the control and its family: Parallelism, an orientation control.
• Picture the tolerance zone: Two planes .003 in apart, parallel to datum A.
• Set up the datums: The surface plate simulates A, as in Lesson 2.
• Collect the readings: Sweep high +.0013 in, low −.0013 in.
• Compare the spread with the tolerance: .0013 − (−.0013) = .0026 in, inside .003 in.
• Check size separately: .2490 to .2512 in sits inside .245 to .255 in.

Answer: Parallelism (.0026 in) and thickness both pass. The size limits allow up to .010 in of variation, so a .003 parallelism is a tighter, extra requirement.

Easy mistakes

Adding datums to a form control

Flatness feels incomplete alone, so people level it to the plate and call that a datum. Form compares a surface only with itself. Leveling is a measuring aid, not part of the requirement.

Thinking orientation locates the feature

A face can be perfectly square to A and still sit in the wrong place. Orientation sets angle only; size or position sets where.

Treating a setup spread as the answer

Leveling on three points is quick, so it’s tempting to report that spread as exact. It’s usually a conservative estimate for the points you measured, not an exact value. Say so, or ask for a minimum-zone evaluation (re-leveling to the smallest spread, or a CMM set to minimum zone).

Checking flatness by resting on the plate

A face that doesn’t rock looks flat. Rocking only shows big gaps, not whether the surface fits .002. A bowed face can still sit steady on its high points. Measure the surface itself.

Skipping the size check

A good indicator sweep feels like a full inspection. Form and orientation never replace size limits, so measure local size with two-point tools, and remember the envelope is a separate check.

Sweeping one line and stopping

One pass up the face is fast. The zone covers the whole surface, so sample enough lines to catch twist or local bumps.

Practice questions with answers

Use Figures 4.1-4.4 unless a question says otherwise.

Q1. Which control never takes datum letters?

A) Parallelism
B) Flatness
C) Angularity
D) Perpendicularity

Q2. What does a circularity zone look like on AH-101’s Ø.257 hole?

Q3. Face B passes perpendicularity .005 to A. Does that prove the first hole is 1.25 from B?

Q4. Another upright leans out .004 in at the top over 1.50 in, with a flat face. Does it pass perpendicularity .005 to A (what if 1)?

Q5. A parallelism sweep (what if 2) reads +.0010 to −.0025 in, and the micrometer reads .2470 to .2505 in. Which checks pass?

A) Both
B) Size only
C) Parallelism only
D) Neither

Q6. A leveled flatness sweep reads +.0012 to −.0010 in. What can you report?

Q7. A technician says the bottom face “doesn’t rock on the plate, so it’s flat”. Accept the part?

FAQs

Is parallelism just flatness with a datum?

Close. On a surface, the parallelism zone is two planes held parallel to the datum, so it also limits that surface’s flatness to the same value. A separate flatness only adds something if it’s smaller. On an axis or a center plane, parallelism doesn’t control any surface’s flatness at all.

Why can’t form controls use datums?

They describe shape, and shape doesn’t depend on any other feature. Tying it to a datum would turn it into an orientation control.

What is the envelope rule?

On ASME drawings, by default, each regular feature of size must have perfect form at its maximum material size (Rule #1). It covers each feature on its own, not the angle or location between features. It doesn’t apply to as-supplied stock, such as bar or sheet, or to flexible parts in their free state. A designer can also switch it off with a circled I (independency). ISO drawings default to independency (ISO 8015): size and form are separate unless the size carries a circled E.

Can a form tolerance be bigger than the size tolerance?

On a surface of a feature of size, such as the base’s bottom face, it usually adds nothing. The envelope already limits that surface’s form to the size tolerance. Straightness of a derived median line, or flatness of a derived median plane, are known exceptions that later material covers.

Do I need special equipment?

A surface plate, height gage and indicator handle most flat-face checks. Round features often go to a CMM or roundness instrument. Your lab’s procedures say which tools are approved, and which fits a CMM must use.

What comes next?

Lesson 5 covers position and profile, and adds MMC to AH-101 as Rev E.

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

• GD&T Basics, form controls: Flatness, Straightness, Circularity, Cylindricity
• GD&T Basics, orientation controls: Perpendicularity, Parallelism, Angularity
• GD&T Basics, Rule #1 and derived median line straightness
• Keyence, International standards and GD&T (ASME envelope vs ISO independency)
• OpenExamPrep, Rule #1 envelope principle (exceptions; secondary study guide)
• Wikipedia, Indicator (distance amplifying instrument), Surface plate, Height gauge, Coordinate-measuring machine, Roundness, Sine bar
• Wikipedia, Geometric dimensioning and tolerancing
• ASME, Y14.5 Dimensioning and Tolerancing product page (current edition 2018, reaffirmed 2024)