Display States in SolidWorks14 Mar, 2011 By: Scott Slovik
Solid Thinking Tutorial: What are display states, and how can you use them with parts and assemblies?
Editor's note: This tutorial courtesy of SolidWorks.
Experienced SolidWorks users know that configurations are a key component of the software. A few years back, SolidWorks added functionality called display states to help users improve efficiency and better manage their designs.
The main difference between a display state and a configuration is that a display state only controls changes in graphical information, whereas a configuration can control dimensional changes and the suppression state of features and parts. Display states can add or remove appearances on faces, features, bodies, or entire parts. This can be very useful by highlighting important faces for special manufacturing operations, or documenting post-manufacturing operations like painting or powder coating. Display states can hide or show multiple bodies or parts within assemblies, and you can change the display mode of those bodies or parts. (Display mode is the option of shaded with edges, shaded, HLR, HLV, or wireframe.) Additionally, you can control the transparency of any specific feature, body, or part model you select.
It's important to note that every new part or assembly in SolidWorks starts with a single display state called Display State-1. By default, SolidWorks will link display states to the configuration you're active in, which means Display State-1 is linked to the Default configuration. If you add another configuration, SolidWorks automatically adds a new display state linked to your new configuration. In the Configuration Manager tab, SolidWorks gives you an option to unlink display states from configurations. This allows any configuration you create to use any display state in that file. This option to link display states is not permanent; it can be turned on or off at any time.
Why Are Display States Important?
In addition to simply displaying your 3D models in different ways, display states can help you improve performance and create 2D drawings faster. Since display states still load the feature history information into your system RAM, changing the graphical display will help reduce the load on your graphics card. This is especially important if you work with large assemblies and use an entry-level or midrange graphics card in your laptop or workstation. (I like to hide all my toolbox hardware in large assemblies using a display state.) In 2D drawings, it can take time to create just the right views, which show only the parts that are necessary in each view. By using display states when creating the 3D assembly, you will have easy access to change the 2D view to show just the parts you intended. Simply select the display state from the Drawing View property manager, as shown below.
Create a Display State
You can create a new display state several ways. If you want to add a new display state, simply go to the Configuration Manager tab, then to RMB in the Display States section, and pick Add Display State. (As a general rule of thumb, you should always add a new display state first, before you make any graphical changes — otherwise you will have just modified your active display state.)
The second method for creating a display state is my favorite. I use the Isolate command in assemblies quite often to focus my effort on only the parts I want to see. (It's the quickest way to hide everything I'm not working on.) In the Isolate toolbar that pops up, you get an option to save the current view as a new display state (see the image below). Once you exit out of the Isolate command, all the hidden parts will come back.
But if you remembered to save the isolated view as a display state, you can see it listed in the Configuration Manager, or activate it from a RMB on the double arrows at the top of the Feature Manager tree.
A third method to add a display state is a new enhancement in SolidWorks 2011. You now have the ability to save your Assembly Visualization view as a display state. The Assembly Visualization tab in the Feature Manager design tree allows you to list all of the components in an assembly, and sort them by file name, quantity, or any custom property you have in the file.
When you click on the color bar in the Assembly Visualization tree, SolidWorks will automatically assign colors to your parts. You can add, delete, or change the assigned colors, and even group identical parts, all from an RMB click by the color bar. This is very useful to graphically sort parts by weight, cost, owner, revision, PDM workflow state, etc.
The last method to create a display state is to simply RMB on an existing display state, regardless of whether it's active or not, and copy it. Unfortunately, SolidWorks doesn't list a paste option from an RMB, but you can always use the standard Microsoft Windows Ctrl + V shortcut to paste, then make your changes. If you want to rename a display state, RMB-click on its name and choose Properties.
One Last Tip
If you want to hide or show parts, but do not want to go back to each display state and modify, here a quick trick. Just like with configurations, simply select the parts you want to change, then go to the Edit menu and choose Hide or Show in Specified Display States.
This will save you a great deal of time if you have many display states that need to be updated!