GD&T basics for custom parts: symbols, datums and control frames

Why a size tolerance is not enough

A diameter tolerance controls the local size of a cylindrical feature. It does not stop the feature from being bent, oval, tilted or in the wrong place. A shaft can measure inside its diameter limits at every cross-section and still fail to enter a bearing because its axis is curved.

GD&T is the language that closes that gap. It describes the zone a surface, axis or centre plane must stay inside. The zone is tied to a datum reference frame, so the supplier and the inspector are measuring from the same origin.

The language is defined in ISO 1101 and, in North America, ASME Y14.5. The two systems share most symbols but differ in defaults and in some rules. A drawing should name the system it uses, especially where the envelope requirement or a material modifier is involved.

The five families of control

Every geometrical control belongs to one of five families. The family tells you what the control can and cannot fix. That is more useful than memorising a list of symbols.

Reading a feature control frame

A feature control frame is read from left to right. The first cell holds the control symbol. The second holds the tolerance value, often with a diameter symbol if the zone is cylindrical. The next cell can hold a material condition modifier such as M or L. The remaining cells list the datum references in order.

The frame is attached to a feature by a leader or placed under a dimension. The tolerance applies to the feature the frame points to, not to the whole part. A frame under a hole dimension controls the hole. A frame on a surface controls that surface.

The order of the datum cells is not decorative. It sets the sequence in which the datum features are contacted and the order in which degrees of freedom are removed. Reversing two datums can change the measured result on the same part.

Datums in one page

A datum feature is a real surface or feature on the part. A datum is the theoretically exact plane, axis or point derived from that feature by a simulator, such as a surface plate, a mandrel or a CMM alignment. The datum reference frame is the set of three mutually perpendicular planes built from the primary, secondary and tertiary datums.

The primary datum removes three degrees of freedom, usually one translation and two rotations. The secondary removes two more, and the tertiary removes the last one. That is the 3-2-1 principle in its simplest form. For a cylindrical primary datum, the axis removes four degrees of freedom and the sequence changes.

Choose datum features that match the assembly. A part that sits on a mounting face in service should use that face as the primary datum. A part that is located by two pins should use the pin features, not a convenient edge that nobody touches.

Basic dimensions and true position

A basic dimension is a theoretically exact value shown in a rectangular frame. It has no tolerance because the tolerance is carried by the feature control frame. Basic dimensions locate the centre of a hole pattern, the true profile of a curve or the ideal angle of a face.

True position is the theoretically exact location defined by those basic dimensions. The position tolerance creates a zone around that location, and the feature axis must lie inside it. If the drawing gives a plus or minus location instead of a basic dimension, the control is not true position in the standard sense.

This is why a position callout and a coordinate tolerance are not interchangeable. A plus or minus 0.1 mm on X and Y creates a square zone. A position tolerance of 0.2 mm creates a round zone with a different acceptance boundary. The round zone usually matches a clearance hole better.

Material condition modifiers

A material modifier changes the size at which the tolerance applies. M means maximum material condition: the smallest hole or the largest shaft. L means least material condition: the largest hole or the smallest shaft. With no modifier, the control applies regardless of feature size.

The M modifier allows bonus tolerance as the feature departs from maximum material. It is useful for a clearance hole that only needs to accept a fastener. The L modifier is useful when a minimum wall thickness or a minimum clearance is the concern.

Modifiers are not a way to make a bad part acceptable. They are a way to tie the tolerance to the function. A hole that must accept a pin at its worst case can use M. A hole that must maintain a wall to an edge should use L or a separate wall control.

Material modifiers also interact with the state of the part. A thin or flexible part can meet a size limit on the bench and fail it when restrained. If the drawing calls for a restrained condition, state the clamping points and the force. If it does not, the default is the free state.

The mistakes that cause the most disputes

The first is a datum that cannot be contacted. If the datum feature is a small boss or a surface buried inside the part, the inspector cannot build the reference frame the drawing assumes. The second is a control that is tighter than the process can hold and tighter than the function needs. That adds cost without adding value.

The third is double dimensioning. A basic dimension and a plus or minus dimension that describe the same location create two requirements that can conflict. The fourth is a missing basic dimension, which leaves the tolerance zone undefined. The fifth is a profile callout without datums when the surface also needs to be located.

A useful review habit is to read the drawing as an inspector. For every frame, ask which feature is measured, which datum is primary and which instrument can reach the feature. If any answer is unclear, the drawing is not finished.

• Use datums that can be contacted and repeated.
• Give every position or profile zone a complete basic definition.
• Match the control to the function, not to a habit.
• State the standard and the revision on the drawing.
• Check that the inspection method exists before release.

Putting GD&T on a custom part

Start with the assembly. Identify the surfaces that locate the part, the features that carry load and the features that must clear another part. Those are the candidates for datums and controls. Most other dimensions can stay under a general tolerance.

Then choose the smallest set of controls that describes the function. A flat mounting face may need flatness and perpendicularity to a bore. A hole pattern may need position at MMC. A rotating surface may need runout. A cosmetic curve may need profile with a generous zone.

Finally, write the inspection plan at the same time as the drawing. If a control needs a CMM program, a fixture or a gauge, say so before the quote. GD&T only works when the measurement method is part of the agreement.

1. 01

   Map the function

   List the locating, sealing, conducting and moving features.

2. 02

   Set the datums

   Choose features that match the assembly and the fixture, then order them.

3. 03

   Apply the controls

   Use form, orientation, location, profile or runout only where the function needs a zone.

4. 04

   Agree the method

   Confirm the instrument, the fixture and the report format before production.