Combine Display States In SolidWorks

SolidWorks has the power to display your models, assemblies and drawings in a number of different ways (or display states in SolidWorks speak). Each display state has it’s own application, for example a shaded view is great for 3D modelling because you can see the surfaces of the part your building where as a view with hidden lines removed is great for a drawing because it de-clutters displaying only the most important information. However, there are certain circumstances where you may wish to combine two different display states together; have you ever wanted to show a translucent part of a model or perhaps wanted a decal to be visible in a drawing with hidden lines removed? This tutorial will show you exactly how that’s done.

In this example, we have a simple sheet metal box with the material 1060 Alloy assigned to it and a Perspex window covering the aperture at the top of it. I have also applied a decal to the bottom right corner of the window:

Screenshot Of SolidWorks Window - Tutorial To Change Display States In SolidWorks

If you tried to make a drawing of this component as it is and needed it to display with hidden lines removed then you’d end up with something like this:

Drawing Screenshot In SolidWorks - Tutorial To Change Display States In SolidWorks

In most circumstances this would be fine; this may be the level of detail needed or you might only need to add a cut out section to show a small detail inside the box. But what if you wanted to show what was inside the box through the Perspex window at the top or you wanted the decal to be visible too? You could always make change the display state of your model to shaded within the drawing, but you would end up with a page like this:

Drawing View Shaded - Tutorial To Change Display States In SolidWorks

Here’s where having the ability to combine display states comes in handy. To do this, you’ll need to add a new display state from within the part or assembly. Go to the configuration tab on your FeatureManager and right click the Display States pane at the bottom. You can then click ‘Add Display State':

Add Display State - Tutorial To Change Display States In SolidWorks

A new display state will appear, which you can re-name by right clicking it and selecting properties. In this case I’ve renamed it ‘Drawing Display State':

Rename Display State - Tutorial To Change Display States In SolidWorks

With your new display state activated, return to the feature tree tab and expand the view pane by clicking on the chevron in the top right corner of the FeatureManager, then expand the the bodies, surface bodies or cut list folder to see the individual elements which make up your model:

Expand Display Pane

You can now set the components you need to be displayed as hidden lines removed and in shaded mode by clicking on the display state icon in the middle of the view pane. In this case, I have set the sheet metal box to show up with hidden lines removed and the Perspex window to be shaded:

Activate Hidden Lines Removed - Tutorial To Change Display States In SolidWorks

Hopefully you can now see where this is going, the Perspex window remains transparent but the sheet metal box is displayed in a non shaded, hidden lines removed state. You may think that the Perspex window looks a bit murky, so we’ll fix that problem next. All I did was to edit the appearance of the Perspex window and set it’s transparency to 1.0 – this step is optional but it does assist with the overall effect:

Set Transparency

Now we can return to the drawing and activate our newly created display state. Simply select the master drawing view (or individual views depending on how your drawing is set up), then under display states select the newly created ‘Drawing Display State’. This final step may seem slightly strange, but you’ll need to set the overall display state of the view to shaded with edges:

Set Display State In Drawing - Tutorial To Change Display States In SolidWorks

Now, with any luck, your drawing should look something along these lines. The components which need to be transparent are transparent, the decals are visible and the rest of the view is displayed with hidden lines removed:

Final Drawing - Tutorial To Change Display States In SolidWorks

If you’d like to view the files used to demonstrate technique, I have them here to download. They are in SolidWorks 2013 format so you will need SolidWorks 2013 SP0.0 or higher to view them (however the files will open in SolidWorks 2012 in interop mode). The key things to look at in these files are the different display states in the .SLDPRT file and the drawing view settings in the .SLDDRW file.


5 Comments

  1. Edward, excellent tutorial. This is exactly what I was looking to do.

  2. This will save you a great deal of time if you have many display states that need to be updated!

  3. Thanks for sharing superb informations. Your web site is very cool. I’m impressed by the details that you’ve on this blog. It reveals how nicely you understand this subject. Bookmarked this web page, will come back for extra articles. You, my pal, ROCK! I found simply the info I already searched all over the place and just could not come across. What a perfect site.

  4. You can manually create a Display State or create one while in the Isolate command (just press the blue disk icon). Display States honor Display Modes too, so that you can create an image with some parts shown with hidden lines removed, for instance.

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