About iParts

Create part families that differ by size, material, or other variables.

If you have stock designs that you use repeatedly, you can create them as iParts. Then you can use the variations, called members, by selecting them from a table. The designs can differ by size, material, mounting configurations, and so on.

iPart Workflow

Working with iParts has two phases: part authoring and part placement.

In part authoring, you design the part and define all of its variations.

Start with a new or existing part or sheet metal part.
Determine the portion of your design that changes with each member.
Rename parameters, establish equations, and create user parameters.
Use the Create iPart command to define table rows that represent versions (members). Specify variations of the part’s parameters, properties, thread information, and so on.
When you save the part, it is automatically saved as an iPart factory.

In part placement, you choose a row in the table to represent the appropriate version. Inventor generates an iPart member, using the values in the table row. Inventor inserts it in your assembly like any other component.

Information an iPart Can Include

Parameters. Use the Parameters Editor to rename parameters, establish equations between parameters, and create user parameters.
Properties. Include information such as part number, stock number, and material. Your bill of materials and parts list are automatically kept up to date.
Threads. Include different thread families, designations, classes, direction, and pipe diameter.
iMates. Include or suppress iMates, or specify offset values, matching names, and sequence number.
Work features. Include or exclude work features or set their visibility status.
Feature suppression status. By suppressing features, you can include several configurations of a single part in one file. For example, one configuration of the part has an extrusion with a cut, while another has an extrusion with a join. In sheet metal iParts, you can suppress features that were added to the flat pattern, making individual flat patterns unique for iPart member files.
iFeatures. Specify iFeatures to include in the iPart. If the iFeature includes a table, you can specify the iFeature row value and the suppression status for each row. (You can also save an entire iPart as a table-driven iFeature.)
Sheet metal iParts can include the Sheet Metal Rule, the Sheet Metal Unfold Rule and the flat pattern orientation.

About iPart Tables and Spreadsheets

You define individual members by specifying values in the iPart Author table. If you prefer, you can add or edit members in an embedded Microsoft Excel spreadsheet. For standard iParts, each table row is a member of the iPart.

A member column in the iPart table generates a default file name based on the factory name. Each member name is incremented. Optionally, click Options in the iPart Author dialog to set up a different naming scheme, or enter a new name in the member cell.

Note: When you place a member in an assembly, the browser displays the member file name. If you remove the file name setting from the member column, the file name is based on concatenated key names, which can result in long file names.

Any feature you select in an iPart Author table highlights in the graphics area. If you select a column or a cell, the owning feature highlights in the graphics area, if possible.

If you do not specify a unit of measure in a table cell, default document units are used.

About Standard and Custom iParts

You can create two types of iPart factories: standard and custom.

A standard iPart factory defines all values in columns. When you publish an iPart using a standard iPart factory, you cannot edit any members or values after placement.
A custom iPart factory contains at least one column identified as a custom parameter column. You can modify the custom parameters in the iPart member when you place it. You can add features to a custom iPart member, which means that two custom iPart members produced with identical parameters can be different. Custom iPart member columns appear with a blue background.

Note: Successive placement of an existing iPart member in an assembly reuses the member file . If a key determines the selection criteria for an iPart member, fixed values from the factory table define it. That iPart member is standard. It implies that there is a finite number of input combinations to create the iPart member. Examples are Nut, Bolt, and Washer.

You cannot edit custom iPart factories directly, but you can choose values for custom parameters when you place a member. For example, with an angle iron factory, you select the iPart to use, and then modify certain values such as length, width, or thickness. You can modify only the values specified when the iPart factory was created.

Note: In custom iPart factories for sheet metal iParts, you cannot apply feature suppression and parameters to features added to flat patterns.

Storing Standard and Custom iParts

We recommend that you store standard IPart factories in a library whose path is included in your active project file. This path is called a proxy path.

The library folder must have the same name as the factory library, preceded with an underscore character. For example, if your factories are stored in a library named Bolts, define a library named _Bolts. Inventor automatically stores all iParts generated by factories in the library _Bolts. You can define multiple proxy paths to designate in your project. This technique is helpful if, for example, you want to group table-driven components by category. You can delete redundant paths (shown in red) in the project file.

