Converts a single feature or a collection of features into a feature you can reuse in other part files.
You can create an iFeature from any sketched feature or part file, and save it. For each iFeature, you define descriptive parameter names that clarify how the parameters affect the placement of the iFeature in a part file.
iFeature are stored in files with the .ide extension in the Catalog folder by default. After you create an iFeature and store it, place it in a part file or modify it.
- Drag it from Windows Explorer into a part file or use Insert iFeature to place it.
- Modify the iFeature file (.ide) before or after it’s placed in a part file.
You can precisely position an iFeature using geometric constraints and dimensions that are specified in parameters. Changes to the feature file (.ide) do not affect placed iFeatures in part files. Likewise, changes to an individual occurrence do not affect other occurrences of the same iFeature in the same or other part files.
Types of iFeatures
- Regular iFeatures
- A regular iFeature is a single version of a feature that you can modify directly by editing its file. When you place an iFeature, position geometry describes the interface that is joined to a feature. Typically the sketch plane is used for this purpose but it can also be a sketch line or point, or another geometric element.
- Table-driven iFeatures
- Table-driven iFeatures contain many variations of the feature in a table. Using the iFeature Author tool, you define unique versions of the same feature. The advantage of using a table-driven iFeature is that you can quickly change the iFeature from one size to another. Simply select the version of the iFeature stored in the parameter table, without having to edit the iFeature. However, in a table-driven iFeature, you can modify values but you can’t add or remove parameters or geometry.
Parameters in iFeatures
Working with parameters is an inherent part of developing a design. Parameters are used to store the dimensional values for sketches, extrusions, fillets, chamfers, and other elements. In iFeatures, parameters are defined for feature size and position geometry, thread variables, and other properties.
- Use descriptive parameter names such as height, width, and depth.
- Give size restrictions.
- Provide instructions or explanation for placement or positioning.
- Add Placement Help to the iFeatures. The help is available (as a document, HTML file, or spreadsheet) when you place or edit the iFeatures.
- Give the same or similar names to the iFeature filename (.ide) and the iFeature in the Extract iFeature dialog.
- Add to the Size Parameters table any values that are subject to change in the iFeature. When you place an iFeature, the value is fixed for any parameter that is not in the Size Parameters table.
The parameters that you create for all of your projects can be viewed in the Parameters dialog (Manage 
Parameters). If you hover over a parameter name in the dialog, a tooltip displays which sketches, features and other parameters (as part of an equation) it is used in.
Best Practices for Creating iFeatures
- Define all necessary parameters before you create the iFeature. After it’s created, you can modify parameters but you can’t add new parameters to the iFeature.
- Make the originating iFeature (or iPart) self-contained. Do not use reference geometry.
- If you create dependent geometry, make it dependent only on geometry in the iFeature. Avoid using the default origin work planes, axes, or center point for work features.
- Use expressions to create proportional relationships among geometric elements rather than numerical dimensions.
- Avoid horizontal and vertical constraints in an iFeature. Use parallel and perpendicular constraints to other geometry in the iFeature.
- You can also use various assembly commands to create iFeatures of : keys, parallel splines,involute splines, o-rings, shafts or gears.
- In the iFeature file (.ide), you can add custom properties that are exposed as Model Properties in the consuming part. These properties are available when in a drawing file you document the part containing the iFeature.
- Create parameters as you create dimensions, or use the Parameters command to name parameters to include in the iFeature. Rename the default parameters, or click Add to define new ones. All parameters that you assign names to are automatically listed in the Extract iFeature dialog box, Size Parameters list.
- When planning, decide how to constrain feature sketches and use equations rather than numeric constants to control size and relationships. Equations reduce the number of parameters to define placement of an iFeature and allow it to resize from the original feature.
- To use an entire part as an iFeature, create a table-driven iFeature from a table-driven iPart.