In this article, manipulating SOLIDWORKS extension lines after being added by dimensions is examined. It is shown that the extension lines could be treated as a separate entity in drawings and we can even decide to show or hide them. Some settings existed under Tools > Options dedicated only for extension lines. You can slant the extension lines, flip the direction of a leader, and drag extension lines between the center, minimum, and maximum attachment points of arcs and circles. In the following, some of the adjustments that could be done to extension or dimension lines are demonstrated.
Change Attachment Points of SOLIDWORKS Extension Lines
You can change the existed attachment point of dimension extension lines. In the following screenshots, it is shown that an extension line is reattached from the left edge to a shaft in the middle. While the dimension is highlighted, a tiny square shows up at the attachment point. By dragging that, the extension line could be reattached to another entity.
Hide or Show SOLIDWORKS Extension Lines
You can hide or show hidden dimension lines and extension lines. Right-click a dimension line or extension line and select Hide Dimension Line or Hide Extension Line. To show hidden lines, right-click the dimension or a visible line and select Show Dimension Lines or Show Extension Lines. The following image shows how one of the extension lines and also one side of the dimension line is hidden.
Break Extension Lines
You can specify in the Dimension PropertyManager that extension lines break when they cross other extension lines and specify in that the lines break only around dimension arrows. In the following image, the diameter 0.63in dimension line has two gaps where it passes over other extension lines.
Display as Centerline
You can set individual extension lines to display as centerline style. This lets you identify when an extension line extends from a hole. To set extension lines to display as centerline style, right-click the extension line and click Set Extension Line as Centerline.
Distance from View
The gaps between two consecutive dimension lines/texts and also gap between the first dimension line/text to the boundary of the model is adjustable in SOLIDWORKS. In addition, the gap between the extension lines’ end-point and the boundary of the model could be set. One can also set how far an extension line must extend beyond the dimension lines. All these setting are under Tools > Options > Document Properties > Dimensions. See below image. After setting all these options, they can be saved in a drawing template and recall that template for any drawings.