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The part browser displays the information about the geometry that make up the part model in a hierarchy. The Filter icon at the top of the browser shows a menu for turning the visibility of certain elements on and off.
The first elements in the browser are the Solid and Surface bodies folders and the Origin folder. If there are no surfaces, only the Solid Bodies folder is present. The number in parentheses next to the folder indicates the number of bodies contained in the folder. The Origin folder contains icons for the reference planes (default work planes), work axes (default work axes), and the center point. If you pause the cursor over an icon, that feature highlights in the graphics window. If you click an icon, that reference feature activates in the window. Click in open space in the graphics window or click another to cancel the selection.
If a note is attached to the part, the Engineer's Notebook folder displays below the origin folder. Expand the folder to view the individual note icons. Double-click a note icon to open the Engineer's Notebook.
Features are listed in the browser in the order they were created. Input surface and work features are consumed and nested under the appropriate feature and participating body by default (for example stitch features consume input surface features and work plane consume input work points). You can also control consumption on individual features. If the feature originates from a sketch, or there is a note attached to the feature, the feature folder expands to show those elements. If the sketch is shared, the sketch appears at the top level in the model tree, and a link to the sketch displays under each feature that uses it.
Select Show Extended Names in the Filter menu to display detailed information about part features.
Extended feature names are available in the Part, Sheet Metal Part, Assembly Modeling View, and Drawing environments. Format or content of extending strings cannot be changed.
Show Me how to display feature details in the browser
Some features take longer to calculate, such as large patterns or coils. You can speed up calculation by dragging the End of Part marker up the model tree. Any features below the symbol are temporarily removed from the model. When you drag the End of File marker back down the model tree, those features are added back into the model.
Shows and hides selected features, filters contents, manages access to feature and sketch editing, and provides alternate access to functions in the context menu.
In a part file, click item to select, then right-click to display the context menu.
In both Assembly and Model environments, options reduce the volume of information presented in the browser by eliminating the display of selected types of information. Click to select or clear check mark to cancel the selection.
- Hide UCS turns display of User Coordinate Systems off or on.
- Hide Work Features turns display of all work features, and the Origin folder, off or on.
- Hide Notes turns display of notes off or on.
- Hide Warnings turns warnings attached to constraints in the browser off or on. It does not hide failures.
- Hide Documents turns embedded documents off or on.
- Show Extended Names turns display of extended information for part features on or off.
Context menu options
The context menu (right-click) accesses functions for operations on the selected feature, sketch, or constraint in the browser. Depending on the browser configuration and the selected item, all options may not be available. The same context menu options are available when you select the item in the graphics window, plus viewing options.
- Adaptive: Sets sketch, feature, or part as adaptive (can change size or shape when constrained to fixed geometry).
- Copy: Copies selected item from the browser or graphics window and places a copy on the Clipboard. May be pasted into the current file, another document, or application. If pasted into the current document, the item is placed at the coordinate origin in the graphics window and at the bottom of the browser tree.
- Create note: Activates the Engineering Notebook and creates a note to attach to the selected object.
- Delete: Removes selected item from the browser and the graphics window.
- Design Assistant: Activates the Design Assistant. Design Assistant creates reports and shows, allows edits of properties, and displays information about items in the part file in a table format.
- Edit feature: Activates the feature dialog box so you can redefine its size, extents, and other values.
- Edit sketch: Activates the sketch. Use commands on the Sketch tab to add, delete, or change dimensions, trim or extend curves, add sketch geometry, add or delete constraints, or drag the sketch to change its shape.
- Find in window: Locates the selected item in the graphics window.
- Consume Inputs: Enables and disables the automatic consumption and nesting of input surface and work features (such as stitch features consume input surface features and work planes consume input work points). Clear the check box if you do not want work features and surface features to consume (where applicable) in the browser.
- How to... : Opens the Help topic for the current operation.
- Measure angle: Measures and displays the angle between two selected lines, points, curves, or planes.
- Measure distance: Measures and displays the distance between two selected points, lines, curves, or planes. Accumulates measurements and displays cumulative total distance.
- New sketch: Creates a sketch on the selected work plane or planar face and activates the sketch.
- Properties: Sets properties for the selected item in the Properties dialog box.
- Redefine sketch: Moves and attaches a sketch to a different plane or face than the one on which it originated.
- Share sketch: Selects a sketch already used in a feature for use in a new feature. Places a copy of the sketch in the browser. Available only when the sketch was consumed by a feature.
- Show dimensions: Shows sketch dimensions for the selected feature. Visible dimensions can be edited or deleted.
- Suppress feature: Removes feature from the graphics window. It remains visible in the browser, designated by a gray box. To unsuppress, right-click in browser, click Suppress and clear the check mark.
- Visibility: Sets component visibility on or off.
- Move EOP Marker: Moves the End of Part marker under selected feature, or Origin folder.
- Move EOP to Top: When the End of Part indicator is located within the part features, moves the End of Part indicator directly to the top of features in the browser. Move EOP to Top is not available when the EOP is already at the top.
- Move EOP to End: When the End of Part indicator is located within the part features, moves the End of Part indicator directly to the end of features in the browser. Move EOP to End is not available when the EOP is already at the end.