Hello everyone, I'm coming to see you because I've exhausted my ideas to solve my problem of the link between bubble and a nomenclature.
- Context: I have recovered an assembly and the corresponding drawing, on which I have some modifications to make, here the bubble works.
I will work on a copy of these files to keep the originals. I redo the link between the copied drawing and the copied assembly: that's OK.
- Problem: But from there, the bubble shows me question marks and I can't seem to redo the link with the existing nomenclature.
I tried to go to the property of the drawing view, but the "Link balloon text to the specified table" box is grayed out!? not possible to check
I also tried to add the BOM template in "System Option" > "File Location" > "BOM Template". It didn't allow me to do anything more neither in the properties of the drawing view, nor in the actions via a bubble... or I missed something somewhere.
It's only when I recreate a BOM with the saved model that I can reconnect with the bubbles.
But I want to keep the existing nomenclature, because it is partly modified on the Article N° and other text, and I don't have to make any changes to it. Beyond that, it allows me to see the possibilities of SolidWorks.
The existing nomenclature has small padlocks, could it block me somewhere? However, I don't really see why because it works in the original file!
There you go, if anyone has an idea to solve this, thank you in advance.
- With the original drawing, the balloons follow the numbering of the nomenclature (I move the arrow on a part and I have the right number).
- With the copy of the drawing in connection with the copy of the assembly, I have "?" in the bubbles and when I move the arrow on a part I end up with a number other than the one in the nomenclature.
- new manipulation: If I redo the link between the copy of the drawing and the original assembly, I find my balloon numbers corresponding to the nomenclature
I don't see what makes the difference between assembly and copying so that the bubbles follow the nomenclature in one case and not the other!?
So check if the MEP view is linked to the correct BOM if multiple BOMs.
I can only see that as an explanation. So to check if the view is linked to the right nomenclature, you click on the desired view, and then you right-click and check if it is linked and above all check the 3 points where the nomenclature you want points to the right configuration and display state.
- Take the original assembly and make a derived configuration with an added part replacing another deleted.
- Select the derived configuration in the drawing.
And there indeed, I can do the manip that you propose to me A.R (and which was not possible with my copies!?) and I find the numbering of the nomenclature on the parts... except the one I added which ends up with * in the bubble. The nomenclature has not changed and still displays the old part.
P.S: That's it, I'm there! We had to choose a configuration for the nomenclature too!
Well on the other hand I don't know why this View option "Link balloon text to the specified table" is not possible with copies?
So "PACK AND GO" allows for example to copy a subset with all the drawings related to the parts and assemblies and at the same time to rename them.
better =>Aggregates all files associated with the design of a model (parts, assemblies, drawings, references, part families, Design Workbook contents, decals, appearances, scenes, and SOLIDWORKS Simulation results) in a folder or zip file.
