Fusion R.U.L.E #1 and #2

[TrippyLighting]

[Post modified to remove "360"]

Fusion R.U.L.E #1
When in doubt, before doing anything, create a component and make sure it's activated.

All objects created after activating the component such as sketches, bodies, construction geometry, joint origins, etc.  are created in that component.

This has several advantages:

1. On activation the timeline is filtered to show only those items in the timeline that pertain to that component. That will make the quickly growing timeline much easier to work with.
2. If a component is exported to the data panel with "save as" this will also export the complete parametric design history.
3. The joints in the "Assemble menu only work with components.
   Drawings can only be created from components
4. Only components show on the BOM.
5. Only components can be added to selection sets.
6. Only components can be isolated.

When another component needs to be edited for example to add geometry, it should be activated before doing so.

the above points apply to assemblies as well.

Exceptions to R.U.L.E #1

There are a number of other workflows that are  perfectly valid but the first step would not be creating a component. For the most part these are top-down design workflows:

1. When you create a skeleton sketch that carries features of several parts of the design and is used to extrude or otherwise create several bodies that then are turned into components. That conversion into a component, however, should happen as soon as possible because features added to a body contained in a component are all added to that components design history.
2. When the design starts with a T-Spline for example the exterior shell of a product that is then split int one or more bodies. Here also conversion into a component should happen as soon as the bodies are created.
3. A design for a single part to be used as an external, linked component (X-REF) in other designs. No component creation is necessary in this case as that design when inserted into another design is inserted as as a component.

 This is also well explained in this 6 minute video tutorial.

Fusion R.U.L.E #2
Name Your Stuff!

No explanation necessary...hopefully 😉

[TrippyLighting]

Please iost it in the Idea Station and link back here.

[elh.maayan]

https://forums.autodesk.com/t5/ideastation-request-a-feature-or/quot-r-u-l-e-1-quot-should-be-implem...

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@TrippyLighting wrote:

Please iost it in the Idea Station and link back here.

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[CLmoss]

Right, so you know, I am designing one thing only and that is a 19" 3-Unit (5.25" tall) Rack Mount Enclosure. That is it.  Also, I am only designing in Fusion what the CNC and Sheet Metal shops need to produce a few of these. I am not designing in Fusion a complete set of assembly drawings.  The Front Panel will need to be milled in a CNC machine includes two 0.25" plates.  What I call the Cage which is the back of the enclosure, has more parts to it. These will need to be stamped and bent.  The Cage parts will have PEM nuts in them. That is it for my use of Fusion right now.  This enclosure will contain the electronics I designed already.  

So, that is my story and I am sticking to it. 🙂

JM

I think I posted to the wrong thread. Oops

[Anonymous]

Very nicely worded and organized.  Most Excellent 🙂

[Anonymous]

Very helpful at all. Thanks a lot

[Anonymous]

As a total noob to Fusion (and anything 3D!) I must say that rule#1 is confusing for a complete starters. Last night I redid my design which I've been working on a few hours a day for a week and did now use components. While this went faster and makes much more sense I think the order of learning for a newbie is

1. learn how to sketch
2. learn how to create bodies and sketch on faces
3. Repeat until you feel comfortable
4. learn about and apply rule #1!

Bram

[lichtzeichenanlage]

I'm a beginner and had no problem to understand this rules. The only thing I can't understand is, why F360 does not create a empty component if I create a new project.

[ToddHarris7556]

@lichtzeichenanlage

Not a definitive answer - but I'm assuming that when you say 'new project' you're referring to a new Fusion Design. In that case, it's probably because each Fusion design file is intended to function as a standalone part by itself. There's no need to create a container component if your design were, for example, a nail. A single body would be enough. Then the Fusion design itself could be inserted into another design, where it would show up as an externally linked component. The container component within would be unnecessary layering. 

[TrippyLighting]

Each design in a Fusion 360 project is already a component. Here's a screenshot of a fresh, yet unnamed component:

So in case you only want to design one discrete part like, for example a single gear for 3D printing you don't need to create another component within that design.

If you want to create more than one discrete part, because you want to design an entire gearbox in one design (file) with all the gears, gaskets and fasteners, then maybe you should start creating a component.

In that case the top level symbol in your design file will change to that of a component group otherwise also called assembly:

As such in most cases it would not make much sense to automatically create a new component in a new design file as it would really create an assembly with one component in it.

The other reason that it is not advisable is described to create a new component automatically in one of the exceptions of R.U.L.E #1 and that is if you create more than one body from a single sketch and then turn each body into it's own component. Thats a valid and sometimes very efficient workflow and creating a new component automatically would not work.

[lichtzeichenanlage]

@ToddHarris7556: Yes, design not project. Thx for correcting my wording

@ToddHarris7556, @TrippyLighting: That's a great explanation and a totally valid reason. Now I understand F360 a bit better.

[nevetsnikam]

Am I missing something?
Common sense would say if that's the number one rule then why does the program not default to a new component or at least present you with an option on creating a new sketch. Or is that just too logical?

[TrippyLighting]

This has been asked before, but I would not support that idea.

The key here is to understand some of the concepts behind Fusion 360. Granted the initial post of this rule did not address that, but that was not the intention behind it either.

If you build a mechanical design, maybe a machine then most discrete components will only contain a single body. You'll have many components and in that case it is best to start the design of each discretion part with a component.

However in product and industrial design it is very common to build a shape comprised of many bodies. Then that final shell is often split into unique pieces, e.g. for injection molding. 

In that case you would not start with a component (this workflow is listed under Exceptions).

