Skip to content
M
MakerStage

Quick Answer

Flatness controls the shape of a surface in isolation — no datum required. Parallelism and perpendicularity control the orientation of a surface relative to a datum (parallel or square, respectively) and inherently control flatness within the same tolerance zone. The decision rule: if the surface mates with or references another feature, use parallelism or perpendicularity. If it stands alone, use flatness — or skip GD&T entirely if the surface is non-functional.

The Core Distinction

Form vs Orientation: Why It Matters

Flatness is a form control — it describes the shape of a single surface without referencing any other feature. Parallelism and perpendicularity are orientation controls — they describe the angular relationship between a surface and a datum. This distinction drives everything: whether a datum is required, what the tolerance zone looks like, how the part is inspected, and what it costs to machine.

For a full introduction to all 14 GD&T symbols and their categories, see the GD&T symbols chart. For how each control maps to CNC cost and inspection methods, see GD&T for CNC machining.

⏤
Flatness
Form — No Datum

The surface must lie between two parallel planes separated by the tolerance value. The planes can be at any orientation in space — flatness only controls waviness, not tilt.

∥
Parallelism
Orientation — Datum Required

The surface must lie between two parallel planes that are parallel to the datum plane. Controls both tilt (orientation) and waviness (form) simultaneously.

⊥
Perpendicularity
Orientation — Datum Required

The surface must lie between two parallel planes that are perpendicular (90°) to the datum plane. Controls both squareness (orientation) and waviness (form) simultaneously.

Side-by-Side

Flatness vs Parallelism vs Perpendicularity

Property⏤ Flatness∥ Parallelism⊥ Perpendicularity
GD&T CategoryFormOrientationOrientation
Symbol⏤∥⊥
Datum Required?NoYesYes
Tolerance ZoneTwo parallel planes (any orientation in space)Two parallel planes that are parallel to the datumTwo parallel planes that are perpendicular to the datum
What It ControlsSurface waviness only (form). Does not control tilt or location.Tilt relative to datum + inherently controls flatness (form).Squareness to datum + inherently controls flatness (form).
Rule #1 OverlapMust be ≤ size tolerance on features of size.Tolerance zone is two planes → surface must also be flat within that zone.Tolerance zone is two planes → surface must also be flat within that zone.
Inspection MethodSurface plate + indicator or CMM scanSurface plate: datum face down, indicator sweeps top face, or CMMSquare + indicator, or CMM with datum plane established
Typical CNC Range (easy)0.002–0.005 in. (0.05–0.13 mm)0.002–0.005 in. (0.05–0.13 mm)0.002–0.005 in. (0.05–0.13 mm)
Typical CNC Range (tight)0.0005–0.001 in. (0.013–0.025 mm)0.0005–0.001 in. (0.013–0.025 mm)0.0005–0.001 in. (0.013–0.025 mm)
CNC Cost Impact (tight)+30–60% (stress-relieved stock, light finish pass)+25–50% (flip part on precision vise, re-indicate)+25–50% (spindle calibration critical, thin-wall risk)
Decision Framework

Which Control Do I Need? (Decision Tree)

Follow these questions in order. The first “yes” gives you the answer.

1

Is the surface non-functional (cosmetic, access pocket, weight reduction)?

No GD&T needed — use the block tolerance from the title block.

2

Does the surface mate with or reference another feature on this part?

If no → use Flatness (the surface stands alone — only waviness matters).

3

Must the surface be parallel (0°) to the datum?

If yes → use Parallelism referenced to the datum. This inherently controls flatness.

4

Must the surface be square (90°) to the datum?

If yes → use Perpendicularity referenced to the datum. This inherently controls flatness.

What about other angles?

If the surface must be at an angle other than 0° or 90° to the datum, use angularity. The basic angle is stated separately; the angularity tolerance controls variation around that angle. Angularity works identically to parallelism and perpendicularity — the only difference is the reference angle.

ASME Y14.5 Rule #1

Why Parallelism Inherently Controls Flatness

This is the concept that eliminates most unnecessary dual callouts. When you specify parallelism of 0.003 in. to datum A, the tolerance zone is two parallel planes separated by 0.003 in. and parallel to datum A. The controlled surface must fit entirely between those planes. If the surface is flat within 0.003 in. but tilted 0.005 in. from datum A, it fails. If the surface is parallel to datum A but wavy by 0.005 in., it also fails. The zone constrains both.

The same logic applies to perpendicularity. A perpendicularity tolerance of 0.003 in. means the surface must be both square to the datum within 0.003 in. and flat within 0.003 in. A separate flatness callout is only needed when the flatness requirement is tighter than the orientation tolerance.

Valid dual callout

Parallelism 0.005 in. to datum A plus flatness 0.001 in. — the surface must be parallel within 0.005 in. (controls tilt) but the local waviness must not exceed 0.001 in. The flatness tolerance is tighter than the parallelism tolerance, so the dual callout adds a real requirement.

