Drawing View Activation and Selection1 Aug, 2002 By: Greg Jankowski
When creating a detail drawing, as shown in Figure 1, SolidWorks software has different methods in which drawing views and sheets can be activated or selected. While fairly apparent, this column will nonetheless explain the differences between an active or selected view, sheet or view focus, and dynamic or manual view activation modes. Being able to recognize these differences when creating sketch geometry or annotations will help you determine whether the sketch entities or annotations are associated with a specific drawing view or with the drawing sheet.
Figure 1. This example of a SolidWorks drawing shows the details of a mechanical part.
An annotation is a note or symbol that can be inserted into a part, assembly, or drawing. When annotations are associated with a drawing view, they will move when the drawing view moves. Annotations that are attached to the model or assembly geometry are automatically associated with the drawing view (such as notes with leaders, surface-finish marks, and so forth). Notes or symbols not attached to drawing view geometry will reference a drawing view or the sheet based on view or sheet selection. If an annotation is referenced by a drawing view, it should be associated with that view.
Active vs. Selected Views
Selected views can be used to move the view, resize the drawing view boundary, or create break lines for a broken view. Figure 2 shows a selected RapidDraft drawing view with a yellow border and a selected non-RapidDraft drawing view with a green border. RapidDraft drawings are designed so you can open and work in drawing files without loading the model files into memory.
Figure 2. The selected non-RapidDraft view is on the right and surrounded by a green border; the RapidDraft view is on the left and bordered in yellow.
To select a view in SolidWorks, either select in an empty area inside the view boundary or select the view name in the FeatureManager design tree. Also note that the parent view's boundary is highlighted when a drawing view is selected. A parent view is the view referenced (projection, section, detail, and so on) to create the drawing view. This visual clue is useful when moving drawing views. A view that has a parent view can also be activated by using the Jump to View function either by pressing the right mouse button over the selected view or over the view name in the FeatureManager design tree. If the view has no parent, this option will not appear.
An active view is used to create sketch geometry and annotations that will become attached to the view. An active view is shown with a gray box around the view boundary. An example of a selected view is shown in Figure 3.
Figure 3. You can select a view, as shown on the left, by choosing the view name in the FeatureManager design tree. The active view, shown on the right, lets you create sketch geometry and annotations.
If sketch entities and annotations are attached to a view and the view moves, the annotations and sketch geometry also move. If the view is deleted, so are these sketch entities and annotations. Sketch entities are typically created in a drawing view to define a section line or detail area. If the parent view is not active, you cannot edit the sketch entities.
Sheet vs. View Focus
There are times when users may not want annotations to be associated with a drawing view. An example would be a set of standard notes. These notes should not be associated or move with any drawing view.
While in dynamic sheet activation mode, the Lock Sheet Focus function can be used to ensure the sketch geometry or the annotations are not tied to a drawing view. To return to dynamic mode, select Unlock Sheet Focus.
If the manual view activation mode is currently selected, then simply double-click in any open space on the sheet outside of a drawing view boundary.
Dynamic vs. Manual Activation
There are two different modes that can be used for view and sheet activation: dynamic and manual. Dynamic mode looks at the cursor location and automatically selects the view closest to the cursor. The Lock View Focus and Lock Sheet Focus functions can be used to temporarily set the view or sheet focus respectively. To return to dynamic activation mode, use Unlock View Focus or Unlock Sheet Focus, depending on what mode is currently active. To activate these functions, select the view or sheet in an open area, press the right mouse button, and then select the desired option. The view or sheet can be selected in the graphics window or in the FeatureManager design tree. The advantage of dynamic view selection is the view is active when the cursor is over it, which automatically associates any sketch entities and annotations you create to that view.
Dynamic view activation is active by default. To set the manual Drawing View activation mode, de-select the option Dynamic View activation from the Tools/Options/Drawings settings dialog box.
You are in the manual activation mode when dynamic view activation is turned off. This means you have to tell SolidWorks when a view should be active. The advantage of manual mode is you do not have to watch to make sure the desired view is active, and you can sketch outside the view boundary without accidentally activating another view. If you have view boundaries crossing one another, manual activation ensures that you associate the sketch entities or annotations to the correct view or to the drawing sheet.
When using manual activation mode, double-clicking inside the view boundary in an empty area can activate a drawing view. To activate the sheet, double-click in any empty area on the sheet that is not inside a view boundary.
Each user may have a preference when it comes to selecting or activating a drawing view. SolidWorks offers various methods that can be adapted to fit your preference or the situation. In most cases, the selection and activation can be handled automatically. When a specific view or sheet needs to be selected, you can use the manual methods. But understanding the differences lets you make an informed choice as to whether to use manual or dynamic selection modes.
About the Author: Greg Jankowski
In her easy-to-follow, friendly style, long-time Cadalyst contributing editor and Autodesk Technical Evangelist Lynn Allen guides you through a new feature or time-saving trick in every episode of her popular AutoCAD video tips. Subscribe to the free Cadalyst Video Picks newsletter and we'll notify you every time a new video tip is published. All exclusively from Cadalyst!