Kevin Kennedy: Understanding the difference between bodies and components is an important step to becoming proficient in Fusion 360. Whether you’re an experienced CAD user coming from Autodesk Inventor or SolidWorks, or you’re completely new to the world of 3D modeling, this is a concept that you must understand. [Logo Chiming] To better understand components and bodies, you should first understand the two common types of assembly structures. CAD programs often utilize a bottom-up assembly structure or a top-down assembly structure. In regards to computer-aided design, the word assembly represents a group of parts gathered in one design file. Let’s first take a look at Bottom-Up Assemblies. This is the traditional assembly modeling technique. If you’re coming from Autodesk Inventor or another CAD program then you’re already familiar with it. The essence of the “Bottom-Up Assembly” technique is that each part is created as an individual file. All of the part files are then inserted into an assembly file, where the parts are constrained to each other. With this method, most programs do not create a link between parts. If the parts need to fit together then you’ll need to make sure you design them to the appropriate size before inserting them into the assembly file. If you change one part, you’d better know which other parts will be affected by the change and make sure that you go back and update them accordingly. On the other hand, we have “Top-Down Assemblies.” The top-down technique means you start with an assembly file and build all your parts within the context of the assembly. Parts can be built in place and can reference each other, making parts capable of automatically adapting when you change size or location. Fusion 360 falls into this top-down assembly category. Each new document you create can be treated as an assembly file. Although, one great thing about Fusion 360 is that you can technically use it in either manner. Later on in the course, we’ll look at inserting components into another design file, in a bottom-up manner. The benefit of top-down assemblies is that we can reference other sketches and parts, so if we change one thing the other features or parts change accordingly. This helps us ensure that parts always fit together, without you having to go back and manually edit single parts each time that we decide to change something. This top-down technique is intuitive and is often much quicker than bottom-up assemblies. Although, it does still have some drawbacks. You can still get yourself into trouble, especially with large assembly files, which is why it’s very important to think about your file’s structure before you start a new design. Another potential drawback is the file size and load time. A large assembly file, consisting of several hundred parts, may take longer to process changes. This is because each change has to reprocess all the references that are tied to other parts. If we look back at how we created our parametric bookshelf, you’ll remember that we started with a new file, and then created each part within the file, making it the top-down technique. If we had taken the bottom-up approach, then we would’ve had to create an individual design file for each of the unique boards. We then would’ve inserted them into another file, which served as the assembly. Now that we’ve briefly discussed “Top-Down” and “Bottom-up” assemblies, let’s dig into this concept further by looking at the difference between Fusion 360’s Bodies and Components. In Fusion 360, a body is any 3D shape used to add or remove geometry to achieve the final shape of your design. Looking at the Browser of our Parametric Bookshelf design, we can toggle open one of the components. We’ll then see a “bodies” folder is nested underneath each component. If we toggle open the bodies folder we’ll see a solid body. If you recall, we created this solid body using the box command. The box command is one of our solid modeling tools, which are all grouped in the solid tab of the toolbar. This solid body represents a solid object in real-life, meaning it contains realistic physical properties, such as density, mass, and volume. Fusion 360 also supports 3 other types of bodies. If we were to use the surface tools, located in the surface tab, then the body would result in a surface body. In the Browser, surface bodies are represented by an orange surface icon. Notice how the color orange correlates to the color of each surface feature. Surface bodies only represent the outer surface of an object, unless they’re closed off and turned into a solid body. Surface bodies are often used when the design is focused solely on the exterior contour. Notice how surface bodies also have a yellow face on one side, which helps us differentiate them from the solid bodies. Solid and Surface bodies are the core body types used in Fusion 360. They allow you to use the full toolset of features for creating assemblies, manufacturing and CAM setups, simulations, and so on. The third type of Fusion 360 body is a T-spline body. These bodies are created in the Form contextual environment, which is often referred to as the Sculpt environment. These bodies are designed to create and modify free-form shapes. In Fusion 360, t-spline modeling is a great way to explore shapes. While you’re in the Form environment, T-spline bodies are represented by the purple body icon in the Browser. Notice the faces and edges that subdivide this body, giving us more control over pushing and pulling the shape. However, once you finish the form, your body will turn into a surface body, resulting in only the outer surfaces. The fourth and final body type is the mesh body. Mesh bodies are often imported STL or OBJ data. These polygon mesh file types are popular among 3D printing platforms. Because polygon mesh modeling contains a different type of data, mesh files can only be used in a limited manner. In