Hole Table does not populate

[Swarfmaker]

In this latest update 'hole table' has appeared.  Useful for something I am just doing I thought.  A simple plate (single body component) with a number of holes, so in 'Drawing' mode I select 'Hole table' and follow the sequence outlined in the update blurb.  Identify a reference point and all I get is a table header - no information about the holes.  I can't find a way to populate the table - what might I be doing wrong?

[jhackney1972]

Please attach your model and we will try and find out.  We do not need the drawing, just the model you are making the drawing from.  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section of a forum post to attach it.

[Swarfmaker]

Hi @jhackney1972 ,

Please find attached file:

I appreciate your taking the time & trouble to respond.

Many thanks,

Fred

[jhackney1972]

The reason the hole table function does not work on your model is because you did not use the Hole command to create any of the holes in your plate.  They are all sketched and extruded holes.  For the hole table to work, the holes must be created using the Hole command.  This is also true to use the Hole Leader command in the 2D drawing also.  

[jhackney1972 · Accepted solution]

I did not have the opportunity to do a demo earlier so I took your model, used the same sketch centers for two holes to use the Hole Command.  I then made drawing added a Hole Table. 

[Swarfmaker]

Thank you @jhackney1972 .   So really a case of when is a hole not a hole!

An engineer would not notice the difference in the way in which a hole had been generated when working from a 2D drawing.

Since much of the basic premise of F360 is sketch and extrude, the hole table is fairly worthless.

Thank you very much for your contribution to my understanding of F360 vagaries!

[Harry2QBU8]

I am using a 2nd party model, so this may be true.  Is there a setting or parameter to allow Fusion to recognize these as holes.   

[jhackney1972]

No, if you have a hole, that was created with an Extrusion or came in a third part neutral format (STEP, SAT), there is no setting or method to change these to "holes" so the Hole Table will recognize them.  You would have to recreate them using the Hole command.

[korpelakaj]

How come an extruded hole is recognized in Inventor but not in Fusion 360? 

[jhackney1972]

They are two different applications with one being a lot more mature, Inventor, than the other.