CATPART File Documentation

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Technical details

Feature	Value
Full name	CATIA V5 Part File
File extension	.CATPart
MIME type	application/octet-stream
Format type	Proprietary binary; parametric B-rep single-part 3D model
Developer	Dassault Systèmes
Introduced	CATIA V5, 1998 (V6 / 3DEXPERIENCE continue the format)
Geometry model	Boundary representation (B-rep): exact surfaces, edges, faces, solids
Design data	Parametric feature tree (specification tree): sketches, pads, pockets, fillets, holes, constraints
Metadata	Material, part number, units, author, model parameters, PMI
Geometry kernel	CGM (Convergence Geometric Modeler), Dassault Systèmes
Standard / specification	Proprietary; no public specification
Open standard	No
Backward compatibility	Limited — a newer CATIA release cannot generally be opened in an older one
Contains executable code	No — passive geometry and metadata
Assembly counterpart	.CATProduct (references multiple parts)
2D drawing counterpart	.CATDrawing
Lightweight view counterpart	.cgr (tessellated visualisation)
Related extensions	.CATProduct, .CATDrawing, .cgr, .3dxml, .stp, .igs
Neutral export formats	STEP (.stp/.step, ISO 10303 AP203/AP214/AP242), IGES (.igs), JT, 3DXML, STL
Vendor page	3ds.com/products/catia

What is a CATPart file?

A .CATPart is the part document of CATIA V5, the high-end 3D CAD/CAM/CAE system that Dassault Systèmes released in 1998. It holds one mechanical component: the exact 3D geometry of a single part plus the parametric design history that built it. CATIA V5 is the standard modelling tool across aerospace and automotive engineering (Airbus, Boeing and most major automakers are long-standing users), which is why the extension turns up constantly when parts are shared between an OEM and its suppliers.

The file is a proprietary Dassault Systèmes binary. Its geometry comes from the CGM (Convergence Geometric Modeler) kernel, and its internal layout is not published: there is no open specification, no documented chunk tree, and no reliably published magic number you can key on. What follows describes what is genuinely known about a CATPart — the concepts the file records and how it sits in the wider CATIA V5 file family — rather than a fabricated byte map. The honest identifier for a CATPart is its extension and its CATIA origin, not a header signature.

The CATIA V5 file family and where a part sits

CATIA V5 splits a design across several document types, and a CATPart is only one of them. Knowing the family explains most “I was sent the wrong file” problems.

.CATPart      one part            single component: geometry + feature tree
.CATProduct   assembly            references many .CATPart files + positioning
.CATDrawing   2D drawing          associative views/sections generated from 3D
.CATMaterial  material library    material definitions applied to parts
.cgr          CGR viewer file     lightweight tessellated mesh, no editable model

A .CATProduct does not embed its parts. It stores references (links) to external .CATPart files plus the assembly constraints that position them, so an assembly delivered without its component parts opens with the geometry missing. A .CATDrawing is associative: its views are generated from a 3D model and update when the model changes. A .cgr is the opposite of a CATPart — a tessellated mesh meant only for fast display and review, with no B-rep and no feature history. If you only need to look at a shape, a CGR is enough; if you need to edit or measure exact geometry, you need the CATPart.

The feature-based design tree

CATIA V5 is a history-based parametric modeller, and a CATPart records that history as an ordered specification tree (usually just called the feature tree). The part is not stored as a static lump of geometry; it is stored as the sequence of operations that build it, evaluated top to bottom.

A typical build starts with a 2D sketch on a plane: a profile of lines, arcs and splines, pinned down by dimensional and geometric constraints (a length of 40 mm, two edges made parallel, a fillet radius of 3 mm). A feature such as a Pad extrudes that profile into a solid; a Pocket removes material; Hole, Fillet, Chamfer, Shell, Draft and pattern features refine it further. Each feature refers back to earlier geometry, so the tree is a dependency graph as much as a list.

The practical consequence is parametric editability. Change the sketched 40 mm to 55 mm, or edit the pad depth, and CATIA re-evaluates every dependent feature and rebuilds the solid. Named parameters and formulas can drive many dimensions at once, so a single input can resize a whole family of related features. This design intent — the sketches, the constraints, the feature order, the parameter relationships — is exactly what lives in the CATPart and exactly what a neutral export cannot carry, a point that matters later.