Fusion 360, you’ll only see a Mesh tab when you have an imported mesh file. Originally, Fusion 360 only allowed mesh geometry to be referenced. However, there are now a limited number of features that will help you adjust the mesh triangles. Because polygon mesh files contain a different type of data, the mesh tab will only be available when design history is turned off. You’ll see that mesh bodies are also represented by a yellow icon. At a technical level, all four of these body types are represented with different underlying math. That means that two bodies of different types cannot interact with one another. You’ll need to convert bodies to the same type before creating interactions between them. Each type of body has several different features that can be used to create new 3-dimensional bodies. In some cases, you’ll see a feature of the same name for each type of body. For example, the common commands for Extrude, Loft, and Sweep can be seen throughout the solid, surface, and form tabs. Once bodies are created, we can split them or modify them by subtracting or adding to them. This can be done using any of their respective features in the contextual tabs. Now that we’ve looked at bodies, let’s take a look at Fusion 360 components and how they differ. In Fusion 360, a component represents a “part” that can be used in an assembly file. Components can have motion and joints associated with them, which helps us manage all the parts within an assembly. You can think of components as a container, which can house any of the following: Bodies, Construction planes, Sketches, Canvases or reference images, Origin Planes, and other Components. If we look at our parametric bookshelf design, you’ll see that we have a total of eight components in the Browser. Each component represents one of the boards that make up the bookshelf. First, notice the component icon is a cube, which differs from the cylindrical solid body icon. Remember, Fusion 360 is most often used with a top-down assembly approach, as we create our components or “parts” all within one file. Because of this, you’ll see the top-level component is representing an assembly or collection of components. Notice the assembly icon is three component icons stacked together. If I open a new tab, you’ll see that the top-level component is a regular component, until components are nested underneath. Components can be grouped and nested within each other, which is commonly referred to as a “Sub-Assembly”. Sub-assemblies are a great way to organize and reuse “sections” of a model. To create a sub-assembly you simply need to head to the Browser and drag one component to another. Watch what happens as I drag the three shelves components to the Top Board component. You’ll see this creates a sub-assembly within our main assembly. This sub-assembly could be used to manage all the shelf components. Whether it be for moving them, copying them, or another relevant workflow. In most common workflows, including our parametric bookshelf design, a single component will only contain a single body. I often get asked by Fusion 360 beginners, “When should I use components and when should I use bodies”? First, it’s important to clarify that this is like comparing apples and oranges. Bodies and components represent two different things. Remember, bodies represent any 3-dimensional object, whether it be a solid, surface, mesh, or t-spline body. Components are not a different type of body. They act as a container that can not only group bodies, but also sketches, construction planes, reference images, more components, and origin planes. The use of components helps us organize the structure of our design. You can think of this concept as being similar to file folders on your computer. For example, say that you have a file folder on your desktop, which includes 100 different files. These files will represent our bodies, reference images, construction planes, and other assets. To further organize the files you may decide to create folders with their own unique names. Each folder represents a Fusion 360 component, helping us keep the file structure organized. All of the assets would be placed in a folder that makes the most sense, keeping their relationship with one another. The advantage of this is that if we decide we no longer need a part of the design or a file folder with this example, then we can delete the container or folder without a concern of it affecting our other parts. If we decide we want to move the component then we can move it without worrying about the component losing its reference geometry. One of the other key differences between components and bodies is that components are required for the use of joints and motion. In Fusion 360, joints are how we force parts to stay together, so we can mimic how they would respond in real-life. In the first intermediate project, the sawhorse design, we’ll take
a look at using joints and motion to make our project mimic reality.
The use of the Drawing workspace, Manufacture workspace, CAM tools, and some other Fusion 360 features also requires components. To summarize, you’ll want to create components to help organize your file structure - housing all of the relevant 3-dimensional bodies, sketches, construction geometry, and other assets. Components, which act as parts, are then used in conjunction with joints and motion, to place 3D bodies into the correct position. Let’s now take a look at
creating new components. In the parametric bookshelf
lesson, we created components in several different ways.
We created new components by using the “New Component” feature.
Remember, that can be activated from the toolbar, the assemble dropdown, by
right-clicking on a component in the Browser, or by using the shortcuts box.
We also created a component from a body, by right-clicking on a body in
the browser, which allowed us to use the feature, “Create Components from Bodies.”