Redundant dual callout

Parallelism 0.003 in. to datum A plus flatness 0.005 in. — the flatness of 0.005 in. is redundant because the parallelism zone already constrains flatness to 0.003 in. This callout adds inspection cost (the inspector must verify flatness separately) with zero functional benefit.

Not Sure If Your Drawing Has Redundant Callouts?

Upload your drawing and get a free DFM review. MakerStage engineers will flag redundant or over-specified flatness, parallelism, and perpendicularity callouts that drive unnecessary inspection cost — and suggest the minimum GD&T that maintains your functional requirements.

Get a Quote with Free DFM Review
Mounting Plate Example

Worked Examples: CNC Aluminum Mounting Plate

A 6061-T6 aluminum mounting plate has four features that each require a different GD&T decision. Datum A is the bottom mounting face.

⏤

Mounting face (bolts to a wall)

Flatness 0.002 in. (0.05 mm)

This face mates with an external surface you do not control. Flatness ensures the face is not warped, but the tilt of the face relative to other features on this part does not matter — the mating wall determines the final orientation.

∥

Top face (parallel to mounting face)

Parallelism 0.003 in. (0.08 mm) to datum A

A sensor mounts on the top face and must be aligned parallel to the mounting face (datum A). Parallelism controls both the tilt and the flatness of the top face relative to datum A. Calling out flatness instead would miss the tilt requirement.

⊥

Side wall (perpendicular to mounting face)

Perpendicularity 0.003 in. (0.08 mm) to datum A

A linear rail mounts on this side wall. The rail must be square to the mounting face so the carriage travels perpendicular to the base. Perpendicularity controls both squareness and flatness of the wall relative to datum A.

—

Access pocket floor (no mating requirement)

No GD&T — block tolerance ±0.005 in. (±0.13 mm)

This pocket exists for weight reduction or tool clearance. Nothing mates to it, nothing references it. Adding flatness or parallelism would increase inspection cost with zero functional benefit.

Cost Reality

CNC Cost Impact: Flatness, Parallelism & Perpendicularity

At standard ranges (0.002–0.005 in.), all three controls are baseline-cost callouts on CNC — they fall within normal process capability. The cost diverges when you tighten below 0.001 in., where stress-relieved stock, light finish passes, and CMM verification become necessary.

ControlStandard Range (Baseline Cost)Tight Range (Premium)What Drives the Premium
⏤ Flatness0.002–0.005 in. (0.05–0.13 mm)0.0005–0.001 in. (+30–60%)Stress-relieved stock, light skim cut, CMM verification. Large surfaces (>8 × 8 in.) are harder to hold flat due to internal stress release during machining.
∥ Parallelism0.002–0.005 in. (0.05–0.13 mm)0.0005–0.001 in. (+25–50%)Requires flipping part on precision vise and re-indicating against datum face. Both faces must be machined in controlled sequence. Thin cross-sections amplify the cost.
⊥ Perpendicularity0.002–0.005 in. (0.05–0.13 mm)0.0005–0.001 in. (+25–50%)Spindle tram must be verified. Tall thin walls deflect under cutting forces — requires climb milling with light radial engagement and spring passes.

Rates based on 2025–2026 US job shop averages. For the full cost table across all 12 GD&T controls, see GD&T for CNC machining.

Avoid These

Common Mistakes with Flatness, Parallelism & Perpendicularity

Using flatness when parallelism is needed

Fix: If the surface must be aligned to another feature (datum), flatness is the wrong control — it allows the surface to be perfectly flat but tilted at any angle. Parallelism or perpendicularity captures both tilt and flatness.

Adding flatness on top of a tighter parallelism callout

Fix: If parallelism is 0.002 in. and you add flatness 0.005 in., the flatness is redundant — the parallelism zone already constrains the surface to be flat within 0.002 in. Every redundant callout adds inspection time with no value.

Calling out perpendicularity without identifying the datum on the drawing

Fix: Perpendicularity requires a datum reference. If the datum feature is not labeled with a datum feature symbol on the drawing, the shop will issue an RFI — or worse, the inspector will assume a datum and the measurement becomes meaningless.

