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 model 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.
Spell Check is disabled in the iProperties dialog box when accessed outside of Inventor, for example, from File Explorer.
Open the iProperties dialog box in one of the following ways:
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.
Always save any open Autodesk Inventor files before using Design Assistant to change iProperties.
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.
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.
Custom properties added to the Custom tab can be copied between documents. More than one property can be copied and pasted.
When pasting properties into another document, if duplicates exist, you are prompted for the action you want to take:
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.
Open the iProperties dialog box in one of the following ways:
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.
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>
The expression is evaluated after you click Apply or press Enter.
Evaluated example expression if G_L = “XYZ”:
DIN1026 - U 140 x XYZ
Tips:
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:
In the Documents Settings/Units dialog box, specify the desired default units.
On the custom tab, in the value tab enter: =<Sheet Metal Length>
Click Add.
Close and then re-open the iProperties/Custom tab dialog box.
The values display
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.