Configure Assemblies in Autodesk Inventor

IMAGINiT Tricks Tutorial: Learn how to prepare an iAssembly for the drawing environment.

Editor's Note: This tutorial courtesy of IMAGINiT Technologies.

I have been asked several times recently about how Autodesk Inventor handles configurations of assemblies at the drawing level. (These are known as iAssemblies and iParts in Inventor. If you are coming from SolidWorks or another modeling program and have no idea what an iPart or iAssembly is, then I recommend taking classes such as "Advanced Part Modeling" or "Advanced Assembly Modeling.") So, I decided it was time to dust off the F7 key and clarify the process.

Stop Wasting Time

First, we will need to turn all the parts that will have configurations into iParts. Try to do this before inserting them into an assembly that will later become an iAssembly. If the assembly already exists, you will have to replace the part with an instance of itself. Doing this will destroy all of the constraints that are associated to that part (cue sinister music).

Again, if the assembly already exists, this has to be done because when the part was originally placed into the assembly, there was no configuration table associated to the part. We need that table to create different configurations for the iAssembly. So, the workflow I suggest is to create the iParts first, then insert the iPart into the assembly. Do this to save time, re-work, and your all-important mental health.

All of This

Now that we have an iAssembly with all the configurations required, it is time to prepare for the drawing environment. Verify that you are on the Assemble tab and click on the BOM button in the Manage panel to view the current configuration. To view all of the configurations at once and make required iProperty changes, click the configuration pull-down and select All Members.



I find this is a great way to add missing iProperties and check that everything looks copacetic before moving on to the drawing environment. Confirming that all essential iProperty fields have been filled out in the BOM view will streamline the creation of the parts list at the drawing level.
 

Just About Done

I have three configurations in my iAssembly that I want to document on one tabulated drawing. After I drop in a couple of iso views of the different configurations, I will use one of them (it doesn’t matter which one) to create my parts list. By default the parts list will only show the current configuration of the iAssembly that was used to create the parts list, but we need to show all three configurations. (Hopefully your company template is configured properly and you are not rearranging or adding and removing columns every time a drawing is created.)

To show all configurations, either double-click on the parts list, or right-click on it and select Edit Parts List. Click the Member Selection button at the top of the dialog box. Check all configuration required for this drawing.



One adjustment that may need to be done on a case-by-case basis is renaming the columns for each configuration. To do this, right-click on the column header and select Format Column.


 

Rename the columns as required; I renamed mine 1138-01, 1138-02, and 1138-03.



You are now the proud creator of a tabulated drawing in Inventor. The parts list should now show every configuration of your iAssembly.



I hope this tutorial has shed some light on the process.