Finding Configurations

SolidWorks configurations are listed in the ConfigurationManager. This is a tab at the top of the FeatureManager area, shown in Figure 11.1.

Deleting Configs

When you're using a standard template, each part has a default config named “Default.” There is nothing special about this config; you can rename it and even delete it. At least one config must always remain in the tree, and you cannot delete the configuration that is currently active. If you want to remove a config, switch to another config (by double-clicking the other configuration in the ConfigurationManager) and then delete the one you want to remove.

If you try to delete a part configuration being used by an open assembly, SolidWorks will simply issue the message “None of the selected entities could be deleted” without explanation.

If you delete a configuration of a part that is used in an assembly, but the assembly is not currently open, the next time the assembly is opened, it will issue the message “The following component configurations could not be found [component configuration name]. If the configuration was renamed the same configuration will be used, otherwise the last active configuration will be substituted for each instance.”

You can delete groups of configs using Windows select tools (Shift+select or Ctrl+select) in the ConfigurationManager. You can also use the right mouse button (RMB) menu, much like regular features in the FeatureManager. None of the configurations selected for deletion may be active or referenced by other open and resolved documents.

Sorting Configs

In the ConfigurationManager, configs can be listed in one of five ways:

• Numeric: Sorts in ascending numeric order
• Literal: Sorts ascending alphabetical order
• Manual: Allows you to determine the order by drag-and-drop
• History-based: Sorts by creation date
• Design Table: Sorts by the order in which they are found in the design table

To control which sorting option is used, right-click on the name of the part in the ConfigurationManager tab and select Tree Order.

Activating Configurations

Within a part file, to change the display from one configuration to another, you must first switch to the ConfigurationManager panel, and then either double-click the desired config or right-click it and select Show Configuration.

Alternatively, you can right-click the config in the ConfigurationManager and select Show Preview, as shown in Figure 11.2. A small preview thumbnail will display in the PropertyManager panel. However, not all configurations have previews. For example, in a part with many configs that have been generated automatically by a design table, the configurations may not have previews because the config itself has never actually been rebuilt. Previews exist only when the configuration has been activated at least once, the image on the screen generated, and the part saved. SolidWorks stores both the body (geometry) and the preview image of the part so that next time you access the configuration, the software does not have to rebuild everything again. Storage space is cheaper than rebuild time.

You can even select a configuration while opening a file. By doing this, you will save time by not needing to rebuild the model. To take advantage of this option, you must use the File ➢ Open interface, which is shown in Figure 11.3. You can select the config from the lower-left drop-down Configurations list.

Creating Configurations

You can create configs manually using the Modify dialog box, using the Configure Feature/Modify Configurations table (shown in Figure 11.4), or through Excel-driven design tables. Design tables are extremely useful for situations where more than a few configs or more than a few items are being controlled, and as always, the more people who will be working with the data, the more tightly you need to control it. It would be a safe best practice to say that any time you use configurations, and the items being controlled can be handled by a design table, you should use the design table.

For now, I'm going to focus on creating and manipulating configs manually so you can become familiar with them without also worrying about Excel and design-table syntax. I will 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. New configurations copy the currently active configuration. If you right-click an existing configuration, SolidWorks makes a derived config, which I will 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.

USING CONFIGURATION PROPERTIES AND OPTIONS

The name of the config is important mainly for quick access and organizational 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 want 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 very many configs to manage. You can display config descriptions through the RMB menu, as shown in Figure 11.6.

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.

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 button, shown in Figure 11.7, appears in the Modify dialog box.

Modify has three options for configuring dimensions: This Configuration, All Configurations, and Specify Configurations. All Configurations is the default option. Choosing the Specify Configurations option opens a dialog box, which is shown in Figure 11.8.

Using the Modify Configurations Dialog Box

The Modify Configurations dialog box, shown in Figure 11.9, enables you to create and modify configured features and dimensions in a more organized way than by using the simple manual methods described earlier, but without getting involved in an Excel-based design table, described later in this chapter. Do not confuse the Modify Configurations dialog box with the Modify dialog box, which is used to change dimensions.

You can access the Modify Configurations dialog box by right-clicking a dimension or feature you want to drive via configurations and selecting Configure Dimension or Configure Feature.

With the Modify Configurations dialog box active, double-click a dimension to add it to the configured features list. You can add configurations on the fly by typing in the appropriate box, and you can change values or states of features by double-clicking and entering numbers or selecting the check box in the appropriate column (suppressed features will use a check box to define whether the feature is suppressed or not).

