Linking Named geometry to callouts on drawing
What do you mean by 'link'? Are you wanting the 'callouts' to be automatically created and arranged around the model when you first place a view, or just the ability to have them be created after the view has been placed?
To have them be automatically created as you place the view would be a fairly big project, because it would likely need to be set-up in an Inventor Add-in, due to it's need to be active in the background, waiting/listening for that specific event (view placement) to happen, then do something very specific when it happens.
Which version of Inventor do you have. I think the NamedEntities interface became available in one of the the Inventor 2019 updates, although some of the 'behind the scenes' capability pre-existed that interface. And some model annotations became available around the same time. Then those model annotations could be retrieved into your drawing view. One idea might be to attach Leader Text notes to the model in the part with the entity name, then after placing the view in your drawing, retrieve the model annotations. When you assign names to model entities in the model, it appears to create 'call-out' notes, but those won't be retrieved by the 'retrieve model annotations' tool in the drawing, they are simply visual aid that can be turned on/off.
Wesley Crihfield
(Not an Autodesk Employee)
The model annotations are only available within Part documents, but those annotations can also be directly accessed and set to visibility on/off within its model tree (as long as you have Object Visibility setting for "Component 3D Annotations" turned on in the assembly (can be annoying though).
With a part open, go to the "Annotate" tab of the ribbon. Then click on the Leader Note tool. It will then be waiting for you to select model geometry to attach it to. Your view orientation at this stage may be important, because since this is a 3D annotation, it needs an annotation plane to reference, and it will attempt to use one that best suits how you are looking at the model (defaults to closest parallel origin plane). Once you place the note, as usual it prompts you to enter some text for it. This uses the same "Format Text" dialog box as used in a drawing, so iProperties and Parameters are available as drop-in references, but unfortunately named entities isn't an available drop-down list, so you will have to enter the entities name manually.
Now in the drawing document for that part, after you have placed a view, there are two ways to get to the 'retrieve model annotations' tool. The ribbon way: go to the "Annotate" tab, then click on the "Retrieve Model Annotations" tool. The more convenient way: simply right-click on the view, then choose "Retrieve Model Annotations..." from the right-click menu. Once the dialog box is showing, click on the "3D Annotations" tab within, then make sure the check boxes next to the appropriate options are checked, then click "OK" button. If more annotations are being shown than you want to retrieve, simply select which ones you want to keep before clicking the OK button, or just delete the ones you don't want afterwords.
Wesley Crihfield
(Not an Autodesk Employee)