Capturing and Reusing Design Intent

1 Jan, 2003 By: Jeff Wymer

The Knowledge Vault contains a set of intelligent technologies for capturing, storing, and reusing the design knowledge embedded within your Autodesk Inventor models. iFeatures, iMates, iParts, and the Engineer's Notebook make up the basis of the Knowledge Vault. In this column we'll focus on iFeatures; we'll move on to iParts and iMates in the next two issues.

Defining iFeatures

iFeatures can be saved and reused in other designs. You can create an iFeature from any sketched feature. Inventor allows you to define the default locations for storing and accessing iFeatures, as shown in Figure 1. If you want to share iFeatures across your entire organization, you can define a network location for storage. To change the default, select Application Options under the Tools pull-down menu, and select the iFeature tab. You'll see that the default location is the Inventor install directory\catalog. The options available include

  • iFeature Root, which specifies the location of iFeature files used by the View Catalog dialog box;
  • iFeature User Root, which specifies the location of iFeature files used by both the Create iFeature and Insert iFeature dialog boxes;
  • Sheet-Metal Punches, which specifies the location of iFeature files used by the Sheet-Metal Punch Tool dialog box.

Figure 1. Autodesk Inventor allows you to easily select the features and parameters to be categorized for reuse.

These directories can be located either on your local computer or a network drive.

Creating iFeatures

To create an iFeature you must extract a feature you want to reuse from an existing part file. Open the part file, select the Tools pull-down menu, and select Extract iFeature. Now select the feature(s) that you want to catalog for reuse. You can either select the feature from the part-feature browser or directly from the model.

Once you've selected the features to extract, they will appear in the Selected Features area of the Create iFeature dialog box. To begin, rename the default prompt in the dialog box for the placement face, plane, and so on. I like to rename the prompt from "Position Geometry" to something more user friendly, such as "Select Face," "Select Center Plane," or "Select Center Point." If I'm defining a feature, I want to make sure I communicate to the others how to place it.

When you expand the feature in the dialog, you will see the model parameters that build the feature. From here, you determine which parameters are allowed to be changed when inserting an iFeature. You can control any aspect of the feature from defining the placement location to selecting dimensions that control feature size. When defining the iFeature sizes, you can set up limits for the dimension values that can be changed by anyone inserting the iFeature. The limits can be a range of values or a dropdown list containing preset values, as shown in Figure 2. This ensures your design intent is fully captured and company standards are followed during downstream use. To set up limits, simply select a variable from the dialog box and pick the >> arrow to place it in the Size Parameters. You can move variables in and out of the parameters section by selecting the variable and choosing << to remove or >> to add.

Figure 2. Table-driven iFeatures allow you to quickly toggle between different design scenarios while still maintaining company standards.

Once a dimension is listed in the Size Parameters field you can define what the user is able to change upon inserting the iFeature. To set up a drop-down list, select None in the edit list and change it to List to bring up the List Values dialog box. Input appropriate values and select OK to close. To set up a range for valid values, select None in the edit list and change it to Range to bring up the Specify Range dialog box. Here you can define the range as a value less than or equal to the default with a predefined minimum value and/or a value less than or equal to a maximum value but does not to exceed the minimum or the default value.

Finally, select Save and give the iFeature a name. You may want to put similar features together by setting up categorical directories (for example, o-ring grooves). Inventor ships with example iFeatures for Geometric shapes, Pockets and Bosses, Punches (for sheet-metal parts), and Slots.

Custom Help for iFeatures

You can add a custom-help file to an iFeature. The file can be a Word document, HTML file, or spreadsheet embedded or linked to the iFeature. When a document is available, an Information button is shown on the Insert iFeature dialog box. To attach a custom help file to your iFeature, open the iFeature for editing and insert an object (choose Object from the Insert pull-down menu). Then select the custom help file. Choose whether the help file is to be linked or embedded within the iFeature. The linked or embedded document is shown in the browser as an icon, nested under the Third Party icon. Select the document in the browser and designate it as Placement Help. After that, you can save your iFeature document. Selecting the Information button when inserting an iFeature, will automatically access the custom help file.

Table-Driven iFeatures

In a table-driven iFeature, as shown in Figure 2, you can modify values but not add or remove parameters or geometry. You can quickly change the iFeature from one size to another by simply activating the appropriate values. To set up a table-drive iFeature, you first need to define the iFeature with all the dimensions to be driven by the table. Next, open the iFeature document and use the iFeature Author Table icon in the feature palette. The iFeature Author is a tool that converts an iFeature to a table-driven iFeature. A table-driven iFeature has multiple versions that are developed and selected by rows in a table. In the iFeature Author dialog box, you can specify parameters, properties, threads, placement geometry, and custom parameters. Each row in the table may contain different values so that the iFeature can have many versions, each with a specific diameter, thread specifications, material, and so on.

In the iFeature table, each selected parameter is a column heading. Right-click a numbered cell, and then insert a row, delete the selected row, or set it as the default row. Right-click a column heading, and then set a key value, a custom column, or delete the selected column. If custom, right-click again, and then specify the value range. In table rows, click in cells, and then enter values to create a unique variation of the iFeature. When done, click OK to convert the iFeature to a table-driven iFeature.

Upon inserting a table-driven iFeature, you will be prompted to specify the values you want to set iFeature to. After inserting a table-driven iFeature, if you want to modify the value, double-click on the new value setting in the feature browser.

Placing iFeatures

You can place an iFeature using the Insert iFeature button or View Catalog button from the feature palette. With the insert option, you browse for the iFeature you want to insert. The View Catalog button allows you to drag and drop the iFeature into your part file from the Windows Explorer or double-click on the iFeature to edit. Both options support browsing the iFeature using thumbnails for easy location and identification.

After selecting the iFeature you will automatically be prompted for the placement variables you defined during the creation process. Once you satisfy these variables you can then select and input the dimensional requirements.

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