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.
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.
There are two types of iParts:
You can include:
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.
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 are iParts stored? in thetopic.
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.
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:
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
Number of members
Finite; one member per row
Typically infinite; each row can produce multiple members based on different custom parameter values
Reused if available
Always newly created
Member editing? (Adding features to members)
Specify member file names through the iPart table?
|Use Flat Pattern Edit Features?|
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:
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.
Sheet metal iParts include additional attributes:
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.
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.
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.
A good candidate for an iPart factory is a basic part you use often in different sizes, materials, or mounting configurations. When you transform a part to an iPart factory, you define the parameters and properties that must change for each part.
You can also create a table-driven iPart and use it to create a table-driven iFeature if the entire part is going to be used as an iFeature. Use the Extract iFeature command to save the iPart as an iFeature. Once the table-driven iFeature is saved to the catalog location, use the iFeature Author to make changes to the table.
In the iPart Author table, you define individual members of the iPart factory by specifying its values. 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.
In previous versions, legacy iParts concatenated Key values to create a file name. Now, 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 box to set up a different naming scheme, or enter a new name in the member cell.
You can create afactory or a factory.
It is a good idea to create the part relatively close to its actual size and then use dimensions to make the sketch geometry precise. You can edit dimensions if you need to when building the iPart table.
If you know that you want the part to be a part factory, create parameters with meaningful names as you add dimensions. For example, in the dimension edit box, type in Length=75mm. The sketch length will change to 75mm, and a parameter will be created and added to the table with the name of Length.
Parameters appear in the order you add them in the iPart table. Give some thought to the order you add them so that related parameter columns are grouped .
If you did not rename the parameters, add them to the table individually.
To remove a parameter, click the parameter in the right pane and then click the Remove arrow.
The Member Name column automatically generates unique names to distinguish each iPart member.
If you alter the member name from the default, it alters the file name.
In the right pane, right-click an attribute and select Key. Click the arrow and select the number to specify the order. For example, if you always select a part by its length, and then its width, designate length as Key1 and width as Key2.
You can continue to add rows and columns as needed. Consider editing the table in a spreadsheet so you can take advantage of functions such as copy and paste, formulas, and sorting.
For more information, see the Edit the iPart spreadsheet section in.
A custom column or cell is indicated by a blue background.
Sheet metal parts can include features added to the flat pattern. When such a part becomes a custom iPart factory these flat pattern features cannot be:
Custom iPart Example: Calculate custom parameters in Microsoft Excel
Setting a column to Custom means that you are able to set the value independently of the iPart table for that member.
You can use custom parameters to calculate values in the iPart table. Cells and columns calculated in Microsoft Excel have a red background when viewed in the iPart table.
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In the iPart factory, a column was added using the Description property.
Using a Microsoft Excel formula in the Description column, each iPart version was automatically calculated.
Consider the iPart example shown previously:
This formula retrieves the values in columns A, B, and C and calculates results in the Description column. Using your values and units, the results look like the following formula:
2 mm x 10 mm x 50 mm
Each member of the iPart is calculated separately.
After you have created member rows in the iPart factory, you can generate the files.
When creating an iPart factory, you select the parameters or properties to define the published iPart. In the iPart Author, each column contains a parameter or property. Each row represents a unique version of the part. To modify the iPart factory, edit in the iPart Author table or in an embedded Microsoft Excel spreadsheet.
Use Excel to incorporate spreadsheet formulas, conditional statements, and multiple sheet data extraction.
Values calculated by equations in the spreadsheet are shown with a red background in the iPart table.
Autodesk Inventor includes the Thread.xls spreadsheet in the folder. The Application Options and/or project settings can affect the file's location. The column headings match the labels on the Specification tab of the Thread feature dialog box. If you prefer, you can use the spreadsheet to create or edit thread parameters included in an iPart factory.
Use the Bend Order command within the Flat Pattern model state to redefine the bend order sequence using one of two automated techniques: directed or sequential as well as a completely manual bend order method. By default, Inventor sets the iPart capture mode set to ‘Factory Scope’ for every iPart factory that is created. This is expected to be the primary workflow. A single (default) bend order is assigned to all centerlines (modeled or cosmetic) that are available within any of the folded members. In this capture mode, any contextual bend order changes applied to a member file’s flat pattern is applied to all member flat patterns within the factory.
Member Scope Editing
Only one method allows the assignment of an individualized bend order to a flat pattern member (verses the factory’s generic default order): setting the factory’s edit mode to ‘Member Scope’ (using the iPart/Assembly panel). Once a sheet metal iPart factory is set to ‘Member Scope’ any bend order changes made within the flat pattern is captured and persisted exclusively for the active member.
The iPart Author transforms a part to an iPart factory. For standard iParts, each row in the factory table represents a unique member, whose variations are specified in columns. Data of several types is specified on tabs and added to the table as column in the order specified.
The iPart Author specifies the attributes of a part that change with each member.
TipAlthough it is not required, edit the part before creating an iPart and use the Parameters tab to rename parameters. Renamed and user parameters are automatically added as columns in the iPart table.
Information to include in an iPart is selected on tabs, according to the type of data.
Shows part attributes, according to the selected tab. Click to select parameters, properties, or other values and then click the Add arrow to add to the selections list or the Remove arrow to remove it.
