New to Engineering? Learn GD&T Explained Simply – Straightness, Flatness, Circularity, Cylindricity, Profile, Angularity, Perpendicularity, Parallelism, Position, Runout, Datums, Tolerance Zones and Inspection

Introduction:

Geometric Dimensioning and Tolerancing (GD&T) is a symbolic language used on engineering drawings to define the allowable variation in the form, orientation, location and size of a part. Unlike traditional plus minus tolerancing which creates square tolerance zones, GD&T focuses on how parts actually fit together in the real world often using circular tolerance zones that provide more usable area for manufacturing.

Feature Control Frame:

To understand a GD&T callout, you have to break down the Feature Control Frame, which acts like a sentence describing the requirement for a specific surface or hole.

Geometric Symbol:

What characteristic are we controlling? (e.g., Is it flat? Is it round? Is it in the right spot?)

Tolerance:

The total amount the feature can vary. For a hole, this is often preceded by a diameter symbol ($\varnothing$).

Material Modifiers:

Most commonly MMC (Maximum Material Condition, symbolized by Ⓜ). This allows for "bonus tolerance" if the part is machined away from its tightest limit.

Datums:

The reference points, lines, or planes (A, B, C) that the part is measured from.

The 14 Main Symbols:

These symbols are categorized into five types of tolerances:

Form:

Flatness, Straightness, Circularity, Cylindricity

Orientation:

Perpendicularity, Angularity, Parallelism

Location:

Position, Symmetry, Concentricity

Profile:

Profile of a Line, Profile of a Surface

Runout:

Circular Runout, Total Runout

Why Use GD&T Instead of Linear Dimensions?

It guarantees that mating parts like a bolt and a hole will always fit together, even at their worst manufacturing limits. By using circular tolerance zones, you gain roughly 57% more tolerance area compared to a square zone meaning fewer parts are wrongly rejected. It removes ambiguity. A "straight" line in linear dimensioning is subjective, in GD&T, it has a mathematically defined limit.

Datums:

Datums are the most critical part of the system. Imagine trying to measure the height of a table on a bumpy floor; the floor is your (unreliable) datum. In machining, we use Datum Simulators (like a high-precision granite surface plate) to create a perfect theoretical plane from which to measure the actual part.

For CNC programming, understanding the Datum Reference Frame is essential because your Work Offset (G54, etc.) is usually aligned with the primary, secondary, and tertiary datums defined in the GD&T.

Feature and Feature of Size:

In GD&T and machining, understanding the difference between a Feature and a Feature of Size (FOS) is the foundation for setting up your work offsets and interpreting blueprints correctly.

What is a Feature?

A Feature is any physical portion of a part. It is a general term for any thing you can point to on the metal. Features do not necessarily have a size in the sense of a diameter or width, they are simply surfaces or shapes. A simple feature is usually controlled by Flatness or Profile.
e.g. A flat top surface, a chamfer, a thread or a single face of a hex bolt.

What is a Feature of Size (FOS)?

A Feature of Size is a specific type of feature that is associated with a size dimension like a diameter or a thickness. To be a FOS, the feature must have opposing points. There are two main categories:

A. Regular Feature of Size:

This is a shape that has two opposing surfaces like a slot or a circular surface like a hole or a cylinder. If you can measure it with a micrometer or a caliper and get a single size reading, it is likely a Regular Feature of Size.

e.g. 

Internal: A bore or a pocket width.

External: A shaft diameter or the total thickness of a block.

B. Irregular Feature of Size:

These are shapes that contain a group of features like a pattern of holes or complex shapes where the size isn't a simple diameter but the features still function together as a single unit for assembly.


The Center is the most important part for a CNC programmer or operator. Features only have a surface. When you probe a single flat face on your VMC, you are touching a surface feature. Features of Size have a center plane or a center axis. When you use a probe to find the center of a hole, you are finding the axis of a Feature of Size.

When you are looking at your Fanuc offset screen (G54, G55, etc.). If you touch off your Z-axis on the top of the part, you are using a Surface Feature. If you probe a bore to find X0, Y0, you are using the axis of a Feature of Size. In PowerMill, when you select a Boundary, you are usually selecting the edges of a feature. But when you define a Workplane at the center of a boss, you are defining it based on the Feature of Size.

At the atomic level, a Feature of Size is defined by the distance between two opposing sets of atomic lattices. If the material expands due to heat, the distance between those lattices increases, changing the Size of the feature which is why we must account for thermal expansion when holding tight tolerances.

Datum:

In the world of manufacturing and GD&T, a Datum is a theoretical, mathematically perfect reference point, line or plane. It is the zero or the anchor from which you measure all other features on a part. Think of a Datum like the ground when you measure the height of a building. Without a flat, stable ground to start from, your height measurement is meaningless.

Datum Feature: This is the actual physical surface on your part i.e. the rough casting or the machined face. It is never perfect, it has high spots, low spots and tilt.

Datum Feature Simulator: This is the precision equipment you use to touch the part like a granite surface plate, a CNC fixture or a machine table. It contacts the high points of the Datum Feature to create a stable base.

Datum: This is the perfect mathematical plane derived from the simulator. It is what your CNC's G54 or your CMM uses as the coordinate system.

The Datum Reference Frame:

A single Datum isn't enough to fully lock a part in space. To stop a part from moving or rotating, we use a Datum Reference Frame (DRF) which consists of three perpendicular planes (X, Y and Z).

Primary Datum (A): Usually a large flat surface. It establishes the orientation of the part and stops it from tilting. Locks 3 degrees of freedom.

Secondary Datum (B): Usually a side or a hole. It stops the part from rotating or sliding in one direction. Locks 2 degrees of freedom.

Tertiary Datum (C): Stops the final sliding movement. Locks the last 1 degree of freedom.

Why Do We Use Datums?

Without Datums, every machinist and inspector would measure the part differently leading to tolerance buildup and parts that don't fit. In the real world, a part doesn't float in air, it sits against a bracket or a motor housing. By labeling that mounting surface as Datum A, the drawing ensures the machinist prioritizes the accuracy of the same surface that will actually touch the mating part. If a drawing says "The hole must be 50mm from the edge," which edge do you mean? The top? The bottom? Is the edge straight? By saying 50mm from Datum B, the drawing tells the machinist exactly which physical surface to touch off on. In CNC programming, your Work Offset (G54, G55) is almost always the intersection of your Datums. Datum A might be the top of the part (Z0). Datum B might be the back jaw of the vise (Y0). Datum C might be a work stop (X0).

What Happens Without Datums?

Imagine trying to measure the distance between two holes on a potato. Because there are no flat, reliable surfaces, every time you pick up the potato, you will get a different measurement. Datums turn your potato (the raw material) into a precision block by establishing a repeatable coordinate system.

How to choose which surface should be Datum A on a complex part?

Choosing Datum A (the Primary Datum) is the most critical decision in a GD&T scheme. Because it is the first surface to touch the simulator like your machine table or a granite block, it sets the orientation for everything else. If you pick a bad Datum A, your measurements will wobble and your tolerances will be much harder to hold. When looking at a complex part, ask yourself these three questions in order:

Which surface actually touches the other part in the assembly?

If your part bolts onto a flat motor housing, that flat mounting face should be Datum A. This ensures that the way you measure the part matches the way it will actually be used.

Which surface is the largest and flattest?

To lock down 3 degrees of freedom (pitch, roll and Z translation), you need a stable base. Using a tiny little boss as Datum A for a giant plate is like trying to balance a table on a single pebble, it will rock.

Can you actually touch this surface during manufacturing and inspection?

If a surface is hidden inside a deep pocket or is a rough, unmachined casting, it makes a poor Datum A. You want a surface that is easy to reach with a probe, a dial indicator or a vise jaw.

Pick the surface that is Big, Flat and Functional.

Depending on the shape of your complex part, Datum A usually falls into one of these categories:

Part Type                  Best Choice for Datum A           Why?

Prismatic (Blocks)       The largest flat face.              Provides the most stability for                                                                                       the 3-2-1 setup.

Cylindrical (Shafts)      The center axis or a              Defines the rotational large                                             mounting flange.                   centerline for runout and 

                                                                                   concentricity.      

Castings/Forgings        Three specific                      Since raw castings are                                                    "Datum Targets"                    never flat, you pick 3                                                       (points).                                specific points to create a                                                                                              stable plane.

If you are a CNC programmer, a great way to choose Datum A is to look at your First Operation. Datum A should ideally be the surface you machine first, or the surface you use to sit the part in the vise/fixture. By making the machining setup match the drawing datums, you eliminate stack up error. If your G54 Z-zero is Datum A, your toolpaths will naturally be more accurate relative to the print.

What to Avoid?

