How to Include a Dynamic Part Number in the Part Drawing View Label

There are various methods of detailing machine parts in Inventor.  Some companies use the method of one part per drawing while others desire to place multiple part details on one drawing.  A common practice is to place part detail drawings as sheets under the top level assembly drawing.  When the decision to place multiple part details on one drawing is used, Inventor needs to be configured to place a unique view label for each part to avoid confusion by fabrication personnel.  This view label must also be dynamic so if the part being detailed is changed, the view label will update to reflect the new part information.  Below is an example of this type of drawing showing view labels containing the part number of each placed part.  The configuration of Inventor to place a dynamic view label, containing the part number, is the focus of this article.

The process beginnings with the editing of the drawing template and the controlling Design Data, sometimes referred to as the Styles Library.  This article will not go over the process of creating a set of Inventor templates and their matching Design Data but it will cover the drawing style configuration, contained in the template, to accomplish our goal.  A drawing template is configured to follow a defined Active Standard as shown in the Document Settings dialog below.  If you open one of your Inventor drawings and choose Document Settings on the Tools tab under the Options panel, you will see the this active standard.  It is coming from the Design Data folder which is defined either in the Inventor Project File or in the Applications Options.

For demonstration, I will be modifying the Design Data for a single demo drawing which will not be permanent for all future drawings.  To make it a permanent setting, the Design Data library must be edited.  For this one drawing I select the Styles Editor command which can be found under the Manage tab on the Styles and Standards panel.

In the Styles and Editor dialog box, I select my Standard then the View Preferences tab.  Notice that the editor is in Read Only mode since I am only editing this one drawing.  

The View Label Defaults is the area where I can configure the information that will be included in my base view label.  The first thing I will set is which model property will be displayed in the view label.  In the Display panel you will notice the standard Inventor view label configuration.  Selecting the "pencil" icon will display the following dialog box.  Follow the numbered steps to replace the default <VIEW> entry with the model property "Part Number".  Select "OK" to finish.

Next I will leave the View Type on "Base" since I want the view label to be automatically placed  on the base view of each part.  Last I will choose the position of the view label and select the Visibility icon to make the bulb "light" indicating that the view label will be displayed.  I finish by selecting Save to exit the Styles Editor.

When I place the base view of my part along with any projected views and select OK the view label appears under the base view.  At this point you can drag the view label to a different position if desired.  If the base view is moved, the label will follow it.

If I wanted to add "PART NUMBER" to the label entry, I simply add it as text in the Display dialog box.

To prove this part number is dynamic, I will use the "Replace Model Reference" command to replace the part in the drawing view.  This command is located on the Modify panel under the Manage Tab while in the drawing.

As you can see, if this modification was made to the Design Data library for all drawings it will make the management of multiple part drawings a lot easier.