I tend to use either the manual or Excel-based techniques. Modify Configurations is valuable for people who want to configure a couple of features without getting involved in a big spreadsheet. It might also be valuable to people who do not have Excel available on their computers but want to create a more structured way to manage configuration data. You can also use it to rename dimensions by following these steps:

1. Turn on the Show Feature Dimensions setting in the Annotations folder.
2. Select a dimension.
3. Use Ctrl+A to select all dimensions.
4. Select Configure Dimension from the RMB menu
5. Use the Modify Configurations dialog to rename multiple dimensions.

In addition, I should mention that much folklore exists surrounding what is perceived as a problematic relationship between Excel and SolidWorks. Some users claim that Excel often causes SolidWorks to crash. Beyond that, many workplaces may not have Excel available to them, either because of the cost or because they use a non-Microsoft solution for spreadsheet applications. These users still want the functionality of design tables even if Excel is not installed on their machines.

The icons in the lower left of the Modify Configurations dialog box enable you to use the dialog box for more than just dimensions and feature suppression, including custom properties.

The Modify Configurations dialog box does not give you control over everything. Some things, such as part color, Some things that you can configure, such a part color, cannot be driven from this dialog box. Design tables are still the most powerful way to go, but Modify Configurations offers lots of flexibility and immediacy.

USING TABLE VIEWS

The Modify Configurations dialog box adds significantly to your options for creating and editing configurations. Two very nice tools that add to the convenience and power of SolidWorks configurations are called Table Views and Hide/Show Custom Properties.

The Table Views tool enables you to keep a small table of only the parameters you want to show. The Parameters drop-down list enables you to select which table view you want to display or to create a new one. Using drop-down lists on the parameter headings, you can suppress the display of any parameter in a new table view.

Dividing what might otherwise be a large design table into several table views helps to keep your data organized and easy to access. Figure 11.10 shows the ConfigurationManager of a part with configurations managed with table views.

Using Custom Property Managers

The Property Tab Builder enables an administrator to create special Task pane tabs that are used to control custom properties and configuration-specific custom properties. Configuration-specific custom properties can be controlled through design tables, Custom Property tabs, or the regular SolidWorks configuration-specific custom property interface. Select the method that works best for the way you and your company use the software.

Figure 11.11 shows the Property Tab Builder interface. You can access the Property Tab Builder by clicking the Windows Start button and choosing SolidWorks ➢ SolidWorks Tools from the menu. This is the place where you actually construct the interface that shows up in the Properties tab of the Task pane on the right side of the SolidWorks graphics window.

Using this type of interface enables the administrator to standardize custom properties values due to spelling or differences in interpretation. The Task Pane interface is easy to use and highly customizable. Notice that you can create regular custom properties or configure custom properties, and that option can be set independently for each property value entered using this interface.

After you create a Property Tab file (called a template), save it to the location indicated at Tools ➢ Options ➢ File Locations ➢ Custom Property Files. If you have only one template for a document type (part, assembly, or drawing), it automatically appears when you display the Custom Properties tab of the Task pane. If you have multiple templates established, the Custom Properties tab lets you choose which one to use. Figure 11.12 shows a Custom Properties tab in use within the SolidWorks Task Pane interface.

Using Derived Configurations

Derived configurations are configs that are dependent on other configs. You can create them from the RMB menu on a configuration, and they appear indented underneath the parent config. Figure 11.13 shows the RMB menu and the position of the derived config in the tree.

Derived configurations maintain the same values and properties of the parent config unless you break the link to the child (derived) config by explicitly changing a value in the child config. For all other configurable items, the child config value changes when the parent config value changes.

One very nice application of derived configs is to use them for simplified configurations and to set the properties so that any features added to the parent config are also added to the derived config. You can do this by deselecting the Advanced Option Suppress Features (turn it off) in the PropertyManager for the configuration. This causes the derived config to inherit only features that are added to the parent, not to other configs. You can use the simplified configs for Finite Element Analysis (FEA), making drawings of models where all the edge breaks have actually been modeled, or simplified large assemblies. You can also use them for the reverse (a complex config rather than a simple one) to have a config that includes fillets for rendering purposes that are otherwise not used in the manufacturing or documentation processes. In addition, you can create and maintain derived configs using design tables, which are discussed in the next section.