Avoid choosing a threaded hole as Datum A. Threads are notoriously difficult to measure as a primary reference. Avoid thin walled surfaces. If the surface flexes when you clamp it, your Datum plane will change shape making all your other measurements look wrong. Avoid inclined surfaces unless necessary. It is much easier to set up a part on a surface that is perpendicular to your machine spindle.

Straightness:

Straightness is a form tolerance that controls how much a specific line on a surface or an axis is allowed to bend, twist or curve. Since it is a Form tolerance, it is independent meaning it does not require a Datum (A, B or C) to be measured. There are two distinct ways Straightness is applied: Surface Straightness and Median Line (Axis) Straightness.

1. Surface Straightness:

This is the most common use. It ensures that a line along the surface of a part stays within a flat, 2D tolerance zone. Two parallel lines spaced a specific distance apart (e.g. 0.1mm). Any line element you trace on that surface must fit between those two lines. Often used on long cylinders like a hydraulic piston to make sure they don't have a hump in the middle or on flat surfaces where one direction needs to be straighter than the overall flatness allows.

2. Derived Median Line (Axis) Straightness:

When the Straightness symbol is placed under a diameter dimension or attached to a Feature Control Frame with a diameter symbol (Ø), it controls the center axis of the part rather than the skin. A 3D cylinder that surrounds the theoretical perfect axis. The actual spine of the part must stay inside that tiny cylinder. This is the only version of Straightness where you can use the Maximum Material Condition (Ⓜ) modifier.

Straightness vs. Flatness:

A common point of confusion is how Straightness differs from Flatness. Straightness is 1D like a single pencil line. You check it by moving an indicator across the part in one direction. Flatness is 2D like the whole tabletop. You check it by moving an indicator across the entire surface area. If you have a rug, Straightness ensures each individual thread is straight. Flatness ensures the whole rug doesn't have any wrinkles across its entire area.

Why Use It?

On long, thin shafts, the part might be within its diameter limits but still be curved like a banana. Straightness prevents this so the shaft can spin without vibrating. On a long manifold, you might need a specific line to be very straight so a gasket can seal properly. Axis straightness (with Ⓜ) is often used to ensure a long pin will always slide into a long hole, even if the pin has a slight bow.

We use Maximum Material Condition (MMC) in axis straightness primarily to guarantee interchangeability and to provide bonus tolerance that reflects the physical reality of how parts fit together. When you apply Ⓜ to an axis straightness callout, you are defining a Virtual Condition, a boundary of perfect air that the part must never cross.

The most common reason to use MMC with axis straightness is for a long pin or bolt that must fit into a long hole.

VC = MMC Size + Straightness Tolerance (for a shaft).

As long as the combination of the shaft's size and its bend (straightness error) doesn't exceed this boundary, it will always slide into the mating part.

Without the Ⓜ symbol, the straightness tolerance is RFS (Regardless of Feature Size). This means if the limit is 0.1, the axis cannot bend more than 0.1, even if the shaft is machined very thin.

With MMC, if the shaft is at its Largest Size (MMC), it has zero "wiggle room" in the assembly. It must be very straight (e.g., 0.1 limit). If the shaft is machined Smaller, there is now extra space between the shaft and the hole. GD&T allows you to use that extra space to let the shaft bend more.

Actual Shaft Size    Bonus        Total Straightness Allowed

10.0 (MMC)               0.0               0.1
9.9                             0.1               0.2
9.8                             0.2               0.3

The biggest practical reason we use MMC for axis straightness is that it allows for a Functional Sleeve Gauge. Instead of using a CMM to mathematically calculate the derived median line which is difficult and time consuming, you can use a simple tube (a Go gauge) bored to the Virtual Condition size.

If the part slides through the tube, it is functional and passes. If the shaft is small and bent, it slides through. If it is large and straight, it slides through. The gauge doesn't care about the math; it only cares about the fit.

Axis Straightness at MMC (Ⓜ) to a Hole:

When we apply Axis Straightness at MMC (Ⓜ) to a hole, we are essentially defining a Minimum Clear Path. This ensures that a perfectly straight bolt of a certain size will always be able to pass through the hole even if the hole itself is slightly bowed or tilted.

To calculate the gauge size for a hole, we use the Virtual Condition (VC). For a hole, the Virtual Condition is the smallest possible hole, made even smaller by the straightness error.

Virtual Condition (VC) = MMC Size - Straightness Tolerance

Imagine you are machining a long sleeve for a hydraulic assembly:

Hole Size: Ø20.0 to Ø20.5

Axis Straightness: Ø0.3 Ⓜ

For a hole, Maximum Material Condition is the smallest size (where there is the most metal).
MMC = 20.0

20.0 - 0.3 = 19.7

Your physical Go gauge (the sleeve gauge) will be a precision-ground pin with a diameter of 19.7. The gauge pin represents the Worst Case mating part.

Actual Hole Size      Bonus Tolerance     Total Allowed Straightness Error

20.0 (MMC)                  0.0                               0.3
20.2                              0.2                               0.5 
20.5 (LMC)                   0.5                               0.8


If you drill the hole to 20.5, it is much larger than the 19.7 gauge pin. This means the hole's axis can curve or bend much more (up to 0.8) and the 19.7 pin will still slide through. As a machinist, if your drill starts to wander or the part warps during heat treat, you might be able to save the part by simply boring the hole out toward the larger limit (20.5).

Measuring the Axis of a hole is technically difficult. A CMM has to take many points inside the hole and mathematically calculate where the center spine of the hole is. A Functional Pin Gauge is much faster and more reliable because it checks the whole length: A CMM might miss a hump in the middle of a long hole. A pin gauge won't. It's a simple Yes/No. If the pin goes through, the assembly will work.

Flatness:

Flatness (▱) is a 3D form tolerance that ensures an entire planar surface is flat preventing it from bowing, cupping or twisting. Because Flatness is a Form control, it is completely independent and never uses a Datum reference. It only controls the shape of the surface itself, regardless of where that surface sits or how it is oriented relative to the rest of the part.

Tolerance Zone:

The tolerance zone for Flatness consists of two parallel planes separated by the specified tolerance value (e.g. 0.05 mm). Every high point and low point on the physical surface must lie between these two theoretical planes. Unlike Straightness which controls a single line path, Flatness acts across the entire surface area simultaneously.

Surface Flatness vs. Derived Median Plane (DMP) Flatness:

The difference between Surface Flatness and Derived Median Plane (DMP) Flatness lies entirely in what the feature control frame is attached to: the outer skin of the material versus the imaginary center plane of the feature size.

Surface Flatness:

When the feature control frame points directly to a flat surface or its extension line, it controls the outer skin of the part.

Tolerance Zone:

Two parallel planes separated by the tolerance value (e.g. 0.1 mm). Every peak and valley on the physical surface must fit between these two planes. No datum is used. The parallel planes can tilt or translate freely to best fit the actual surface. You cannot use the Maximum Material Condition (Ⓜ) modifier on surface flatness. Sealing gasket faces, mounting flanges or granite surface plates where direct contact and surface contact area matter.

Derived Median Plane (DMP) Flatness:

When the feature control frame is placed directly under a thickness dimension or attached to the size callout arrow, it controls the centerline plane of the material rather than the surface skin. For every pair of opposing points on the physical surfaces, a mathematical midpoint is calculated. The collection of these midpoints forms the Derived Median Plane.

Tolerance Zone: 

Two parallel planes separated by the tolerance value, surrounding this calculated center plane. The imaginary spine or center plane of the part must lie within the tolerance zone. You can use the Maximum Material Condition (Ⓜ) modifier, granting bonus tolerance as the feature moves away from its MMC size.

Controlling overall bow or warpage in sheet metal, plates, or keys to ensure they slide into a slot, regardless of local surface roughness.

Flatness vs. Straightness:

Straightness is a 2D line check like sweeping an indicator across one line. Flatness is a 2D/3D surface check covering the full length and width.

Flatness vs. Parallelism:

Flatness does not require a datum, the tolerance zone can tilt freely in space to envelope the surface. Parallelism requires a datum and locks the orientation parallel to that reference plane.

Inspection:

To check Surface Flatness manually, support the part on three adjustable jacks on a granite surface plate. Adjust the jacks until three outer points of the surface read equal height on a dial indicator. Traverse the indicator across the entire surface area. The total peak to valley variance is your Flatness value.

Calculation for a slot or tab using Derived Median Plane Flatness at MMC:

For an external feature (Tab) or an internal feature (Slot), calculating Derived Median Plane (DMP) Flatness at Maximum Material Condition (MMC) determines the Virtual Condition (VC), the maximum functional envelope used to size fixed limit gauges.

Calculation for an External Feature (Tab):

Part Callout:

Tab Thickness: 12.0 mm - 12.4 mm

Tolerance: Flatness 0.2 mm Ⓜ (placed directly under the 12.0-12.4 dimension)

For a tab (male feature), Maximum Material Condition is the largest physical size.
MMC Size = 12.4 mm

Virtual Condition (VC):

The Virtual Condition represents the worst case combined outer boundary (thickness + maximum bow).

