Hours of research and no results: I have not been able to recover the custom properties of my parts inserted in my welded construction.... And yet I know that SW2012 did it very well.
FYI, my version of SW is a 2016 SP5...
I put as an example my parts files (with their properties filled) but also my welded construction part file as well as its drawing.
I'm waiting for your feedback, I'm starting to despair!!
Thank you
Eric
See my message on this subject, which talks exactly about the downfall of properties:
http://www.lynkoa.com/forum/solidworks/propri%C3%A9t%C3%A9-de-pi%C3%A8ce
there is the "classic" descent for a library part without config (its properties must be in the "general", not in the config)
And now there is the "advanced" descent of the subbodies const.welded with two target destinations: either the subbodies or the target file.
To fully understand these possibilities, the best thing to do is to test all your options, to see how they behave.
Ok Olivier, thank you for your answer..... But that doesn't answer my question....
And as you must have read at the beginning of my email, I did a lot of tests... A trainer from Visiativ who came to us last week was also stuck on the subject without being able to answer me.
If you open the zip that I attached to my post you will be dismayed that everything has been done as you indicate on your post. However, I can't get these properties back in the nomenclature of my welded part (also attached).
Thank you anyway for your help
If you want the "Mother Piece" to have a "Soldered Nomenclature"
You have to check in the Insert part function:
Properties / Welded Parts List
do it for everyone...
then in your MEP, you put a Nomenclature-ASM-TAB on a PRT,
it is better to put a "Welded Parts List" as a table.
No need to have the first BOM line by the "Mother Part",
This will be the cartridge that will have this information.
And as usual, whatever the table (ASM or PRT) when you bubble a view, you check in the properties of the view "Linked to table..." " and we choose the right one.
"May the dark side reign over the galaxy... "
Hello
The BOM can only be filled if the custom properties of the mechanically welded elements have been met.
I have opened all your parts in none, the welded parts list has not been updated.
I updated one of the list of welded parts of your parts and now, magic, it updates in the MEP.
Yves
Ok I looked following your remark.... Indeed, some of my lists were not up to date...
On the other hand, I would like to know where you clicked for the drawing to be updated: at home the nomenclature remains empty from empty....
Olive tree
I looked at something that is bothering me.... I don't want to get my welded parts list back... Anyway, my list took the names of the files of the inserted parts but not the one of my custom properties.... In short, I didn't get anything back at all
Similarly, I can't find where to link the bubbles to the table in question....
How did you create your final welded parts assembly?
You created your parts separately and then exported the list of welded parts in parts and then you created your assembly?
open the PRT "which contains everything"
For each "part insert" right click "Open in context"
then re-edit each "part insertion" and check "Personal properties",
then there is a choice with 2 boxes (this is the destination), choose "Welded parts list"
for the built PRT , it's a little more subtle, either we treat it as a simple PRT (do as above),
or we go back down the information from the profiles....
do "control+Q" between each insertion
then in the MEP deleted the "ASM Table",
select a view, then insert "Welded parts list"
then choose the right columns you want, you get this (see image)
Note Methodological BE :
in the design offices I went to, for boiler assemblies like this, complete abandonment of the "part within part" method because for sheet metal work it can become too complex, and for the function "move body (constraint mode)" it's a buggy function from the beginning, unstable after a while, and this has never been solved (moving in absolute mode is already a little less buggy).
And when you have to change a component by the same one of another size, everything goes awry: in the asm we lose our constraints, in the MEP the dimensions are wobbly...
So we used ASMs (with the "part mode" option) and in config parts, for the welds, we had a library of 3d representation to config, the same for standard profiles to connfigs, or use of the "ASM-PRT hybrid mode".
In addition, if you want to do calculations, you export the ASM in PRT, which allows you to make adjustments for the calculation, without modifying the original.
Time saving for the user, for MEPs, for modifications, size changes, or others...
With the ASM mode (and therefore library in configs) the loss of constraints, and in the MEP the wobbly dimensions , all this disappeared, no longer hesitates!!
And the time to make a modification that was counted in hours in "PRT in PRT" mode simply becomes a few minutes (or even seconds)...
Time saving for the BE = PHENOMENAL !!
I finally got an answer on this subject.... Thank you for your participations but none of your answers suited me...
It was the MyCADServices support that brought it to me: the 2016 version of SW had a bug on this subject. It was impossible to retrieve these properties (which were well filled on my models).
On the 2017 version (SP4) this point was improved and I was able to do what I was looking to do! There is still a bug in the nomenclature but we are getting closer to the goal!
Thank you
Weird, because I'm also in SW2016 SP5.0,
and I was able to have all the properties of the parts revived...
(see capture.jpg in my previous message)
I had tried but it didn't work.... and neither did the supports (and I passed a few...). And indeed, what you told me is working very well in 2017!