I am a follower of the use of the skeleton regardless of the software. One of the designers I work with used the skeleton method by inserting a piece (the skeleton) into another piece. It uses the sketch profiles from the skeleton directly in the functions. It does not involve the creation of a sketch, since it already exists in the skeleton. The problem: As soon as this function is created, we can see the sketch of the function, and edit the sketch, knowing that it comes from the skeleton. We edit the function , and there the sketch is not constrained (So blue) + (-), and we can move the sketch strokes without any problem. No constraints, no dimensions, and as soon as you validate, the piece is in freestyle mode.
My question, how do we insert a part into a room with these sketches, and as soon as we use it in the function, that the sketches are constrained??
A real problem that forces us to create plans, and create a new sketch where we project from the skeleton sketch to the new sketch.
very dangerous problem for the reliability of a project
Hello +1 with @Sylk Otherwise, in the import of part 1 in room 2, you have to select the elements to be imported (sketch, dimensions, etc.). On the 2024, the edition of the sketch in the context of the second piece is not possible.
Also, I am not very fond of the use of the skeleton in CAD. I used it with Inventor, having it is to be faster in design, but I don't really believe in it, here is an article that corresponds to my knowledge=> https://cadxp.com/topic/40790-squelette-pour-ou-contre/ On Solidworks, a skeleton is used for a complex part that has the same shape, for example a hexagon or others. That is my opinion. Good luck. @+. AR.
Hello A.R. And yet the skeleton on large complex assemblies or not, I won't go back, especially when you don't know where you're going!! But I understand it depends on the size of the assemblies, but handy when making dimensional changes. But nothing is perfect, and I even less On inventor no problem, but as any skeleton rigor and methods are the key elements
Thank you for the feedback. The options you offer are well selected. Now Edit one of the functions, and move one of the sketch elements. And validate, I'll let you admire the result
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
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.
I think you can report a bug at SW. I am on SW2020 Sp 5.0 and I am indeed behaving abnormally:
It is impossible to edit the sketch by clicking on it (it has its little prohibition logo) which is normal
but it is possible to edit the sketch by using the right click ' Edit Sketch ' on the function that uses it (and there it is indeed blue): abnormal
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...)
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.
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