UX/UI schema and concepts - total confusion

[Anonymous]

Is there a basic one or two page document that describes Fusion 360's UI/UX schema?  I've been reading up on the distinction between components, bodies, designs, etc. and it's still not clear.  And how do these things map to UI features?  I have moused myself into a corner where I have (I think) two components in my design that I'd like to combine, but I can't figure out for the life of me how to do it (screenshot attached).  I have a small rectangular knob as one component and I've started on a machine screw that is used with it, but how do I combine them?

The most maddening part is that I don't even know how to ask the question to do what I want!  People are pretty loose with their terminology in documentation and videos.  Am I trying to combine components?  Do I want to make an assembly?  A subassembly? (is there a difference?)  I've read that Fusion360 doesn't distinguish between a component and an assembly?

Is my first step to turn the body + hole into a component?  I tried that and it didn't seem to open any options.

I also want to rotate the screw object around the x-axis (front<->back), but when I tried that as a component it didn't move the hexagonal hole I created with it.

And what do tabs correspond to?  Components / assemblies?  Something else?  None of the UI docs I've seen (annotated screenshots and such) speak to the fundamental concepts in Fusion360, only unhelpful stuff like "this is the measure menu".

I'm trying very hard to convince myself that I'm not an idiot and the software isn't bad, I just need to get my head around the concepts and learn a little more CAD.  But the concepts themselves in Fusion360 feel so non-orthogonal it's very hard to make sense of it.  And the UI does not help in this regard: in my screenshot are the squares in the left panel components?  There's nothing obvious to tell me what the listing of these things is called, such as a heading that says "Components".  And if I hit the "<" arrow in the upper left corner I see "Projects" and "Samples"... are those types of design objects?  Or is a project an even higher abstraction than design?

For a start, I wish I could just find a simple taxonomy/schema of the types of... things... in Fusion360 and how they relate.  No multi-hour youtube playlists please, just a page or two should do.  Here's a stab at it, based on what I've seen in the UI and documents online, please someone correct me:

Project > Design > Assembly / Component > [Body | Sketch?]

PS - there's a lot of ugly little UI bugs on macOS, I've included one in my screenshot with the low-DPI history tooltip.  Actually, that tooltip appears to be a completely separate Quartz window frame, which is a bizarre choice and probably the reason for this bug.

[Anonymous]

Distinguishing a Body from a Component is easy - a Body will be listed under a Bodies section in the Browser tree, and there will be nothing UNDER the Body in the tree.  A Component will expand to show its Origin, Sketches, Bodies, and other entities UNDER it.  Assemblies are made from Components, which CONTAIN Bodies, but are NOT themselves Bodies.  A Sub-Assembly is simply an Assembly - NO difference whatsoever, other than semantics.

If you're at all familiar with other CAD systems, Components are the same as "Parts" in systems like Solidworks, GeoMagic, etc.  As with most other CAD systems, an Assembly can be used exactly like any Component in a larger design.  In most systems, Parts and Assemblies are actually physically different, and are stored in different file types.  In Fusion, they're actually all the same.  Assemblies and Components are stored in the same way, and can be used interchangeably.  Assemblies contain Components, and can be use in all the same ways as Components.  So, the only real distinction is in how YOU decide to create and use them.  Fusion itself does not really distinguish between them in any significant way.

The unofficial Rule #1 of Fusion is always create Components, in the same way you would start by creating Parts in other CAD systems.  You do have a choice as to whether you create a bunch of components, each in its own file, or create a bunch of components in a single file (NOT an option in most CAD systems).  There are benefits and costs to either approach, and only you can decide which approach makes the most sense for the way you choose to work.  You also get the choose whether you copy external components into an assembly, or link to the original component file.  There, again, there are benefits and costs.  These are all things you can really only learn by doing trial designs, and seeing for yourself how each approach actually works, and what limitations each approach imposes.

ALL 3D CAD systems have a steep learning curve.  Fusion is, in some ways, worst than most, in that it gives you so many more choices than most, and also does things in such a fundamentally different way that most other CAD systems.  If you're coming from another system, the hardest part of learning Fusion will be UN-LEARNING what you already know, as much of it no longer applies.  Personally, I've used many CAD systems, most recently Solidworks, and I REALLY like Fusion, for the most part.  It has its problems, and is still VERY much a work in progress, but the overall concept is great, and when it's finally "done", it is going to be really something special.

The best advise I can give is watch lots of tutorial videos, ask lots of questions here, and be patient.

Regards,

Ray L

[Anonymous]

Thank you for the reply, it's helpful.  I still have some questions, though.