If you recall, this feature is only used when we forget to create a component
before we created a 3-dimensional body. The last way to create a new component
is by selecting “New Component” as the operation when using a
modeling feature, such as Extrude. However, note that this route will
not place the relevant reference geometry, such as sketches and
construction planes, in the component. That is why you must avoid using
“New Component” from within command dialogs when you intend
to make copies of a component. This option is great for a design that
requires motion, hence the need for new components, but the sketch and body are
fine remaining in the parent component. Once components are created, you’ll
want to make sure you activate the component before conducting any work.
Activating components offers many advantages.
There are two ways to activate a component.
We can select the radio button that appears on hover, or we can
right-click and select “Activate”. Activating a component allows
you to focus solely on the active part, and the other components
will be shown with transparency. Again, the reason you need to first
“activate” a component is so that bodies, sketches, components, or
other features you create will be nested within that component.
Now that you’re aware of the various ways we can create a new component,
let’s look at a few tricks that will help us while working with components.
When components are placed in assemblies, they’re automatically visible and enabled.
Looking at our parametric bookshelf, you’ll remember that when we had one
component active, the others were automatically “ghosted” by default.
This is simply a visual setting that helps you focus on the active component.
It does not affect the physical integrity of the other parts.
It may not help much with smaller design files, but with large assembly files,
it will make a significant difference in being able to focus on the active part.
There are also a few other options that can be used
regarding component visibility. First, in the Browser, we can
simply click the corresponding eyeball icons to hide the component.
Of course, we simply need to click the visibility icon again
to get the component to reappear. Viewing and hiding components can
also be done with the keyboard shortcut letter “V,” as in Victor.
Note that this can be done at any time by selecting either a
component in the browser or a component in the canvas window.
The next option is the ability to isolate a component or sub-assembly
so it’s easier to work on. To isolate a component simply
right-click on the component in the Browser, and select the isolate option.
Notice how the component now appears by itself.
The isolate feature is simply a more efficient way to
hide the other components. Notice how all of their visibility
icons are now turned off. To change things back we
can “unisolate” the feature. You can also always use the “Unisolate
All” feature when you right-click on the top-level component,
which represents the assembly. Another option in the right-click menu
is to make a component unselectable. Notice how the red “no” symbol appears
on the component in the Browser. If I now try to select the component,
you’ll see that it cannot be selected until the unselectable option is disabled.
We also can set the opacity of a component to an exact percentage.
This can be helpful if you want to lower the opacity of certain
components or subassemblies, making it easier to look at others.
Last but not least, there are two options that help us find a component in the
canvas window or the parametric timeline. If we select the “Find in Window”
option, you’ll see that Fusion 360 not only zooms in on the component
until it fills the frame, but it also highlights the component in blue.
The “Find in Timeline” option will highlight the component
in our parametric timeline. This feature is extremely helpful
in finding certain features as your parametric timeline continues to grow.
Now that you have a better understanding of component visibility,
let’s take a look at the dubbed #1 and #2 rules of Fusion 360.
Having a basic understanding of the difference between Bodies and Components leads us to the unofficial rule #1 from the Fusion 360 forums. Rule #1, which represents one of the most important “best practices,” is to always start your file off with a new component. Rule #1 was something created by the forum community, over the first few years of Fusion 360’s existence. As users transitioned from SolidWorks and other programs, it was discovered that if you always start with a component, you’ll be setting yourself up for success to have a better file structure in the Browser. This helps avoid any reference and relation issues that are present when components are not used before the creation of 3D bodies. Rule #2 suggests that you always rename your components and bodies right after you create them. I often advocate for renaming everything. This includes components, bodies, sketches, construction planes, reference images, and so on. This will make it easier to manage your file as your components or parts lists start to grow. Renaming assets in the Fusion 360 Browser will not only speed up your workflow in the long-term, but it will ensure you’re manipulating the correct body or component. To summarize this entire section, remember that in Fusion 360 the term “bodies” simply represents any 3-dimensional object. Components represent “containers” which group relevant assets, and they’re required to add joints and motion. Last but not least, I want to give a quick shoutout to all those who supported the channel over the last three weeks. Special thanks to the new Patrons... Jordon B, Kurt L, Jon R, Christopher M, Govianni V, Thomas W, Albert P, Peter B, Travis C, Mark L, Matt R, Collin S, Adam C, Alfred G, Lynda W, Z26, Mike B, Sean B, and Michael V. And thanks to those who support via my Buy Me a Coffee page... Faton S, @scacks, Marcus M, Jono, Ray, Adam C, Ted F, Fanny, and the anonymous contributors. [Upbeat Music] Be sure to subscribe to the channel so you don’t miss out on future lessons and click that playlist in the lower right-hand corner so you can learn more about Fusion 360’s core concepts. [End Upbeat Music]