VC = MMC Size + DMP Flatness Tolerance

VC = 12.4 mm + 0.2 mm = 12.6 mm

As the tab is machined thinner toward LMC = 12.0 mm, it gains bonus flatness tolerance:

Bonus Tolerance = MMC Size - Actual Manufactured Size

Total Allowed Flatness = Specified Flatness + Bonus Tolerance

Actual Tab Thickness   Bonus Tolerance   Total Allowed DMP      Outer                                                                                           Flatness                  Functional                                                                                                                    Envelope

12.4 mm (MMC)               0.0 mm                      0.2 mm                       12.6 mm
12.3 mm                           0.1 mm                      0.3 mm                       12.6 mm
12.2 mm                           0.2 mm                      0.4 mm                       12.6 mm
12.1 mm                           0.3 mm                      0.5 mm                       12.6 mm
12.0 mm (LMC)                0.4 mm                      0.6 mm                       12.6 mm

To verify this tab on the shop floor, build a receiver block with two parallel plates separated by a gap equal to the Virtual Condition:

Gauge Gap Width = 12.6 mm

Calculation for an Internal Feature (Slot):

Part Callout:

Slot Width: 15.0 mm - 15.4 mm

Tolerance: Flatness 0.3 mm Ⓜ

For a slot (female feature), MMC is the smallest opening (most internal metal remaining).

MMC Size = 15.0 mm

Virtual Condition (VC):

The Virtual Condition is the smallest clear passage through the bowed slot.

VC =MMC Size - DMP Flatness Tolerance
VC = 15.0 mm - 0.3 mm = 14.7 mm

Bonus Tolerance Across Manufacturing Sizes:

Bonus Tolerance = Actual Manufactured Size - MMC Size

Actual Slot Width   Bonus Tolerance  Total Allowed DMP      FlatnessInner                                                                                                              Clear Passage

15.0 mm (MMC)         0.0 mm                     0.3 mm                         14.7 mm
15.1 mm                     0.1 mm                     0.4 mm                         14.7 mm
15.2 mm                     0.2 mm                     0.5 mm                         14.7 mm
15.3 mm                     0.3 mm                     0.6 mm                         14.7 mm
15.4 mm (LMC)          0.4 mm                     0.7 mm                         14.7 mm

The functional GO gauge for this slot is a ground parallel plate with a thickness equal to the Virtual Condition:

Gauge Plate Thickness = 14.7 mm

Circularity:

Circularity often called Roundness is a 2D form tolerance that controls how close a cross section of a cylindrical or spherical object is to a perfect circle. Because it is a Form tolerance, it does not require a Datum. It only cares about the shape of the part itself not where the part is located in space.

Tolerance Zone:

The tolerance zone for circularity consists of two concentric circles one inside the other on a plane perpendicular to the axis. The distance between the inner and outer circle is the tolerance value (e.g. 0.05). Every point on the surface of that specific cross section must fall within that narrow ring.

How is it Different from Cylindricity?

This is the most common point of confusion. Circularity is a 2D check. You check one slice of the part at a time. It doesn't care if the next slice is a different size (taper) or if the slices don't line up (straightness). Cylindricity is a 3D check. It covers the entire length of the part at once, including taper and straightness. If you are checking a stack of coins, Circularity checks if each individual coin is round. Cylindricity checks if the whole stack forms a perfect, straight and non tapered column.

Circularity vs. Diameter:

A part can be within its Diameter tolerance but fail Circularity.
A classic example is a lobed shape like a Reuleaux triangle. If you measure it with a micrometer at any two opposite points, the distance might always be 10.0mm passing diameter, but the shape is clearly not a circle failing circularity.

Why Use It?

In rotating shafts, if a shaft isn't round, it will create runout and vibration even if the average diameter is correct. Ball bearings must be extremely round to distribute loads evenly. Even a tiny flat spot will cause heat and premature failure. For a rubber O-ring to seal a fluid, the groove it sits in must be circular. If the groove is oval, the ring will be pinched in some areas and loose in others, causing a leak.

Inspection:

V-Block Method: Placing the part in a V-block and rotating it under a dial indicator.

CMM/Roundness Tester: A probe traces the circumference and a computer calculates the Least Squares Circle to determine how much the actual shape deviates from a perfect one.

Cylindricity:

Cylindricity is a 3D form tolerance that ensures a feature is a perfect cylinder. Unlike circularity which only checks one 2D slice at a time, cylindricity controls the entire surface of the part simultaneously. Think of Cylindricity as the ultimate control for a shaft or a hole. While Straightness only cares about how much the part bows or curves, Cylindricity manages the entire 3D form. If a part passes a Cylindricity check, it is guaranteed to be straight, round and have zero taper. Cylindricity is considered a powerful and expensive tolerance because it automatically controls three other characteristics at once:

Circularity (Roundness): Every cross section must be a circle.

Straightness: The part cannot be bowed or bent like a banana.

Taper: One end cannot be larger than the other like a cone.

If any of these three elements are out of spec, the part will fail the cylindricity check.

The Tolerance Zone:

The tolerance zone for Cylindricity is a 3D envelope consisting of two concentric cylinders, one inside the other. The distance between the inner cylinder and the outer cylinder is your tolerance value (e.g. 0.05). The entire surface of your part must fall perfectly within that thin wall of space.

Why Use Cylindricity?

Cylindricity is reserved for high precision components where a perfect fit is mandatory over a long distance. You use this symbol when the total form is critical for high precision movement. In engine pistons & bore, to maintain a seal and prevent blow by, the cylinder walls must be perfectly round and straight. To maintain compression, the piston and cylinder wall must stay perfectly cylindrical throughout the entire stroke. In hydraulic spools, if a valve spool is tapered or bowed, it will either leak oil or jam inside the housing. In high speed bearings, any deviation in the 3D form of a shaft will cause uneven loading and premature bearing failure. If the shaft is tapered or oval, the bearing will wear unevenly and fail.

Inspection:

As a machinist or programmer, you should know that Cylindricity is much harder to achieve and inspect than Straightness. Because it is difficult to measure, only use cylindricity when the functional fit of the entire cylinder is critical. If you only care about the part being round, use Circularity, it's much cheaper to manufacture and inspect.

Manual Inspection: You cannot accurately check cylindricity with a micrometer or a simple V-block. A micrometer only checks two point diameter which can miss lobing or bowing.

CMM/Roundness Tester: To truly verify cylindricity, a CMM must take a spiral scan or multiple circular scans at different heights and mathematically verify they all fit within the concentric cylinder envelope. On a CNC Lathe achieving great cylindricity requires perfect alignment of the tailstock and extremely sharp tooling to prevent deflection which causes taper.

If the drawing only cares about the part not being bowed, use Straightness. Only use Cylindricity if the roundness and taper are just as important as the straightness.

Parallelism:

Parallelism is an orientation control in GD&T that describes the condition of a surface or axis being equidistant at all points from a datum plane or axis. In simpler terms, if you have two lines or surfaces that are parallel, they will never meet, no matter how far they extend. In manufacturing, parallelism defines how level one feature is relative to another.

The Tolerance Zone:

Unlike a simple ± dimension, a parallelism tolerance creates a 3 dimensional envelope. For a flat surface, the tolerance zone consists of two parallel planes separated by the tolerance value (e.g. 0.05 mm). These planes are oriented perfectly parallel to the specified datum. The entire surface being controlled must live inside this 0.05 mm thick sandwich.

Feature Control Frame:

When you see a parallelism requirement on a technical drawing, it will look like this:

Symbol: Two slanted parallel lines (//).

Tolerance: The total width of the zone (e.g., 0.1).

Datum: The reference surface (e.g., A) that the feature must be parallel to.

Parallelism does not control the distance between the two surfaces that is controlled by a linear dimension. It only controls the shape and orientation of the second surface relative to the first.

At the atomic level, no surface is perfectly flat. When you machine a metal block, the parallel surface is actually a rugged landscape of atoms. While the internal crystal lattice of the metal might be uniform, the machining process like a face mill pass shears the top layers of atoms. Parallelism error occurs when the peaks and valleys of this atomic landscape trend upward or downward relative to the datum. If the tool vibrates or the part expands due to thermal energy (atoms vibrating more violently), the surface can warp, pushing the material outside the allowable parallel planes.

Inspection Methods:

To verify parallelism in a workshop, you typically use:
Surface Plate and Dial Indicator: Place the datum surface (A) down on a precision granite plate. Run a dial indicator across the top surface. The Total Indicator Reading (TIR) is your parallelism error.
CMM (Coordinate Measuring Machine): The probe takes multiple points on the datum to establish a "perfect" plane, then compares the points on the controlled surface to that plane.

