One of Inventor 2016 new commands is "Import". It allows the import of various types of CAD files into the Inventor part environment and then allows the referencing of the geometry into feature sketches. One of the key features of this process is that it creates an associative link to the imported CAD file. If the imported CAD file in opened and edited in its native application then saved, the Inventor model will request to make all sketch geometry, created from reference geometry of the import CAD model, to update. I only have access to AutoCAD so this is the imported CAD model I will demonstrate. I have tried it with SolidWorks and ProE models and the importing and referencing of geometry works great, but I do not have either of these applications to test the update function.
The "Import" function can be found in two locations in the part environment. These are shown below.
Selecting the function you are asked to browse and select the file you wish to import. You can change the CAD type as desired but it defaults to "All Models". If the file is an AutoCAD 2D file the next prompt is to select one of the part origin planes and then an origin point. Normally I use the Center Point because I know I can move it later if needed. The AutoCAD drawing appears and a notice about the associative link you are about to create.
Since it is highly unlikely that the AutoCAD drawing was places on the AutoCAD 0,0 point, you will notice that the drawing is also not located at the origin of the Inventor part either. For AutoCAD drawings, there is a "Translate" function to help you move the AutoCAD drawing to the required location. Of course it is not required to move the drawing, you can use the entities from where they came in. Right click in the imported AutoCAD drawing in the browser and select "Translate".
A two directional/rotational (2D/R) icon will appear. Two function options are also displayed in the head-up menu.
I made the Inventor Origin Center Point visible and then select the "Snap To" function of the 2D/R icon. When I select the Origin Center Point, the AutoCAD drawing will snap to the point centering it in my part model. You can use the Origin Center Point in the browser if you do not want to make it visible. You can also select either directional arrow or the rotational ball to enter exact movement. Select OK to finish.
Using either of these tools will give you the familiar reference geometry your are used to in earlier Inventor versions. Remember this reference geometry is associated to the original AutoCAD drawing. I have placed a reference dimension on the hole to track associative changes.
The associativity between the AutoCAD drawing and the Inventor sketch/model can be controlled in a similar fashion to a derived part. Right click on the referenced AutoCAD drawing in the browser and select either "Suppress Link" or "Break Link".