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Color Display mode toggles between the display of assigned colors and standard sketch state colors. This is primarily used in drawings when you are making sketches where sketch relations are important. This setting is used to control the display of sketch entities only.

Hiding and Showing Edges

Sometimes, for illustrative purposes, it is desirable to hide certain edges in drawing views. The Hide/Show Edge toolbar button is on the Line Format toolbar, although it may not be on the toolbar by default. You can choose Tools⇒Customize to put it on a toolbar.

To use the Hide Edge tool, simply select the edges that you would like to hide, and click the Hide Edge toolbar button. To show the edges, click the Show Edge toolbar button; the cursor will now be able to select the hidden edges.

Be aware that if your view is in Draft Mode, edges that you hide will still be shown until the view is made into a High Quality view.

Note

Hide/Show Edges was formerly two separate toolbar buttons. In SolidWorks 2010, they became a single button.

Tutorial: Using Drawing Display Tools

Some of the functions described in this chapter are difficult to understand until you actually use them. This tutorial guides you through the functions step by step so that you can see them in action. Start here:

1. From the DVD, open the drawing called Chapter 18 – Tutorial.slddrw. Make sure that the Layer and Line Format toolbars are active and that the Hide/Show Edges buttons are available on the Line Format toolbar.

2. Right-click a blank space and select Edit Sheet Format from the menu.

3. Window+select everything on the format and use the drop-down list on the Layers toolbar to assign the selection to the Border layer. Notice that this changes the color and the thickness of the sketch lines.

4. Right-click a blank space and select Edit Sheet.

5. Click the Layer Properties button on either the Layer or Line Format toolbar. Add new layers for each of the part groups, bracket, clevis, pins, and blocks, assigning different colors to each layer. Figure 18.7 shows the Layers dialog box with these layers created.

Figure 18.7

The Layers dialog box

Caution

Be aware that creating new layers leaves the last layer that you created active, as indicated by the yellow arrow in Figure 18.6. There is no way to set the active layer to None from the Layers dialog box; you have to do this using the drop-down list in the Layer toolbar.

6. Set the active layer to None in the Layer toolbar drop-down list.

7. Right-click the Bracket part in one of the views and select Component Line Font. Deselect the Use Document Defaults option, and select the Bracket layer from the drop-down list in the lower-right corner of the dialog box, as shown in Figure 18.8. Make sure that the Drawing View option is set to All views.

Figure 18.8

The Component Line Font dialog box

8. Repeat Step 7 for all the components, assigning each component to its own layer. Notice how this makes the parts easier to identify.

Note

Alternatively, you could simply change the line style and thickness for each component. This saves you creating the layers, but you lose the color settings. The way SolidWorks handles line thickness and thickness values has changed significantly in SolidWorks 2010. The line thickness assignments in the Print dialog are still the old format.

9. Open the Component Line Font dialog box for the Bracket part again. This time, set the Line thickness to 0.0787, and click OK. You may have to rebuild the drawing to show the change (Ctrl+B or Ctrl+Q). Figure 18.9 shows a detail of the corners that are created by the thick lines. Notice the notches created at the corners.

Figure 18.9

Applying thick edges

10. These notches are supposed to be fixed using the End Cap setting at Tools⇒Options⇒Document Properties⇒Line Font. Set the End Cap Style to Square. Click OK to exit the Document Properties. In the drawing, select inside the view where you are working and make sure that it is set to High Quality. (The setting