iPart fundamentals

Most designers have parts that differ by size, material, or other variables, although the same design works in many models. You can create these designs as iParts, and then use one or more of the variations.

You use the iPart Author to create part families that contain a table. For standard iParts, each iPart variation is an iPart member, which is defined by a row in the table. When placing the part in an assembly, select the row (member) needed.

In general:

• Start with a new or existing part or sheet metal part.
• Determine the portion of your design that changes with each member.
• Use the Parameters command to rename parameters, establish equations, and create user parameters.
• Use the Create iPart command to define one or more table rows that represent members of the iPart factory, specifying variations of its parameters, properties, thread information, iMate information, feature suppressions, and work features.
• For sheet metal iParts variations of the Sheet Metal Rule, Sheet Metal Unfold rule and Flat Pattern orientation can be defined.
• Save the part, which is automatically saved as an iPart factory.

Tip: Optionally, create only one row in the iPart table, and then add additional rows by editing the spreadsheet. You can take advantage of copying and pasting, formulas, and other spreadsheet commands.

Workflow for iParts

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

In part authoring, you design the part and define all of its variations. You create a row in a table for each possible version. Each version, called a member, is stored in an iPart factory.

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

In part placement, choose a row in the table to represent the appropriate version. An iPart member is generated, using the values in the table row, and inserted in your assembly like any other component.

Types of iParts

There are two types of iParts:

• A Standard iPart Factory defines all values in columns. When you publish an iPart using a standard iPart factory, the member parts cannot be modified after placement.
• A Custom iPart Factory contains at least one column identified as a Custom Parameter Column. When you publish an iPart using a custom iPart factory, the custom parameters in the member parts can be modified when the iPart member is placed. You can add features to a custom iPart member.

Note: Feature suppression and parameters cannot be applied to features added to flat patterns in custom iPart Factories for sheet metal iParts.

Information to include in iPart

You can include:

• Parameters. Use the Parameters Editor to rename parameters, establish equations between parameters, and create User parameters.
• Properties, so that you can include information such as part number, stock number, and material. Your bill of materials and parts list are automatically kept up to date.
• Threads, including different thread families, designations, classes, direction, and pipe diameter.
• iMates, specifying which should be included or suppressed, offset values, matching names, and sequence number.
• Work features, including which should be included or excluded and visibility status.
• Feature Suppression status. Using feature suppression, you can include several configurations of a single part in one file. For example, one configuration of the part may have an extrusion with a cut, while another has an extrusion with a join. Sheet metal iParts can have feature suppression applied to features that were added to the flat pattern making individual flat patterns unique for iPart member files.
• iFeatures and table-driven iFeatures. You can specify which inserted 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.
• Sheet Metal iParts can include: the Sheet Metal Rule, the Sheet Metal Unfold rule and the Flat Pattern orientation.

Where to store iParts

Standard iPart factories generate parts that have fixed values. Because these parts are reused in many assemblies, we recommend that you store them in a library whose path is included in your active project file. This path is called a proxy path.

The library directory where you want to save the iParts 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, you can define a library named _Bolts. Autodesk Inventor automatically stores all iParts generated by factories in the library _Bolts. You can define multiple proxy paths, and you can designate them in your project. This technique is helpful if, for example, you want to group table-driven components by category. Redundant paths are shown in red. You can delete these in the project file.

You are not required to specify a proxy path. When iPart members are placed in the assembly, Autodesk Inventor creates a subdirectory in the same directory that contains the iPart factory. For example, consider you have an iPart called Bolt.ipt in C:\temp. When you place an iPart member in the assembly, a subdirectory called Bolt is created (C:\temp\Bolt), and the iPart member file is created there.

Custom iPart members always are stored in a location specified using Browse in the Place Custom iPart dialog in assemblies.

Differences in standard and custom iParts

When creating an iPart factory, you determine whether or not parameters can be modified when an iPart is placed in an assembly. Parts created from standard iPart factories cannot be modified. Parts created from custom iPart factories can have designated parameters modified when placed.