Parallelism vs. Flatness:

It is common to confuse these two, but they are distinct:

Flatness: Does NOT need a datum. It only cares if the surface itself is wavy or bowed.

Parallelism: MUST have a datum. It cares how the surface is oriented compared to another surface.

Perpendicularity:

Perpendicularity is an orientation control in GD&T that ensures a surface, axis, or center plane is maintained at a precise 90⁰ angle relative to a datum (reference) plane or axis. While we often call this squareness, perpendicularity provides a specific 3D tolerance zone that defines exactly how much the angle can deviate while still being functional.

Tolerance Zone:

Perpendicularity does not measure the error in degrees (like ±0.5⁰). Instead, it defines a linear width within which the surface must exist.

For a Surface, the tolerance zone is formed by two parallel planes exactly 90⁰ from the datum. The distance between these planes is the tolerance value (e.g. 0.05 mm).

For an Axis like a hole, the tolerance zone is often a cylinder centered at 90⁰ to the datum. The axis of the hole must stay within that cylinder.

Feature Control Frame:

On a blueprint, the requirement is identified by the perpendicularity symbol (⊥):

Symbol: ⊥

Tolerance: The total allowable wobble (e.g. 0.1 mm).

Datum: The base surface or axis (e.g. B) that the 90⁰ angle is measured from.

Perpendicularity requires a Datum. You cannot have a surface that is perpendicular to nothing, it must be square to something else.

When you machine a vertical wall on a VMC using an end mill, several atomic level factors influence perpendicularity. As the cutter hits the metal, the pressure causes the tool to bend slightly away from the cut. At the atomic level, the bonds in the tool steel stretch, causing the wall to taper or lean which violates the perpendicularity zone. If the workpiece or the spindle heats up, the atoms move further apart causing the physical dimensions to shift. This can lead to a part being square when hot but out of tolerance once it cools. If the Z axis of the machine is not perfectly 90⁰ to the X-Y table, every part you make will have a built-in perpendicularity error.

Inspection Techniques:

To check if your part is truly perpendicular:

Cylinder Square & Dial Indicator: Place the part on a surface plate against a precision cylinder square. Run an indicator up the wall.

Squareness Block: Use a precision 90⁰ block as a reference.

CMM: The machine probes the bottom surface (Datum) to establish the 90⁰ vector, then probes the side wall to see if any points poke out of the allowed tolerance zone.

Perpendicularity vs. Angularity:

Perpendicularity: A specific case of angularity where the angle is fixed at exactly 90⁰.

Angularity: The general term for any angle like 30⁰ or 60⁰ but it can also be used for 90⁰. However, most engineers use the ⊥ symbol for clarity when 90⁰ is required.

Perpendicularity at MMC (Ⓜ):

Perpendicularity at MMC (Ⓜ) is essentially Axis Straightness with a Datum attached. While straightness just cares if the hole is bowed, perpendicularity cares if the hole is leaning or tilting relative to a flat surface (Datum A). The math for the Virtual Condition (VC) and the gauge design is identical to what we just covered for axis straightness.

Just like before, we are calculating the size of a perfect pin that must be able to slide into the hole when that pin is perfectly square (90 degree) to the datum surface.

Virtual Condition (VC) = MMC Size - Perpendicularity Tolerance

Hole Size: Ø10.0 to Ø10.2

Perpendicularity: Ø 0.1 Ⓜ to Datum A

MMC: Smallest hole = 10.0

Subtract Tolerance: 10.0 - 0.1 = 9.9

To check this on the shop floor, you build a gauge with a 9.9 diameter pin that is permanently fixed at exactly 90⁰ to a flat base.

The Base: Represents Datum A.

The Pin: Represents the Virtual Condition (9.9).

You press the part flat against the gauge base. If the 9.9 pin slides into the hole, the part passes. If you machine the hole to 10.2 (the large end), the hole has a 0.3 gap (10.2 - 9.9) around the pin. This allows the hole to tilt significantly more than if it were a tight 10.0 hole.

Without the Ⓜ symbol, perpendicularity is RFS (Strict).

RFS: If your hole is leaning by 0.15 and your limit is 0.1, the part is Scrap, even if the hole is huge (10.2).

MMC: If that same hole is 10.2, your allowed tilt grows to 0.3. Your 0.15 error is now Pass.

Angularity:

In Geometric Dimensioning and Tolerancing (GD&T), Angularity is a orientation control used to ensure that a surface, axis or center plane is maintained at a specific angle relative to a datum (reference) plane or axis. Unlike parallelism (0⁰) or perpendicularity (90⁰), angularity allows for any specific angle such as 30⁰, 45⁰ or 60⁰.

The Tolerance Zone:

Angularity does not define the tolerance in degrees (e.g. ± 1⁰). Instead, it creates a 3D tolerance zone consisting of two parallel planes oriented at the exact basic angle to the datum. The entire controlled surface or axis must lie between these two planes. The distance between these planes is the tolerance value specified in the feature control frame.

The Feature Control Frame:

To read an angularity requirement on a drawing, you look for the angularity symbol (∠) followed by the tolerance and the datum reference:

Symbol: ∠

Tolerance: A numerical value (e.g. 0.2) representing the total width of the envelope.

Datum: The reference surface (e.g., A) that the angle is measured from.

For angularity to be valid, the angle on the drawing must be a Basic Dimension enclosed in a box. This tells the inspector that the angle itself is theoretically exact and the allowable error is captured by the tolerance zone width.

Why Use Angularity?

Angularity is critical when the functional fit of a part depends on a precise slope. Common applications include: V-blocks and specialized fixtures, Countersinks or angled bores where a bolt head must sit flush, Cam surfaces where the timing of a machine depends on the slope of the part.

Measuring Angularity:

In a machining environment like using a VMC, angularity is typically inspected using:

Sine Bars and Gauge Blocks: To set the part at the precise theoretical angle and then sweep the surface with a dial indicator.

CMM (Coordinate Measuring Machine): Probing the surface and comparing the data points to the CAD model’s basic angle.

How to calculate the tolerance zone for a specific angled cut you're working on?

To calculate the angularity tolerance zone, we focus on the linear distance between two parallel planes, rather than the angular degrees of error. In a machining context, this is crucial because your dial indicator or CMM measures displacement not just angle.

When you have a surface at a basic angle (α) and a specified angularity tolerance (t), the tolerance zone is a sandwich of space. If you are inspecting this on a surface plate using a Sine Bar, the height (H) you need to set for your gauge blocks is calculated using:

H = L × sin(α)

Where,
L = The length of the sine bar (typically 5 inches or 100 mm).
α = The basic angle specified on your drawing.

Example:

Imagine you are machining a block with a 30⁰ sloped face and a feature control frame specifying an angularity of 0.05 mm relative to Datum A.

The Basic Angle: 30⁰ (This is the perfect theoretical path).

The Tolerance (t): 0.05 mm.

The Zone: You have two imaginary planes exactly 0.05 mm apart, tilted at exactly 30⁰. Your actual machined surface must stay entirely inside that 0.05 mm gap.

Checking for Out of Tolerance:

If you are using a dial indicator to sweep the surface after setting it up on a sine bar:

Step 1: Set the part on the sine bar at the basic angle so the sloped surface is now technically parallel to the surface plate.

Step 2: Zero your indicator at one end of the cut.

Step 3: Move the indicator across the length of the cut.

Result: If the total indicator reading (TIR) is ≤ 0.05 mm, the part is within the angularity tolerance.

When we look at this flat surface at a microscopic level, we aren't seeing a smooth line. We are seeing a landscape of atoms held together by metallic bonds. The Tolerance Zone essentially defines how much vertical displacement is allowed for those atomic structures relative to the theoretical plane. Even if the angle feels correct, a high-frequency vibration during the cut or a slightly dull tool can cause the atomic peaks to exceed that 0.05 mm boundary even if the average slope is perfect.

Profile of a Line:

Profile of a Line is a 2D geometric tolerance that controls the shape or contour of an individual cross section of a feature. While Straightness or Circularity only control specific types of shapes like straight lines or circles, Profile of a Line can control any shape from a simple flat edge to a complex, wavy curve like a turbine blade or a car's body panel.

Tolerance Zone:

Imagine taking a thin slice of your part. The True Profile is the mathematically perfect shape defined by the basic dimensions on your drawing. Two parallel lines follow the path of that True Profile. The distance between these two lines is your tolerance value (e.g. 0.05). The actual edge of your part in that specific slice must stay within that 0.05 ribbon.

How it Differs from Profile of a Surface?

This is the most important distinction in GD&T:

Profile of a Line (2D): Only checks individual ribbons or slices. It does not care if the next slice is slightly different or shifted. It is like checking a loaf of bread by looking at one slice at a time.

