Work with iProperties in files or templates

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

Set iProperties in Autodesk Inventor files or templates

1. Open the iProperties dialog box in one of the following ways:
   • Click iProperties to display the Properties dialog box for the active file.
   • Right-click a referenced file in the browser, and then select Properties to display the Properties dialog box.
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.

Use Design Assistant to set iProperties

Use Design Assistant to set iProperties without opening the file in Autodesk Inventor.

1. Open Design Assistant using one of these methods:
   • Click Manage Design Assistant
   • Click the Start menu, then click Programs Autodesk Autodesk Inventor Design Assistant.
2. In Design Assistant, click File Open File or Open Folder. Right-click a file in the browser, and then select iProperties.
3. In the iProperties dialog box, click the Summary, Project, Status, or Custom tab and set the values for properties.

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

Additional property tabs may be available, depending on the file type and the method used to open the dialog box.

Note: If you open Design Assistant from Microsoft Windows Explorer and change the iProperties of a file that is open in Autodesk Inventor, you can lose unsaved changes. 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 iProperties in the Properties dialog box. An expression can contain a combination of custom text and Parameter and iProperty names enclosed by brackets. The Parameter and iProperty names are substituted by the Parameter and iProperty values when the expression is evaluated.

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 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.
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.

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.