Controlling Display States and Configurations

Display states can be either independent of configurations or linked to them, depending on your settings. To control the display, you can use the Display pane that pops out when you click the double-arrow icon in the upper-right corner of the FeatureManager (or you can press F8). Figure 19.1 shows the Display pane in action, along with an assembly showing parts in different display states.

The column symbols for the Display pane are as follows:

• Hide or show state of the part
• Display Mode options for each component:
• Appearances
• Transparency
• Default Display
• Component/Part Color

Appearance overrides are settings that apply color to different aspects of model geometry. There is a hierarchy in which the appearances are applied, so an appearance applied to a feature may override or be overridden by another appearance applied to the part or an individual face. The appearance override hierarchy is summarized here, showing the highest priority at the top:

• Assembly
• Component
• Face
• Feature
• Body
• Part

So, you can read into this that the part appearance is overridden by every other type of appearance, and the appearance applied to the assembly overrides everything else.

If you override the appearance or display mode for a component in a subassembly, and the upper-left triangle appears in the Display pane, you can remove the override through the left mouse button (LMB) or the right mouse button (RMB) menu. Figure 19.2 shows the LMB menu from a component of a subassembly with overrides.

When you select Clear Override, SolidWorks clears any overrides for the currently selected component. Clear All Top Level Overrides clears all overrides in all the subassemblies in the entire top-level assembly. There is no intermediate option to clear all top-level overrides for a particular subassembly; if you want to distinguish between overrides at that level, you need to clear several individual overrides. The options to remove overrides do not affect top-level components.

The active display state appears in angle brackets after the configuration name and the filename at the top of the FeatureManager, as shown in the image on the left in Figure 19.3. Display states are created and managed in a panel at the bottom of the ConfigurationManager, as shown in the image on the right in Figure 19.3. To create a new display state, simply right-click in the Display pane and choose Add Display State. As an alternative, you can isolate the components you need to show and then click the Save icon on the Isolate tab to create a new display state.

SolidWorks also allows you to open display states right from the Open dialog. This can be a big time-saver when you're opening very large assemblies that make good use of display states.

Using Display States with Drawings

Display states can be shown on drawings. If you only show or hide parts in display states, you can still use display states on drawings. For display states that change the display mode (Wireframe, Shaded, and so on) to work properly, you must set the view to the desired display mode and then select the display state from the PropertyManager for the view.

Using Part Display States in Parts

Parts can also have display states, including separate bodies within parts. You can control the part display state for specific instances of a part within an assembly in the Component Properties dialog box. Using part display states offers the same advantages as using assembly display states (mainly display speed), especially when compared to configurations.

Applying Configurations for Performance

Assembly configurations are some of the best tools to make working with large assemblies easier. You can use several techniques to improve the speed of working with assemblies. Selecting a method that is appropriate to the situation is important because each method has its strengths and weaknesses.

GETTING FAMILIAR WITH THE ADVANCED COMPONENT SELECTION

The Advanced Component Selection dialog box, shown in Figure 19.4, was formerly called Advanced Show/Hide Components. You can access this dialog box by right-clicking the configuration name in the ConfigurationManager and selecting Advance Select.

This tool enables you to establish search criteria and show or hide parts based on the criteria. Multiple criteria can be used, stored, and retrieved. This tool is generally underused, and people are often surprised to find it in the software. The Category 1 options enable you to search on things such as document name, in-context status, part mass, and other standard SolidWorks information. Category 2 can be either custom property information or structured options for Category 1, such as specific in-context conditions.

LOOKING AT THE ISOLATE FUNCTION

Isolate works like the inverse of the Hide command. If you select multiple parts and click Isolate from the RMB menu, the selected parts remain shown, and everything else becomes hidden. A little pop-up menu gives you the option to show the removed components in a Wireframe or Transparent display mode, or to save the current display as a new display state. This is a very useful function, as shown in Figure 19.5.

CONTROLLING DISPLAY PERFORMANCE

Overall, SolidWorks performance is split into two categories: CPU processing and GPU (graphics processing unit) processing. Which of these functions your computer performs better depends on your hardware, drivers, and system maintenance, among other factors.

When trying to speed up the performance of an assembly, you can make the biggest impact by reducing the load on both the CPU and the GPU. You can do this by suppressing a part. When a part is suppressed, it is neither calculated nor displayed; this means the load on each processor for that part is zero.