Shows selected values and adds a column in the iPart table. Specifies keys to represent the nesting order in the part browser and on the Key tab of the Place iPart dialog box. Only columns designated as keys are shown in the browser.
Right-click an attribute and select Key such as material or size. In the iPart table, a key icon in column headings identify designated values.
Select the Key order to set the nesting order. For example, if you select an iPart by its length, and then its width, set Length as Key1 and Width as Key2.
Contains columns in the order selected. Some cell or column settings can also be specified in the right pane.
Member is automatically created as the first column. Its default value is the file name, indexed per member, such as bolt-01, bolt-02, and so on. For more information about Member Name and Part Number, click to see
If you rename a member from the default file name, a prompt reminds you that a name change alters the file name and asks you to confirm.
NoteThe Member column is the default file name column. If you remove the file name setting, the member file name is based on key names. Key names can result in long file names as all key names are concatenated in the file name.
Rows represent individual iPart members. Right-click to specify:
Columns indicate the values that are unique for each iPart member. Right-click to specify:
Options opens the Options dialog box. You can create or edit part numbers and member names. For more information about Member Name and Part Number, click to see
Verify checks the table for cell values that are not valid for the column type, improper column headers, and if numeric values have correct units. Cells with errors are highlighted with a yellow background.
Specifies the attributes used to define an iPart factory. A row is added for each iPart member, with values specified to differentiate among variations.
The number of columns in an iPart is limited to 256, but usually variations that differentiate among members are limited to a few columns. Columns are added to the iPart table in the order selected.
Contains parameters specified when the part was created, such as features, dimensions, renamed parameters, and custom parameters.
Renamed and custom parameters are automatically added as columns to the iPart table, but other parameters can be individually selected.
Lists summary, project, and physical properties. If an iFeature with Custom properties is present, the iFeature custom properties are included. Properties can be used in drawings and the bill of materials. Useful properties can include:
Specifies individual features to compute or suppress. When creating the part, suppress features and add additional features that define members, such as a cut or extrusion. Using this method, you can include multiple variations of a part in one file, and then specify the compute or suppression status of each feature for each member in the iPart table.
Depending on the amount of discretion you want to allow when the part is placed, you can:
|Specifies table driven iFeatures to include in the iPart table. When included, a unique iFeature row can be specified for each iPart row. You can specify the suppression status for the iFeature in each row of the iPart table.|
Specifies individual iMates to include in an iPart member. You can include or suppress, set offset values, specify matching name, and sequence number.
Specifies work features to include in an iPart. For electrical parts, work points that represent pins are included by default. For non-electrical parts, work features are excluded by default, except the features with associative iMates.
When included in a member, a work feature has the same visibility setting as in the original part. Consider:
Specifies thread parameters for each iPart member. Define columns for each regular or tapered thread parameter. Include all parameters that may vary to match the replacement thread. For example:
Thread1:Family="ANSI Unified Screw Threads" Thread1:Designation="7/16-14 UNC"
Thread1:Family="ANSI Unified Screw Threads" Thread1:Designation="7/16-18 UNS"
In most cases, this iPart would fail because the Thread1:Class was not added to the table. In the existing thread, three classes are available: 1A, 2A, and 3A. In the replacement thread, only 2A is available. Unless the specified thread is a complete match (both are 2A), it fails because a thread feature cannot be generated.
In this case, select the Class parameter in addition to Family and Designation to prevent this error:
Thread1:Family="ANSI Unified Screw Threads" Thread1:Designation="7/16-14 UNC" Thread1:style-class="1A"
Thread1:Family="ANSI Unified Screw Threads" Thread1:Designation="7/16-18 UNS" Thread1:style-class="2A"
Specifies the optional inclusion of: Sheet Metal Rule, Sheet Metal Unfold (if needed due to being different from that specified in the Sheet Metal Rule) and a named Flat Pattern Orientation as columns in the iPart Factory table.
Creates custom column headings in the table, such as cost per unit, that do not control size or placement of a member. Values can contain text or numeric data.
In the Prompt section, adds a prompt for placement instructions or other information.
Optionally defines a convention for setting part numbers and member names for members of the iAssembly factory. A Member Name column is automatically created for each member and has a generated name, based on settings for part number and member name.
Do Not Set
Set to Value
Establishes a custom value; the default is the factory part number.
Set to Member Part Number
Available only if Part Number Set to Value is specified.
Set to Factory File Name
Specifies each member name as the factory file name, automatically incremented by row. Default setting.
Set to Value
Allows entry of a custom member name.
Select the check box to activate Separator, Initial Value, Step, and Digits.
Sets the character used to precede incremental member numbers. The default is a hyphen.
Sets the first member value. The default is 1.
Sets the increment between members. The default is 1.
Sets the number of significant digits. The default is 2.
Displays format of preferences.
In the table, right-click a column, and then select Custom Parameter Column. Right-click again, and then select Specify Range for Column.
Sets minimum, default, and maximum values for a Custom Parameter column.
Click the arrow to select the limit (less than or equal, or no lower bound). If less than or equal, enter a value to represent the bottom end of the range. This value must be less than the default or maximum.
Shows the current value of the parameter. This value must be greater than the minimum and less than the maximum.
Click the arrow to select the limit (less than or equal, or no upper bound). If less than or equal, enter a value to represent the top end of the range. This value must be greater than the default or minimum.