Document Assemblies with Level of Detail21 Sep, 2011 By: Kevin Keene
IMAGINiT Tricks Tutorial: Suppress components and create views in Autodesk Inventor.
Editor's note: This tutorial courtesy of IMAGINiT Technologies.
Level of Detail (LOD) can be used for more than just large assembly management. Here, I'll explain how you can use an LOD to document your assembly.
Like most people, you've probably created an assembly that needed to be documented. And like most, you've probably run into the scenario where the full assembly has too much information for one drawing view, so you needed the ability to display only a portion of that assembly in your drawing.
There are several ways to go about this, and as I've made my way around to different companies, I've come across a variety of methods. One tool that I haven't seen used as much as it could be is LOD representations. LODs have often been used or talked about in the context of large assembly management, but they can be used in smaller assemblies as well. You can use them to both reduce the resource footprint of an assembly by suppressing components, and to create views that will be used in your documentation.
LOD views are created in your assembly file and you can create as many as needed. If you've never created one before, follow these steps:
When in your assembly file, click the + symbol next to the Representations folder. Right-click on the Level of Detail: Master line and select New Level of Detail.
You can then single-click on the new Level of Detail1 line twice to rename it, giving it a meaningful name that represents the parts being displayed. Once you have a name, simply right-click on the unneeded components and suppress them, then save your assembly. That's all it takes.
Once the file has been saved, you can activate any of the LODs that you created to switch back and forth between the views. If you need additional views, just repeat the process again, this time choosing other objects to suppress.
Once you have your new LODs defined in your assembly file, you can use them in your documentation. Start a new drawing file, then start the Base View command, and you will see the LODs displayed in the middle of the Drawing View dialog box. Here, you can select which LOD you want to use.
In my example, I created six LODs for my assembly, and placed all six views on a single sheet in my drawing file. I then renamed my views and turned on the visibility of the View Label.
You can use your LODs on the same sheet (as in this example), on separate sheets in the same drawing, or in separate drawings. The nice thing about these views is that when you right-click on the view and choose Open, the assembly file will open directly to that LOD.
By default, the Parts List will display all of the components regardless of the LOD you selected for your view, but there is a way to display the correct items. Once you have added balloons to your view, you can add a parts list based on that view, and then use the Filter option to display only the components that have balloons.
Note: Data sets used in this tutorial are from Autodesk.