When you hide a part, its parametric features are still calculated by the CPU; however, because the part is hidden, it does not create a load on the GPU. If you have a good main processor and a questionable video card, then you will achieve a greater benefit from removing graphics load from your display. Simply unload the hidden component from RAM.

Using Lightweight Parts Settings

If you want to show a part, but not calculate any of its parametric relations, you can use lightweight parts. You can access the Lightweight default settings by choosing Tools ➢ Options on both the Assemblies and Performance pages. You can make parts lightweight through the RMB menu. The opposite of lightweight is resolved. Resolved means that the part is fully loaded, its parametrics are loaded and calculated by the CPU, and its graphics display data is calculated and shown by the GPU. In lightweight, the body data is loaded, along with the reference geometry features and the mates for the top-level components. The graphics data will always be computed in the current session in both Resolved and Lightweight modes. The LDR mode is the only mode where the graphics data is read from the file and not computed in the session.

Working with SpeedPak

There is some confusion about where the SpeedPak functionality falls in this scheme of things. With a SpeedPak, the parametrics are not loaded, but the graphics are. In addition, some of the geometry is selectable, as if it were imported geometry (actual geometry but without rebuildable parametrics). However, a SpeedPak applies only to subassemblies, where the need for improvement is much higher.

There is a five-way relationship among the Resolved, SpeedPak, Lightweight, Hidden, and Suppressed states, as shown in Figure 19.6.

Comparing Resolved to Unsuppressed

The terminology becomes a little convoluted here because of the relationships between the five different states. In parts, the feature states are easy to remember because features can be either suppressed or unsuppressed. However, in assemblies, there are five states instead of two, so unsuppressed could mean anything that is not suppressed, which still leaves three states. For this reason, resolved is used instead of unsuppressed when dealing with components in an assembly.

Using Configurations for Positions

When you use configurations to display an assembly in various positions, you can do it either by changing mates or by changing a layout sketch. Mates are configurable in two ways: Mates can be suppressed and unsuppressed, and angle and distance mate values can be configured in the same way that sketch dimensions can be configured. Although creating a mate scheme that enables you to reposition the assembly using mate suppression states and values is essential to this method, it may not be the best approach. When mates are suppressed, the components move, and if the mates are later unsuppressed, the assembly may not return to the original position. Mates can often be solved in different orientations and may flip if turned on and off in this way.

Using a skeleton or layout sketch to mate parts may be a better approach, although this also has drawbacks. If you mate to a layout sketch, you cannot use Dynamic Assembly Motion. If you use the mate scheme discussed previously, this generally means having a fully defined assembly, and this doesn't allow for Dynamic Assembly Motion.

As a compromise, a good way to handle this is by using one configuration for Dynamic Assembly Motion, with one or more open degrees of freedom. You can use other configurations to fully define the mechanism and show it in particular positions using either method. Probably the best way to demonstrate this idea is with an example using the robot arm assembly.

POSITIONING WITH MATES

First, look at positioning with mates. On an assembly such as this one, the goal is to position the grippers. You can do this a couple of ways, both directly and indirectly. In the assembly used for this chapter, the grippers have been rebuilt as a subassembly, which allows different types of control. Notice that the subassembly has a configuration for the closed position and one that allows Dynamic Assembly Motion. In addition, the subassembly is being solved as Flexible. Figure 19.7 shows the assembly and the FeatureManager.

Driving the Position Directly

A sketch point has been added to the subassembly to identify the precise point on the gripper that is to be positioned. Sketch points have also been added to the main assembly to represent parts that need to be picked up by the robotic arm.

Check the derived configurations under the default configuration. Notice that when you switch between certain configurations, the parts seem to separate. Moving one of the links causes the parts to snap back together again. This is probably because there are so many options when moving between configurations that the software has difficulty choosing a final position. This is definitely one of the potential problems when using configured mates to show an assembly in various positions.

Notice also that although the grippers are positioned correctly, the arm is still allowed to swivel around the intended target point. You can correct this by defining an orientation for the grippers for each location. If an additional pivot were added to the assembly, then fully defining the parts would become more difficult. The arm would not be able to reach any additional points, but it would not be so limited in orienting the grippers at each point.

Driving the Position Indirectly

You can also use mates to drive configured positions of the assembly using a series of angle mates. This makes it more difficult because to get to a particular location, you have to do some calculations, but the angle mates are more stable than simply relying on moving parts to unconstrained positions.

