SolidWorks 2010 Bible

Chapter 4: Creating Simple Parts, Assemblies, and Drawings

12. You need to place two more screws in the assembly, but these cannot be automati-
    cally mated; you need to do this manually. Copy two instances of the screws. To copy
    a screw, Ctrl+drag the part either from the graphics window or from the FeatureManager
    and drop it into the graphics window.


13. Position the part and the view so that you can see the cylindrical body of the screw
    and the cylindrical face of the threaded hole in the C-channel. With the Mate function
    active, select both faces and click OK. Repeat the process for the other screw and hole.


14. Now click the underside of the screw head and the counterbored surface of the slot,
    making sure they will be coincident, and click OK. Repeat the process for the other
    screw.


15. Save and close the assembly.

This is a quick overview of the basic assemblies’ functionality, which is expanded on in later

chapters.

Tutorial: Making a Simple Drawing

If you are coming to SolidWorks from a dedicated 2D software, you will be creating drawings very

differently from what you may be used to. In 2D software, you draw each view individually, and

when a change occurs, you have to go back through the views and ensure that each view is

updated appropriately. In 2D, views are sometimes created sparingly because they are difficult to

create and to update. This includes view types such as Isometric views, complex sections, and

views projected at non-orthogonal angles.

In SolidWorks, drawing views are almost free, because they are simply projected from the 3D

model. Updates are made in the 3D model, and all views update automatically from there. You can

handle dimensions in a couple of ways, either using the dimensions that you used to create the

model, or placing new dimensions on the drawing (best practice for modeling is not necessarily the

same as best practice for manufacturing drawings). To make a simple drawing, follow these steps:

1. Click the New button from the Standard toolbar or choose File ➪ New. From the
   New SolidWorks Document window, select the Drawing template. The template contains
   all the document-specific settings.


2. After selecting the drawing template, the Sheet Format/Size dialog box appears, as
   shown in Figure 4.22. Select the D-Landscape sheet size, as well as the format that auto-
   matically associates with that sheet size, and click OK. If the Model View
   PropertyManager appears, click the red X icon to exit.


3. Before creating any views on the drawing, set up some fields in the format to be
   filled out automatically when you bring the part into the drawing. Right-click any-
   where on the drawing sheet (on the paper), and select Edit Sheet Format.