Standard iPart factories, such as bolt factories, are not edited. Because bolts are parts that do not change, you select the individual iPart member to use, but you do not edit any values. Usually, standard iPart members are stored in a library. By default, files for standard iPart members are located in a folder of the same name as the factory or in a location designated as the proxy path. For more information, see the section Where to store iParts in the Use iParts in assemblies topic.

If an iPart member is created already, successive placement of the iPart member in an assembly reuses the member file. If a key determines the selection criteria for an iPart member, meaning that the member is defined by fixed values from the factory table, then the 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.

Custom iPart factories are not edited directly, but you can choose the value for custom parameters when you place a member from the factory. For example, with an angle iron factory, you select the iPart to use, and then modify certain values such as length, width, or thickness. Only the values specified when the iPart factory was created can be modified. Custom iPart members are usually specific to a particular assembly and can be stored anywhere other parts are stored.

Note: Feature suppression and parameters cannot be applied to features added to flat patterns in custom iPart Factories for sheet metal iParts.

The location of files created for custom iPart members is based on the path specified using Browse in the Place Custom iPart dialog box. With custom iPart members, you can input a custom value not contained in the table. Custom iPart member columns appear with a blue background in the iPart factory. You can edit custom iPart members by adding additional features, sketches, and so on. It means that two custom iPart members produced with identical parameters can be different.

Differences at a glance between standard and custom iPart members:
iPart Behavior	Standard iPart	Custom iPart
Parameter values for member creation	Select from a list	For custom parameters, typically you can specify any value. For other parameters, you select from a list.
Location of member files	Determined when the file is created by subdirectory of the same name 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

Behavior of work features in iParts

Work features are useful in iParts 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, and then determine which work features to include or exclude in iPart members.

In the iPart Author dialog box, work features have default Include or Exclude settings. You can override the setting by selecting work features to include or exclude in the iPart table. Each row can have work features Included or Excluded. Default settings are:

• Work features constrained with iMates are Included.
• Pins (work points) in electrical parts are Included.
• All other work features are Excluded, except the features constrained with iMates.

For standard iParts, each row in the iPart table represents a member. A column for each work feature indicates whether it is included or excluded. You can modify the setting for each row in the table.

Note: Work feature visibility is determined in the original part and cannot be modified, but after you place an iPart member, you can use ViewVisibility Object Visibility to turn work features on and off globally.

Sheet metal iPart factory considerations

Sheet metal iParts include additional 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.

Effectively taking advantage of these attributes requires additional consideration when the sheet metal iPart is to include the suppression of features which eliminate bends, thereby impacting 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 already exists within the sheet metal document.

• If no flat pattern exists when the part is transformed into an iPart factory, each member row’s flat pattern receives the exact same bend order (accounting for feature suppression) upon generation of the flat pattern.
• 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). This means that if a flat pattern has been customized with a specific bend order prior to 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.

Suppressed Features Within Members - 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 prior to 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 iPart factories

• Determine the part of your design that changes with each version.
• After you create the basic part, use the Parameters command to rename system parameters and to create unique parameter names. Then use the iPart Author command to create the iPart factory. Named parameters are automatically added to the iPart table.
• 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 iPart table.
• In the iPart Author, right-click materials, sizes, or other critical values in the right pane and designate as keys. Only key values are shown in the model browser. Key numbers determine the nesting hierarchy, such as key 3 is nested under key 2, which is nested under key 1.
• Default document units are used if you do not specify a unit of measure in a table cell.
• 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.
• To include part properties in drawings include them in the iPart table, even if their values do not vary between members.
• Place standard iPart factories in a library and include the library path in your project file.

Publish DWF data

Publishing from an iPart factory produces a DWF file containing an iPart table. Activate the iPart table in the browser, and then use Save As Save Copy As. Specify the DWF file type and appropriate options.

Note: Publishing a sheet metal iPart member can now include a flat pattern. Publishing a sheet metal iPart factory can include all folded and flat patterns for all members in addition to the iPart table.