Fusion
Accepted solution
Hi thoralin -
So - there are a couple of things in here....first: I'm guessing you couldn't move the components you wanted most likely because another command was active. Its a guess....a complete shot in the dark. Normally I would say there is some timeline issue, but you say you checked that....so it's all I've got. (or - you indeed did not drag to the top-line...which is where you have to do it.)
Second - OK, so now it works - but yes - you do have to drag to the top line. You refer to these as "containers" but that is not what Fusion calls them. In effect - these top level items are parts....which, when you drag other parts to them, become sub-assemblies. This is something that is kinda special about Fusion 360 compared to other CAD systems. We don't have different file formats for assemblies or parts, so we can switch back and forth all you like. It has many advantages - but you do need to know how it works. (Look for videos or information on Top-Down Design for more on this...) Anyway - to move the parts into a subassembly, Fusion wants you to move it "to" that subassembly (the first time, it will be a part) so this is as intended.
Third - the copy paste at the end of the timeline. This too is something peculiar to Fusion. Since you are basically moving a part out of one assembly (the "top level" assembly) and moving it into another, Fusion wants to record this activity....and it does! Other systems, because they use a different file system (see the top-down stuff from before) DON'T do this - which is considered normal...but is actually kinda weird. By tracking this, we can do some logical, and neat stuff: you could do a boolean operation using a body, then move it to another assembly, and do another boolean, for example. In other systems, if you moved the part, the boolean would go with it....because the move operation is not recorded in the timeline. In your case....how to get rid of it? While I can't really recommend - you could just turn off the history after you've made your changes, but then, you lose the history. If you just want to clean things up a bit - you could select the copy/pastes in the timeline with Shift, and then right click and put them in a folder....that might be something...
BTW - a side note: we tend to view the assembly structure as being dependent on manufacturing, meaning, we want to organize the assembly in a way that "makes sense" for manufacture or assembly. If what you are doing is more about visual stuff - which is totally understandable - then we would indeed suggest selection sets to do it. The key, IMO - is that the assembly is a manufacturing document - and its organization should reflect this.
Not that you are wrong - I'm hoping that the background will help you to at least understand what we were thinking.
Mickey Wakefield
Fusion 360 Community Manager
Hi
Component....part....its the same thing. You can actually have an "empty" component (part) in Fusion....all that means is that this "component" is a subassembly made up of other parts, or something like that. Another possibility might be that someone would add an empty part called "grease"....to account for a tube of grease in the parts list....there are many possibilities - but the driving principle is that these components - even if they are empty, are not simply organizational "folders" - they are parts! The way I think of it is that every time I add a component - it WILL appear on my parts list. Its not just an organizational thing.....hope it helps.
Re: making part moves "optional" in the timeline....not possible, if you want to keep using parametrics. This, again, has to do with the data structure of Fusion. Short version: all other CAD systems I know have the concept of parts, and assemblies. Parts are created just like in Fusion, for the most part, but then, to make an assembly - one must insert the parts into a separate file type. This is a separate file, and they have a different file extension. When you open such a file, you are not actually opening the parts in it - these are referenced from the original part files, and their positions in the assembly are defined by constraints that are stored in the assembly, not in the parts. When you move stuff about in the assembly - the standard in the other CADs is that they aren't 100% parametric, really, inside the assembly....you move things....and that is that. You can undo - but you couldn't really move, do something, and then move the part again. I should note that this is a big simplification - some tools out there have indeed added features to make this possible, but all of these work around the basic structure of this referenced file system.
When we made Fusion 360 - we elected to do it differently because of the many advantages we would have by only having one file, with everything in it. We don't have referenced files by default - so, among other things, it means that when you open a Fusion assembly - it opens without trouble. In most other systems, that assembly goes looking for all the referenced files and starts spitting out errors because it can't find them, or doesn't have access to them. (this is admittedly a bigger problem in big companies than with single users) It also means that when you are designing something like a coffee machine - its likely that because all the parts of that machine are referencing the same sketches, reference geometry and such - if you make any changes, the machine's parts are more likely to remain "fitting"..... and indeed - you can even do stuff like the boolean I was talking about. A more concrete example: imagine you make gas grills. These all have an igniter on them. and that part needs to be "set into" the face of the grill. In Fusion - its a snap to make an assembly of the igniter and to include a body (not a part) of the support structures around it, all the connections, etc. If you place the igniter assembly into the grill face - you can easily add the support structures to the face of the grill - which is actually a separate part. Stuff like this is very handy.
There are disadvantages of course. From your point of view, one is that we must account for the movement of parts in the timeline, and this causes extra entries. I think that is very much a benefit. Another, more important issue is that a part designed in a top-down assembly is ALWAYS a part of that assembly - so one of the most obvious issues would be if you attempted to re-use such a part in another assembly. You may do so - but when you insert the part, you are effectively inserting the entirety of the other assembly as well! It is for this reason that Fusion does indeed allow you to use a bottom-up approach if you wish. If you do - it will behave just other CAD systems do. A great many people do this, and they call the method "rule number 1".....I must admit - I'm a huge fan of top-down design, so I don't prescribe to the idea that one should ALWAYS use rule number 1....but if you understand both methods - you'll be able to decide which is best for you.
Mickey Wakefield
Fusion 360 Community Manager
PS - moving sketches around is a different story. These are INDEED in a folder. They are generally - following the top-down principle - not in a part....they are at the top level! But you can't move sketches from INSIDE a part to another part without a copy/paste, and moving them about in the folder doesn't really do anything. ALL this is only true if you are working with history on - if you turn it off - you can move everything all over the place, I would guess.
Mickey Wakefield
Fusion 360 Community Manager