Inventor's iAssemblies (Avatech Tricks Tutorial)1 Sep, 2007 By: Allen Hudson
Built-in tools help you create drawing parts lists and tables easily.
Create an iAssembly
To begin, let's start with an assembly that has already been created and converted into an iAssembly. For more information about this functionality, read this Tech Tip available on Avatech Solutions' Web site.
Add Constraints, Name Parameter
To design this product, we needed several variations based on a distance between the center mounting eyelets. Because it is important, the Inventor assembly was constrained with this parameter in mind and a constraint was added with a distance value assigned. The parameter for this constraint is renamed Center Distance. To accomplish this task, select the Parameter button on the Panel Bar, find the parameter desired, click within that field, and enter text.
Select the Parameter button on the Panel Bar.
Enter text in the correct field.
You can confirm the status of the iAssembly by reviewing the browser to see if a table was created. By selecting each of the members listed, the product's design updates to reflect the specific configuration of that product. Note that three iParts in this design allow different components to be used in the product.
Confirm the status of the iAssembly.
Create a Drawing
Create a drawing with the desired views. Add a general dimension from centers of mounting eyelets at each end. Then edit that dimension by double-clicking on dimension, check the hide dimension, then enter text, and click OK.
Insert Parts List and Edit
Next, insert a parts list and show the different parts in each design variation. Start by selecting Parts List from the Panel Bar, select the view that you want the parts list to be built from, and then locate the parts list on the drawing. The next step is to edit the parts list to show more than one design. Locate your cursor on some text in the parts list, right-click, and select Edit Parts List. In the Parts List dialog box, select the Member Selection button. In the Select Member dialog box, place a check mark in front of each member you desire to be represented. Notice that in the parts list that there is a column for each product and that certain assemblies use different components.
Place a check mark in front of each member you want to be represented.
Note that in the parts list there is a column for each product.
Create and Edit Table Data for Dimensions
The other purpose of a chart drawing is to show different dimensional values without creating additional views or sheets. You can accomplished this goal by inserting a table and referencing the parameter that was created earlier. Select Table from the Panel Bar.
Select Table from the Panel Bar.
Select the view you wish to build the table from and then select the Column Chooser button. In the Table Column Chooser dialog box, you can then set your table to display your data. In this case, the member name is present as one of the columns, but Center Distance must be added. Select Center Distance from left column and then the Add button. Notice that Center Distance has been added to the Selected Column Fields. Now, select OK and place table on the drawing.
Add Center Distance to the table.
Place the table on the drawing.
As you can see, documenting a series of products on one drawing sheet is very simple. This best part of using this process is that as changes occur in the drawing, the parts list and table automatically update. Plus, you don't have to edit generic text, stretch lines, and mess with rectangles. It's all automated in Inventor.
In her easy-to-follow, friendly style, long-time Cadalyst contributing editor Lynn Allen guides you through a new feature or time-saving trick in every episode of her popular AutoCAD Video Tips. Subscribe to the free Cadalyst Video Picks newsletter, and we'll notify you every time a new video tip is published. All exclusively from Cadalyst!