Capturing Design Intent with iParts1 Feb, 2003 By: Jeff Wymer
The Knowledge Vault consists of a set of intelligent technologies that allow you to capture, store, and reuse the embedded design knowledge in your Autodesk Inventor models. These technologies are iParts, iFeatures, and iMates. This month I've chosen to delve into iParts and show you how to use them to build a library of parts. Once you know how it works, you can standardize your designs, thus saving you time and effort.
An iPart is an Autodesk Inventor part (IPT) that you use to define a family of parts (also referred to as table-driven parts or charted parts). You can create iParts for bearings, structural members, fasteners, fittings, enclosures, motors, gears, and other various hardware components. However, to effectively apply it, you have to know how to use the iPart Author, as shown in Figure 1, and how to place iParts into an assembly.
Figure 1. The iPart Author is an easy-to-use dialog box that assists in developing a family of parts within Autodesk Inventor.
You start by modeling a sample component from which a family of parts can be generated. As you build this sample part, be sure to incorporate design intent, ensuring that you have defined all the dimensions and constraints necessary for easy modification of this part to a different size, as defined by your family of parts.
Now you are ready to create your iPart. First, select Tools from the menu bar and pick Create iPart. This will open up the iPart Author dialog box. Within the dialog, you will find an iPart table along with a series of tabs marked Parameters, Properties, Suppression, iMates, Threads, and Other.
The Parameters tab contains the bulk of the information you'll use to define your iParts. On the left-hand side, you'll find a list box, referred to as the model list, which contains the feature list of the iPart. Under each feature is a list of parameters that define it. Select the required parameters from the model list to define your family of parts, and then use the direction arrows (>>) to copy them to the Selected Items list box on the right-hand side. Once the parameters appear in the Selected Items list, a new column will appear in the iPart table below. (Note: If you define user parameters while creating the part, they will automatically fill in the first row in the iPart table within the dialog.)
Once the parameters appear within the iPart Table, you can begin generating a family of parts. All parameters appear as a column in the table, while each row acts as a different member of the part family. To create a new row, and, subsequently, a new family member, simply right click over the iPart table and select Insert Row. Next, edit the values within the various cells to define the sizes of the iPart family members. Be sure to set the most frequently used family member as the default part for insertion. To do this, right click on the row, or family member, and select Set as Default Row.
Figure 2. When placing an iPart family member into an assembly, you generate the family member that you require by selecting key parameters that define the parts. Some part may even request a user-defined value when placed.
When placing iParts into assemblies, Autodesk Inventor uses the parameters you've specified earlier as keys to generate the correct iPart family member, as shown in Figure 2. Once you have defined all of the values required for your family of parts within the iPart table, you need to flag the parameter(s) that you want to use as key(s). Keys are used to properly configure an iPart family member when it is placed into an assembly, as shown in Figure 2. You can have up to nine keys per iPart, with one being a primary key and eight being secondary. To set a parameter as a key, right click on the parameter name in the selected items list box and select a key number. For example, you've selected a bearing iPart for placement into an assembly, and the primary key flagged is the bearing series. When placing the iPart, you must first configure what bearing series you would like to insert, fulfilling the first key. Now that you've narrowed down the series of bearing you want to use, you can select the outside and inside diameters, which are your secondary keys.
If one of the parameters is to vary on placement, convert that parameter into a custom parameter within the iPart table. You do this by right clicking over the desired column or on the parameter name in the Selected Items list. Next, select Custom Parameter Column. A custom parameter column will appear in blue within the iParts table. By right clicking again over the same column or parameter, you can set a range of valid values that limit what the user can input, thus enforcing company standards. Extruded stock is a great application for this, as the profiles have standard values but the length can vary.
Properties such as material, supplier, and cost often vary among a family of parts. To ensure correct content, you can embed the appropriate information within your iPart table. To access this information, select the Properties tab within the iPart author. Here you will find all of the meta-data commonly stored within a component's iProperties, as shown in Figure 3. Simply select the properties you would like to include within the iPart and move it to the selected items list. This will generate new columns within the iPart table, similar to how the dimensional parameters worked, as explained earlier.
Figure 3. Intellectual properties, such as cost, manufacturer, and material, may vary through a family of parts. Autodesk Inventor allows you to capture that meta-data through the iPart Author, ensuring consistency among engineering, manufacturing, and purchasing.
Now that you've taken a look at the basic information an iPart contains, press OK to generate the iPart table and embed the spreadsheet within the Autodesk Inventor part file. The part file you are currently working in is referred to as the iPart Factory--the parent component of your new family of parts. To edit the iPart table, simply open the iPart factory and double click on the table entry within the browser.
The workflow for placing an iPart into an assembly is similar to that for placing normal components. You begin by starting the Place Component command, and then you browse to the iPart Factory within the Open dialog box. After selecting the part file, pick the options button. Autodesk Inventor will provide you with a choice to either Place an iPart or Place the iPart Factory directly. By placing an iPart Factory itself into an assembly, all instances of the part change simultaneously when a different family member is selected. On the other hand, when you place an iPart into the assembly, you're placing an independent member of the iPart family. If you change the iPart to a different member, that instance updates independently from the rest of the iParts in the assembly.
After selecting the iPart and pressing open, you are automatically prompted for the placement keys defined during the authoring process. You may also be required to enter a unique value if you used custom parameters. Once you satisfy these variables, you can hit OK and insert your iPart.
Autodesk Inventor allows you to capture your design intent and leverage the intellectual capital in your models to create better designs. Leveraging this capital ensures that the design and process knowledge that reside in one designer's mind can be accessed and used by multiple designers.
Autodesk Technical Evangelist Lynn Allen guides you through a different AutoCAD feature in every edition of her popular "Circles and Lines" tutorial series. For even more AutoCAD how-to, check out Lynn's quick tips in the Cadalyst Video Gallery. Subscribe to Cadalyst's Tips & Tricks Tuesdays free e-newsletter and we'll notify you every time a new video tip is available. All exclusively from Cadalyst!
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