You can save display configurations of an assembly and exploded views of an assembly. When you save a display configuration with the Display Configurations command, the current display status is stored so you can use it later.
Note:
Display configurations store both the show/hide and the simplified/designed status of the parts in the assembly.
For example, if you hide several parts in an assembly, you can save the display configuration to a name you define. Later, if you want to quickly hide the same parts, you can apply the display configuration using the Configuration drop list on the Home tab in the Configurations group. You can also save, apply, edit, and delete display configurations using the Display Configurations dialog box.
You can also apply a saved display configuration when doing the following:
Opening an assembly document
Placing a subassembly in another assembly
Creating a drawing of an assembly
Creating a drawing of an exploded assembly
Display configurations are stored in a document that has the same name as the assembly document, but with a (.CFG) extension. The configuration document is stored in the same folder as the assembly document.
Note:
To support concurrent design, the configuration file allows multiple users to simultaneously add, delete, and edit display configurations.
Both assembly configurations and exploded view configurations are saved to the same configuration file. To use display configurations effectively, your company should define a naming convention so all users can easily distinguish between types of configurations.
Note:
You should avoid using special characters in configuration names. For example, special characters such as \ / : ! are not allowed.
You can apply an assembly configuration to an exploded view to control the show/hide status of the parts and subassemblies. You cannot apply an exploded view configuration to a regular assembly window. For this reason, configuration names of exploded views are not displayed in the Configuration list on the Home tab when you are working in a regular assembly window.
When working with large assemblies, you can open the document faster if you use a display configuration where some parts and subassemblies were hidden or where simplified versions of the parts were defined. To apply a display configuration when you open an assembly, use the Configuration list on the Open File dialog box.
You can select an assembly configuration name in the Use Configurations dialog box when placing a subassembly into an assembly. Subassemblies will place faster and can be easier to visualize if you apply a configuration where parts not necessary for placement are hidden. Exploded view configuration names are not displayed in the configuration list on the Use Configurations dialog box.
To use a display configuration when placing a subassembly, you must first set the Use Configurations command on the Parts Library shortcut menu. When you set this option and then drag and drop a subassembly into the assembly, the Use Configuration dialog box is displayed so you can select the configuration name you want to use.
There are many ways you can use display configurations in the Draft environment.
You can use both assembly and exploded view configurations when creating drawings in the Draft environment. When you use the Drawing View Wizard command and choose an assembly document from the Select Model dialog box, you also can select an assembly configuration or an exploded view configuration. When you select either configuration type, the drawing view is placed with the parts displayed or hidden as they were when the configuration was saved.
You can control the display of weld beads and material addition features in an assembly drawing view. For example, you can hide the display of weld beads and material addition features, and then save a display configuration. You can then use the display configuration to place a drawing view of the assembly with these features hidden.
You can reduce complexity in a drawing view. For example, you can display tube, pipe, or frame centerlines without displaying the solid bodies of the tubes, pipes, or frames. Use the Show/Hide All Components command to Show All of the centerlines and Hide All of the design bodies in the assembly model before you create the display configuration file.
In the Draft document, you can then use the Include reference, sketch, and construction items check box in either of the following locations:
On the General tab (Solid Edge Options dialog box), you can define a document level preference.
On the Display tab (Drawing View Properties dialog box), you can override individual show and hide settings for design bodies and centerlines.
Display configurations are available when working with alternate assemblies. The behavior of display configurations based on whether you specify that the alternate assembly is a family of assemblies or an alternate position assembly.
For a family of assemblies, a display configuration is member-specific. In other words, the family of assembly member which is active when you create the display configuration is the only member in which you can use the display configuration later. The Configuration list on the Home tab filters the available display configurations automatically.
For alternate position assemblies, display configurations are not member-specific. In other words, you can use any display configuration for any active member. The Configuration list on the Home tab displays all the display configurations.
The functionality of zones and display configurations differ in a number of ways. For more information, see the Comparing display configuration and zones section of the Displaying parts in assemblies Help topic.