Profile of a Surface (3D): Checks the entire face of the part at once. It ensures the whole loaf is the right shape, not just the slices.

With Datums vs. Without Datums:

Profile of a Line is unique because it can be used in two ways:

Without Datums (Form): It only controls the shape. As long as the curve is the right wiggle, it doesn't matter where it sits on the part.

With Datums (Location/Orientation): It controls the shape AND where it is located relative to the rest of the part. This is common for critical mating edges.

Why Use It?

You typically see Profile of a Line on parts where the 2D cross section is more important than the 3D surface, such as:

Extrusions: If you are manufacturing aluminum trim or a heat sink, you care that the 2D cross section is correct but the length is just a straight pull.

Gaskets: A flat gasket's sealing power depends on the shape of its edge in 2D.

Camshafts: The specific lift profile of a cam lobe at a specific angle is often controlled by Profile of a Line.

Inspection on the Shop Floor:

Optical Comparator: This is the classic tool. You project a shadow of the part's slice onto a screen and compare it to a template or overlay that shows the tolerance ribbon.

CMM: The probe takes points along a single path across the part and compares those points to the CAD model.

Profile of a Surface:

Profile of a Surface is arguably the most powerful and versatile tool in the GD&T toolbox. While Profile of a Line only checks individual slices, Profile of a Surface controls the entire 3D skin of a part at once. It is a 3D boundary that can control Form, Orientation and Location all in one single symbol.

The 3D Tolerance Zone:

Imagine your part's surface is wrapped in a sandwich of two perfectly shaped boundaries. The True Profile is the mathematically perfect surface defined by your CAD model or basic dimensions. Two surfaces offset from that True Profile. If your tolerance is 0.2, you have a 0.2 thick zone that follows every curve, flat and angle of the part. Every single point on the actual physical surface of your part must fall between those two boundaries.

With Datums vs. Without Datums:

Depending on whether you use Datums, Profile of a Surface changes what it polices.

Without Datums (Form): It only controls the Form. Is the part the right shape? Like Flatness or Cylindricity.

With Datums (Location/Orientation): It only controls the Form, Orientation, & Location. Is the part the right shape, is it tilted correctly and is it in the right spot?

Bilateral vs. Unilateral:

By default, the tolerance zone is Bilateral. If the tolerance is 0.2, it's 0.1 extra material and 0.1 less material. However, you will often see the Unequally Disposed Profile (Ⓤ) symbol:

[⌢ | 0.2 Ⓤ 0 | A | B | C]: This means the 0.2 tolerance is all inside the part (you can only remove material).

[⌢ | 0.2 Ⓤ 0.2 | A | B | C]: This means the 0.2 is all outside the part (the part can only be larger).

Why is it used so much today?

In modern CNC machining and 3D printing, we don't just make blocks and cylinders anymore, we make complex organic shapes like a turbine blade, a car door or a plastic phone case. In Traditional GD&T, you would need 50 different dimensions to describe a car's fender. In Profile of a Surface, you just point to the whole surface and say Stay within 0.5 of the CAD model relative to Datums A, B and C. It simplifies the drawing and tells the CMM or scanner exactly what to check against the digital model.

Inspection:

On the shop floor, the best way to visualize Profile of a Surface is through a CMM Color Map. When you scan the part, the software compares the physical points to the CAD model.

Green: Perfect (middle of the zone).
Red: Too much material (outside the boundary).
Blue: Not enough material (inside the boundary).

Position:

In GD&T, Position (⌖) is a location control that defines how far a feature's true center i.e. axis or center plane is allowed to vary from its True Position i.e. the exact theoretical location defined by basic dimensions. It is the most widely used GD&T characteristic for features of size like holes, pins, slots, and studs.

Cylindrical Tolerance Zone:

Unlike standard ± linear dimensions that create a square tolerance box, position typically creates a cylindrical tolerance zone around the theoretical center line. A 3D cylinder centered at the basic X and Y coordinates relative to Datums A, B, and C. The central axis of your machined hole or pin must lie completely inside this cylinder along its entire depth. A square ± 0.1 box restricts diagonal variation. A circular zone with diameter Ø0.28 covers the corners of that square, giving you 57% more usable area without compromising fit.

Feature Control Frame:

A typical callout looks like [ ⌖ | ⌀0.1 Ⓜ | A | B | C ]:

Symbol (⌖): Position.

Zone Diameter (Ø 0.1): Specifies a cylindrical zone of diameter 0.1 mm.

Modifier (Ⓜ): Maximum Material Condition (MMC), meaning you gain Bonus Tolerance if the feature size departs from MMC.

Datums (A | B | C): Establishes the reference coordinate system (Primary, Secondary, Tertiary).

Why we gain 57% more area?

To understand why we gain 57% more area, we have to compare how a hole's location is defined in Coordinate (Plus-Minus) Tolerancing versus GD&T Position.

1. Coordinate Tolerancing:

In traditional dimensioning, you might see a hole located with a tolerance of ± 0.1. This creates a Square Tolerance Zone. The hole can move 0.1 units up, down, left or right. The total width of the square is 0.2 and the total height is 0.2.

Area of the Square = 0.2 * 0.2 = 0.04 units².

The problem with the square is the corners. If a hole is drilled exactly at the corner of that square at 0.1, 0.1, the actual distance from the true center is calculated using the Pythagorean theorem:

√0.1² + 0.1² ≈ 0.141

If the part functions perfectly fine when the hole is 0.141 units away at the corner, why would we reject a part that is 0.141 units away but sitting directly to the right?

In coordinate tolerancing, a hole at 0.141 to the right is out of spec (because 0.141 > 0.1), even though it is the same distance from the center as the good corner hole. This is where parts are wrongly scrapped.

2. The Circle Solution (GD&T):

GD&T uses a Circular Tolerance Zone centered on the true position. Instead of saying ± 0.1, we say Position Ø0.282. This circle's diameter is equal to the diagonal of the old square (0.141 * 2 = 0.282). Now, let's look at the math for the area of that circle with radius of 0.141.

Area of the Circle (πr²) = π * 0.141² ≈ 0.0628 units².

3. The 57% Gain:

When you compare the two areas: Square Area (0.04) and Circle Area (0.0628).

The increase in area is: (0.0628 - 0.04)/(0.04) * 100 = 57%.

By using the circle, you aren't lowering your standards, you are simply acknowledging that if the part works at the corner of a square, it works at that same distance in any direction.

Bonus Tolerance:

Bonus Tolerance is a powerful GD&T concept that allows you to grow your positional tolerance as the hole size gets larger. It is represented by the Maximum Material Condition (MMC) symbol: Ⓜ. Think of it as a reward for manufacturing. If you drill a hole larger than the minimum required size, you have more wiggle room for that hole's location before it interferes with a mating bolt.

MMC (Maximum Material Condition):

For a hole, the Maximum Material Condition is the smallest allowable hole size because that’s when the part has the most metal/material left. Let’s use an example:

Hole Size Spec: Ø10.0 to Ø10.5

Position Tolerance: Ø0.2 at Ⓜ (MMC)

In this case, the MMC is 10.0. The positional tolerance of 0.2 is only strictly enforced when the hole is exactly at 10.0.

Bonus Tolerance:

The rule is simple: Any deviation from the MMC size is added directly to the positional tolerance.

Actual Hole Size   Deviation from MMC (Bonus)   New Total Position Tolerance

10.0 (MMC)                0.0                                              Ø0.2
10.1                            0.1                                              Ø0.3
10.2                            0.2                                              Ø0.4
10.3                            0.3                                              Ø0.5
10.5 (LMC)                 0.5                                              Ø0.7


As the hole gets bigger approaching the Least Material Condition or LMC, the positional tolerance zone grows from a diameter of 0.2 to a diameter of 0.7.

The goal of the Ⓜ symbol is to maintain a constant Virtual Condition. This is the worst case boundary that the hole's surface will never cross:

Virtual Condition = MMC Size - Positional Tolerance
                            = 10.0 - 0.2 = 9.8

As long as no part of your hole enters that 9.8 no-fly zone, the part is functional.

Why is this allowed?

Imagine you are trying to fit a 9.8 diameter peg into a 10.0 diameter hole. If the hole is exactly 10.0, you only have 0.2 of total clearance. If the hole is off-center by more than that, the peg won't fit. But if you drill the hole to 10.5, you now have 0.7 of total clearance (10.5 - 9.8). Because there is more physical space between the peg and the hole walls, the hole can be more out of position than originally planned and the parts will still assemble perfectly.

Why This Matters on the Shop Floor?

A part that fails a position check at Ø0.2 might be perfectly good once the inspector measures the actual hole size and adds the bonus. MMC allows for the use of Functional Hard Gauges (physical pins). If the part slides onto the pins, it passes. You don't even need a CMM (Coordinate Measuring Machine) to calculate the math, the physical fit proves the bonus tolerance is working.

