Inventor 2018 Hole Annotation - It's Your Choice

Autodesk introduced Model Based Dimensions (MBD) for part models in the 2018 release and for assembly models in the 2018.1 update for subscription customers.  If you have used this new functionality you have found it to be lacking is a some areas and the operation needs to be polished in others.  If you agree with me, take a look at this Inventor Ideas post and give it a "Vote Up".

This article is to demonstrate two methods of applying Hole/Thread Notes to a part model with my main focus on how to overcome the lack of the hole count being included in the call out.  This is a standard function in the 2D drawing and it should be added for all multiple hole call outs in the part model.  My sample part consist of multiple holes and types.  Some of the holes are patterns which some are simple placed on multiple sketch points. 

The first method is to use the "Hole/Thread Note" command and  manually add the hole count during placement.  This method requires you to know the total number of holes of the type you are placing the note.  The application will not count them for you.  This means if you have similar types of holes, you will have to be sure and count accurately.  For example if there were four (4) 1/4" drill holes and two (2) 17/64" drill holes you may have a hard time telling them apart to get an accurate count especially if you did not create the part.

After selecting the hole and placing the call out, the configuration dialog is displayed.  Select the indicated icon to bring up the Edit Hole Note dialog box.

You will notice that the "Hole Count" icon is unavailable.  Position your cursor on the hole text and type in your desired count indicator.  Select "OK" to return to the hole configuration screen, verify and then place the hole note on the model.

The second method requires a little more hole note configuration but it has the advantage of placing the hole count automatically on the hole note.  You will be using the "Tolerance Feature" command to place hole notes.  The first tolerance feature you need to place is a "datum" on the surface the holes originate from.  When selecting the type of tolerance feature to place use the "Planar Surface" note, it is the simplest.  I will be hiding this note anyway.

I next will select this tolerance note in the browser and turn off the visibility.  This is your choice but since all I needed to establish was a datum surface, I can turn it off.  Next select the "Tolerance Feature" command and select a hole.  If there are more than one hole of the type you selected, it will highlight them all and give you a list of the arrangement it found.  I selected a counter-bored hole, one of four, and in the drop down list, I will choose "Multi-Element Hole Parallel Axes Pattern" to pick up the clearance hole and the counter-bored hole.  These selections will vary depending on the type of hole you select.

Next, I will select the "OK" icon.  Because this is a counter-bored hole, the command will prompt me to select the "Reference Feature".  Select the face you earlier place the datum surface which is the same surface the holes were place on.

Once you do this, you can place the hole note and bring up the hole note configuration screen.

The next steps are optional depending on the information you wish to display.  I do not want the datum to show so I will un-check the "datum" icon.

I do not want the GD&T call out so left click on the GD&T position symbol and then select "Remove Feature Control Frame".  Last I select "OK" or "+" if I need to add more hole call outs.

Even though this method is a little more work, it automatically counts the number of similar holes on the face.  Also, if you go back and select the hole call out, all the matching holes are highlighted in the model.

I am hoping Autodesk will add this hole counting feature to the "Hole/Thread Note" command in a future release or update.