Manufacturing

Drawing Views 101

1 Oct, 2002 By: Greg Jankowski


Drawings are still the most widely used communication tool in the engineering community. While a number of tools and technologies have come along with the promise to eliminate the need for drawings, they continue to be the main vehicle for communicating and documenting design intent. The primary reason for this is because drawings often serve as documentation of requirements. Suppliers use drawings to produce quotes, determine manufacturing methods or processes, and inspect parts to ensure they meet the requirements defined within the drawings.

Making a readable drawing is key to assuring that design team members can look at it and understand what's required. SolidWorks offers a number of different options and types of views that can make detailing flexible and effective.

Types of Views
Users have a number of different types of drawing views to communicate their design. Drawings are used to create views based on one or more parts and/or assemblies, and they may contain a combination of different parts and assemblies. These functions are available via the Drawing toolbar or from the Insert/Drawing View menu. There are 12 different drawing view types.

Standard 3 Views. This function will create three views (top, front, and right side) and is typically used when creating a new drawing.

Projected View. Using this, you can add a new view orthographically projected from an existing drawing view. To create the view, select a parent view and drag the cursor up, down, left, or right from the original view and drop the new view into place.

Named View. This function creates a new view based on a saved (named) orientation from the part or assembly.

Empty. An empty view is used to create a new view with no related part or assembly geometry. This allows you to create and group sketches in a drawing. By creating one or more empty views, multiple 2D sketches can be created and controlled separately (for instance, move, scale, and so forth) on the drawing.

Section View. A section view shows the internal details of a part or assembly. Section views show details better than hidden-line views do. The section line is sketched in the drawing on top of an existing (parent) view. The section view is created from this sketch line.

Aligned Section View. This is similar to a section view, but the section line consists of two lines at an angle to each other. The section view rotates the geometry on the angled segment so the section can be projected.

Detail View. A detail view is a blown-up portion of an existing view. The detail view is defined by a closed profile on an existing view, typically a circle.

Auxiliary View. This view is defined by folding the new view normal (perpendicular) to an existing view's part or assembly edge.

Crop View. A crop view displays just a portion of an existing view. It is defined by a closed profile sketched in the active view.

Alternate Position View. This view consists of two configurations shown on top of one another. For example, you can show a door in the open and closed position within a single view and display dimensions based on both positions. The view can be created from existing configurations, or they can be made on-the-fly using this function.

Broken-Out Section. This view shows a partial section inside an existing standard view. A closed profile is used to define the broken-out section. The depth of the section can also be controlled.

Relative to Model View. This view is defined by two faces or places within the part or assembly.

figure
Figure 1. This example drawing shows several different view options.

Display Modes
The selected display mode for the drawing views has an effect on drawing readability and performance. The example in Figure 1 shows a drawing created in shaded mode. Using SolidWorks, you have the flexibility of changing the display mode of a drawing view. For example, if an exploded-view assembly is easier for you or someone else looking at the drawing to understand in shaded mode, just that view can be shaded. While wireframe is listed as the fastest mode, it is typically difficult to work with and is not practical. The modes and relative speeds (fastest on top) are as follows:

  • Wireframe
  • Shaded
  • HLR (Hidden Lines Removed)
  • HLG (Hidden Lines Gray)

Viewing Tips
Now you can put your new viewing knowledge to use. To select a view, pick near the drawing frame of the active view, as shown in Figure 2. The selected view will highlight its parent view or section line in yellow.

figure
Figure 2. Here you can see active and selected views in action.

If there is no parent, no other view is highlighted. If you want to move a view, select on the view frame, and drag the view to the desired location. The first view in the drawing (first view listed in the FeatureManager design tree) is typically the front view. Many of the other views were created from that view. Note also that a projected or aligned view will move only along the projected direction, and if you select a line or vertex, it will highlight in all views.

When a view is selected, resize handles show up on the corner and mid-points of the drawing frame. These can be dragged to make the view frame larger. By default, the frame is slightly larger than the overall size of the part or assembly, which makes it easier to select. This feature is often used for overlapping or enclosed boundaries. The re-size handles allow you to alter the view frame so the view is easier to select and manipulate.

You can also use the right mouse-button over a selected view to display these three options: view alignment functions (Break, Align, Default); Jump to Parent View, which allows users to go to the view that was used to define (parent) the current view; and view properties.

Other viewing options to keep in mind include the properties dialog box, which is accessed via the right mouse button; you can use it to create a different configuration for a drawing or a single view. A configuration allows for different variations of a design to be derived from a single part or assembly. Also, when creating a new view, you can use the Ctrl key to create an unaligned view, and don't forget that drawing views can be copied and pasted from the clipboard.

Conclusion
Drawings are used to describe and document your designs. Make sure your layout is easy to understand and tells the story behind your design intent. When creating drawing views, think about your target audience, keep the drawing layout simple and easy to read. Remember that the recipient of your drawing may not have the understanding and background you had when creating the original design.


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