Annotating Single Parts While Retaining Item Number in BOM

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There seems to be an issue with Inventor where it seems impossible to link a balloon on a single part view to the BOM of an assembly that the part exists in.  The item number on the single part will always be “1”.

The frustrating part is that when you place a balloon on a view of a single part the following dialogue box appears showing the path to the file source – this cannot be edited! 

Request to Autodesk – it would be nice to have a browse button here, or even better, a vault style “where used”.

So, here is a suggested workaround.

Once your assembly is complete, convert the assembly to a weldment, even though your model contains no welded parts.

You will receive the following warning message stating that once converted you cannot return.  Choose “yes” to continue.

The only things that you really can’t do in a Weldment Assembly is create assembly features, for example, an extruded cut at the assembly level.  This can easily be overcome however by utilizing the “machining” area of a weldment assembly.  Also, a welded assembly cannot be made “flexible” if added a s a subassembly.

In the next dialogue box choose the correct BOM structure.  Here we will choose “Normal”.

Now start a new drawing, place a base view of the assembly, a parts list, and annotate with balloons.

Choose “Base View” again, browse to the same assembly file, choose the “Model State” tab and choose the single part you wish to create a view of from the pull down menu shown below.

Place your view of the chosen single part and annotate with a balloon.  Notice the Item number is automatically linked to the assembly BOM.

 

 

Brent

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