Would there be a method or a way to merge several pieces into one? A kind of conversion of the pieces into different bodies, then brought together in a prt.
To put it simply, it comes down to:
bodies remain bodies,
the parts become bodies (the bodies then adopt the positions of the parts in the assembly),
The assembly becomes a part.
So far I proceed the opposite, i.e. I model and position (as much as possible) all the elements in PRT, and I isolate them afterwards to make them independent parts (and end up in an asm). But sometimes we don't anticipate, or the installation of a body is much more complicated than that of a part in an assembly. So I would like to know if I anticipate or if I can pass an asm in loan.
See if this method can help you. The part keeps a link with the assembly, so if you modify the assembly the part will follow because it has a link. https://www.lynkoa.com/contenu/créer-une-pièce-partir-dun-assemblage-pour-facilter-les-simulations or else you can work in a room and build everything in it but when you do the extrusion for a new body you shouldn't merge it with the ones already built
Hello I think I didn't understand the question well, but to switch an assembly to prt, you just have to "save" the assembly and choose prt. The pieces then become bodies in the prt.
It's a trick I do often. In fact, I receive WWTP from customers in assembly mode (mechanically welded and sheet metal): I open the step in SW and I do "save as" but I change the format: I force it to SLDPRT. SW therefore saves the assembly as a part and all the parts of the assembly as a body in my part file. This allows me to do a sheet metal function recognition and to go through the SheetMetalManufacturing mill and others in a single step. On the other hand, there is no link between the part file created and the original assembly.
I also made file saved under but it was when modifying the assembly, whereas here the part keeps a link with the assembly and in case of biting a part in the assembly, it updates in the part created from the assembly.
@Rim-B with a "registered under PRT" parts become solid without the functions. I would like to keep the design integrity of the piece. And when I validate the recognition of functions when opening I get an error of overlapping volumes... However, it is not abnormal for parts to be in contact in an assembly...
Out of curiosity; What is the goal? For me, it was to limit the weight of the final assembly by transforming all the sub-assemblies into parts that save time at the opening and in fluidity.
I am attaching ac-cobra, for what purpose? It happens rather in reverse, and above all it will complicate the publication of the plans, otherwise is the top-down modeling not enough!?
Yes, reducing weight is part of the goal. I also want to have an independent "complete assembled object" file, complete but not dependent on external references. This facilitates, shares, stores, and at least ensures that the object can be exploited no matter what.
In my ideal world, I would program a macro that would just create a blank PRT file from an open assembly, extract the trees of each part in the assembly and copy them into the PRT (renaming items if necessary) but modifying the local origin of each part by the origin of the assembly, to ensure that their placement conforms to the assembly.
So first of all, thank you for the trick that I didn't know about and that will inevitably be useful to me one day. Unfortunately it does not respond to the request, but I understand the confusion because the word "merge" that I used is not the most appropriate. We had to understand "group".
I'm a bit lost, because I don't really understand whether to have a part with bodies or not because it can't be modified and the visual will be the same as a file saved in prt.
So first of all, my error in the recognition of functions is caused by the screws from the toolbox. If I exclude them from the loan, the recognition goes well. It's a shame but hey, let's just say it's already not bad. Except that apparently you have to manually run a function recognition for each imported object, one after the other... We can't do a multiple recognition??
I probably expressed myself badly but to be clearer, let's say that I want what "register ASM as PRT" does, except that I don't want to have to go through useless reconversions of geometry conversions, nor a (des!!) recognition of functions. I want to keep functions, relationships, quotations, original names. A stupid cloning of the original tree of each room* in another common room, you know. (even more qd I see the time it takes to recognize the functions and that you have to restart it for each of the parts..., then rename them...). In the common room tree, the room trees should be hierarchized in individual folders of the room names.
We would be more on the "join" tool but without merging, just an addition of each tree*, as is, one after the other in the new target part. A concatenation without conversion, as a result. And always, ideally, in separate folders (in the featureManager eh).
It seems that only a macro will be able to meet these requirements
*When I talk about "original tree", I mean "all the functions, plans, etc. that make up the room".
In fact, I would like all the parts of an assembly to be "embedded" as they are in a single PRT. The only difference visible in the tree is that the yellow "part" icon becomes a blue "folder" icon.
And indeed, it would allow you to edit all the "parts" (their functions grouped in folders) from the common room.
I don't think it's possible to do that The only way is to anticipate and build in a multi-body room and it won't help you in terms of lightening the part compared to an assembly because it's the functions that are heavy ... Good luck because you're going to need some
Hello Basically, what you'd like to do is use the " insert part " function but instead of a part, it would be an assembly (impossible with this command) and be able to use the " propagate from the original part" option. I specify that you have to break the link with the original part to recover the construction tree.
The whole problem is in these two words: extract and copy. In other words: copy/paste...
Scanning the assembly component tree to identify the " source " parts is easily conceivable, but to my knowledge there is no copy/paste procedure of the build tree of each " source " part into the same " destination " part. The only entities that can be " copied " from one part to another are sketches, curves, surfaces, and bodies, not geometric features.
In the absence of concatenation in a part, another avenue can be explored, which allows the backup to be reduced to a single file: virtualize all the components, i.e. integrate them into the assembly document. The logic meets your expectations, even if the final document is an assembly and not a part. The " Make Virtual " feature exists in the SolidWorks APIs. The links of the virtualized parts to the original parts are broken, but the build tree is preserved.
