Sylk
I'll let you look on the forum, a skeleton topic that I launched.
The problem is that with this method the reliability of the sketches is not good. As soon as a function is edited, the sketches are accessible and can be distorted because they are not dimensioned and not constrained
I just retested, so indeed the sketch is not constrained on an origin or anything else so it moves in space (not to mention that once the positioning is validated I have SW which makes me crash).
Maybe using the blocks?
Cyril
I just tried but it actually crashed SW.
I'm trying to find a solution, because the only solution that has been found is to block the parts in the tree. and the updates are blocked and when you have 1000 coins, the updates are a bit long!!
Cyril
But when there is no crash, it's artistic.
And above all dangerous because it is unreliable.
Imagined, you move the sketch a little and then it's the drama.
If the solution comes to you, I'm a taker 
Hi FRED78,
I confirm on Inventor it works well... As you say, no one is perfect... 
@+.
AR.
Hello again FRED78,
So here is an article from August 2024=>https://forum.mycad.visiativ.com/t/methode-squelette-solidworks/111471?locale=fr&lang=fr
And maybe this one =>https://www.reddit.com/r/SolidWorks/comments/salzdq/advice_for_good_habits_for_large_steel_structures/?tl=fr
Good luck, @+.
AR.
Personally, I'm more adept at the Master Model method with or without a basic sketch (what you call the skeleton).
.
Here's where the illustration above is taken from:
SolidWorks Webcast: Episode 17 — Spanner
SolidWorks Webcast: Episode 18 — Spanner
Unfortunately, this method, which I particularly like, currently suffers from a bug in the Save bodies function, a bug of the kind that is annoying but not insurmountable.
As for the problem of sketches transferred via the Insert Part function, some have submitted it in the improvement ideas:
But since the gentleman didn't use the form and wasn't clear enough for the team that collects and analyzes the ideas submitted, well they simply took it out...
I confirm on inventor it works well.
I make an assembly of several skeletons with the master method (revisited) mentioned below.
This allows me not to have skeletons with 100000 sketches. Easier for those who have to start back, even if there are research solutions on inventor.
The principle also applies to solidworks, but I prefer to make an assembly of several skeletons, example GC, structure, etc...
I would like you to develop the subject in a post. Would be instructive.
What is the bug? I don't use this function but it can be interesting in a context with method. But this is the principle of a WWTP
The Save Bodies function allows you to save each body as a part from a multibody part design, if necessary to redefine the location of the origin for each body in the destination part file, and to be able to generate an assembly file automatically.
(I love this feature 
)
A posteriori, it is very easy to re-register a new or existing body in a new or existing file, not only from the master model, but also from the destination part file.
The bug: if everything goes well when the function is created (yes, Save Bodies creates a function in the tree) it's at the first re-edit of the function in the master model that everything goes wrong.
→ the origin locations of the bodies that may have been defined are lost, and all derived parts have their origin match the origin of the master model.
SPR323068 - DS Support Knowledge Base / Bug Report
The workaround is to replace the body with a move/copy function.
Yes indeed I know, it's the same principle finally your different bodies registered in several rooms allow you to insert them with the same origin
Good evening
I think you can report a bug at SW.
I am on SW2020 Sp 5.0 and I am indeed behaving abnormally:
I personally think that the second possibility is a hole in the Solidworks racket: this editing possibility should NOT exist for an imported sketch of a part.
I'll let you report the bug to SW (lucky little guy goes...)
Thank you for your feedback,
Why lucky boy?? 
Basically, I don't use this method on solidworks to insert one part into another. For less than that (thread on MEP) I have problems.
I recommend a very different method with a skeleton in an assembly. Method that works correctly, everything is in external reference. Advantage, you know where to look for references, and there is no longer any constraint. But others have decided to do otherwise.
The problem is reliability! But isn't this function misused? Originally it is designed to integrate WWTP or Part in a multibody part. It's a gimmick.
Moreover the problem was found by someone other than me, and I leave the paternity to him. This person has chosen this method. I gave him the solution to solve this problem. Dassault is not too far from his office.
In short, the solution to remedy this inconvenience, create a sketch plan on the skeleton, create a sketch on this plan and project the skeleton on it. It is no longer possible to access the sketch (-) of the skeleton by the function.
Solidworks is a great tool, too bad there are all these problems, and often the PC is one too.
Hello again FRED78,
So here is an article from August 2024=>Skeleton Method / SOLIDWORKS
And maybe this one =>Reddit - Dive into anything
Good luck, @+.
AR.
Yes I think I know the author of the first topic 
, I started this post hoping to find the solution to this problem
For the second one, I'm going to read it.
We use both methods at home.
Mainly the pilot sketch in the assembly with external references (all parts being virtualized to avoid having assemblies driven by another assembly: problem of updating external references during copies).
The part inserted into a part is more for the remachining of a casting part: at least we know exactly what we are doing. Parts with raw/machined configuration by managing the removal of functions often go to a peanut if the designer does not have a very good command of his creation tree (this is often the case during subsequent modifications to the part).
For the internal parts I'm not a fan.
But if the method and the follow-up is strict and integrated into the customs
I don't have this possibility on my side (SW2022 SP5.0). To add relationships and freeze the sketch, you need to edit the function that uses it and manipulate the sketch. But there is no longer any possibility of going back after recording.
In any case, I completely agree with you:
Hello
It is possible to make an update, it implies a modification of the sketch. I'm not sure that changing a call number works, because they are already there. By adding a line, for example, it should work. To test there I don't have time but I'll look.
We have been offered to block sketch and function changes in parts directly, via the block bar. But I think it's a mistake, it prevents updates, which means acting on all the parts with each modification.
In conclusion, I prefer my skeleton method or working on Inventor, much more stable, less error from the software or the user. I'm changing tack 
Hello
If you start not using a function anymore because it bugs, you can directly change the software...
The art of the Solidworks designer is to deal with the multiple bugs and more or less reliable functions of this software.
In practice for your subject, everything works but there is a possibility to edit a sketch imported from a part (hole in the racket from SW) IF you directly use the sketch of the imported part in a function.
→ You forbid your team to directly use the sketch of the imported part in a function and you force them to go through an intermediate sketch with ' convert entities ': it's stable and bug-free so a good workaround.
Hello Froussel
Yes, you forbid, but you can't pass on in an uncertain future, and you can't always be behind.
But hey, software and bugs become the norm, and frankly we pay for a software for which we report work that should already be done. It is clearly recognized that today companies no longer bother testing their software, releasing a version every two years. No, they make a version every year, marketing obliges, and you test for them...
You want a reliable Catia software, it's not the same price, you want a less expensive SolidWorks software but you have the bugs.
Today, telephone, pc, games, CAD, etc... Companies work the same, you do their jobs, well part of it because I don't know their constraints.
In practice I do with an external skeleton, and external references. Easier and safer in every way. It's good to do it on inventor without any problem but I don't have a bug, graphics and other. However, I am a loyal Catia/SolidWorks customer. But they ended up doing just that, to the detriment of the profession. And I join my managers sometimes the automatic side is fed up with autocad 2D