I need to represent a thread that goes through two bodies (let's say two plates of a chassis that are welded). Only, when I do it as usual (see tree capture), the representation is not good. The thread stops at the first body...
The only solution I have found for the moment is to make a first threaded hole on the first body, then to do a second one on the second body. So yes it works, but given the size of the chassis I'm going to do and the number of holes, it's going to be really heavy for future modifications or on the size of the file.
Exactly, I get the same result by making a view of apparent hidden lines... So between the 2017 sp5 (which I have) and the 2018 sp5, the problem would still be present. Drat!
I'd rather be tempted to say that it was before there was a bug. ;-)
If we enter into the logic of a CAD software including our beloved SW: what dominates is the notion of body and part. So in the creation tree when you draw a part, you don't have the option to merge into a single body.
In your case it is different because you are in the case of an assembly of two parts so two bodies.
Since solidWorks considers only one body for drilling and tapping actions, it is normal for the tapping to be only on one or the other part but not both since they are two bodies.
So the dilemma is this: do the tapping in the assembly but then rusk to have it in each part during the MEP. On the other hand, if we think "prod", it is almost certain that the tapping is done once the part is welded, otherwise there is no chance that the thread entries will be aligned after welding.
So from the production point of view, we do the tapping on the outer part and after welding we re-tap the second part by entering the tap through the first part and thus we are not sure to have the thread entries well aligned.
So clearly for me there is necessarily a re-machining or there is a technique that I don't know or at least that is not explained by the requester ;-)
I guess we have a part (sldprt file) and not an assembly (sldasm)
Is the "action area" box at the bottom of the feature manager correctly filled?
@Zozo_mp: you can also make the hole and tap after welding the 2 pieces. In this case, it should be possible to make a thread in assembly mode (in the SW sense).
PS: I don't have SW on hand at the moment to do tests
[[ You can also make the hole and the tapping after welding the 2 pieces. ]] Totally agree with you, it' s a choice made with the production or according to the habits and constraints of the workshop or the subcontractor. ;-) ;-)
PS: for my personal culture what is it ( Is the "action zone" box, at the very bottom of the feature manager correctly filled in ? ) this because I don't have that myself ;-[
@Zozo_mp: To clarify the case, from a production point of view, the material flows will be done, then welding and finally cubing/drilling/tapping of the frame. I am obliged to make the holes appear in the same drawing as the flows, because all the element will be made by a supplier.
@stefbeno: It is indeed modeled from a part (.sldprt) and not from an assembly. The PLM/ERP management that comes behind will be simpler that way, and the tracking of part changes will also be facilitated.
As for the area of action, I tried all three possibilities (all bodies / Only body 1 / Only body 2) without being able to achieve the desired result.
The only solution I have at the moment is to do the function in two times: a drilling/tapping through everything on the first body, then a drilling/tapping at the right values on the second body
It seems to me that this also applies to the wizard for drilling, the problem is that the pad is often folded and in addition you have to use the feature manager's elevator to get there.
@kloffel Thank you for these clarifications on the case you share with us. ;-) The solution you indicate in your last post seems to me to be the right one, even if I understand it, it's much heavier at first to manage. But you'll find yourself there one day or another (at least I hope so)
If you have a support contract, it would be worth opening a ticket. I'd be curious to know SW's position on this issue.
I'm still quite surprised, regularly making mechanically welded chassis, I don't remember having this problem. The only difference I see for now is that I haven't worked much with SW17 or 18 yet.
Under your advice, I opened a ticket. So much for the answer:
"This bug was already reported at SW: SPR 1086062: Parts - Cosmetic Threads: Cosmetic Thread through all 2 bodies of Multi body part ends after body 1 in the Section View. It will be fixed in 2019 sp3 version."
According to them, the problem has existed since the 2016 sp3 version. Nothing to do, but at least I know it's not a user error:D