Understanding How File Size Affects Speed

A long-standing dispute has raged over the effects of file size on speed. Here are the facts: When SolidWorks creates a configuration, it can store information about the 3D geometry and a preview thumbnail of the configuration inside the part file. While this is not the default (sometimes only the active configuration data is saved), it can make it faster to access the configuration the next time because it has only to read the stored display data, rather than read parameters and then recalculate new display data. As a result, saving the stored data makes the file larger but also enables you to avoid recalculating.

Many people assign more importance to file size than I do, and they use it as a criterion on which to base decisions about which features or techniques to use or not use. If I have a choice between using a single file instead of multiple files by using configurations, I prefer the single-file technique, even though it is guaranteed to produce larger files—and in some cases, much larger files. This is true especially when the choice is between larger files or longer calculation time. Libraries of parts can often be made more manageable by using configured parts rather than many individual parts. Storage space is cheaper and easier to upgrade than processors. In the end, reading stored data rather than recalculating it is faster, hence cheaper. This is why when SolidWorks can store data that will probably be needed again at some point, it’s a good idea to take advantage of the storage. It is useful to take advantage of the single-file technique. Storage space is cheaper than rebuild time. The result is that configurations definitely increase file size. While SolidWorks never loads all of the data by default, larger files take longer to open, save, move, and perform just about any operation.

Fortunately, SolidWorks can work with very large data sets. There are a couple of options that can tip the balance in your favor between saved data and recalculated data. In the ConfigurationManager, right-click the name of the part and select Add Rebuild On Save Mark. Figure 11.14 shows the options available.

Add Mark For This Configuration means that a Rebuild On Save Mark will be added to the current configuration. The next time the part is saved, that configuration (the active one) will be rebuilt and the data saved.

Add Mark For All Configurations will force the software to rebuild and update all configurations the next time the part is saved. Be aware of the time required for an operation like this. It will vary depending on the complexity of your part (the number of features versus the number of configurations).

Add Mark For Specified Configurations presents you with a dialog box to select which configurations to rebuild and for which to save data.

Remove Mark And Purge Data For All Configurations reduces the size of the file by purging all the configuration data. This is great for file size, but it has an adverse effect on performance when SolidWorks must rebuild configurations.

These four options give you the choice of and control over what is important to you. Figure 11.15 shows what happens when you just right-click on a specific configuration. Notice that some of the configs have a floppy disk symbol. These individual configurations have been marked to be rebuilt and saved. The RMB menu shown reflects that the selected configuration is currently marked with the disk symbol, but it can be unmarked.

To use these options on a larger scale, a new system option purges all cached configuration data. You can find this setting at Tools ➢ Options ➢ Performance ➢ Purge Cached Configuration Data.

Controlling Dimensions

Controlling dimensions with configurations is simple. You need only three things to start: one dimension and two configurations. Because you already know how to create these elements, you are ready to start. Configurations require that you spend some time developing “design intent” for parts. Configurations drive changes in models; if they are properly modeled, you can avoid feature or sketch failures due to dimension changes—or at least you can understand the limits that each dimension needs to remain within.

I will start with the example of a simple block. A fully dimensioned block has three dimensions. Make sure that you have manually created at least two configurations. Double-clicking a model face opens all the dimensions, and double-clicking one of the dimensions opens the familiar Modify dialog box. Figure 11.7 shows that there is a small difference in the Modify dialog box. It now has a drop-down list where you can specify whether this change applies only to this config, to all configs, or to specified configs. If you select specified configs, then a dialog box listing the existing configurations will allow you to select which configurations get the change.

After you're finished, you can toggle back and forth between the configs by double-clicking each of the configs in the ConfigurationManager. Although this is simple, if you forget to change the drop-down list from the All Configurations setting to either the This Configuration or the Specify Configurations setting, you will apply the change to all the configurations. Building a configuration manually is fine for a few simple changes, but it can become unwieldy if you are changing more than a few dimensions or handling only a few configurations in this way. You would then have to remember which dimensions were changed to what in which configurations. As you can see, using design tables is a better method for multiple dimensions.

Controlling Suppression

Suppressing a feature is just like turning it off; the feature appears as grayed-out text in the FeatureManager. With configurations, you can suppress a feature in one config and unsuppress it in another. Also, while a feature may be suppressed, the sketch associated with it is not necessarily suppressed. When you're dealing with manual configuration techniques, there are two methods for controlling suppression: manually suppressing features and creating configurations with the appropriate options for the inclusion of new features, which I discussed previously in this chapter.