When you shift from a hole i.e. internal feature to a shaft or boss i.e. external feature, the logic stays the same, but the numbers flip. For a shaft, Maximum Material Condition (MMC) is the largest allowable size because that is when the part has the most material.

MMC (Maximum Material Condition):

If a shaft is at its maximum size, it is hardest to fit into a mating hole. If you turn that shaft down to a smaller diameter, you gain bonus space in the assembly which GD&T allows you to use as extra positional tolerance. Let's look at an example:

Shaft Size Spec: Ø10.0 down to Ø9.5

Position Tolerance: Ø0.2 at Ⓜ (MMC)

In this scenario, the MMC is 10.0. The positional tolerance of 0.2 is only strictly enforced when the hole is exactly at 10.0.

Bonus Tolerance:

The Bonus is still the difference between the Actual Size and the MMC Size.

Actual Shaft Size  Deviation from MMC (Bonus)   New Total Position Tolerance

10.0 (MMC)                    0.0                                          Ø 0.2
9.9                                  0.1                                          Ø 0.3
9.8                                  0.2                                          Ø 0.4
9.7                                  0.3                                          Ø 0.5
9.5 (LMC)                       0.5                                          Ø 0.7


Notice the trend: As the shaft gets smaller i.e. moving away from MMC), the positional tolerance gets larger. This is the opposite of the hole example where the tolerance grew as the hole got bigger.

For a shaft, the Virtual Condition (VC) is the maximum boundary that the shaft will never cross, even if it is at its largest size and worst position.

Virtual Condition = MMC Size + Positional Tolerance
                              = 10.0 + 0.2 = 10.2

This 10.2 is the size of the "perfect" hole that this shaft is guaranteed to fit into. As long as your shaft stays within that 10.2 envelope, the assembly works.

Why Use MMC for Shafts?

It ensures that even if your machinist creates a shaft at the high end of the size limit, it will still fit the mating part. Just like with holes, you can use a Ring Gauge or a plate with a hole bored to the Virtual Condition (10.2). If the shaft passes through that hole, it is a good part, no complex math required on the shop floor.

Regardless of Feature Size (RFS):

Regardless of Feature Size (RFS) is the no nonsense default in GD&T. While MMC (Ⓜ) is a generous system that gives you bonus room, RFS is strict: the positional tolerance stays exactly the same, no matter how large or small you machine the part. According to the ASME Y14.5 standard, RFS is the automatic default for all geometric tolerances unless a specific modifier like Ⓜ or Ⓛ is placed in the Feature Control Frame.

How RFS Works?

In an RFS callout, the size of the hole or shaft and the location of the hole are treated as two completely separate problems. If your print calls for a position tolerance of 0.2, that value is a hard ceiling.

If you drill a Ø10.0 hole ----> Your position tolerance is 0.2
If you drill a Ø10.5 hole ----> Your position tolerance is 0.2

There is no bonus. You don't get rewarded for leaving more wiggle room in the assembly.

When Do You Use RFS?

You might wonder why anyone would choose a stricter system. RFS is used when balance or alignment is more important than simple assembly. If you are machining a high speed shaft or a turbine, you need it to be perfectly centered for balance. If you used MMC, the shaft could be off center but still pass because it was small. In a rotating machine, that off center part causes vibration and failure. If a part is being pressed into another with zero clearance, the bonus tolerance logic of MMC doesn't apply because there is no extra space to begin with. Where parts are designed to be slightly larger than the hole they are going into.

MMC vs. RFS:

Imagine you are a machinist. Here is how your allowable error changes based on the symbol:

Feature Size         MMC (Ⓜ) Tolerance        RFS (Default) Tolerance

10.0 (Smallest)            0.2                                              0.2
10.2 (Middle)               0.4                                              0.2
10.5 (Largest)              0.7                                              0.2

RFS is significantly harder to inspect than MMC.

You cannot use a Go/No-Go pin gauge to check an RFS position. Because a physical pin can't tell the difference between a hole that is off center and a hole that is too small. To inspect RFS, you almost always need a Coordinate Measuring Machine (CMM) or a high-precision dial indicator to find the actual axis of the feature and compare it to the theoretical center.

If you see a Feature Control Frame with no circles (no Ⓜ or Ⓛ), you are in RFS territory. You have to be much more precise with your setup because the software won't give you any free tolerance based on your tool wear or hole size.

When you have a hole with an MMC (Ⓜ) modifier, you can think of it as a trade-off: If you lose accuracy in position, you can buy it back by making the hole larger. If your CNC machine’s positioning isn't perfect or if your drill walks slightly during the cut, the hole's center axis will be off center.

In RFS (Strict), if the axis is off by 0.25 and your limit is 0.2, the part is Scrap. It doesn't matter how big the hole is.

In MMC (Flexible), if the axis is off by 0.25, you can simply run a larger drill or boring bar through that same (off center) hole. By removing more material and making the hole larger, you create the extra clearance needed for the bolt to pass through.

The reason this works is because the assembly only cares about a boundary of air.

Imagine a Virtual Plug that represents the bolt. As long as your hole is large enough and positioned well enough that the Virtual Plug can pass through without hitting a wall, the part works. Small Hole must be positioned very accurately to keep the Plug from hitting the sides. Large Hole can be sloppy in its position because there is so much extra space inside the hole for the Plug to move around.

Imagine you are checking a part:

Spec: Hole Ø10.0 to 10.5 | Position Ø0.2 Ⓜ.

Inspection: Your CMM says the hole position is off by 0.3 (Fail!).

You measure the hole size and see it's currently at 10.0. You go back to the machine and bore that hole out to 10.4. You just gained 0.4 of Bonus Tolerance.

Your new allowed position error is 0.2 + 0.4 = 0.6.

Your 0.3 error is now well within the 0.6 limit. The part is Saved.

By machining more material out of the hole, you shift the inner wall of the hole further away from the center. Even though the center of the hole is still in the wrong place, the wall of the hole has moved far enough back that it no longer interferes with the mating part.

In MMC, the surface of the hole is what matters, not just the theoretical center point. Making the hole bigger moves the surface out of the way.

Example:

When you have a pattern of holes like a 4 bolt flange, GD&T becomes your best friend. In a pattern, you aren't just controlling where one hole is, you are controlling how all four holes relate to each other (Feature to Feature) and how they relate to the rest of the part (Feature to Datum).

The easiest way to visualize a pattern of holes at MMC is to imagine a Functional Gauge. This is a solid plate with four perfectly positioned steel pins sticking out of it. Each pin is exactly at the Virtual Condition size i.e. MMC Hole Size - Position Tolerance. If your 4 bolt flange slides onto these four pins, the part is Good. If it gets stuck, the part is Scrap or needs rework.

Imagine you are machining the flange. Your drill is slightly off position on Hole 3.

If the hole is small (MMC), it will hit the side of the gauge pin. The part won't slide on. You go back to the machine and bore Hole 3 to its maximum allowable size. Because the hole is now larger, there is more air around that specific pin. Even though the center of the hole is still in the wrong place, the edge of the hole has moved out of the way. The flange now slides onto the gauge.

In a pattern, the bonus tolerance is calculated individually for each hole. If Hole 1 is large, it gets a big bonus. If Hole 2 is small, it gets no bonus.

When you use MMC on a pattern, you allow the pattern to float. If all your holes are drilled at their maximum size, the entire bolt circle can shift slightly left or right and still allow the bolts to pass through.

Without GD&T and the Ⓜ symbol, a machinist would have to hold every single hole to a very tight coordinate (±) tolerance leading to high scrap rates for parts that would have actually functioned perfectly.

To design a physical gauge for a 4 hole pattern, we calculate the Virtual Condition (VC). The VC is the size of the perfect pin on your gauge that represents the worst-case scenario for the mating part. For a hole, the Virtual Condition is the smallest possible hole shifted as far as the tolerance allows.

The VC Formula for Holes:

Virtual Condition = MMC Size - Positional Tolerance

Imagine a 4 bolt flange with the following specs:
Hole Size: Ø10.0 to Ø10.4
Position: Ø0.5 Ⓜ relative to Datums A, B, and C.

For a hole, MMC is the smallest size and it is 10.0. The tolerance at MMC is 0.5.

VC = 10.0 - 0.5 = 9.5

Now that you have the VC (9.5), you can design your check gauge. A flat plate representing your Primary Datum usually the face of the flange. Four hardened steel pins each with a diameter of exactly 9.5. The pins must be located at the Basic Dimensions (the perfect theoretical coordinates) specified on the drawing.

How the Gauge Works?

If the flange slides onto all four 9.5 pins, the pattern is Good. If the flange gets stuck, it means at least one hole is either too small or too far out of position. The beauty of this 9.5 pin is that it automatically accounts for the bonus tolerance.

