Learning Fusion 360 Underlying Principles

[juliangall]

I have come to Fusion 360 from Sketchup and have no background in CAD. I feel I understand exactly how Sketchup models work and what is happening when I use the various tools and manipulations. When I'm editing a Sketchup model, the parts of it feel real, physical, to me. However, after going through the Fusion 360 tutorials and creating some models, I don't have the same level of feeling and understanding of Fusion 360.

For example, if I already have one body, I can use a create command to create a new body, merge a new body with the existing body or cut/intersect the existing body. If I select Cut for the second body, what has actually been created? Is it a body the same as would be created if I selected New Body, but invisible? What is a body, exactly, if it can have no physical existence in the drawing apart from its effect on other bodies? This is an example of what I would find helpful to learn. Another example: what does it mean to edit something in the timeline? Am I editing an object in the drawing, or am I editing a command that is then (with all subsequent commands in the timeline) re-executed?

Is anyone writing a book on Fusion 360? Alternatively, can you recommend any books on similar CAD packages that would explain the principles (as opposed to the commands). This is my question, although answers to my examples would help my Fusion 360 learning too.

Thanks in advance.

Julian

[John.Peros]

Hey Julian, those are all some really good questions and completely understandable hurdles for someone coming from the Sketchup environment.

Let me start off with the learning content question.  There is no one currently writing a book that I know of but there is a LOT of learning content out there for Fusion.  When you say you have gone through the tutorials, have you done just the in product tutorials (the lamp) or have you gone through the broader course which includes examples like the box cutter?  If you haven't done the latter, you can see a full list of our learning content here and that would provide a great start and a very solid foundation:

http://fusion360.autodesk.com/learning/learning.html?guid=GUID-CC9A8E39-356C-43EA-9EDD-0E9C1321E0F2

We also have a very content rich youtube page with many videos on specific topics to help you out.  It can be found here:

https://www.youtube.com/user/AutodeskFusion360

In addition to our own content, Companies like Solid Professor (http://www.solidprofessor.com/training-plans/autodesk-fusion-360/), Solidbox (https://www.solidbox.tv/software/fusion360/) and Plural Site (https://www.pluralsight.com/courses/getting-started-modeling-fusion-360-2271) are creating their own online learning curriculums for Fusion right now.

A lot of the non-Autodesk content is free but some has a cost associated with it.  Its definitely worth checking out though.

As for your specific questions, let me see if I can tackle those as well:

1) If you edit something in the timeline you are effectively editing that command at the point in time where it was created and it will then recalculate and could affect any number of commands that came after it if they reference the resulting geometry.

2) When using the combine command with the cut option you can have two different results.  In my attached screen shot (combine.png), the Cube is Body1 and the Sphere is Body2.  The cube is selected at the target body and the sphere is selected as the tool body.  In this case, with the options exactly as you see the result will be that the part of the sphere that touches the cube will be removed from the cube and the sphere body will be consumed.  So in essence, you will be left with Body1 only and it will be a cube with a half-sphere cutout in it.  If you change the highlighted option for "Keep Tools" the result on the cube will be the same, but the sphere will not be consumed.  So you will have a Cube with a half sphere cutout AND the sphere.

3) A body in general is the definition of a volume (or a surface) based on a number of operations and that volume (or surface) has 0 degrees of freedom in reference to other bodies and does not show up in a BOM as a part.  Any body can be turned into a component and when you turn something into a component, you then give it 6 degrees of freedom in relation to other components and you can lock down those degrees of freedom as you see fit (think creating the motion for a mechanism) and Components now become active entries in a BOM.

Hopefully that clears things up for you a little bit but if not, let me know and we can dive a bit deeper.

Thanks,

John

[juliangall]

Thanks for those really helpful answers, John. Just to clarify your answer 2, I understand this is what happens when you combine two bodies using the combine command. However, it is also possible to achieve the same effect (as I understand it) by creating a second body that touches the first, and then selecting New Body, Cut, Intersect etc from the dropdown on the new body (e.g. Sphere) dialog. It seems that this Sphere command actually performs different functions depending on what you select from the dialog. i.e. It creates a sphere as a new body, modifies an existing body by adding a sphere to it, intersecting a sphere with it or subtracting a sphere from it, or creates a sphere as a new component. I am used to less powerful software where a command does just one thing, although I can certainly see the benefits of this. As a beginner with Fusion 360, I would find it helpful if the tip boxes were clearer. e.g. The Create Sphere tip says "creates a solid body sphere", but that's not the whole of it. I can also understand why you wouldn't want to clutter beginners' tip boxes with too much information 🙂

I have been through many of the video tutorials including the box cutter, but they seem to focus on telling you the commands to use, rather than helping you understand what's actually going on. e.g. Your answer 3 about what a body is, is really helpful and just the sort of thing that helps me understand the software. Where do you learn that sort of thing? 🙂

Thanks for your help. Much appreciated.

Julian

[TrippyLighting]

The introductory videos an written documentation in the "Learn" section is very helpfu and watchin the videos takes less than one hour.

Do yourself a favor and watch these.

The there is Fusion 360 Rule #1. The first thing you should be doing is to create a component and ctivate it. For newly created components activation is automatic.

This link explains the difference between Bodies and Components.

[juliangall]

Thanks, TrippyLightning.

[John.Peros · Accepted solution]

Ah, I see what you are saying Julian.  Yes, when creating the sphere you can get kind of get the same result as the combine command.  If you create the spehere and choose "Cut" you will get the same result as combine if you have keep tools unchecked.  There is no way to get the result of combine with the keep tool option checked though, that can only be created through the combine command.

As for the full list of commands you see, here is what each of them do just in specific:

Join - Adds material to the existing body intersected by the operation.  If the operation crosses two or more bodies, it will combine those bodies as well (you can prevent that by hiding bodies).

Cut - Removes material to the existing body intersected by the operation. If the operation crosses two or more bodies, it will remove material from all bodies (you can prevent that by hiding bodies).

Intersect - The result will be the intersecting volume of the two bodies

New Body - Creates a body that behaves as described in my first post

New Component - Turns the body into a component immediately with 6 degrees of freedom

Just to add something to the body vs component discussion for you, when you decide to create a component affects the history of that component.  If you do a sketch, then extrude a body, then convert the body to a component the only "history" of the component will be the convert to component action.  If you create a component first and then do a sketch and extrude the full history will be contained in that component.

I learned all this stuff simply by using the software and asking questions because they isn't much of a theory curriculum out there but I think that is what is great about these forums.  I have learned a lot of stuff just searching the forum and reading forum posts.

[TrippyLighting]

On the other hand, if you really want to understand some of Fusion 360's underpinnings, you may want to go through some of @jeff_strater's posts.

I've been thinking of creating  a link collection and pehaps some commedium of all those I find useful. That'd be quite a book!