If you do not specify a proxy path, Inventor creates the member file in a subdirectory of the folder that contains the iPart factory. For example, suppose you have an iPart called Bolt.ipt in C:\temp. When you place an iPart member in the assembly, Inventor creates the iPart member file in C:\temp\Bolt.

In contrast, custom iPart members can be stored anywhere other parts are stored; you specify a location in the Place Custom iPart dialog in assemblies.

Summary of Differences Between Standard and Custom iPart Members

iPart Behavior	Standard iPart	Custom iPart
Parameter values for member creation	Select from a list	Specify value (for custom parameters) or select from a list (for other parameters)
Location of member files	Determined when a subdirectory of the same name creates the file, or by proxy path	User-specified
Number of members	Finite; one member per row	Typically infinite; each row can produce multiple members based on different custom parameter values
Member reuse	Reused if available	Always newly created
Member editing? (Adding features to members)	No	Yes
Specify member file names through the iPart table?	Yes	No
Use Flat Pattern Edit Features?	Yes	No

Work Features in iParts

Work features are useful in iParts. In Inventor, work features are useful to constrain parts in assemblies and to create pins in electrical parts.

Create work features in a part before you transform it into an iPart factory. Then, in the iPart Author dialog, select work features to include or exclude in the iPart table. By default, all work features are excluded except pins (work points) in electrical parts and work features constrained with iMates.

Note: Work feature visibility is determined in the original part. It cannot be modified, but after you place an iPart member, you can use View

Visibility

Object Visibility to turn on and off work features globally.

About Sheet Metal iParts

Sheet metal iParts include more attributes:

specification of Sheet Metal Rule,
specification of Sheet Metal Unfold Rule,
optional specification of alternative, named flat pattern orientation,
optional individual control of bend order sequence designation on flat pattern members captured using the factory Member Scope option.

Taking advantage of these attributes requires more consideration when the sheet metal iPart is to include the suppression of features that eliminate bends and impact the bend order sequence.

When a sheet metal iPart factory is created, a default bend order is created. The default bend order depends on whether a flat pattern body exists within the sheet metal document.

If no flat pattern exists when the part is transformed into an iPart factory, each member row flat pattern receives the exact same bend order (accounting for feature suppression).
If a flat pattern exists when the part is transformed into an iPart factory, the existing bend order is copied to each resulting flat pattern member (accounting for feature suppression). Therefore, if a flat pattern is customized with a specific bend order before transformation to an iPart factory, the default (factory scope) bend order for each member has customizations already in place. By utilizing the member scope option to edit individual flat patterns, each flat pattern can have a unique bend order defined.

In the case of factory scope editing, the default bend order behaves identically to that of a regular sheet metal component flat pattern, but it may appear to behave differently within the context of the iPart factory. The flat pattern automatically manages the bend order based upon the visible centerlines (modeled or cosmetic) for the active member. Centerlines which are absent for a given member (due to suppression) release their bend order number to maintain a gapless sequence order on the remaining features.

Note: Sheet metal parts created before Inventor R2009, which are transformed into iPart factories using Inventor R2010 (or later), do not support bend order editing from within the iPart factory.

Tips for Creating iParts

We recommend that you create the part relatively close to its actual size. Then use dimensions to make the sketch geometry precise. You can edit dimensions when building the iPart table, if necessary.
After you create the basic part, use the Parameters command to rename system parameters and to create meaningful parameter names. Then use iPart Author to create the iPart factory. Named parameters are automatically added to the iPart table.
Parameters appear in the order in which they have been added to the iPart table. When you add parameters, give some thought to the order so that related parameter columns are grouped.
When creating an iPart factory, use Suppress and Unsuppress features to make significant changes between members. Add the features to the iPart table, and then specify the suppression status for the features in each row of the table.

Note: You can also specify a Custom Parameter Cell or Custom Parameter Column for each feature to compute or suppress. When the iPart is placed, you enter the needed suppression status.
In iPart Author, right-click materials, sizes, or other critical values in the right pane and designate as keys. Key numbers determine the nesting hierarchy in the model browser, but only key values are shown there.

Note: You cannot designate a column or cell as both a custom value and a key.
If you select the Material property from the Design Assistant Properties list, use the Material Column option on the Other tab to ensure that the current appearance is set to As Material.
To include part properties in drawings and bills of materials, include them in the iPart table, even if their values do not vary between members.