Specifying tight flatness on a large thin plate

Fix: Flatness below 0.001 in. on surfaces larger than 6 × 6 in. (150 × 150 mm) may require stress-relieved material, vacuum fixturing, and multiple light passes. This can double the machining time. If the mating surface is only 2 × 2 in., call out flatness on that local area using a note — not on the entire surface.
Common Questions

Flatness vs Parallelism vs Perpendicularity FAQ

What is the difference between flatness and parallelism in GD&T?
Flatness is a form control that constrains a surface between two parallel planes without referencing any datum — it only controls whether the surface is wavy or bowed. Parallelism is an orientation control that constrains a surface (or axis) between two parallel planes that are parallel to a datum plane. Parallelism controls both the tilt of the surface relative to the datum and inherently controls the flatness of the surface (the surface must be flat within the parallelism tolerance zone). Use flatness when the surface does not relate to any other feature. Use parallelism when two surfaces must be aligned parallel to each other.
When should I use flatness vs parallelism vs perpendicularity?
The decision follows a simple tree: (1) Does the surface relate to another feature on the part? If no → use flatness (or no GD&T at all if the surface is non-functional). If yes → ask: what angle must it be relative to the datum? If 0° (parallel) → use parallelism. If 90° (square) → use perpendicularity. If any other angle → use angularity. Flatness is for isolated surfaces; parallelism and perpendicularity are for surfaces that must be aligned relative to a datum.
Does parallelism control flatness?
Yes. Parallelism inherently controls flatness because the tolerance zone is two parallel planes — the surface must fit between those planes, which means it must also be flat within that zone. Per ASME Y14.5-2018, if you call out parallelism of 0.003 in. to a datum, the surface must be both parallel to the datum within 0.003 in. and flat within 0.003 in. There is no need to add a separate flatness callout unless you need flatness tighter than the parallelism tolerance (which is unusual).
Does perpendicularity control flatness?
Yes, for the same reason as parallelism. The perpendicularity tolerance zone for a surface is two parallel planes that are perpendicular to the datum. The surface must fit between those planes, so it must be flat within the perpendicularity tolerance. A perpendicularity callout of 0.003 in. means the surface is both square to the datum within 0.003 in. and flat within 0.003 in. Adding a separate flatness callout is only necessary if the flatness requirement is tighter than the perpendicularity tolerance.
Can I call out both flatness and parallelism on the same surface?
Yes, but only when the flatness requirement is tighter than the parallelism requirement. For example: parallelism 0.005 in. to datum A (controls tilt) plus flatness 0.001 in. (controls local waviness). The flatness tolerance must be less than or equal to the parallelism tolerance — calling out flatness of 0.010 in. with parallelism of 0.003 in. is contradictory because parallelism already forces flatness within 0.003 in. In practice, dual callouts are uncommon. If you need tight flatness and parallel alignment, set the parallelism tolerance to the tighter value.
What is ASME Y14.5 Rule #1 and how does it relate to flatness?
Rule #1 (the Envelope Principle) states that the form of a regular feature of size (e.g., a shaft diameter, a slot width) at any cross-section must not extend beyond the envelope of perfect form at Maximum Material Condition. In practical terms: a shaft with a diameter tolerance of ±0.005 in. is implicitly constrained in straightness and circularity by the size tolerance — the shaft must fit within a perfect cylinder at MMC. Rule #1 does not directly apply to non-features-of-size like flat surfaces, but it establishes that separate form callouts (flatness, cylindricity, circularity, straightness) are only needed when the form requirement is tighter than what the size tolerance already controls.
How much does flatness or parallelism cost on CNC parts?
At standard ranges (0.002–0.005 in. / 0.05–0.13 mm), flatness and parallelism are baseline-cost callouts — CNC milling naturally produces surfaces within this range without special setup. Tighter values (0.0005–0.001 in. / 0.013–0.025 mm) add 25–60% to per-part cost due to stress-relieved stock, light finish passes, and CMM verification. Parallelism may require flipping the part on a precision vise and re-indicating against the datum face. The inspection cost is similar for both: surface plate with indicator for routine checks, CMM for tight tolerances or formal documentation.
How does CNC machine perpendicularity on a part?
CNC machines produce perpendicularity naturally because the spindle axis is aligned perpendicular to the machine table (typically within 0.0002 in. per foot / 0.005 mm per 300 mm). Any face milled in a single setup is inherently perpendicular to the face sitting on the vise jaws (which serves as the datum). Tight perpendicularity (0.001 in. or tighter) requires careful attention to spindle tram, rigid fixturing, and avoiding thin walls that deflect under cutting forces. For tall, thin walls, climb milling with light radial engagement and multiple spring passes is the standard approach.

Related Resources

GD&T Guide
Complete guide: datums, symbols, form/orientation/location controls
GD&T for CNC Machining
Cost impact and inspection method per GD&T control
GD&T Symbols Chart
All 14 symbols with zone shapes and datum rules
Surface Finishes Guide
Ra values, coatings, and specification per process
CNC Tolerances Guide
Standard, precision, and ultra-precision tolerances
DFM Guidelines
15 design-for-manufacturing rules for CNC and sheet metal

CNC Parts to GD&T Spec — Free DFM Review

Upload your drawing with flatness, parallelism, or perpendicularity callouts. MakerStage engineers review every feature control frame and flag redundant or over-specified tolerances before quoting.

Get Free Quote Fast