CATIA V5 – Working with large sets

Managing large assemblies in the CATIA V5 system can be very demanding and frustrating to operate. Even with the use of extremely powerful computers, working with large circuits often leads to the destruction of the system with the message "Click OK to terminate". Here are recommendations for optimizing the system in order to minimize the demolition of the program and to make it easy to work with large sets.

          A. Cache System 

Activating Cache drastically improves system performance. When this mode is activated, CATIA loads all parts of a set in a visualization mode. Visualization mode does not load the whole history of a particular part, but only visualization, so the computer memory load is significantly lower.
To activate the Cache System, you need to click on Tools / Options / Infrastructure / Product Structure, and then turn on the Work with the cache system option in the menu. In addition, it is necessary to set the location for the Cache directory and set the maximum size of the directory depending on the available resources.


Then click Ok and restart the program. The next time you open the circuit, CATIA will load all the parts in the visualization mode. If you want to edit individual Part, you need to switch it to Design mode, which is done by right clicking on Part, then Representations / Design Mode.


          B. CGR Management

You can optimize CGR format files for large circuits. To optimize this, you need to click on Tools / Options / Infrastructure / Product Structure, then click on the CGR Management menu.


          C. Display options

By adjusting some of the performance settings, it can be greatly improved. Settings are determined by clicking Tools / Options / General / Display. It is recommended that you turn off Occlusion culling, set 3D Accuracy to 0.1 (increase in value improves performance), increase Level of Detail while Moving (increasing the value improves performance), increase Pixel culling while Moving (increasing the value improves performance).

          D. Disable Automatic Saving

By default, CATIA automatically records data every 30 minutes. During the recording, resources are significantly reduced, or the system slows down. You can turn off automatic data recording by clicking Tools / Options / General and turning on No automatic backup in the Data save settings.


          E. Stack size

Stack size is the number of "Undo" operations assigned to the CATIA session. Reducing this number increases the memory capacity and thus the performance. To set the value, click on the PCS tab in the General menu.


          F. Product Visualization Representation

Opening sets in such a way that all components are deactivated, and subsequently activated as needed, will improve memory utilization. To change this setting, you need to enable the Do not activate default shapes on open option within the Product Visualization (Tools / Options / Infrastructure / Product Structure) menu.