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Chapter 15: Working with Drawing Views

In This Chapter

Using common view types

Exploring other view types

Assigning hotkeys to View items

Sketching in a view versus sketching on a sheet

Working with view types, settings, and options tutorial

In SolidWorks drawings you do not create lines to create views. The drawing view is a snapshot of the 3D model from a particular point of view. To change the lines on the view, you have to change the 3D model; you do not just move lines around the view.

If you are coming from AutoCAD, this might seem a little bit confining. However, this method will become liberating rather than confining. It means that you do not have to worry about the drawing views being inconsistent or incorrect. All you have to worry about is the 3D model being correct.

SolidWorks automatically maintains the views better than you could do it manually. It can update any type of view from any point of view of even the most complex model or assembly geometry perfectly.

Creating Common View Types

The previous chapter discussed Pre-defined Views in templates. Pre-defined Views make it faster to automatically create drawings with consistently placed, simple views. However, sometimes you may need to create views on templates that do not have Pre-defined Views, or you may need a special arrangement of views. SolidWorks has a good assortment of view types to make practically any type of view that you may need.

Note

When creating or changing either the geometry or the settings that control how a view is displayed, the view may become cross-hatched, indicating that the model needs to be rebuilt. To resolve this problem, press Ctrl+B to rebuild the drawing.

Using the View palette

The View palette is shown in Figure 15.1. It is activated automatically if you use the Make Drawing From Part tool, unless the drawing template that you select has Pre-defined Views on it. In this case, the Pre-defined Views are populated and the View palette is not activated.

FIGURE 15.1

The View palette

The View palette contains all the standard named views, the current view of the model, custom named views, and any annotation views (views that the model was in when annotations were added to it). You can drag-and-drop these views on the drawing.

If multiple parts are available, they are listed in the drop-down list at the top of the panel. You can also browse, refresh, or cancel out of the view from this same area.

To activate the View palette without using the Make Drawing From Part tool, simply create a new drawing document, ensure that the Task Pane is available, and click the View Palette tab in the Task Pane. Then use the ellipsis button (...) to browse to a part. After you select a part, the palette window is populated with views of the model. This method has the advantage of enabling you to see the views before you put them down. It does not link views in the same way that the Predefined and projected views are linked, however. I find this interface somewhat difficult to use, and prefer to set up the Pre-defined Views in templates or to use the Multiple Views option in the Model Views PropertyManager, which is shown later in this chapter.

Using Model Views

Model Views are one of the few types of views that are not dependent on another view. Everything has to start from somewhere, and most drawings have to start with either a named or Pre-defined View. A Model View starts from a named view in the model.

You can place named views by clicking the Model View button on the Drawings toolbar or by choosing Insert⇒Drawing View⇒Model. Using the Model View PropertyManager is a two-step process, and is shown in Figure 15.2. In the first step, you select the model, and in the second step, you set the options for the view. Views dragged from the View palette are also Model Views.

FIGURE 15.2

The Model View PropertyManager

The Model View PropertyManager has seen several changes in SolidWorks