To Work with iProperties in Files or Templates

What's New: 2020.1, 2021.1, 2022

Every Inventor file has a set of file attributes called iProperties. If the file has more than one Model State, each Model State can have unique iProperties.

When you create models states, it is important to be aware of the edit scope status. If Edit Member Scope is enabled, changes to iProperties are applied only to the active member. If Edit Factory Scope is enabled, changes to iProperties are applied to all members.

You can toggle between Edit Member Scope and Edit Factory Scope in the browser by clicking the pencil icon at top of the Model States browser entry.

Use iProperties to classify, manage, and search for files, to create reports, and to automatically update title blocks and parts lists in drawings and bill of materials in assemblies. When searching for files, Find uses iProperties to locate files.

Tip: With Spell Check enabled (Application Options dialog box/General tab), Inventor checks spelling automatically as you type in any text field in the iProperties dialog box.

Spell Check is disabled in the iProperties dialog box when accessed outside of Inventor, for example, from File Explorer.

Set file or template iProperties

1. Open the iProperties dialog box in one of the following ways:
   • Click File iProperties to display the Properties dialog box for the active file or Model State.
   • Right-click a referenced file in the browser, and then select iProperties to display the iProperties dialog box for the active Model State.
   • Activate a Model State and then right-click the Model State in the browser to display the iProperties dialog box for the active Model State.
   • In the browser, select multiple files, right-click, and then select iProperties to display the iProperties dialog box.
   • Open Design Assistant: Click File Manage Design Assistant.
   • In Design Assistant, click File Open File or Open Folder. Right-click a file in the browser, and then select iProperties.
2. In the Properties dialog box, click the Summary, Project, Status, or Custom tab and set the values for the properties that you use.

   Only the settings on these tabs are used to search files and update information in bills of material, parts lists, and other information pieces.

Note: Depending on the type of file and the method you used to open the dialog box, additional tabs may be displayed.

Always save any open Autodesk Inventor files before using Design Assistant to change iProperties.

Copy iProperties into drawing

You can copy values of model iProperties to a drawing. If you copy the iProperties to a drawing template, they are accessible to drawings created from the template.

1. Open the drawing and click Tools tab Options panel Document Settings .
2. On the Drawing tab of the Document Settings dialog box, click Copy Model iProperty Settings.
3. In the Copy Model iProperty Settings dialog box, select Copy Model iProperties, and then select iProperties to copy to the drawing.
4. Click OK to close the Copy Model iProperty Settings dialog box.
5. Click Apply and OK to save the document settings and close the Document Settings dialog box.

When you place the first drawing view, the selected iProperties are copied to the drawing from the referenced model file, overwriting any existing drawing iProperties.

Note: Model iProperties are copied and updated from a source model. The source model is always the top model from the first drawing view on the first drawing sheet.

Tip: Copied iProperties are not associative so they do not update when the source file is updated. Click Manage Update Copied Model iProperties to update the iProperties in the drawing.

Create or edit expressions for iProperties

You can create and edit expressions for text type iProperties in the Properties dialog box. An expression contains a combination of custom texts and Parameter and iProperty names enclosed by brackets. The Parameter and iProperty names are substituted by the Parameter and iProperty value, when the expression is evaluated. The iProperties fields that include an expression, are marked by the expression icon , and the tooltip shows the current expression.

Note: Expressions are created for text type iProperties only. Expressions are not evaluated mathematically and cannot be used for numeric or date iProperties.

The Properties dialog box displays iProperty entries and evaluated values of iProperty expressions. iProperty fields which contain expressions, are marked by the expression icon. The actual expression is shown in a tooltip if the mouse pointer pauses over the iProperty field.

1. Open the iProperties dialog box in one of the following ways:
   • Click File iProperties to display the Properties dialog box for the active file.
   • Right-click a referenced file in the browser and select Properties to display the Properties dialog box.
   • Right-click a Part, Assembly, or Drawing in the Model browser, and select iProperties.
   • Right-click a Part or Drawing in the Model browser, and select iProperties.
2. In the Properties dialog box, open the Summary, Project, Status, or Custom tab and click at the field where you want to create an expression.
   • To edit an existing expression, right-click in the field and select Edit Expression. The equal sign displays when the expression can be edited.
3. Insert the equal sign, if not already present, and then create or modify the expression. Enclose each Parameter and iProperty name in brackets.
   • Example expression:

     =DIN1026 - U 140 x <G_L>

4. The expression is evaluated after you click Apply or press Enter.
   • Evaluated example expression if G_L = “XYZ”:

     DIN1026 - U 140 x XYZ

Note: iParts, iAssemblies, and Content Center ignore the expressions (formulas) saved in Properties.

Note: iParts ignore the expressions (formulas) saved in Properties.

Tips:

• You can create a template file with pre-defined expressions for iProperties to unify your parts lists, or other documentation.
• Use the Property Expression builder in the Bill of Materials dialog box to create expressions for iProperties. See Edit bills of materials for more information.

Important: The units for the values "Flat Pattern Length", "Flat Pattern Width" and "Flat Pattern Area", only honor cm units even if you specify a different value in Document Settings. To change the units for flat patterns to a unit different than cm, you must use the following strings in the iProperties > Custom tab dialog box and specify a different unit:

• =<Sheet Metal Length>
• =<Sheet Metal Width>
• =<Sheet Metal Area>

To make the units for flat patterns different than cm, you must first create a sheet metal part with a flat pattern, and then create the sheet metal expressions in the iProperties/custom tab dialog box. For example:

1. In the Documents Settings/Units dialog box, specify the desired default units.
2. On the custom tab, in the value tab enter: =<Sheet Metal Length>
3. Click Add.
4. Close and then re-open the iProperties/Custom tab dialog box.

   The values display

5. 

Note: You can also create an iLogic rule to create custom units for flat patterns.

Instance properties are properties assigned to individual component instances that are stored in the parent assembly. Unlike iProperties, instance properties don't affect the referenced component files. Instance property values have a higher priority than the values of custom iProperties. When a custom iProperty exists and you create an instance property of the same name, instance property covers the custom iProperty. To learn how to work with instance properties, see To Work with Instance Properties.