Working on CATIA by yourself and managing a large multi-person project are two completely different challenges.
“Opened a part and got a wall of ‘Linked Document not found’ warnings. Opened an assembly and half the components are showing red exclamation marks.”
Nine times out of ten, this traces back to poor file path management and a poorly planned folder structure. This article covers how to design a scalable CATProduct hierarchy, how to repair broken links using the Desk tool, and how to set up file naming and folder conventions that prevent link failures before they happen.
1. CATProduct Structure — How to Organize Your Assembly
In CATIA V5, the assembly file is a .CATProduct and the individual part files are .CATPart. For a simple project, dumping all your parts directly into one CATProduct works fine. But once you’re dealing with hundreds of parts across a team, that flat structure becomes unmanageable fast.
The proven approach in production environments is a hierarchical sub-assembly structure: a top-level CATProduct that contains sub-assembly CATProducts organized by function, each of which holds its own set of parts.
| Level | File Type | Purpose |
|---|---|---|
| Level 0 (Top) | ASSY_TOTAL.CATProduct | Full assembly. Rarely edited — used mainly as a viewer to check the overall fit. |
| Level 1 (Sub-assembly) | base_assy.CATProduct unit_assy.CATProduct |
Mid-level assemblies grouped by functional unit. Each can be assigned to a different engineer. |
| Level 2 (Parts) | BASE_PLATE.CATPart PIN_A.CATPart |
The actual modeling files where design work happens. |
With this setup, Engineer A works exclusively in base_assy.CATProduct while Engineer B works in unit_assy.CATProduct — no conflicts, full parallel workflow. The top-level CATProduct is only opened when it’s time to review how all the sub-assemblies fit together.
In jig and fixture design, splitting by functional unit — Base, UNIT01, UNIT02, etc. — is the standard approach. In aerospace and automotive, customers often dictate the entire tree structure, part numbering scheme, and even color-coding rules through a formal specification document.
Regardless of the method, the one rule that applies everywhere: don’t change the structure mid-project. Reorganizing the hierarchy after work has started will break every reference path in the affected assemblies.
2. Repairing Broken Links — Using the Desk Tool
When CATIA opens a CATProduct, it internally resolves the path to each linked CATPart — either as an absolute or relative path. Move a file to a different folder, copy it to another PC, or change a NAS path, and those references break. The affected components show up as “Missing Link” in the spec tree.
That’s what File > Desk is for. The Desk window gives you a complete view of every document in the current session and its resolved file path — all in one place.
- Go to File > Desk from the menu bar.
- The Desk window opens showing the full document tree for the current session. Files with broken links will have a red icon or question mark.
- Right-click the problematic file and select Find (or Change Location).
- Point it to the correct file location and the link is restored.
- After fixing, save with File > Save All to write the updated path information back into the CATProduct.
You can also repair a broken link by double-clicking the component directly in the spec tree and redirecting it manually. But if multiple links are broken at once, using the Desk window to batch-fix them is far faster.
If you’ve moved an entire project folder to a different drive, correcting the root path just once in Desk will often cascade and fix all the sub-paths automatically.
3. Absolute vs. Relative Paths
CATProduct files can store part references using either absolute or relative paths. Which one you use has a direct impact on link stability across the team.
| Path Type | How It Works | Best For |
|---|---|---|
| Absolute Path | Stores the full path from the drive root, e.g. C:\Projects\JIG_A\Parts\base.CATPart | Solo work, or environments where file locations never change. |
| Relative Path | Stores the path relative to the CATProduct file, e.g. .\Parts\base.CATPart | Team environments and NAS setups. The entire folder can be moved or copied without breaking links. |
In collaborative environments, relative paths are the standard. Team members may have different drive letters or mount points, making absolute paths a liability.
The setting that controls this behavior in V5 is Linked Document Localization, found under Tools > Options > General > Document. Move Relative Folder to the top of the list, and CATIA will always look for linked files by relative position before trying the absolute path. This is what makes it possible to copy an entire project folder to a new drive or PC and have all the links survive intact — as long as the internal folder structure is preserved.
4. File Naming & Folder Conventions — The First Line of Defense
The Desk tool is a great safety net, but the best strategy is to never need it. Here are the naming and structure rules that have proven effective in real production environments.
Standardize the Folder Structure
Define a fixed set of subfolders under the project root and enforce it across the entire team. Everyone must use exactly the same layout.
- 00_ASSY — CATProduct files only. Top-level and all sub-assembly files go here.
- 01_PARTS — CATPart files only. Add sub-folders by unit or by engineer if the part count is high.
- 02_DRAWING — CATDrawing files only.
- 03_REF — External reference data from the client: STEP, IGES, PDFs, etc.
- 04_RELEASE — Finalized deliverable files. Always keep these separate from the active working files.
File Naming Rules
No spaces, no non-ASCII characters, no special symbols in file names. CATIA treats the file name as part of the reference path, and spaces or non-Latin characters can cause link resolution failures in some environments.
- Use uppercase letters, numbers, and underscores only. Example: BASE_PLATE_01.CATPart
- If you have a part numbering system, prefix with the part number. Example: P001_BASE_PLATE.CATPart
- Prefix assemblies with ASSY_; identify parts by part number or functional name.
- Don’t embed version numbers in file names. Instead, version by copying the whole folder as a snapshot. Example: a folder named RELEASE_20260301.
Naming files like BASE_PLATE_v2.CATPart or BASE_PLATE_20260301.CATPart feels intuitive, but it’s a serious problem in any CATIA assembly environment.
CATProduct files reference parts by file name. The moment you rename a part file, every single CATProduct that references it will show a Missing Link. Version control must happen at the folder level — not the file level.
For example: copy the unit01 folder to unit01_v0 as a backup snapshot, then continue working in the original unit01 folder. Since the folder name — and therefore the reference path — doesn’t change, no CATProduct links are affected.
5. Additional Considerations for NAS and Shared Server Environments
When the team is sharing files through a NAS or file server, a few more things need to be locked down.
- Standardize the drive letter: When mounting the NAS share, everyone on the team must use the same drive letter — for example, Z:. If absolute paths are unavoidable in your workflow, this is the most reliable way to keep links from breaking across machines.
- Never use raw UNC paths: Do not work directly from a path like \\192.168.0.x\project. Always map the network share to a drive letter and access it via Z:\project. If the IP address changes or a team member opens files on a machine that can’t reach that address, CATIA will hang while waiting for Windows’ network timeout — which can stretch out to several minutes before it gives up. A mapped drive letter, by contrast, fails fast: the OS returns an error immediately if the drive isn’t connected. This is a well-documented, real-world issue in CATIA environments.
- Prevent simultaneous editing: CATIA has no built-in file locking. If two people open the same file and both save, the last save wins and overwrites the first. Establish a team protocol for file ownership — whether that’s a PDM system like ENOVIA, a shared spreadsheet, or even a team chat agreement, something needs to be in place.
- Share the CGR cache: For large assemblies, pointing the CGR cache folder to a shared NAS location means every team member benefits from cached geometry that others have already generated — significantly cutting down load times across the board.
Wrap-Up
CATProduct file management is an entirely separate discipline from modeling skill. You can be the best CATIA modeler on the team and still bring the whole project to a halt if your file structure and path management are a mess.
Two habits will eliminate the vast majority of link-related firefighting at the end of a project: agree on folder structure and file naming rules in writing before work begins, and put Relative Folder at the top of the Linked Document Localization list. Getting those two things right from day one is worth far more than any amount of Desk-window recovery work later.