Part V: Creating Drawings
Open documents
The large selection box in the Part/Assembly to Insert panel displays any models that are open in
SolidWorks at the moment. If the model that you are looking for is not in the list, then you can use
the Browse button to look for it.
I typically use Create Drawing From This Part/Assembly if the part is open, and if not, I drag-and-
drop the part onto a new drawing created from a template with Predefined and projected views on
it. This combination saves a lot of extra steps.
If you click in the drawing window for some reason (for example, if you are expecting it to simply
place a view), then a prompt appears, stating that you have selected a drawing document, and that
only parts and assemblies can be inserted into drawings.
Thumbnail Preview
This is a nice option that shows the part that you selected in the Open Documents window. It is a
useful feature, but because it is collapsed by default, it is easy to miss. After it is used the first time,
it remembers the expanded setting.
Start Command When Creating New Drawing Option
The Start Command When Creating New Drawing option causes this PropertyManager to open
immediately when a new drawing is created. If you click in the drawing window, then the prompt
appears, telling you that you are not paying attention.
Reference Configuration
The Reference Configuration list enables you to select which configuration of the part to show in
the view. This shows up not only when creating new views, but also in the generic Drawing View
PropertyManager that shows up when you select any view.
Select Bodies
When a part has multiple bodies, a button called Select Bodies also shows up in this panel. If the
part does not have multiple bodies, you will not see this button, When you click the button, it
immediately takes you out to another PropertyManager, the smaller one shown in Figure 21.3
called Drawing View Bodies, where you are sent back to the model window to select a body.
Clicking the green check after selecting a solid body in Drawing View Bodies then sends you back
to the drawing to place the view. It does not send you back to the Model View PropertyManager.
If you click the red X in the Drawing View Bodies PropertyManager, SolidWorks leaves you in the
part window, and you will have to press Ctrl+Tab to get back to the drawing window.
Cosmetic thread display
Many people see the High and Draft quality options and assume that the option refers to the qual-
ity of the view, while in fact it refers to the quality of the cosmetic thread display. Cosmetic threads
can display in either high or draft quality. The distinction is made for performance reasons. The
