How to Verify CAD Geometry Against an Engineering Drawing

What verification means: requirement by requirement

A model looks right when it is overlaid on the drawing. It is verified when every requirement on the drawing has been checked against the model and the result written down. The unit of work is the requirement, not the part.

A requirement is anything the drawing states that the geometry must satisfy: a size, a location, a count, a feature type, an orientation, or a note such as “all fillets R1”. Each one becomes a row with its source on the drawing, the expected value, the measured value, the method and the result.

Write the expected values down before measuring. It is easy to see what you expect in a model. A requirement that cannot be checked on the model, such as surface finish or an edge-break note, still gets a row with the reason, so the list shows what was not covered as clearly as what passed.

Model verification and part inspection are different jobs. Verifying a model compares one nominal shape with the drawing. Inspecting a part compares a physical, imperfect part with the drawing's tolerances. This guide covers the first.

Measuring the model

Every CAD system and most STEP viewers have measurement tools. These are the useful ones for verification, with what each one can and cannot catch.

Bounding box

The bounding box gives the overall envelope: length, width and height. It catches a wrong overall size, a wrong unit (a 100 mm plate modeled as 100 inches is 2,540 mm long) and a part built in the wrong orientation. It says nothing about interior features. Two cautions apply. An axis-aligned box depends on how the model sits in its coordinate system, so align the model to the drawing's datums first. Some systems also return a fast box that can be slightly larger than the solid, so use the precise or minimal option where one exists.

Volume and mass

Volume is a cheap global check and a coarse one. Work out the expected value from the drawing's nominal dimensions and compare. For a 100 × 60 × 10 mm plate with four Ø6.6 through holes, the block is 60,000 mm³ and each hole removes π × 3.3² × 10 ≈ 342 mm³, so the expected volume is about 58,630 mm³. A missing hole shows up as a difference of about 0.6 %.

A hole in the wrong place changes nothing, and neither does a hole pattern mirrored to the wrong side. Mass is volume times density, so it can also check the material assignment, but the density in the model is whatever someone entered.

Hole position and diameter

Measure a hole's diameter from its cylindrical face, not from edges and not from a mesh. On an exact B-rep solid the cylinder carries a radius, and the measurement returns the modeled value. On an STL or other tessellated mesh the hole is a polygon, and a measurement across it reads a little differently depending on which vertices or facets you pick.

Measure position as the coordinates of the hole axis in the frame the drawing uses. If the drawing locates holes with basic dimensions from datums B and C, measure the axis from datum features B and C, at the face that is datum A, not from the model origin. Check the axis direction too: a through hole drawn perpendicular to A should be perpendicular in the model. Then check that it goes through.

Threaded holes need one more decision. CAD models often show a tapped hole as a plain cylinder at the nominal diameter, the tap-drill diameter or the thread's minor diameter, with the thread itself as a cosmetic attribute. Find out which convention the model uses before you compare a diameter.

Feature counts

Counting catches what volume hides: a pattern of six that has five holes, a pattern with an extra instance, or a chamfer applied to three corners of four. Count by feature type and size against each callout. “6X Ø5.5 THRU” means six through holes of that size, and an extra Ø5.5 hole elsewhere is an error even if the six are right. Feature trees can mislead here, because a suppressed or failed feature may still be listed, so count on the solid's faces.

Datums: measuring in the drawing's frame

A drawing's datums say where measurement starts. In ASME Y14.5 and ISO 5459 terms, datum features are real surfaces or features of the part, and the datum reference frame is the set of planes and axes they establish, in order of precedence. For three planar datums, the primary constrains the most freedom, the secondary the next, and the tertiary what is left. On a nominal model the datum features are perfect, so establishing the frame is simple, but it still has to be done.

1. Find the datum features on the drawing (A, B, C) and the matching faces or axes in the model.
2. Build or select a coordinate system on them, with origin and axes as the datum reference frame defines them.
3. Measure locations from that frame, against the basic dimensions that the feature control frames refer to.
4. If the model was built with its origin elsewhere, such as the part center, convert the coordinates instead of reading the model's values directly.

Models are often built symmetric about the origin, while drawings locate features from an edge. A hole at x = 35 from the center of a 100 mm plate is 15 mm from one end and 85 mm from the other. Mixing the two frames is a common source of mirrored or shifted features that pass a casual look.

Tolerances: recorded versus checked

A drawing dimension carries a nominal value and a tolerance. A CAD model normally carries one value for each feature, usually the nominal. Two different statements follow from that, and they should not be confused.

• Recorded: the tolerance is captured with the requirement, so it is available for manufacture, inspection planning and tolerance analysis. A Ø12 bore with ±0.05 has that band written down next to it.
• Checked: something has been measured against the band. On a nominal model the measured bore is 12.000 and the check passes trivially. That shows the model was built at 12, not that any part will fall between 11.95 and 12.05.

A model check can still add something on tolerances. It can show that the modeled value sits inside the band, which fails if the model was built at a rounded or wrong value, or if the band lies entirely to one side of nominal (a g6 shaft modeled at nominal is outside its own zone). It can show that each tolerance is recorded against the right feature. Whether a chain of tolerances closes is an analysis of the design, done with a tolerance stack-up, and whether parts conform is decided by inspecting parts. The guide to drawing tolerances and CAD goes further.

A verification checklist

Why a passing export is not manufacturing approval

Four statements are easy to blur together:

1. The file is valid: the STEP opens, holds a closed solid and uses the right units.
2. The model matches the drawing: every nominal requirement was checked and passed.
3. The part can be made as specified: the tolerances, material, finish and features suit a process, and a supplier has accepted them.
4. The design is released: the drawing and the model are at an approved revision, under change control, with the sign-offs your organization requires.

A clean verification report establishes the second statement at most. Manufacturing approval adds a design-for-manufacture review, a decision about which document governs (the drawing or the model), and in many industries a first article inspection of real parts against the drawing. In aerospace, first article inspection is commonly documented to SAE AS9102. A model can pass every geometric check and still carry a wrong revision, a wrong material or a tolerance the shop cannot hold.