CATIA V5 Large Assembly Performance: Cache, Level of Detail, and Visualization Mode

CATIA V5 Large Assembly Performance: Cache, Level of Detail, and Visualization Mode

I work with CATIA assemblies in the automotive supply chain — our typical product assembly has 8,000 to 12,000 instances, and the full vehicle assembly at our OEM customer exceeds 50,000. Over the years, I've learned that CATIA V5 can handle these sizes, but only if you configure it correctly. Out of the box, CATIA loads every component's full geometry into memory, which is fine for 100-part assemblies but catastrophic for 10,000-part ones. The three settings that make the biggest difference are the CGR cache, visualization mode, and level of detail.

Understanding CGR (Catastrophically Good Resolution — Just Kidding)

CGR stands for CATIA Graphic Representation. A CGR file is a lightweight representation of a CATPart — it contains only the tessellated graphics data (triangles for display), not the precise B-rep geometry. A typical CATPart might be 50MB, but its CGR representation is 1-2MB. When you load an assembly in CGR mode, CATIA loads the CGR files instead of the full CATParts, reducing memory consumption by 90%+.

Enabling the CGR Cache

1. Go to Tools → Options → Infrastructure → Product Structure
2. Under the Cache Management tab:
   • Check Enable cache system
   • Set Cache size to at least 4096 MB (4GB) — I use 8192 MB (8GB) on workstations with 32GB+ RAM
   • Set Cache location to a local SSD path (e.g., C:\CATCache)
3. Under Cache Settings:
   • Set Time stamp to Check timestamp — this ensures CATIA uses the latest version of each CGR
   • Set Release cache to Automatic

How the Cache Works

When you open an assembly with the cache enabled:

1. CATIA checks the local cache for each component's CGR file
2. If the CGR exists and is current, it loads from the local cache (fast)
3. If the CGR doesn't exist or is outdated, CATIA generates it from the CATPart and stores it in the cache
4. The first load is slower (generating CGRs), but subsequent loads are much faster

Generating CGRs in Batch

For a large assembly, the first load can be very slow as CATIA generates CGRs for every component. You can pre-generate CGRs using a batch process:

1. Open a command prompt
2. Navigate to your CATIA installation's code\bin directory
3. Run: cgrbatch -file "C:\path\to\assembly.CATProduct" -output "C:\CATCache"
4. This generates all CGR files without opening the full CATIA UI

Schedule this as a weekly task to keep the cache fresh.

Visualization Mode vs. Design Mode

CATIA V5 has two loading modes:

• Design Mode: Loads the full CATPart with all geometry and feature tree. You can edit the part.
• Visualization Mode: Loads only the CGR representation. You can see the part, measure it, and create sections, but you can't edit features.

For large assemblies, you should work in Visualization Mode by default and only switch individual components to Design Mode when you need to edit them.

Setting the Default to Visualization Mode

1. Tools → Options → Infrastructure → Product Structure
2. Under the Product Structure tab:
   • Set When loading a product to Do not activate default components
   • This prevents CATIA from loading all components automatically
3. Under the Cache Management tab:
   • Ensure Work with CGR only when the cache system is activated is checked

Switching Components Between Modes

• To switch a component to Design Mode: Right-click → Components → Define Design Mode
• To switch back to Visualization Mode: Right-click → Components → Define Visualization Mode
• You can also use the Representations toolbar to switch modes for selected components

Level of Detail (LOD)

CATIA V5 supports Level of Detail for CGR files. A LOD is a coarser tessellation — fewer triangles, less memory, faster display. You can define multiple LODs for each component.

Defining LODs

1. Open the CATPart
2. Tools → Options → General → Display → Performance
3. Under 3D Accuracy:
   • Set Proportional to a value between 0.01 and 0.5
   • Lower values = higher quality but more triangles
   • Higher values = lower quality but fewer triangles
4. For large assemblies, I use:
   • High LOD: 0.01 (for close-up work on specific components)
   • Medium LOD: 0.1 (for general assembly navigation)
   • Low LOD: 0.3 (for overview and large assembly navigation)

Switching LODs at Runtime

1. View → Navigation Mode → Level of Detail
2. Select the LOD you want to use
3. CATIA will switch all CGR representations to the selected LOD
4. This is nearly instant if the CGRs already have the LOD data cached

Additional Performance Settings

Deactivate Default Components

When opening a large assembly, CATIA can load only the top-level structure without activating any components:

1. Tools → Options → Infrastructure → Product Structure
2. Set When loading a product to Do not activate default components
3. When you open the assembly, you'll see the tree but no geometry
4. Right-click the components you want to see and select Activate Node

This is useful when you need to work on a specific subassembly within a large assembly — you only load what you need.

Disable Shadow Rendering

Shadows are computationally expensive, especially with thousands of components:

1. Tools → Options → General → Display → Performance
2. Uncheck Activate shadows
3. This alone can improve frame rates by 20-30% in large assemblies

Reduce Anti-Aliasing

1. Tools → Options → General → Display → Performance
2. Set Anti-aliasing to None or 2x (not 4x or 8x)
3. Anti-aliasing smooths edges but requires significant GPU computation

Performance Impact: Real Measurements

I measured the impact of these settings on a 9,200-instance assembly:

| Configuration | Load Time | Memory Usage | Frame Rate | |--------------|-----------|-------------|------------| | No cache, Design Mode | 42 min | 38 GB | 2-5 FPS | | Cache, Design Mode | 18 min | 38 GB | 2-5 FPS | | Cache, Visualization Mode | 3 min | 6 GB | 15-25 FPS | | Cache, Vis Mode, LOD 0.3 | 1.5 min | 3 GB | 30-45 FPS | | Cache, Vis Mode, LOD 0.3, No Shadows | 1.5 min | 3 GB | 40-60 FPS |

The difference between the worst and best configuration is dramatic: 42 minutes vs. 1.5 minutes load time, 38GB vs. 3GB memory, 2 FPS vs. 60 FPS.

Summary

For large CATIA V5 assemblies, the three most impactful settings are:

1. Enable the CGR cache — 90% memory reduction
2. Work in Visualization Mode by default — only load full geometry for components you're editing
3. Use Level of Detail — coarser tessellation for overview navigation

With these settings, a 10,000-instance assembly that would normally take 40+ minutes to load and consume 38GB of RAM can be loaded in under 2 minutes using 3GB of RAM. You'll need to switch individual components to Design Mode when you need to edit them, but the time savings on every other operation more than compensates.