CAD Basics

What CAD is, and what it is not

A CAD model is a mathematical description of geometry, not a picture of it. Mechanical CAD commonly stores a part as a boundary representation: exact analytic and spline surfaces trimmed and stitched into a closed volume, which is the geometry that gets mapped into exchange files and handed to manufacturing and metrology software. Because the shape is described rather than drawn, the software can compute things from it - volume, surface area, center of mass, moments of inertia, section views, clearances - instead of asking you to measure a drawing.

What CAD does not do is decide whether the part is any good. It enforces the constraints you gave it and no others, and it will build an elegant, watertight, fully dimensioned model of something that cannot be machined, cannot be assembled, or will not carry its load. The value of the model is entirely a function of the judgment poured into it, which is why NIST's economic work on model-based engineering frames design data in terms of accuracy, completeness and how well it transfers, rather than in terms of whether a shape exists. CAD is where engineering judgment gets recorded and passed on. It is not where judgment happens.

Parametric feature-based modeling

The dominant paradigm in mechanical CAD is parametric, history-based, feature-based modeling. It works in three layers.

First, the sketch. You draw a two-dimensional profile on a plane and then constrain it. Commercial systems split sketch constraints into two kinds: geometrical constraints, which state relationships without numbers (coincident, parallel, perpendicular, tangent, concentric, symmetric), and dimensional constraints, which state lengths, angles and positions. A sketch that carries exactly enough of both to leave nothing free to move is called iso-constrained, or fully constrained; systems typically signal that difference visually, so you can see at a glance which geometry is still loose.

Second, features. A sketch becomes solid through a feature: extrude, revolve, sweep or loft. Further features modify what exists - fillet, chamfer, shell, hole, draft - or repeat it, through linear, circular and mirrored patterns. Each feature is an operation with its own parameters, and each can reference geometry created by earlier features.

Third, the tree. The system records every feature in the order it was created. That ordered history is the model: edit a dimension near the top and the software replays everything below it. This is the source of parametric CAD's power and of its characteristic failure mode. Because later features depend on earlier ones, an edit can leave a downstream feature pointing at a face or edge that no longer exists in the same form, and the rebuild fails or, worse, succeeds with the wrong shape.

Design intent, and why models break

Design intent is the point of the whole exercise. ISO 10303-108, as quoted in the research literature, defines it in terms of the designer's intentions about how a model may later be instantiated or modified, and the working test is simple: change a parameter and see whether the model changes the way you meant it to.

The common failures are well documented. Geometry can overlap itself once a dimension grows. Lines can flip when constraints that were consistent at one size become inconsistent at another. An iso-constrained sketch can become over-constrained under variation, and an over-constrained sketch has no unique configuration. Most dangerous is the case where the model rebuilds cleanly and is simply wrong - the shape regenerates, no error appears, and the design intent has quietly been lost.

How you attach dimensions decides which of those happens. Dimension a bolt pattern from a shared datum edge and the holes keep their relationship to that edge when the plate changes size. Chain the same dimensions hole to hole and the pattern marches off toward one end. Neither scheme is wrong in the abstract; the question is which one states what you actually meant. This is a teachable skill, not a talent: in a 2023 study, fewer than thirty minutes of training on three sketch-robustness principles produced a statistically significant improvement for all fourteen participants - nine graduate students and five industrial CAD specialists - across dimensional variation of up to plus or minus eighty percent.

Direct modeling, and choosing between paradigms

The contrasting paradigm is direct, or explicit, modeling: you push, pull and offset faces on the geometry itself. There is no history and there are no parameters, so nothing replays and nothing rebuilds. That removes the regeneration failure mode entirely, and it removes the ability to drive the model from numbers.

Each fits different work. Parametric modeling earns its overhead when the shape will be revised many times, when a family of sizes comes from one model, when dimensions feed an optimization or a sensitivity study, or when a revision has to be auditable. Direct modeling earns its place when there is no history to work with - imported neutral geometry arrives as solids with no sketches or features - and when you need one quick change, a concept explored in minutes, or a model simplified for analysis. A history-free model keeps no change log of features, which is exactly why it cannot support parametric sensitivity studies. Most mainstream systems now offer both modes, and the practical skill is knowing which one the situation calls for rather than defending one on principle.

Assemblies, drawings, and model-based definition

An assembly is a set of part instances positioned by mates, also called assembly constraints. A rigid body free in space has six degrees of freedom - translation and rotation about three orthogonal axes - and each mate removes some of them. A part fully located has none left; a part deliberately left with one rotational degree of freedom can be dragged through its motion so you can watch a mechanism sweep. Assemblies also let the software find volumes that two parts occupy at once. Interference checking is not an academic exercise: in vehicle concept design, engineers analyze space claims and run interference checks in the process called packaging, to confirm that occupants and components actually fit inside the exterior before anything is built.

