CATIA · CGR · Assembly Management
If you’ve ever opened a large CATIA assembly — one with hundreds or even thousands of parts — and watched your PC grind to a halt, you know the frustration. To handle this, CATIA offers two distinct loading modes: Design Mode and CGR Mode (Visualization Mode / Cache Management).
“Keep the full assembly light in CGR mode, and switch only the parts you need into Design mode — that’s the standard workflow for heavy assemblies.”
In this post, I’ll walk through the difference between the two modes, what a CGR file actually is, and a practical tip for sharing the CGR cache over NAS to drastically speed up loading times for your entire team.
1. What Is Design Mode?
Design mode loads the full, original data of every part into your PC’s RAM. Nothing is held back.
- What you get: All sketches, features, constraints, and design history are fully active. Parts in the specification tree show a green icon, indicating they’re loaded in Design mode.
- The upside: You have complete access — edit dimensions, modify geometry, add or update assembly constraints. Anything goes.
- The downside: It’s heavy. Opening a large assembly entirely in Design mode puts enormous strain on your RAM and GPU. This is the most common reason CATIA slows down or becomes unresponsive.
2. What Is CGR Mode (Visualization Mode)?
CGR mode strips away all the heavy design history and loads only the visual shell of each part — a lightweight file format called CGR (CATIA Graphical Representation) — cached locally for fast access.
- What you get: The 3D shape is visible, but there’s no underlying sketch or feature tree. Parts in the tree show a blue or gray icon, making it easy to tell them apart from Design mode parts at a glance.
- The upside: Assembly loading times drop dramatically, and memory usage is a fraction of Design mode. It’s ideal for reviewing overall geometry, checking for interference, or taking section cuts — anything that doesn’t require editing.
- The downside: You can’t edit geometry in this mode. To make changes to a specific part, right-click it in the tree and select Represent → Design Mode to switch just that part over.
3. Design Mode vs. CGR Mode — At a Glance
| Category | Design Mode | CGR Mode |
|---|---|---|
| Data Loaded | Full original data (history included) | Visual shell only (CGR cache) |
| Tree Icon Color | Green | Blue / Gray |
| Geometry Editing | Yes ✓ | No ✗ |
| Loading Speed | Slow | Very fast |
| Memory Usage | High (heavy) | Low (lightweight) |
| Best For | Design work, editing, modifications | Review, interference check, section view |
4. What Exactly Is a CGR File?
A CGR file is essentially a lightweight visual snapshot of a CATIA part (.CATPart) or product (.CATProduct). Think of it as a stripped-down, display-only version of the 3D geometry — no history, no sketches, just the shape.
- How it’s generated: Once you enable Cache Management in the CATIA options, CGR files are created automatically whenever you open an assembly. No manual steps required — CATIA handles it in the background.
- Default storage location: By default, CATIA saves CGR files to your local PC at C:\Users\[username]\AppData\Local\DassaultSystemes\CATCache. You can change this path in the options.
- File size: Typically around 1/5 to 1/10 the size of the original CATPart. The more complex the geometry, the more dramatic the size reduction.
5. Pro Tip: Share CGR Cache Over NAS for Team-Wide Speed
Most users leave the CGR cache path pointing to their local C drive — which works fine for solo work. But if your team shares CAD data over a NAS (Network Attached Storage), there’s a smarter setup that can make a real difference.
In CATIA, go to Options > Infrastructure > Product Structure > Cache Management and set the Path to the local cache to a shared folder on your NAS — for example, Z:\CATIA_Cache — on every workstation.
5-1. Why This Works So Well
- Cache files get shared across the team: The first person to open a large assembly takes the hit — CATIA generates CGR files for every part and saves them to the NAS folder. When the next person opens the same assembly, CATIA just reads the already-generated CGR files from NAS instead of rebuilding them from scratch. After that first load, everyone else opens it fast.
- No duplicate cache data, less disk usage: Instead of every PC storing its own copy of the cache, there’s one shared set on NAS. Teams stay in sync, local drives stay clean, and everyone’s working from the same up-to-date visualizations.
- Cache goes stale when geometry changes: If someone modifies a part, the old CGR file on NAS still shows the previous shape. Make sure to clear the cache for that part (Clear Cache), or verify that CATIA’s auto-update option is enabled — otherwise teammates may unknowingly view outdated geometry.
- Network speed matters: On a wired gigabit (1Gbps) LAN, the NAS cache feels just as snappy as local storage. But on slower connections — Wi-Fi, 100Mbps — it can actually be slower than reading from a local drive. Make sure your network infrastructure is up to the task.
Wrapping Up
The go-to workflow for handling large CATIA assemblies is straightforward: open everything in CGR mode to keep things light, and switch only the parts you’re actively working on into Design mode.
- Green icon in the tree = Design mode (fully loaded)
- Blue / gray icon = CGR mode (visualization only)
- Right-click any part → Represent → Design Mode to switch when you need to edit
- On a team using NAS? Unify the CGR cache path across all workstations for a serious loading speed boost