After you've split the shape into the discrete pieces you might turn each of the pieces into a component.

Also, each new design file in Fusion is it's own component already, so if you are designing a singe object, say for 3D printing, there is no need to create another component in the design. That's also an Exception to the rule.

[lichtzeichenanlage]

You missed the same thing I missed. Here is the answer (again from @TrippyLighting)

[GRSnyder]

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@TrippyLighting wrote: Each design in a Fusion 360 project is already a component.

You know, this seems like quite an important thing to know, but it's really not obvious in the UI. I had always assumed the top level was a different kind of entity, e.g., a "document". Fusion 360 even points you explicitly in that direction by including a Document Options blob. (Where would document options be found if not in a "document"?)

The top-level component never gets gets much opportunity to demonstrate its component-ness. You can't assemble it to anything else. You can't work outside its context. 

But now that you point this out, it seems blindingly obvious to me that the missing feature isn't a preference for "auto-create a subcomponent in new documents" but a Demote command that you can apply to an existing component. Demote would create a new component at the same level as the selected component and then move the selected component into it as a subcomponent. Root-level entities like Document Options would be bumped up a level automatically.

You can already do this by hand for any component but the root: just do New Component and then drag the old component into it. But you can't do it for the root.

This is really what Rule #1 is about, is it not? You can't restructure the root, so if you need structure, you better create it as your very first step. But if you could demote the root, Rule #1 violations would be trivial to fix and there would be no need for Rule #1 at all.

[lichtzeichenanlage]

I'm just a hobbyist, but I can not agree to your argumentation

• Sure, you can move a sketch from a root component and all the related features will follow. And you're right, that it doesn't work the same way if you want to reverse the process. But IMHO the conclusion is wrong. I would say, that if you have sub components, the root component should only contain common thinks like sketches or planes used in several other components. Sure, you can use such things across components, but it's a nice documentation of your thoughts if you move it to a common layer. 
• You can create an As-Built-Joint between the root component and any other component as a replacement for the Ground feature. You can find a video and some thoughts about this topic here.
• There is at least one other component type, that has a settings sections. Just look at the sheet metal components. And this describes the behavior of the inside of the component. That's what document settings are doing, too. That makes sense to me. 
• Allowing several roots is more of a philosophical discussion for me. If AD would allow more than one root element, they should shouln't keep the document settings inside a component and they should move it a level up. But since you can just start a new design and insert the previous one, there is the way for "several roots". And by the way: The documents folder is then no longer available in the imported component.

[GRSnyder]

I don't think I explained myself very well. I'm not suggesting that it be possible to have more than one root. 

The idea is just that if you have a situation like this where you forgot to apply Rule #1:

     

You could then do something like this:

     

To achieve this:

 

In many cases, you can achieve a similar effect by manually creating a new component and dragging sketches and bodies into it. But sometimes the situation seems to get too complex to allow this.

Nothing about the component or document model would change. In particular, you could still create entities at the root level, just as you can now. You'd just have the option to move all the non-document-related entities in the root down a level as a unitary operation. Because everything moves at once, dependency interlocks aren't a problem.

My claims are that if you could do this:

1) Literally nothing about the existing UI or conceptual model would change, and

2) There would be no need to drill Rule #1 into the head of every new Fusion 360 user, because failure to follow Rule #1 could be fixed in one step.

[TrippyLighting]

I've looked at hundreds of Fusion 360 assemblies here on the forum from simple to complex, from noobs to pro's. I don't think a single demote feature would be able to address the number of situations that arise.

The first thing that is need in order to determine what went wrong is to see all the relationships between objects. Another user first called this a dependency graph and it could be implemented for example like a node system perhaps similar to SideFX Houdini.

Then in order to fix things you need to be able to re-connect the node connections. However it is implemented, full visibility of relationships is needed.

There are many tools where Fusion hides complexity and makes assumptions on a users behalf. What is needed for advanced users is another deeper layer of access to data so we can fix what's broken. I don't think that can be addressed with a single feature.

[chrisplyler]

There is an exception to Rule #2: When you need it to be named "Component."

[GRSnyder]

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@TrippyLighting wrote: I don't think a single demote feature would be able to address the number of situations that arise...[need to] see all the relationships between objects...re-connect the node connections...What is needed for advanced users is another deeper layer of access to data so we can fix what's broken. I don't think that can be addressed with a single feature.

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This sounds wonderful and I agree that it would be of great benefit. But it's clearly a heavyweight development project that doesn't appear to be on the current roadmap. That is not a reason not to advocate for it, but realistically, it probably doesn't have much chance of appearing in Fusion 360 within the next couple of years.

I'm not trying to answer the general question, "How could Fusion 360 better support arbitrary reorganization of elements among components?" I'm asking, "Given that there is an obvious pain point within Fusion 360 that necessitates Rule #1 being propagated as oral folklore, is there a simple, low-impact change that might help to alleviate this specific issue?"

Auto-creating a subcomponent in new documents is one possible approach, but it has some drawbacks as noted in this thread. I'm proposing something that I think would be less intrusive.

I also wonder if you're interpreting my suggestion in the following way:

    

I actually had in mind something far more stupid and less generally useful:

     

The point being that if all relative relationships are preserved, there shouldn't be any real change to the dependency graph.

Yes, the need for a general solution for sorting out dependencies would remain. This addresses only the problem of "Oops, I accidentally made a few things in the root and now Fusion 360 won't let me drag them into a new component."

[Anonymous]

How can i show hide the left side model tree of show hide parts in fusion 360