Some of what you are asking for is extremely simple. Others not so much. I'll start you off with some help on the easier portions.
@john.vanderhoven wrote:
THICKNESS: ? - would like to see "3mm" as it is the part thickness
FINISH: ? - would like to see "-2B" as this is the finish as specified in the part
If you have already created custom iProperties for these items, then inserting them into a symbol is no different from any of the properties you have already figured out, except for one critical point. You must place a view in the drawing of a part that contains the properties. Once you have done that, those properties will show up under "Custom Properties - Model" category. Until you place the view, this entire category is omitted from the dropdown list.
Once you create the symbol, it can be copy-pasted into any drawing, and the properties will just show up as blank if they don't exist. But to create them initially, you must have a view placed from a part that contains them. Inventor has no idea those properties exist until you do so.
@john.vanderhoven wrote:
QTY: ? - promoted for a value
SCALE: ? - flat pattern scale
These items are more difficult. With more information about your specific application, it may be possible to solve them as well, but the solution will probably involve custom programming. There are specific reasons why this is the case. Not knowing the details of your application, I'll explain why these items are issues instead of proposing specific solutions at this point.
- QTY: A part does not know (or care) how many times it has been used. The same part file might be used once in Assembly A, 3 times in Assembly B, and 250 times in Assembly C. Which one should it consider to be the quantity shown on the drawing? There's no straightforward way for the program to know this, so instead all quantity information is tracked by the assembly, not the parts.
- Similarly, there may be multiple views on a drawing. They may or may not all be views of the same part, and might not be the same scale. How would Inventor know which scale you are talking about? Instead, the way Inventor handles this is that the scale is a property of the View, not the Drawing. As such, the scale isn't available to insert into a Symbol, but is trivially easy to insert into a View Label.
Depending on the specifics of your usage, there may be ways around this. For example, let's say your parts are always specific to a particular assembly, and never get reused (common in welded structures, for example). It might be possible to write some iLogic code in the assembly that reads the part quantity and writes it to a custom property in the part. You can probably search these forums a bit and find discussions about this topic, possibly even with sample code.
Similarly, if your drawing only contains one view, it might be possible to write code that reads that scale and writes it to a custom property of the drawing, which could then be used in the symbol. If the drawing contains multiple views but only one flat pattern view, it might still be possible to write the code in such a way that it ignores all the views except the flat pattern.
Regarding the Scale, if the only reason to have it is to check that it is 1:1, another option might be to write code that simply forces all views in that drawing to be 1:1 scale when the drawing is saved. This may arguably be better, since instead of just giving a method to check for the problem, it directly fixes it.
