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FIGURE 11.4

Selecting a configuration from the Open dialog box

Creating configurations

You can create configs manually using the Modify dialog box, using the Configure Feature/Modify Configurations table, or through Excel-driven design tables. Design tables are extremely useful for situations where there are more than a few configs or more than a few items are being controlled. You should use design tables because they keep things very organized within the spreadsheet grid.

For now, I am going to focus on creating and manipulating configs manually so that you can become familiar with them without also worrying about Excel and design table syntax. I talk about design tables near the end of this chapter.

Creating a new config

To make a new config, you can right-click the top-level icon in the ConfigurationManager, which displays a part symbol and the name of the part, and select Add Configuration. If you right-click an existing configuration, SolidWorks will make a derived config, which I discuss later in this chapter. Figure 11.5 shows the RMB menu and the Properties dialog box that you can use to set up the new config.

FIGURE 11.5

Creating a new configuration

Using Configuration properties and options

The name of the config is important mainly for quick access and organization purposes. The configuration description is also important, because it can display in the ConfigurationManager, and even in the Assembly tree. (You can also use the FeatureManager Filter to search configuration descriptions.) This is important when the name of the config is numerical rather than descriptive, and you would like to also have a description but not include it in the name. The config description can also appear in place of the filename in the Assembly tree display. Config descriptions can be driven manually through the Configuration Properties dialog box or through a design table if you have many configs to manage. You can display config descriptions through the RMB menu, as shown in Figure 11.6.

FIGURE 11.6

Enabling configuration descriptions

The Bill of Materials (BOM) option is set in the Configuration Properties to use the filename, the configuration name, or a custom name that the user specifies. You can save this setting with a template. You achieve control over configurations through the combination of the Configuration Properties and the Advanced Options, which I discuss next.

Best Practice

Although you can change the preferred settings at any time, it is definitely a best practice to make a template early on when you are using SolidWorks to model parts. SolidWorks remembers the BOM options and Advanced options that you set for the Default configuration and uses them in document templates. This is true for both part and assembly templates.

Using Advanced options

Two advanced configuration options are found in the bottom panel of the Configuration Properties PropertyManager: Suppress features and Use configuration specific color. While the second option is self-explanatory, the first one is not and often catches new and even experienced users off-guard.

Suppress features refers to how inactive configurations should handle new features that are added to the part. For example, if you have two configs, 1 and 2, and config 1 is active and you add a new Fillet feature, what happens to that feature in config 2? If this option is turned on, the new features are suppressed in the inactive configs. If it is turned off, the new features will be unsuppressed when the inactive configs are activated. This creates a much bigger challenge for manually created configurations than for design table-driven configs because changing suppression states for several features across multiple configs is much easier in a design table than in manual config management.

Using the Modify dialog box

The Modify dialog box enables you to change dimensions by just double-clicking the dimension and changing the value. When you change a dimension using the Modify dialog box in a part that has more than one configuration, an additional