Identifying parts on drawings

[nwk23]

I have a drawing stack where the top sheet is multiple views of the assembly, BOM/Parts List and I've ballooned all the parts. The following pages have drawings for the parts.  Some sheets have several parts on, spaced enough that there is no confusion. I've added balloons to the subsequent pages, but manually edit balloon to make the numbers correct.  Is there an automated way to identify and label parts on subsequent pages?

[swalton]

Maybe, depending on your workflow.

Parts List Item Numbers are assembly-only values.  Each individual part or sub-assembly file does not know anything about an assembly's item numbering.  Alice.ipt could be Item 1 in Bob.iam and Item 27 in Charlie.iam.  

Here are possible workarounds:

1. Assign unique part numbers to each component and adopt the one-model-per-drawing-file and filename=part number habits. Make sure to include a Part Number column in the Parts Lists.
2. Assign unique part numbers to each component.  Replace the Item Number column in the Parts List with the Part Number column.  Edit the balloon styles to show the Part Number iproperty.  Add a leader note to each part view that shows Part Number.  It may be possible to add the Part Number iproperty to the View Label style.
3. Write or find some iLogic code that pushes the Item Number from the assembly to each sub-component.  The code will need to handle the case where Alice.ipt is used in many different assembly files.  Use a leader note or view label to show each component's custom iprop with the assembly Item Number info.
4. Create custom view reps in the assembly that isolate each component.  Place views of the assembly and select the proper view rep when detailing each component.  Don't place views of the component file directly.  You should be able to balloon each component with the correct item number.

[Anonymous]

The only way I know to do this, there might be others, is to create the view you want from the assembly linked to BOM and turn on or turn off visibility of parts in that view.  So you can place the assembly in the drawing, off of the sheet, and create section or end views for each part.  In each of those views you would need to turn off visibility in the feature tree of the parts you don't want to see in that view. You can then orient them to your liking, by editing the view sketches or rotating or both. 

You can do this in first drawing and drag the views in the feature tree into another drawing if you prefer to see the section/end views on your general arrangement.

[lkrenzler]

We had the same issue and someone on this forum (sadly I can't remember who at the moment) helped us out by giving us an I-logic script.  I've attached it here.  We set it to run before save so that every time you save the drawing it updates it.  It adds a tag to each part with the number.  We find it very handy.

[nwk23]

That looks promising, but the script didn't attach properly.  I can't seem to download it.

[lkrenzler · Accepted solution]

OK, I'll try zipping it.  Let me know if this works.  Maybe it doesn't like raw text files.

[nwk23]

That is dang near perfect!

All I need to do is figure out what part of the code says "put label below view" and change that to "above" and it will be perfect.  

[lkrenzler · Accepted solution]

I think that might not be in the script but in your Inventor settings (styles editor).  I think it just uses a standard "View Label".

[nwk23]

Now I just need to remember how to make changes to the Styles stick...