If your hole is exactly 10.0 (MMC), it only has 0.5 of room to wiggle around the 9.5 pin.
If you machine the hole to 10.4 (LMC), it now has 0.9 of room (10.4 - 9.5 = 0.9).

The gauge doesn't care how you got there, it only cares that the surface of the hole never crosses the 9.5 boundary. This is why functional gauges are so much faster than using a CMM for high volume production.

Internal (Hole)
Pin Diameter = Smallest Hole - Positional Tol

External (Shaft)
Hole in Gauge = Largest Shaft + Positional Tol

How to handle the Datum Shift (the Ⓜ symbol next to a Datum like A|BⓂ|C) which allows the entire gauge to move slightly during inspection?

Datum Shift is one of the most cost effective secrets in GD&T. While Bonus Tolerance (the Ⓜ next to the tolerance value) gives an individual hole more room to wiggle, Datum Shift (the Ⓜ next to a Datum letter) allows the entire pattern of holes to shift or rotate on the part. Think of it this way: Bonus Tolerance is like having a larger hole for a bolt, Datum Shift is like having a slightly loose fit between the part and the fixture itself.

You will see it in the Feature Control Frame, specifically in the Datum section:
[⌖ | ⌀ 0.5 Ⓜ | A | B Ⓜ | C]

⌀ 0.5 Ⓜ: This is your Bonus Tolerance related to the hole size.

B Ⓜ: This is your Datum Shift related to the size of the Datum feature, like a center pilot hole or a boss.

Imagine you are mounting a 4-bolt wheel onto a car's axle. The axle has a large center pilot (Datum B). The wheel has a center hole that fits over that pilot. If the wheel's center hole is machined slightly larger than the pilot, the entire wheel can jiggle slightly before you tighten the lug nuts. That jiggle is Datum Shift. Because the wheel can move, the four lug bolt holes don't have to be perfectly centered, you can simply shift the whole wheel until the bolts line up.

Datum Shift only occurs if the Datum Feature i.e. the physical part of the object used as a reference is machined away from its Maximum Material Condition (MMC).

e.g.

Datum B (Center Hole): Ø20.0 to Ø20.2
MMC of Datum B: 20.0 (Smallest hole = most metal).

Actual Size of Datum B               Available Datum Shift

20.0 (MMC)                                  0.0 (Tight fit on the gauge)

20.1                                              0.1 (The part can move 0.1)

20.2 (LMC)                                   0.2 (The part can move 0.2)

When you build a physical functional gauge for a part with Datum Shift, the gauge remains rigid, but the part is allowed to float. The Gauge Pin for Datum B is made exactly at the MMC size (20.0). You slide the part onto the 20.0 Datum pin. If the part's center hole is actually 20.2, there is a 0.2 gap. You are allowed to slide, shake or rotate the part within that 0.2 gap to help the four pattern pins find their holes. If the part fits on the gauge in any shifted position, the part is Good.

Datum Shift is used when the fit of the part depends on a primary or secondary feature. It prevents you from scrapping a perfectly functional part just because the hole pattern is slightly off center relative to a datum that itself has a loose fit.

Concentricity:

Concentricity is a complex GD&T location control used to ensure that the median points of all diametrically opposed elements of a cylindrical or spherical feature are congruent with a datum axis. In simpler terms, it controls how well the center of one circle aligns with the center of another. Concentricity focuses on the balance of a part. It ensures that the median points of all diametrically opposed elements of a cylinder or sphere are aligned with a datum axis. In simpler terms, it doesn't just check if a circle is in the right place, it checks if the material is distributed evenly around the center.

Tolerance Zone:

The tolerance zone for concentricity is a 3D cylindrical space or a sphere centered on the datum axis. Unlike other controls, concentricity does not just look at the surface. It requires the inspector to find the median points i.e. the middle point between two opposite sides of the part throughout the entire feature. All of these derived middle points must fall within the tiny cylindrical tolerance zone. To pass inspection, an inspector must measure pairs of points on opposite sides of the feature. The midpoint (median) of every single pair must fall inside that tiny cylindrical tolerance zone.

Feature Control Frame:

On a drawing, concentricity is represented by two circles with a shared center:

Symbol: ◎

Tolerance: Usually preceded by a diameter symbol (Ø), representing the width of the cylindrical zone (e.g. Ø0.03).

Datum: The reference axis (e.g. A) that the feature must stay centered on.

The High Speed Shaft:

Imagine you are machining a drive shaft for a high performance engine on your VMC. You have a large diameter (Datum A) and a smaller diameter that must be concentric to it within 0.02 mm. If your lathe chuck has a tiny bit of wobble or if your milling tool pressure causes the part to deflect, one side of the shaft wall might be 10.05 mm thick while the opposite side is 9.95 mm thick. Even if the average center looks okay, the median points are shifted toward the thicker side. At 5,000 RPM, that extra mass on one side creates centrifugal force leading to vibration that can destroy bearings.

Why is it Difficult?

Concentricity is one of the most challenging controls to measure and machine. A part can be perfectly round but still have poor concentricity if the center of that circle is off compared to the datum. At the atomic level, if the material density is inconsistent or if the part warps during cooling, the mass center and the geometric center may shift making it difficult to maintain the median point alignment. You cannot simply use a dial indicator on the surface that would be measuring Runout. To measure concentricity, you must map the entire surface and mathematically calculate where the center points are.

Applications in Machining:

Concentricity is typically reserved for high speed rotating parts where balance is critical. In High speed Spindles, if the centers aren't aligned, the atoms of the metal will experience uneven centrifugal forces leading to vibration and bearing failure. In Engine Pistons, ensuring the outer diameter and the inner wrist pin bore share the same center.

Concentricity vs. Runout:

In your daily work, you might find Runout more common. Here is the difference:

Runout: Measured with a dial indicator on the surface. it catches everything. If the part is out of round, it fails. If the part is off center, it fails.

Concentricity: Only cares about the center of mass. A part could technically be egg shaped but still have perfect concentricity if the fat parts of the egg are perfectly balanced on opposite sides.

Concentricity is notoriously difficult to measure. You cannot check it with a standard dial indicator or a manual micrometer. It requires a CMM to map thousands of points and mathematically find the midpoints. Unlike Position, concentricity does not allow for "Maximum Material Condition" (MMC). You don't get extra tolerance if your hole is slightly larger. Because it relies on the symmetry of the material, internal stresses in the metal (released during machining) can cause the median points to shift as the atoms rearrange even if your toolpath was perfect.

How concentricity is different from position with example?

While Concentricity and Position both aim to keep a circular feature on center, they look at the part through two very different lenses. In modern CNC machining, Position is much more common because it is easier to measure and more functional for assembly. Imagine you are machining a large, thick walled pipe on your VMC.

Position:

You need to ensure a bolt can pass through this pipe into a baseplate. You care about the Axis. Even if the pipe is slightly egg shaped (out of round) as long as the theoretical center line (the axis) is within the tolerance zone, the bolt will fit. Position allows the surface to be a bit wavy as long as the hole is in the right spot for the bolt.

Concentricity:

Now imagine that same pipe is a high speed driveshaft spinning at 5,000 RPM. You care about Concentricity. If one side of the pipe wall is thicker than the other even if the axis is perfect, the median points of the material will be offset. At the atomic level, the extra mass on the thick side creates an unbalanced centrifugal force. This causes vibration and eventually destroys the bearings. Concentricity forces every slice of that pipe to have its center of mass exactly on the datum axis.

Use Position if you want to make sure a pin fits into a hole. Use Concentricity if you are making a high speed rotating shaft where vibration/balance is the no. 1 priority.

Why Position is Usually Preferred?

In your PowerMill workflow or Fanuc programming, you will almost always see Position used instead of Concentricity for three reasons. You can build a Go gauge (a physical pin) to check Position. You cannot build a physical gauge to check Concentricity, it must be measured with a CMM. With Position, if your hole is slightly larger than the minimum size, you gain extra tolerance (Bonus). Concentricity is Regardless of Feature Size (RFS), meaning you get zero extra room even if the hole is huge. A CMM can find the axis of a cylinder in a few seconds by probing 4–8 points. To measure Concentricity accurately, the CMM must probe hundreds of points to find the median of every opposing pair.

Symmetry:

In GD&T, Symmetry is a location control that ensures the median points of all opposing elements of two surfaces are congruent with a datum axis or center plane. While it looks like Position for a slot or a tab, symmetry is much more restrictive because it focuses specifically on the balance of the part relative to its center.

Tolerance Zone:

The tolerance zone for symmetry is a 3D area defined by two parallel planes centered perfectly around a datum center plane. To pass inspection, you don't just measure the outer walls, you must find the midpoint between every pair of opposing points on the surfaces. All of these derived median points must lie within the tolerance zone (e.g. 0.05 mm).

