Why Standard Parts Libraries Matter
Every mechanical design uses standard hardware: bolts, nuts, washers, bearings, seals. Modeling these from scratch every time is wasteful. Importing geometry from internet catalogs is unreliable — you get whatever the supplier decided to include, in whatever quality they provided, with no guaranteed consistency between components.
A company-standard parts library solves this. You build or validate the geometry once, define the parameters, and deploy it to the team. Every engineer pulls the same component, with the same properties, with the correct part number and material definition. BOMs are correct by construction.
In CATIA V5, the tool for building and deploying standard parts libraries is the Catalog Browser and Catalog Editor, combined with Power Copy and User Features for parametric component families.
The CATIA V5 Catalog Structure
A catalog (.catalog file) is a hierarchical structure of chapters and components. The top level is the catalog file. Within it, chapters organize components by type (e.g., “Fasteners” > “Hex Bolts” > “ISO 4762”). At the leaf level, catalog items are component definitions — either links to CATProduct/CATPart files or parametric family definitions (User Features or Power Copies).
Access the catalog browser in any workbench: Insert > Catalog Browser, or through the infrastructure menu depending on your CATIA configuration. The browser shows the catalog structure and allows drag-and-drop insertion of components into the active document.
Catalog Editor
Build and modify catalogs in the Catalog Editor workbench (found in CATIA V5 under Infrastructure or Product Synthesis depending on configuration). Open Catalog Editor with File > New > Catalog.
Creating chapters
Chapters organize the catalog. Right-click the catalog root and select Add Chapter. Name chapters logically: “ISO_Fasteners,” “DIN_Fasteners,” “Bearings_SKF,” “Seals_Parker.” Sub-chapters nest as needed: “ISO_Fasteners” > “Hex_Cap_Screws” > “ISO4762.”
Adding components to a chapter
Simple approach: add existing CATProduct or CATPart files. Right-click a chapter, select Add Component, and browse to the part file. Each unique component variant (M8x20, M8x25, M8x30) is a separate entry in the catalog.
Parametric approach: use Power Copy or User Features to represent a family of components with configurable parameters. This is more powerful — one definition covers all sizes of a component through parameters, rather than requiring a separate file for each size.
Power Copy: Parametric Component Families
Power Copy is a CATIA V5 feature that packages a group of features — including sketches, geometry, and constraints — as a reusable template. When you instantiate a Power Copy, CATIA prompts you to define inputs (reference geometry or parameters) and creates an instance tailored to those inputs.
Use case: an M-series hex socket head cap screw (ISO 4762) whose head diameter, head height, thread diameter, and overall length are all functions of the nominal diameter M.
Creating a Power Copy:
- Model a parametric CATPart of the bolt with equations: “Head_Dia” = “M_nom” * 1.5, “Head_H” = “M_nom”, etc. Use global variables for all key dimensions.
- In Insert > Knowledge Templates > Power Copy, define the inputs (the parameters that the user specifies when instantiating) and the outputs (the geometry produced).
- Save the CATPart. Add it to the catalog chapter as a Power Copy entry.
When an engineer inserts this catalog item, CATIA prompts: “Enter M_nom value.” They enter 8 (for M8), confirm length, and the bolt is instantiated at the correct geometry for M8.
User Features
User Features (UDFs) are similar to Power Copy but defined at the feature level rather than the body level. A User Feature represents a parametric set of features that can be applied to an existing solid — for example, a countersunk hole pattern that takes an existing face as input and adds the hole geometry to it.
Key difference from Power Copy: UDFs modify existing geometry. Power Copies create standalone geometry. For fastener bodies (the bolt itself), Power Copy is appropriate. For features applied to a part (a threaded hole, a counterbore, a bearing pocket), User Features are more appropriate.
Define a User Feature in Insert > Knowledge Templates > User Defined Feature. Specify the feature inputs (the faces and edges that the UDF uses as reference), the parameters the user sets at instantiation, and the features it creates.
Linking to Excel Spreadsheets
CATIA V5 can drive design parameters from Excel through the Design Table feature (Tools > Design Table in Part Design). A spreadsheet column corresponds to a parameter name matching a global variable in the CATPart. Each row represents a standard size variant.
Workflow: define an M-series bolt part with global variables for all key dimensions. Create an Excel spreadsheet with rows for M4, M5, M6, M8, M10, M12, M16, M20 and columns for each variable. Activate the design table. Now the catalog item for each bolt size is a configuration of the single parametric part, driven by the spreadsheet row.
This approach is maintainable: adding a new size means adding a row to the spreadsheet, not creating a new part file. Updating a dimension standard means editing one spreadsheet, not editing dozens of part files.
Deploying the Library Across a Design Team
- Store catalog files on a shared network location accessible to all design engineers. Path example: \server\CATIA_Standards\Catalogs\
- Set the catalog path in CATIA options: Tools > Options > Infrastructure > Product Structure > External Components > Catalogs Path. Set this to the shared network location so all users access the same catalog files.
- Control write access: only the library administrator should have write access to the catalog files. Design engineers have read-only access. This prevents accidental modification by individual users.
- Version the catalog files: store catalog files in the PDM vault or a version-controlled folder. Track changes with change records — when a catalog component is updated (e.g., a dimensional correction), all engineers need to know which assemblies using that component need to be reviewed.
Comparison to SolidWorks Toolbox
| Aspect | CATIA V5 Catalog + Power Copy | SolidWorks Toolbox |
|---|---|---|
| Setup complexity | High — requires Power Copy/UDF knowledge | Medium — configuration tool provided |
| Parametric component families | Excellent (Power Copy + Design Table) | Good (configurations) |
| Custom components | Flexible — any geometry | Supported — add to database |
| Standard library coverage | Depends on what you build/import | Extensive ISO/ANSI/DIN built-in |
| Team deployment | Network folder + CATIA options path | Network folder + SolidWorks options path |
| PDM integration | Manual / ENOVIA | SolidWorks PDM native support |
Key Takeaways
- CATIA V5 catalogs built on Power Copy and Design Tables are the most robust approach to standard parts libraries. One parametric definition covers entire size families without duplicating files.
- Store catalogs on a shared network path with read-only access for design engineers. The catalog is a shared resource that should be maintained centrally.
- User Features are the right choice for features applied to existing geometry (holes, pockets, boss features). Power Copy is for standalone geometry (fastener bodies).
- Link to Excel spreadsheets for size families. Maintaining one spreadsheet is far easier than maintaining dozens of part files.
- Version-control the catalog files. When a catalog component changes, assemblies using that component need to be reviewed for impact.
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