I have been looking for a solution to this since I started using Solidworks... Unless I have missed something there doesn't seem to be an easy or automatic way to do what you want.
Neither cut lists nor BOMs support this functionality how I'd like. 2017 claims to do a better job, but I did a quick investigation and it doesn't work how I would like.
This is what I have found and I hope you don't waste a lot of time like I did trying to sort this out.
Create the balloon, as you have done, then change the settings to not have a bounding box:
Now create the title in the view and select the balloon, this will insert the cut list or BOM item number into the annotation.
Now add the title text you want after the link to the cut list or Bom item number:
You can delete the balloon you initially created and the link remains. If you modify the cut list the reference will update in the title.
If someone else has a less manual way to do this, please let us know.
If you consider 2-3 hours "a lot" of time then it's already too late for me...
Thanks for the walk through. I'm beginning to think SW devs just don't use drawings seeing as how simple this is.
I've been saying for years that any property that can be used in a Balloon should also be available to link to in a Note, but so far it hasn't happened. They've added one or two, but not all.
Hence the work around
Matt Peneguy - Grant Kirkland - did you ever consider using notes and using Custom Property information - Here I have a series of notes that I use and within those notes I have the Part Number property typed in the note body... This is a really quick way to add additional detail notes. I have the notes in my Product Library Folder which is within the Design Library Folder.... You can show with or without leaders as well
I don't believe this will work for a relative view, will it? I want to show the detail of a plate in a weldment part. Linking the part number is linking mine to the literal part number, not the item number in the cut list.
I don't use weldments - but I think your 100% right, I wasn't thinking about weldments.. Not sure if you could add another custom property easily and use that..
That is good information to include in this thread. And actually after a lot of trial and error, I have abandoned the method I listed above because it is too labor intensive for what I do. I usually end up with very long BOMs with many fabricated parts. I use distinct part names as custom properties and those custom properties are used in my part titles as well as my BOMs. So, having the item number from the BOM or Cut list in the part title would really make my job a lot easier. Part "326 Balance Wheel Axle" is a lot easier to find in an ordered BOM than "Balance Wheel Axle". This is especially true if the BOM spans more than one sheet. But, it is too labor intensive to justify doing it for more than a few parts.
It appears that some people have already created some SPRs about this:
Provide ability to extract Item number and Quantity information as separate entities so that they can be placed as linked note
Ability to create a label for a drawing view that is linked to the item number in the BOM of the part / assembly in the view
BOM item number linked with custom property
I think the last one may not even be desirable if you have a part in more than one assembly.
I don't know if any of these really state this particular problem. Should I create a new SPR, "Ability to link Cut List or BOM item number in annotations in a similar manner as custom properties. The item number should be able to be displayed in annotations without a manual work around."
Please everyone let me know if that gets the point across, or edit it and I'll create a SPR. When I do, I'll post the number here.
That would be awesome to have - and it will more then likely be available in the future, but till then I would definitely make up another Custom Property, (they're not hard), and by using the Custom Property Tab Builder, (which is the most underrated SW tool, available to us), you could get really creative and not spend a lot of time doing it.....
I do include a field for all my parts called BOM Name as the title for all of my parts on my drawings. Problem is that it is difficult to find the part quickly if there are 200 parts in the BOM. I agree Custom Property Tab Builder is a great tool.
I submitted the Enhancement Request:
Ability to link Cut List or BOM item number in annotations in a similar manner as custom properties. The item number should be able to be displayed in annotations without a manual work around.
Product Version in Use : SW2014
Explanation : When dealing with parts or items in a cut list or BOM the item number should be displayed
next to or under the part in the drawing. However item numbers not available in the same
manner as custom properties. The new ability in 2017 doesn't solve this problem.
If the BOM or Cut List has many parts it is very difficult to identify where the part is in the
BOM, especially if the BOM spans multiple sheets.
They have created or linked this to SPR# 967064:
Ability to link notes to a table cell, with the BOM/Table on a different drawing sheet
This doesn't seem to address the issue I presented. Do they have the ER when they go to fix the bug, or do they just work from the SPR? If it is the latter I will contact my VAR to have this fixed.
If you don't need the text with it you can attach a balloon to the drawing view in the regular way, then hide the leader. You can still do that even with the text if you group the note and leaderless balloon. And you can copy and paste it from one view to another. It will pick up the properties from the new view, but when pasting you'll need to click on the model itself, not in an open space within the drawing view.
If you have 2017, take a look at this help topic
Linking a Note to a Table Cell
This will allow you to create a note based on a field in your cutlist. You can then apply a border to the linked text and you'll have a balloon that updates.
I haven't tried it myself, but I've been watching for this enhancement
Yes, this is available in 2017 and it does update if things in the BOM get moved around. And if you are dealing with a BOM with only say 5 parts, you may make use of this functionality (but, if you only have 5 parts you can use John Stoltzfus suggestion of using a custom property as the part title, which is easier and better). However, the item number isn't a "property" and there seems to be no way to create an annotation that references the item number in the BOM automatically. What this amounts to for my workflow is too much manual work to justify using this functionality. For instance, if I have a BOM with 200 items in it, if I want the item number from the BOM in the part title for each part I'd have to manually assign it for each part. So, I don't bother with it because it is "half-baked" functionality. There is more chance that I'll make a mistake than get all of the assignments correct.
I'd really like this to work correctly because if I have a BOM with 200 parts in it sorted by "item number" it is a lot easier to find the part by that number than it is by another field (in my case a custom property called "BOM Name").
The original post refers to Cut Lists, and as far as I know, all of what I have written above applies to Cut Lists, too. Someone please correct me if I'm wrong.
Correct. I would like to be able to have a relative view label in our weldment drawings which is linked to the cutlist item number. Something to the effect of "Relative View: Item 7, Scale 1:4" where that view is of the body of the #7 item in the cutlist.
This may not be at all possible, due to using "Select Body" in the relative view feature. But it should would help our the guys in the shop.
Unfortunately, "Link a Note to a Table Cell" does not work with cutlist item numbers. At least, not any of mine.
I come from the 2D CAD world and was amazed at how much better the SolidWorks world is in almost every way. When I stumbled on this problem I was reminded of how I used to have to manually manage titles and update BOMs in 2D CAD. I thought, surely there is a way to automatically link the item number to the part title... But, apparently there isn't.
Hopefully, the ER/SPR gets resolved and they fix this.