Re twathle,
Well I added a column in my " welded parts" nomenclature of my MEP, then I click on the column, then in the column properties I link the mass by checking the property of the column.
But I always know how to insert my modified nomenclature in my MEP.=>
And there you have it, @+.
AR
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Re twathle,
So I just found how to do it for my welded parts nomenclature by having previously added the column in my welded parts list and my MEP.
Here it is in picture=>
And here is also the small file that is fine=>
EssaiListePiécesSoudée.zip (1.9 KB)
.
@+.
AR.
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This is the right method to customize the welded parts list template.
this " nomenclature " fetches the " mass " PRP of each body from the 3D
but the bodies in my 3D don't have this property...
In your case, how did you get the value 44 in the mass column of rep. 5?
Hello re-twathle,
If that's okay with you, then close the question ...=>
@+.
AR
Re-twathle,
To obtain the mass of each body, you have to enter it in the properties of the list of welded parts.
Then on your MEP you insert my file " essaiListePièces Soudées " for the general options, mentioned above in my answers.
@+.
AR.
@A.R
I understand the whole process but the problem is that I can't afford to fill in the properties of each body one by one.
Some of my pieces feature over 150 bodies!
Hence the topic of this thread, how to add the last line of this default capture to the creation of each mechanically welded body? like the length property.
To customize it is necessary to customize the soldered list properties file from memory:
https://help.solidworks.com/2021/french/SolidWorks/sldworks/c_Custom_Properties_in_Weldments.htm
Siinon see to modify the model part (I have a doubt between the 2 solutions)
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Hello @sbadenis
If I'm not mistaken, modifying the " welded construction properties file" allows you to have in a drop-down list the properties contained in this text file.
But they are not necessarily used by default.
On my screenshot, you can see that I added the " sw_masse " prp which is available in the drop-down menu but it is not used by default (like the " revision " or " origin " prp)
I'll try the second solution
Re twathle,
So here is how I put it in pictures
1 =>On your 3D
2=>On your MEP
3=>Svg your nomenclature under " EssaiListePièces Soudées.sldwldtbt "
4=>In your system options
…
That's it, I've skipped steps, I'll tell you tomorrow...
@+.
Good night.
AR.
Re @A.R !
My problem is having to fill in the masses manually in your first capture. (we agree that we are far from writing the weight manually, you just have to select the variable in the drop-down list but it's still an important number of clicks especially since it happens that I have parts with 150-170 bodies)
Especially since it is not necessary with the prp Length for which everything is done automatically...
No worries, they say that the night brings advice!
in any case thank you for the investment and the time spent 
Hello
I just tested something on SW2023 and I think it's the same on all versions.
To propagate the ground in the list of welded construction bodies, you have to fill in the " WEIGHT " property (in my case) and associate the SW mass with it.
Initial state:
Adding ground to the properties of the welded construction function
The update is present in all listings.
I think then you can create a base model with just the build function welded into the model parameterized with the ground property and rolls.
2 Likes
Here is a Visiativ method for welded construction profiles:
For sheet metal bodies it's different:
https://help.solidworks.com/2021/french/SolidWorks/sldworks/c_Sheet_Metal_Properties.htm?format=P&value=
2 Likes
Hello @Cyril.f !
Thank you very much for your suggestion, it perfectly meets my need! (all you have to do is do that on all profiles)
I didn't know the first method. It is good but its disadvantage is that it remains a bit manual.
To summarize the solution:
1- Open the .sldlfp profile
2- add the desired property in the " Configuration Properties" tab
(here " SW_MASSE ")
3- Propagate this property to all configurations
4- You can check that everything is in order in the " Property Summary" tab
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Hello
It can always be done by macro. I don't have the MyCADTool utilities but maybe Visiativ has developed something in this direction.
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Hello Twathle,
Back for my last message, here is my tutorial for information =>https://mycad.visiativ.com/contenu/ajout-la-masse-pour-chaque-corps-dun-mécanosoudé-dans-sa-liste-de-piéces-soudées?tuto
And here is also the model of the " Welded Parts List", make good use of it!! OL. 
EssaiListePiécesSoudée.zip (1.9 KB)
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Hello
What is unfortunate is that you have to fill in the mass property for each item in the welded parts list. That said, it works well.
Another solution is to enter the ground property for each profile... 
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Hello Le_Bidule,
And yes indeed you have to inform.
It's possible with a macro, but I don't know how to do it ... @+.
AR.
Hello;
Here is a small macro to automatically add the " Mass " property on all mechanically welded elements (Welded Parts List):
=> If specific materials are assigned to certain elements they will be taken into account, otherwise the density of the Global material is kept...
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swFeat As SldWorks.Feature
Dim swCustPropMgr As SldWorks.CustomPropertyManager
Dim FileName As String
Sub main()
On Error Resume Next
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
If swModel Is Nothing Then
MsgBox "Pas de fichier Pièce Solidworks actif..."
End
End If
If swModel.GetType <> 1 Then
MsgBox "Pas de fichier Pièce Solidworks actif..."
End
End If
'swModel.Save
FileName = Mid(swModel.GetPathName, InStrRev(swModel.GetPathName, "\") + 1)
Set swFeat = swModel.FirstFeature
Do While Not swFeat Is Nothing
If swFeat.GetTypeName() = "CutListFolder" Then
Set swCustPropMgr = swFeat.CustomPropertyManager
swCustPropMgr.Add3 "Masse", swCustomInfoText, Chr(34) & "SW-Mass@@@" & swFeat.Name & "@" & FileName & Chr(34) & " Kg", 1
End If
Set swFeat = swFeat.GetNextFeature
Loop
End Sub
Note: it is possible to customize the line.
swCustPropMgr.Add3 " Mass ", swCustomInfoText, Chr(34) & " SW-Mass@@@ " & swFeat.Name & " @ " & FileName & Chr(34) & " Kg", 1
=> " Mass " is the Name of the property to be created
=> & " Kg " (optional text)
Macro for use exclusively on Solidworks Parts files.
Kind regards.
3 Likes
@Cyril.f I temporarily suspended your " Best Answer " to bring up this discussion... But I keep in mind the value of your answer. 
1 Like
I don't chase the best answers 
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