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The gap refers to the gap between the break lines in the finished broken view. The setting here overrides the default for this view only. The default setting is a template setting found in Tools⇒Options⇒Document Properties⇒Detailing. Other options that you can set in this location are the break line extension (the distance the lines extend past the model edges) and the break line font (on the Line Font page of the Document Properties tab). The setting that enables the broken symbol on a dimension is found on the Dimensions page and is named Show Dimensions As Broken In Broken Views.

FIGURE 15.22

Selecting the break symbol

You can remove individual breaks in a broken view by selecting one of the break lines and pressing Delete. You can add breaks by applying the Break command and adding more breaks to a view. You can alter breaks by simply dragging the break lines. In past versions, it was possible to get the view very confused by dragging one set of breaks to interfere with another set of breaks. That problem has been fixed by not allowing break lines to be dragged past one another.

Broken views enable you to dimension the break lines themselves so that when the model changes, you can control the location of the break lines relative to part geometry.

Consider using the Unbreak option from the RMB menu to temporarily unbreak a view to make dimensioning more convenient.

Using an Auxiliary View

An Auxiliary View is a view that is projected from a non-orthogonal edge. This type of view is often necessary to view features (such as holes drilled at an angle) square on, so that they appear circular in the view rather than foreshortened and elliptical. An Auxiliary View is shown in Figure 15.23 in the image to the left. If the edge that the view was created from is updated, then the Auxiliary View will reorient itself. The image to the right shows an Auxiliary View projected from an arbitrarily drawn sketch line. The line or edge used to project an Auxiliary View cannot be reselected; however, if a sketch is used to project the view, then the Edit Sketch option is available through the view arrow RMB menu.

FIGURE 15.23

Two Auxiliary Views

Using an Alternate Position View

While assemblies are dealt with in detail in the SolidWorks 2011 Assemblies Bible (Wiley, 2011), this assembly-only view type is introduced here only to offer all of the drawing view types in a single location. (Additional information on this and other assembly functionality is located in the above referenced book.) The Alternate Position View is only available for views of an assembly and shows the assembly in two different positions (not from different viewpoints; this requires an assembly that moves). This is another view type that does not create a new view but alters an existing view. Figure 15.24 shows the PropertyManager interface for the Alternate Position View, a sample view that it creates, and the way that it is represented in the drawing FeatureManager.

FIGURE 15.24

The Alternate Position View

To create an Alternate Position View, ensure that you have an assembly on the active drawing that can have multiple positions, and click the Alternate Position View button from the Drawings toolbar, or choose Insert⇒Drawing View⇒Alternate Position and then select the Alternate Position View.

Next, click in the drawing view to which you want to add the alternate position. The PropertyManager shown in Figure 15.24 prompts you to select an existing configuration for the alternate position or to create a new configuration. If you choose to create a new config, then the model window appears, a new config is created, and you are required to reposition the assembly. The alternate position is shown in a different line font on the same view, from the same orientation as the original.

Tip

The best way to create this view is to either create two configurations used exclusively for the Alternate Position View or to have two configurations where you know that parts will not be moved, suppressed, or hidden. The main idea is that you need to ensure