Bodies vs Components in Fusion 360 Explained - Learn Autodesk Fusion 360 in 30 Days: Day #13

hey there it's Kevin Kennedy and welcome to day number 13 of learn fusion 360 in 30 days by the end of this tutorial you'll have a solid understanding of the difference between bodies and components also be sure to watch to the end where I'll discuss the dubbed rule number one of fusion 360 now I've noticed a lot of explanations forget to talk about one important thing which is the difference of bottom-up assemblies vers top-down assemblies which may help you better understand why fusion 360 is set up the way it is so let's take a look at bottom-up assemblies first now this is the traditional assembly modeling technique and if you're coming from Autodesk Inventor or another CAD program then you're likely already familiar with it the essence of the bottom-up assembly technique is that each part is created individually and then all of the parts are inserted into an assembly document and constrained to each other there is no link between parts so the parts fit together because you design them to fit together and if you change one part you better know which other parts will be affected by the change and make sure that you update them accordingly now on the other hand we have top-down assemblies which means you start with an assembly file and you build all of your parts within the context of the assembly itself now fusion 360 falls into the top-down assembly category which is why you'll never see create new assembly under the file menu but you will an Autodesk Inventor in SolidWorks the benefit of top-down assemblies is that we can reference other sketches and parts so if we change one thing the other features change accordingly now this is a great way of ensuring that parts that need to fit together always fit together without you having to go back and manually edit them each time now this top-down technique is intuitive and much quicker but it does still have a few drawbacks you can still get yourself into a pickle especially with large assemblies that contain many different components which is why I recommend to plan out your model before you even start your very first sketch already so now that you know fusion 360 is based on the top-down assembly technique let's take a look at the difference between bodies and components bodies can be seen as modeling tools you use separate bodies to add or remove geometry to achieve the final shape of your design an example of a body could be a ceramic mug you would create one body for the cylindrical part of a cup and another body for the handle and of course join them together contrary components represent real-world parts you can think of them as things that are manufactured with multiple pieces you'll want to use components when your design consists of multiple parts that may be assembled to one another now a good example of a component would be a door hinge as it consists of three different components one for the left wing of the hinge one for the right wing and the third is the pin that holds the hinge together now let's take a deeper dive into both of these concepts with bodies you'll create a new one anytime you turn a sketch into a 3d object if we take a look at the ceramic mug once again you'll see that the downside to bodies is that they can't be copied to another file unless it's in direct modeling mode now this is mainly because copying the parametric timeline can be difficult so if for some reason you do want to copy a body to a completely different file then you'll have to change it to direct modeling mode by clicking on that little Settings icon in the lower right hand corner then you'll have to select do not capture design history and click continue and as you will see it will delete the timeline so if I go to copy this mug again to a file that is also in direct modeling mode you'll see that now it will actually let me paste it into the other file now with that said if you're planning on copying you should make it into a component and we'll discuss that in just a bit before we do that let's take a look at a few other cons in regards to bodies first off they won't show up in a parts list which could become troublesome if you need to create a drawing that includes all of the parts second pattern bodies will act independently from their parent so if you alter one of these bodies you'll notice that others don't change whereas if I had made them components and I alter one then the other two will update accordingly now if we take a look at the screws that our bodies will notice that components can be created from anything that is in the body folder here but components cannot be created from sketches so if we right click you'll see that there is no option to create a new component but if we right-click on the body that we can create a new component now in order to turn a body into a component it does not have to be closed and in fact there are three different types of bodies in fusion 360 we have solid or surface bodies we have skull two bodies and we have mesh bodies now there are two main ways we can create a component from a body we can either right-click on a body and select create components from bodies or we can go up to a symbol and hit create new component select from bodies and we'll select the body and then we can hit OK now another quick thing to note if I select two bodies here that does not mean it will put them in the same component if I go ahead and do that it will actually create two different components and if we take a look at it in the browser we'll see the bodies here now another thing to know is that they are both labeled body number one so this is where the dubbed rule number two from the fusion 360 form comes in place which is to always always rename your components and bodies right after you create them and it's even a good idea to get into the habit of renaming any sketches decals or any other layers you may have as well so what the heck are components and why should we use them instead of bodies if we take another look at our door hinge example will see that components contain bodies and they also contain sketches planes and other objects these three components of our door hinge make up our assembly now in the beginning of this video I talked about bottom-up first top-down assemblies I mentioned that fusion 360 is the top-down assembly type because we can create all of our components within the same file and they're driven by one another so if we look at the browser tree we'll see that we have the master assembly at the top and then we have the components nested underneath we'll also see that the assembly is signified by the three cube icon the components are one cube and a body is a cylinder icon now let's take a look at some more advantages of using components over bodies first you can drag bodies and other objects from one component to another in the browser a component can also contain other components which is often referred to as a sub assembly components allow us to use joints to assemble and create mechanical relationships so we take a look at this door hinge example you'll see that it moves based on the joints I applied but if I created this with bodies and not components then I would not be able to apply these joints another trick and handy thing with components is that you can activate components which offers many advantages so if I click on this little circle icon to activate it and take a look at this component then I can focus solely on it and other components will be shown with some transparency now the advantage of activating components means that all the body sketches components or any other features that I create will automatically be nested within that component lastly and probably one of the most important things about components is that they can be reused or copy and pasted in a design so we can do this by right-clicking on the component and selecting copy and paste and we can duplicate them as many times as we would like and as we discussed earlier component instances update when a change is made to one of them now having a basic understanding of the difference between bodies and components leads us to the dubbed rule number one from the fusion 360 forum which is to always start your file off with a new component now rule number one was created by the fusion 360 community on the forums and the idea is that if you always start with a component you'll never be kicking yourself in the foot when your browser tree is messed up because you're trying to create components after creating your bodies so let's go ahead and recap everything it's okay to use bodies if you're just creating a small simple or quick model for something like 3d printing or something just to play around with while you're learning fusion 360 specifically if you know you don't plan on using it for any assemblies and you don't need to copy it otherwise it's a good practice get into the habit of always using components at the beginning of your design which will ensure that you can successfully create joints sub assemblies and assemblies without any major headaches now as we looked at previously it is possible to create components from bodies but again it's not recommended to do it afterwards because it won't always work and sometimes it will cause a lot of errors in your model thanks for watching I hope this clears up some of the confusion between bodies and components if you have any questions at all about components or bodies then be sure to hit that thumbs up icon and comment your questions below also be sure to hit that subscribe button to be notified of more fusion 360 tutorials

Channel: Product Design Online

Views: 67,873

Keywords: fusion 360, autodesk fusion 360, kevin kennedy fusion 360, product design online, fusion 360 tutorials, fusion tutorials, fusion 360 30 days, learn fusion 360 in 30 days, lars christensen fusion 360, fusion 360 beginners, fusion 360 kevin kennedy, autodesk fusion 30 days, #larslive, learn fusion 360 or die trying, bodies vs components, fusion 360 bodies vs, fusion 360 assembly, fusion 360 top-down modeling, fusion 360 bodies vs components, fusion 360 activate component

Id: 46UNmpQdbVc

Length: 10min 46sec (646 seconds)

Published: Thu Aug 09 2018

Reddit Comments

[u/G2nickk]

Ya this should've been first

[u/productdesignonline]

Did this clear up some of the confusion between BODIES and COMPONENTS? Let me know if you still have questions (in the comments on YouTube)!

[u/bent-grill]

you posted a link to the first video, not the 13th