I know it can be done, or used to be able to be done, because i have done it. There is either a parameter or an options command you have to imbed in the drw file first. something like "alow_asm_mbr_name_note".
I worked for company that did a lot of work for DuPont and thier drawing files were loaded up with many params andoption commands.
How would one attach note or symbol to components in assembly drawing view to show partnumber (file name)of the component the note or symbol is attached to?
I must have missed this when it was first asked back in April. You can attach a note with the text "&<parameter>:att" and it will pull the parameter value from the part the note is attached to.
With cross section views, it gets a little tricky. You need to query select and watch at the bottom of the screen when selecting edges. The first edge it will select is the edge belonging to the cross section, you should be able to toggle to another edge behind that one that belongs to the part. If you use the section edge, there's no parameters for the note to use.
I have been trying to apply this to a drawings note section. All looks great. I enter &PART_NUMBER:"session id"for each item I would like in the notes.Again all is great. The notes show correct with all the part numbers, until I repaint. As soon as I repaint a bunch of the part numbers change to *** and even one went as far as changin to be a date and time. Yes on its own it change the symbol to be proi_created_on:d. I have found the difference to be that the ones that didn't work were done as INSERT, COMPONENT, INCLUDE. I have these items added this way to populate the bom and not add any weight to the model. The note they were goining into was a not shown note. My work around might have to be assembling them in as an empty rep. But it is unfotunate that I will have to deal with the extra weight in my master rep. Am I missing something or is this another one of those really cool PTC item that only does 90% of what it should.
FYI: I have figured out a work around. I am able to createsome relations and parametersin the drawing. The relationsdon't seem to loose their reference tothe included items like the note did.
not_shown=not_shown_a +", "+ not_shown_b +", "+ not_shown_c +"."