> Distinguishing a Body from a Component is easy - a Body will be listed under a Bodies section in the Browser tree, and there will be nothing UNDER the Body in the tree.  A Component will expand to show its Origin, Sketches, Bodies, and other entities UNDER it.

Telling me that origins, sketches, bodies, etc. show up under components in the UI is something I can see for myself.   But that doesn't really explain why, and what bodies/components/assemblies are supposed to represent.  I've come to this understanding, correct me if I'm wrong:

- Bodies are abstract 3D shape definitions that are used in the construction of components.  They are basic geometry that can be parameterized and combined (intersect, etc.) but do not themselves represent a real-world thing.

- A component represents a concrete object, a real-world thing that can be created.  It is defined by and contains bodies (and axes, origins, sketches, etc.).  Conceptually it is a single piece of solid, combined geometry.  A single unit.

- Assemblies (or subassemblies) are logical combinations/groupings of components, where "logical" is relative to the project and a judgement you as the designer must make.

And although there is a conceptual difference between components and assemblies as a matter of CAD convention, Fusion360 doesn't distinguish between them.  Which raises the question: is an "assembly" even a concept referenced in Fusion360?  I mean, is there any "Create assembly from components" button?  Does the word "assembly" appear in the UI at all?

> ALL 3D CAD systems have a steep learning curve.  Fusion is, in some ways, worst than most, in that it gives you so many more choices than most, and also does things in such a fundamentally different way that most other CAD systems.  If you're coming from another system, the hardest part of learning Fusion will be UN-LEARNING what you already know, as much of it no longer applies.

The only CAD I can say I genuinely have a handle on is OpenSCAD, which is much simpler and wildly different.  To even call them the same class of software is probably a stretch.  You're absolutely correct that the hardest part is the proliferation of choice.  The program gives so little guidance and feedback about how organizational choices in your project will affect things later that it's very hard to have the confidence to spend time and effort fighting through learning the little details of designing your parts without knowing if you'll end up in a dead-end and have to redo everything.

> Personally, I've used many CAD systems, most recently Solidworks, and I REALLY like Fusion, for the most part.  It has its problems, and is still VERY much a work in progress, but the overall concept is great, and when it's finally "done", it is going to be really something special.

This sentiment is good to hear.  That Fusion360 is not fully baked reflects my experience, it's good to hear that I'm not perceiving that incorrectly.

> The best advise I can give is watch lots of tutorial videos, ask lots of questions here, and be patient.

There's a lot of terrible tutorial videos for Fusion360, and even the good ones show interfaces that are older and subtly different.  And virtually all of them are long-winded to the point of exhausting the viewer.  Fusion360 would really benefit from something like the gifrecipes phenomenon, small and focused <1minute videos that show a single technique cleanly and with no filler.  Even better if they are silent, to force the discipline of showing the technique and not saying it.  Of course, the UI would have to be self-explanatory enough for this to be possible, which I don't think it currently is.

Asking questions and being patient are always excellent advice.  Thank you for reminding me.

[cekuhnen]

@Anonymous @Anonymous

I think you are overcomplicating things.

In fusion you have a design.

The design starts with a xyz 0 point. Then you can add sketches onto the XYZ planes and add geometry features.

But if you want to work with assemblies you need to have components.

So with a new design you create your components. Each component then has their own XYZ 0 point.

This is important to understand.

The main design file has a globale XYZ while components have their own local XYZ.

This is important to understand because when I in an assembly preposition a component the component XYZ 0 point in theory is further way from the global design XYZ

yet when you edit the sketch you see that locally nothing changed.

Fusion has actually a pretty low learning curve - 3D however is not always easy like ShetchUp. When you understand the concepts of solid surface parametric modeling

you can easily jump to any app. It is then only the quest to find where what function is in the UI.

Yes many published videos are already outdated because the UI changed. But again when you know the foundation this does not matter.

What can be helpful is also to meet online and have a short screensharing session to help.

[Anonymous]

> I think you are overcomplicating things.

>

> In fusion you have a design.

>

> The design starts with a xyz 0 point. Then you can add sketches onto the XYZ planes and add geometry features.

Ok, right off the bat I have no idea how what I intuitively know of as the English word "design" maps to the UI in Fusion360.  I'm going to assume that the whole interface represents a design.  But when you say "the design starts with a xyz 0 point" do you actually mean "a design starts with a single component that has an origin, and until you work with more components this single component's origin effectively is the global design origin"?

Or does that mean that a brand-new design actually doesn't have any components?