In addition to the Suppress toolbar button, you can also use the Unsuppress and Unsuppress With Dependents functions. When you suppress a feature, any feature that is dependent on it is also suppressed. If you then use the Unsuppress feature, it unsuppresses only the feature itself. However, Unsuppress With Dependents brings back all the dependent features as well.

Generally, SolidWorks users employ a combination of these methods, mainly because configurations are not usually started on a complete model; they are often added when the model is still in progress, so features are added after the users create the configurations.

On the left side of Figure 11.16, you can see a feature that is alternately unsuppressed and suppressed in the tree. The text and icon for the suppressed feature are grayed out. You can suppress features from the RMB menu on the feature, from the Edit menu, or through a tool on a toolbar. The Suppress button is not on a toolbar by default, but you can find it in the Commands dialog box (Tools ➢ Customize ➢ Commands), along with the other buttons for the Features toolbar. Only the Edit menu offers the options of Unsuppress With Dependents and This Configuration, All Configurations, Specify Configurations options for each of the Suppress, Unsuppress, Unsuppress With Dependents functions.

Using Unsuppress With Dependents can save you lots of time or the hassle of looking for all the features dependent upon a feature that has been suppressed. Because it is not available on the RMB menus, this function is used less than it might otherwise be.

You may also need more control than the use of the simple suppress and unsuppress features. All three options (Suppress, Unsuppress, and Unsuppress With Dependents) have three options: This Configuration, All Configurations, and Specified Configurations. This is a case where the drop-down menu options (Edit ➢ Suppress) offer more detailed functionality than you can find in the RMB menus.

Controlling Custom Properties

Several reasons may compel you to use custom properties, including integration with searches for a Product Data Management system, automatically filling out drawing title blocks, or adding information to the BOM.

When you use custom properties with configurations, you must use the Configuration Specific Custom Properties interface (or an appropriately configured custom property tab or the Modify Configurations dialog box), which enables you to have custom properties that change with each configuration. Standard custom properties apply to the top-level part and keep the same value for all configurations. The configuration-specific functionality is useful for situations such as different part numbers for configurations and many other situations that are limited mostly by your use of configs. The Custom tab of the Summary Information dialog box still applies custom properties that do not change with the configurations to the part.

The interface for managing custom properties manually is shown in Figure 11.17. You can access this dialog box by choosing File ➢ Properties from the menu.

You can also link custom properties to mass properties, model dimensions, link values, sketch text, and global variables by selecting from the drop-down list under the Value/Text Expression column, which appears when you select a cell in the column. To link a custom property to a model dimension, simply activate the Value/Text Expression box in the Summary Information interface that you want to populate and click a dimension in the graphics window. Again, managing this data for a single config or only a few configs is easy enough; however, it can quickly become unwieldy, which is where using design tables can make a huge difference.

Controlling Sketch Relations

You can individually suppress or unsuppress sketch relations using configurations. Figure 11.18 shows the Display/Delete Relations PropertyManager interface, at the bottom of which is the Configurations panel. To suppress a relation, select it from the list and select the Suppressed option in the Relations section above the Delete buttons.

Remember that Display/Delete Relations can be located through the menus at Tools ➢ Relations ➢ Display/Delete, or by double-clicking a sketch relation symbol within a sketch.

Controlling Sketch Planes

You can configure the Offset distance in the From option for extrudes, and you can configure the sketch plane for the sketch that is used in the feature. The Sketch Plane PropertyManager interface expands when configurations are present, as shown in Figure 11.19. To access the Sketch Plane PropertyManager, right-click on a closed sketch and select the Edit Sketch Plane option.

Controlling Configurations of Inserted Parts

Inserted parts may also be called derived or base parts. However, both of these terms are obsolete. Inserted parts are discussed in detail in Chapter 31, “Modeling Multibodies,” and Chapter 33, “Employing Master Model Techniques”.

Inserted parts place the features for one part inside another part. The inserted part becomes a feature in the FeatureManager of the child part. You can insert just the body geometry itself, or you can bring forward reference geometry, sketch data, features, and configuration-specific custom properties and break the link to the original part if you like.

