Glenn Schroeder

How can I show a single body of a multi-body Part in a Drawing?

Blog Post created by Glenn Schroeder on Dec 23, 2017

As with most things with SolidWorks, there are several ways to do this.  Select the one that works best for you.


I'll start with what I believe is the simplest, and the one I almost always use (I like simple).  When you've selected the model to insert in the drawing, go to the "Select Bodies..." button in the drawing view's property manager.



That will take you to the Part file where you can select which body, or combination of bodies, you want to show in the drawing view.  You can also use this feature to add or remove bodies from existing drawing views, not just when creating new ones.


Another method is to insert the drawing view, then right-click on an edge of a body you want to hide and choose Show/Hide > Hide Body.  If you want to get it back just find the body in the tree and right-click on it.  There will be an option in the menu to show it again.



A third option is to save out the bodies as separate Part files by right-clicking on the body and choosing "Insert into New Part..." from the drop-down.  A number of people use this method, but I don't think I've ever had a reason or need to.  If you have to have a separate Drawing for each body because of company standards then you should likely use this method, especially if you have title block notes that are driven by the Part's custom properties.  Unfortunately, at this time title block notes can't be driven by cut list properties. 



Still another option would be to create multiple Display States in your Part, hiding bodies in each as needed, and then reference the appropriate Display State in the Drawing.


Remember I said there are multiple ways to do most things in SolidWorks?  Here's the 5th.  Go ahead and insert a view, then right-click on it and choose Drawing Views > Relative View.



That will take you to the model, where you can choose which faces (or Planes) you want front and right, and you will also have an option to choose which body or bodies you want included in the view.  When you click OK in your model it will place a new drawing view oriented according to your selections.  You can now delete the original view if it's not needed.  Relative View was one method commonly used for showing selected bodies before the Select Bodies... button shown above was added.  I've rarely used it since then, but if you have a body at a weird angle, such as a brace, it can be very useful.