Chapter 4: Creating Simple Parts, Assemblies, and Drawings
You can delete the Horizontal relation by selecting the icon on the screen and pressing
Delete on the keyboard. As a reminder, you can show and hide the sketch relation icons
from the View menu. You can check to ensure that the relations were created to the
sketch rather than the model edges by clicking the Display/Delete Relations button on the
Sketch toolbar, clicking the relation icon to check, and expanding the Entities panel in
the PropertyManager. The Entities box shows where the relation is attached to, as shown
in Figure 4.8. In this case, it is a point in Sketch1. Without custom programming, there is
no way to identify items in a sketch by name, but you already know which point it is;
you just needed to know whether it was in the sketch or on the model. The second
sketch trick involves the use of a setting.FIGURE 4.8
The Display/Delete Relations dialog box- Choose Tools ➪ Options ➪ Sketch and ensure that Prompt to Close Sketch is turned
on; then click OK to close the dialog box. - Open another new sketch on the same face that was used by the last extrusion.
Draw an angled line across the left and bottom sides of the box with the dimensions
shown in Figure 4.9. In this case, for this technique to work, the endpoints of the line
have to be coincident with the model edges rather than the sketch entities.
This line by itself constitutes an open sketch profile, meaning that it does not enclose an
area and has unshared endpoints. Ordinarily, this results in a Thin Feature, as described
earlier, but when the endpoints are coincident with model edges that form a closed loop
and the setting mentioned previously is turned on, SolidWorks automatically gives you
the option of using the model edges to close the sketch. This saves several steps com-
pared to selecting, converting, and trimming manually.