After finally solving my problem with the nomenclature of the lists of welded parts that were no longer updated (small bug),
I come to another question concerning the names of welded construction profiles.
To give properties to what I usually create on SW I use the icon in the top bar "document properties".
But for the welded construction profiles that I create, I can't make their names appear. However I manually add a "Description" field (which I have to write because I can't find a predefined list for this purpose)
It obviously doesn't work. Is there a better method to do it maybe completely differently?
PS: until now I haven't set up the "custom property" tool available in the right column on the screen, with the "forms".
Indeed it works, and I can correct my little problem.
BUT, it forces me to do it again every time, and for each group of welded parts.
but my predecessor had managed to fill in a "Description" field which therefore appeared systematically in the groups using this same profile. (I could see it by opening one of the SLDLFP and right-clicking ownership of the document on the sketch)
Now I can indeed "troubleshoot" myself but is it possible to do it automatically? because I would never rename a welded mechanic group differently if it uses the same profile.
Frédéric was right. You need to open the original SLDLFP (-file > open -> in the library folder. If you go through a click on the sketch in the part file, I'm not sure it influences the following ones)
And there you modify your properties as usual. Be careful though, if it's managed by configuration, you have to do the config properties (the 3rd tab of the properties). If not, check that the config properties are empty
If still doesn't work, go to "configuration manager" (the 3rd tab of the construction tree) and right-click -> property on the only existing config (or the one you're interested in)
Then in "BOM option", look at what is the number of the part displayed in the BOM (name of the part, name of the config or name specified by the user). And choose the one that suits you best
Edit: On the other hand, be careful. When you modify and save your SLDLFP, I'm not sure that the changes are reflected in the already existing part. So I would advise you to create a new one to check ;)
Small addition following the very good solution given by @coin37coin, for existing files, the only solution to make the properties that have been filled in after the fact in the sldlfp appear is to edit each mechanically welded function, choose a different profile and re-select the right profile, so it's very tedious and your tree will have a lot of error as you change, In some cases, it is easier and faster to redo the part.
coin37coin, I'm almost sure that modifying the SLDLFP is reflected on the mechanically welded part already made (you have to re-edit the function to recall the SLDLFP).
@Frédéric. It's the almost that I also lack^^. But with the re-release you still have a 1 in 2 chance of no longer having your constraints on the right sides. Personally, I avoid as much as possible
To recap, as I'm not sure I understood everything, I tried 3 ways.
1) I clicked doir on the sketch of my SLDLFP and instead of sketch1, I renamed it square tube 40 x 40.
2) I added a description field in "File Properties" (at the top), manually with the same title.
3) Then I saw when I saved the named file, just before clicking save, under the "file name" field there is "add a description written in blue, small.
These three techniques didn't work on my already created files. Then it worked on a new profile created. but I'm still not sure which technique worked well... I feel like the 3 is the best, but it works to create a new piece.
I'm going to keep digging unless someone has already done it among you^^
I hadn't seen all your answers, but I tested a lot of ways to add this famous "descirption" field
No technique works on existing files, they are no longer displayed in the nomenclatures, even if this has been specified.
On the other hand, when re-creating a part, when saving it in its folder I just click on "add a description" just below, and there it works.
My old profiles have been used in a lot of assembly so I'm afraid I'll have to redo everything with new, better created profiles.
Maybe reopen these same sldlfp, to make "save as" keep the same name in order to replace the old one, but still adding the "description" field just below?
I will try... From memory I had already tried but a "read only" error had appeared...
Maybe you can try something (with no guarantee of success)
You modify your SLDLFP, save them etc.
Then, you change the name of their directory (an extra letter, a space, whatever you want)
So, when you open your old documents he should ask you to repoint the folder (logically?). This should update the whole.
What scares me is that I have the impression that he imports the sketch into the room and therefore Solidworks doesn't ask to point to it again. In short, to be tested, with a little luck ..
I'm not going to embark on this technique which is ultimately as laborious as mine and uncertain.
To recap, the only technique that works for me... (hoping that a reader has a better one)
In the library, go to the relevant profile, right-click, "Properties" there you can add (in the second or third tab) a "Description" line and associate it for example "square 20 x 20" once this is done you apply, save.
Your profile is up to date, but to make this new info appear in old nomenclature, you must first delete it I think. Then replace the profile temporarily in your whole one, with another one, save, put back the right profile, re-register, at this point the welded parts list will import the complete info again.