I need ballons, but the bom-table from quick tables is way too big, how do I create ballons from my own table?
I create them manually. Much more stable. I know how to check a drawing for accuracy. In 25 years of CAD, this is the one automation I never liked. Same with the BOM itself, I want it stable, including "freezing" the find numbers.
How do you create them manually? Every button I've tried doesn't work unless a BOM table is present, or do you mean manually as in after you print it out?
Hahaha... nonono... I use a balloon note Annotate>Annotations(drop-down)>Balloon Note
Most larger organizations I've worked for use other BOM (ERP) systems so a table BOM on the drawing is not used. Balloons are added to the drawings to correspond to the external BOM system. So today, as a contractor, I have to make custom BOMs for every client to match their format, so I simply make a table and add text. In this instance, I believe in applying the KISS principle.
You can create balloons from any repeat region table - the balloons will show the repeat index by default but you can change that to other values in the table if you want. The quick table bom is probably a good place to start, edit the columns to display the info you want, then edit the repeat region filters and recursive attributes to get rid of components you don't want in the BOM - you may need to add extra parameters to your models to accomplish this. Once you have a table you like save it out as a table and you can re-use it on any drawing or even on drawing formats.
Antonius - you can also use this method to 'freeze' the find numbers, add them to your parts as a parameter and display in place of the repeat index in your repeat region table, then use 'Alt Ballon Symbol' to select those values.
Your best bet is probably to start with the quick table BOM (already a repeat region table) and edit the repeat region filters so the table only includes the parts you are looking for. You may need to add parameters to your models for this. Filters would be something like:
&asm.mbr.nobom != true
Where nobom is a yes/no parameter we have in our models that we use to exclude them from our BOM's.
Also, you can add or delete columns as needed to show more or less info. All of these functions are in the Table menu (or ribbon tab depending on the version you are running). Look at the cell contents in the first row of the repeat region to see how the parameter callouts are formatted.
There are way too many options to go through it all, especially since I don't really know exactely what you are trying to accomplish. If you have specific questions feel free to ask. Also a good idea to look this up in the help center.
For enterprise solutions to BOM generation and maintenance, most people will hire someone to codify such endeavors. This helps to assure consistency by providing training and procedures on how to use the functionality. This also helps corporate policies with regard to part numbering if it is ill defined to begin with.
In general, I do not promote self-development of things that cannot be sustained years down the road by the average user. If these efforts do go toward development of a standard method, then by all means. Just document what you are doing for future users of your efforts.
Having said that, I definitely encourage self-learning. If a tool such as this will help with product quality or checking for drawing completeness, it is all good. Just be mindful what you maintain in released CAD data. All too often I have paid a huge price for some "clever" drafting practices.