If you cycle through the derived configurations under the Indirect top-level configuration, you will notice that mates are not suppressed and unsuppressed; instead, the values are changed. This makes it more difficult to position the grippers precisely, but because it is specific about the positions of the individual parts, there is no ambiguity.

POSITIONING WITH SKETCHES

Although this technique still uses mates to position the parts and to change the position, you change sketch dimensions rather than mate values. Sketches used to drive parts from an assembly are sometimes called layout sketches or skeletons. They are also discussed in Chapter 16, “Working with Assembly Sketches and Layouts,” for in-context or top-down assembly techniques. Figure 19.8 shows the assembly that is used for the rest of this chapter.

This particular assembly is driven by two sketches on different planes to govern the position of the parts. Keep in mind that this assembly has been used for all the other techniques as well; this means that all these techniques can exist together simultaneously and are controlled by configurations.

Examine the assembly to see how the parts are mated to the sketches. This is important. The first time you create a part such as this, you may be tempted to mate part planes to the sketch lines.

Applying Configurations for Product Variations

In this case, product variations are variations in size or part replacement. Some examples are a 4-foot cabinet and an 8-foot cabinet, or a two-button mouse and a three-button mouse.

As a simple example, Figure 19.9 shows the familiar robotic arm assembly, but with a variation: one of the arms has been replaced with a subassembly. The subassembly is made of the original replaced part using configurations, and there are configurations of the subassembly, which is again being used as a flexible subassembly.

Through the course of this chapter, the robot arm assembly has greatly increased in complexity, but it has retained the original information that was in the first version. Maintaining valid assembly data through manually managed configurations is difficult, and all it takes is a simple mistake to wipe out lots of assembly configuration data. Appropriately, the next section discusses assembly design tables.

Using Design Tables for Assembly Configurations

This chapter augments information that you need to know to use design tables effectively in assemblies. Assembly design tables can do everything that part design tables can do, except for selecting configurations of base parts and split parts, which are not valid assembly functions. Assembly design tables can also do some things that a part design table cannot, including the following:

• Suppressing the state of a part (R for Resolved or S for Suppressed)
• Assigning the component configuration for the assembly configuration
• Enabling you to activate the Never Expand In BOM option

Figure 19.10 shows the design table results from auto-creation using the robot arm assembly. Some columns have been hidden to make it small enough to fit on the page. If you want to see the entire table, you must open the assembly. If you edit the design table, you will probably want to use the Open In Separate Window option, which is easier to navigate and control.

Working with Modify Configurations and the Configuration Publisher

The Modify Configuration interface is a dialog box where you can create configurations to configure dimensions, features, and custom properties in parts; you can use it in assemblies as well. It is sometimes used in place of design tables when you do not need the advanced functionality of Excel.

The Configuration Publisher is used to create a PropertyManager that pops up when the part is placed into an assembly. The PropertyManager enables you to select a configuration to go into the assembly. You can also create new configurations on demand, inside the constraints defined in the Configuration Publisher. It is a great tool for assemblies with zillions of possible variations (for example, the catalog of a crane vendor). The Configuration Publisher is also available in assemblies; this means you can use a pop-up PropertyManager when assemblies are placed into other assemblies as well. Library subassemblies may be less common than library parts, where the pop-up PropertyManager would be used to best effect.

Both tools are useful for managing assembly configurations. Design tables offer the most complete control, but they also have some drawbacks associated with being tied to Microsoft Excel. Both Modify Configurations and the Configuration Publisher are internal to SolidWorks, regardless of the level of the software you have purchased, so if you use one of them, you can be sure that whomever you send data to can access all the functionality.

Looking at Assembly Configuration Dos and Don'ts

Assembly configurations have some potential pitfalls that you can avoid if you pay attention to some of these dos and don'ts.

• Avoid using Delete as an editing option when working with configurations. Delete is forever and removes items from all configurations.
• Avoid the use of in-context relations to size parts when you are also using configurations to size parts. A nonconfigured part driven by a configured part only causes confusion.
• Avoid using configurations to represent document control-type revisions. When people attempt to do this, it ultimately limits the kinds of edits they can make to their parts and assemblies, and it is far too easy to make a mistake that wipes out all their work. In the end, this is not a viable technique.
• If you are working with manually created configurations, you should create a new configuration and activate it before making the changes. Otherwise, you will end up trying to set the original configuration back to the way it was.
• Remember to select the This Configuration Only option for changed dimensions instead of leaving it at the default All Configurations setting.