Hi all
Following my question: http://www.lynkoa.com/forum/3d/semelle-soudee-sur-une-structure-solidworks
I created my soles by doing extrusions, so I get bodies in the part of the welded elements, bodies that I renamed:
However, I do not find these items in the drawing nomenclature, whether I am doing a general nomenclature or a nomenclature of welded parts.
I only get the tubes inserted.
How do you get these bodies in the nomenclature?
Aurélien
Hello
Do your insoles have the properties of welded bodies?
By right-clicking on the body from the list of welded bodies.
Edit: and did you update the list of welded parts before reinserting your table?
I don't understand how to see with the right-click the property of welded bodies, can you explain?
And how do you update the list of welded parts?
To update the list of welded parts, go to the 3D, and right-click on the shaft line:
"Welded Parts List (80)"
Right-click to update it. then CTRL + Q to rebuild everything.
Then delete and reinsert the table into the plan.
See here:
http://help.solidworks.com/2015/french/SolidWorks/sldworks/t_Updating_Cut_Lists_weld.htm
Négait, it didn't change anything...
Try creating a section for your turntables
and saves them in a mechanical library welded like a flat iron
All you have to do is create your sketch to the desired length and you will have your plates in the welded bodies
It's up to you to create your fixing holes
@+
Hello
For me you have to right click on one of the plates or on the article folder welded part 44 and enter the properties of the welded parts and assign a description because from your image I think you just renamed the bodies but did not assign properties.
@+
@coyote is also what I suspected in my first message.
See here for welded body properties:
http://help.solidworks.com/2012/French/SolidWorks/sldworks/Custom_Properties_in_Weldments.htm?id=b23dd78154fe45519a7a10f115995638
Personally, all the welded bodies (which are not tubes, angles, etc....) I transform them into sheet metal.
I add, via smartpoperties (but it could be done manually) properties in automatic and it gives me the following table:
+1 with @Coyotte (yes, my interaction is very productive.)
And indeed, if it doesn't work, right-clicking updates, solves a lot of problems. ON THE other hand, you have the choice between two updates. One automatic and another. The automatic is not always very well developed and it may be necessary to click on the second choice
Well I had done everything well but I had divided my structure into two welded-sub-assemblies (I thought it was more practical as I had "standard" steel and stainless steel), so SW only put 2 items and took the values of the profiles to fill the table (you can see that I had 80 different parts but 23 profiles).
So I had to right-click and remove all my components from my soldered parts list to remove the organization I had made. Then with the auto-update, it recreated subfolders that I also had to delete.
So I now have 38 different items in my nomenclature and I get the lsite of my various parts!
Indeed, I hadn't noticed that you had created subfolders...
@flegendre: On the other hand, I'm still interested in your solution of converting to sheet metal!