The role of configurations with inserted parts is that the configuration of the inserted part can be controlled from the child component. For example, you may have designed an engine block for an automobile. This engine block is a casting, and using configurations, you have both the six-cylinder and the eight-cylinder blocks in a single-part file. This model represents the “as-cast” engine block. The next step is to make the block with all the secondary machining operations, such as facing mating surfaces, boring cylinders, drilling and tapping holes for threaded connections, and so on. As a result, the as-cast part is inserted into the as-machined part, and the configuration is selected before you add the cut features. As the name suggests, you add inserted parts by choosing Insert ➢ Part from the menu.

The interface for assigning the configuration is shown in Figure 11.20. Simply right-click the inserted part feature, and select List External References. It would seem to make more sense if the configuration could be selected when the part is first inserted, but it does not work this way; you must select the configuration after the part is inserted.

Using Library Features

Library features can have configurations, and they carry those configurations with them into the part in which they are placed. Unfortunately, part configs cannot reference different library-feature configs. Although library features can be configured, after you drop them into a part and click OK, the configurations will no longer be accessible (unless you have selected Link To Library Part), so a part's configurations cannot select the configuration of a library feature. A part's configurations can change the dimensions of a library feature.

Configurations for library features are created in exactly the same ways that configurations are created for other parts. The technique for saving the configs to the library feature is discussed in Chapter 18, “Using Libraries, Assembly Features, and Hole Wizard.”

Identifying What Can Be Driven by a Design Table

Just because something can be configured does not necessarily mean that it can also be driven by a design table. Here is a small list of items that fit into this category:

• Sketch plane configuration
• Suppressed sketch relations
• Suppressed dimensions (Suppressed dimensions become driven dimensions.)

However, the good news is that many items can be driven by a design table. Table 11.1 lists these items, along with their associated syntax. For the most up-to-date list, check the SolidWorks Help documentation.

Editing Design Table Settings

Figure 11.22 shows the PropertyManager for design tables. After you have created the table, you can edit the table settings by right-clicking the table and selecting Edit Feature. Edit Feature enables you to edit the settings for the table only; it does not enable you to edit values within the table.

• Linked Design Table By selecting the From File source option, you can create a design table from an external file; you can also link the table to the external file. When you use the other two options, Blank and Auto-Create, SolidWorks stores the Excel file within the SolidWorks document. Linking to an external file may be useful if you have a non-SolidWorks user who is entering data into the design table or if a single table controls multiple parts.
• Edit Control The Edit Control panel has two options, which act as a toggle. The Allow Model Edits To Update The Design Table option is self-explanatory, as is its opposite, the Block Model Edits That Would Update The Design Table option. If the Allow Model Edits option is selected and you make a manual change to the model, the next time you open the design table, SolidWorks will warn you about the change and that it will update the design table. Likewise, if you try to make a manual change and the Block Model Edits option is selected, you will receive a warning that the value cannot be changed.
• Options The Options settings determine the behavior when you are using the Allow Model Edits option and a new item has been configured. For example, the design table may already exist, and you manually add a configuration and suppress a feature.

Configurations that have been added manually are displayed somewhat differently from configs that are being managed by the design table. Figure 11.26 shows the two configurations at the bottom of the tree with square symbols, while the design table configs have X (Excel) symbols.

After you manually add the config and suppress the feature, the next time you open the design table, the Add Rows And Columns dialog box appears. Many users are simply annoyed by this, but that may be because they don't understand what it does or why it appears. In the example shown in Figure 11.27, a new configuration has been manually added; it appears in the Configurations box as ManuallyAddedConfig, and in the Parameters box, it looks like a feature named BodyChamfer has been either suppressed or unsuppressed manually. The appearance of this dialog box means that SolidWorks is asking if you want to include these items in the design table. If so, simply select the items you want to add to the design table and click OK. If you do not want to include the items in the design table, simply click OK or Cancel. If you click OK, you will not be offered these choices again; if you click Cancel, the next time you open the table, the dialog box with the same choices will reappear. If you never want to see this dialog box again, make sure that all the options in the Options panel shown in Figure 11.22 are deselected.

Editing the Design Table

As I mentioned earlier, working with a design table opened inside the SolidWorks window can sometimes be difficult. One way to handle this problem is to edit the design table inside SolidWorks only when you want to add new features to the column headers; when adding new configurations or editing the field values, edit the table in a separate window. This option appears on the RMB menu as Edit Table In New Window. It gives you much more flexibility in resizing the Excel window, changing the zoom scale, and other operations, but it doesn't enable you to double-click a dimension so it is added automatically to the column header.