When you create a section view in a SOLIDWORKS drawing, the faces through which you are cutting will be displayed differently than the faces beyond the section plane. This is often achieved through hatching. The hatching is usually a series of inclined lines running across the cut faces, though the style depends on the material being cut. Drafting standards dictate what pattern to use for a particular class of material, so from the hatching you can identify the type of material.
An important question, though, is “How can you control which pattern SOLIDWORKS uses?” This came up in a training class a few weeks ago, and the answer was more elaborate than I had expected. It is complicated by the fact that there are two distinct categories of options associated with hatch patterns, and the one that controls the section view display is a bit difficult to find. To understand the difference, let’s take a look at the drawing below.
In this example, the cut faces are filled in with black rather than with a hatch pattern similar to the one shown earlier. This doesn’t match the standard I want to follow for this drawing, so I need to change it.
In the Drawings category of System Options, there is a subcategory dedicated to Area Hatch/Fill. While this seems like a promising place to look, you can see that the settings here are different from what appears on my drawing.
These options do not affect section views. Instead, they determine the default values for the Area Hatch/Fill annotation type in drawings. This annotation is used to manually add hatching to or shade in a face or bounded region in a drawing view. Since the hatching in a section view is generated automatically rather than with a separate Area Hatch/Fill annotation, the settings come from somewhere else.
As I had mentioned before, the hatch pattern changes depending on the material being cut. As a result, the hatch properties are actually defined at the part level, not at the drawing level. In the model’s Document Properties, there is a category for Material Properties. If a material is not applied to the part, then SOLIDWORKS uses these “Area hatch/fill” settings for the section view.
My model does not currently have a material, and the Material Properties settings have “Solid” enabled rather than one of the “Hatch” patterns, explaining the shaded black regions on my section view.
If a material is applied to the part, the material’s assigned Crosshatch settings will override what is set in the Document Properties. So, by changing my part material to Aluminum Bronze, for instance, I can see its hatch pattern, ANSI33 (Bronze Brass), applied in the section view.
It is worth noting that the hatch pattern can also be modified independently of the part’s Material Properties settings. Clicking on a face of the hatched region opens the Area Hatch/Fill PropertyManager, where there is a checkbox for “Material crosshatch.” This option, enabled by default, is what ties the section view’s hatch settings back to the part material. If this is unchecked, the hatch properties can be customized as needed.
Thank you for reading! I hope this gives you a better understanding of section views in SOLIDWORKS. Feel free to reach out if you have any questions.
Computer Aided Technology, Inc.