And for clearing up what a design is, in the Data Panel, if I click "<" it takes me to a top-level navigation of  lists of "Projects" and "Samples", with a button for "New Project".  Is "project" synonymous with "design"?  Or do projects contain multiple designs?  Or is that data panel just a huge waste of time that I should ignore?

> So with a new design you create your components. Each component then has their own XYZ 0 point.

> This is important to understand.

>

> The main design file has a globale XYZ while components have their own local XYZ.

> This is important to understand because when I in an assembly preposition a component the component XYZ 0 point in theory is further way from the global design XYZ yet when you edit the sketch you see that locally nothing changed.

I don't believe this was the source my confusion.  I've done enough graphics programming to know that independent relative origins and axes are important when composing smaller things into a larger things.  I figured that was integral to building multi-part designs, which is why I already started down the road of having two components.

> But if you want to work with assemblies you need to have components.

This is where the confusion is.

I didn't even know that I needed an "assembly" for what I was working on, and so I didn't even have the vocabulary to ask the very simple question that would get me this answer.

But it raises more questions.  So, are assemblies required for any multi-part design?  @Anonymous indicated that Fusion360 doesn't really distinguish between components and assemblies and that I could have a component with multiple independent things in it, but I've looked at some videos (official AutoDesk ones) and the presenters imply that there's a big difference between components and assemblies which just reinforces what you've said.  So which is it?

There's no doubt that a huge part of my confusion is that I'm a relative newcomer to serious CAD like this, but I'm still really fuzzy on how Fusion360's data model maps designs/assemblies/components.  I'm being a real stickler here for terminology because being precise with words is the only way users who aren't CAD experts can help ourselves and find documentation.  I'd love (prefer, really) to have an intuitive sense of how all this fits together, but I just don't think that's in the cards for Fusion360 beginners so I'm trying for a more intellectual understanding of it.

BTW, if desiring precision in communication is "overcomplicating things", well... guilty as charged.

[Anonymous]

UGH.  Staring at the interface (screenshot from first post), I just realized that the data panel is showing two designs, and I thought they were components.  I think that clears a few things up for me:  the data panel is showing an entire project, which contains multiple designs ; the main window is showing a single design and I want my multiple components in there.

[cekuhnen]

@Anonymous

Hoenstly some concepts are easier to explain via a screensharing which I could do for you.

[daniel_lyall]

@Anonymous Have you read through the support and Learning section.

[Anonymous]

@cekuhnen, I think I may take you up on that.  I'm going to hack on this over the weekend and maybe I won't need it.  I'll reach out if I'm still struggling in a day or two.

@daniel_lyall, are you referring to the Support section of the forum or a different resource?

[daniel_lyall]

Look at the very top of this page http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-18445C60-F9AD-4217-8066-CA48FA11E514

There are a couple of user manuals they are on amazon https://www.amazon.com/s/ref=nb_sb_noss_2?url=search-alias%3Daps&field-keywords=Fusion+360

And there is one in the forum whats done by a user a link to its here https://forums.autodesk.com/t5/design-validate-document/pdf-user-manual-for-fusion-360-ultimate/td-p...

[TrippyLighting]

Hopefully my screencast helps your understanding.

In one of you posts above you perfectly describe the difference between bodies and components, which is a very important distinction  many new users don't get.

As such in order to work successfully with components I will refer you to Fusion 360's R.U.L.E #1, which is the second link in this link collection.

Also in that link collection is another link to recorded classes from Autodesk University. The 1st two explain basic concepts, which would put you well on your way. Once you get your feet a little wet, I can recommend the others.

[cekuhnen]

@Anonymous  Yeah ping me or others here to help. You questions for me are not difficult answers are pretty easy yet text is not the ideal start.

Here is a quick vid about global local space components and timeline

https://drive.google.com/file/d/0Byzv_NlyKp_2Y3RwYmxqLTFqMUk/view

Here is one about joints/assembly and why we group bodies in components and do joints only with components

https://drive.google.com/file/d/0Byzv_NlyKp_2TWhZSmxMdWRHM0U/view

[Paul.Normand]

Do you know about the guided tutorial learning experience in Inventor? Each lesson consists of a series of tasks that includes the model in the correct start state for the task, and a task video that is approximately 1 minute long. The tutorial also contains a text panel that describes what the video is showing and active pointers to the commands being used. You can start on any task in the tutorial to focus only on what you need to learn (without having to do the whole tutorial up to that point).  Does it sound like this is the type of experience that would help you in Fusion?

[daniel_lyall]

Yes