Working With Large Assemblies

How to work with Large Assemblies in almost any version of NX. The following Best Practices show how to increase performance, reduce time spent, reduce system demand, and eliminate loading not needed components.

Working with Large Assemblies, Best Practices

REDUCE OVERHEAD

Load Options: Use "Partial Loading” NX can load components 3 different ways, Fully loaded, Partially loaded, with/with out wave data. Partial Loading loads enough information to show the part, but does not evaluate expression or interpart expressions Downside is if parts rely on other parts via interpart expressions and it has changed since last time it was fully loaded, you will not see the change. Making the part the work or displayed part causes NX to fully load the part

Load only Need Components: Large assemblies you may want to load no components and only turn on the necessary components as needed This may be a slow process picking and choosing the right component. For companies that deal with large assemblies and open them a lot it is more efficient to use "Design in Context". Design in Context is a Teamcenter Engineering application

Reference Sets: Use Reference sets to Display only the needed geometry. Usually reference sets only consist of solid geometry, occasionally it may contain wireframe to show a centerline or other similiar information Component

Filters/Sets: When working on specific assemblies for an extended period of time create a Component Filter so that you can quickly return to the previous configuration

Faceted Bodies: Loading a component with a specific reference set that is only a faceted body will lower the resources needed to start NX Faceted bodies consist of the outer skin of the body and approximations of the solid bod

 

INCREASE PERFORMANCE

Work Part Emphasis Assembly Preference: Making a component the work part, the system “grays-out” the non-work parts. To save on resources you can turning on Preferences -> Assemblies -> Emphasize. When enabled, the work part remains displayed in its current color, but the rest of the assembly is dimmed in the color specified in the color option.

Disable Smooth View Change: When switching between views, NX has eye candy to smoothly transition between views. This feature helps keep the user orientated to what view they are coming from and going to. The downside is that it requires more resources. In single parts and small assemblies this is not an issue but with large assemblies this may have a performance hit.

Backface Culling: Specifies whether the graphics driver should disable rendering of backfacing polygons in shaded views. When backface culling is enabled, any surface facets that have normals directed away from the viewer are not rendered. This reduction in the number of facets rendered can significantly improve graphics performance, especially on low-end and mid-range graphics devices. This should be enabled for large assemblies. Fixed

Frame Rate: Improve zoom, pan, and rotate by turning on Preferences -> Visual Performance -> Fixed Frame Rate. This will make Objects like components to be converted to cubes or hidden. Depending on the current zoom small features and components may be hidden or greatly simplified The lower the frames per second is best for performance.

Scene Reduction Method: If enabled, when rotating this will hide objects. When you stop the rotation NX will render the components correctly back to recognizable parts instead of cubes

View Frustum Culling: If enabled, Objects not displayed in the current view window will not be rendered