SolidWorks 2011 Parts Bible - Matt Lombard [211]
Display State
On the drawing you can now select the Display State. This is probably meant for situations like using Display States for hide and show operations, but remember that there is a lot more to Display States than just hide and show. You can also change display styles and colors, and transparency, which you might think do not have any place on a technical drawing.
Display Style
You can set the default Display Style by choosing Tools⇒Options⇒System Options⇒Drawings⇒Display Style. This panel provides an override for views being placed. This panel also enables you to control High or Draft quality views, which are described later in this chapter.
Scale
SolidWorks drawings always default to showing views at the overall sheet scale unless the System Option on the Drawings page called Automatically Scale New Drawing Views is selected. If this setting is selected, the sheet scale saved with the drawing template is overridden. For example, a 1:1 sheet scale can be changed automatically by the setting to 1:4.
You can change the sheet scale through the sheet properties, which were discussed in Chapter 14. Controlling views with the sheet scale makes it much easier to change the size of a drawing and to scale all the views together. Individual views can be displayed at the view scale, and detail views are typically created at a different scale automatically. To locate the scale setting, choose Tools⇒Options⇒System Options⇒Drawings⇒Detail View Scaling. Detail Views, covered later in this chapter, automatically get a note showing the custom scale for the view.
You can automatically add a label or note to an orthogonal drawing view displayed at a scale different than the sheet scale. You access this setting at Tools⇒Options⇒Document Properties⇒View Labels⇒Orthographic. Enable the Show Label If View Scale Differs From Sheet Scale option, and specify the rest of the settings shown in Figure 15.4 as appropriate.
FIGURE 15.4
Displaying a label to show the view scale when it is different from the sheet scale
Tip
You could consider creating a note style or block for a note that automatically links to the scale of a drawing view.
Dimension Type
Even in non-orthogonal (isometric) views, true dimensions should be used for most drawing views. Projected dimensions depend on the angle of the edge to the view plane.
Cosmetic Thread Display
If something is worth having, it is worth having twice. This panel appears in both steps, just in case you missed it in the first step.
Using the Projected View
The Projected View type simply makes a view that is projected in the direction that you dragged the cursor from the selected view. Be aware that first-angle and third-angle projections result in views that are opposite from one another. For example, if you drag at a 45-degree angle, the result is an isometric view. When placing an isometric view that you have created in this way, SolidWorks constrains the new view to a 45-degree-angle line through the Origins of the two views. To place the view somewhere other than along this line, press the Ctrl key while placing the view to break the alignment. The PropertyManager for the Projected View is shown in Figure 15.5.
FIGURE 15.5
The Projected View PropertyManager
When you use the pushpin on the Projected View PropertyManager, you can place multiple projected views from the originally selected view or select a new view to project views from. Display properties and scale of the projected views are taken from the parent view.
Using Standard 3 View
You can access the Standard 3 View tool on the Drawings toolbar by choosing Insert⇒Drawing View⇒Standard 3 View. This places a Front view, and projects Top and Right views for third-angle projection drawings. Figure 15.6 shows the PropertyManager for the Standard 3 View function.
Use the PropertyManager to select open models that you want to place on the drawing. Also select configuration and body or bodies to place here as well.
Using Detail View
You activate the Detail View from the Drawings toolbar