SolidWorks

The SolidWorks FeatureManager Design Tree (Solid Thinking SolidWorks Tutorial)

1 Apr, 2008 By: Richard Doyle

There's more to this feature than meets the eye.


The SolidWorks FeatureManager Design tree is always front (left?) and center, but have you really looked at it lately? The FeatureManager Design tree provides an outline view of the active part or assembly document, making it easy to see how a model or assembly was constructed. In a drawing document, you can see the various drawings' sheets and views. But there's much more to the FeatureManager Design tree than meets the eye.

FeatureManager Design Tree Items
Several items appear in the FeatureManager Design tree when you start a new part or assembly document. The top entry is the default file name (it will change when you save the file). The remaining items may contain important information about the model, which you can use to help convey design intent or to analyze the part or assembly document.

The Design Binder
Perhaps one of the most underutilized features in SolidWorks, the Design Binder initially contains the Design Journal, a Microsoft Word document that resembles an engineering journal. The Design Journal contains headings for File Name, Description, and Material. These fields are linked to document properties. You can also paste images of your model into the Design Journal. The Design Binder also accepts other types of documents; simply right-click on the Design Binder and select Add Attachment. The Design Journal can be tailored to your needs by modifying the Design Journal template.

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An image of the Design Journal.

Annotations Folder
3D annotations and views are stored in the Annotations folder. Annotation views are used to convey dimensions, notes, and geometric tolerance information in accordance with ANSI/ASME Y14-41-2003. You can automatically insert annotation views into a drawing.

Lights, Cameras, and Scenes
Lights and Scenes are used with PhotoWorks and RealView Graphics to create realistic views of your models. Cameras can be used in conjunction with Motions Studies to create walk-through animations or to view models from the perspective of the camera. The Lights, Cameras, and Scenes folder contains all of these items.

Solid Bodies (Parts Only)
The Solid Bodies folder contains information about each solid body in a part document. The folder gives you access to each individual body so you can edit the body properties, change the appearance of selected bodies, and delete individual bodies. The Solid Bodies folder appears only after you have added features to the model.

Material (Parts Only)
A right-click on the material icon allows you to add material properties to your model. Adding material properties to your model gives you the ability to analyze real-world physical properties such as weight and moments of inertia.

Equations
Equations are mathematical relations between model dimensions. The Equations folder also stores linked dimension values, as well as global variables that you can assign in your model. For sheet metal models, the assigned thickness is stored in the Equations folder as a linked value.

Default Planes
The default planes (Front, Top, and Right) are visible in the FeatureManager Design tree, and you can modify the names of each plane by right-clicking and selecting Properties.

Origin
As the name implies, the Origin is the 0,0,0 coordinates of your model. Origin is used in the model properties to calculate the center of mass, axes of inertia, etc.

Feature Names and Part Names
When you add a feature to a part model, the feature names are added to the FeatureManager Design tree in the order they were created. When you add components to an assembly model, the components are listed in the order in which they were added.

FeatureManager Design Tree Conventions and Symbols

Sketches
(+) over defined sketch
(-) under defined sketch
(?) the sketch could not be solved

Features
error icon  an error with the feature
warning icon  a warning with the feature

Assembly Components
(+) over constrained
(-) under constrained
(f) fixed component

Assembly Mates
(+) over defined mate
(?) not solved

External References
--> part or feature has an external reference
-->? external reference out-of-context
-->* external reference is locked
-->x external reference is broken
The FeatureManager Design tree uses a variety of symbols to help you understand what's in your model. The symbol symbol next to each item's icon indicates that it contains associated items, such as sketches, lights and cameras, or solid bodies. Click on the symbol to expand the item and display its contents. To collapse all of the expanded items, you can right-click the document name at the top of the tree and select Collapse Items. Better yet, press Shift + C, and the tree collapses as well.

Other FeatureManager Design tree symbols provide information on individual items. The table shows a list of symbols and their meaning.

