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Manufacturing

Leverage Solid Edge's Ability to Manage Large Assemblies

14 Nov, 2004 By: Russell Brook Cadalyst

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Adequate hardware and optimized software add up to increased system performance

This month we are going to take a look at working with large assemblies. The term "large assembly" is relative, but Solid Edge customers are routinely creating assemblies that have several thousand components, and assemblies with tens of thousands of components are not uncommon. Drawings are the currency of many design offices, so we also have to consider being able to create drawing views of large assemblies efficiently. Many design engineers need to open the top-level assembly to take advantage of Solid Edge's top-down assembly modeling. The development team for Solid Edge understands this, and it spends a great deal of time and consideration on projects that ensure that Solid Edge can handle large amounts of data efficiently. Following is a discussion of the factors you should consider if you design large assemblies.

Hardware
Three main hardware components affect performance: main memory (RAM), CPU, and graphics card -- in that order. Your workstation will be doing a lot of number crunching. Main memory of 1GB-2GB is ideal for large assembly work. Secondly, you'll need a fast CPU -- 2GHz-3GHz or more. A twin processor is not essential, but it will improve performance if you are running other applications at the same time. Finally, choose a capable, professional graphics card that can be optimized for 3D CAD. For further information, see the "Graphic Card Testing" information on the UGS support Web site. Also check to see that you have installed the latest WHQL-certified graphics card drivers.

Networks
Another thing to consider is your network, especially if you are working in a collaborative environment. Make sure all client workstations have a least 100Mbit network access.

One ingenious solution is to install Solid Edge Insight. Not only will it allow you to work in a managed environment, Insight also offers technology that allows users to cache projects to local hard disk, thus removing the delays often created by heavy network traffic. The first time a project is checked out, performance on a 100Mbit network is about the same as that of a standard network drive. This is where the real benefits lie: From now on, every time you access or save the data, Insight checks with the server to see which documents have changed and then only transmits the changed data. This saves a lot of time and network bandwidth, a very clever solution!

Memory Optimization
The key to working with large assemblies is using the main RAM as efficiently as possible. Solid Edge takes advantage of simplified parts, culling, selection sets, display management, selection tools, and file open overrides. Some of these technologies within Solid Edge are automatic, such as culling, and some have to be driven manually, such as display configurations.

Graphics Performance
Reducing the amount of work required of the graphics card allows smooth manipulation of the views without sacrificing display quality. New to Solid Edge v16, you can now interrogate your graphics card and specify the best settings for display performance for it -- Software Driven being the slowest option and Graphics Card Driven (Advanced) being the fastest. You can manually select and experiment with these settings (figure 1) to see if a faster option works better for you.

Culling, display quality, and refresh scale are other factors that influence display performance. Culling is active during dynamic view manipulations, it instructs the display system to ignore display requests for certain objects if it detects that the display is taking an excessive amount of time. Culling can be controlled under View options as shown in figure 1 and can be turned off or made more sensitive using a slider bar. You might also want to consider turning off the View Transition option if the display becomes choppy when you transition to the sketch plane during the creation of a new feature or whilst editing an existing feature. Both functions are highly influenced by the power of the graphics card.

Refresh scale controls the speed and precision of the magnification commands, such as Zoom Area, Zoom, and Fit. The value indicates the scale factor to which you can zoom in before the geometry display refreshes. High values make the display refresh more slowly and increase the memory required to display lists.

The Sharpen command, is used to fine tine the display quality, it can be changed with Change View icons found this icon is found on the main tool bar (fig 2, improves the display quality of the graphics. As you specify a finer display quality, the graphics card has more work to do, therefore a faster display can be achieved by using a courser display setting, but for top quality images Solid Edge has the settings you need.

Display Settings. Solid Edge offers tools to change the display of the model, such as Wireframe, Wireframe with Hidden Edge Display, Shaded Only, and Shaded VHL (visible hidden line). Shaded is the fastest mode of display

Simplified Parts. When working with an assembly, you might find it useful to work with a simplified version of a complex part. For example, a part that contains numerous round chambers and holes will process more slowly than a part from which these features have been temporarily removed. The commands in the Simplify environment allow you to reduce the complexity of a part so it processes more quickly when used in an assembly. The goal of parts simplification is to reduce the number of surfaces that make up the part. You can also control whether the simplified version or the designed version of the part is displayed in the assembly (figure 3). And, unlike more traditional tools, the Simplify feature in Solid Edge does not break or remove any assembly relationships that rely on those features.

The follow methods of controlling the display of parts within an assembly are very clever ways to filter out unnecessary detail within a large assembly, things that are either to small to be displayed or turning off parts that are not being worked on, these settings have the added advantage, that when a drawing is produced, the drawing view wizard can make use of these setting to speed up drawing production. I will elaborate on this in next month's column.

Selection Sets. These tools help you quickly select the parts you are working on and turn off any unneeded parts; this not only makes the focus for design more understandable, it also frees up valuable resources by unloading all undisplayed parts from memory

• 2D and 3D Range Box. Simply drag a range box around the display and any parts inside the box are highlighted. You then have the ability not only to show and hide the components, but also to "show only," as well as zoom to the selected part or scroll to a part that will expand the pathfinder assembly structure. The 3D range box is slightly different in that a component is selected and then a range box is set for height and width and also depth.
• Select All Identical Parts. Selects all the parts in the assembly that are identical to the selected part.
• Select Small Parts. Selects parts based on the size of a box you draw (figure 4). Click and drag the mouse to define a 2D box, and parts that are smaller than the box are selected.

• Select Visible Parts. Selects parts that are fully or partially visible in the active window at its current view orientation. This gives you the ability to peel away the external components, moving progressively into a design from the outside.
• Query Select. Is something that can save a lot of time and frustration. it allows you to search on part properties such as categories, keywords, document number, or any other Solid Edge document property, including any custom properties that have been added. Query select does this even if not all the parts are displayed or active (saving valuable recourses) it also has the advantage of being able to find components in an assembly, even if they are several levels deep.

Activation Override
When Solid Edge is installed, an option is set to open all inactive parts when an assembly is opened. You can open an assembly with active and inactive parts as last saved by turning off the Activation Override; however, leaving this option on provides the most efficient means of opening an assembly. The Activation Override option is available on the General tab of the Options dialog box.

Assembly Configurations lets you open an assembly displaying only the parts of interest, saving resources while opening the top-level assembly. The Configuration select control is available on the Open dialog box.

Drafting
Solid Edge drafting will be covered in a future article. It is worth mentioning now, however, that assembly configurations can be used when laying down drawing views. Consider that if all you want to do is show a pictorial view, there is no need to process all the internal components of a large assembly. Simply use a configuration from an assembly with only those parts showing, creating views in a fraction of the time. Use Simplified parts and only the part edges that are required will be processed; at this level of detail small parts and features do not show up on a drawing anyway. Exploded view configurations are also useful for assembly instructions. One other thing to consider is to use Snap Shot view; this will quickly create plot-quality drawing views of an assembly.

Conclusion
Solid Edge offers some fantastic technology for helping you to work on large assemblies, optimizing your precious system resources. Drawing production has not been overlooked, either. Take advantage of these offerings, and you will be rewarded with a responsive system.

See you On the Edge next month.