B-rep solid and surface geometry

Underneath the feature tree, the actual shape is stored as a boundary representation (B-rep). A B-rep model describes a solid by its boundary: a closed set of trimmed faces, bounded by edges, meeting at vertices, with an explicit record of which face lies on which side of each edge (the topology) laid over the underlying mathematical surfaces and curves (the geometry).

Solid
 └─ Shell (closed set of faces enclosing a volume)
     └─ Face      trimmed patch of an underlying surface (plane, cylinder, NURBS...)
         └─ Loop  ordered ring of edges bounding the face
             └─ Edge     trimmed curve shared by two faces
                 └─ Vertex   point where edges meet

This is “exact” geometry: a cylindrical face is a true analytic cylinder, and a freeform face is a NURBS surface with precise control points, not a triangle approximation. That precision is why CATIA parts are suitable for machining and analysis. It also contrasts sharply with mesh formats such as STL or a .cgr, where the same cylinder becomes a fan of flat triangles that only approximate the curve. CATIA can model both solids and open surfaces (the Generative Shape Design workflow), and a single CATPart can hold solid bodies, surface geometry and construction elements side by side. The CGM kernel owns all of this internally, which is a large part of why the on-disk format stays closed.

Backward compatibility and release levels

CATIA V5 shipped as a long run of releases — V5R7, V5R8 and onward through the V5-6Rxxxx line (for example V5-6R2019, V5-6R2024). The CATPart binary is version-tagged internally by the release that wrote it, and this creates the single most common “won’t open” problem in practice.

CATIA V5 is not backward compatible. A part saved in a newer release generally cannot be opened by an older CATIA installation, and Dassault provides no native downgrade path to save a part back to an earlier release format. So a supplier on V5-6R2019 who receives a part authored in V5-6R2024 simply cannot open it in CATIA, even though both sides own valid licences. The fix is not technical trickery on the file; it is process. Either the sender re-saves in the recipient’s release (if they can), or — far more reliably — the sender exports a neutral format that carries no release lock at all.

Neutral-format exchange via STEP

Because the CATPart binary is proprietary, release-locked and undocumented, real cross-tool interoperability does not happen by reading the CATPart directly. It happens by exporting the model to a neutral CAD exchange format. The primary one is STEP, standardised as ISO 10303. STEP files (.stp / .step) open in effectively every mainstream CAD system, and CATIA exports them through Save As / Export.

STEP is defined in application protocols, and the choice matters:

Protocol	What it carries
AP203	Baseline solid/geometry exchange; no structured colour or PMI
AP214	Automotive-oriented; adds colours and presentation on top of AP203
AP242	Current protocol; merges AP203/AP214 and adds 3D PMI (tolerances, annotations)

For a part that needs geometry only, AP203 or AP214 is fine; when tolerances and annotations must travel with the model, export AP242. Alongside STEP, CATIA can write IGES (.igs, an older surface/solid exchange format), JT (a lightweight visualisation and PLM exchange format common in automotive and aerospace review), 3DXML (Dassault’s own XML-based lightweight format), and STL for 3D printing.

There is one unavoidable trade-off. A neutral export transfers the exact B-rep geometry but drops the editable feature tree. Open a STEP export of a CATPart in another CAD system and you get a precise solid body with no sketches, no parametric features and no design history — a “dumb” solid. You can machine it, measure it and add new features to it, but you cannot go back and change the original 40 mm sketch dimension, because that intent lived only in the CATPart. This is why teams that need to keep editing a part push for the native CATPart (matching release levels), while teams that only need the shape are well served by STEP.

What a CATPart is not: geometry, not code

A CATPart is passive engineering data: geometry, topology, parameters and metadata. It contains no executable code, so opening one in CATIA or a viewer does not run anything. The genuine cautions around CATParts are not about malware. They are the release-compatibility trap described above, the loss of feature history on neutral export, and confidentiality — a production aerospace or automotive part is valuable intellectual property, so files should come from a trusted source and sensitive parts should not be uploaded casually to free online viewers. None of these are safety issues in the code-execution sense; they are engineering-workflow issues specific to how the format stores and shares design intent.

References

• Dassault Systèmes — CATIA (native .CATPart format)
• ISO 10303-242 (STEP AP242) — neutral CAD exchange standard
• Open Cascade — CAD Assistant (free CATPart viewer / STEP-STL converter)

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