Flatness, straightness and parallelism: form versus orientation

The one question that separates them

Look at the feature control frame. If there is no datum reference, the control is a form control. Flatness and straightness are in that group. If there is a datum reference, the control is an orientation control, and parallelism is in that group.

Form controls describe the shape of a feature on its own. They do not say where the feature sits or which way it points. Orientation controls describe the angle between a feature and a datum. They still do not say where the feature sits along the datum.

That is why a flatness call cannot replace a parallelism call, and a parallelism call cannot replace a location call. Each one answers a different question. Using the wrong one leaves the function uncontrolled even though the drawing looks precise.

Flatness

Flatness applies to a surface. The tolerance zone is two parallel planes, and every point on the surface must lie between them. The zone has no datum and no fixed orientation. It can sit anywhere in space, as long as its width is the stated tolerance.

Flatness is the right control for a sealing face, a mounting pad, a vacuum table or a wear surface. It is also useful as a refinement on a large face where the general tolerance would allow a bulge that the function cannot accept.

Flatness does not control the thickness of the part, the angle of the face or its height. A face can be perfectly flat and still be machined at the wrong angle. If the angle matters, add parallelism or angularity to a datum.

Straightness

Straightness applies to a line element on a surface or to the derived median line of a feature of size. For a surface, the zone is two parallel lines, and the line element must lie between them. For an axis, the zone can be a cylinder or two parallel planes, depending on the callout.

Surface straightness is useful on a slide way, a rail or an edge that must not bow. Axis straightness is useful on a shaft, a pin or a bore where the centre line must not curve. The two are not interchangeable, even though they share a symbol.

Axis straightness is often specified at maximum material condition so that a functional gauge can check the combined effect of size and bend. When the envelope requirement applies, the size limits already restrict form, so a straightness tolerance that is larger than the size tolerance adds little. Check which rule the drawing invokes before adding the call.

Parallelism

Parallelism applies to a surface or an axis and always has a datum. For a surface, the zone is two parallel planes oriented parallel to the datum. For an axis, the zone is a cylinder or two parallel planes parallel to the datum axis or plane.

Parallelism controls orientation and, within the zone, form. It does not control location. A surface can be perfectly parallel to a datum and still be 20 mm away from where the drawing says it should be. The distance needs its own size or location control.

This is the most common misunderstanding in a drawing review. A designer adds parallelism to a face to fix its height. The supplier holds the parallelism and the face still sits at the wrong height, because parallelism never controlled height.

Refining a broader tolerance

A geometrical control is useful when it refines a broader tolerance that already applies. Flatness can refine the form allowed by a thickness tolerance. Parallelism can refine the orientation allowed by a general tolerance. Straightness can refine the bend allowed by a length tolerance.

The refinement should be tighter than the broader tolerance, otherwise it does not change the acceptance boundary. Where a size tolerance already limits the same variation, such as axis straightness under the envelope requirement, a larger geometrical tolerance may be redundant. The drawing should not carry two controls that fight for the same space.

A stack of controls is not automatically better. Each one adds inspection time. Use the smallest set that describes the function: a general tolerance for the non-critical face, flatness for the seal, parallelism for the mounting angle and a size dimension for the height.

How each one is measured

Flatness is measured against a fitted plane, not against a surface plate that forces the part flat. A surface plate and a dial indicator can work for a small part, but the part must be supported so that its own shape is measured. A CMM or a laser scanner fits a plane to the measured points and reports the separation of the extreme points.

Straightness is measured along a line. A straightedge and feeler gauge can give a quick check on a surface. A dial indicator on a surface plate or a CMM can give a value. Axis straightness needs a method that finds the derived median line, such as a V-block setup, a functional gauge or a scan of the feature.

Parallelism is measured as the variation in distance between the feature and the datum. Take readings at several points along the feature, fit the datum, and report the spread. The result includes both the orientation error and the form error within the zone, which is why a wavy surface can fail parallelism even when its average angle is correct.

• Do not clamp a flexible part flat before measuring flatness.
• Record the fitted plane or datum alignment.
• Take enough points to cover the whole surface.
• Report the maximum and minimum deviation, not only the average.
• State the instrument and the software filter where relevant.

Drawing mistakes to catch

The first mistake is a parallelism call with no datum. The frame is incomplete and the inspector cannot apply it. The second is a flatness call used to control height. The third is a straightness call on a surface when the axis is the feature that matters, or the reverse.

The fourth is a control that is looser than the general tolerance, which adds text without changing the part. The fifth is a control on a flexible part that cannot be measured in the free state. The sixth is a datum that is not accessible, which makes the orientation call unmeasurable.

A good review asks three questions. What variation is the function sensitive to? Which control describes that variation? Can the supplier measure it with the part in its free or assembled state? If the answers do not line up, the control is not ready.

A selection sequence

Start with the function. If the surface must seal or sit flat against another surface, start with flatness. If a line or axis must not bow, start with straightness. If the feature must maintain an angle to a datum, start with parallelism or angularity.

Then check the datum. A form control needs none. An orientation control needs a datum that matches the assembly. If no datum is available or meaningful, the orientation control is probably the wrong choice.

Finally, check the inspection. A control that cannot be measured in the production state is a source of disputes. The drawing, the fixture and the report should describe the same part in the same condition.

1. 01

   Name the variation

   Waviness, bow, tilt or height. Each points to a different control.

2. 02

   Choose the family

   Form for shape alone, orientation for angle to a datum, location for position.

3. 03

   Set the datum

   Use the assembly or fixture feature that actually controls the part.

4. 04

   Check the measurement

   Confirm the part can be measured in its free or assembled state.