Drawings, where they are still produced, are generated from the model rather than drawn alongside it, and that relationship is called associativity. MIL-STD-31000B makes it a contractual requirement: derived engineering design data, whether a 2D drawing, a lightweight viewable or a neutral file, must be based on and derived from the master native 3D model, and there must be no conflict between the master and anything derived from it.

The longer trend is model-based definition, which moves the authority out of the drawing and into the model. MIL-STD-31000B defines MBD as using 3D datasets containing the exact solid representation, the associated 3D geometry, and 3D annotations of dimensions, tolerances, materials, finishes and other notes, to specify a complete product definition; it cross-references ASME Y14.41, Digital Product Definition Data Practices, which is the standard that governs how that annotation is presented. The annotation itself is product and manufacturing information, or PMI. NIST distinguishes semantic PMI, which downstream software can consume directly, from graphical PMI, which preserves the appearance of an annotation for a human reader. How to dimension and tolerance a feature - projection, line conventions, and GD&T symbology - belongs to the technical-drawing topic; what matters here is that MBD changes where that information lives, not what it means. Adoption is still partial: a vendor survey summarized by NIST in 2019 found an estimated 26.8 percent of respondents releasing 51 percent or more of their designs with PMI-embedded 3D models.

Files, interoperability, and what happens downstream

MIL-STD-31000B sorts CAD data three ways. Native data is what the authoring system wrote, generally readable and editable only by that system, and generally the only format fit to serve as master technical data. Neutral data is derived from the native file into a widely available published standard such as STEP, and generally cannot be the master. Viewable data, such as 3D PDF, is for looking at.

STEP is ISO 10303. Its application protocol AP242, ISO 10303-242, is titled 'Managed model-based 3D engineering'; it was first published in December 2014, extends earlier STEP protocols for PMI, kinematics and tessellation, and in its first edition has been deployed by all major CAD vendors, with edition 3 the current published edition and edition 4 still in preparation. NIST was the original secretariat for STEP in the 1990s and still builds the test cases and file-checking tools the vendor community uses. IGES is the older neutral format, designed mainly to communicate design geometry; the 1999 NIST-commissioned study already reported that its custodian intended IGES 6.0 to be its last upgrade and was shifting development effort to STEP, and it is STEP that NIST and the vendor community have built on since. STL is different in kind: it supports only a surface mesh, so exporting to it replaces exact surfaces with flat triangles and carries none of the tolerancing, material or process information a model-based definition holds. That is why the additive manufacturing file format standardized as ISO/ASTM 52915 adds curved triangle patches, color, texture, material specification and substructures on top of what STL can express.

Interoperability remains a real cost rather than a solved problem. A neutral format is cheaper than the alternative - point-to-point translation needs n(n-1) translators for n systems, so eight systems means fifty-six, while a neutral hub needs only two per system, sixteen - but every transformation is still an opportunity for loss. NIST-sponsored work on CAD-to-CAM and CAD-to-inspection exchange requires that data be validated after each transformation to confirm nothing was corrupted, and notes that once the definition is no longer a visually inspectable drawing, automated algorithms are needed to check it. Managing which version is authoritative is the job of product data management and, more broadly, product lifecycle management: systems that check models in and out, hold revision history, tie models to part numbers and change orders, and control who may release what. Ordinary text-oriented source control fits badly, because native CAD data can generally be read and interpreted only by the system that authored it, so the files do not diff and merge the way source code does.

Downstream, the model feeds computer-aided manufacturing, finite-element and computational fluid dynamics preprocessing, rendering, and additive manufacturing. Two honest caveats apply. First, a model that looks right can still be unmanufacturable, because the geometry carries no knowledge of tool access, fixturing, draft, or what a process can actually hold; NIST's review of model-based engineering records the Boeing 787 case in which parts did not fit together and caused extensive rework, traced back to a failure to communicate requirements and data to suppliers. Second, simulation results depend on assumptions the CAD model does not carry. NASA-STD-7009B defines a modeling assumption as information asserted to simplify or focus the model or to presume parameter values, defines model uncertainty as variation arising from assumptions, formulas and representations rather than from the real system, and requires that a model's abstractions, assumptions, inclusions, exclusions and limits be stated and its credibility assessed for critical decisions. The geometry is an input to that argument, never the argument itself.

One boundary before you go. This is educational material about how CAD systems represent and exchange design information. It is not engineering design guidance, and nothing here should be applied to a real structure, pressure vessel, electrical installation, vehicle or machine; real design work requires a licensed or otherwise qualified engineer working to the governing code.