Broken-out Sections can be applied to existing drawing views of Parts or Assemblies to reveal internal features or components. In this article, we’ll take a look at different ways to specify the shape and depth of broken-out section views in SOLIDWORKS Drawings.
Section Profile Shape
By default, the Broken-out Section view uses irregular spline shapes as the input. When you first select the Broken-out Section view command from your toolbar, you’ll notice that your cursor changes to a pencil with the spline icon on it.
This is your sign to start drawing a spline shape on the specified drawing view. The shape will need to be closed, meaning that your shape must start and end at the same spot.
But what if you need the Broken-out Section cut to be a specific shape like a rectangle or circle? The solution is simple, it just requires a slightly different workflow. First, navigate to the Sketch tab in your Command Manager, then pick the shape you want (we’ll use a rectangle for example) and sketch it.
Cutting a Specific Shape
After you’ve sketched the shape, select it (make sure it is highlighted in the graphics area). With the rectangle selected, click the Broken-out Section View Command, and the rectangle will be used – no need to mess with sketching a spline.
Specifying the Depth of the Section
There are two ways to specify the depth of the Section view:
- Using a numerical value, and
- Selecting an edge reference from the model.
For whichever method you plan to use, I would always recommend checking the “Preview” box in the Broken-out Section PropertyManager right away. This will create temporary preview planes of your section depth on your additional drawing views. If you change the depth dimension in the PropertyManager, these yellow preview planes will update as well.
The other method for selecting the depth of the broken-out section is to select an edge on the model. This is typically done by selecting an edge that is visible from a different drawing view. If selecting a linear edge, it will need to be parallel to the yellow preview plane of the drawing it is on. See in the screenshot below how the position of the Preview planes updates when I select a vertical edge from the Front View.
If a circular edge is selected for the depth reference, the cutting plane will be placed at the center of the circle or arc. In the screenshot below, you can see that the blue highlighted edge is used as the depth reference, and the cutting plane is placed at the centerpoint of that arc (which coincides with the midplane of this model).
While detailing Broken-out Section views of your models in SOLIDWORKS, utilizing these profile, depth, and preview options will ensure that your drawings are clear and accurate.