Chapter 21: Working with Drawing Views
- Click any spot inside the sheet and press Ctrl+V. SolidWorks pastes the copied view
from the other sheet. Delete the section line. You may also need to delete the sketch lines
separately.
- Click the Projected View tool from the Drawings toolbar, and then click the pasted
view. Practice making a couple of projected views, including dragging one off at a
45-degree angle to make an isometric. Make sure that one of the views is a side view
showing the angled edge, as shown in Figure 21.36. Once you create the views, click
model edges in the views and drag them around to a better location.
FIGURE 21.36
Projecting views
Create at least one of these views
- Select the angled edge from one of the side views and click the Auxiliary View tool-
bar button. While placing the view, press and hold the Ctrl key to break the alignment.
You can resize the view arrow by selecting the corners and dragging. If you drag the line
itself, then you can move it between the views. Alternatively, with the view arrow selected
and the PropertyManager displayed, you can deselect the green check mark icon in the
Arrow panel at the top of the window to turn off the arrow.
- Create a new drawing from the New dialog box. Select a template without predefined
views on it, so the Inch B Bible Template (no Views).drwdot will work. If you select a
default SolidWorks template, you need to verify that the template uses thrid-angle rather
than first-angle projection. An easy way to do this is to switch the drafting standard from
ISO to ANSI in Tools ➪ Options ➪ Document Properties ➪ Drafting Standard. If the auto-
matic Model View interface appears in the PropertyManager, click the red X icon to can-
cel out of it.