Feature Control Frame:

Symmetry is identified by a symbol consisting of three horizontal lines:

Symbol: ⌯

Tolerance: The total width of the sandwich zone (e.g. 0.1).

Datum: The reference center plane (e.g. A) that the feature must be balanced around.

Think of symmetry as the Concentricity of flat parts. At the Atomic Level, if you are machining a keyway into a shaft, symmetry ensures the atoms are distributed evenly on both sides of the center.

If a part is spinning or moving at high speeds, even if the width of a slot is correct, if it is shifted to one side (asymmetric), it creates an unbalanced load. This uneven distribution of mass leads to vibration and mechanical wear.

Symmetry vs. Position:

In most modern CNC shops using Fanuc or PowerMill, Position has replaced Symmetry because Symmetry is notoriously difficult to measure.

Machining Challenges:

When you are programming a symmetrical feature like a pocket centered on a block. If your end mill deflects more on one side than the other, the median points will shift, even if the total width of the pocket measures correctly with a vernier. If your VMC has any play in the lead screws, the center of the pocket might drift relative to the datum, throwing the symmetry out of tolerance. As the machine warms up, the distance between the spindle center and the table zero can shift slightly affecting the symmetry of features cut at different times during the cycle.

Circular Runout:

Circular Runout is about the relationship of that shape to a spinning axis. Think of it this way, a perfectly cylindrical tire is useless if it’s mounted off center on the axle. Runout catches that wobble. Circular Runout requires a Datum usually the center axis. It cares if the surface hops up and down as you rotate it around that axis. Circular Runout is a 2D check. It is measured at one specific cross section at a time.

It controls a combination of:

Circular Roundness: Is the cross section a circle?

Concentricity/Off center: Is the circle centered on the datum axis?

Circular Runout does not control taper or the straightness of the whole part. If you check the runout at the front of a shaft and it's 0.02 then check the back and it's 0.02, the part could still be tapered, the back circle is larger than the front and it would still pass Circular Runout.

How to Inspect?

This is the most common test on a machine shop floor. Mount the part on the Datum between centers or in a precision chuck. Place a dial indicator against the surface. Rotate the part 360°. The FIM (Full Indicator Movement) or TIR (Total Indicator Reading) is your runout.

Why Choose Runout Over Cylindricity?

As a programmer or machinist, you'll see Runout much more often because it’s functional. Most cylindrical parts rotate (gears, pulleys, shafts). Runout tells you if the part will vibrate when it spins. You don't need a $100,000 CMM scan. You just need a set of centers and a $50 dial indicator. Runout is the best way to check if your part is clocked or indicated in correctly in your CNC 4th axis or lathe chuck. If you care about the shape of the cylinder, use Cylindricity. If you care about the wobble of the cylinder while it spins, use Runout.

How Circular Runout is different than Circularity?

Circularity is about the shape (form) while Circular Runout is about the stability of that shape as it rotates around a specific axis. Think of a bicycle wheel. If the rim is dented, it has poor Circularity. If the rim is perfectly round but the hub is welded on off-center, it has poor Runout, it will hop up and down as you ride.

Requirement of a Datum:

This is the biggest technical divider. Circularity (○) has no datum. You can take a part, put it on a precision turntable, and measure its roundness. It doesn't matter where the part's center is; the software just looks for a perfect circle. Circular Runout (↗) must have a datum usually an axis. It measures the wobble of a surface relative to that datum.

Circular Runout is a composite tolerance. When you check a cross section for runout, the result is a combination of two things:

Circular Error: Is the part actually round?

Off-Center Error (Concentricity/Coaxiality): Is the center of that circle exactly on the datum axis?

If your runout tolerance is 0.05, and your part is off center by 0.04, you only have 0.01 left for roundness error. If the part is perfectly centered, you can use the full 0.05 for roundness.

Both Circularity and Circular Runout are 2D tolerances. When you measure Circularity, you check one circular slice. When you measure Circular Runout, you check one circular slice while the part rotates. If you want to check the entire length of a cylinder (including its straightness and taper) relative to an axis, you move up to Total Runout.

Why the Machinist Cares?

As a programmer or operator, you use these differently. Use Circularity when you are boring a hole for a press fit bearing. The hole needs to be round so the bearing doesn't get squashed, but the exact location of the hole might be controlled by a different Position tolerance. Use Circular Runout for a pulley or a gear. If the teeth are perfectly round but the hole is 0.1mm off center, the gear will vibrate and make noise. Runout ensures the wobble is kept in check.

Total Runout:

Total Runout (⌰) is a 3D geometric control that regulates the entire surface of a revolving feature relative to a datum axis. While Circular Runout only checks individual 2D slices one at a time, Total Runout controls the entire 3D surface simultaneously as the part rotates 360⁰. Total Runout is how much one entire feature or surface varies with respect to a datum when the part is rotated 360° around the datum axis. Total runout controls both the amount of variation in the surface as the part is rotated, and the amount of variation in the axial dimension. Both radial variation and axial variation are measured and held within the tolerance. Total Runout is usually called on a part that is rotated about an axis where the entire surface is critical to be in spec.

Tolerance Zone:

The tolerance zone for Total Runout consists of two coaxial cylinders or two parallel planes, if applied to a flat face centered on the Datum Axis. For Cylinders, two concentric cylindrical boundaries spaced a distance equal to the tolerance value apart (e.g. 0.05 mm). Every single point across the entire surface must remain between these two boundaries while the part is rotated 360⁰ and the measuring probe is swept across the full length of the feature.

What Total Runout Controls?

Total Runout is one of the most restrictive controls in GD&T because it simultaneously limits multiple geometric errors relative to a datum axis:

Circularity (Roundness): Ensures cross-sections are circular.

Cylindricity / Straightness: Prevents bowing, waist-shapes, or tapering along the length.

Coaxiality / Concentricity: Ensures the feature's center axis aligns with the datum axis.

Angularity / Parallelism: Prevents the surface from tilting relative to the datum.

Inspection:

To measure Total Runout on the shop floor, secure the part on its datum axis (e.g. between precision centers, on a mandrel or in a precision V block setup). Place a dial indicator or CMM probe at one end of the feature. Rotate the part 360⁰ while traversing the indicator along the entire axial length of the feature. The Full Indicator Movement (FIM) or Total Indicator Reading (TIR) across the entire travel must not exceed the specified tolerance value.

Total Runout is reserved for high speed or high precision rotating assemblies where any surface variation causes severe vibration, wear or fluid leakage. In Machine Tool Spindles, it ensures tools run true without chatter at high RPM. In Turbine Shafts & Rotors, it prevents massive centrifugal imbalance forces at elevated speeds. In Precision Motor Shafts, it ensures uniform air gaps between rotor and stator surfaces.

How Total Runout is different than cylindricity?

Total Runout (⌰) is the most restrictive all in one cylindrical control in GD&T. It is effectively Cylindricity with a Datum requirement. While Cylindricity only cares if the part is a perfect tube, Total Runout cares if that tube is wobbling, tapered or bowed as it spins around a specific axis.

3D Tolerance Zone:

The tolerance zone for Total Runout consists of two concentric cylinders centered exactly on the Datum Axis.

Cylindricity: The two cylinders can float and tilt to find the part.

Total Runout: The two cylinders are locked in space around the Datum. The part must fit inside that locked sleeve as it rotates.

Total Runout is the Final Boss of tolerances because it controls everything at once:

Circular Roundness: Is the slice a circle?

Cylindricity: Is the whole surface straight and non-tapered?

Coaxiality / Concentricity: Is the center of the part lined up with the Datum?

Parallelism / Angularity: Is the cylinder tilting relative to the axis?

Circular Runout vs. Total Runout:

This is the most important distinction for a machinist:

Circular Runout (↗): You check one slice at a time. You can reset your indicator at different positions along the shaft. It ignores taper.

Total Runout (⌰): You must sweep the indicator across the entire length of the part in one continuous motion or multiple connected motions while the part rotates. If the part is tapered, the indicator will move and the part will fail.

Inspection:

To check Total Runout, you typically use a dial indicator and a lathe or set of centers. Mount the part on its Datum (e.g., between centers). Place the dial indicator at one end of the surface. Rotate the part and slowly move the indicator along the entire length of the cylinder. The Total Indicator Reading (TIR), the difference between the highest and lowest points found anywhere on the entire surface must be within the tolerance.

Why Choose Total Runout?

Because it is so strict, you only use it for high performance rotating equipment. In Transmission Shafts, any taper or wobble at high RPM will cause the gears to whine or fail. In Machine Tool Spindles, the shaft holding your CNC tool must have near zero Total Runout to ensure the tools don't vibrate or chatter during a cut. In Turbine Rotors, at 10,000+ RPM, even a tiny amount of Total Runout creates massive centrifugal forces that can destroy the machine.