Why does CATIA V5 slow down when working with large assemblies?

Performance issues in CATIA V5 often occur due to the high computational demands of managing large assemblies. Factors such as recalculating inertia measures, high 3D accuracy settings, and insufficient hardware resources can cause delays, freezing, or crashes.

Activate the cache system:

• Load assemblies in visualization mode to reduce memory usage.
• Go to tools > options > infrastructure > product structure > cache management, and enable work with cache system.

Optimize CGR management:

• Use CGR (CATIA graphical representation) files for lightweight visualization.
• Go to tools > options > infrastructure > product structure > CGR management, and enable optimization for large assemblies.

Adjust display settings:

• Go to tools > options > general > display > performance.
• Set 3D accuracy to a coarser value (e.g., 0.2 or higher).
• Enable level of detail (LOD) to reduce polygonal representation for distant objects.
• Disable occlusion culling and lower anti-aliasing for better performance.

Reduce undo stack size:

• Lower the undo stack size from 10 to 5 to free up memory.
• Navigate to tools > options > general > PCS, and adjust the stack size.

Disable automatic inertia recalculation:

• In assemblies where inertia updates are unnecessary, disable automatic recalculation.
• Go to tools > options > mechanical design > assembly design, and turn off inertia measure updates.

Use approximate view mode in drafting:

• For large assembly drawings, enable approximate view generation mode.
• Navigate to tools > options > mechanical design > drafting, and select approximate view mode.

Clean data regularly with CATDUA V5:

• Use the CATDUA tool to clean corrupted data and optimize assembly files.
• Go to file > desk, right-click on a part or product, and run CATDUA with priority set to 3.