Hello, I didn't know how to title my request. I searched a little on the forum but I found nothing concrete.
So here's my problem:
I built an assembly in which I used parts of the weld element (lib feat part) and I was wondering if it was possible to easily know the maximum dimensional values of these parts by going through an analysis or a tool that I do not yet know how to use on Solidworks (I still use the 2016 version). Knowing that I must know the yardage of each of my aluminum profiles that make up my assembly and that I must have close to ~25-30 parts per assembly and about thirty assemblies per zone distributed in about ten zones.
Of course, each part does not have the same axial orientations. As a result, I'm a bit lost. I am asked for the footage of each of my bars to help the production to cut my profiles and I look in vain for a quick solution to my problem.
I'm sure someone here has the solution to my problem.
Thank you again in advance. :)
If the PRTs all have their "up-to-date welded parts list" in the 3D,
you have to take the ASM, and set an ASM nomenclature with the "Tab" option ,
After that, you just need to have the right columns, generally:
Description / LENGTH
1 Like
I'm a little lost by the explanation. I go to the assembly (ok), I put a bill of materials (ok) with the tab option (1st *sic)... Then the length column (2nd *sic).
Just additional information, I used individually welded parts that I cut back to make them stick to my design. So, knowing that the coordinate system changes according to the configuration of my element in its general environment, the overall length after cutting can be found how?
To be honest, I think I'm not far from finding it because with the "cost" option (I think it should be called that in French), solidworks generates an overall outline of my part with a transparent volume body but doesn't give me the overall dimensions of this body. Then I manage to generate a word file that gives me the price for each of the pieces.
If I could have this document but with the maximum lengths of each piece, I would be over the moon (see the *doc file I just generated to understand my problem).
r30l8fra_report_1.docx
no need to go through "Costs", a simple nomenclature is enough.
each PRT (3D file) must have its list up to date (see up to date icon, 4th in the page here)
then, take the ASM, place it in a MEP or not according to taste,
then click put a Nomenclature, this brings up the panel on the left, where you can choose the nomenclature template
link
and choose:
Tab Type
then validate, and set the table.
Then you just have to add the right columns to the table if not present.
2 Likes
Great, we're making progress... THANK YOU!
Okay, now, despite the fact that in the properties of the document, the tab to update my "CutList" is checked, I have a few parts that haven't updated their list. So, can we update all the cutlists of an assembly in order to have all the lengths of our welded parts in the nomenclature?
Not to my knowledge,
you have to go back to the PRT and update the cutlist, have Crtl+B rebuilt and then update the "CutList" list manually, unless it's automatic.
When working with the PRT Const.Soudées you must forget at all costs the bad habit of using Ctrl+Q it is to be forgotten !!!!
too many people believe that Crtl+Q means "Rebuild" but it's not (classic mistake among many others...).
to Rebuild you have to do Crtl+B (or the green light icon).
EDIT: if some lines are still empty at the "Description" level, it probably comes from the fact that the function points to an old incomplete LibFeatPart file that didn't have the description.
2 Likes
Well, I feel like I'm going to complain that I didn't check that damn option to automatically update the cut lists in the document properties when we did our first item.
I will have to check and if necessary update in the worst case more than 7500 shares in order to have the length in the BoM.
On the other hand, I just tested on an assembly that I had symmetrical and of course, Solidworks takes it as a dead solid (so no length for these elements in the nomenclature)... There are no tricks I guess to find these lengths in symmetrical assemblies?
No, there is no problem with symmetrical parts,
You just have to check the right option in the symmetrical parts:
Welded Parts List Properties
http://help.solidworks.com/2016/french/solidworks/sldworks/HIDD_DVE_IMPORT_FEATURES.htm
2 Likes
Well, I'll look at all of that. In any case, thank you again for your advice.
Now I have parts to update. :-p
1 Like