FeatureManager Design Tree Options
Several options are available for customizing the display of the FeatureManager Design tree. Click Tools / Options / System Options / FeatureManager to access these options. Use the check boxes to set display and navigation options. A pull-down menu determines how and when warnings will be displayed, and in SolidWorks 2008, a new set of options controls which items will be displayed.

Scroll Selected Item into View
With this option selected, when you select a feature (part) or component (assembly) from the graphics area, the FeatureManager Design tree will automatically highlight and scroll the selected item into view. This can be important in part or assembly models with many items that require scrolling with the slider bars to bring the items into view.

Name Feature on Creation
Good design intent necessitates that all features in a part model be labeled with a descriptive name. With this option turned on, each time you create a feature, the feature name will be highlighted and ready for you to enter a name.

Arrow Key Navigation
Using arrow key navigation in the FeatureManager Design tree offers an easy way to traverse your model feature by feature. With this option turned on, you can select the Rollback Bar and use your up and down arrow keys to step backward or forward through your model. The left and right arrows can be used to expand or collapse the FeatureManager Design tree. If you have never used arrow key navigation, give it a try.

Dynamic highlight
When this option is selected, geometry in the graphics area (edges, faces, axes, etc.) is highlighted when the cursor passes over the item in the FeatureManager Design tree.

Display warnings
This pull-down menu allows you to specify if and when warnings are displayed in your models. You can set it to Always, Never, or All But Top Level.

Hide/Show Tree Items
New in SolidWorks 2008 is the ability to remove items from the FeatureManager Design Tree. Options allow you to Show, Hide, or set to Automatic all of the FeatureManager Design tree items.

figure
Hide/Show Tree Items options for the FeatureManager Design tree.

Tips for Using the FeatureManager Design Tree

The FeatureManager Design tree is the lifeblood of your model. Learning how to quickly and easily navigate it makes working with your part and assembly models easier. Here are a few tips.

Use Arrow Key Navigation
As previously mentioned, using arrow key navigation makes it easy to traverse through your model, rolling backward or forward to analyze features. You can add new features or edit existing features while the model is in the rolled-back state. Select the Rollback Bar to highlight it, and use the up and down arrow keys. When your cursor is on a feature, you can use the left and right arrow keys to expand or collapse items.

Use Right-Click to Roll Back or Roll Forward
Instead of using the Rollback Bar, you can right-click on an item in the FeatureManager Design tree and select Rollback to roll your part back to the feature directly above the selection. Right-click again to roll the model forward.

Selecting Items from the FeatureManager Design Tree
You can select features or components by clicking on the item in the FeatureManager Design tree. Hold the Shift key to select multiple consecutive items, or use the Ctrl key to select multiple items that are not consecutive. Box select and cross select also work in the FeatureManager Design tree. Select an empty region of the panel and drag to select items.

Search for Items
If you right-click on any item in the FeatureManager Design tree (except Materials or Lights, Cameras, and Scene), you can search the FeatureManager Design tree by selecting Go To. Enter a search string in the Go To dialog box to find the item you are looking for.

figure
The Go To dialog box.

Filtering the FeatureManager Design Tree A nifty new feature in SolidWorks 2008 is the ability to filter the FeatureManager Design tree. Place your cursor in the search bar at the top of the tree and start typing. As you type, only the features or components that match the search string are displayed in the FeatureManager Design tree. In an assembly document, you can also filter the graphics area. With the option Filter Graphics View selected, only those components that are filtered are displayed in the graphics area. You can also add tags or keywords to SolidWorks documents or features to make them easier to search.

figure
Part document filtered.

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Assembly document filtered.

Summary
Every time you open or start a SolidWorks document, you are automatically presented with the FeatureManager Design Tree. Sometimes we may take it for granted, but it's the most important part of your SolidWorks file. Learn all of the ins and outs of the FeatureManager Design tree, and your models will be easier to work with, will contain important information for downstream edits or processes, and will be presented in a clean, organized fashion.


About the Author: Richard Doyle


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