Hello!
Here is my case:
My part represents different tube segments created by the mechanically welded Element function and a 3D sketch.
In the properties of the welded parts list, I find the TOTAL LENGTH property
What I would like to do is retrieve the value of this property and add it to one of my properties in the configuration.
Is it possible?
Thanks in advance!
As part of the creation of a family of parts?
No, no family of parts.
The property in which I want the total length to appear is called NoArticle. This is the property that appears in the nomenclatures of my ASMs.
The goal is to have a value of the type: 058796 L2500
Where 058796 is an item number that matches my raw tube and 2500 is the total length.
Hello @damien.grandjean,
Is this the expected result?
if so, then simply copy the variable present in the " total lenght " PRP of the mechanically welded elements.
Yes, that's it. 
The problem is that you have to copy the variable in the properties of the welded parts list each time... To be able to copy the variable, you have to remove the " linked " checkmark (which I don't fully understand, by the way).
I wonder if there is a way to " call " this variable with a text like $PRP"TOTAL LENGHT" (which doesn't work by the way...).
Hoping I'm clear enough...
If it's really recurring, one way could be to put this property in the room model. (. PRTDOT)
On the other hand, I don't have a precise idea of how to get there and to be honest I don't have a little time to do the tests myself 
.
Good luck in your search.
PS: I believe that body PRPs only work in welded parts lists or bills of materials with the " Detailed list of welded parts" option.
To check
Hello
Unless I'm mistaken, see this topic " sw-mass " properties in the list of welded parts - Uncategorized - myCAD forum for adding a property to all the articles of the list of welded parts at once.
Re
By redoing a test, if the welded construction has a unique reference (for the 058796), it is possible to make a property line at the level of the welded construction function formatted as follows:
It will then propagate in all the articles and retrieve the length value associated with each article in the list (it updates the increment of the article in the list).
Hi @Cyril.f ,
I believe that the need here is to put a property in the part and not in the mechanically welded bodies.
For me it would be enough to copy the variable as I did in my previous message, then save the document as a part template.
but I ask myself questions...
The Total Lenght property includes the info of the type of mechanically welded elements it is (example: hollow square tube 50×3 steel)
So, if you make a round tube it doesn't work anymore?
The day you have 2 different types of profile in the same room, how does it work?
In fact, I come to wonder what the objective behind it is...
Would a bill of materials with the "Detailed list of welded parts" option not meet the need?
Hi @twathle ,
Exactly, read a little diagonally.
Copying the property does work but yes if the item type changes it's dead.
For my part, it doesn't show me the type of element, it only shows me a tree structure with the name " Article-list-of-welded-parts" in the header (n being an increment).
I don't do a lot of welded constructions so I don't have files with different types of profiles (in this case the model in my example is square profiles called Square 20x20)
Yes, if the type of item changes, the solution would no longer work, but in my case, it's not a problem.
The goal is to have one .prt file per type of pipe, these .prt will be in an .asm as well as other "standard " pieces.
In the nomenclature of this .asm, I want to have something like:
Pos. - Item No. - Qty - Description
1 - xxxxxx - 12 - Socket ø20/10x15
2 - yyyyyyy L2500 - 1 - Tube ø50x2
3 - zzzzzz L1200 - 1 - Tube ø40x3
In this case, the solution of @twathle seems good to me.
You have to create a template for a document.
For existing ones, a snippet of code (macro) will do the trick to add and format the property
Unfortunately, I don't think so...
because you'll have to create a doc template for each profile you have...
50×3 Steel
50×5 Steel
50×3 Stainless Steel
50×5 Stainless Steel
UPN80 Steel
UPN100 Steel
UPN120 Steel
ETC...
very long and unmanageable in the event of future developments...
maybe see with a new column in your nomenclature?
a column whose value would be an equation equal to " name " + " total lenght " + " ... »
Hello;
I wonder if it wouldn't be more " practical " to simply create a template for Annotation of the style:
$PRPWLD: " Description " (" Designation " in my case, see below)
$PRP"TOTAL LENGHT" mm
or even better, directly in the Nomenclature?
I think I've managed to create a macro that takes the name of the first part from the list of soldered parts in the tree, and uses it to complete my NoArticle property as I wish:
XXXXXX THE "TOTAL LENGTH@@@Article-welded-parts-list1@SW-File Name.SLDPRT"
I'm going to continue with this idea! Thank you so much for the leads!